Navigation

  • Page 1

    Programming Manual For all Doosan Machining Centers Using Fanuc Controls ©Phil Misseldine 2007

  • Page 2

    Forward While similar in appearance your CNC Machining Center operates somewhat differently from your conventional mill. Although they may share the same work envelope and number of axis the CNC does not have the array of knobs, levers or handles associated with the manual machine. In place ...

  • Page 3

    Introduction to Programming Programming of your Doosan Machining Center involves the sequential study of the operations required to produce a component, using established engineering methods. Study Part DrawingMethodize the Part Programthe Part Set upMachineMachine Part Finished Part Exampl...

  • Page 4

    Most Commonly Used G-Codes G-Code Function G00 Rapid Positioning Standard G01 Feedrate Positioning Standard G02 Arc Clockwise Standard G03 Arc counter Clockwise Standard G04 Dwell Standard G05 High Speed Machining Optional G08 Look Ahead Control Optional G09 Exact Stop Standard G10 Data Setting...

  • Page 5

    Most Commonly Used M-Codes For a complete M-code list please refer to your Doosan Manual. M Code Function Vertical Horizontal M00 Program Stop Standard Standard M01 Optional Stop Standard Standard M02 Program End Standard Standard M03 Spindle Clockwise Rotation Standard Standard M04 Spindle Ant...

  • Page 6

    Control Panel EMERGENCY STOPMODEMODE SELECTMDITAPEMEMORYEDITREF.RTN.JOGHANDLEMACHINE READY EMERGENCY RELEASEFEED HOLDCYCLE STARTFEED OPERATIONREF.POINTRAPID OVERIDEFEEDRATE OVERIDEAXIS SELECTRAPID020406080100120130140180SPINDLESPINDLE OVERIDE01020304050608090100ALARMRESETM02/M30 LUB. MACHINEWORK ...

  • Page 7

    Axis Movement Every Vertical Machining Center has three axes: X - side to side Y - forwards and backwards Z - up and down All Horizontal Machining Centers have four axes: X - side to side Y - up and down Z - forwards and backwards B - rotary 7

  • Page 8

    Manual Pulse Generator XYZ4THX1X10X1000908070605040302010_+The Manual Pulse Generator (MPG) or Hand Wheel is used during the setup of the machine. This is separate from the machine control and gives better control of all axis during setup. 8

  • Page 9

    TOOL LENGTH OFFSET When a cutting tool is inserted into its holder, the cutting edge is located at an imprecise distance from the gauge line of the holder. By specifying G43 and the corresponding offset value (H) it is possible to compensate the difference without changing the part program. ...

  • Page 10

    Tool Length Setting Method Using a combination of the jog buttons and MPG, bring the tool down to the predetermined "Z" point. Operators choice of 'Z' zero position.(This example uses the top of the work piece).Work piecePress the function key and then the [OFFSET] soft key...

  • Page 11

    Tool Offset Memory 'C' (Optional) Tool Offset Memory 'C' allows you to use the same number for Length (H) and Diameter (D) offsets. Press the function key and then the [OFFSET] soft key to display the following screen. Cursor down to tool number to be set. Press 'Z' and then the 'INP.C' soft...

  • Page 12

    Work Coordinates Every CNC machine has a reference or machine zero. This is a position that is constant to the machine. When a machine is turned on or powered up by the operator it must first be referenced. When the machine reaches its limit switches the control registers this location as home...

  • Page 13

    Work Coordinate System Setting Method To set the work piece co-ordinates the user has the choice of six co-ordinate systems to choose from G54 to G59. Press function key and then the [WORK] soft key to display the following page. Method Using an edge finder or indicator l...

  • Page 14

    Work Coordinate System G54 - G59 and G54.1 P1 -P300 The desired Work Coordinate number should always be called at the start of every tool. Example. N4 (.75 DIA. ENDMILL ) N5 G0 G54 G90 X-2.25 Y.625 S8000 M3 N6 G43 Z.1 H1 N7 G1 Z-1. F25 This option expands the Wo...

  • Page 15

    Linear Interpolation (G00/G01) PROGRAMMING All axis of the machine tool will move in linear at either RAPID or FEEDRATE traverse rates. Any movement preceded by G00 will occur at RAPID traverse G00 X4.0 Y-3.0 Any movement preceded by G01 will occur at...

  • Page 16

    Co-Ordinate Programming (G90/G91) Absolute co-ordinate programming (G90) In absolute programming all dimensioning is taken from a fixed point. Incremental co-ordinate programming (G91) In incremental programming dimensioning is taken from the last position programmed and NOT from a fixed point. 16

  • Page 17

    Absolute and Incremental Programming Example X+Y+DatumFind the absolute and Incremental co-ordinates of the points listed. Answers are on page 100. ABSOLUTE (G90) INCREMENTAL (G91) A X __________ _ Y__ ...

  • Page 18

    Plane Selection (G17, G18, G19) Before an arc can be machined the correct plane must be selected. When generating an arc in the 'X' and 'Y' axis G18 must be selected. G17 G18 When generating an arc in the 'X' and 'Z' axis G17must be selected. G19 G02G03X+Z+View from front of machineView from top ...

  • Page 19

    Circular Interpolation (G02, G03) There are two directions in which you can produce an arc - G02 Clockwise and G03 Counter Clockwise. To machine an arc the machine tool requires the following information. Tool finish position in 'X' Tool finish position in 'Y' Arc offset in 'X'...

  • Page 20

    Circular Interpolation G02 O1066 (Program number) N1G17G40G80G90 (Safe start) N2T1M6 (Calls T1 and changes tool) N3G54G90G0X-1.5Y0.S718M3 (Tool moves to start position) N4G43Z.1H1 (Picks up tool length value) N5G1Z-.1F20. (Feeds to Z-depth) N6G2X0.Y1.5I1.5F40. (Clock-wise move) N7G1X3.75Y.75 (Li...

  • Page 21

    Circular Interpolation G03 O1066 (Program number) N1G17G40G80G90 (Safe start) N2T1M6 (Calls T1 and changes tool) N3G54G90G0X-1.5Y0.S718M3 (Tool moves to start position) N4G43Z.1H1 (Picks up tool length value) N5G1Z-.1F20. (Feeds to Z-depth) N6G3X0.Y-1.5I1.5F40. (Counter Clock-wise move) N7G1X3.7...

  • Page 22

    Radius Command (R) As an alternative to using the 'I' and 'J' commands it is possible to program an arc using the 'R' command. 81234567This example machines a ½” radius on each corner. The datum is the top left-hand corner of the part. The tool diameter is .500”. ...

  • Page 23

    Cutter Compensation (G41/G42) Cutter compensation allows a program to be written without considering the size of the cutter. The three G-codes used to control cutter compensation are G41 - Cutter compensation Left G42 - Cutter compensation Right G40 - Cutter compensation Cancel If your c...

  • Page 24

    Cutter Compensation (G41) G41 - Cutter compensation to the Left of the work piece. Always apply cutter compensation at 90 degrees to the work piece. The program for applying cutter compensation should look like this. G1G41Y0 D1 F25. or if using cutter compensation 'B' it should look like this G...

  • Page 25

    Cutter Compensation (G42) G42 - Cutter compensation to the Right of the work piece. Always apply cutter compensation at 90 degrees to the work piece. The program for applying cutter compensation should look like this. G1G42Y0D1F25. or if using cutter compensation 'B' it should look like this G1...

  • Page 26

    Canned (Fixed) Cycles (G73, G81, G83, G86) Canned cycles are designed to make it easier for the programmer to create programs. With the use of a single 'G' function the canned cycle can be performed in a single block. This makes program-ming quicker and also saves on program memory. The formats ...

  • Page 27

    Initial and Rapid Planes (G98/G99) When using canned cycles the controller provides the ability to return to one of two reference planes. G98G99Point ZPoint ZInitial Point LevelR Point Level G98 - Returns the tool to the INITIAL plane. G99 - Returns the tool to the RAPID plane. 27

  • Page 28

    High Speed Peck Drilling (G73) Example G98 G73 X0.0 Y0.0 Z-1.25 Q.250 R.250 F20. Unlike G83 (peck drilling) G73 does not rapid to the R plane after each peck. When G98 is used 'Z' will return to the Initial point.When G99 is used 'Z' will return to the R point.Initial Point (G43 Z1. H01)Tool...

  • Page 29

    Drilling (G81) Example G98 G81 X0.0 Y0.0 Z-1.25 R.25 F20. Initial Point (G43 Z1. H01)Tool will stop 1.0" above part.R Point(R.25)Final Hole Depth (Z-1.25)When G99 is used 'Z' will return to the R point.When G98 is used 'Z' will return to the Initial point.'Z' - Zero is top of part.29

  • Page 30

    Peck Drilling (G83) Example G98 G83 X0.0 Y0.0 Z-1.25 Q.25 R.25 F20. After each peck 'Z' will rapid to the 'R' plane and then back to within 0.1" of where it finished cutting. When G98 is used 'Z' will return to the Initial point.When G99 is used 'Z' will return to the R point.Initial P...

  • Page 31

    Tapping (G84) Example G98 G84 X0.0 Y0.0 Z-1.25 R.25 F10. You must use a floating tap holder when using G84. For Rigid Tapping example please see page 33. Final Hole Depth (Z-1.50)'Z' - Zero is top of part.Initial Point (G43 Z1. H01)Tool will stop 1.0" above part.R Point(R.25)When G99 i...

  • Page 32

    Fine Boring (G76) Example G98 G76 X0.0 Y0.0 Z-1.5 R.25 Q.005 F10. Please consult your machine operation manual for correct orientation when using a single point-boring tool. 'Q' represents the amount tool will move away from machined face before lifting out of hole. Set the direction and ax...

  • Page 33

    Rigid Tapping (G84) Example (1/2-13 Tap) G0 G90 G54 X0 Y0 G43 H01 Z.25 M8 G95 S1000 (G95 feed per rotation) M29 (Rigid tapping mode) G98 G84 Z-1.5 R.25 F.0769 (Tapping cycle with 'F' = pitch of thread) G80 M9 G94 (Feed per minute) G91 G28 Z0 M5 G90 M30 Important thing to remember when Rigid Tapp...

  • Page 34

    Rigid Tapping Using an Alternate Axis It is possible to rigid tap using an axis other than Z. This is often used when the use of a right angled head is necessary. Parameters. Before starting set the following parameter. 5101 bit 0 to 1 (FXY) If an axis other than Z is ...

  • Page 35

    Repetition of Canned Cycles (K) By placing an 'K' on the same line as the canned cycle command it is possible to repeat the cycle. The 'K' command should only be used with G91(incremental). If G90 (absolute) were to be used only the 1st hole would be machined. Example 2 G0 G90 X0 Y0 (1st hole p...

  • Page 36

    Use of 'K0' in Canned Cycles Placing a 'K0' at the end of a canned cycle will prevent the cycle from being executed at that position. This allows the operator to have all the hole positions in a subprogram and define canned cycles in the main program. T01 M6 (SPOT DRIL) G90 G54 X0. Y0. S8000 M...

  • Page 37

    Thread Milling (Helical Interpolation) Helical Interpolation provides a method of thread cutting without having to use a machine tap. PitchOne revolution must equal pitch of threadAlways feed on using cutter compensasion37

  • Page 38

    Thread Milling (Helical Interpolation) Example This example machines a 11/2 - 6 thread .50" deep Pitch of thread is .1666 N10 G0 G90 G54 X0. Y0. S1000 M3The machine moves to the part datum using the G54 work coordinate and starts the spindle at 1000 r.p.m.N20 G43 Z.250 H1 M8The machine appli...

  • Page 39

    Manual Data Input (MDI) In MDI mode you can create and run a program without having to store it in the controls memory. Select MDI using the Mode Select Switch. Press the PROG hard key and the following screen will be displayed. Enter the program manually using the key pad, include end of block...

  • Page 40

    Starting a Program Press the PROG hard key and the following screen will be displayed. All programs must start with the letter 'O' Manually key in the program number and then press the insert hard key. Before any more lines can be added you must enter an end of block. Example O1234 - INSERT - EO...

  • Page 41

    Program Numbers Technically the numbers O0000 through O9999 are available for creating program numbers. However some numbers are used by other functions and are best avoided when creating a program. To prevent accidental editing or deletion of programs, turn program protect key to lock and remove...

  • Page 42

    Editing a Program The following is the procedure for Inserting, Altering and Deleting a command in a program which is registered in the controls memory. Using the cursor keys highlight the command to be changed. Press the PROG hard key and make sure that the program requiring editing is displayed...

  • Page 43

    Extended Part Program Edit Extended Part Program Edit is the name given to the copy, move and merge function. This allows the programmer to duplicate whole or parts of a program without having to rewrite the whole program. Copy Example O1234 G90 G80 G40 T1 M6 G90 G0 G54 X0.0 Y0.0 S3500 M3 G43 Z.1...

  • Page 44

    Extended Part Program Edit (Move) Move Example O1234 G90 G80 G40 T1 M6 (CRSR~) G90 G0 G54 X0.0 Y0.0 S3500 M3 G43 Z.1 H1 M8 G98 G81 Z-1. R.1 F15. G80 M9(~CRSR) G91 G28 Z0 Y0 M30 Press MOVE key Position 1st cursor [CRSR~] Position 2nd cursor [~CRSR] Enter new program number (O2468) Press INPUT key...

  • Page 45

    Extended Part Program Edit (Merge) If you want to insert part of a program into another program. Press soft key [MERGE]. Then move the cursor to the position at which the new information is to be inserted. And press soft key [~CRSR] or press [~BTTM] if you want the new information to be inserted ...

  • Page 46

    Extended Part Program Edit (Change) The change feature gives the operator the ability to 'Mass Edit' a program. Press the 'Change' soft key and the above screen appears. Enter the data that you want to change. e.g. F100. Then press the 'Before' soft key the screen below will be displayed. Enter t...

  • Page 47

    Background Edit Background Edit gives the programmer the ability to create a new program or edit an existing program while a program is being executed. While the machine is running press the hard key PROG then press soft key [(OPRT)] and then soft key [BG-EDT]. When you have finished using Backg...

  • Page 48

    Program Stop, Optional Stop and Block Delete M0 Program Stop. A program stop is used whenever the operator requires the program cycle to stop and allow the operator to perform some manual function such as inspection, manual tool change, coolant adjustment, etc. M1 / Optional Program Stop. This M...

  • Page 49

    Program Restart This function gives you the option of restarting a tool anywhere in a program Before starting you must set parameter 7310 X = 1 Y = 2 Z = 3 PROGRAM RESTART1) Retract the spindle, send all the axis to reference point. 2) Reset Tool. 3) Go to Edit Mode. 4) Hit Reset Button. ...

  • Page 50

    Tool Registry To access the machines tool registry SYSTEM PMC PMCPRM DATA G.DATA 450 Tool in spindle 452 Waiting tool Use the Page down key to display the complete Tool Registry on one page. Tool Registry only applies to machines with random select tool magazines. ADDRESS POCKET No ...

  • Page 51

    Changing Parameters Before changing parameters you must first enable parameter write Select MDI using the Mode Select switch. MODEMODE SELECTMDITAPEMEMORYEDITREF.RTN.JOGHANDLEPress the function key and then the [setting] soft key to display the Setting screen. Offset Setting Cha...

  • Page 52

    Sample Program In this sample program the following operations are performed. Tool 1 - 3/4" end mill, machines part profile & roughs 2" hole. Tool 2 - 5/8" Spot drill, spots all holes. Tool 3 - 27/64" drill, drills 4 holes. Tool 4 - 1/2-13 tap, taps 4 holes. Tool 5 - 1/2&q...

  • Page 53

    Sample Program Program Start O1066 (DEMO) - - - - - - - - - -- Program Number with comment N1G0G90G80G40G17- - - - - G80 & G40 Cancels any offsets stored in memory, G17 sets plane selection N2G91G28Y0Z0- - - - - - - - - - Sends Z & Y to the G28 reference position N3T1M6- - - - - -...

  • Page 54

    Sample Program Tool 2 N29M01- - - - -- - - - - - - - - - - - Optional stop N30T2- - - - - - - - - - - - - - - - - -Verifies tool 2 is in waiting pocket N31M6- - - - - - - - - - - - - - - - - Change to tool 2 ( .625 DIA. SPOT DRILL )- - - - -Tool description N32G0G54G90X-2.Y-2.S6000M3- Moves to 1s...

  • Page 55

    Sample Program Tool 4 N51M1- - - - -- - - - - - - - - - - - - Optional stop N52T4- - - - - - - - - - - - - - - - - - Verifies tool 4 is in waiting pocket N53M6- - - - - - - - - - - - - - - - - Change to tool 4 ( 1/2-13 UNC TAP )- - - - -- - - - - Tool description N54G0G54G90X-2.Y-2.- - - - - - -...

  • Page 56

    Sub Programs The control has the ability to access 'sub programs' from outside the program that is running in the control memory. This is useful when tools are using the same information when machining a part e.g. center drill, drill and tapping a number of holes. Sub programs are accessed b...

  • Page 57

    Searching Programs It is possible to search for information contained in a program. You can search Line numbers, Tool numbers, G-codes, Feedrate, etc. Select EDIT using the Mode Select switch. MODEMODE SELECTMDITAPEMEMORYEDITREF.RTN.JOGHANDLEPress the PROG hard key and the following screen will b...

  • Page 58

    Searching for a Program When there are multiple programs in the controls memory you can search for a particular program in several ways. Select EDIT using the Mode Select switch. MODEMODE SELECTMDITAPEMEMORYEDITREF.RTN.JOGHANDLEPress the PROG hard key and the following screen will be displayed. ...

  • Page 59

    Deleting a Program When no longer needed, programs stored in the controls memory can be deleted, either one at a time or all programs at once. Make sure that parameter 3202 bit 5 is set to a 1. If you do not set this parameter once you press the 'Delete' key the program is removed immediately. S...

  • Page 60

    PCMCIA Card (Memory Card) Doosan Machining Centers using the i series controls (not including the 0i) now have the ability to read from a PCMCIA card. This is a memory card and is used in the same way as you would use a 31/2” floppy. With the cards you can upload and download programs and it i...

  • Page 61

    Uploading and Downloading Programs Using the PCMCIA Card Insert PCMCIA card Select EDIT using the Mode Select switch. Press the PROG hard key then the + soft key and CARD soft key to display the following screen. To send a program to the card. Select Edit mode. Press PRGRN - OPRT - PUNCH - enter ...

  • Page 62

    DNC Operation using the PCMCIA Card Insert PCMCIA card. Select TAPE using the Mode Select Switch. MODEMODE SELECTMDITAPEMEMORYEDITREF.RTN.JOGHANDLEPress the PROG hard key then the + soft key twice and then DNC-CD soft key to display the following screen. Parameter 138 bit 7 must be set to 1 to di...

  • Page 63

    Subprogram call from PCMCIA Card You can access a program stored on the PCMCIA card at any time and use it as a subprogram. Main program Program stored on PCMCIA card (.625 DIA. SPOT DRILL) N32G0G54G90X-2.Y-2.S6000M3 N33G43Z.1H2M8T3 N34G81G98X-2.Y-2.Z-.275R.1F10. N35M198P1066- -(call subprogram f...

  • Page 64

    Uploading and Downloading programs using a Laptop computer When using suitable communication software it is also possible to load programs into the control through the RS232 connection from a laptop computer. Your communication software should match these settings. Your control parameters should ...

  • Page 65

    Restarting a program when using the PCMCIA Card You can search and restart a program which is being run from the PCMCIA card in the same manor you would if the program was running from the controls memory. Load the desired program (see page 61) Turn Single Block Switch On Press PROG hard key t...

  • Page 66

    Uploading programs using a Laptop computer To read a program from a laptop to the control. First connect the RS232 cable. Then prepare the communication software to send. Select EDIT using the Mode Select Switch. MODEMODE SELECTMDITAPEMEMORYEDITREF.RTN.JOGHANDLEPress the PROG hard key then the O...

  • Page 67

    DNC Operation using a Laptop Computer To DNC from a laptop to the control. First connect the RS232 cable. Then select the pro-gram you wish to run and prepare the communication software to send. Select TAPE using the Mode Select Switch. MODEMODE SELECTMDITAPEMEMORYEDITREF.RTN.JOGHANDLEPress the P...

  • Page 68

    RS 232-C Communication Interface Connections The cable from your computer to the machine should be wired in one of the fol-lowing configurations. 68

  • Page 69

    Additional Options Look Ahead Control (G08) This option is designed for high-speed-machining applications that require precession and accuracy. When rounding corners and curves the delay due to acceleration/deceleration in the servo system is suppressed. Use the following format to turn G08 on an...

  • Page 70

    Artificial Intelligence contour control (AICC) This option allows High-Speed, High-Precision machining without the special need for additional hardware. AICC is mainly used for mold applications. Use the following format to turn AICC on and off G05.1 Q1 - Turns AICC ON G05.1 Q0 - Turns AICC...

  • Page 71

    Programmable Data Input (G10) It is possible to write directly to the work offsets using the G10 option. This is useful when setting up a previously run part where the work coordinates are already know. To write to the G54 offset the line of information would be G10L2P1X16.234Y-3.435Z-1.0 P1 = G...

  • Page 72

    Mirror Image There are two types of Mirror Image available for the machine. One is to set the desired axis manually in the Offset Setting screen. The second is using programmable mirror image in the program (G51.1). Manual Setting Machine your 1st part and then at the end of the program move to y...

  • Page 73

    Mirror Image Programmable Mirror Image There are two ways of including Mirror Image in the program. 1. Using G51.1 2. Using M-code G51.1 (Turns Mirror Image On) G50.1 (Turns Mirror Image Off) The program format should look like this: P1066 M98 - - - Main program containing all inf...

  • Page 74

    Coordinate System Rotation By using this option it is possible to rotate a programmed shape. G68 is used to turn on Coordinate System Rotation, along with 'X' & 'Y' position which is the center of rotation and 'R' which is the angle of rotation. To use Coordinate System Rotation the program ...

  • Page 75

    Scaling Using the Scaling option it is possible to enlarge or reduce the size of a part without having to change the program. ABCIf part A is the original part size, to produce part B which is 1.5 times original. The program should look like this. G90 G0 G54 X0 Y0 (Move to center of part) G5...

  • Page 76

    Tool Life Management Tool Life Management gives the operator the ability to change a worn tool to another tool during program run without stopping the machine. Tools are classified into groups and a tool life is set for each group in either number of times used or length of time. When a tool exce...

  • Page 77

    Tool Life Management O0001 G10L3 (Sets Tool Life Management) P1L15 (Sets group 1 with a tool life of 15 uses) T1H1 (Tool # and tool length offset #) T2H2 (Tool # and tool length offset #) P2L15 (Sets group 2 with a tool life of 15 uses) T3H3 (Tool # and tool length offset #) T...

  • Page 78

    Tool Life Management To display the TLM screen press the Offset Setting hard key then the + soft key and then the TOOLLF soft key. A @ sign is displayed next to the tool that is being used. A * appears when the tool life has expired. 78

  • Page 79

    Tool Path Graphics Pressing the GRAPH hard key will bring up the Tool Path Graphic screen. Setting parameter 6500 bit 6 to 1 will always position the graphic in the center of the screen. 79

  • Page 80

    Horizontal Setup The horizontal machining center gives the operator the ability to set up multiple parts. It is also possible to machine three sides of a part in one setup. Choose a face to set all you Tool Length Offsets from. This is usually the face of the part at G54 B0. ...

  • Page 81

    Horizontal Setup All faces to be machined should be assigned there own work offset numbers. This gives better control over each work piece. G54G55G56G57G59G58B0G54 P1G54 P2G54 P4G54 P6G54 P5G54 P3B90G54 P07G54 P8G54 P10G54 P12G54 P11G54 P9B180G54 P13G54 P14G54 P16G54 P18G54 P17G54 P15B270The abov...

  • Page 82

    Horizontal Machining Example Typically when using a horizontal machining center you will be machining the same part in several locations on the tombstone. The use of sub-programs will save on program size, control memory and also make proving out the program easier. O2000 (MAIN PROGRAM) M61 (Cal...

  • Page 83

    Bore Mill Machining Example Set up and use of the horizontal boring mill is very similar to a standard horizontal machining center. The major difference is that the boring mill has a 'W' axis. When the 'W' axis is at its home position (G91G28 W0), enter this position into the work offset numb...

  • Page 84

    Macro Programming Fanuc controls have an option feature known as custom Macro. This is powerful program language that allows programs to be written using variables instead of fixed numbers. There are several ways to call a Macro program. 1. Using G65 followed by the Macro program number. e.g. G...

  • Page 85

    Macro Programming This Bolt Hole Macro allows for quick and easy programming of a bolt hole circle without the operator having to calculate the position of each hole. The line of information in the program to call this macro should look like this: G100 X0.0 Y0.0 Z-.750 D2.0 R.1 C83. A45. H4. F20....

  • Page 86

    Macro Programming (Circular Pocket) The line of information in the program to call this macro should look like this, G102 X0. Y0. Z-750 R1. A.05 I.02 J.02 K.25 W.8 C5.0 D3 F20. X X axis center Y Y axis center Z Depth of pocket R Radius of pocket D Direction of cut. D2 CW / D3 CCW C Feedrate for p...

  • Page 87

    Milling Formulas The following formulas are used to calculate speed and feeds, metal removal rate, surface feet per minute and horse power used. Symbols and Measurement Units D = diameter of milling cutter (inches) d = depth of cut (inches) F = feed rate (inches per minute) f = feed (in...

  • Page 88

    Trouble Shooting 88

  • Page 89

    Side Mounted Tool Changer Recover This is the procedure for recovering a side mounted tool changer should the machine loose power or if the tool is inadvertently load wrong. 1. Restore Power (It is not necessary to Zero return the machine) 2. On the Automatic Tool Changer (ATC) box at the bac...

  • Page 90

    Horizontal Machining Center Tool Changer Recover (DHP and DHC 400) During a normal tool change (1) Next tool is placed in spindle. (2) Tool from spindle is returned to waiting pot. (3) Tool is returned to correct pocket in magazine. After this ...

  • Page 91

    Horizontal Machining Center Tool Changer Recover (DHP and DHC 400) Occasionally due to tool changing errors (2) pots will be in the waiting pot position. For this example we have T5 in the spindle and T10 as the waiting tool. The Pot position's were the spindle tool and waiting tool came from ...

  • Page 92

    DHP-500 and 630 Tool Change Recovery This is the procedure to recover the Tool Changer should the machine loose power during a tool change or if a tool is inadvertently loaded wrong. 1. Restore power. 2. Set Mode switch to Jog. 3. Make sure that the ATC box is connected to the tool changer ...

  • Page 93

    DHP-500 and 630 Pallet Change Recovery This is the procedure to recover the pallet changer should the machine lose power during a pallet change. 1. Restore Power. 2. Set Mode switch to Jog. 3. Make sure that the APC box is connected to the pallet changer, and set to Manual. 4. On APC box se...

  • Page 94

    CAT 50 PULL STUD This pull stud will fit all 50 taper Doosan Machining Centers. Dimensions are for reference only. Part No 316-45 (With through hole) 311-18 (No through hole) To Order Call: Retention Knob Supply Company Tel: 937-686-6405 ...

  • Page 95

    CAT 40 PULL STUD This pull stud will fit all 40 taper Doosan Machining Centers. Dimensions are for reference only. Part No 711-23 (With through hole) 711-25 (No through hole) To Order Call: Retention Knob Supply Company Tel: 937-686-6405 Fa...

  • Page 96

    BT 30 PULL STUD This pull stud will fit all 30 taper Doosan Machining Centers. 25mm18 mm11mmM12 x 1.757mmDimensions are for reference only. Part No 311-09H (With through hole) To Order Call: Retention Knob Supply Company Tel: 937-686-6405 Fax: 937-686-4125 96

  • Page 97

    Heavy Tool Limitations Before using a heavy tool you must first calculate the tools 'Moment' before attempting a tool change. This should not exceed the machines maximum tool weight. Weight CenterTaper Gage LineCalculate the tools 'Moment' as follows 1. Find the tools center of gravity 2. Measur...

  • Page 98

    Uses of Large Tool The following method is recommended when using a large diameter tool. Empty PocketsTool's with numbers 70 and higher are considered 'large Tools'. Before you start to use a large tool you must first set the 'Tool Registry'. To access the Tool Registry see page 50 When loading...

  • Page 99

    Lubrication Requirements The following is a list of oils used on Doosan machining Centers. Way Lube 'G' Oil Hydraulic 'B' Oil Spindle Cooler 'A' Oil Grease 'Y' Oil Air Service Unit 'B2' Oil Table 'E' Oil Mold cut on DMV 3016LS In 1 Hour 32 minutes. H13 Tool Steel RC50 Comparative Oils ...

  • Page 100

    Absolute and Incremental Programming Example X+Y+DatumAnswers from page 17 ABSOLUTE (G90) INCREMENTAL (G91) A X 4.000 Y-2.000 A X4.000 Y-2.000 B X 8.000 Y-3.000 B X4.000 Y-1.000 C X 1.000 Y-6.000 C X2.000...

  • Page 101

    Index A. Axis Movement - 7 Absolute Coordinate Programming (G90) - 16,17 Additional Options - 69 Artificial Intelligence Contour Control (AICC) - 70 Artificial Intelligence Advanced Preview Control (AI APC) - 70 B. Boring, Fine Boring (G76) - 32 Back Ground Edit - 47 Block Delete - 4...

  • Page 102

    E. Extended Part Program, Edit - 43 Move - 44 Merge - 45 Change - 46 F. Fixed Cycles - 28,33 G. G - Codes (Most Commonly Used) - 4 Graphics (Tool Path) - 79 H. High Speed Peck Drilling (G73) - 28 Helical Interpolation - 37,38 Horizontal Machining Center Setup - 80,81 Horizo...

  • Page 103

    M. M-Codes (Most Commonly Used) - 5 M.P.G (Manual Pulse Generator) - 8 M.D.I (Manual Data Input) - 39 Memory Card - 60 Milling Formulas - 87 MBL APC (Multi Block Look-a-head Advanced Preview Control) - 70 Mirror Image - 71,73 Macro Programming Example - 84,86 N. O. Optional Stop - ...

  • Page 104

    P. Continued, Restarting a program - 64 Programmable Data Input (G10) - 71 Pull Studs - 93,95 Q. R. Radius Command - 22 Rapid Plane - (G99) -27 Rigid Tapping - 33 Rigid Tapping Using an Alternative Axis - 34 Repetition of canned cycles (L) - 35 Restart - 49 RS231C Communication - 6...

  • Page 105

    T. Continued, Trouble Shooting, Side Mounted Tool Changer - 88 Horizontal Tool Changer (400 series) - 89,90 Horizontal Tool Changer (HP500/630) - 91 Pallet Recovery (HP500/630) - 92 Heavy Tool Limitations - 96 Uses of Large Tool - 97 U. Uploading from PCMCIA Card -61 Uploading fr...

  • Page 106

    Phil Misseldine Applications Engineer Machining Centers Doosan Infracore America Corporation 8 York Avenue West Caldwell, New Jersey 07006 Main Tel: 973-618-2500 Direct: 973-618-2436 Fax: 973-618-2472 E-mail: phil.misseldine@dhiac.com 106 04202007

x