Navigation

  • Page 1

    GE Fanuc AutomationComputer Numerical Control ProductsSeries 21i / 210i―MBfor Machining CenterOperator's ManualGFZ-63614EN/01July 2001

  • Page 2

    GFL-001Warnings, Cautions, and Notesas Used in this PublicationWarningWarning notices are used in this publication to emphasize that hazardous voltages, currents,temperatures, or other conditions that could cause personal injury exist in this equipment or maybe associated with its use.In situatio...

  • Page 3

    s–1SAFETY PRECAUTIONSThis section describes the safety precautions related to the use of CNC units. It is essential that these precautionsbe observed by users to ensure the safe operation of machines equipped with a CNC unit (all descriptions in thissection assume this configuration). Note th...

  • Page 4

    SAFETY PRECAUTIONSB–63614EN/01s–21 DEFINITION OF WARNING, CAUTION, AND NOTEThis manual includes safety precautions for protecting the user and preventing damage to themachine. Precautions are classified into Warning and Caution according to their bearing on safety.Also, supplementary informa...

  • Page 5

    B–63614EN/01SAFETY PRECAUTIONSs–32 GENERAL WARNINGS AND CAUTIONSWARNING1. Never attempt to machine a workpiece without first checking the operation of the machine.Before starting a production run, ensure that the machine is operating correctly by performinga trial run using, for example, the ...

  • Page 6

    SAFETY PRECAUTIONSB–63614EN/01s–4WARNING8. Some functions may have been implemented at the request of the machine–tool builder. Whenusing such functions, refer to the manual supplied by the machine–tool builder for details of theiruse and any related cautions.NOTEPrograms, parameters, an...

  • Page 7

    B–63614EN/01SAFETY PRECAUTIONSs–53 WARNINGS AND CAUTIONS RELATED TOPROGRAMMINGThis section covers the major safety precautions related to programming. Before attempting toperform programming, read the supplied operator’s manual and programming manual carefullysuch that you are fully famili...

  • Page 8

    SAFETY PRECAUTIONSB–63614EN/01s–6WARNING6. Stroke checkAfter switching on the power, perform a manual reference position return as required. Strokecheck is not possible before manual reference position return is performed. Note that when strokecheck is disabled, an alarm is not issued even ...

  • Page 9

    B–63614EN/01SAFETY PRECAUTIONSs–74 WARNINGS AND CAUTIONS RELATED TO HANDLINGThis section presents safety precautions related to the handling of machine tools. Before attemptingto operate your machine, read the supplied operator’s manual and programming manual carefully,such that you are fu...

  • Page 10

    SAFETY PRECAUTIONSB–63614EN/01s–8WARNING7. Workpiece coordinate system shiftManual intervention, machine lock, or mirror imaging may shift the workpiece coordinatesystem. Before attempting to operate the machine under the control of a program, confirm thecoordinate system carefully.If the ma...

  • Page 11

    B–63614EN/01SAFETY PRECAUTIONSs–95 WARNINGS RELATED TO DAILY MAINTENANCEWARNING1. Memory backup battery replacementOnly those personnel who have received approved safety and maintenance training may performthis work.When replacing the batteries, be careful not to touch the high–voltage circ...

  • Page 12

    SAFETY PRECAUTIONSB–63614EN/01s–10WARNING2. Absolute pulse coder battery replacementOnly those personnel who have received approved safety and maintenance training may performthis work.When replacing the batteries, be careful not to touch the high–voltage circuits (marked andfitted with an...

  • Page 13

    B–63614EN/01SAFETY PRECAUTIONSs–11WARNING3. Fuse replacementBefore replacing a blown fuse, however, it is necessary to locate and remove the cause of theblown fuse.For this reason, only those personnel who have received approved safety and maintenancetraining may perform this work.When replac...

  • Page 14

    B–63614EN/01Table of Contentsc–1SAFETY PRECAUTIONSs–1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . I. GENERAL1. GENERAL3. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...

  • Page 15

    B–63614EN/02Table of Contentsc–25. FEED FUNCTIONS56. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5.1GENERAL57. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...

  • Page 16

    B–63614EN/01Table of Contentsc–311.3THE SECOND AUXILIARY FUNCTIONS (B CODES)116. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12.PROGRAM CONFIGURATION117. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12.1PROGRAM COMPONENTS OTHER THAN PRO...

  • Page 17

    B–63614EN/02Table of Contentsc–414.7SCALING (G50,G51)266. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14.8COORDINATE SYSTEM ROTATION (G68, G69)271. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ....

  • Page 18

    B–63614EN/01Table of Contentsc–519.4AI ADVANCED PREVIEW CONTROL365. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20.AXIS CONTROL FUNCTIONS381. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20.1SIMPLE SYNCHRONOU...

  • Page 19

    B–63614EN/02Table of Contentsc–63. MANUAL OPERATION442. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.1MANUAL REFERENCE POSITION RETURN443. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.2JOG FEED445. . . . ....

  • Page 20

    B–63614EN/01Table of Contentsc–78. DATA INPUT/OUTPUT522. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8.1FILES523. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ....

  • Page 21

    B–63614EN/02Table of Contentsc–89.6EXTENDED PART PROGRAM EDITING FUNCTION603. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9.6.1Copying an Entire Program604. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9.6....

  • Page 22

    B–63614EN/01Table of Contentsc–911.5SCREENS DISPLAYED BY FUNCTION KEY SYSTEM683. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11.5.1Displaying and Setting Parameters684. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...

  • Page 23

    B–63614EN/02Table of Contentsc–10E. STATUS WHEN TURNING POWER ON, WHEN CLEAR AND WHEN RESET762. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . F. CHARACTER–TO–CODES CORRESPONDENCE TABLE764. . . . . . . . . . . . . . . . . . G. ALARM LIST765. . . . . . . . . . . ...

  • Page 24

    I. GENERAL

  • Page 25

    GENERALB–63614EN/011. GENERAL31 GENERALThis manual consists of the following parts:I. GENERALDescribes chapter organization, applicable models, related manuals,and notes for reading this manual.II. PROGRAMMINGDescribes each function: Format used to program functions in the NClanguage, characte...

  • Page 26

    GENERAL1. GENERALB–63614EN/014This manual uses the following symbols:Indicates a combination of axes such as X__ Y__ Z (used inPROGRAMMING.).Indicates the end of a block. It actually corresponds to the ISO code LFor EIA code CR.The following table lists the manuals related to Series 16i, Serie...

  • Page 27

    GENERALB–63614EN/011. GENERAL5Manual nameSpecificationnumberPMCPMC Ladder Language PROGRAMMING MANUALB–61863EPMC C Language PROGRAMMING MANUALB–61863E–1NetworkFANUC I/O Link–II CONNECTION MANUALB–62714ENProfibus–DP Board OPERATOR’S MANUALB–62924ENDeviceNet Board OPERATOR’S MAN...

  • Page 28

    GENERAL1. GENERALB–63614EN/016When machining the part using the CNC machine tool, first prepare theprogram, then operate the CNC machine by using the program.1) First, prepare the program from a part drawing to operate the CNCmachine tool.How to prepare the program is described in the Chapter I...

  • Page 29

    GENERALB–63614EN/011. GENERAL7ToolSide cuttingFace cuttingHole machiningPrepare the program of the tool path and machining conditionaccording to the workpiece figure, for each machining.

  • Page 30

    GENERAL1. GENERALB–63614EN/018CAUTION1 The function of an CNC machine tool system depends notonly on the CNC, but on the combination of the machinetool, its magnetic cabinet, the servo system, the CNC, theoperator ’s panels, etc. It is too difficult to describe thefunction, programming, and ...

  • Page 31

    II. PROGRAMMING

  • Page 32

    PROGRAMMINGB–63614EN/011. GENERAL111 GENERAL

  • Page 33

    PROGRAMMING1. GENERALB–63614EN/0112The tool moves along straight lines and arcs constituting the workpieceparts figure (See II–4).The function of moving the tool along straight lines and arcs is called theinterpolation.ProgramG01 X_ _ Y_ _ ;X_ _ ;ToolWorkpieceFig. 1.1 (a) Tool movement alon...

  • Page 34

    PROGRAMMINGB–63614EN/011. GENERAL13Symbols of the programmed commands G01, G02, ... are called thepreparatory function and specify the type of interpolation conducted inthe control unit.(a) Movement along straight lineG01 Y_ _;X– –Y– – – –;(b) Movement along arcG03X––Y––R–...

  • Page 35

    PROGRAMMING1. GENERALB–63614EN/0114Movement of the tool at a specified speed for cutting a workpiece is calledthe feed.ToolWorkpieceTableFmm/minFig. 1.2 Feed functionFeedrates can be specified by using actual numerics. For example, to feedthe tool at a rate of 150 mm/min, specify the followin...

  • Page 36

    PROGRAMMINGB–63614EN/011. GENERAL15A CNC machine tool is provided with a fixed position. Normally, toolchange and programming of absolute zero point as described later areperformed at this position. This position is called the reference position.Reference positionToolWorkpieceTableFig. 1.3.1 R...

  • Page 37

    PROGRAMMING1. GENERALB–63614EN/0116ZYXPart drawingZYXCoordinate systemZYXToolWorkpieceMachine toolProgramCommandCNCFig. 1.3.2 (a) Coordinate systemThe following two coordinate systems are specified at different locations:(See II–7)(1) Coordinate system on part drawingThe coordinate system is ...

  • Page 38

    PROGRAMMINGB–63614EN/011. GENERAL17The positional relation between these two coordinate systems isdetermined when a workpiece is set on the table.Y YTableWorkpieceXXCoordinate system spe-cified by the CNC estab-lished on the tableCoordinate system onpart drawing estab-lished on the work-pieceFi...

  • Page 39

    PROGRAMMING1. GENERALB–63614EN/0118(2) Mounting a workpiece directly against the jigJigProgram zero pointMeet the tool center to the reference position. And set the coordinate systemspecified by CNC at this position. (Jig shall be mounted on the predeterminedpoint from the reference position....

  • Page 40

    PROGRAMMINGB–63614EN/011. GENERAL19Command for moving the tool can be indicated by absolute command orincremental command (See II–8.1).The tool moves to a point at “the distance from zero point of thecoordinate system” that is to the position of the coordinate values.B(10.0,30.0,20.0)YXTo...

  • Page 41

    PROGRAMMING1. GENERALB–63614EN/0120The speed of the tool with respect to the workpiece when the workpieceis cut is called the cutting speed.As for the CNC, the cutting speed can be specified by the spindle speedin min-1 unit.min-1f D mmm/minToolV: Cutting speedWorkpieceSpindle speed NTool diam...

  • Page 42

    PROGRAMMINGB–63614EN/011. GENERAL21When drilling, tapping, boring, milling or the like, is performed, it isnecessary to select a suitable tool. When a number is assigned to each tooland the number is specified in the program, the corresponding tool isselected.0102Tool numberATC magazine <Whe...

  • Page 43

    PROGRAMMING1. GENERALB–63614EN/0122When machining is actually started, it is necessary to rotate the spindle,and feed coolant. For this purpose, on–off operations of spindle motor andcoolant valve should be controlled.WorkpieceToolCoolant The function of specifying the on–off operations of...

  • Page 44

    PROGRAMMINGB–63614EN/011. GENERAL23A group of commands given to the CNC for operating the machine iscalled the program. By specifying the commands, the tool is moved alonga straight line or an arc, or the spindle motor is turned on and off.In the program, specify the commands in the sequence o...

  • Page 45

    PROGRAMMING1. GENERALB–63614EN/0124 The block and the program have the following configurations.N ffff G ff Xff.f Yfff.f M ff S ff T ff ;1 blockSequence numberPreparatory functionDimension wordMiscel-laneous functionSpindle functionTool func-tionEnd of blockFig. 1.7 (b)...

  • Page 46

    PROGRAMMINGB–63614EN/011. GENERAL25When machining of the same pattern appears at many portions of aprogram, a program for the pattern is created. This is called thesubprogram. On the other hand, the original program is called the mainprogram. When a subprogram execution command appears duringe...

  • Page 47

    PROGRAMMING1. GENERALB–63614EN/0126Usually, several tools are used for machining one workpiece. The toolshave different tool length. It is very troublesome to change the programin accordance with the tools.Therefore, the length of each tool used should be measured in advance.By setting the dif...

  • Page 48

    PROGRAMMINGB–63614EN/011. GENERAL27Limit switches are installed at the ends of each axis on the machine toprevent tools from moving beyond the ends. The range in which tools canmove is called the stroke.ÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇMotorLimit switchTableMachine zero pointSpecify these di...

  • Page 49

    PROGRAMMING2. CONTROLLED AXESB–63614EN/01282 CONTROLLED AXES

  • Page 50

    PROGRAMMING2. CONTROLLED AXESB–63614EN/0129Item21i–MB210i–MBNo. of basic controlled axes3 axesControlled axes expansion (total)Max. 4 axes (included in Cs axis)Basic simultaneously controlled axes2 axesSimultaneously controlled axes expansion (total)Max. 4 axesNOTEThe number of simultaneous...

  • Page 51

    PROGRAMMING2. CONTROLLED AXESB–63614EN/0130The increment system consists of the least input increment (for input) andleast command increment (for output). The least input increment is theleast increment for programming the travel distance. The least commandincrement is the least increment for...

  • Page 52

    PROGRAMMINGB–63614EN/013. PREPARATORY FUNCTION(G FUNCTION)313 PREPARATORY FUNCTION (G FUNCTION)A number following address G determines the meaning of the commandfor the concerned block.G codes are divided into the following two types.TypeMeaningOne–shot G codeThe G code is effective only in t...

  • Page 53

    PROGRAMMING3. PREPARATORY FUNCTION(G FUNCTION)B–63614EN/01321. When the clear state (bit 6 (CLR) of parameter No. 3402) is set atpower–up or reset, the modal G codes are placed in the states described below.(1) The modal G codes are placed in the states marked with asindicated in Table 3.(2...

  • Page 54

    PROGRAMMINGB–63614EN/013. PREPARATORY FUNCTION(G FUNCTION)33Table 3 G code list (1/3)G codeGroupFunctionG00PositioningG01Linear interpolationG02 01Circular interpolation/Helical interpolation CWG03Circular interpolation/Helical interpolation CCWG04Dwell, Exact stopG05High speed cycle machiningG...

  • Page 55

    PROGRAMMING3. PREPARATORY FUNCTION(G FUNCTION)B–63614EN/0134Table 3 G code list (2/3)G codeGroupFunctionG45Tool offset increaseG46Tool offset decreaseG4700Tool offset double increaseG48Tool offset double decreaseG4908Tool length compensation cancelG50Scaling cancelG5111ScalingG50.1Programmable ...

  • Page 56

    PROGRAMMINGB–63614EN/013. PREPARATORY FUNCTION(G FUNCTION)35Table 3 G code list (3/3)G codeGroupFunctionG90Absolute commandG9103Increment commandG92Setting for work coordinate system or clamp at maximum spindle speedG92.100Workpiece coordinate system presetG94Feed per minuteG9505Feed per rotati...

  • Page 57

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/01364 INTERPOLATION FUNCTIONS

  • Page 58

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS37The G00 command moves a tool to the position in the workpiece systemspecified with an absolute or an incremental command at a rapid traverserate.In the absolute command, coordinate value of the end point isprogrammed.In the incremental command ...

  • Page 59

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/0138The rapid traverse rate cannot be specified in the address F.Even if linear interpolation positioning is specified, nonlinearinterpolation positioning is used in the following cases. Therefore, becareful to ensure that the tool does not foul t...

  • Page 60

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS39For accurate positioning without play of the machine (backlash), finalpositioning from one direction is available.Start positionTemporary stopEnd positionOverrunStart position _ : For an absolute command, the coordinates of an end position, an...

  • Page 61

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/0140D During canned cycle for drilling, no single direction positioning iseffected in Z axis.D No single direction positioning is effected in an axis for which nooverrun has been set by the parameter.D When the move distance 0 is commanded, the sin...

  • Page 62

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS41Tools can move along a lineF_:Speed of tool feed (Feedrate) _:For an absolute command, the coordinates of an end point , and for an incremental commnad, the distance the tool moves.G01 _F_;IPIPA tools move along a line to the specified posi...

  • Page 63

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/0142A calcula;tion example is as follows.G91 G01 X20.0B40.0 F300.0 ;This changes the unit of the C axis from 40.0 deg to 40mm with metricinput. The time required for distribution is calculated as follows:202) 402300400.14907The feed rate for the C...

  • Page 64

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS43The command below will move a tool along a circular arc.G17G03 Arc in the XpYp planeArc in the ZpXpplaneG18Arc in the YpZpplaneXp_Yp_G02G03G02G03G02G19Xp_ p_Yp_ Zp_I_ J_R_F_ ;I_ K_R_F_J_ K_R_F_Table 4.4 Description of the command formatCommandD...

  • Page 65

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/0144“Clockwise”(G02) and “counterclockwise”(G03) on the XpYp plane(ZpXp plane or YpZp plane) are defined when the XpYp plane is viewedin the positive–to–negative direction of the Zp axis (Yp axis or Xp axis,respectively) in the Cartesia...

  • Page 66

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS45The distance between an arc and the center of a circle that contains the arccan be specified using the radius, R, of the circle instead of I, J, and K.In this case, one arc is less than 180°, and the other is more than 180° areconsidered. Wh...

  • Page 67

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/01461006040090120 14020060R50RY axisX axisThe above tool path can be programmed as follows ;(1) In absolute programmingG92X200.0 Y40.0 Z0 ;G90 G03 X140.0 Y100.0R60.0 F300.;G02 X120.0 Y60.0R50.0 ;orG92X200.0 Y40.0Z0 ;G90 G03 X140.0 Y100.0I-60.0 F300...

  • Page 68

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS47Helical interpolation which moved helically is enabled by specifying upto two other axes which move synchronously with the circularinterpolation by circular commands.G03 Synchronously with arc of XpYp planeSynchronously with arc of ZpXp planeG1...

  • Page 69

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/0148The amount of travel of a rotary axis specified by an angle is onceinternally converted to a distance of a linear axis along the outer surfaceso that linear interpolation or circular interpolation can be performed withanother axis. After inter...

  • Page 70

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS49To perform tool offset in the cylindrical interpolation mode, cancel anyongoing cutter compensation mode before entering the cylindricalinterpolation mode. Then, start and terminate tool offset within thecylindrical interpolation mode.In the c...

  • Page 71

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/0150Example of a Cylindrical Interpolation ProgramO0001 (CYLINDRICAL INTERPOLATION ); N01 G00 G90 Z100.0 C0 ; N02 G01 G91 G18 Z0 C0 ; N03 G07.1 C57299 ;N04 G90 G01 G42 Z120.0 D01 F250 ; N05 C30.0 ; N06 G02 Z90.0 C60.0 R30.0 ; N07 G01 Z70.0 ; N08 G0...

  • Page 72

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS51Straight threads with a constant lead can be cut. The position codermounted on the spindle reads the spindle speed in real–time. The readspindle speed is converted to the feedrate per minute to feed the tool.G33 _ F_ ;PIF : Long axis dire...

  • Page 73

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/01521 The spindle speed is limited as follows :1 x spindle speed x Spindle speed : min-1Thread lead : mm or inchMaximum feedrate : mm/min or inch/min ; maximum command–specified feedrate forfeed–per–minute mode or maximum feedrate that is det...

  • Page 74

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS53Linear interpolation can be commanded by specifying axial movefollowing the G31 command, like G01. If an external skip signal is inputduring the execution of this command, execution of the command isinterrupted and the next block is executed.T...

  • Page 75

    PROGRAMMING4. INTERPOLATION FUNCTIONSB–63614EN/0154G31G91X100.0 F100;Y50.0;50.0100.0Skip signal is input hereActual motionMotion without skip signalYXFig. 4.8 (a) The next block is an incremental command G31G90X200.00 F100;Y100.0;Y100.0X200.0Skip signal is input hereActual motionMotion without ...

  • Page 76

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS55The skip function operates based on a high–speed skip signal (connecteddirectly to the NC; not via the PMC) instead of an ordinary skip signal.In this case, up to eight signals can be input. Delay and error of skip signal input is 0 – 2 ms...

  • Page 77

    PROGRAMMING5. FEED FUNCTIONSB–63614EN/01565 FEED FUNCTIONS

  • Page 78

    PROGRAMMINGB–63614EN/015. FEED FUNCTIONS57The feed functions control the feedrate of the tool. The following two feedfunctions are available:1. Rapid traverseWhen the positioning command (G00) is specified, the tool moves ata rapid traverse feedrate set in the CNC (parameter No. 1420).2. Cutti...

  • Page 79

    PROGRAMMING5. FEED FUNCTIONSB–63614EN/0158If the direction of movement changes between specified blocks duringcutting feed, a rounded–corner path may result (Fig. 5.1 (b)).0Programmed pathActual tool pathYXFig. 5.1 (b) Example of tool path between two blocks In circular interpolation, a radi...

  • Page 80

    PROGRAMMINGB–63614EN/015. FEED FUNCTIONS59G00 IP_ ;G00 : G code (group 01) for positioning (rapid traverse) IP_ ; Dimension word for the end pointIPIPThe positioning command (G00) positions the tool by rapid traverse. Inrapid traverse, the next block is executed after the specified feedratebe...

  • Page 81

    PROGRAMMING5. FEED FUNCTIONSB–63614EN/0160Feedrate of linear interpolation (G01), circular interpolation (G02, G03),etc. are commanded with numbers after the F code. In cutting feed, the next block is executed so that the feedrate change fromthe previous block is minimized.Four modes of specif...

  • Page 82

    PROGRAMMINGB–63614EN/015. FEED FUNCTIONS61After specifying G94 (in the feed per minute mode), the amount of feedof the tool per minute is to be directly specified by setting a number afterF. G94 is a modal code. Once a G94 is specified, it is valid until G95 (feedper revolution) is specified....

  • Page 83

    PROGRAMMING5. FEED FUNCTIONSB–63614EN/0162When a one–digit number from 1 to 9 is specified after F, the feedrateset for that number in a parameter (Nos. 1451 to 1459) is used. WhenF0 is specified, the rapid traverse rate is applied.The feedrate corresponding to the number currently selected ...

  • Page 84

    PROGRAMMINGB–63614EN/015. FEED FUNCTIONS63Cutting feedrate can be controlled, as indicated in Table 5.4.Table 5.4 Cutting Feedrate ControlFunction nameG codeValidity of G codeDescriptionExact stopG09This function is valid for specifiedblocks only.The tool is decelerated at the end pointof a bl...

  • Page 85

    PROGRAMMING5. FEED FUNCTIONSB–63614EN/0164Exact stopG09 IP_ ;Exact stop modeG61 ;Cutting modeG64 ;Tapping modeG63 ;Automatic corner overrideG62 ;IPThe inter–block paths followed by the tool in the exact stop mode, cuttingmode, and tapping mode are different (Fig. 5.4.1).0Y(1)(2)Position check...

  • Page 86

    PROGRAMMINGB–63614EN/015. FEED FUNCTIONS65When cutter compensation is performed, the movement of the tool isautomatically decelerated at an inner corner and internal circular area.This reduces the load on the cutter and produces a smoothly machinedsurface.When G62 is specified, and the tool pat...

  • Page 87

    PROGRAMMING5. FEED FUNCTIONSB–63614EN/0166When a corner is determined to be an inner corner, the feedrate isoverridden before and after the inner corner. The distances Ls and Le,where the feedrate is overridden, are distances from points on the cuttercenter path to the corner (Fig. 5.4.2.1 (b),...

  • Page 88

    PROGRAMMINGB–63614EN/015. FEED FUNCTIONS67Regarding program (2) of an arc, the feedrate is overridden from point ato point b and from point c to point d (Fig. 5.4.2.1 (d)).cdaLsLebLsLe(2)Programmed pathCutter center pathToolFig. 5.4.2.1 (d) Override Range (Straight Line to Arc, Arc to Straight...

  • Page 89

    PROGRAMMING5. FEED FUNCTIONSB–63614EN/0168For internally offset circular cutting, the feedrate on a programmed pathis set to a specified feedrate (F) by specifying the circular cutting feedratewith respect to F, as indicated below (Fig. 5.4.2.2). This function is validin the cutter compensati...

  • Page 90

    PROGRAMMINGB–63614EN/015. FEED FUNCTIONS69DwellG04 X_ ; or G04 P_ ; X_ : Specify a time (decimal point permitted) P_ : Specify a time (decimal point not permitted)By specifying a dwell, the execution of the next block is delayed by thespecified time. In addition, a dwell can be specified to mak...

  • Page 91

    PROGRAMMING6. REFERENCE POSITIONB–63614EN/01706 REFERENCE POSITIONA CNC machine tool has a special position where, generally, the tool isexchanged or the coordinate system is set, as described later. Thisposition is referred to as a reference position.

  • Page 92

    PROGRAMMINGB–63614EN/016. REFERENCE POSITION71The reference position is a fixed position on a machine tool to which thetool can easily be moved by the reference position return function.For example, the reference position is used as a position at which toolsare automatically changed. Up to fou...

  • Page 93

    PROGRAMMING6. REFERENCE POSITIONB–63614EN/0172Tools are automatically moved to the reference position via anintermediate position along a specified axis. Or, tools are automaticallymoved from the reference position to a specified position via anintermediate position along a specified axis. Wh...

  • Page 94

    PROGRAMMINGB–63614EN/016. REFERENCE POSITION73Positioning to the intermediate or reference positions are performed at therapid traverse rate of each axis.Therefore, for safety, the cutter compensation, and tool lengthcompensation should be cancelled before executing this command.The coordinates...

  • Page 95

    PROGRAMMING6. REFERENCE POSITIONB–63614EN/0174NOTE1 To this feedrate, a rapid traverse override (F0 ,25,50,100%)is applied, for which the setting is 100%.2 After a machine coordinate system has been establishedupon the completion of reference position return, theautomatic reference position ret...

  • Page 96

    PROGRAMMINGB–63614EN/016. REFERENCE POSITION75The lamp for indicating the completion of return does not go on when themachine lock is turned on, even when the tool has automatically returnedto the reference position. In this case, it is not checked whether the toolhas returned to the reference...

  • Page 97

    PROGRAMMING7. COORDINATE SYSTEMB–63614EN/01767 COORDINATE SYSTEMBy teaching the CNC a desired tool position, the tool can be moved to theposition. Such a tool position is represented by coordinates in acoordinate system. Coordinates are specified using program axes.When three program axes, th...

  • Page 98

    PROGRAMMINGB–63614EN/017. COORDINATE SYSTEM77The point that is specific to a machine and serves as the reference of themachine is referred to as the machine zero point. A machine tool buildersets a machine zero point for each machine.A coordinate system with a machine zero point set as its ori...

  • Page 99

    PROGRAMMING7. COORDINATE SYSTEMB–63614EN/0178A coordinate system used for machining a workpiece is referred to as aworkpiece coordinate system. A workpiece coordinate system is to be setwith the CNC beforehand (setting a workpiece coordinate system).A machining program sets a workpiece coordin...

  • Page 100

    PROGRAMMINGB–63614EN/017. COORDINATE SYSTEM79The user can choose from set workpiece coordinate systems as describedbelow. (For information about the methods of setting, see II– 7.2.1.)(1) Once a workpiece coordinate system is selected by G92 or automaticworkpiece coordinate system setting, a...

  • Page 101

    PROGRAMMING7. COORDINATE SYSTEMB–63614EN/0180The six workpiece coordinate systems specified with G54 to G59 canbe changed by changing an external workpiece zero point offset valueor workpiece zero point offset value. Three methods are available to change an external workpiece zeropoint offset ...

  • Page 102

    PROGRAMMINGB–63614EN/017. COORDINATE SYSTEM81With the G10 command, each workpiece coordinate system can bechanged separately.By specifying G92IP_;, a workpiece coordinate system (selected with acode from G54 to G59) is shifted to set a new workpiece coordinatesystem so that the current tool pos...

  • Page 103

    PROGRAMMING7. COORDINATE SYSTEMB–63614EN/0182XXYYA160100100100200If G92X100Y100; is commanded when the toolis positioned at (200, 160) in G54 mode, work-piece coordinate system 1 (X’ – Y’) shifted byvector A is created.60G54 workpiece coordinate systemTool positionNew workpiece coordinate...

  • Page 104

    PROGRAMMINGB–63614EN/017. COORDINATE SYSTEM83The workpiece coordinate system preset function presets a workpiececoordinate system shifted by manual intervention to the pre–shiftworkpiece coordinate system. The latter system is displaced from themachine zero point by a workpiece zero point of...

  • Page 105

    PROGRAMMING7. COORDINATE SYSTEMB–63614EN/0184(a) Manual intervention performed when the manual absolute signal is off(b) Move command executed in the machine lock state(c) Movement by handle interrupt(d) Operation using the mirror image function (e) Setting the local coordinate system using G52...

  • Page 106

    PROGRAMMINGB–63614EN/017. COORDINATE SYSTEM85Besides the six workpiece coordinate systems (standard workpiececoordinate systems) selectable with G54 to G59, 48 additional workpiececoordinate systems (additional workpiece coordinate systems) can beused. Alternatively, up to 300 additional workp...

  • Page 107

    PROGRAMMING7. COORDINATE SYSTEMB–63614EN/0186When an absolute workpiece zero point offset value is specified, thespecified value becomes a new offset value. When an incrementalworkpiece zero point offset value is specified, the specified value is addedto the current offset value to produce a n...

  • Page 108

    PROGRAMMINGB–63614EN/017. COORDINATE SYSTEM87When a program is created in a workpiece coordinate system, a childworkpiece coordinate system can be set for easier programming. Such achild coordinate system is referred to as a local coordinate system.G52 IP _; Setting the local coordinate syste...

  • Page 109

    PROGRAMMING7. COORDINATE SYSTEMB–63614EN/0188WARNING1 When an axis returns to the reference point by the manual reference point return function,thezero point of the local coordinate system of the axis matches that of the work coordinate system.The same is true when the following command is issu...

  • Page 110

    PROGRAMMINGB–63614EN/017. COORDINATE SYSTEM89Select the planes for circular interpolation, cutter compensation, anddrilling by G–code. The following table lists G–codes and the planes selected by them.Table 7.4 Plane selected by G codeG codeSelectedplaneXpYpZpG17Xp Yp planeX–axis or an...

  • Page 111

    PROGRAMMING8. COORDINATE VALUE AND DIMENSIONB–63614EN/01908 COORDINATE VALUE AND DIMENSIONThis chapter contains the following topics.8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91)8.2 POLAR COORDINATE COMMAND (G15, G16)8.3 INCH/METRIC CONVERSION (G20, G21)8.4 DECIMAL POINT PROGRAMMING

  • Page 112

    PROGRAMMINGB–63614EN/018. COORDINATE VALUEAND DIMENSION91There are two ways to command travels of the tool; the absolutecommand, and the incremental command. In the absolute command,coordinate value of the end position is programmed; in the incrementalcommand, move distance of the position itse...

  • Page 113

    PROGRAMMING8. COORDINATE VALUE AND DIMENSIONB–63614EN/0192The end point coordinate value can be input in polar coordinates (radiusand angle). The plus direction of the angle is counterclockwise of the selected planefirst axis + direction, and the minus direction is clockwise.Both radius and a...

  • Page 114

    PROGRAMMINGB–63614EN/018. COORDINATE VALUEAND DIMENSION93Specify the radius (the distance between the current position and thepoint) to be programmed with an incremental command. The currentposition is set as the origin of the polar coordinate system.RadiusCommand positionActual positionAngleW...

  • Page 115

    PROGRAMMING8. COORDINATE VALUE AND DIMENSIONB–63614EN/0194N5 G15 G80 ;Canceling the polar coordinate commandIn the polar coordinate mode, specify a radius for circular interpolationor helical cutting (G02, G03) with R.Axes specified for the following commands are not considered part of thepol...

  • Page 116

    PROGRAMMINGB–63614EN/018. COORDINATE VALUEAND DIMENSION95Either inch or metric input can be selected by G code.G20 ;G21 ;Inch inputmm inputThis G code must be specified in an independent block before setting thecoordinate system at the beginning of the program. After the G code forinch/metric ...

  • Page 117

    PROGRAMMING8. COORDINATE VALUE AND DIMENSIONB–63614EN/0196Numerical values can be entered with a decimal point. A decimal pointcan be used when entering a distance, time, or speed. Decimal points canbe specified with the following addresses:X, Y, Z, U, V, W, A, B, C, I, J, K, Q, R, and F.Th...

  • Page 118

    PROGRAMMINGB–63614EN/019. SPINDLE SPEED FUNCTION (S FUNCTION)979 SPINDLE SPEED FUNCTION (S FUNCTION)The spindle speed can be controlled by specifying a value followingaddress S.This chapter contains the following topics.9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE9.2 SPECIFYING THE SPINDLE SPEE...

  • Page 119

    PROGRAMMING9. SPINDLE SPEED FUNCTION (S FUNCTION)B–63614EN/0198When a value is specified after address S, the code signal and strobe signalare sent to the machine to control the spindle rotation speed.A block can contain only one S code. Refer to the appropriate manualprovided by the machine t...

  • Page 120

    PROGRAMMINGB–63614EN/019. SPINDLE SPEED FUNCTION (S FUNCTION)99Specify the surface speed (relative speed between the tool and workpiece)following S. The spindle is rotated so that the surface speed is constantregardless of the position of the tool.G96 Sfffff ;↑ Surface speed (m/min or feet/m...

  • Page 121

    PROGRAMMING9. SPINDLE SPEED FUNCTION (S FUNCTION)B–63614EN/01100G96 (constant surface speed control command) is a modal G code. Aftera G96 command is specified, the program enters the constant surfacespeed control mode (G96 mode) and specified S values are assumed as asurface speed. A G96 com...

  • Page 122

    PROGRAMMINGB–63614EN/019. SPINDLE SPEED FUNCTION (S FUNCTION)101G96 modeG97 modeSpecify the surface speed in m/min (or feet/min)G97 commandStore the surface speed in m/min (or feet/min)Command forthe spindlespeedSpecifiedThe specifiedspindle speed(min-1) is usedNot specifiedThe surface speed (m...

  • Page 123

    PROGRAMMING10. TOOL FUNCTION (T FUNCTION)B–63614EN/0110210 TOOL FUNCTION (T FUNCTION)Two tool functions are available. One is the tool selection function, andthe other is the tool life management function.General

  • Page 124

    PROGRAMMINGB–63614EN/0110. TOOL FUNCTION(T FUNCTION)103By specifying an up to 8–digit numerical value following address T, toolscan be selected on the machine.One T code can be commanded in a block. Refer to the machine toolbuilder’s manual for the number of digits commandable with address...

  • Page 125

    PROGRAMMING10. TOOL FUNCTION (T FUNCTION)B–63614EN/01104Tools are classified into various groups, with the tool life (time orfrequency of use) for each group being specified. The function ofaccumulating the tool life of each group in use and selecting and usingthe next tool previously sequen...

  • Page 126

    PROGRAMMINGB–63614EN/0110. TOOL FUNCTION(T FUNCTION)105Tool life management data consists of tool group numbers, tool numbers,codes specifying tool compensation values, and tool life value.The Max. number of groups and the number of tools per group that canbe registered are set by parameter (GS...

  • Page 127

    PROGRAMMING10. TOOL FUNCTION (T FUNCTION)B–63614EN/01106In a program, tool life management data can be registered in the CNC unit,and registered tool life management data can be changed or deleted.A different program format is used for each of the four types of operationsdescribed below.After a...

  • Page 128

    PROGRAMMINGB–63614EN/0110. TOOL FUNCTION(T FUNCTION)107G10L3 ;PL ;TH D ;TH D ;PL ;TH D ;TH D ;G11 ;M02 (M30) ;G10L3 :Register with deleting all groupsP:Group numberL:Life valueT:Tool numberH:Code specifying tool offset value (H code)D:Code specifying tool offset value (D code)G11:End of regis...

  • Page 129

    PROGRAMMING10. TOOL FUNCTION (T FUNCTION)B–63614EN/01108G10L3 orG10L3P1);PL Q ;TH D ;TH D ;PL Q ;TH D ;TH D ;G11 ;M02 (M30) ;⋅⋅Q_ : Life count type (1:Frequency, 2:Time)Meaning of commandFormatD Setting a tool life couttype for groupsCAUTION1 When the Q command is omitted, the value set ...

  • Page 130

    PROGRAMMINGB–63614EN/0110. TOOL FUNCTION(T FUNCTION)109The following command is used for tool life management:Toooo; Specifies a tool group number.The tool life management function selects, from a specified group, atool whose life has not expired, and outputs its T code. In oooo,specify a numb...

  • Page 131

    PROGRAMMING10. TOOL FUNCTION (T FUNCTION)B–63614EN/01110For tool life management, the four tool change types indicated below areavailable. The type used varies from one machine to another. For details,refer to the appropriate manual of each machinde tool builder.Table 10.2.3 Tool Change TypeToo...

  • Page 132

    PROGRAMMINGB–63614EN/0110. TOOL FUNCTION(T FUNCTION)111Suppose that the tool life management ignore number is 100.T101;A tool whose life has not expired is selected from group 1.(Suppose that tool number 010 is selected.)M06T102;Tool life counting is performed for the tool in group 1.(The life ...

  • Page 133

    PROGRAMMING10. TOOL FUNCTION (T FUNCTION)B–63614EN/01112The life of a tool is specified by a usage frequency (count) or usage time(in minutes).The usage count is incremented by 1 for each tool used in a program.In other words, the usage count is incremented by 1 only when the firsttool group nu...

  • Page 134

    PROGRAMMINGB–63614EN/0111. AUXILIARY FUNCTION11311 AUXILIARY FUNCTIONThere are two types of auxiliary functions ; miscellaneous function (Mcode) for specifying spindle start, spindle stop program end, and so on,and secondary auxiliary function (B code) for specifying index tablepositioning.When...

  • Page 135

    PROGRAMMING11. AUXILIARY FUNCTIONB–63614EN/01114When a numeral is specified following address M, code signal and astrobe signal are sent to the machine. The machine uses these signals toturn on or off its functions.Usually, only one M code can be specified in one block. In some cases,however, u...

  • Page 136

    PROGRAMMINGB–63614EN/0111. AUXILIARY FUNCTION115In general, only one M code can be specified in a block. However, up tothree M codes can be specified at once in a block by setting bit 7 (M3B)of parameter No. 3404 to 1. Up to three M codes specified in a block aresimultaneously output to the m...

  • Page 137

    PROGRAMMING11. AUXILIARY FUNCTIONB–63614EN/01116Indexing of the table is performed by address B and a following 8–digitnumber. The relationship between B codes and the correspondingindexing differs between machine tool builders.Refer to the manual issued by the machine tool builder for detai...

  • Page 138

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION11712 PROGRAM CONFIGURATIONThere are two program types, main program and subprogram. Normally,the CNC operates according to the main program. However, when acommand calling a subprogram is encountered in the main program,control is passed to the...

  • Page 139

    PROGRAMMING12. PROGRAM CONFIGURATIONB–63614EN/01118A program consists of the following components:Table 12 Program componentsComponentsDescriptionsTape startSymbol indicating the start of a program fileLeader sectionUsed for the title of a program file, etc.Program startSymbol indicating the s...

  • Page 140

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION119This section describes program components other than program sections.See II–12.2 for a program section.Fig. 12.1(a) Program configurationThe tape start indicates the start of a file that contains NC programs.The mark is not required when pr...

  • Page 141

    PROGRAMMING12. PROGRAM CONFIGURATIONB–63614EN/01120NOTEIf one file contains multiple programs, the EOB code forlabel skip operation must not appear before a second orsubsequent program number.Any information enclosed by the control–out and control–in codes isregarded as a comment.The user c...

  • Page 142

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION121A tape end is to be placed at the end of a file containing NC programs.If programs are entered using the automatic programming system, themark need not be entered. The mark is not displayed on the screen. However, when a file is output,the mark...

  • Page 143

    PROGRAMMING12. PROGRAM CONFIGURATIONB–63614EN/01122This section describes elements of a program section. See II–12.1 forprogram components other than program sections.%(COMMENT)%TITLE;O0001 ;N1 … ;M30 ;Program sectionComment sectionProgram numberSequence numberProgram endFig. 12.2(a) Pr...

  • Page 144

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION123A program consists of several commands. One command unit is called ablock. One block is separated from another with an EOB of end of blockcode. Table 12.2(a) EOB codeNameISOcodeEIAcodeNotation in thismanualEnd of block (EOB)LFCR;A...

  • Page 145

    PROGRAMMING12. PROGRAM CONFIGURATIONB–63614EN/01124A block consists of one or more words. A word consists of an addressfollowed by a number some digits long. (The plus sign (+) or minus sign(–) may be prefixed to a number.)Word = Address + number (Example : X–1000)For an address, one of th...

  • Page 146

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION125Major addresses and the ranges of values specified for the addresses areshown below. Note that these figures represent limits on the CNC side,which are totally different from limits on the machine tool side. Forexample, the CNC allows a tool to...

  • Page 147

    PROGRAMMING12. PROGRAM CONFIGURATIONB–63614EN/01126When a slash followed by a number (/n (n=1 to 9)) is specified at the headof a block, and optional block skip switch n on the machine operator panelis set to on, the information contained in the block for which /ncorresponding to switch number ...

  • Page 148

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION127The end of a program is indicated by programming one of the followingcodes at the end of the program:Table 12.2(d) Code of a program endCodeMeaning usageM02For main programM30M99For subprogramIf one of the program end codes is executed in progr...

  • Page 149

    PROGRAMMING12. PROGRAM CONFIGURATIONB–63614EN/01128If a program contains a fixed sequence or frequently repeated pattern, sucha sequence or pattern can be stored as a subprogram in memory to simplifythe program.A subprogram can be called from the main program. A called subprogram can also call ...

  • Page 150

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION129NOTE1 The M98 and M99 code signal and strobe signal are notoutput to the machine tool.2 If the subprogram number specified by address P cannot befound, an alarm (No. 078) is output.l M98 P51002 ;l X1000.0 M98 P1200 ;l Execution sequence of subp...

  • Page 151

    PROGRAMMING12. PROGRAM CONFIGURATIONB–63614EN/01130If P is used to specify a sequence number when a subprogram isterminated, control does not return to the block after the calling block, butreturns to the block with the sequence number specified by P. Note,however, that P is ignored if the mai...

  • Page 152

    PROGRAMMINGB–63614EN/0112. PROGRAM CONFIGURATION131A subprogram can be executed just like a main program by searching forthe start of the subprogram with the MDI.(See III–9.3 for information about search operation.)In this case, if a block containing M99 is executed, control returns to thesta...

  • Page 153

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/0113213 FUNCTIONS TO SIMPLIFY PROGRAMMINGThis chapter explains the following items:13.1CANNED CYCLE13.2RIGID TAPPING13.3OPTIONAL ANGLE CHAMFERING AND CORNER ROUNDING13.4EXTERNAL MOTION FUNCTION13.5INDEX TABLE INDEXING FUNCTIONGeneral

  • Page 154

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING133Canned cycles make it easier for the programmer to create programs.With a canned cycle, a frequently–used machining operation can bespecified in a single block with a G function; without canned cycles,normally more than one block ...

  • Page 155

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01134A canned cycle consists of a sequence of six operations (Fig. 13.1 (a))Operation 1 Positioning of axes X and Y(including also another axis)Operation 2 Rapid traverse up to point R levelOperation 3 Hole machiningOperation 4 Oper...

  • Page 156

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING135Assume that the U, V and W axes be parallel to the X, Y, and Z axesrespectively. This condition is specified by parameter No. 1022.G17 G81 ………Z _ _ : The Z axis is used for drilling.G17 G81 ………W _ _ : The W axis is us...

  • Page 157

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01136When the tool reaches the bottom of a hole, the tool may be returned topoint R or to the initial level. These operations are specified with G98 andG99. The following illustrates how the tool moves when G98 or G99 isspecified....

  • Page 158

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING137This cycle performs high–speed peck drilling. It performs intermittentcutting feed to the bottom of a hole while removing chips from the hole.G73 (G98)G73 (G99)G73 X_ Y_ Z_ R_ Q_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance...

  • Page 159

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01138The high–speed peck drilling cycle performs intermittent feeding alongthe Z–axis. When this cycle is used, chips can be removed from the holeeasily, and a smaller value can be set for retraction. This allows, drillingto b...

  • Page 160

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING139This cycle performs left–handed tapping. In the left–handed tappingcycle, when the bottom of the hole has been reached, the spindle rotatesclockwise.G74 (G98)G74 (G99)G74 X_ Y_ Z_ R_P_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The ...

  • Page 161

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01140Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Specify P in blocks that perform drilling. If it is specified ...

  • Page 162

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING141The fine boring cycle bores a hole precisely. When the bottom of the holehas been reached, the spindle stops, and the tool is moved away from themachined surface of the workpiece and retracted.G76 (G98)G76 (G99)G76 X_ Y_ Z_ R_ Q_ P...

  • Page 163

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01142When the bottom of the hole has been reached, the spindle is stopped atthe fixed rotation position, and the tool is moved in the direction oppositeto the tool tip and retracted. This ensures that the machined surface is notdam...

  • Page 164

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING143This cycle is used for normal drilling. Cutting feed is performed to thebottom of the hole. The tool is then retracted from the bottom of the holein rapid traverse.G81 (G98)G81 (G99)G81 X_ Y_ Z_ R_ F_ K_ ;X_ Y_ : Hole position dat...

  • Page 165

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01144Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Do not specify a G code of the 01 group (G00 to G03 or G60 (when...

  • Page 166

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING145This cycle is used for normal drilling. Cutting feed is performed to the bottom of the hole. At the bottom, a dwellis performed, then the tool is retracted in rapid traverse. This cycle is used to drill holes more accurately with...

  • Page 167

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01146Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Specify P in blocks that perform drilling. If it is specified i...

  • Page 168

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING147This cycle performs peck drilling. It performs intermittent cutting feed to the bottom of a hole whileremoving shavings from the hole.G83 (G98)G83 (G99)G83 X_ Y_ Z_ R_ Q_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from point...

  • Page 169

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01148Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Specify Q in blocks that perform drilling. If they are specifie...

  • Page 170

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING149An arbor with the overload torque detection function is used to retract thetool when the overload torque detection signal (skip signal) is detectedduring drilling. Drilling is resumed after the spindle speed and cuttingfeedrate are...

  • Page 171

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01150*Positioning along the X–axis and Y–axis*Positioning at point R along the Z–axis*Drilling along the Z–axis (first drilling, depth of cut Q, incremental)Retraction (bottom of the hole → small clearance ∆, incrementa...

  • Page 172

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING151In a single G83 cycle, drilling conditions are changed for each drillingoperation (advance → drilling → retraction). Bits 1 and 2 of parameterOLS, NOL No. 5160 can be specified to suppress the change in drillingconditions.1. Ch...

  • Page 173

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01152The forward or backward traveling speed can be specified with addressI in the same format as address F, as shown below:G83 I1000 ; (without decimal point)G83 I1000. ; (with decimal point)Both commands indicate a speed of 1000 m...

  • Page 174

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING153N01M03 S___ ;N02Mjj ;N03G83 X_ Y_ Z_ R_ Q_ F_ I_ K_ P_ ; N04X_ Y_ ;::N10G80 ;<Description of each block>N01: Specifies forward spindle rotation and spindle speed.N02: Specifies the M code to execute G83 as the small–hole pec...

  • Page 175

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01154Tapping is performed by rotating the spindle clockwise. When the bottomof the hole has been reached, the spindle is rotated in the reverse directionfor retraction. This operation creates threads.Feedrate overrides are ignored...

  • Page 176

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING155This cycle is used to bore a hole.G85 (G98)G85 (G99)G85 X_ Y_ Z_ R_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from point R to the bottom of the holeR_ : The distance from the initial level to point R levelF_ : Cutting feed ...

  • Page 177

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01156Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Do not specify a G code of the 01 group (G00 to G03 or G60 (when...

  • Page 178

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING157This cycle is used to bore a hole.G86 (G98)G86 (G99)G86 X_ Y_ Z_ R_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from point R to the bottom of the holeR_ : The distance from the initial level to point R levelF_ : Cutting feed ...

  • Page 179

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01158Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Do not specify a G code of the 01 group (G00 to G03 or G60 (when...

  • Page 180

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING159This cycle performs accurate boring.G87 (G98)G87 (G99)G87 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from the bottom of the hole to point ZR_ : The distance from the initial level to point R (the bottom of ...

  • Page 181

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01160After positioning along the X– and Y–axes, the spindle is stopped at thefixed rotation position. The tool is moved in the direction opposite to thetool tip, positioning (rapid traverse) is performed to the bottom of the ho...

  • Page 182

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING161This cycle is used to bore a hole.G88 (G98)G88 (G99)G88 X_ Y_ Z_ R_ P_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from point R to the bottom of the holeR_ : The distance from the initial level to point R levelP_ : Dwell time...

  • Page 183

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01162Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Specify P in blocks that perform drilling. If it is specified i...

  • Page 184

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING163This cycle is used to bore a hole.G89 (G98)G89 (G99)G89 X_ Y_ Z_ R_ P_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from point R to the bottom of the holeR_ : The distance from the initial level to point R levelP_ : Dwell time...

  • Page 185

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01164Before the drilling axis can be changed, the canned cycle must becanceled.In a block that does not contain X, Y, Z, R, or any other axes, drilling isnot performed.Specify P in blocks that perform drilling. If it is specified i...

  • Page 186

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING165G80 cancels canned cycles.G80 ;All canned cycles are canceled to perform normal operation. Point R andpoint Z are cleared. This means that R = 0 and Z = 0 in incremental mode.Other drilling data is also canceled (cleared).M3 S100 ...

  • Page 187

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01166400150250250150YXXZT 11T 15T 31#1#11#7#3#2#8#13#12#10#9#6#5#4# 11 to 16 Drilling of a 10mm diameter hole# 17 to 10 Drilling of a 20mm diameter hole# 11 to 13 Boring of a 95mm diameter hole(depth 50 mm)19020015025010010010010035...

  • Page 188

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING167Offset value +200.0 is set in offset No.11, +190.0 is set in offset No.15, and +150.0 is set in offset No.31Program example;N001G92X0Y0Z0;Coordinate setting at reference positionN002G90 G00 Z250.0 T11 M6;Tool changeN003G43 Z0 ...

  • Page 189

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01168The tapping cycle (G84) and left–handed tapping cycle (G74) may beperformed in standard mode or rigid tapping mode. In standard mode, the spindle is rotated and stopped along with amovement along the tapping axis using misce...

  • Page 190

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING169When the spindle motor is controlled in rigid mode as if it were a servomotor, a tapping cycle can be sped up.G84(G98)G84(G99)G84 X_ Y_ Z_ R_ P_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from point R to the bottom of the ho...

  • Page 191

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01170In feed–per–minute mode, the thread lead is obtained from theexpression, feedrate × spindle speed. In feed–per–revolution mode, thethread lead equals the feedrate speed.If a tool length compensation (G43, G44, or G49)...

  • Page 192

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING171Z–axis feedrate 1000 mm/minSpindle speed 1000 min-1Thread lead 1.0 mm <Programming of feed per minute>G94 ; Specify a feed–per–minute command.G00 X120.0 Y100.0 ;PositioningM29 S1000 ;Rigid mode specificationG84 Z–...

  • Page 193

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01172When the spindle motor is controlled in rigid mode as if it were a servomotor, tapping cycles can be sped up.G74 (G98)G74 (G99)G74 X_ Y_ Z_ R_ P_ F_ K_ ;X_ Y_ : Hole position dataZ_ : The distance from point R to the bottom of ...

  • Page 194

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING173In feed–per–minute mode, the thread lead is obtained from theexpression, feedrate × spindle speed. In feed–per–revolution mode, thethread lead equals the feedrate.If a tool length offset (G43, G44, or G49) is specified in ...

  • Page 195

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01174Z–axis feedrate 1000 mm/minSpindle speed 1000 min-1Thread lead 1.0 mm <Programming for feed per minute>G94 ;Specify a feed–per–minute command.G00 X120.0 Y100.0 ;PositioningM29 S1000 ;Rigid mode specificationG84...

  • Page 196

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING175Tapping a deep hole in rigid tapping mode may be difficult due to chipssticking to the tool or increased cutting resistance. In such cases, the peckrigid tapping cycle is useful. In this cycle, cutting is performed several times u...

  • Page 197

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01176After positioning along the X– and Y–axes, rapid traverse is performedto point R. From point R, cutting is performed with depth Q (depth of cutfor each cutting feed), then the tool is retracted by distance d. The DOVbit (...

  • Page 198

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING177Do not specify a group 01 G code (G00 to G03) and G73 in the same block.If they are specified together, G73 is canceled.In the canned cycle mode, tool offsets are ignored.The rigid tapping canned cycle is canceled. For how to cance...

  • Page 199

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01178Chamfering and corner rounding blocks can be inserted automaticallybetween the following:⋅Between linear interpolation and linear interpolation blocks⋅Between linear interpolation and circular interpolation blocks ⋅Betwee...

  • Page 200

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING179N001 G92 G90 X0 Y0 ;N002 G00 X10.0 Y10.0 ;N003 G01 X50.0 F10.0 ,C5.0 ;N004 Y25.0 ,R8.0 ;N005 G03 X80.0 Y50.0 R30.0 ,R8.0 ;N006 G01 X50.0 ,R8.0 ;N007 Y70.0 ,C5.0 ;N008 X10.0 ,C5.0 ;N009 Y10.0 ;N010 G00 X0 Y0 ;N011 M0 ;010.020.030.040...

  • Page 201

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01180Chamfering and corner rounding can be performed only in the planespecified by plane selection (G17, G18, or G19). These functions cannotbe performed for parallel axes.A block specifying chamfering or corner rounding must be fo...

  • Page 202

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING181Upon completion of positioning in each block in the program, an externaloperation function signal can be output to allow the machine to performspecific operation.Concerning this operation, refer to the manual supplied by the machine...

  • Page 203

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01182By specifying indexing positions (angles) for the indexing axis (onerotation axis, A, B, or C), the index table of the machining center can beindexed.Before and after indexing, the index table is automatically unclamped orclamp...

  • Page 204

    PROGRAMMINGB–63614EN/0113. FUNCTIONS TO SIMPLIFY PROGRAMMING1832. Using no miscellaneous functionsBy setting to bits 2, 3, and 4 of parameter ABS, INC,G90 No.5500,operation can be selected from the following two options.Select the operation by referring to the manual written by the machinetool ...

  • Page 205

    PROGRAMMING13. FUNCTIONS TO SIMPLIFY PROGRAMMINGB–63614EN/01184Table13.5 Index indexing function and other functionsItemExplanationRelative position displayThis value is rounded down when bit 1 of parameter REL No. 5500specifies this option.Absolute position displayThis value is rounded d...

  • Page 206

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION18514 COMPENSATION FUNCTIONThis chapter describes the following compensation functions:14.1 TOOL LENGTH OFFSET (G43, G44, G49)14.2 AUTOMATIC TOOL LENGTH MEASUREMENT (G37)14.3 TOOL OFFSET (G45–G48)14.4 OVERVIEW OF CUTTER COMPENSATION C (G40–G42...

  • Page 207

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01186This function can be used by setting the difference between the tool lengthassumed during programming and the actual tool length of the tool usedinto the offset memory. It is possible to compensate the difference withoutchanging the program.Sp...

  • Page 208

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION187Select tool length offset A, B, or C, by setting bits 0 and 1 of parameterTLC,TLB No. 5001.When G43 is specified, the tool length offset value (stored in offsetmemory) specified with the H code is added to the coordinates of the endposition spe...

  • Page 209

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01188(2) Cutter compensation CWhen the offset numbers for cutter compensation C are specified ormodified, the offset number validation order varies, depending on thecondition, as described below.O××××; H01 ; :G43P_ ;(1) :G44P_H02 ;(2) ...

  • Page 210

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION189NOTEThe tool length offset value corresponding to offset No. 0,that is, H0 always means 0. It is impossible to set any othertool length offset value to H0.Tool length offset B can be executed along two or more axes when the axesare specified i...

  • Page 211

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01190Actual positionProgrammed positionoffsetvalueε=4mmt1203030120t3t2+Y+X3050+Z3353018228Tool length offset (in boring holes No.1, 2, and 3)(1)(2)(3)(4)(5)(6)(7) (8)(9)(13)(10)(11)(12)⋅ProgramH1=–4.0(Tool length offset value)N1 G91 G00 X120.0 ...

  • Page 212

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION191This section describes the tool length offset cancellation and restorationperformed when G53, G28, G30, or G31 is specified in tool length offsetmode. Also described is the timing of tool length offset. (1) Tool length offset vector cancellati...

  • Page 213

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01192NOTEWhen tool length offset is applied to multiple axes, allspecified axes involved in reference position return aresubject to cancellation.When tool length offset cancellation is specified at the same time, toollength offset vector cancellatio...

  • Page 214

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION193In tool length offset modeTypeEVO (bit 6 of pa-rameter No. 5001)Restoration block1Block containing a G43/G44blockA/B0Block containing an H commandand G43/44 commandCIgnoredBlock containing aG43P_H_/G44P_H_ commandWARNINGWhen tool length offset ...

  • Page 215

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01194By issuing G37 the tool starts moving to the measurement position andkeeps on moving till the approach end signal from the measurementdevice is output. Movement of the tool is stopped when the tool tipreaches the measurement position.Differenc...

  • Page 216

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION195The difference between the coordinates of the position at which the toolreaches for measurement and the coordinates specified by G37 is addedto the current tool length offset value.Offset value = (Current compensation value) + [(Coordinates of ...

  • Page 217

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01196WARNINGWhen a manual movement is inserted into a movement ata measurement federate, return the tool to the!positionbefore the inserted manual movement for restart.NOTE1 When an H code is specified in the same block as G37, analarm is generated....

  • Page 218

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION197G92 Z760.0 X1100.0 ; Sets a workpiece coordinate system withrespect to the programmed absolute zero point.G00 G90 X850.0 ;Moves the tool to X850.0.That is the tool is moved to a position that is aspecified distance from the measurementposition ...

  • Page 219

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01198The programmed travel distance of the tool can be increased or decreasedby a specified tool offset value or by twice the offset value.The tool offset function can also be applied to an additional axis.ÇÇÇÇÇÇÇÇÇProgrammed pathTool cente...

  • Page 220

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION199As shown in Table 14.3(a), the travel distance of the tool is increased ordecreased by the specified tool offset value.In the absolute mode, the travel distance is increased or decreased as thetool is moved from the end position of the previous...

  • Page 221

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01200WARNING1 When G45 to G48 is specified to n axes (n=1–6) simultaneously in a motion block, offset isapplied to all n axes.When the cutter is offset only for cutter radius or diameter in taper cutting, overcutting orundercutting occurs. Theref...

  • Page 222

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION201NOTE1 When the specified direction is reversed by decrease as shown in the figure below, the toolmoves in the opposite direction.2 Tool offset can be applied to circular interpolation (G02, G03) with the G45 to G48 commandsonly for 1/4 and 3/4 ...

  • Page 223

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01202ÇÇÇÇÇÇÇÇÇTool diameter:20φOffset No.:01Tool offset value:+10.0805040504030RN1N2N3N4N5N6N7N8N9N10N11N12N13N14303040X axisY axisProgram using tool offsetOrigin30RProgramN1 G91 G46 G00 X80.0 Y50.0 D01 ;N2 G47 G01 X50.0 F120.0 ;N3 Y40.0 ;...

  • Page 224

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION203When the tool is moved, the tool path can be shifted by the radius of thetool (Fig. 14.4 (a)). To make an offset as large as the radius of the tool, CNC first creates anoffset vector with a length equal to the radius of the tool (start–up). ...

  • Page 225

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01204D Start up(Tool compensationstart)G00(or G01)G41(or G42)P_ D_ ;G41G42P_D_: Cutter compensation left (Group07): Cutter compensation right (Group07): Command for axis movement: Code for specifying as the cutter compensation value(1–3digits) (D...

  • Page 226

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION205In the offset mode, when a block which satisfies any one of the followingconditions is executed, the CNC enters the offset cancel mode, and theaction of this block is called the offset cancel. 1. G40 has been commanded. 2. 0 has been command...

  • Page 227

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01206If the offset amount is negative (–), distribution is made for a figure inwhich G41’s and G42’s are all replaced with each other on the program.Consequently, if the tool center is passing around the outside of theworkpiece, it will pass a...

  • Page 228

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION207Offset calculation is carried out in the plane determined by G17, G18 andG19, (G codes for plane selection). This plane is called the offset plane.Compensation is not executed for the coordinate of a position which is notin the specified plane...

  • Page 229

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01208ÇÇÇÇÇÇÇÇÇY axisX axisUnit : mmN1Start position650RC2 (1550,1550)650RC3 (–150,1150)250RC1(700,1300)P4(500,1150) P5(900,1150)P6(950,900)P9(700,650)P8(1150,550)P7(1150,900)P1(250,550)P3(450,900)P2(250,900)N2N3N4N5N6N7N8N9N10N11G92 X0 Y...

  • Page 230

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION209This section provides a detailed explanation of the movement of the toolfor cutter compensation C outlined in Section 14.4.This section consists of the following subsections:14.5.1 General14.5.2 Tool Movement in Start–up14.5.3 Tool Movement i...

  • Page 231

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01210When the offset cancel mode is changed to offset mode, the tool movesas illustrated below (start–up):αLSG42rLαSrLCG42Tool center pathStart positionProgrammed pathWork-pieceLinear→CircularStart positionWorkpieceTool center pathLinear→Lin...

  • Page 232

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION211Tool path in start–up has two types A and B, and they are selected byparameter SUP (No. 5003#0).Linear→LinearαProgrammed pathTool center pathLSG42rLLinear→CircularrType AType BαLSG42LWorkpieceStart positionrLLinear→LinearLinear...

  • Page 233

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01212Tool path in start–up has two types A and B, and they are selected byparameter SUP (No.5003#0).αLSG42rLS CType AType BrG42LG42LLLLSrrG42LLLSrrCLLLinear→LinearLinear→CircularLinear→LinearLinear→CircularWorkpieceWork-pieceWorkpiece...

  • Page 234

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION213If the command is specified at start–up, the offset vector is not created.SN9N6N7N8SSG91 G40 … ; :N6 X100.0 Y100.0 ;N7 G41 X0 ;N8 Y–100.0 ;N9 Y–100.0 X100.0 ;Programmed pathTool center pathrNOTEFor the definition of blocks that d...

  • Page 235

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01214In the offset mode, the tool moves as illustrated below:αLLαCSLSCLSCSCLinear→CircularLinear→LinearProgrammed pathIntersectionTool center pathWorkpieceWork-pieceTool center pathIntersectionProgrammed pathWorkpieceProgrammed pathTool center...

  • Page 236

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION215rrSrIntersectionProgrammed pathTool center pathIntersectionAlso in case of arc to straight line, straight line to arc and arc to arc, thereader should infer in the same procedure.D Tool movement aroundthe inside(α<1°) with anabnormally lon...

  • Page 237

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01216αLrCSLSCLSLLrLLLSrr Linear→LinearLinear→CircularProgrammed pathTool center pathIntersectionWorkpieceCircular→LinearCircular→CircularIntersectionTool center path Programmed pathWork-pieceIntersectionTool center pathProgrammed pathWorkpi...

  • Page 238

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION217αLLLLSrrLLrrCLLLLLLrrLSLSrrLCCLLinear→LinearProgrammed pathTool center pathWorkpieceLinear→CircularCircular→LinearCircular→CircularProgrammed pathWork-pieceTool center pathWorkpieceProgrammed pathTool center pathWork-pieceTool center p...

  • Page 239

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01218If the end of a line leading to an arc is programmed as the end of the arcby mistake as illustrated below, the system assumes that cuttercompensation has been executed with respect to an imaginary circle thathas the same center as the arc and p...

  • Page 240

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION219If the center of the arc is identical with the start position or end point, P/Salarm (No. 038) is displayed, and the tool will stop at the end position ofthe preceding block.N5N6N7rAlarm(No.038)is displayed and the toolstops(G41)N5 G01 X100.0 ;...

  • Page 241

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01220LLLSrrG42G41G41G42rrSCrrLCSSG41G41G42G42CCrrLinear→LinearLinear→CircularProgrammed pathTool center pathWorkpieceProgrammed pathTool center pathWorkpieceWorkpieceWorkpieceWorkpieceProgrammed pathTool center pathCircular→LinearCircular→Ci...

  • Page 242

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION221When changing the offset direction in block A to block B using G41 andG42, if intersection with the offset path is not required, the vector normalto block B is created at the start point of block B.G41(G42)(G42)LLLABrrSG42G41LSLS(G41)G42ABLSrLL...

  • Page 243

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01222Normally there is almost no possibility of generating this situation.However, when G41 and G42 are changed, or when a G40 wascommanded with address I, J, and K this situation can occur.In this case of the figure, the cutter compensation is not ...

  • Page 244

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION223If the following command is specified in the offset mode, the offset modeis temporarily canceled then automatically restored. The offset mode canbe canceled and started as described in II–15.6.2 and 15.6.4.If G28 is specified in the offset ...

  • Page 245

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01224The offset vector can be set to form a right angle to the moving directionin the previous block, irrespective of machining inner or outer side, bycommanding the cutter compensation G code (G41, G42) in the offsetmode, independently. If this co...

  • Page 246

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION225The following blocks have no tool movement. In these blocks, the toolwill not move even if cutter compensation is effected.M05 ;M code output. S21 ;S code output. G04 X10.0 ; DwellG10 L11 P01 R10.0 ; Cutter compensation value setting(G17) Z200...

  • Page 247

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01226When two or more vectors are produced at the end of a block, the toolmoves linearly from one vector to another. This movement is called thecorner movement. If these vectors almost coincide with each other, the corner movementisn’t performed ...

  • Page 248

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION227N4 G41 G91 G01 X150.0Y200.‘0 ;N5 X150.0 Y200.0 ;N6 G02 J–600.0 ; N7 G01 X150.0 Y–200.0 ; N8 G40 X150.0 Y–200.0 ;P1P2 P3 P4P5P6N5N6N4N7N8Programmed pathTool center pathIf the vector is not ignored, the tool path is as follows:P1 → P2 ...

  • Page 249

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01228αSrLCαLSG40rLWorkpieceG40LProgrammed pathProgrammed pathTool center pathTool center pathWork-pieceLinear→LinearCircular→Linear14.5.4Tool Movement inOffset Mode CancelExplanationsD Tool movement aroundan inside corner(180°xα)

  • Page 250

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION229Tool path has two types, A and B; and they are selected by parameter SUP(No. 5003#0).αLSG40rLαSrCType AType BαLSG40LIntersectionrαSCrrLLG40LG40LProgrammed pathWorkpieceTool center pathLinear→LinearCircular→LinearLinear→LinearWor...

  • Page 251

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01230Tool path has two types, A and B : and they are selected by parameter SUP(No. 5003#0)αLSG40rLSCType AType BrαG40LLLLrrLLSrrCLLG42αG40LG42LαSLinear→LinearCircular→LinearProgrammed pathTool center pathWorkpieceWork-pieceTool center ...

  • Page 252

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION231Start positionrG40(G42)LLS1°or lessProgrammed pathTool center pathWhen a block without tool movement is commanded together with anoffset cancel, a vector whose length is equal to the offset value is producedin a normal direction to tool motion...

  • Page 253

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01232If a G41 or G42 block precedes a block in which G40 and I_, J_, K_ arespecified, the system assumes that the path is programmed as a path fromthe end position determined by the former block to a vector determinedby (I,J), (I,K), or (J,K). The ...

  • Page 254

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION233In the example shown below, the tool does not trace the circle more thanonce. It moves along the arc from P1 to P2. The interference checkfunction described in II–15.6.5 may raise an alarm.(I, J)N5N6N7P1P2(G41)N5 G01 G91 X100.0 ;N6 G02 J–...

  • Page 255

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01234Tool overcutting is called interference. The interference check functionchecks for tool overcutting in advance. However, all interference cannotbe checked by this function. The interference check is performed even ifovercutting does not occur.(...

  • Page 256

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION235(2) In addition to the condition (1), the angle between the start point andend point on the tool center path is quite different from that betweenthe start point and end point on the programmed path in circularmachining(more than 180 degrees).Ce...

  • Page 257

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01236(1) Removal of the vector causing the interference When cutter compensation is performed for blocks A, B and C andvectors V1, V2, V3 and V4 between blocks A and B, and V5, V6, V7and V8 between B and C are produced, the nearest vectors are check...

  • Page 258

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION237(Example 2) The tool moves linearly from V1, V2, V7, to V8V6V3V5CCCrrV1V2V4V7V8AO1 O2BV4, V5 : InterferenceV3, V6 : InterferenceV2, V7 : No InterferenceProgrammed pathTool centerpath(2) If the interference occurs after correction (1), the too...

  • Page 259

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01238(1) Depression which is smaller than the cutter compensation valueTool center pathABCStoppedProgrammed pathThere is no actual interference, but since the direction programmed inblock B is opposite to that of the path after cutter compensation t...

  • Page 260

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION239When the radius of a corner is smaller than the cutter radius, because theinner offsetting of the cutter will result in overcuttings, an alarm isdisplayed and the CNC stops at the start of the block. In single blockoperation, the overcutting i...

  • Page 261

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01240When machining of the step is commanded by circular machining in thecase of a program containing a step smaller than the tool radius, the pathof the center of tool with the ordinary offset becomes reverse to theprogrammed direction. In this ca...

  • Page 262

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION241The above example should be modified as follows:ÊÊÊÊÊÊÊÊÊÊÊÊÊÊÊÊÊÊÊÊN1N1 G91 G00 G41 X500.0 Y500.0 D1 ;N3 G01 Z–250.0 ;N5 G01 Z–50.0 F100 ;N6 Y1000.0 F200 ;N6(500, 500)N3, N5:Move command for the Z axisAfter compensation...

  • Page 263

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01242Cutter compensation C is not performed for commands input from theMDI.However, when automatic operation using the absolute commands istemporarily stopped by the single block function, MDI operation isperformed, then automatic operation starts a...

  • Page 264

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION243A function has been added which performs positioning by automaticallycanceling a cutter compensation vector when G53 is specified in cuttercompensation C mode, then automatically restoring that cuttercompensation vector with the execution of th...

  • Page 265

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01244(1) G53 specified in offset modeWhen CCN (bit 2 of parameter No.5003)=0 Oxxxx;G90G41_ _;G53X_Y_; G00[Type A]Start–uprrss(G41G00)G53sG00[Type B]Start–uprrssG53sG00G00When CCN (bit 2 of parameter No.5003)=1G00[FS15 Type]rss(G41G00)G53sG00 (2)...

  • Page 266

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION245When CCN (bit2 of parameter No.5003)=1G90G00[FS15 Type]rss(G91G41G00)G53G00(3) G53 specified in offset mode with no movement specified When CCN (bit2 of parameter No.5003)=0Oxxxx;G90G41_ _;G00X20.Y20. ;G53X20.Y20. ; G00[Type A]Start–uprrss(G4...

  • Page 267

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01246WARNING1 When cutter compensation C mode is set and all–axis machine lock is applied, the G53command does not perform positioning along the axes to which machine lock is applied. Thevector, however, is preserved. When CCN (bit 2 of paramete...

  • Page 268

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION247NOTE1 When a G53 command specifies an axis that is not in the cutter compensation C plane, aperpendicular vector is generated at the end point of the previous block, and the tool does notmove. In the next block, offset mode is automatically re...

  • Page 269

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01248When G28, G30, or G30.1 is specified in cutter compensation C mode,an operation of FS15 type is performed if CCN (bit 2 of parameter No.5003) is set to 1.This means that an intersection vector is generated in the previous block,and a perpendicu...

  • Page 270

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION249(b) For return by G00When CCN (bit 2 of parameter No. 5003) = 0G00[Type A](G42G01)G01srrssOxxxx;G91G41_ _ _;G28X40.Y0 ;G00[Type B]s(G42G01)G01srrssReference position or floatingreference positionReference position or floatingreference positions...

  • Page 271

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01250When CCN (bit 2 of parameter No. 5003) = 1G29[FS15 Type]G28/30/30.1s(G42G01)G01srsG01Intermediate position = return positionReference position or floatingreference position(b) For return by G00When CCN (bit 2 of parameter No.5003)=0Oxxxx;G91G41...

  • Page 272

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION251(3) G28, G30, or G30.1, specified in offset mode (with movement to a reference position not performed)(a) For return by G29When CCN (bit 2 of parameter No.5003)=0Oxxxx;G91G41_ _ _;G28X40.Y–40.;G29X40.Y40.;G29[Type A]rs(G42G01)[Type B]G28/30/3...

  • Page 273

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01252(4) G28, G30, or G30.1 specified in offset mode (with no movementperformed)(a) For return by G29When CCN (bit 2 of parameter No.5003)=0O××××;G91G41_ _ _;G28X0Y0;G29X0Y0;[Type A]rs(G41G01)[Type B]G28/30/30.1/G29(G41G01)G28/30/30.1/G29G01rsG0...

  • Page 274

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION253When CCN (bit 2 of parameter No.5003)=1G00[FS15 Type]G28/30/30.1(G41G01)G01rsReference position or floatingreference position=Intermediate positionWARNING1 When a G28, G30, or G30.1 command is specified during all–axis machine lock, aperpendi...

  • Page 275

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01254NOTE1 When a G28, G30, or G30.1 command specifies an axis that is not in the cutter compensationC plane, a perpendicular vector is generated at the end point of the previous block, and the tooldoes not move. In the next block, offset mode is a...

  • Page 276

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION255When G29 is specified in cutter compensation C mode, an operation ofFS15 type is performed if CCN (bit 2 of parameter No. 5003) is set to 1.This means that an intersection vector is generated in the previous block,and vector cancellation is per...

  • Page 277

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01256(b) For specification made other than immediately after automaticreference position returnWhen CCN (bit 2 of parameter No.5003)=0O××××;G91G41_ _ _;G29X40.Y40.; [Type A]G29[Type B](G42G01)G01ssrssssr(G42G01)rrG01Return positionIntermediate p...

  • Page 278

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION257When CCN (bit 2 of parameter No.5003)=1G29[FS15 Type]G28/30/30.1(G42G01)G01srssReturn positionReference position or floatingreference position=Intermedi-ate position(b) For specification made other than immediately after automaticreference posi...

  • Page 279

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01258(3) G29 specified in offset mode (with movement to a reference positionnot performed)(a) For specification made immediately after automatic referenceposition returnWhen CCN (bit 2 of parameter No.5003)=0O××××;G91G41_ _ _;G28X0Y0;G29X0Y0; [T...

  • Page 280

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION259(b) For specification made other than immediately after automaticreference position returnO××××;G91G41_ _ _;G29X0Y0; [Type A](G42G01)G29[Type B]s(G42G01)ssrssG29sG01G01G01G01Intermediate position=Return positionIntermediate position=Return ...

  • Page 281

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01260(4) G29 specified in offset mode (with movement to an intermediateposition and reference position not performed)(a) For specification made immediately after automatic referenceposition return When CCN (bit 2 of parameter No.5003)=0O××××;G91...

  • Page 282

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION261(b) For specification made other than immediately after automaticreference position returnWhen CCN (bit 2 of parameter No.5003)=0O××××;G91G41_ _ _;G29X0Y0;[Type A](G41G01)sr[Type B](G41G01)ssrG01G01G01G01sG29G29Intermediate position=return ...

  • Page 283

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01262By specifying G39 in offset mode during cutter compensation C, cornercircular interpolation can be performed. The radius of the corner circularinterpolation equals the compensation value. In offset modeorG39 ;;I_J_I_K_J_K_G39When the command...

  • Page 284

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION263X axisY axis(0.0, 10.0)(–10.0, 10.0)Block N1Offset vectorBlock N2Block N3Programmed pathTool center path(In offset mode)N1 Y10.0 ; N2 G39 ; N3 X-10.0 ; ........X axisY axis(In offset mode)N1 Y10.0 ; N2 G39 I–1.0 J2.0 ; N3 X-10.0 Y20.0 ;.....

  • Page 285

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01264Tool compensation values include tool geometry compensationvalues and tool wear compensation (Fig. 14.6 (a)).OFSGOFSWOFSG:Geometric compensation valueOFSW:Wear compensation valueÇÇÇÇÇÇÇÇÇÇReference positionFig. 14.6 (a) Geometric comp...

  • Page 286

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION265Tool compensation memory A, B, or C can be used.The tool compensation memory determines the tool compensation valuesthat are entered (set) (Table 14.6 (b)).Table14.6 (b) Setting contents tool compensation memory and tool compensation valueTool ...

  • Page 287

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01266A programmed figure can be magnified or reduced (scaling).The dimensions specified with X_, Y_, and Z_ can each be scaled up ordown with the same or different rates of magnification.The magnification rate can be specified in the program.Unless ...

  • Page 288

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION267Least input increment of scaling magnification is: 0.001 or 0.00001 It isdepended on parameter SCR (No. 5400#7) which value is selected. Then,set parameter SCLx (No.5401#0) that enables scaling for each axis. Ifscaling P is not specified on t...

  • Page 289

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01268Even if different magnifications are applie to each axis in circularinterpolation, the tool will not trace an ellipse.When different magnifications are applied to axes and a circularinterpolation is specified with radius R, it becomes as follow...

  • Page 290

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION269This scaling is not applicable to cutter compensation values, tool lengthoffset values, and tool offset values (Fig. 14.7 (e) ).Cutter compensation values are not scaled.Programmed figureScaled figureFig. 14.7 (e) Scaling during cutter compens...

  • Page 291

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01270NOTE1 The position display represents the coordinate value after scaling.2 When a mirror image was applied to one axis of the specified plane, the following!results:(1)Circular command Direction of rotation is reversed.(2)Cutter compensation CO...

  • Page 292

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION271A programmed shape can be rotated. By using this function it becomespossible, for example, to modify a program using a rotation commandwhen a workpiece has been placed with some angle rotated from theprogrammed position on the machine.Further...

  • Page 293

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01272(α, β)XZCenter ofrotationAngle of rotation R (incremental value)Angle of rotation (absolute value)Fig. 14.8 (b) Coordinate system rotationNOTEWhen a decimal fraction is used to specify angulardisplacement (R_), the 1’s digit corresponds to...

  • Page 294

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION273In coordinate system rotation mode, G codes related to reference positionreturn (G27, G28, G29, G30, etc.) and those for changing the coordinatesystem (G52 to G59, G92, etc.) must not be specified. If any of these Gcodes is necessary, specify...

  • Page 295

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01274N1 G92 X0 Y0 G69 G01 ;N2 G42 G90 X1000 Y1000 F1000 D01 ;N3 G68 R*30000 ;N4 G91 X2000 ;N5 G03 Y1000 R1000 J500 ;N6 G01 X*2000 ;N7 Y*1000 ;N8 G69 G40 G90 X0 Y0 M30 ;It is possible to specify G68 and G69 in cutter compensation C mode.The rotation ...

  • Page 296

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION2752. When the system is in cutter compensation model C, specify thecommands in the following order (Fig.14.8(e)) :(cutter compensation C cancel)G51 ; scaling mode startG68 ; coordinate system rotation start: G41 ;cutter compensation C mode start:...

  • Page 297

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01276It is possible to store one program as a subprogram and recall subprogramby changing the angle.Programmed pathWhen offset isapplied(0, –10.0)Subprogram(0, 0)Sample program for when the RIN bit (bit 0 of parameter 5400) is setto 1. The specif...

  • Page 298

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION277When a tool with a rotation axis (C–axis) is moved in the XY plane duringcutting, the normal direction control function can control the tool so thatthe C–axis is always perpendicular to the tool path (Fig. 14.9 (a)). ToolToolProgrammed tool...

  • Page 299

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01278Center of the arcFig. 14.9 (c) Normal direction control right (G42.1)Programmed pathCutter center pathFig. 14.9 (b) Normal direction control left (G41.1)Cutter center pathProgrammed path When viewed from the center of rotation around the C...

  • Page 300

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION279SN1N2SN3SProgrammed pathS : Single block stop pointCutter center pathFig. 14.9 (e) Point at which a Single–Block Stop Occurs in the Normal Direction Control ModeBefore circular interpolation is started, the C–axis is rotated ...

  • Page 301

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01280Movement of the tool inserted at the beginning of each block is executedat the feedrate set in parameter 5481. If dry run mode is on at that time,the dry run feedrate is applied. If the tool is to be moved along the X–andY–axes in rapid t...

  • Page 302

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION281Specify the maximum distance for which machining is performed withthe same normal direction as that of the preceding block.D Linear movementWhen distance N2, shown below, is smaller than the set value,machining for block N2 is performed using t...

  • Page 303

    PROGRAMMING14. COMPENSATION FUNCTIONB–63614EN/01282A mirror image of a programmed command can be produced with respectto a programmed axis of symmetry (Fig. 14.10 (a)).Y100605050X60100(1)(2)(3)(4)(1) Original image of a programmed commandAxis of symmetry (X=50)Axis of symmetry(Y=50)(2) Image sy...

  • Page 304

    PROGRAMMINGB–63614EN/0114. COMPENSATION FUNCTION283If the programmable mirror image function is specified when thecommand for producing a mirror image is also selected by a CNC externalswitch or CNC setting (see III–4.7), the programmable mirror imagefunction is executed first.Applying a mirr...

  • Page 305

    PROGRAMMING15. CUSTOM MACROB–63614EN/0128415 CUSTOM MACROAlthough subprograms are useful for repeating the same operation, thecustom macro function also allows use of variables, arithmetic and logicoperations, and conditional branches for easy development of generalprograms such as pocketing an...

  • Page 306

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO285An ordinary machining program specifies a G code and the travel distancedirectly with a numeric value; examples are G100 and X100.0.With a custom macro, numeric values can be specified directly or usinga variable number. When a variable number is used,...

  • Page 307

    PROGRAMMING15. CUSTOM MACROB–63614EN/01286Local and common variables can have value 0 or a value in the followingranges :–1047 to –10–2910–29 to 1047If the result of calculation turns out to be invalid, an P/S alarm No. 111is issued.When a variable value is defined in a program, the dec...

  • Page 308

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO287(b) Operation< vacant > is the same as 0 except when replaced by < vacant>When #1 = < vacant >When #1 = 0#2 = #1##2 = < vacant >#2 = #1##2 = 0#2 = #1*5##2 = 0#2 = #1*5##2 = 0#2 = #1+#1##2 = 0#2 = #1 + #1##2 = 0(c) Conditional ex...

  • Page 309

    PROGRAMMING15. CUSTOM MACROB–63614EN/01288Program numbers, sequence numbers, and optional block skip numberscannot be referenced using variables.Example:Variables cannot be used in the following ways:O#1;/#2G00X100.0;N#3Y200.0;Limitations

  • Page 310

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO289System variables can be used to read and write internal NC data such astool compensation values and current position data. Note, however, thatsome system variables can only be read. System variables are essentialfor automation and general–purpose pr...

  • Page 311

    PROGRAMMING15. CUSTOM MACROB–63614EN/01290Table 15.2 (d) System variables for tool compensation memory CTool length compensation (H)Cutter compensation(D)CompensationnumberGeometriccompensationWear compensationGeomet-ric com-pensationWearcom-pensation1:200:400#11001(#2201):#11201(#2400):#11400...

  • Page 312

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO291Time information can be read and written.Table 15.2 (f) System variables for time informationVariablenumberFunction#3001This variable functions as a timer that counts in 1–millisecond in-crements at all times. When the power is turned on, the value ...

  • Page 313

    PROGRAMMING15. CUSTOM MACROB–63614EN/01292Table 15.2 (h) System variable (#3004) for automatic operation control#3004Feed holdFeedrate OverrideExact stop0EnabledEnabledEnabled1DisabledEnabledEnabled2EnabledDisabledEnabled3DisabledDisabledEnabled4EnabledEnabledDisabled5DisabledEnabledDisabled6E...

  • Page 314

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO293Settings can be read and written. Binary values are converted todecimals.#9 (FCV) : Whether to use the FS15 tape format conversion capability#5 (SEQ) : Whether to automatically insert sequence numbers#2 (INI): Millimeter input or inch input#1 (ISO): Wh...

  • Page 315

    PROGRAMMING15. CUSTOM MACROB–63614EN/01294NOTEDo not substitute a negative value.Modal information specified in blocks up to the immediately precedingblock can be read.Table 15.2 (j) System variables for modal informationVariable numberFunction#4001#4002#4003#4004#4005#4006#4007#4008#4009#4010...

  • Page 316

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO295Position information cannot be written but can be read.Table 15.2 (k) System variables for position informationVariablenumberPositioninformationCoordinatesystemTool com-pensationvalueReadoperationduringmovement#5001–#5004Block end pointWorkpiececoord...

  • Page 317

    PROGRAMMING15. CUSTOM MACROB–63614EN/01296Workpiece zero point offset values can be read and written.Table 15.2 (l) System variables for workpiece zero point offset valuesVariablenumberFunction#5201:#5204First–axis external workpiece zero point offset value :Fourth–axis ex...

  • Page 318

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO297The following variables can also be used:AxisFunctionVariable numberFirst axisExternal workpiece zero point offsetG54 workpiece zero point offsetG55 workpiece zero point offsetG56 workpiece zero point offsetG57 workpiece zero point offsetG58 workpiece z...

  • Page 319

    PROGRAMMING15. CUSTOM MACROB–63614EN/01298The operations listed in Table 15.3(a) can be performed on variables. Theexpression to the right of the operator can contain constants and/orvariables combined by a function or operator. Variables #j and #K in anexpression can be replaced with a const...

  • Page 320

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO299S Specify the lengths of two sides, separated by a slash (/).S The solution ranges are as follows:When the NAT bit (bit 0 of parameter 6004) is set to 0: 0o to 360_[Example] When #1 = ATAN[–1]/[–1]; is specified, #1 is 225.0.When the NAT bit (bit ...

  • Page 321

    PROGRAMMING15. CUSTOM MACROB–63614EN/01300With CNC, when the absolute value of the integer produced by anoperation on a number is greater than the absolute value of the originalnumber, such an operation is referred to as rounding up to an integer.Conversely, when the absolute value of the integ...

  • Page 322

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO301Brackets ([, ]) are used to enclose an expression. Note that parenthesesare used for comments.Errors may occur when operations are performed.Table 15.3 (b) Errors involved in operationsOperationAverageerrorMaximumerrorType of errora = b*c1.55×10–10...

  • Page 323

    PROGRAMMING15. CUSTOM MACROB–63614EN/01302S Also be aware of errors that can result from conditional expressionsusing EQ, NE, GE, GT, LE, and LT.Example:IF[#1 EQ #2] is effected by errors in both #1 and #2, possibly resultingin an incorrect decision.Therefore, instead find the difference betwee...

  • Page 324

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO303The following blocks are referred to as macro statements:S Blocks containing an arithmetic or logic operation (=) S Blocks containing a control statement (such as GOTO, DO, END)S Blocks containing a macro call command (such as macro calls byG65, G66, G6...

  • Page 325

    PROGRAMMING15. CUSTOM MACROB–63614EN/01304In a program, the flow of control can be changed using the GOTOstatement and IF statement. Three types of branch and repetitionoperations are used:Branch and repetitionGOTO statement (unconditional branch)IF statement (conditional branch: if ..., then....

  • Page 326

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO305Specify a conditional expression after IF.If the specified conditional expression is satisfied, a branch to sequencenumber n occurs. If the specified condition is not satisfied, the next blockis executed.IF [#1 GT 10] GOTO 2 ;N2 G00 G91 X10.0 ; ...

  • Page 327

    PROGRAMMING15. CUSTOM MACROB–63614EN/01306The sample program below finds the total of numbers 1 to 10.O9500; #1=0;Initial value of the variable to hold the sum #2=1;Initial value of the variable as an addendN1 IF[#2 GT 10] GOTO 2; Branch to N2 when the addend is greater than. 10 #1=#1+#2; Calcu...

  • Page 328

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO307The identification numbers (1 to 3) in a DO–END loop can be used asmany times as desired. Note, however, when a program includes crossingrepetition loops (overlapped DO ranges), P/S alarm No. 124 occurs.1. The identification numbers(1 to 3) can be us...

  • Page 329

    PROGRAMMING15. CUSTOM MACROB–63614EN/01308The sample program below finds the total of numbers 1 to 10.O0001;#1=0;#2=1;WHILE[#2 LE 10]DO 1;#1=#1+#2;#2=#2+1;END 1;M30;Sample program

  • Page 330

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO309A macro program can be called using the following methods:Macro callSimple call (G65)modal call (G66, G67)Macro call with G codeMacro call with M codeSubprogram call with M codeSubprogram call with T codeMacro call (G65) differs from subprogram call (M9...

  • Page 331

    PROGRAMMING15. CUSTOM MACROB–63614EN/01310When G65 is specified, the custom macro specified at address P is called.Data (argument) can be passed to the custom macro program.G65 P p L <argument–specification> ;P : Number of the program to call: Repetition count (1 by default)Argument ...

  • Page 332

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO311Argument specification II Argument specification II uses A, B, and C once each and uses I, J, andK up to ten times. Argument specification II is used to pass values suchas three–dimensional coordinates as arguments.ABCI1J1K1I2J2K2I3J3#1#2#3#4#5#6#7#8...

  • Page 333

    PROGRAMMING15. CUSTOM MACROB–63614EN/01312S The level of the main program is 0.S Each time a macro is called (with G65 or G66), the local variable levelis incremented by one. The values of the local variables at the previouslevel are saved in the CNC.S When M99 is executed in a macro program, ...

  • Page 334

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO313G65 P9100 X x Y y Z z R r F f I i A a B b H h ;X: X coordinate of the center of the circle (absolute or incremental specification)(#24). . . . . . . . . . . . . . . . . Y: Y coordinate of the center of the circle (absolute or incremental speci...

  • Page 335

    PROGRAMMING15. CUSTOM MACROB–63614EN/01314Once G66 is issued to specify a modal call a macro is called after a blockspecifying movement along axes is executed. This continues until G67is issued to cancel a modal call.O0001 ; :G66 P9100 L2 A1.0 B2.0 ;G00 G90 X100.0 ;Y200.0 ;X150.0 Y300.0 ;G...

  • Page 336

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO315The same operation as the drilling canned cycle G81 is created using acustom macro and the machining program makes a modal macro call. Forprogram simplicity, all drilling data is specified using absolute values.Z=0RZThe canned cycle consists of the fol...

  • Page 337

    PROGRAMMING15. CUSTOM MACROB–63614EN/01316By setting a G code number used to call a macro program in a parameter,the macro program can be called in the same way as for a simple call(G65).O0001 ; :G81 X10.0 Y20.0 Z–10.0 ; :M30 ;O9010 ; : : :N9 M99 ;Parameter No.6050 = 81By ...

  • Page 338

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO317By setting an M code number used to call a macro program in a parameter,the macro program can be called in the same way as with a simple call(G65).O0001 ; :M50 A1.0 B2.0 ; :M30 ;O9020 ; : : :M99 ;Parameter No.6080 = 50By setting an M...

  • Page 339

    PROGRAMMING15. CUSTOM MACROB–63614EN/01318By setting an M code number used to call a subprogram (macro program)in a parameter, the macro program can be called in the same way as witha subprogram call (M98).O0001 ; :M03 ; :M30 ;O9001 ; : : :M99 ;Parameter No.6071 = 03By setti...

  • Page 340

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO319By enabling subprograms (macro program) to be called with a T code ina parameter, a macro program can be called each time the T code isspecified in the machining program.O0001 ; :T23 ; :M30 ;O9000 ; : : :M99 ;Bit 5 of parameter 6001 ...

  • Page 341

    PROGRAMMING15. CUSTOM MACROB–63614EN/01320By using the subprogram call function that uses M codes, the cumulativeusage time of each tool is measured.S The cumulative usage time of each of tools T01 to T05 is measured.No measurement is made for tools with numbers greater than T05.S The following...

  • Page 342

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO321O9001(M03);Macro to start counting. . . . . . . . . . . . . . . . . . . . . . . . . . M01;IF[#4120 EQ 0]GOTO 9;No tool specified. . . . . . . . . . . . . . . . . . . . . IF[#4120 GT 5]GOTO 9;Out–of–range tool number. . . . . . . . . . . . . #3002=0;...

  • Page 343

    PROGRAMMING15. CUSTOM MACROB–63614EN/01322For smooth machining, the CNC prereads the NC statement to beperformed next. This operation is referred to as buffering. During AIadvanced preview control mode, the CNC prereads not only the nextblock but also the multiple blocks. And in the cutter comp...

  • Page 344

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO323N1 X100.0 ;>> : Block being executedj : Block read into the bufferNC statementexecutionMacro statementexecutionBufferN1N2N3N4N2 #1=100 ;N3 #2=200 ;N4 Y200.0 ; :N4When N1 is being executed, the next NC statement (N4) is read into thebuffer.T...

  • Page 345

    PROGRAMMING15. CUSTOM MACROB–63614EN/01324N1 G01 G41 X100.0 G100 Dd ;>> : Block being executedj : Blocks read into the bufferN1N2N3N2 #1=100 ;N3 Y100.0 ;N4 #2=200 ;N5 M08 ;N6 #3=300 ;N7 X200.0 ; :N4N3N5N6N7NC statementexecutionMacro statementexecutionBufferWhen the N1 is being exec...

  • Page 346

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO325Table 15.7.2 (a)MeaningNote(In case not to command M code preventing buffering or G53 block.)Number of VariableReadWriteProgram stopwith messageWrite#3006Program stops at maximum 2 blocks before a macro program.Time informa-tionReadWrite#3001,#3002The d...

  • Page 347

    PROGRAMMING15. CUSTOM MACROB–63614EN/01326Example)O0001O2000N1 X10.Y10.;(Mxx ;) Specify preventing buffering M code or G53N2 M98P2000;N100 #1=#5041; (Reading X axis current position) N3 Y200.0; N101 #2=#5042; (Reading Y axis current position) : : M99;In above case, the buffering of N2 b...

  • Page 348

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO327Custom macro programs are similar to subprograms. They can beregistered and edited in the same way as subprograms. The storagecapacity is determined by the total length of tape used to store both custommacros and subprograms.15.8REGISTERINGCUSTOM MACR...

  • Page 349

    PROGRAMMING15. CUSTOM MACROB–63614EN/01328The macro call command can be specified in MDI mode. Duringautomatic operation, however, it is impossible to switch to the MDI modefor a macro program call.A custom macro program cannot be searched for a sequence number.Even while a macro program is b...

  • Page 350

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO329In addition to the standard custom macro commands, the following macrocommands are available. They are referred to as external outputcommands.– BPRNT– DPRNT– POPEN– PCLOSThese commands are provided to output variable values and charactersth...

  • Page 351

    PROGRAMMING15. CUSTOM MACROB–63614EN/01330Example )LF12 (0000000C)M–1638400(FFE70000)Y410 (0000019A)XSpaceCBPRNT [ C** X#100 [3] Y#101 [3] M#10 [0] ]Variable value #100=0.40956 #101=–1638.4 #10=12.34DPRNT [ a #b [ c d ] … ]Number of significant decimal placesNumber of sig...

  • Page 352

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO331Example )spspspspspspDPRNT [ X#2 [53] Y#5 [53] T#30 [20] ]Variable value #2=128.47398 #5=–91.2 #30=123.456(1) Parameter PRT(No.6001#1)=0L FTY –X9120012847423spLFT23Y–91.200X128.474(2) Parameter PRT(No.6001#1)=0PCLOS ;The PCLOS command releas...

  • Page 353

    PROGRAMMING15. CUSTOM MACROB–63614EN/01332NOTE1 It is not necessary to always specify the open command(POPEN), data output command (BPRNT, DPRNT), andclose command (PCLOS) together. Once an opencommand is specified at the beginning of a program, it doesnot need to be specified again except aft...

  • Page 354

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO333When a program is being executed, another program can be called byinputting an interrupt signal (UINT) from the machine. This function isreferred to as an interruption type custom macro function. Program aninterrupt command in the following format:M96...

  • Page 355

    PROGRAMMING15. CUSTOM MACROB–63614EN/01334CAUTIONWhen the interrupt signal (UINT, marked by * in Fig. 15.11)is input after M97 is specified, it is ignored. And the interruptsignal must not be input during execution of the interruptprogram.A custom macro interrupt is available only during progr...

  • Page 356

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO335NOTEFor the status–triggered and edge–triggered schemes, seeItem “Custom macro interrupt signal (UINT)” of II– 15.11.2.There are two types of custom macro interrupts: Subprogram–typeinterrupts and macro–type interrupts. The interrupt typ...

  • Page 357

    PROGRAMMING15. CUSTOM MACROB–63614EN/01336(i) When the interrupt signal (UINT) is input, any movement or dwellbeing performed is stopped immediately and the interrupt programis executed.(ii) If there are NC statements in the interrupt program, the command inthe interrupted block is lost and the...

  • Page 358

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO337The interrupt signal becomes valid after execution starts of a block thatcontains M96 for enabling custom macro interrupts. The signal becomesinvalid when execution starts of a block that contains M97.While an interrupt program is being executed, the i...

  • Page 359

    PROGRAMMING15. CUSTOM MACROB–63614EN/01338There are two schemes for custom macro interrupt signal (UINT) input:The status–triggered scheme and edge– triggered scheme. When thestatus–triggered scheme is used, the signal is valid when it is on. Whenthe edge triggered scheme is used, the s...

  • Page 360

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO339To return control from a custom macro interrupt to the interruptedprogram, specify M99. A sequence number in the interrupted programcan also be specified using address P. If this is specified, the program issearched from the beginning for the specifie...

  • Page 361

    PROGRAMMING15. CUSTOM MACROB–63614EN/01340NOTEWhen an M99 block consists only of address O, N, P, L, orM, this block is regarded as belonging to the previous blockin the program. Therefore, a single–block stop does notoccur for this block. In terms of programming, the following and are basi...

  • Page 362

    PROGRAMMINGB–63614EN/0115. CUSTOM MACRO341(2) After control is returned to the interrupted program, modalinformation is specified again as necessary.O∆∆∆∆M96PxxxNffff;M99(Pffff);Oxxx;Interrupt signal (UINT)(Without P specification)Modify modalinformationModalinformation remainsunchanged...

  • Page 363

    PROGRAMMING15. CUSTOM MACROB–63614EN/01342When the interrupt signal (UINT) is input and an interrupt program iscalled, the custom macro modal call is canceled (G67). However, whenG66 is specified in the interrupt program, the custom macro modal callbecomes valid. When control is returned from...

  • Page 364

    PROGRAMMINGB–63614EN/0116. PATTERN DATA INPUTFUNCTION34316 PATTERN DATA INPUT FUNCTIONThis function enables users to perform programming simply by extractingnumeric data (pattern data) from a drawing and specifying the numericalvalues from the MDI panel. This eliminates the need for programmin...

  • Page 365

    PROGRAMMING16. PATTERN DATA INPUTFUNCTIONB–63614EN/01344Pressing the OFFSETSETTING key and [MENU] is displayed on the followingpattern menu screen. 1. BOLT HOLE 2. GRID 3. LINE ANGLE 4. TAPPING 5. DRILLING 6. BORING 7. POCKET 8. PECK 9. TEST PATRN10. BACKMENU : HOLE PATTERN ...

  • Page 366

    PROGRAMMINGB–63614EN/0116. PATTERN DATA INPUTFUNCTION345Menu title : C1 C2 C3 C4 C5 C6 C7 C8 C9C10 C11 C12C1,C2, ,C12 : Characters in the menu title (12 characters)Macro instructionG65 H90 Pp Qq Rr Ii Jj Kk :H90:Specifies the menu titlep : Assume a1 and a2 to be the codes of characters C1 and C...

  • Page 367

    PROGRAMMING16. PATTERN DATA INPUTFUNCTIONB–63614EN/01346Pattern name: C1 C2 C3 C4 C5 C6 C7 C8 C9C10C1, C2, ,C10: Characters in the pattern name (10 characters)Macro instructionG65 H91 Pn Qq Rr Ii Jj Kk ;H91: Specifies the menu titlen : Specifies the menu No. of the pattern namen=1 to 10 q : As...

  • Page 368

    PROGRAMMINGB–63614EN/0116. PATTERN DATA INPUTFUNCTION347Custom macros for the menu title and hole pattern names. 1. BOLT HOLE 2. GRID 3. LINE ANGLE 4. TAPPING 5. DRILLING 6. BORING 7. POCKET 8. PECK 9. TEST PATRN10. BACKMENU : HOLE PATTERN O0000 N00000> _MDI **** *** ***...

  • Page 369

    PROGRAMMING16. PATTERN DATA INPUTFUNCTIONB–63614EN/01348When a pattern menu is selected, the necessary pattern data isdisplayed.NO. NAMEDATA COMMENT500 TOOL0.000501 STANDARD X0.000*BOLT HOLE502 STANDARD Y0.000 CIRCLE*503 RADIUS0.000SET PATTERN504 S. ANGL0.000DATA TO VAR.505 HOLES N...

  • Page 370

    PROGRAMMINGB–63614EN/0116. PATTERN DATA INPUTFUNCTION349Menu title : C1 C2 C3 C4 C5 C6 C7 C8 C9C10C11C12C1 ,C2,…, C12 : Characters in the menu title (12 characters)Macro instructionG65 H92 Pp Qq Rr Ii Jj Kk ;H92 : Specifies the pattern namep : Assume a1 and a2 to be the codes of characters C...

  • Page 371

    PROGRAMMING16. PATTERN DATA INPUTFUNCTIONB–63614EN/01350One comment line: C1 C2 C3 C4 C5 C6 C7 C8 C9 C10 C11 C12C1, C2,…, C12 : Character string in one comment line (12 characters)Macro instructionG65 H94 Pp Qq Rr Ii Jj Kk ; H94 : Specifies the commentp : Assume a1 and a2 to be the codes of ...

  • Page 372

    PROGRAMMINGB–63614EN/0116. PATTERN DATA INPUTFUNCTION351Macro instruction to describe a parameter title , the variable name, anda comment.NO. NAMEDATA COMMENT500 TOOL0.000501 STANDARD X0.000*BOLT HOLE502 STANDARD Y0.000 CIRCLE*503 RADIUS0.000SET PATTERN504 S. ANGL0.000DATA TO VAR.50...

  • Page 373

    PROGRAMMING16. PATTERN DATA INPUTFUNCTIONB–63614EN/01352Table.16.3(a) Characters and codes to be used for the pattern data input functionChar-acterCodeCommentChar-acterCodeCommentA0656054B0667055C0678056D0689057E069032SpaceF070!033Exclama–tion markG071”034QuotationmarkH072#035Hash signI073...

  • Page 374

    PROGRAMMINGB–63614EN/0116. PATTERN DATA INPUTFUNCTION353Table 16.3 (b)Numbers of subprograms employed in the pattern data input functionSubprogram No.FunctionO9500Specifies character strings displayed on the pattern data menu.O9501Specifies a character string of the pattern data corresponding t...

  • Page 375

    PROGRAMMING17. PROGRAMMABLE PARAMETERENTRY (G10)B–63614EN/0135417 PROGRAMMABLE PARAMETER ENTRY (G10)The values of parameters can be entered in a lprogram. This function isused for setting pitch error compensation data when attachments arechanged or the maximum cutting feedrate or cutting time c...

  • Page 376

    PROGRAMMINGB–63614EN/0117. PROGRAMMABLE PARAMETERENTRY (G10)3551. Set bit 2 (SBP) of bit type parameter No. 3404G10L50 ; Parameter entry modeN3404 R 00000100 ; SBP settingG11 ; cancel parameter entry mode 2. Change the values for the Z–axis (3rd axis) and A–axis (4th axis) inaxis type param...

  • Page 377

    PROGRAMMING18. MEMORY OPERATION USING FS10/11 TAPE FORMATB–63614EN/0135618 MEMORY OPERATION USING FS10/11 TAPE FORMATMemory operation of the program registered by FS10/11 tape format ispossible with setting of the setting parameter (No. 0001#1).Data formats for cutter compensation, subprogram...

  • Page 378

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS35719 HIGH SPEED CUTTING FUNCTIONS

  • Page 379

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01358When an arc is cut at a high speed in circular interpolation, a radial errorexists between the actual tool path and the programmed arc. Anapproximation of this error can be obtained from the followingexpression:0YXr∆r:Error∆r :Maximu...

  • Page 380

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS359This function is designed for high–speed precise machining. With thisfunction, the delay due to acceleration/deceleration and the delay in theservo system which increase as the feedrate becomes higher can besuppressed.The tool can then...

  • Page 381

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01360⋅ External deceleration⋅ Simple synchronous control⋅ Sequence number comparison and stop⋅ Position switch(Bit 3 (PSF) of parameter No. 6901 can be set to also use this functionin the advanced preview control mode. Setting this pa...

  • Page 382

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS361A remote buffer can continuously supply a large amount of data to theCNC at high speeds when connected to the host computer or input/outputequipment via a serial interface.CNCRS–232–C / RS–422Remote bufferHost computerInput/output e...

  • Page 383

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01362VBinary input operation enabled :G05;VBinary input operation disabled :The travel distance alongall axes are set to zero.VData format for binary input operationL Data sequence1st axis2nd axisNth axisCheck byteByteHigh byteHigh byteHigh...

  • Page 384

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS363**************1514131211109876543210000000000000111111Example: When the travel distance is 700 µm per unit time (millimeter machine with increment system IS–B)1514131211109876543210All bytes of the block except for the check byte ([2*...

  • Page 385

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01364High–speed remote buffer A uses binary data. On the other hand,high–speed remote buffer B can directly use NC language coded withequipment such as an automatic programming unit to perform high–speedmachining.G05P01 ;Start high–sp...

  • Page 386

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS365G05.1 Q_ ;Q 1 : AI advanced preview control mode onQ 0 : AI advanced preview control mode offNOTE1 Please command G05.1 with an independent block.2 AI advanced preview control mode is released by the reset.The following functions become...

  • Page 387

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01366Linear interpolation,circle interpolation, etcPulseDistributionFeedrateCommandLinear acceleration/ decelerationbefore interpolationFeedrateCalculationServoControlAcceleration/ decelerationafterinterpolationInterpolationCalculation(Example...

  • Page 388

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS367 N1 N2 F3 F2 F1TimeFeedrate Specified feedrateFeed after acceleration / decelerationbefore interpolation is applied(2) Automatic corner decelerationThe feedrate at a corner is calculated for the axis for which the permissiblefeedra...

  • Page 389

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01368N1N2N2N1F1000 F500F1000 F500F1000 F500N2N1Tool path when the tooldoes not decelerated atthe cornerTool path when the tooldecelerates at the cornerN1 G01 G91 X100. F1000 ;N2 Y100. ;FeedrateFeedrateFeedrateWhen the tool does not decelerate ...

  • Page 390

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS369(3) Feedrate clamp based on accelerationAs shown below, when a curve is formed by very short successive linesegments, there is no significant feedrate difference along each axis ateach corner. Consequently, the tool need not be decelerate...

  • Page 391

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01370N9N5N1N9N5N1(4) Feedrate clamp based on arc radiusIn order that the acceleration in a circular interpolation block mustbecome a permissible value, the maximum permissible feedrate v for theprogrammed circle radius r is calculated from the...

  • Page 392

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS371NOTEThe maximum permissible feedrate v lowers as the circleradius becomes small. When the calculated feedrate islower than the parameter setting value (No.1732), themaximum permissible feedrate v will be assumed to be theparameter setting...

  • Page 393

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01372 Linear type acceleration /deceleration Bell type acceleration /decelerationtaIt depends on linear type acceleration.tbBell type acceleration / decelerationtcAcceleration / decelerationtime of bell typetc = ta + tbta is not constant. It d...

  • Page 394

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS373NOTE1 The overlapping rapid traverse blocks is ineffective.2 In case of using bell–shaped type acceleration /deceleration, the option of rapid traverse bell–shapedacceleration / deceleration is necessary.(6) Specifications listControl...

  • Page 395

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01374ItemFunctionHelical interpolation(G02, G03)f (Circular inter polation+Linear interpolation (up to 2 axes)Dwell (G04)f (Dwell in seconds and dwell in revolution)In case of dwell in revolution, the option ofthreading, synchronous cutting is...

  • Page 396

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS375ItemFunctionRapid traverse override1% step0 – 100 %Feed per minute (G94)fFeed per revolution(G95)×Rapid traverse bell–shapedAcceleration / decelera-tionfLinear acceleration / de-celerationBefore cutting feed in-terpolationf (Maximum ...

  • Page 397

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01376ItemFunctionProgrammable mirrorimage (G51.1)f(The option of programmable mirror image is needed.)Scaling (G51)f(The option of scaling is needed.)Coordinate system rotation (G68)f(The option of coordinate system rotation is needed.)Tool co...

  • Page 398

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS377ItemFunctionTool life management-Function×Macro executer(Execution macro)×MDI operationfManual intervention× (When the manual intervention is done, it is nec-essary to return coordinate to the position inter-vened at program restart. I...

  • Page 399

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01378Meaning of parameterParameter No.AIadvancedpreviewAdvancedpreviewcontrolNormalAllowable feedrate difference (controlled by feedrate difference)1780–Allowable feedrate difference for eachaxis (controlled by feedrate difference)1783(3) Fe...

  • Page 400

    PROGRAMMINGB–63614EN/0119. HIGH SPEED CUTTINGFUNCTIONS379NoMessageContents5110IMPROPER G–CODE(G05.1 Q1 MODE)A G–code which can not be used in the AIadvanced preview control mode is specified.5111IMPROPER MODALG–CODE (G05.1 Q1)When the AI advanced preview control modeis specified, a modal ...

  • Page 401

    PROGRAMMING19. HIGH SPEED CUTTINGFUNCTIONSB–63614EN/01380NOTE1 When this function is used, the option of the AI advancedpreview control is needed. And when there is the AIadvanced preview control option, it is possible to specify thelook–ahead control (G08 P1).2 The deceleration of the axis i...

  • Page 402

    PROGRAMMINGB–63614EN/0120. AXIS CONTROL FUNCTIONS38120 AXIS CONTROL FUNCTIONS

  • Page 403

    PROGRAMMING20. AXIS CONTROL FUNCTIONSB–63614EN/01382It is possible to change the operating mode for two or more specified axesto either synchronous operation or normal operation by an input signalfrom the machine.Synchronous control can be performed for up to four pairs of axes withthe Series 1...

  • Page 404

    PROGRAMMINGB–63614EN/0120. AXIS CONTROL FUNCTIONS383This operating mode is used for machining different workpieces on eachtable. The operation is the same as in ordinary CNC control, where themovement of the master axis and slave axis is controlled by theindependent axis address (Y and V). It...

  • Page 405

    PROGRAMMING20. AXIS CONTROL FUNCTIONSB–63614EN/01384In synchronous axis control, commands that require no axis motion, suchas the workpiece coordinate system setup command (G92) and the localcoordinate system setup command (G52), are set to the Y axis by programcommand Yyyyy issued to the maste...

  • Page 406

    PROGRAMMINGB–63614EN/0120. AXIS CONTROL FUNCTIONS385The roll–over function prevents coordinates for the rotation axis fromoverflowing. The roll–over function is enabled by setting bit 0 ofparameter ROAx 1008 to 1.For an incremental command, the tool moves the angle specified in thecommand....

  • Page 407

    III. OPERATION

  • Page 408

    OPERATIONB–63614EN/011. GENERAL3891 GENERAL

  • Page 409

    OPERATION1. GENERALB–63614EN/01390The CNC machine tool has a position used to determine the machineposition.This position is called the reference position, where the tool is replacedor the coordinate are set. Ordinarily, after the power is turned on, the toolis moved to the reference position....

  • Page 410

    OPERATIONB–63614EN/011. GENERAL391Using machine operator’s panel switches, pushbuttons, or the manualhandle, the tool can be moved along each axis.ToolWorkpieceMachine operator’s panelManualpulse generatorFig. 1.1 (b) The tool movement by manual operationThe tool can be moved in the follow...

  • Page 411

    OPERATION1. GENERALB–63614EN/01392Automatic operation is to operate the machine according to the createdprogram. It includes memory, MDI and DNC operations. (See SectionIII–4).ProgramTool01000;M_S_T;G92_X_ ;G00...;G01...... ;....Fig.1.2 (a) Tool movement by programmingAfter the program is o...

  • Page 412

    OPERATIONB–63614EN/011. GENERAL393Select the program used for the workpiece. Ordinarily, one program isprepared for one workpiece. If two or more programs are in memory,select the program to be used, by searching the program number (SectionIII–9.3).G92O1001Program numberM30G92O1002G92M30Pro...

  • Page 413

    OPERATION1. GENERALB–63614EN/01394While automatic operation is being executed, tool movement can overlapautomatic operation by rotating the manual handle.ZXProgrammeddepth of cutDepth of cut by handle interruptionTool position afterhandle interruptionTool position during automatic operationFig....

  • Page 414

    OPERATIONB–63614EN/011. GENERAL395Before machining is started, the automatic running check can beexecuted. It checks whether the created program can operate the machineas desired. This check can be accomplished by running the machineactually or viewing the position display change (without run...

  • Page 415

    OPERATION1. GENERALB–63614EN/01396When the cycle start pushbutton is pressed, the tool executes oneoperation then stops. By pressing the cycle start again, the tool executesthe next operation then stops. The program is checked in this manner.Cycle startCycle startCycle startCycle startStopSto...

  • Page 416

    OPERATIONB–63614EN/011. GENERAL397After a created program is once registered in memory, it can be correctedor modified from the MDI panel (See Section III–9).This operation can be executed using the part program storage/editfunction.Program registrationMDI CNC CNCProgram correction or modifi...

  • Page 417

    OPERATION1. GENERALB–63614EN/01398The operator can display or change a value stored in CNC internalmemory by key operation on the MDI screen (See III–11).Data settingMDIData displayScreen KeysCNC memoryFig. 1.6 (a) Displaying and setting dataTool compensationnumber1 12.3 25.0Tool co...

  • Page 418

    OPERATIONB–63614EN/011. GENERAL399Machinedshape1st tool path2nd tool pathOffset value of the 1st toolOffset value of the 2nd toolFig. 1.6 (c) Offset valueApart from parameters, there is data that is set by the operator inoperation. This data causes machine characteristics to change.For exampl...

  • Page 419

    OPERATION1. GENERALB–63614EN/01400The CNC functions have versatility in order to take action incharacteristics of various machines.For example, CNC can specify the following:S Rapid traverse rate of each axisS Whether increment system is based on metric system or inch system.S How to set comman...

  • Page 420

    OPERATIONB–63614EN/011. GENERAL401The contents of the currently active program are displayed. In addition,the programs scheduled next and the program list are displayed.(See Section III–11.2.1)PROGRAMMEM STOP * * * * * *13 : 18 : 14110000005>_PRGRMN1 G90 G17 G00 G41 D07 X250.0 Y550.0 ...

  • Page 421

    OPERATION1. GENERALB–63614EN/01402The current position of the tool is displayed with the coordinate values.The distance from the current position to the target position can also bedisplayed. (See Section III–11.1.1 to 11.1.3)YXxyWorkpiece coordinate system ACTUAL POSITION (ABSOLUTE)* * * * ...

  • Page 422

    OPERATIONB–63614EN/011. GENERAL403When this option is selected, two types of run time and number of partsare displayed on the screen. (See Section lll–11.4.5)ACTUAL POSITION (ABSOLUTE)* * * * O0003 N00003(OPRT)X 150.000Y 300.000Z 100.000MEM STRT20 : 22 : 23RUN TIME0H16M CYCLE TIME 0H 1M 0...

  • Page 423

    OPERATION1. GENERALB–63614EN/01404Programs, offset values, parameters, etc. input in CNC memory can beoutput to paper tape, cassette, or a floppy disk for saving. After onceoutput to a medium, the data can be input into CNC memory.MemoryProgramOffsetParametersReader/puncherinterfacePortable t...

  • Page 424

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES4052 OPERATIONAL DEVICESThe available operational devices include the setting and display unitattached to the CNC, the machine operator’s panel, and externalinput/output devices such as a Handy File.

  • Page 425

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01406The setting and display units are shown in Subsections 2.1.1 to 2.1.6 ofPart III.7.2”/8.4” LCD–Mounted Type CNC control unitIII–2.1.1. . . . . . . 9.5”/10.4” LCD–Mounted Type CNC control unitIII–2.1.2. . . . . . Stand–Alone type sm...

  • Page 426

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES4072.1.17.2″/8.4″ LCD–MountedType CNC Control Unit2.1.29.5″/10.4″ LCD–MountedType CNC Control Unit

  • Page 427

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01408Function keysAddress/numeric keysShift keyCancel (CAN) keyInput keyEdit keysHelp keyReset keyCursor keysPage change keys2.1.3Stand–Alone TypeSmall MDI Unit

  • Page 428

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES409Shift keyPage change keysCursor keysFunction keysInput keyCancel (CAN) keyEdit keysAddress/numeric keysReset keyHelp key2.1.4Stand–Alone TypeStandard MDI Unit

  • Page 429

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01410Page change keysHelp keyReset keyAddress/numeric keysCursor keysShift keyFunction keysEdit keysCancel (CAN) keyInput key2.1.5Stand–Alone Type 61Full–Key MDI Unit

  • Page 430

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES411Table 2.2 Explanation of the MDI keyboardNumberNameExplanation1RESET keyPress this key to reset the CNC, to cancel an alarm, etc.2HELP keyPress this button to use the help function when uncertain about the operation ofan MDI key (help function).In ...

  • Page 431

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01412Table 2.2 Explanation of the MDI keyboardNumberExplanationName10Cursor move keysThere are four different cursor move keys. :This key is used to move the cursor to the right or in the forwarddirection. The cursor is moved in short units in the forw...

  • Page 432

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES413The function keys are used to select the type of screen (function) to bedisplayed. When a soft key (section select soft key) is pressedimmediately after a function key, the screen (section) corresponding to theselected function can be selected.1Pre...

  • Page 433

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01414Function keys are provided to select the type of screen to be displayed.The following function keys are provided on the MDI panel:Press this key to display the position screen.Press this key to display the program screen.Press this key to display th...

  • Page 434

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES415To display a more detailed screen, press a function key followed by a softkey. Soft keys are also used for actual operations.The following illustrates how soft key displays are changed by pressingeach function key.: Indicates a screen that can be d...

  • Page 435

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01416Monitor screen[(OPRT)][PTSPRE][EXEC][RUNPRE][EXEC][ABS]Absolute coordinate displayPOS[(OPRT)][REL](Axis or numeral)[ORIGIN][PRESET][ALLEXE](Axis name)[EXEC][PTSPRE][EXEC][RUNPRE][EXEC][ALL][HNDL][MONI]Soft key transition triggered by the function ke...

  • Page 436

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES417[ABS][(OPRT)][BG–EDT][O SRH][PRGRM]Program display screenPROGSoft key transition triggered by the function keyin the MEM modePROG[N SRH][REWIND]See “When the soft key [BG–EDT] is pressed”[(OPRT)][CHECK]Program check display screen[REL]Curren...

  • Page 437

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01418[FL.SDL][PRGRM]File directory display screen[(OPRT)][DIR][SELECT][EXEC](number)[F SET]Schedule operation display screen[(OPRT)][SCHDUL][CLEAR](Schedule data)[CAN][EXEC][INPUT]Return to(1) (Program display)(2)2/2

  • Page 438

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES4191/2[(OPRT)][BG–EDT](O number)[O SRH][PRGRM]Program displayPROG(Address)[SRH↓][REWIND](Address)[SRH↑][F SRH][CAN](N number)[EXEC][READ][CHAIN][STOP][CAN][EXEC][PUNCH][STOP][CAN][EXEC][DELETE][CAN][EXEC][EX–EDT][COPY][CRSR∼][∼CRSR][∼BTTM...

  • Page 439

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01420(1)2/2[(OPRT)][BG–EDT](O number)[O SRH][LIB]Program directory display[READ][CHAIN][STOP][CAN][EXEC][PUNCH][STOP][CAN][EXEC](O number)(O number)Return to the programSee"When the soft key [BG-EDT] is pressed"[F SRH][CAN][EXEC][READ][STOP][...

  • Page 440

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES421[(OPRT)][BG–EDT][PRGRM]Program displayPROGSoft key transition triggered by the function keyin the MDI modePROGPROGRAM SCREEN[(OPRT)][BG–EDT][MDI]Program input screen(Address)(Address)[SRH↓][SRH↑]Current block display screen[(OPRT)][BG–EDT]...

  • Page 441

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01422[(OPRT)][BG–EDT][PRGRM]Program displayPROGSoft key transition triggered by the function keyin the HNDL, JOG, or REF modePROGPROGRAM SCREENCurrent block display screen[(OPRT)][BG–EDT][CURRNT]Next block display screen[(OPRT)][BG–EDT][NEXT]Progra...

  • Page 442

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES4231/2[(OPRT)][BG–END](O number)[O SRH][PRGRM]Program displayPROG(Address)[SRH↓][REWIND](Address)[SRH↑][F SRH][CAN](N number)[EXEC][READ][CHAIN][STOP][CAN][EXEC][PUNCH][STOP][CAN][EXEC][DELETE][CAN][EXEC][EX–EDT][COPY][CRSR∼][∼CRSR][∼BTTM...

  • Page 443

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01424[(OPRT)][BG–EDT](O number)[O SRH][LIB]Program directory display[READ][CHAIN][STOP][CAN][EXEC][PUNCH][STOP][CAN][EXEC](1)(O number)(O number)[F SRH][CAN][EXEC][READ][STOP][CAN][PUNCH][F SET][F SET][EXEC][O SET][STOP][CAN][F SET][EXEC][O SET][DELETE...

  • Page 444

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES425[(OPRT)][OFFSET]Tool offset screenSoft key transition triggered by the function keyOFFSETSETTING(Number)(Axis name)(Numeral)(Numeral)[NO SRH][INP.C.][+INPUT][INPUT][(OPRT)][SETING]Setting screen(Numeral)(Numeral)[NO SRH][+INPUT][INPUT][ON:1][OFF:0][...

  • Page 445

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01426[(OPRT)][MENU]Pattern data input screen[SELECT](Number)[OPR]Software operator’s panel screen[(OPRT)][TOOLLF]Tool life management setting screen(Numeral)[NO SRH][INPUT](Number)[CAN][EXEC][CLEAR]2/2(1)

  • Page 446

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES427Soft key transition triggered by the function key[(OPRT)][PARAM]Parameter screen(Numeral)(Numeral)[NO SRH][+INPUT][INPUT][ON:1][OFF:0](Number)SYSTEMSYSTEM[READ][CAN][EXEC][PUNCH][CAN][EXEC][(OPRT)][DGNOS]Diagnosis screen[NO SRH](Number)[PMC]PMC scre...

  • Page 447

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01428[W.DGNS]Waveform diagnosis screen(4)[W.PRM][W.GRPH][STSRT][TIME→][←TIME][H–DOBL][H–HALF][STSRT][CH–1↑][V–DOBL][V–HALF][CH–1↓][STSRT][CH–2↑][V–DOBL][V–HALF][CH–2↓]2/2[(OPRT)][SV.PRM]Servo parameter screen[ON:1][OFF:0][...

  • Page 448

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES429Soft key transition triggered by the function key[ALARM]Alarm display screenMESSAGEMESSAGE[MSG]Message display screen[HISTRY]Alarm history screen[(OPRT)][CLEAR]MESSAGE SCREEN[ALAM]Soft key transition triggered by the function keyAlarm detail screenH...

  • Page 449

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01430Soft key transition triggered by the function key GRAPHGRAPHIC SCREENTool path graphics[(OPRT)][PARAM]Tool path graphicsGRAPH[EXEC][AUTO][STSRT][STOP][REWIND][CLEAR][(OPRT)][ZOOM][EXEC][←][→][↑][↓][POS]

  • Page 450

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES431When an address and a numerical key are pressed, the charactercorresponding to that key is input once into the key input buffer. Thecontents of the key input buffer is displayed at the bottom of the screen.In order to indicate that it is key input ...

  • Page 451

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01432After a character or number has been input from the MDI panel, a datacheck is executed when INPUTkey or a soft key is pressed. In the case ofincorrect input data or the wrong operation a flashing warning messagewill be displayed on the status displ...

  • Page 452

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES433There are 12 soft keys in the 10.4″LCD/MDI or 9.5″LCD/MDI. Asillustrated below, the 5 soft keys on the right and those on the right andleft edges operate in the same way as the 7.2″LCD or 8.4″ LCD, whereasthe 5 keys on the left hand side ar...

  • Page 453

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01434Five types of external input/output devices are available. This sectionoutlines each device. For details on these devices, refer to thecorresponding manuals listed below.Table 2.4 External I/O deviceDevice nameUsageMax.storagecapacityReferenceman...

  • Page 454

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES435Before an external input/output device can be used, parameters must beset as follows.CNCMOTHER BOARDOPTION–1 BOARDChannel 1Channel 2Channel 3JD5AJD5BRS–422RS–232–CRS–232–CJD5CJD6ARS–232–CReader/puncherHost computerHost computerReader...

  • Page 455

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01436The Handy File is an easy–to–use, multi function floppy diskinput/output device designed for FA equipment. By operating the HandyFile directly or remotely from a unit connected to the Handy File,programs can be transferred and edited.The Handy ...

  • Page 456

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES437An FA Card is a memory card used as an input medium in the FA field.It is a card–shaped input/output medium featuring a high reliability, smallsize, high capacity, and maintenance–free operation.When an FA Card is connected to the CNC via the ca...

  • Page 457

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01438The portable tape reader is used to input data from paper tape.}+++RS–232–C Interface(Punch panel, etc.)2.4.5Portable Tape Reader

  • Page 458

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES439Procedure of turning on the power1Check that the appearance of the CNC machine tool is normal. (For example, check that front door and rear door are closed.)2Turn on the power according to the manual issued by the machinetool builder.3After the po...

  • Page 459

    OPERATION2. OPERATIONAL DEVICESB–63614EN/01440If a hardware failure or installation error occurs, the system displays oneof the following three types of screens then stops.Information such as the type of printed circuit board installed in each slotis indicated. This information and the LED sta...

  • Page 460

    OPERATIONB–63614EN/012. OPERATIONAL DEVICES441DDH1 – 01SLOT 01 (3046) : ENDSLOT 02 (3050) :Blank: Setting not completedModule IDSlot numberEND: Setting completedDDH1 – 01CNC control softwareOMM : yyyy–yyPMC : zzzz–zzOrder–made macro/macrocompilerPMCThe software configuration ...

  • Page 461

    OPERATION3. MANUAL OPERATIONB–63614EN/014423 MANUAL OPERATIONMANUAL OPERATION are six kinds as follows :3.1 Manual reference position return3.2 Jog feed3.3 Incremental feed3.4 Manual handle feed3.5 Manual absolute on and off

  • Page 462

    OPERATIONB–63614EN/013. MANUAL OPERATION443The tool is returned to the reference position as follows :The tool is moved in the direction specified in parameter ZMI (bit 5 of No.1006) for each axis with the reference position return switch on themachine operator’s panel. The tool moves to the ...

  • Page 463

    OPERATION3. MANUAL OPERATIONB–63614EN/01444Bit 0 (ZPR) of parameter No. 1201 is used for automatically setting thecoordinate system. When ZPR is set, the coordinate system isautomatically determined when manual reference position return isperformed. When a, b and g are set in parameter 1250, ...

  • Page 464

    OPERATIONB–63614EN/013. MANUAL OPERATION445In the jog mode, pressing a feed axis and direction selection switch on themachine operator’s panel continuously moves the tool along the selectedaxis in the selected direction.The jog feedrate is specified in a parameter (No.1423)The jog feedrate ca...

  • Page 465

    OPERATION3. MANUAL OPERATIONB–63614EN/01446Feedrate, time constant and method of automatic acceleration/deceleration for manual rapid traverse are the same as G00 in programmedcommand.Changing the mode to the jog mode while pressing a feed axis anddirection selection switch does not enable jog ...

  • Page 466

    OPERATIONB–63614EN/013. MANUAL OPERATION447In the incremental (INC) mode, pressing a feed axis and directionselection switch on the machine operator’s panel moves the tool one stepalong the selected axis in the selected direction. The minimum distancethe tool is moved is the least input incr...

  • Page 467

    OPERATION3. MANUAL OPERATIONB–63614EN/01448In the handle mode, the tool can be minutely moved by rotating themanual pulse generator on the machine operator’s panel. Select the axisalong which the tool is to be moved with the handle feed axis selectionswitches.The minimum distance the tool is...

  • Page 468

    OPERATIONB–63614EN/013. MANUAL OPERATION449Parameter JHD (bit 0 of No. 7100) enables or disables the manual handlefeed in the JOG mode.When the parameter JHD( bit 0 of No. 7100) is set 1,both manual handlefeed and incremental feed are enabled.Parameter THD (bit 1 of No. 7100) enables or disable...

  • Page 469

    OPERATION3. MANUAL OPERATIONB–63614EN/01450Up to three manual pulse generators can be connected, one for each axis.The three manual pulse generators can be simultaneously operated.WARNINGRotating the handle quickly with a large magnification suchas x100 moves the tool too fast. The feedrate is...

  • Page 470

    OPERATIONB–63614EN/013. MANUAL OPERATION451Whether the distance the tool is moved by manual operation is added tothe coordinates can be selected by turning the manual absolute switch onor off on the machine operator’s panel. When the switch is turned on, thedistance the tool is moved by manu...

  • Page 471

    OPERATION3. MANUAL OPERATIONB–63614EN/01452The following describes the relation between manual operation andcoordinates when the manual absolute switch is turned on or off, using aprogram example.G01G90X200.0Y150.0X100.0Y100.0F010X300.0Y200.0;;;The subsequent figures use the following notation:...

  • Page 472

    OPERATIONB–63614EN/013. MANUAL OPERATION453Coordinates when the feed hold button is pressed while block is beingexecuted, manual operation (Y–axis +75.0) is performed, the control unitis reset with the RESET button, and block is read again(300.0 , 275.0)(200.0,150.0)(300.0 , 200.0)(150.0 , 20...

  • Page 473

    OPERATION3. MANUAL OPERATIONB–63614EN/01454When the switch is ON during cutter compensationOperation of the machine upon return to automatic operation after manualintervention with the switch is ON during execution with an absolutecommand program in the cutter compensation mode will be describe...

  • Page 474

    OPERATIONB–63614EN/013. MANUAL OPERATION455Manual operation during corneringThis is an example when manual operation is performed during cornering.VA2’, VB1’, and VB2’ are vectors moved in parallel with VA2, VB1 and VB2by the amount of manual movement. The new vectors are calculatedfr...

  • Page 475

    OPERATION3. MANUAL OPERATIONB–63614EN/01456In manual handle feed or jog feed, the following types of feed operationsare enabled in addition to the conventional feed operation along aspecified single axis (X–axis, Y–axis, Z–axis, and so forth) based onsimultaneous 1–axis control:D Feed ...

  • Page 476

    OPERATIONB–63614EN/013. MANUAL OPERATION457For jog feedThe feedrate can be overridden using the manual feedrate overridedial.The procedure above is just an example. For actual operations, referto the relevant manual provided by the machine tool builder.For feed along an axis, no straight line/...

  • Page 477

    OPERATION3. MANUAL OPERATIONB–63614EN/01458(2) Linear feed (simultaneous 2–axis control)By turning a manual handle, the tool can be moved along the straightline parallel to a specified straight line on a simultaneous 2–axiscontrol basis. This manual handle is referred to as the guidance ha...

  • Page 478

    OPERATIONB–63614EN/013. MANUAL OPERATION459FeedrateThe feedrate depends on the speed at which a manual handle is turned.A distance to be traveled by the tool (along a tangent in the case of linearor circular feed) when a manual handle is turned by one pulse can beselected using the manual handl...

  • Page 479

    OPERATION3. MANUAL OPERATIONB–63614EN/01460Even in JOG mode, manual handle feed can be enabled using bit 0 (JHD)of parameter No. 7100. In this case, however, manual handle feed isenabled only when the tool is not moved along any axis by jog feed.Never use the mirror image function when perform...

  • Page 480

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION4614 AUTOMATIC OPERATIONProgrammed operation of a CNC machine tool is referred to as automaticoperation.This chapter explains the following types of automatic operation:• MEMORY OPERATIONOperation by executing a program registered in CNC memory• MD...

  • Page 481

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01462Programs are registered in memory in advance. When one of theseprograms is selected and the cycle start switch on the machine operator’spanel is pressed, automatic operation starts, and the cycle start LED goeson.When the feed hold switch on the ...

  • Page 482

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION463b. Terminating memory operationPress the RESET key on the MDI panel. Automatic operation is terminated and the reset state is entered. When a reset is applied during movement, movement deceleratesthen stops.After memory operation is started, the fo...

  • Page 483

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01464When the optional block skip switch on the machine operator’s panel isturned on, blocks containing a slash (/) are ignored.A file (subprogram) in an external input/output device such as a FloppyCassette can be called and executed during memory ope...

  • Page 484

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION465In the MDI mode, a program consisting of up to 10 lines can be createdin the same format as normal programs and executed from the MDI panel.MDI operation is used for simple test operations.The following procedure is given as an example. For actual ...

  • Page 485

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/014665To execute a program, set the cursor on the head of the program. (Startfrom an intermediate point is possible.) Push Cycle Start button onthe operator’s panel. By this action, the prepared program will start.(For the two–path control, sele...

  • Page 486

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION467The previous explanation of how to execute and stop memory operationalso applies to MDI operation, except that in MDI operation, M30 doesnot return control to the beginning of the program (M99 performs thisfunction).Programs prepared in the MDI mode...

  • Page 487

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01468When the custom macro option is provided, macro programs can also becreated, called, and executed in the MDI mode. However, macro callcommands cannot be executed when the mode is changed to MDI modeafter memory operation is stopped during execution ...

  • Page 488

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION469By activating automatic operation during the DNC operation mode(RMT), it is possible to perform machining (DNC operation) while aprogram is being read in via reader/puncher interface, or remote buffer.If the floppy cassette directory display option ...

  • Page 489

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01470PROGRAMO0001 N00020N020 X100.0 Z100.0 (DNC–PROG) ;N030X200.0Z200.0 ;N040X300.0 Z300.0 ;N050X400.0 Z400.0 ;N060 X500.0 Z500.0 ;N070 X600.0 Z600.0 ;N080 X700.0 Z400.0 ;N090 X800.0 Z400.0 ;N100 x900.0 z400.0 ;N110 x1000.0 z1000.0 ;N120 x800.0 z800.0 ...

  • Page 490

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION471In program display, no more than 256 characters can be displayed.Accordingly, character display may be truncated in the middle of a block.In DNC operation, M198 cannot be executed. If M198 is executed, P/Salarm No. 210 is issued.In DNC operation, c...

  • Page 491

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01472This function specifies Sequence No. of a block to be restarted when a toolis broken down or when it is desired to restart machining operation aftera day off, and restarts the machining operation from that block. It can alsobe used as a high–spe...

  • Page 492

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION473Procedure for Program Restart by Specifying a Sequence Number1Retract the tool and replace it with a new one. When necessary,change the offset. (Go to step 2.)1When power is turned ON or emergency stop is released, perform allnecessary operations ...

  • Page 493

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/014745 The sequence number is searched for, and the program restart screenappears on the CRT display.PROGRAM RESTARTDESTINATIONX 57. 096Y 56. 877Z 56. 943M12121212121* * * * * * * ** * * * * * * ** * * * * * * *T* * * * * * * ** * * * * * * *S * * * * *...

  • Page 494

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION475Procedure for Program Restart by Specifying a Block Number1Retract the tool and replace it with a new one. When necessary,change the offset. (Go to step 2.)1When power is turned ON or emergency stop is released, perform allnecessary operations at ...

  • Page 495

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01476The coordinates and amount of travel for restarting the program canbe displayed for up to five axes. If your system supports six or moreaxes, pressing the [RSTR] soft key again displays the data for thesixth and subsequent axes. (The program resta...

  • Page 496

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION477< Example 2 >CNC ProgramNumber of blocksO 0001 ;G90 G92 X0 Y0 Z0 ;G90 G00 Z100. ;G81 X100. Y0. Z–120. R–80. F50. ;#1 = #1 + 1 ;#2 = #2 + 1 ;#3 = #3 + 1 ;G00 X0 Z0 ;M30 ;123444456Macro statements are not counted as blocks.The block number i...

  • Page 497

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01478When single block operation is ON during movement to the restartposition, operation stops every time the tool completes movement alongan axis. When operation is stopped in the single block mode, MDIintervention cannot be performed.During movement t...

  • Page 498

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION479The schedule function allows the operator to select files (programs)registered on a floppy–disk in an external input/output device (HandyFile, Floppy Cassette, or FA Card) and specify the execution order andnumber of repetitions (scheduling) for p...

  • Page 499

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01480Procedure for Scheduling Function1Press the MEMORY switch on the machine operator’s panel, thenpress the PROG function key on the MDI panel.2Press the rightmost soft key (continuous menu key), then press the[FL. SDL] soft key. A list of files reg...

  • Page 500

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION4814Press the REMOTE switch on the machine operator’s panel to enterthe RMT mode, then press the cycle start switch. The selected file isexecuted. For details on the REMOTE switch, refer to the manualsupplied by the machine tool builder. The selec...

  • Page 501

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01482Move the cursor and enter the file numbers and number of repetitionsin the order in which to execute the files. At this time, the currentnumber of repetitions “CUR.REP” is 0.5Press the REMOTE switch on the machine operator’s panel to enterthe ...

  • Page 502

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION483During the execution of file, the floppy directory display of backgroundediting cannot be referenced.To resume automatic operation after it is suspended for scheduledoperation, press the reset button.Alarm No.Description086An attempt was made to exe...

  • Page 503

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01484The subprogram call function is provided to call and execute subprogramfiles stored in an external input/output device(Handy File, FLOPPYCASSETTE, FA Card)during memory operation.When the following block in a program in CNC memory is executed, asubp...

  • Page 504

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION485NOTE1 When M198 in the program of the file saved in a floppycassette is executed, a P/S alarm (No.210) is given. Whena program in the memory of CNC is called and M198 isexecuted during execution of a program of the file saved ina floppy cassette, M...

  • Page 505

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01486The movement by manual handle operation can be done by overlappingit with the movement by automatic operation in the automatic operationmode.ZXProgrammed depth of cutDepth of cut by handle interruptionTool position afterhandle interruptionTool posit...

  • Page 506

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION487The following table indicates the relation between other functions and themovement by handle interrupt.DisplayRelationMachine lockMachine lock is effective. The tool does not moveeven when this signal turns on.InterlockInterlock is effective. Th...

  • Page 507

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01488(a) INPUT UNIT: Handle interrupt move amount in input unitsystem Indicates the travel distance specified by handleinterruption according to the least inputincrement.(b) OUTPUT UNI : Handle interrupt move amount in output unitsystem Indicates the tra...

  • Page 508

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION489During automatic operation, the mirror image function can be used formovement along an axis. To use this function, set the mirror image switchto ON on the machine operator’s panel, or set the mirror image setting toON from the MDI panel.YXY–axis...

  • Page 509

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/014902–4 Move the cursor to the mirror image setting position, then set thetarget axis to 1.3Enter an automatic operation mode (memory mode or MDI mode),then press the cycle start button to start automatic operation.D The mirror image function can also...

  • Page 510

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION491In cases such as when tool movement along an axis is stopped by feed holdduring automatic operation so that manual intervention can be used toreplace the tool: When automatic operation is restarted, this functionreturns the tool to the position whe...

  • Page 511

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01492N1N2N1 Point AN2N1 Point AN2Point BN1 Point AN2B1. The N1 block cuts a workpieceToolBlock start point2. The tool is stopped by pressing the feed hold switch inthe middle of the N1 block (point A).3. After retracting the tool manually to point ...

  • Page 512

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION493“DNC operation with Memory Card” is a function that it is possible toperform machining with executing the program in the memory card,which is assembled to the memory card interface, where is the left sideof the screen.There are two methods to us...

  • Page 513

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01494NOTE1 To use this function, it is necessary to set the I/O channel(the parameter of No.20) to 4 by setting screen. No.20 [I/O CHANEL: Setting to select an input/output unit]Setting value is 4.: It means using the memory cardinterface.2 When CNC co...

  • Page 514

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION495When the following block in a program in CNC memory is executed, asubprogram file in memory card is called.1. Normal formatM198 Pffff ∆∆∆∆ ;File number for a file inthe memory cardNumber of repetitionMemory card call instruction2. FS15 tap...

  • Page 515

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/01496(1) The memory card can not be accessed, such as display of memory cardlist and so on, during the DNC operation with memory card.(2) It is possible to execute the DNC operation with memory card on multipath system. However, it is not possible to ca...

  • Page 516

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION497SpecificationRemarksA02B–0236–K160For 7.2″ LCD or 8.4″ LCDA02B–0236–K161For 9.5″ LCD or 10.4″ LCD1) How to assemble to the unitAssemble an attachment guide and a control unit to the cabinet byscrewing together as follow figure.The at...

  • Page 517

    OPERATION4. AUTOMATIC OPERATIONB–63614EN/014982) How to mount the card(a) Insert the card to slit of the attachment. Please pay attention to thedirection of the card. (Please mach the direction of ditch on thecard.)(b) Push up the card to the upper end of the attachment.3) Assembling of the a...

  • Page 518

    OPERATIONB–63614EN/014. AUTOMATIC OPERATION4994) Appearance after connectionNOTE1 In both case of stand–alone type i series and LCD mountedtype i series, the memory card interface where is the left sideof the screen of the display unit. (The memory card interfaceon the stand–alone type con...

  • Page 519

    OPERATION5. TEST OPERATIONB–63614EN/015005 TEST OPERATIONThe following functions are used to check before actual machiningwhether the machine operates as specified by the created program.5.1 Machine Lock and Auxiliary Function Lock5.2 Feedrate Override5.3 Rapid Traverse Override5.4 Dry Run5.5 S...

  • Page 520

    OPERATIONB–63614EN/015. TEST OPERATION501To display the change in the position without moving the tool, usemachine lock.There are two types of machine lock: all–axis machine lock, which stopsthe movement along all axes, and specified–axis machine lock, whichstops the movement along specifi...

  • Page 521

    OPERATION5. TEST OPERATIONB–63614EN/01502M, S, T and B commands are executed in the machine lock state.When a G27, G28, or G30 command is issued in the machine lock state,the command is accepted but the tool does not move to the referenceposition and the reference position return LED does not g...

  • Page 522

    OPERATIONB–63614EN/015. TEST OPERATION503A programmed feedrate can be reduced or increased by a percentage (%)selected by the override dial.This feature is used to check a program.For example, when a feedrate of 100 mm/min is specified in the program,setting the override dial to 50% moves the t...

  • Page 523

    OPERATION5. TEST OPERATIONB–63614EN/01504An override of four steps (F0, 25%, 50%, and 100%) can be applied to therapid traverse rate. F0 is set by a parameter (No. 1421).ÇÇÇÇÇÇÇÇÇÇÇÇRapid traverserate10m/minOverride50%5m/minFig. 5.3 Rapid traverse overrideRapid Traverse OverrideSel...

  • Page 524

    OPERATIONB–63614EN/015. TEST OPERATION505The tool is moved at the feedrate specified by a parameter regardless ofthe feedrate specified in the program. This function is used for checkingthe movement of the tool under the state taht the workpiece is removedfrom the table.ToolTableFig. 5.4 Dry r...

  • Page 525

    OPERATION5. TEST OPERATIONB–63614EN/01506Pressing the single block switch starts the single block mode. When thecycle start button is pressed in the single block mode, the tool stops aftera single block in the program is executed. Check the program in the singleblock mode by executing the pro...

  • Page 526

    OPERATIONB–63614EN/015. TEST OPERATION507If G28 to G30 are issued, the single block function is effective at theintermediate point.In a canned cycle, the single block stop points are the end of , , and shown below. When the single block stop is made after the point or , the feed hold LED light...

  • Page 527

    OPERATION6. SAFETY FUNCTIONSB–63614EN/015086 SAFETY FUNCTIONSTo immediately stop the machine for safety, press the Emergency stopbutton. To prevent the tool from exceeding the stroke ends, Overtravelcheck and Stroke check are available. This chapter describes emergencystop., overtravel check,...

  • Page 528

    OPERATIONB–63614EN/016. SAFETY FUNCTIONS509If you press Emergency Stop button on the machine operator’s panel, themachine movement stops in a moment.EMERGENCY STOPRedFig. 6.1 Emergency stopThis button is locked when it is pressed. Although it varies with themachine tool builder, the button c...

  • Page 529

    OPERATION6. SAFETY FUNCTIONSB–63614EN/01510When the tool tries to move beyond the stroke end set by the machine toollimit switch, the tool decelerates and stops because of working the limitswitch and an OVER TRAVEL is displayed.YXDeceleration and stopStroke endLimit switchFig. 6.2 OvertravelWhe...

  • Page 530

    OPERATIONB–63614EN/016. SAFETY FUNCTIONS511Three areas which the tool cannot enter can be specified with stored strokecheck 1, stored stroke check 2, and stored stroke check 3.ÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇ...

  • Page 531

    OPERATION6. SAFETY FUNCTIONSB–63614EN/01512(I,J,K)ÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇ(X,Y,Z)X>I, Y>J, Z>KX–I >ζ (In least command increment)Y–J >ζ (In least command increment)Z–K >ζ ((In least command increment)G 22X_Y_Z_I_J_K_;ζ (mm)=750...

  • Page 532

    OPERATIONB–63614EN/016. SAFETY FUNCTIONS513ÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇABabThe position of thetool after referenceposition returnArea boundaryFig. 6.3 (d) Setting the forbidden areaArea can be set in piles.ÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇ...

  • Page 533

    OPERATION6. SAFETY FUNCTIONSB–63614EN/01514When G23 is switched to G22 in the forbidden area, the following results.(1) When the forbidden area is inside, an alarm is informed in the nextmove.(2) When the forbidden area is outside, an alarm is informed immediately.Parameter BFA (bit 7 of No. 13...

  • Page 534

    OPERATIONB–63614EN/017. ALARM AND SELF–DIAGNOSISFUNCTIONS5157 ALARM AND SELF–DIAGNOSIS FUNCTIONSWhen an alarm occurs, the corresponding alarm screen appears to indicatethe cause of the alarm. The causes of alarms are classified by alarmnumbers. Up to 25 previous alarms can be stored and d...

  • Page 535

    OPERATION7. ALARM AND SELF–DIAGNOSIS FUNCTIONSB–63614EN/01516When an alarm occurs, the alarm screen appears.ARALMALARM MESSAGEMDI* * * * * * * * * *18 : 52 : 05000000000100PARAMETER WRITE ENABLE510OVER TR1AVEL :+X417SERVO ALARM :X AXIS DGTL PARAM417SERVO ALARM :X AXIS DGTL PARAMMSGHI...

  • Page 536

    OPERATIONB–63614EN/017. ALARM AND SELF–DIAGNOSISFUNCTIONS517Alarm numbers and messages indicate the cause of an alarm. To recoverfrom an alarm, eliminate the cause and press the reset key.The error codes are classified as follows:No. 000 to 255: P/S alarm (Program errors) (*)No. 300 to 349: ...

  • Page 537

    OPERATION7. ALARM AND SELF–DIAGNOSIS FUNCTIONSB–63614EN/01518Up to 25 of the most recent CNC alarms are stored and displayed on thescreen.Display the alarm history as follows:Procedure for Alarm History Display1 Press the function key MESSAGE .2Press the chapter selection soft key [HISTRY]...

  • Page 538

    OPERATIONB–63614EN/017. ALARM AND SELF–DIAGNOSISFUNCTIONS519The system may sometimes seem to be at a halt, although no alarm hasoccurred. In this case, the system may be performing some processing.The state of the system can be checked by displaying the self–diagnosticscreen.Procedure for ...

  • Page 539

    OPERATION7. ALARM AND SELF–DIAGNOSIS FUNCTIONSB–63614EN/01520Diagnostic numbers 000 to 015 indicate states when a command is beingspecified but appears as if it were not being executed. The table belowlists the internal states when 1 is displayed at the right end of each line onthe screen....

  • Page 540

    OPERATIONB–63614EN/017. ALARM AND SELF–DIAGNOSISFUNCTIONS521The table below shows the signals and states which are enabled when eachdiagnostic data item is 1. Each combination of the values of the diagnosticdata indicates a unique state.0200210220230240251111111111111100000000000000000000000...

  • Page 541

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/015228 DATA INPUT/OUTPUTNC data is transferred between the NC and external input/output devicessuch as the Handy File. Information can be read into the CNC from a memory card and writtenfrom the CNC to the memory card, using the memory card interface at t...

  • Page 542

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT523Of the external input/output devices, the FANUC Handy File use floppydisks as their input/output medium.In this manual, these input/output medium is generally referred to as afloppy.Unlike an NC tape, a floppy allows the user to freely choose from sev...

  • Page 543

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01524The floppy is provided with the write protect switch. Set the switch tothe write enable state. Then, start output operation.(2) Write–enabled (Reading, writing, and deletion are possible.)Write protect switch of a cassette(1) Write–protected(Only...

  • Page 544

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT525When the program is input from the floppy, the file to be input firstmust be searched.For this purpose, proceed as follows:File 1File searching of the file nFile nBlankFile 2File 3File heading1 Press the EDIT or MEMORY switch on the machine operator...

  • Page 545

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01526Alarm No.Description86The ready signal (DR) of an input/output device is off.An alarm is not immediately indicated in the CNC even when analarm occurs during head searching (when a file is not found, orthe like).An alarm is given when the input/output...

  • Page 546

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT527Files stored on a floppy can be deleted file by file as required.File deletion1Insert the floppy into the input/output device so that it is ready forwriting.2Press the EDIT switch on the machine operator’s panel.3Press function key PROG, then the pr...

  • Page 547

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01528This section describes how to load a program into the CNC from a floppyor NC tape.Inputting a program1Make sure the input device is ready for reading.For the two–path control, select the tool post for which a program tobe input is used with the tool...

  • Page 548

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT529• When a program is entered without specifying a program number.⋅ The O–number of the program on the NC tape is assigned to theprogram. If the program has no O–number, the N–number in the first block isassigned to the program.⋅ When the p...

  • Page 549

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01530S Pressing the [CHAIN] soft key positions the cursor to the end of theregistered program. Once a program has been input, the cursor ispositioned to the start of the new program.S Additional input is possible only when a program has already beenregist...

  • Page 550

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT531A program stored in the memory of the CNC unit is output to a floppy orNC tape.Outputting a program1Make sure the output device is ready for output.2To output to an NC tape, specify the punch code system (ISO or EIA)using a parameter.3Press the EDIT s...

  • Page 551

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01532Punch operation can be performed in the same way as in the foreground.This function alone can punch out a program selected for foregroundoperation.<O> (Program No.) [PUNCH] [EXEC]: Punches out a specified program.<O> H–9999I [PUNCH] [EXE...

  • Page 552

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT533Offset data is loaded into the memory of the CNC from a floppy or NCtape. The input format is the same as for offset value output. See III– 8.5.2.When an offset value is loaded which has the same offset number as anoffset number already registered i...

  • Page 553

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01534All offset data is output in a output format from the memory of the CNCto a floppy or NC tape.Outputting offset data1Make sure the output device is ready for output.2Specify the punch code system (ISO or EIA) using a parameter.3Press the EDIT switch o...

  • Page 554

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT535Parameters and pitch error compensation data are input and output fromdifferent screens, respectively. This chapter describes how to enter them.Parameters are loaded into the memory of the CNC unit from a floppy orNC tape. The input format is the sam...

  • Page 555

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/0153615Turn the power to the CNC back on.16Release the EMERGENCY STOP button on the machine operator’spanel.All parameters are output in the defined format from the memory of theCNC to a floppy or NC tape.Outputting parameters1Make sure the output device...

  • Page 556

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT537Pitch error compensation data are loaded into the memory of the CNCfrom a floppy or NC tape. The input format is the same as the outputformat. See III–8.6.4. When a pitch error compensation data is loadedwhich has the corresponding data number as...

  • Page 557

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01538All pitch error compensation data are output in the defined format fromthe memory of the CNC to a floppy or NC tape.Outputting Pitch Error Compensation Data1Make sure the output device is ready for output.For the two–path control, select the tool po...

  • Page 558

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT539The value of a custom macro common variable (#500 to #999) is loadedinto the memory of the CNC from a floppy or NC tape. The same formatused to output custom macro common variables is used for input. SeeIII–8.7.2. For a custom macro common variab...

  • Page 559

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01540Custom macro common variables (#500 to #999) stored in the memoryof the CNC can be output in the defined output format to a floppy or NCtape.Outputting custom macro common variable1Make sure the output device is ready for output.2Specify the punch cod...

  • Page 560

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT541On the floppy directory display screen, a directory of the FANUC HandyFile, FANUC Floppy Cassette, or FANUC FA Card files can be displayed.In addition, those files can be loaded, output, and deleted. O0001 N00000 (METER) VOLEDIT * * * * * * * ...

  • Page 561

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01542Displaying the directory of floppy cassette filesUse the following procedure to display a directory of all thefiles stored in a floppy:1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (nex...

  • Page 562

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT543Use the following procedure to display a directory of filesstarting with a specified file number :1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key(next–menu key).4Press soft key [FLOPPY]...

  • Page 563

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01544NO :Displays the file numberFILE NAME: Displays the file name.(METER): Converts and prints out the file capacity to paper tapelength.You can also produce H(FEET)I by setting the INPUT UNIT to INCH of the setting data.VOL.: When the file is multi–vol...

  • Page 564

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT545The contents of the specified file number are read to the memory of NC.Reading files1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (next–menu key).4Press soft key [FLOPPY].5Press soft ...

  • Page 565

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01546Any program in the memory of the CNC unit can be output to a floppyas a file.Outputting programs1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key(next–menu key).4Press soft key [FLOPPY].5...

  • Page 566

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT547The file with the specified file number is deleted.Deleting files1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (next–menu key).4Press soft key [FLOPPY].5Press soft key [(OPRT)].6Pres...

  • Page 567

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01548If [F SET] or [O SET] is pressed without key inputting file number andprogram number, file number or program number shows blank. When0 is entered for file numbers or program numbers, 1 is displayed.To use channel 0 ,set a device number in parameter...

  • Page 568

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT549CNC programs stored in memory can be grouped according to theirnames, thus enabling the output of CNC programs in group units. SectionIII–11.3.3 explains the display of a program listing for a specified group.Procedure for Outputting a Program List...

  • Page 569

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01550To input/output a particular type of data, the corresponding screen isusually selected. For example, the parameter screen is used for parameterinput from or output to an external input/output unit, while the programscreen is used for program input or...

  • Page 570

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT551Input/output–related parameters can be set on the ALL IO screen.Parameters can be set, regardless of the mode. Setting input/output–related parameters1Press function key SYSTEM.2Press the rightmost soft key (next–menu key) several times.3Pre...

  • Page 571

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01552A program can be input and output using the ALL IO screen.When entering a program using a cassette or card, the user must specifythe input file containing the program (file search).File search1Press soft key [PRGRM] on the ALL IO screen, described in ...

  • Page 572

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT5536Press soft keys [F SRH] and [EXEC]. The specified file is found.When a file already exists in a cassette or card, specifying N0 or N1 hasthe same effect. If N1 is specified when there is no file on the cassette orcard, an alarm is issued because the...

  • Page 573

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01554Inputting a program1Press soft key [PRGRM] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode. A program directory is displayed.3Press soft key [(OPRT)]. The screen and soft keys change as shownbelow.⋅ A program directory is ...

  • Page 574

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT555Outputting programs1Press soft key [PRGRM] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode. A program directory is displayed.3Press soft key [(OPRT)]. The screen and soft keys change as shownbelow.⋅ A program directory is ...

  • Page 575

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01556Deleting files1Press soft key [PRGRM] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode. A program directory is displayed.3Press soft key [(OPRT)]. The screen and soft keys change as shownbelow.⋅ A program directory is displ...

  • Page 576

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT557Parameters can be input and output using the ALL IO screen.Inputting parameters1Press soft key [PARAM] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode.3Press soft key [(OPRT)]. The screen and soft keys change as shownbelow.RE...

  • Page 577

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01558Outputting parameters1Press soft key [PARAM] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode.3Press soft key [(OPRT)]. The screen and soft keys change as shownbelow.READ/PUNCH (PARAMETER)O1234 N12345MDI * * * * * * * *...

  • Page 578

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT559Offset data can be input and output using the ALL IO screen.Inputting offset data1Press soft key [OFFSET] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode.3Press soft key [(OPRT)]. The screen and soft keys change as shownbelow...

  • Page 579

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01560Outputting offset data1Press soft key [OFFSET] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode.3Press soft key [(OPRT)]. The screen and soft keys change as shownbelow.READ/PUNCH (OFFSET)O1234 N12345MDI * * * * * * * * ...

  • Page 580

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT561Custom macro common variables can be output using the ALL IO screen.Outputting custom macro common variables1Press soft key [MACRO] on the ALL IO screen, described in SectionIII–8.10.1.2Select EDIT mode.3Press soft key [(OPRT)]. The screen and soft...

  • Page 581

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01562The ALL IO screen supports the display of a directory of floppy files, aswell as the input and output of floppy files.Displaying a file directory1Press the rightmost soft key (next–menu key) on the ALL IOscreen, described in Section III–8.10.1.2P...

  • Page 582

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT563READ/PUNCH (FLOPPY) No.FILE NAMEO1234 N12345(Meter) VOLEDIT * * * * * * * * * * * * *12:34:56F SRHEXEC0001PARAMETER0002ALL.PROGRAM0003O00010004O00020005O00030006O00040007O00050008O00100009O0020F SRHFile No.=2>2_CAN46.112.311.911.911.911...

  • Page 583

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01564Inputting a file1Press the rightmost soft key (next–menu key) on the ALL IOscreen, described in Section III–8.10.1.2Press soft key [FLOPPY].3Select EDIT mode. The floppy screen is displayed.4Press soft key [(OPRT)]. The screen and soft keys cha...

  • Page 584

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT565Outputting a file1Press the rightmost soft key (next–menu key) on the ALL IOscreen, described in Section III–8.10.1.2Press soft key [FLOPPY].3Select EDIT mode. The floppy screen is displayed.4Press soft key [(OPRT)]. The screen and soft keys ch...

  • Page 585

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01566Deleting a file1Press the rightmost soft key (next–menu key) on the ALL IOscreen, described in Section III–8.10.1.2Press soft key [FLOPPY].3Select EDIT mode. The floppy screen is displayed.4Press soft key [(OPRT)]. The screen and soft keys chan...

  • Page 586

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT567Data held in CNC memory can be saved to a memory card in MS–DOSformat. Data held on a memory card can be loaded into CNC memory.A save or load operation can be performed using soft keys while the CNCis operating.Loading can be performed in either o...

  • Page 587

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01568Data held in CNC memory can be saved to a memory card in MS–DOSformat.Saving memory data1Press the rightmost soft key (next–menu key) on the ALL IOscreen, described in Section 8.10.1.2Press soft key [M–CARD].3Place the CNC in the emergency stop...

  • Page 588

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT569The file name used for save operation is determined by the amount ofSRAM mounted in the CNC. The file to be saved is divided into 512 KBblocks.SRAM fileAmount of SRAM256KB512KB1.0MB2.0MB3.0MBNumber of files123456SRAM256A.FDBSRAM0_5A.FDBSRAM1_0A.FDBSR...

  • Page 589

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01570CNC memory data that has been saved to a memory card can be loaded(restored) back into CNC memory.CNC memory data can be loaded in either of two ways. In the firstmethod, all saved memory data is loaded. In the second method, onlyselected data is lo...

  • Page 590

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT57110Upon the completion of loading, the message ”COMPLETED” isdisplayed in the message field, with the message ”PRESS RESETKEY.” displayed on the second line.11Press the RESET key. The messages are cleared from the screen.To cancel file load pr...

  • Page 591

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01572Before a file can be saved to a memory card, the memory card must beformatted.Formatting a memory card1Press the rightmost soft key (next–menu key) on the ALL IOscreen, described in Section III–8.10.1.2Press soft key [M–CARD].3Place the CNC in ...

  • Page 592

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT573Unnecessary saved files can be deleted from a memory card.Deleting files1Press the rightmost soft key (next–menu key) on the ALL IOscreen, described in Section III–8.10.1.2Press soft key [M–CARD].3Place the CNC in the emergency stop state.4When...

  • Page 593

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01574MessageDescriptionINSERT MEMORY CARD.No memory card is inserted.UNUSABLE MEMORY CARDThe memory card does not contain device information.FORMAT MEMORY CARD.The memory card is not formatted. Format the memory card before use.THE FILE IS UNUSABLE.The fo...

  • Page 594

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT575CodeMeaning99A portion that precedes the FAT area on the memory card isdisrupted.102The memory card does not have sufficient free space.105No memory card is mounted.106A memory card is already mounted.110The specified directory cannot be found.111Ther...

  • Page 595

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01576Setting the I/O channel (parameter No. 20) to 4 enables files on a memorycard inserted in the memory card interface beside the indicator to bereferenced. It also enables different types of data such as part programs,parameters, and offset data to be ...

  • Page 596

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT577Displaying a directory of stored files1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (continuous–menu key).4Press soft key [CARD]. The screen shown below is displayed. Usingpage key...

  • Page 597

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01578Searching for a file1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (continuous–menu key).4Press soft key [CARD]. The screen shown below is displayed.PROG(OPRT)DIR +DIRECTORY (M–CA...

  • Page 598

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT579Reading a file1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (continuous–menu key).4Press soft key [CARD]. Then, the screen shown below is displayed.PROG(OPRT)DIR +DIRECTORY (M...

  • Page 599

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/015808To specify a file with its file name, press soft key [N READ] in step 6above. The screen shown below is displayed.F NAMEEXECSTOPO SETCANDIRECTORY (M–CARD) No.FILE NAMECOMMENTO0001 N000100012O0050(MAIN PROGRAM)0013 TESTPRO(SUB PROGRAM–1)0014O00...

  • Page 600

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT581Writing a file1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (continuous–menu key).4Press soft key [CARD]. The screen shown below is displayed.PROG(OPRT)DIR +DIRECTORY (M–CARD) N...

  • Page 601

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01582When a file having the same name is already registered in the memorycard, the existing file will be overwritten.To write all programs, set program number = –9999. If no file name isspecified in this case, file name PROGRAM.ALL is used for registrat...

  • Page 602

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT583Deleting a file1Press the EDIT switch on the machine operator’s panel.2Press function key PROG.3Press the rightmost soft key (continuous–menu key).4Press soft key [CARD]. The screen shown below is displayed.PROG(OPRT)DIR +DIRECTORY (M–CARD) ...

  • Page 603

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01584Batch input/output with a memory cardOn the ALL IO screen, different types of data including part programs,parameters, offset data, pitch error data, custom macros, and workpiececoordinate system data can be input and output using a memory card; thesc...

  • Page 604

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT585When this screen is displayed, the program data item is selected. The softkeys for other screens are displayed by pressing the rightmost soft key (continuous–menu key). Soft key [M–CARD] represents a separatememory card function for saving and r...

  • Page 605

    OPERATION8. DATA INPUT/OUTPUTB–63614EN/01586File format and error messagesAll files that are read from and written to a memory card are of text format.The format is described below.A file starts with % or LF, followed by the actual data. A file always endswith %. In a read operation, data bet...

  • Page 606

    OPERATIONB–63614EN/018. DATA INPUT/OUTPUT587CodeMeaning99A portion that precedes the FAT area on the memory card isdisrupted.102The memory card does not have sufficient free space.105No memory card is mounted.106A memory card is already mounted.110The specified directory cannot be found.111Ther...

  • Page 607

    OPERATION9. EDITING PROGRAMSB–63614EN/015889 EDITING PROGRAMSThis chapter describes how to edit programs registered in the CNC.Editing includes the insertion, modification, deletion, and replacement ofwords. Editing also includes deletion of the entire program and automaticinsertion of sequenc...

  • Page 608

    OPERATIONB–63614EN/019. EDITING PROGRAMS589This section outlines the procedure for inserting, modifying, and deletinga word in a program registered in memory.Procedure for inserting, altering and deleting a word1Select EDIT mode.2Press PROG.3Select a program to be edited.If a program to be edit...

  • Page 609

    OPERATION9. EDITING PROGRAMSB–63614EN/01590A word can be searched for by merely moving the cursor through the text(scanning), by word search, or by address search.Procedure for scanning a program1Press the cursor key .The cursor moves forward word by word on the screen; the cursor isdisplayed a...

  • Page 610

    OPERATIONB–63614EN/019. EDITING PROGRAMS591Procedure for searching a wordExample) of Searching for S12PROGRAMO0050 N01234O0050 ;X100.0 Z1250.0 ;S12 ;N56789 M03 ;M02 ;%N01234N01234 is beingsearched for/scanned currently.S12 is searchedfor.1Key in addressS .2Key in 12 .⋅ S12 cannot be s...

  • Page 611

    OPERATION9. EDITING PROGRAMSB–63614EN/01592The cursor can be jumped to the top of a program. This function is calledheading the program pointer. This section describes the three methodsfor heading the program pointer.Procedure for Heading a Program1Press RESET when the program screen is sele...

  • Page 612

    OPERATIONB–63614EN/019. EDITING PROGRAMS593Procedure for inserting a word1Search for or scan the word immediately before a word to be inserted.2Key in an address to be inserted.3Key in data.4Press the INSERT key.Example of Inserting T151Search for or scan Z1250.ProgramO0050 N01234O0050 ;N0123...

  • Page 613

    OPERATION9. EDITING PROGRAMSB–63614EN/01594Procedure for altering a word1Search for or scan a word to be altered.2Key in an address to be inserted.3Key in data.4Press the ALTER key.Example of changing T15 to M151Search for or scan T15.ProgramO0050 N01234O0050 ;N01234 X100.0 Z1250.0S12 ;N56...

  • Page 614

    OPERATIONB–63614EN/019. EDITING PROGRAMS595Procedure for deleting a word1Search for or scan a word to be deleted.2Press the DELETE key.Example of deleting X100.01Search for or scan X100.0.ProgramO0050 N01234O0050 ;N01234S12 ;N56789 M03 ;M02 ;%X100.0X100.0 issearched for/scanned.Z1250.0 M...

  • Page 615

    OPERATION9. EDITING PROGRAMSB–63614EN/01596A block or blocks can be deleted in a program.The procedure below deletes a block up to its EOB code; the cursoradvances to the address of the next word.Procedure for deleting a block1Search for or scan address N for a block to be deleted.2Key in EOB.3...

  • Page 616

    OPERATIONB–63614EN/019. EDITING PROGRAMS597The blocks from the currently displayed word to the block with a specifiedsequence number can be deleted.Procedure for deleting multiple blocks1Search for or scan a word in the first block of a portion to be deleted.2Key in address N .3Key in the seque...

  • Page 617

    OPERATION9. EDITING PROGRAMSB–63614EN/01598When memory holds multiple programs, a program can be searched for.There are three methods as follows.Procedure for program number search1Select EDIT or MEMORY mode.2Press PROGto display the program screen.3Key in addressO .4Key in a program number to ...

  • Page 618

    OPERATIONB–63614EN/019. EDITING PROGRAMS599Sequence number search operation is usually used to search for asequence number in the middle of a program so that execution can bestarted or restarted at the block of the sequence number. Example)Sequence number 02346 in a program (O0002) issearched f...

  • Page 619

    OPERATION9. EDITING PROGRAMSB–63614EN/01600Those blocks that are skipped do not affect the CNC. This means that thedata in the skipped blocks such as coordinates and M, S, and T codes doesnot alter the CNC coordinates and modal values.So, in the first block where execution is to be started or ...

  • Page 620

    OPERATIONB–63614EN/019. EDITING PROGRAMS601Programs registered in memory can be deleted,either one program by oneprogram or all at once. Also, More than one program can be deleted byspecifying a range.A program registered in memory can be deleted.Procedure for deleting one program1Select the E...

  • Page 621

    OPERATION9. EDITING PROGRAMSB–63614EN/01602Programs within a specified range in memory are deleted.Procedure for deleting more than one program by specifying a range1Select the EDIT mode.2Press PROG to display the program screen.3Enter the range of program numbers to be deleted with address and...

  • Page 622

    OPERATIONB–63614EN/019. EDITING PROGRAMS603With the extended part program editing function, the operations describedbelow can be performed using soft keys for programs that have beenregistered in memory.Following editing operations are available :⋅ All or part of a program can be copied or mo...

  • Page 623

    OPERATION9. EDITING PROGRAMSB–63614EN/01604A new program can be created by copying a program.AOxxxxAOxxxxAfter copyAOyyyyCopyBefore copyFig. 9.6.1 Copying an entire programIn Fig. 9.6.1, the program with program number xxxx is copied to a newlycreated program with program number yyyy. The prog...

  • Page 624

    OPERATIONB–63614EN/019. EDITING PROGRAMS605A new program can be created by copying part of a program.BOxxxxOxxxxAfter copyBOyyyyCopyBefore copyFig. 9.6.2 Copying part of a programACBACIn Fig. 9.6.2, part B of the program with program number xxxx is copiedto a newly created program with program...

  • Page 625

    OPERATION9. EDITING PROGRAMSB–63614EN/01606A new program can be created by moving part of a program.BOxxxxOxxxxAfter copyBOyyyyCopyBefore copyFig. 9.6.3 Moving part of a programACACIn Fig. 9.6.3, part B of the program with program number xxxx is movedto a newly created program with program num...

  • Page 626

    OPERATIONB–63614EN/019. EDITING PROGRAMS607Another program can be inserted at an arbitrary position in the currentprogram.OxxxxBefore mergeBOyyyyMergeFig. 9.6.4 Merging a program at a specified locationAOxxxxAfter mergeBOyyyyBACCMergelocationIn Fig. 9.6.4, the program with program number XXXX ...

  • Page 627

    OPERATION9. EDITING PROGRAMSB–63614EN/01608The setting of an editing range start point with [CRSR] can be changedfreely until an editing range end point is set with [CRSR] or [BTTM].If an editing range start point is set after an editing range end point, theediting range must be reset starting ...

  • Page 628

    OPERATIONB–63614EN/019. EDITING PROGRAMS609Alarm no.Contents70101Memory became insufficient while copying or insertinga program. Copy or insertion is terminated.The power was interrupted during copying, moving, orinserting a program and memory used for editing mustbe cleared. When this alarm oc...

  • Page 629

    OPERATION9. EDITING PROGRAMSB–63614EN/01610Replace one or more specified words.Replacement can be applied to all occurrences or just one occurrence ofspecified words or addresses in the program.Procedure for hange of words or addresses1Perform steps 1 to 5 in III–9.6.1.2Press soft key [CHANGE...

  • Page 630

    OPERATIONB–63614EN/019. EDITING PROGRAMS611The following custom macro words are replaceable:IF, WHILE, GOTO, END, DO, BPRNT, DPRINT, POPEN, PCLOSThe abbreviations of custom macro words can be specified.When abbreviations are used, however, the screen displays theabbreviations as they are key in...

  • Page 631

    OPERATION9. EDITING PROGRAMSB–63614EN/01612Unlike ordinary programs, custom macro programs are modified,inserted, or deleted based on editing units.Custom macro words can be entered in abbreviated form.Comments can be entered in a program.Refer to the III–10.1 for the comments of a program.Wh...

  • Page 632

    OPERATIONB–63614EN/019. EDITING PROGRAMS613Editing a program while executing another program is called backgroundediting. The method of editing is the same as for ordinary editing(foreground editing).A program edited in the background should be registered in foregroundprogram memory by performi...

  • Page 633

    OPERATION9. EDITING PROGRAMSB–63614EN/01614The password function (bit 4 (NE9) of parameter No. 3202) can be lockedusing parameter No. 3210 (PASSWD) and parameter No. 3211(KEYWD) to protect program Nos. 9000 to 9999. In the locked state,parameter NE9 cannot be set to 0. In this state, program ...

  • Page 634

    OPERATIONB–63614EN/019. EDITING PROGRAMS615When 0 is set in the parameter PASSWD, the number 0 is displayed, andthe password function is disabled. In other words, the password functioncan be disabled by either not setting parameter PASSWD at all, or bysetting 0 in parameter PASSWD after step 3...

  • Page 635

    OPERATION10. CREATING PROGRAMSB–63614EN/0161610 CREATING PROGRAMSPrograms can be created using any of the following methods:⋅ MDI keyboard⋅ PROGRAMMING IN TEACH IN MODE⋅ CONVERSATIONAL AUTOMATIC PROGRAMMING FUNCTION⋅ AUTOMATIC PROGRAM PREPARATION DEVICE (FANUCSYSTEM P)This chapter descr...

  • Page 636

    OPERATIONB–63614EN/0110. CREATING PROGRAMS617Programs can be created in the EDIT mode using the program editingfunctions described in III–9.Procedure for Creating Programs Using the MDI Panel1Enter the EDIT mode.2Press the PROGkey.3Press address key O and enter the program number.4Press the I...

  • Page 637

    OPERATION10. CREATING PROGRAMSB–63614EN/01618Sequence numbers can be automatically inserted in each block when aprogram is created using the MDI keys in the EDIT mode.Set the increment for sequence numbers in parameter 3216.Procedure for automatic insertion of sequence numbers1Set 1 for SEQUENC...

  • Page 638

    OPERATIONB–63614EN/0110. CREATING PROGRAMS6199Press INSERT. The EOB is registered in memory and sequence numbersare automatically inserted. For example, if the initial value of N is 10and the parameter for the increment is set to 2, N12 inserted anddisplayed below the line where a new block i...

  • Page 639

    OPERATION10. CREATING PROGRAMSB–63614EN/01620When the playback option is selected, the TEACH IN JOG mode andTEACH IN HANDLE mode are added. In these modes, a machine positionalong the X, Y, and Z axes obtained by manual operation is stored inmemory as a program position to create a program.The...

  • Page 640

    OPERATIONB–63614EN/0110. CREATING PROGRAMS6211 Set the setting data SEQUENCE NO. to 1 (on). (The incremental valueparameter (No. 3216) is assumed to be “1”.)2 Select the TEACH IN HANDLE mode.3 Make positioning at position P0 by the manual pulse generator.4 Select the program screen.5 Enter...

  • Page 641

    OPERATION10. CREATING PROGRAMSB–63614EN/01622The contents of memory can be checked in the TEACH IN mode by usingthe same procedure as in EDIT mode.PROGRAMO1234 N00004(RELATIVE)(ABSOLUTE)X –6.975X 3.025Y 23.723Y 23.723Z –10.325Z –0.325O1234 ;N1 G92 X10000...

  • Page 642

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA62311 SETTING AND DISPLAYING DATATo operate a CNC machine tool, various data must be set on the MDI panelfor the CNC. The operator can monitor the state of operation with datadisplayed during operation.This chapter describes how to display an...

  • Page 643

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01624POSScreen transition triggered by the function key POSPOSITION DISPLAY SCREENCurrent position screenPosition display ofwork coordinatesystem⇒ See III-11.1.1.Display of partcount and runtime⇒ See III-11.1.6.Display of actualspeed⇒ See ...

  • Page 644

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA625Program screenDisplay of program contents⇒ See III-11.2.1.Display of currentblock and modaldata⇒ See III-11.2.2.PRGRMCHECKCURRNTNEXT(OPRT)PROGScreen transition triggered by the function keyin the MEMORY or MDI modePROGPROGRAM SCREENMEM...

  • Page 645

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01626Program editingscreen⇒ See III-9Program memoryand program directory⇒ See III-11.3.1.PRGRMLIB(OPRT)PROGEDITFLOPPY(OPRT)EDITFile directoryscreen forfloppy disks⇒ See III-8.8Program screenPROGRAM SCREENScreen transition triggered by the...

  • Page 646

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA627Software operator's panel switchåSee subsec. 11.4.10.Tool offset valueDisplay of tooloffset value⇒ See III-11.4.1.OFFSETSETTINGWORK(OPRT)Screen transition triggered by the function keyOFFSETSETTINGOFFSETSETTINGOFFSET/SETTING SCREENDispla...

  • Page 647

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01628Parameter screenPARAMDGNOSSYSTEM(OPRT)PITCH(OPRT)SYSTEMSYSTEMSYSTEM SCREENPMCDisplay ofparameter screen⇒ See III-11.5.1Setting of parameter⇒ See III-11.5.1Display ofdiagnosisscreen⇒ See III-7.3SV.PRMSP.PRMDisplay of pitcherror data⇒...

  • Page 648

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA629The table below lists the data set on each screen.Table.11. Setting screens and data on themNo.Setting screenContents of settingReferenceitem1Tool offset valueTool offset valueTool length offset valueCutter compensation valueIII–11.4.1Too...

  • Page 649

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01630Press function key POS to display the current position of the tool.The following three screens are used to display the current position of thetool:⋅Position display screen for the work coordinate system.⋅Position display screen for the ...

  • Page 650

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA631Displays the current position of the tool in the workpiece coordinatesystem. The current position changes as the tool moves. The least inputincrement is used as the unit for numeric values. The title at the top ofthe screen indicates tha...

  • Page 651

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01632Displays the current position of the tool in a relative coordinate systembased on the coordinates set by the operator. The current position changesas the tool moves. The increment system is used as the unit for numericvalues. The title a...

  • Page 652

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA633Procedure to reset all axes1Press soft key [(OPRT)].2Press soft key [ORIGIN].3Press soft key [ALLEXE].The relative coordinates for all axes are reset to 0.Bits 4 and 5 of parameter 3104 (DRL, DRC) can be used to select whetherthe displayed ...

  • Page 653

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01634Displays the following positions on a screen : Current positions of thetool in the workpiece coordinate system, relative coordinate system, andmachine coordinate system, and the remaining distance. The relativecoordinates can also be set...

  • Page 654

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA635A workpiece coordinate system shifted by an operation such as manualintervention can be preset using MDI operations to a pre–shift workpiececoordinate system. The latter coordinate system is displaced from themachine zero point by a work...

  • Page 655

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01636The actual feedrate on the machine (per minute) can be displayed on acurrent position display screen or program check screen by setting bit 0(DPF) of parameter 3105. On the 9.5″/10.4″ LCD, the actual feedrate isalways displayed.Display...

  • Page 656

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA637In the case of movement of rotary axis, the speed is displayed in units ofdeg/min but is displayed on the screen in units of input system at that time.For example, when the rotary axis moves at 50 deg/min, the following isdisplayed: 0.50 IN...

  • Page 657

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01638The run time, cycle time, and the number of machined parts are displayedon the current position display screens.Procedure for displaying run time and parts count on the current position display screen1Press function key POS to display a cur...

  • Page 658

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA639The reading on the load meter can be displayed for each servo axis andthe serial spindle by setting bit 5 (OPM) of parameter 3111 to 1. Thereading on the speedometer can also be displayed for the serial spindle.Procedure for displaying the...

  • Page 659

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01640Although the speedometer normally indicates the speed of the spindlemotor, it can also be used to indicate the speed of the spindle by settingbit 6 (OPS) of parameter 3111 to 1.The spindle speed to be displayed during operation monitoring i...

  • Page 660

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA641This section describes the screens displayed by pressing function keyPROG in MEMORY or MDI mode.The first four of the following screensdisplay the execution state for the program currently being executed inMEMORY or MDI mode and the last sc...

  • Page 661

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01642Displays the program currently being executed in MEMORY or MDImode.Procedure for displaying the program contents1Press function key PROG to display the program screen.2Press chapter selection soft key [PRGRM].The cursor is positioned at the...

  • Page 662

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA643Displays the block currently being executed and modal data in theMEMORY or MDI mode.Procedure for displaying the current block display screen1Press function key PROG.2Press chapter selection soft key [CURRNT].The block currently being execu...

  • Page 663

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01644Displays the block currently being executed and the block to be executednext in the MEMORY or MDI mode.Procedure for displaying the next block display screen1Press function key PROG.2Press chapter selection soft key [NEXT].The block current...

  • Page 664

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA645Displays the program currently being executed, current position of thetool, and modal data in the MEMORY mode.Procedure for displaying the program check screen1Press function key PROG.2Press chapter selection soft key [CHECK].The program cu...

  • Page 665

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01646The program check screen is not provided for 12 soft keys display unit.Press soft key [PRGRM] to display the contents of the program on theright half of the screen. The block currently being executed is indicatedby the cursor. The current...

  • Page 666

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA647Displays the program input from the MDI and modal data in the MDImode.Procedure for displaying the program screen for MDI operation1Press function key PROG.2Press chapter selection soft key [MDI].The program input from the MDI and modal dat...

  • Page 667

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01648This section describes the screens displayed by pressing function keyPROG in the EDIT mode. Function key PROG in the EDIT mode candisplay the program editing screen and the program list screen (displaysmemory used and a list of programs). ...

  • Page 668

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA649PROGRAM NO. USEDPROGRAM NO. USED: The number of the programs registered (including the subprograms)FREE: The number of programs which can beregistered additionally.MEMORY AREA USEDMEMORY AREA USED: The capacity of the program memory in whic...

  • Page 669

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01650 PROGRAM (NUM.)MEMORY (CHAR.) USED:603321FREE: 2 429O00013601996–06–1214:40O00022401996–06–1214:55O00104201996–07–0111:02O00201801996–08–1409:40O00401,1401996–03–2518:40O0050601996–08–2616:40O01001201996–04...

  • Page 670

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA651When no program has been deleted from the list, each program isregistered at the end of the list.If some programs in the list were deleted, then a new program isregistered, the new program is inserted in the empty location in the listcreat...

  • Page 671

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01652In addition to the normal listing of the numbers and names of CNCprograms stored in memory, programs can be listed in units of groups,according to the product to be machined, for example.To assign CNC programs to the same group, assign name...

  • Page 672

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA6538Pressing the [EXEC] operation soft key displays the group–unitprogram list screen, listing all those programs whose name includesthe specified character string. PROGRAM (NUM.)MEMORY (CHAR.) USED:603321FREE: 2 429O0020 (GEAR–1000 ...

  • Page 673

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01654[Example of using wild cards](Entered character string)(Group for which the search will be made)(a)“*”CNC programs having any name(b)“*ABC”CNC programs having names which endwith “ABC”(c)“ABC*”CNC programs having names which...

  • Page 674

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA655Press function key OFFSETSETTING to display or set tool compensation values andother data.This section describes how to display or set the following data:1. Tool offset value2. Settings3. Run time and part count4. Workpiece origin offset va...

  • Page 675

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01656Tool offset values, tool length offset values, and cutter compensationvalues are specified by D codes or H codes in a program. Compensationvalues corresponding to D codes or H codes are displayed or set on thescreen.Procedure for setting a...

  • Page 676

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA6573Move the cursor to the compensation value to be set or changed usingpage keys and cursor keys, or enter the compensation number for thecompensation value to be set or changed and press soft key[NO.SRH].4To set a compensation value, enter a...

  • Page 677

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01658OFFSETNO.DATANO.DATA 001 0.000 017 0.000 002 0.000 018 0.000 003 0.000 019 0.000 004 0.000 020 0.000 005 0.000 021 0.000 006 0.000 022 0.000 007 0.000 023 0.000 008 0.000 024 0.000 009 0.000 025 0.000 010 0.000 026 0.000 011 0.000 027 0.000...

  • Page 678

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA659The length of the tool can be measured and registered as the tool lengthoffset value by moving the reference tool and the tool to be measured untilthey touch the specified position on the machine. The tool length can be measured along the ...

  • Page 679

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/016608Press the soft key [INP.C.]. The Z axis relative coordinate value isinput and displayed as an tool length offset value.ÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇÇA prefixed positionReferencetoolThe difference is set as a toollength offset valueINP.C.

  • Page 680

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA661Data such as the TV check flag and punch code is set on the setting datascreen. On this screen, the operator can also enable/disable parameterwriting, enable/disable the automatic insertion of sequence numbers inprogram editing, and perfor...

  • Page 681

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/016624Move the cursor to the item to be changed by pressing cursor keys , , , or .5Enter a new value and press soft key [INPUT].Setting whether parameter writing is enabled or disabled.0 : Disabled1 : EnabledSetting to perform TV check.0 : ...

  • Page 682

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA663If a block containing a specified sequence number appears in the programbeing executed, operation enters single block mode after the block isexecuted.Procedure for sequence number comparison and stop1Select the MDI mode.2Press function key ...

  • Page 683

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01664After the specified sequence number is found during the execution of theprogram, the sequence number set for sequence number compensationand stop is decremented by one. When the power is turned on, the settingof the sequence number is 0.If...

  • Page 684

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA665Various run times, the total number of machined parts, number of partsrequired, and number of machined parts can be displayed. This data canbe set by parameters or on this screen (except for the total number ofmachined parts and the time d...

  • Page 685

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01666This value is incremented by one when M02, M30, or an M code specifiedby parameter 6710 is executed. The value can also be set by parameter6711. In general, this value is reset when it reaches the number of partsrequired. Refer to the ma...

  • Page 686

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA667Displays the workpiece origin offset for each workpiece coordinatesystem (G54 to G59, G54.1 P1 to G54.1 P48 and G54.1 P1 to G54.1P300) and external workpiece origin offset. The workpiece origin offsetand external workpiece origin offset ca...

  • Page 687

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01668This function is used to compensate for the difference between theprogrammed workpiece coordinate system and the actual workpiececoordinate system. The measured offset for the origin of the workpiececoordinate system can be input on the sc...

  • Page 688

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA6695To display the workpiece origin offset setting screen, press thechapter selection soft key [WORK]. NO. DATA NO. DATA 00X0.00002 X0.000 (EXT) Y0.000(G55) Y0.000 Z0.000Z0.000 01X0.00003 X0.000 (G54) Y0.000(G5...

  • Page 689

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01670Displays common variables (#100 to #149 or #100 to #199, and #500 to#531 or #500 to #999) on the screen. When the absolute value for acommon variable exceeds 99999999, ******** is displayed. The valuesfor variables can be set on this scre...

  • Page 690

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA671This subsection uses an example to describe how to display or setmachining menus (pattern menus) created by the machine tool builder.Refer to the manual issued by the machine tool builder for the actualpattern menus and pattern data. See I...

  • Page 691

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/016724Enter necessary pattern data and press INPUT.5After entering all necessary data, enter the MEMORY mode and pressthe cycle start button to start machining.HOLE PATTERN : Menu titleAn optional character string can be displayed within 12 cha...

  • Page 692

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA673With this function, functions of the switches on the machine operator’spanel can be controlled from the CRT/MDI panel.Jog feed can be performed using numeric keys.Procedure for displaying and setting the software operator’s panel1Press ...

  • Page 693

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/016744Move the cursor to the desired switch by pressing cursor key or .5Push the cursor move key or to match the markJ to anarbitrary position and set the desired condition.6On a screen where jog feed is enabled, pressing a desired arrow key,s...

  • Page 694

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA675Tool life data can be displayed to inform the operator of the current stateof tool life management. Groups which require tool changes are alsodisplayed.The tool life counter for each group can be preset to an arbitraryvalue. Tool data (ex...

  • Page 695

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/016765To display the page containing the data for a group, enter the groupnumber and press soft key [NO.SRH].The cursor can be moved to an arbitrary group by pressing cursor key or .6To change the value in the life counter for a group, move the...

  • Page 696

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA677TOOL LIFE DATA : O3000 N00060 SELECTED GROUP 000GROUP 001 :LIFE 0150 COUNT 00070034007800120056009000350026006100000000000000000000000000000000GROUP 002 :LIFE 1400 COUNT 000000620024004400740000000000...

  • Page 697

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01678The extended tool life management function provides more detailed datadisplay and more data editing functions than the ordinary tool lifemanagement function.Moreover, if the tool life is specified in units of time, the time which hasbeen se...

  • Page 698

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA679⋅ Deleting a tool group :7–4⋅ Deleting tool data (T, H, or D code) :7–5⋅ Skipping a tool :7–6⋅ Clearing the life count (resetting the life) :7–77–1Setting the life count type, life value, current life count, and tooldata (...

  • Page 699

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/016807–4Deleting a tool group(1) In step 3, position the cusor on a group to be deleted and display theediting screen.(2) Press soft key [DELETE].(3) Press soft key [GROUP].(4) Press soft key [EXEC].7–5Deleting tool data (T, H, or D code)(1)...

  • Page 700

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA681LIFE DATA EDIT GROUP : 001 O0010 N00001 TYPE: 1 (1:C 2:M)NEXT GROUP: *** LIFE: 9800USE GROUP : *** COUNT : 6501SELECTED GROUP : 001NO.STATET–CODEH–CODED–CODE01*003401100502#007800003303@001200401804*005600000005009000000006...

  • Page 701

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01682When the extended tool life management function is provided, thefollowing items are added to the tool life management screen:S NEXT: Tool group to be used nextS USE: Tool group in useS Life counter type for each tool group (C: Cycles, M:...

  • Page 702

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA683When the CNC and machine are connected, parameters must be set todetermine the specifications and functions of the machine in order to fullyutilize the characteristics of the servo motor or other parts.This chapter describes how to set para...

  • Page 703

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01684When the CNC and machine are connected, parameters are set todetermine the specifications and functions of the machine in order to fullyutilize the characteristics of the servo motor. The setting of parametersdepends on the machine. Refer...

  • Page 704

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA685Procedure for enabling/displaying parameter writing1Select the MDI mode or enter state emergency stop.2Press function key OFFSETSETTING.3Press soft key [SETING] to display the setting screen.SETTING (HANDY) O0001 N00000&g...

  • Page 705

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01686If pitch error compensation data is specified, pitch errors of each axis canbe compensated in detection unit per axis. Pitch error compensation data is set for each compensation point at theintervals specified for each axis. The origin of...

  • Page 706

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA687The bidirectional pitch error compensation function allows independentpitch error compensation in different travel directions. (When the movementis reversed, compensation is automatically carried out as in a backlash.)To use this function,...

  • Page 707

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/016882Press function key SYSTEM.3Press the continuous menu key , then press chapter selection softkey [PITCH].The following screen is displayed:PIT-ERROR SETTINGO0000 N00000NO.DATA00000000100002000030000400005000060000700008000090NO.DATA00100001...

  • Page 708

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA689The program number, sequence number, and current CNC status arealways displayed on the screen except when the power is turned on, asystem alarm occurs, or the PMC screen is displayed.If data setting or the input/output operation is incorrec...

  • Page 709

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01690The current mode, automatic operation state, alarm state, and programediting state are displayed on the next to last line on the screen allowingthe operator to readily understand the operation condition of the system.If data setting or the ...

  • Page 710

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA691––EMG––:: Indicates emergency stop.(Blinks in reversed display.)––RESET–– : Indicates that the reset signal is being received.ALM: Indicates that an alarm is issued. (Blinks in reversed display.)BAT: Indicates that the batt...

  • Page 711

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01692By pressing the function key MESSAGE, data such as alarms, alarm historydata, and external messages can be displayed.For information relating to alarm display, see Section III.7.1. Forinformation relating to alarm history display, see Sec...

  • Page 712

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA693When an external operator message number is specified, updating of theexternal operator message history data is started; this updating iscontinued until a new external operator message number is specified ordeletion of the external operator...

  • Page 713

    OPERATION11. SETTING AND DISPLAYING DATAB–63614EN/01694When screen indication isn’t necessary, the life of the back light for LCDcan be put off by turning off the back light.The screen can be cleared by pressing specific keys. It is also possible tospecify the automatic clearing of the scree...

  • Page 714

    OPERATIONB–63614EN/0111. SETTING AND DISPLAYING DATA695The CNC screen is automatically cleared if no keys are pressed during theperiod (in minutes) specified with a parameter. The screen is restored bypressing any key.Procedure for automatic erase screen displayThe CNC screen is cleared once t...

  • Page 715

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/0169612 GRAPHICS FUNCTIONTwo graphic functions are available. One is a graphic display function,and the other is a dynamic graphic display function.The graphic display function can draw the tool path specified by aprogram being executed on a screen. The...

  • Page 716

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION697It is possible to draw the programmed tool path on the screen, whichmakes it possible to check the progress of machining, while observing thepath on the screen.In addition, it is also possible to enlarge/reduce the screen.Before drawing, graphic para...

  • Page 717

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/016986Automatic operation is started and machine movement is drawn onthe screen.MEM * * * * * * * * * *14 : 23 : 03000100012GRAPHPARAMZXYS 0TX 0.000Y 0.000Z 0.000The size of the graphic screen will be as follows:Gc : Center...

  • Page 718

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION699Set the center of the graphic range to the center of the screen. If thedrawing range in the program can be contained in the above actualgraphics range, set the magnification to 1 (actual value set is 100).When the drawing range is larger than the ma...

  • Page 719

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/01700When the actual tool path is not near the center of the screen, method 1will cause the tool path to be drawn out of the geaphics range if graphicsmagnification is not set properly.To avoid such cases, the following six graphic parameters are prepared...

  • Page 720

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION701⋅ AXESSpecify the plane to use for drawing. The user can choose from thefollowing six coordinate systems.With two–path control, a different drawing coordinate system can beselected for each tool post.YZXXXXYYZZZZYY(1)(2)(3)(4)(5)(6)= 0 : Selec...

  • Page 721

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/01702⋅ GRAPHIC CENTERX=Y=Z=Set the coordinate value on the workpiece coordinate system atgraphic center.NOTE1 When MAX. and MIN. of RANGE are set, the values will beset automatically once drawing is executed2 When setting the graphics range with the gra...

  • Page 722

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION703There is the following function in Dynamic Graphics.Path graphicThis is used to draw the path of tool center com-manded by the part program.The path graphic function is used to precisely check the part program fordrawing the tool path with a line. Th...

  • Page 723

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/01704The first six functions above (1. to 6.) are available by setting the graphicparameters. The seventh to ninth functions (7. to 9.) are mainly executedusing soft keys after drawing has been setup. The tenth function (10.) isenabled by setting a par...

  • Page 724

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION7055Press the INPUT key.The input numerics are set by these operations and the cursorautomatically moves to the next setting items. The set data is held evenafter the power is turned off.6Set the operation mode to the memory mode, press function keyPRO...

  • Page 725

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/0170611For partial drawing enlargement, display the PATH GRAPHIC(SCALE) screen by pressing the soft key [ZOOM] on the PATHGRAPHIC (PARAMETER) screen of step 1 above. The tool path isdisplayed. Next, press soft key [(OPRT)].MEM * * * * * * * * * *...

  • Page 726

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION70715To display a mark at the current tool position, display the PATHGRAPHIC (POSITION) screen by pressing soft key [POS] on thePATH GRAPHIC (PARAMETER) screen of step 1 above. Thismark blinks at the current tool center position on the tool path.14 : 2...

  • Page 727

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/01708Projector view by isometric can be drawn.YXYZXZYZXYXZP=4P=5Fig.12.2.1(b) Coordinate systems for the isometric projectionXYZXP=6Fig.12.2.1 (c) Coordinate systems for the biplane viewBiplanes (XY and XZ) can be drawn simultaneously. The maximum andmi...

  • Page 728

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION709The tilting angle of the vertical axis is set in the range of –90°to +90°inreference to the horizontal axis crossing the vertical axis at a right angle.When a positive value is set, the vertical axis slants to the other side ofthe graphic screen....

  • Page 729

    OPERATION12. GRAPHICS FUNCTIONB–63614EN/01710It is possible to set whether the tool path is drawn by making the toollength offset or cutter compensation valid or invalid.Setting valueTool length offset or cutter compensation0Perform drawing by making tool compensation valid(An actual tool path...

  • Page 730

    OPERATIONB–63614EN/0112. GRAPHICS FUNCTION711No part program which has not been registered in memory can be drawn.Also, it is necessary that the M02 or M30 should be commanded at theend of the part program.The period of mark blinking is short when the tool is moving and becomeslonger when the ...

  • Page 731

    OPERATION13. HELP FUNCTIONB–63614EN/0171213 HELP FUNCTIONThe help function displays on the screen detailed information aboutalarms issued in the CNC and about CNC operations. The followinginformation is displayed.When the CNC is operated incorrectly or an erroneous machiningprogram is executed...

  • Page 732

    OPERATIONB–63614EN/0113. HELP FUNCTION7132Press soft key [ALAM] on the HELP (INITIAL MENU) screen todisplay detailed information about an alarm currently beingraised.Normal explana–tion on alarmFig.13(b) ALARM DETAIL screen when alarm P/S 027 is issuedFunction classificationAlarm detailsAlarm...

  • Page 733

    OPERATION13. HELP FUNCTIONB–63614EN/017143To get details on another alarm number, first enter the alarm number,then press soft key [SELECT]. This operation is useful forinvestigating alarms not currently being raised.Fig.13(d) How to select each ALARM DETAILS>100S 0 T0000MEM **** *** **...

  • Page 734

    OPERATIONB–63614EN/0113. HELP FUNCTION715Fig.13(g) How to select each OPERATION METHOD screen>1S 0 T0000MEM **** *** ***10:12:25[ ] [ ][ ] [ ][ SELECT ]When “1. PROGRAM EDIT” is selected, for example, the screen inFigure 13 (...

  • Page 735

    OPERATION13. HELP FUNCTIONB–63614EN/01716The current page No. is shown at the upper right corner on the screen.Fig. 13(j) PARAMETER TABLE screenHELP (PARAMETER TABLE)01234 N000011/4* SETTEING(No. 0000∼)* READER/PUNCHER INTERFACE(No. 0100∼)* AXIS CONTROL/SETTING UNIT(No. 1000∼)* COORDINAT...

  • Page 736

    OPERATIONB–63614EN/0114. SCREEN HARDCOPY71714 SCREEN HARDCOPYThe screen hardcopy function outputs the information displayed on theCNC screen as 640*480–dot bitmap data. This function makes it possibleto produce a hard copy of a still image displayed on the CNC.The created bitmap data can be ...

  • Page 737

    OPERATION14. SCREEN HARDCOPYB–63614EN/01718NOTE1 During the screen hardcopy operation, key input is disabledfor several tens of seconds. Until the screen hardcopyoperation ends, the screen image lies still. During thisperiod, the hardcopy in progress signal (F061#3) is tied to1. No other sig...

  • Page 738

    OPERATIONB–63614EN/0114. SCREEN HARDCOPY719The number of colors used in created bitmap data depend on the displaycontrol card, the LCD hardware, and the display mode of the CNC screen.Table 14 (a) indicates the relationships.Table 14 (a) Colors of BMP data created by the screen hardcopy functi...

  • Page 739

    IV. MAINTENANCE

  • Page 740

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY7231 METHOD OF REPLACING BATTERYThis chapter describes how to replace the CNC backup battery andabsolute pulse coder battery. This chapter consists of the followingsections:1.1 REPLACING BATTERY FOR LCD–MOUNTED TYPE iSERIES1.2 REPLACING TH...

  • Page 741

    MAINTENANCE1. METHOD OF REPLACING BATTERYB–63614EN/01724When a lithium battery is usedPrepare a new lithium battery (ordering code: A02B–0200–K102(FANUC specification: A98L–0031–0012)).1) Turn on the power to the CNC. After about 30 seconds, turn off thepower.2) Remove the old battery ...

  • Page 742

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY725CAUTIONSteps 1) to 3) should be completed within 30 minutes (orwithin 5 minutes for the 160i/180i with the PC function). Donot leave the control unit without a battery for any longerthan the specified period. Otherwise, the contents ofme...

  • Page 743

    MAINTENANCE1. METHOD OF REPLACING BATTERYB–63614EN/017261) Prepare two alkaline dry cells (size D) commercially available.2) Turn on the power to the Series 16i/18i/160i/180i.3) Remove the battery case cover.4) Replace the cells, paying careful attention to their orientation.5) Reinstall the co...

  • Page 744

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY727If a lithium battery is used, have A02B–0200–K102 (FANUC internalcode: A98L–0031–0012) handy.(1) Turn the CNC on. About 30 seconds later, turn the CNC off.(2) Remove the battery from the top area of the CNC unit.Disconnect the co...

  • Page 745

    MAINTENANCE1. METHOD OF REPLACING BATTERYB–63614EN/01728NOTEComplete steps (1) to (3) within 30 minutes. (or, for the 210iwith the PC functions, within 5 minutes)If the battery is left removed for a long time, the memorywould lose the contents.If there is a danger that the replacement cannot b...

  • Page 746

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY729(1) Have commercial D–size alkaline dry cells handy.(2) Turn the CNC on.(3) Remove the lid from the battery case.(4) Replace the old dry cells with new ones. Mount the dry cells in acorrect orientation.(5) Replace the lid on the battery...

  • Page 747

    MAINTENANCE1. METHOD OF REPLACING BATTERYB–63614EN/01730A lithium battery is used to back up BIOS data in the PANEL i. Thisbattery is factory–set in the PANEL i. This battery has sufficient capacityto retain BIOS data for one year.When the battery voltage becomes low, the LCD screen blinks....

  • Page 748

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY731BAT1Lithium batteryRear viewSide viewFrontFig.1.3 Lithium battery connection on the PANEL i

  • Page 749

    MAINTENANCE1. METHOD OF REPLACING BATTERYB–63614EN/01732One battery unit can maintain current position data for six absolute pulsecoders for a year.When the voltage of the battery becomes low, APC alarms 306 to 308 (+axis number) are displayed on the CRT display. When APC alarm 3n7is displayed...

  • Page 750

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY733When the battery voltage falls, APC alarms 306 to 308 are displayed onthe screen. When APC alarm 307 is displayed, replace the battery as soonas possible. In general, the battery should be replaced within one or twoweeks of the alarm first...

  • Page 751

    MAINTENANCE1. METHOD OF REPLACING BATTERYB–63614EN/01734The battery is connected in either of 2 ways as follows.Method 1: Attach the lithium battery to the SVM.Use the battery: A06B–6073–K001.Method 2: Use the battery case (A06B–6050–K060).Use the battery: A06B–6050–K061 or D–size...

  • Page 752

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY735[Attachment procedure](1) Check the item 1 to 4 of ”Replacement procedure”.(2) Have four D–size alkaline batteries on hand.(3) Loosen the screws on the battery case. Remove the cover.(4) Replace the alkaline batteries in the case. Pa...

  • Page 753

    MAINTENANCE1. METHOD OF REPLACING BATTERYB–63614EN/01736SVU–12, SVU–20BatteryBattery coverPass the battery cable to this slit.SVU–40, SVU–80CAUTIONSD The connector of the battery can be connected with eitherof CX5X and CX5Y.D Replacement of batteries in the battery case. (Method 2)Repla...

  • Page 754

    MAINTENANCEB–63614EN/011. METHOD OF REPLACING BATTERY737[Attachment procedure](1) Check the item 1 to 3 of ”Replacement procedure”.(2) Have four D–size alkaline batteries on hand.(3) Loosen the screws on the battery case. Remove the cover.(4) Replace the alkaline batteries in the case. Pa...

  • Page 755

    APPENDIX

  • Page 756

    APPENDIXB–63614EN/01A. TAPE CODE LIST741ATAPE CODE LISTISO codeEIA codeMeaningCharacter 8 7 6 5 43 2 1 Character 8 7 6 5 43 2 1WithoutCUSTOMMACRO BWithCUSTOMMACRO B0f ff0ffNumber 01ff fff1ff Number 12ff fff2ffNumber 23f fff f3fff f Number 34ff fff4ffNumber 45f ffff5ffff Number 56f fff f6fff fNu...

  • Page 757

    APPENDIXA. TAPE CODE LISTB–63614EN/01742ISO codeEIA codeMeaningCharacter 8 7 6 5 43 2 1Character8 7 6 5 43 2 1WithoutCUSTOMMACRO BWithCUSTOMMACRO BDELf f f f f ff f fDelf f f f ff f f××NULfBlankf××BSff fBSff ff××HTf ffTabf f f ff f××LF or NLf ffCR or EOBffCRff fff××SPfffSPffjj%fffffER...

  • Page 758

    APPENDIXB–63614EN/01A. TAPE CODE LIST743NOTE1 The symbols used in the remark column have the following meanings.(Space) :The character will be registered in memory and has a specific meaning.It it is used incorrectly in a statement other than a comment, an alarm occurs.×:The character will not...

  • Page 759

    APPENDIXB. LIST OF FUNCTIONS AND TAPE FORMATB–63614EN/01744BLIST OF FUNCTIONS AND TAPE FORMATSome functions cannot be added as options depending on the model.In the tables below, PI:presents a combination of arbitrary axisaddresses using X,Y,Z,A,B and C (such as X_Y_Z_A_).x = 1st basic axis (X ...

  • Page 760

    APPENDIXB–63614EN/01B. LIST OF FUNCTIONS AND TAPE FORMAT745FunctionsTape formatIllustrationAI advanced preview control (G05.1)G05.1 Q1; AI advanced preview control mode onG05.1 Q0 ; AI advanced preview control mode offCylindrical interpolation(G07.1)G07.1 IP_r_; Cylindrical interpolation modeG0...

  • Page 761

    APPENDIXB. LIST OF FUNCTIONS AND TAPE FORMATB–63614EN/01746FunctionsTape formatIllustrationReference position return(G28)2nd, reference position return(G30)PIReference positionIntermediate position(G28)2nd referenceposition (G30)Start pointG27 _ ;PIReturn from reference position to start poi...

  • Page 762

    APPENDIXB–63614EN/01B. LIST OF FUNCTIONS AND TAPE FORMAT747FunctionsTape formatIllustrationTool length offset C (G43, G44, G49)G43a_ H_ ;G44a : An optional address of one axisH : Tool offset numberG49 : CancelTool offset (G45 – G48)IPIPIncreaseDecrease2 timesincrease2 timesdecreaseCompensatio...

  • Page 763

    APPENDIXB. LIST OF FUNCTIONS AND TAPE FORMATB–63614EN/01748FunctionsTape formatIllustrationCutting mode (G64)Exact stop mode (G61)Tapping mode (G63)Automatic corner override(G62)vtG64vG61tG64_ ; Cutting modeG61_ ; Exact stop modeG63_ ; Tapping modeG62_ ; Automatic corner overrideCustom macro(G...

  • Page 764

    APPENDIXB–63614EN/01B. LIST OF FUNCTIONS AND TAPE FORMAT749FunctionsTape formatIllustrationConstant surface speedcontrol (G96, G97)Surface speed(m/min or feet/min)Spindle speed N (min–1)G96 S_ ; Starts constant surface speed control(Surface speed command)G97 S_ ; Constant surface speed is can...

  • Page 765

    APPENDIXC. RANGE OF COMMAND VALUEB–63614EN/01750CRANGE OF COMMAND VALUEIncrement systemIS–BIS–CLeast input increment0.001 mm0.0001 mmLeast command increment0.001 mm0.0001 mmMax. programmable dimension±99999.999 mm±9999.9999 mmMax. rapid traverse Note240000 mm/min100000 mm/minFeedrate ran...

  • Page 766

    APPENDIXB–63614EN/01C. RANGE OF COMMAND VALUE751Increment systemIS–BIS–CLeast input increment0.0001 inch0.00001 inchLeast command increment0.0001 inch0.00001 inchMax. programmable dimension±9999.9999 inch±9999.9999 inchMax. rapid traverse Note9600 inch/min4000 inch/minFeedrate range Not...

  • Page 767

    APPENDIXC. RANGE OF COMMAND VALUEB–63614EN/01752Increment systemIS–BIS–CLeast input increment0.001 deg0.0001 degLeast command increment0.001 deg0.0001 degMax. programmable dimension±99999.999 deg±9999.9999 degMax. rapid traverse Note240000 deg/min100000 deg/minFeedrate range Note1 to 2400...

  • Page 768

    APPENDIXB–63614EN/01D. NOMOGRAPHS753DNOMOGRAPHS

  • Page 769

    APPENDIXD. NOMOGRAPHSB–63614EN/01754The leads of a thread are generally incorrect in δ1 and δ2, as shown in Fig.D.1 (a), due to automatic acceleration and deceleration.Thus distance allowances must be made to the extent of δ1 and δ2 in theprogram.Fig.D.1(a) Incorrect thread positionδ2δ...

  • Page 770

    APPENDIXB–63614EN/01D. NOMOGRAPHS755First specify the class and the lead of a thread. The thread accuracy, α,will be obtained at (1), and depending on the time constant of cutting feedacceleration/ deceleration, the δ1 value when V = 10mm / s will beobtained at (2). Then, depending on the s...

  • Page 771

    APPENDIXD. NOMOGRAPHSB–63614EN/01756Fig. D.2 (a) Incorrect threaded portionδ2δ1R : Spindle speed (min-1)L : Thread lead (mm)* When time constant T of the servo system is 0.033 s.d2+ LR1800 * (mm)d1+ LR1800 *(–1–lna)+ d2(–1–lna)Following a is a permited value of thread.a–1–lna0.00...

  • Page 772

    APPENDIXB–63614EN/01D. NOMOGRAPHS757Fig D.2 (b) Nomograph for obtaining approach distance δ1D Reference

  • Page 773

    APPENDIXD. NOMOGRAPHSB–63614EN/01758When servo system delay (by exponential acceleration/deceleration atcutting or caused by the positioning system when a servo motor is used)is accompanied by cornering, a slight deviation is produced between thetool path (tool center path) and the programmed p...

  • Page 774

    APPENDIXB–63614EN/01D. NOMOGRAPHS759The tool path shown in Fig. D.3 (b) is analyzed based on the followingconditions:Feedrate is constant at both blocks before and after cornering.The controller has a buffer register. (The error differs with the readingspeed of the tape reader, number of chara...

  • Page 775

    APPENDIXD. NOMOGRAPHSB–63614EN/01760Fig. D.3(c) Initial valueY0X0V0The initial value when cornering begins, that is, the X and Y coordinatesat the end of command distribution by the controller, is determined by thefeedrate and the positioning system time constant of the servo motor.X0+ VX1(T1) ...

  • Page 776

    APPENDIXB–63614EN/01D. NOMOGRAPHS761When a servo motor is used, the positioning system causes an errorbetween input commands and output results. Since the tool advancesalong the specified segment, an error is not produced in linearinterpolation. In circular interpolation, however, radial errors...

  • Page 777

    APPENDIXE. STATUS WHEN TURNING POWER ON,WHEN CLEAR AND WHEN RESETB–63614EN/01762E STATUS WHEN TURNING POWER ON, WHEN CLEARAND WHEN RESETParameter CLR (No. 3402#6) is used to select whether resetting the CNCplaces it in the cleared state or in the reset state (0: reset state/1: clearedstate).The...

  • Page 778

    APPENDIXB–63614EN/01E. STATUS WHEN TURNING POWER ON,WHEN CLEAR AND WHEN RESET763ItemResetClearedWhen turning power onAction in Movement×××opera-Dwell×××tionIssuance of M, S andT codes×××Tool length compensa-tion×Depending onparameterLVK(No.5003#6)f : MDI modeOther modes dependon param...

  • Page 779

    APPENDIXF. CHARACTER–TO–CODES CORRESPONDENCE TABLEB–63614EN/01764F CHARACTER–TO–CODES CORRESPONDENCE TABLEChar-acterCodeCommentChar-acterCodeCommentA0656054B0667055C0678056D0689057E069032SpaceF070!033Exclamation markG071”034Quotation markH072#035Hash signI073$036Dollar signJ074%037P...

  • Page 780

    APPENDIXB–63614EN/01G. ALARM LIST765GALARM LIST1) Program errors (P/S alarm)NumberMessageContents000PLEASE TURN OFF POWERA parameter which requires the power off was input, turn off power.001TH PARITY ALARMTH alarm (A character with incorrect parity was input). Correct the tape.002TV PARITY ALA...

  • Page 781

    APPENDIXG. ALARM LISTB–63614EN/01766NumberContentsMessage029ILLEGAL OFFSET VALUEThe offset values specified by H code is too large.Modify the program.030ILLEGAL OFFSET NUMBERThe offset number specified by D/H code for tool length offset or cuttercompensation is too large. Modify the program.031...

  • Page 782

    APPENDIXB–63614EN/01G. ALARM LIST767NumberContentsMessage060SEQUENCE NUMBER NOT FOUNDCommanded sequence number was not found in the sequence numbersearch. Check the sequence number.070NO PROGRAM SPACE INMEMORYThe memory area is insufficient.Delete any unnecessary programs, then retry.071DATA NO...

  • Page 783

    APPENDIXG. ALARM LISTB–63614EN/01768NumberContentsMessage090REFERENCE RETURN INCOM-PLETEThe reference position return cannot be performed normally becausethe reference position return start point is too close to the reference posi-tion or the speed is too slow. Separate the start point far enou...

  • Page 784

    APPENDIXB–63614EN/01G. ALARM LIST769NumberContentsMessage122QUADRUPLICATE MACRO MODAL–CALLA total of four macro calls and macro modal calls are nested. Correctthe program.123CAN NOT USE MACRO COMMANDIN DNCMacro control command is used during DNC operation.Modify the program.124MISSING END ST...

  • Page 785

    APPENDIXG. ALARM LISTB–63614EN/01770NumberContentsMessage153T–CODE NOT FOUNDIn the registration of tool life data, a T code was not specified in ablock where it is required. Alternatively, only M06 was specified in ablock for tool change type D. Correct the program.154NOT USING TOOL IN LIFE...

  • Page 786

    APPENDIXB–63614EN/01G. ALARM LIST771NumberContentsMessage203PROGRAM MISS AT RIGID TAPPINGIn the rigid tapping, position for a rigid M code (M29) or an S command is incorrect. Modify the program.204ILLEGAL AXIS OPERATIONIn the rigid tapping, an axis movement is specified between the rigidM code ...

  • Page 787

    APPENDIXG. ALARM LISTB–63614EN/01772NumberContentsMessage5010END OF RECORDThe end of record (%) was specified.5020PARAMETER OF RESTARTERRORThe parameter for specifying program restart is not set correctly.5046ILLEGAL PARAMETER (ST.COMP)An illegal parameter has been specified for straightness co...

  • Page 788

    APPENDIXB–63614EN/01G. ALARM LIST773NumberContentsMessage5212SCREEN COPY : PARAMETERERRORThere is a parameter setting error. Check that 4 is set as the I/O channel(parameter No.0020).5213SCREEN COPY :COMMUNICATION ERRORThe memory card cannot be used. Check the memory card. (Checkwhether the ...

  • Page 789

    APPENDIXG. ALARM LISTB–63614EN/017742) Background edit alarmNumberMessageContents???BP/S alarmBP/S alarm occurs in the same number as the P/S alarm that occurs inordinary program edit.(P/S alarm No. 070, 071, 072, 073, 074, 085 to 087)Modify the program.140BP/S alarmIt was attempted to select o...

  • Page 790

    APPENDIXB–63614EN/01G. ALARM LIST7754) Serial pulse coder (SPC) alarmsNo.MessageDescription360n AXIS : ABNORMAL CHECKSUM(INT)A checksum error occurred in the built–in pulse coder.361n AXIS : ABNORMAL PHASE DATA(INT)A phase data error occurred in the built–in pulse coder.362n AXIS : ABNORMAL...

  • Page 791

    APPENDIXG. ALARM LISTB–63614EN/01776#7202#6CSA#5BLA#4PHA#3PCA#2BZA#1CKA#0SPH#6 (CSA) : Check sum alarm has occurred.#5 (BLA) : Battery low alarm has occurred.#4 (PHA) : Phase data trouble alarm has occurred.#3 (PCA) : Speed count trouble alarm has occurred.#2 (BZA) : Battery zero alarm has occu...

  • Page 792

    APPENDIXB–63614EN/01G. ALARM LIST777NumberContentsMessage415SERVO ALARM: n–TH AXIS –EXCESS SHIFTA speed higher than 524288000 units/s was attempted to be set in the n–thaxis (axis 1–8). This error occurs as the result of improperly set CMR.417SERVO ALARM: n–TH AXIS –PARAMETER INCOR...

  • Page 793

    APPENDIXG. ALARM LISTB–63614EN/01778NumberContentsMessage440n AXIS : CNV. EX DECELERATIONPOW.1) PSMR: The regenerative discharge amount is too large.2)α series SVU: The regenerative discharge amount is too large. Al-ternatively, the regenerative discharge circuit is abnormal.441n AXIS : ABN...

  • Page 794

    APPENDIXB–63614EN/01G. ALARM LIST779NumberContentsMessage467n AXIS : ILLEGAL SETTING OFAXISThe servo function for the following has not been enabled when anaxis occupying a single DSP (corresponding to two ordinary axes) isspecified on the axis setting screen.1. Learning control (bit 5 of para...

  • Page 795

    APPENDIXG. ALARM LISTB–63614EN/017806) Over travel alarmsNumberMessageContents500OVER TRAVEL : +nExceeded the n–th axis + side stored stroke limit I.(Parameter No.1320 or 1326 Notes)501OVER TRAVEL : –nExceeded the n–th axis – side stored stroke limit I.(Parameter No.1321 or 1327 Notes)5...

  • Page 796

    APPENDIXB–63614EN/01G. ALARM LIST7819) Rigid tapping alarmNumberMessageContents740RIGID TAP ALARM : EXCESSERRORDuring rigid tapping, the position deviation of the spindle in the stopstate exceeded the setting.741RIGID TAP ALARM : EXCESSERRORDuring rigid tapping, the position deviation of the sp...

  • Page 797

    APPENDIXG. ALARM LISTB–63614EN/01782The details of spindle alarm No. 750 are displayed in the diagnosis display(No. 409) as shown below.#7409#6#5#4#3SPE#2S2E#1S1E#0SHE#3 (SPE) 0 : In the spindle serial control, the serial spindle parameters fulfill thespindle unit startup conditions.1 : In the ...

  • Page 798

    APPENDIXB–63614EN/01G. ALARM LIST783Alarm List (Serial Spindle)When a serial spindle alarm occurs, the following number is displayed onthe CNC. n is a number corresponding to the spindle on which an alarmoccurs. (n = 1: First spindle; n = 2: Second spindle; etc.)NOTE*1Note that the meanings...

  • Page 799

    APPENDIXG. ALARM LISTB–63614EN/01784No.DescriptionFaulty location and remedySPMindica-tion(*1)Message7n07SPN_n_ : OVERSPEED07Check for a sequence error. (Forexample, check whether spindlesynchronization was specified whenthe spindle could not be turned.)The motor speed has exceeded115% of its ...

  • Page 800

    APPENDIXB–63614EN/01G. ALARM LIST785No.DescriptionFaulty location and remedySPMindica-tion(*1)Message7n26SPN_n_ : DISCONNECTC–VELO DE-TECT261 Replace the cable.2Re–adjust the pre–amplifier.The signal amplitude of the detec-tion signal (connector JY2) on theCs contour control motor side is...

  • Page 801

    APPENDIXG. ALARM LISTB–63614EN/01786No.DescriptionFaulty location and remedySPMindica-tion(*1)Message7n36SPN_n_ : OVERFLOWERRORCOUNTER36Check whether the position gainvalue is too large, and correct thevalue.An error counter overflow occurred.7n37SPN_n_ : SPEED DE-TECT PAR.ERROR37Correct the va...

  • Page 802

    APPENDIXB–63614EN/01G. ALARM LIST787No.DescriptionFaulty location and remedySPMindica-tion(*1)Message7n50SPN_n_ : SPNDL CON-TROL OVER-SPEED50Check whether the calculated valueexceeds the maximum motorspeed.In spindle synchronization, thespeed command calculation valueexceeded the allowable limi...

  • Page 803

    APPENDIXG. ALARM LISTB–63614EN/01788No.DescriptionFaulty location and remedySPMindica-tion(*1)Message7n79SPN_n_ : INITIAL TESTERROR79Replace the SPM control printed–circuit board.An error was detected in an initialtest operation.7n81SPN_n_ : 1–ROT MO-TOR SENSORERROR811 Check and correct the...

  • Page 804

    APPENDIXB–63614EN/01G. ALARM LIST789No.DescriptionFaulty location and remedySPMindica-tion(*1)Message9n02SPN_n_ : EX SPEED ER-ROR021 Check and correct the cuttingconditions to decrease the load.2 Correct parameter No. 4082.The motor speed cannot follow aspecified speed.An excessive motor load t...

  • Page 805

    APPENDIXG. ALARM LISTB–63614EN/01790No.DescriptionFaulty location and remedySPMindica-tion(*1)Message9n18SPN_n_ : SUMCHECKERROR PGM DATA18Replace the SPM control printed cir-cuit board.Abnormality in an SPM control cir-cuit component is detected. (Pro-gram ROM data is abnormal.)9n19SPN_n_ : EX...

  • Page 806

    APPENDIXB–63614EN/01G. ALARM LIST791No.DescriptionFaulty location and remedySPMindica-tion(*1)Message9n32SPN_n_ : RAM FAULT SERIAL LSI32Replace the SPM control printed cir-cuit board.Abnormality in an SPM control cir-cuit component is detected. (TheLSI device for serial transfer is ab-normal.)...

  • Page 807

    APPENDIXG. ALARM LISTB–63614EN/01792No.DescriptionFaulty location and remedySPMindica-tion(*1)Message9n46SPN_n_ : SCREW1–ROT POS–COD. ALARM461 Check and correct the parame-ter.2 Replace the cable.3Re–adjust the BZ sensor signal.An abnormality equivalent to alarm41 was detected during thre...

  • Page 808

    APPENDIXB–63614EN/01G. ALARM LIST793No.DescriptionFaulty location and remedySPMindica-tion(*1)Message9n58SPN_n_ : OVERLOAD INPSM581 Check the PSM cooling status.2 Replace the PSM unit.The temperature of the radiator ofthe PSM has increased abnormally.(PSM alarm indication: 3)9n59SPN_n_ : COOLI...

  • Page 809

    APPENDIXG. ALARM LISTB–63614EN/01794ERROR CODES (SERIAL SPINDLE)NOTE*1Note that the meanings of the SPM indications differdepending on which LED, the red or yellow LED, is on.When the yellow LED is on, an error code is indicated witha 2–digit number. The error code is not displayed on theCNC...

  • Page 810

    APPENDIXB–63614EN/01G. ALARM LIST795SPMindica-tion(*1)DescriptionFaulty location and remedy12During execution of the spindle synchronization com-mand, do not specify another operation mode. Beforeentering another mode, cancel the spindle synchro-nization command.Although spindle synchronizatio...

  • Page 811

    APPENDIXG. ALARM LISTB–63614EN/0179611) System alarms (These alarms cannot be reset with reset key.)NumberMessageContents900ROM PARITYROM parity error (CNC/OMM/Servo)Rewrite the flash ROM with the indicated ROM number.910SRAM PARITY : (BYTE 0)RAM parity error in the tape memory SRAM module. Cl...

  • Page 812

    IndexB–63614EN/01i–1[Numbers]7.2″/8.4″ LCD–Mounted Type CNC Control Unit, 4079.5″/10.4″ LCD–Mounted Type CNC Control Unit,407[A]Absolute and Incremental Programming (G90, G91),91Actual Feedrate Display, 636Adding Workpiece Coordinate Systems (G54.1 orG54), 85Advanced Preview Contr...

  • Page 813

    IndexB–63614EN/01i–2Data Input/Output On the All IO Screen, 550Data Input/Output Using a Memory Card, 576Decimal Point Programming, 96Deleting a Block, 596Deleting a Word, 595Deleting All Programs, 601Deleting Blocks, 596Deleting Files, 547Deleting More Than One Program by Specifying aRange, ...

  • Page 814

    B–63614EN/01Indexi–3Functions to Simplify Programming, 132[G]G53, G28, G30, and G30.1 Commands in Tool LengthOffset Mode, 191G53,G28,G30,G30.1 and G29 Commands in CutterCompensation C Mode, 243General Flow of Operation of CNC Machine Tool, 6General Screen Operations, 413Graphic Display, 403Gr...

  • Page 815

    IndexB–63614EN/01i–4Manual Operation, 390, 442Manual Reference Position Return, 443Maximum Stroke, 30MDI Operation, 465Memory Card Input/Output, 567Memory Operation, 462Memory Operation Using FS10/11 Tape Format, 356Merging a Program, 607Method of Replacing Battery, 723Mirror Image, 489Modal ...

  • Page 816

    B–63614EN/01Indexi–5Reference Position (Machine–Specific Position), 15Reference Position Return, 71Register, Change and Delete of Tool Life Manage-ment Data, 106Registering Custom Macro Programs, 327Repetition (While Statement), 306Replacement of Words and Addresses, 610Replacing Battery fo...

  • Page 817

    IndexB–63614EN/01i–6Tool Length Measurement, 659Tool Length Offset (G43,G44,G49), 186Tool Life, 112Tool Life Management Command in a Machining Pro-gram, 109Tool Life Management Data, 105Tool Life Management Function, 104Tool Movement Along Workpiece Parts Figure– Inter-polation, 12Tool Move...

  • Page 818

    Revision RecordFANUCSeries21i/210i–MB OPERATOR’S MANUAL (B–63614EN)01Jul., 2001EditionDateContentsEditionDateContents

  • Page 819

    · No part of this manual may bereproduced in any form.· All specifications and designsare subject to change withoutnotice.

  • Abstract

    PROGRAMMINGB–63614EN/014. INTERPOLATION FUNCTIONS49To perform tool offset in the cylindrical interpolation mode, cancel anyongoing cutter compensation mode before entering the cylindricalinterpolation mode. Then, start and terminate tool offset within thecylindrical interpolation mode.In the cylindrical interpolation mode, the amount of travel of a rotary axisspecified by an angle is once internally converted to a distance of a linearaxis on the outer surface so that linear interpolation or circularinterpolation can be performed with another axis. After interpolation,such a distance is converted back to an angle. For this conversion, theamount of travel is rounded to a least input increment.So when the radius of a cylinder is small, the actual amount of travel candiffer from a specified amount of travel. Note, however, that such an erroris not accumulative.If manual operation is performed in the cylindrical interpolation modewith manual absolute on, an error can occur for the reason describedabove.Specified valueThe actual amountof travel2×2πRMOTION REV MOTION REVMOTION REV: The amount of travel per rotation of the rotation axis (Set-ting value of parameter No. 1260)R::Rounded to the least input incrementWorkpiece radius= 2×2πRIn the cylindrical interpolation mode, an arc radius cannot be specifiedwith word address I, J, or K.If the cylindrical interpolation mode is started when cutter compensationis already applied, circular interpolation is not correctly performed in thecylindrical interpolation mode.In the cylindrical interpolation mode, positioning operations (includingthose that produce rapid traverse cycles such as G28, G53, G73, G74,G76, G80 through G89) cannot be specified. Before positioning can bespecified, the cylindrical interpolation mode must be cancelled.Cylindrical interpolation (G07.1) cannot be performed in the positioningmode (G00).In the cylindrical interpolation mode, a workpiece coordinate system(G92, G54 through G59) or local coordinate system (G52) cannot bespecified.In the cylindrical interpolation mode, the cylindrical interpolation modecannot be reset. The cylindrical interpolation mode must be cancelledbefore the cylindrical interpolation mode can be reset.A tool offset must be specified before the cylindrical interpolation modeis set. No offset can be changed in the cylindrical interpolation mode.Cylindrical interpolation cannot be specified when the index table indexfunction is being used.D Tool offsetD Cylindrical interpolationaccuracyLimitationsD Arc radius specificationin the cylindricalinterpolation modeD Circular interpolationand cutter compensationD PositioningD Coordinate systemsettingD Cylindrical interpolationmode settingD Tool offsetD Index table indexingfunction

x