Navigation

  • Page 1

    1 NC-Programming Manual for Turning Centers with Fanuc 30 Series Controls

  • Page 2

    2 1 _____________________________________________________________________________________ 5 Meaning of addresses ____________________________________________________________________ 5 Tool Number Designation _________________________________________________________________ 2 2 Introduction to ...

  • Page 3

    3 7.4 Work Coordinate System ______________________________________________________ 24 7.5 Work Offsets & Work Coordinate Systems ________________________________________ 25 7.6 Work Coordinate System Grid __________________________________________________ 26 7.7 Absolute Coordinate Command _...

  • Page 4

    4 14.5 G74 Peck Drilling & Face Grooving (trepanning) On The Z Axis _____________________ 67 14.6 G75 Peck Grooving on the X Axis _______________________________________________ 70 15 Thread Cutting Cycles ______________________________________________________________ 72 15.1 Thread Cutting L...

  • Page 5

    5 Meaning of addresses Function Address Meaning of address Program number O(EIA / ISO) Program number Block sequence number N Sequence number Preparatory function G Specifies a motion or function X, Z Command of moving position (absolute type) of each position U,W Instruct moving dist...

  • Page 6

    2 Tool Number Designation T Function is used for the designation of tool numbers and tool compensation. T Function is a tool selection code usually made of 4 digits. T 0 2 0 2 Designation of tool offset compensation number Designation of tool number Example: If th...

  • Page 7

    1 2 Introduction to NC-programming To write a program for the NC means to translate all of the action that is required for machining a work piece into a language format that the control can understand. NC programming is done in an internationally standardized language that consists of coded text...

  • Page 8

    2 The program-text is input to the NC-memory by using the keypad as provided on the system. It is also possible to upload a program text file that has been created on a personal computer by connecting a PC to the RS-232 communication interface device at the NC unit. The FANUC 18-I, 21-I and 30i ...

  • Page 9

    3 2.2 How to key-in a program on a FANUC control 1. Switch the mode selector to “EDIT”-mode 2. Memory-protect key in OFF position 3. Press the “PROGRAM”-key. Now, either the program “TEXT” of an existing program is displayed or the program “DIRECTORY” is displayed. Pressing the ...

  • Page 10

    4 3 List of Commands used in NC-Lathe programming This chapter provides an overview of the basic commands and function codes that are used in NC-programming. 3.1 Addresses A NC-address consists of a single letter that addresses an assigned function on the control system. The table below expla...

  • Page 11

    5 Function Address Application / Use Machine function M M8; Used for activating various machine functions, such as spindle, coolant, etc. (See M-code list for details) Search function P Used for sub program call M98P_ and for sequence number search command M99P_. Dwell function P,U Dwell comman...

  • Page 12

    6 3.3 Blocks One or more words make up a command-line that is referred to as a block. A block may contain as many words as is required in order to specify different types of commands at the same time. This is a block: When the data is processed by the control the whole block is read at once...

  • Page 13

    7 3.6 The use of decimal fractions in programming In words with addresses G, L, M, N, O, P, Q, S, T the use of a decimal point is prohibited. Whole numbers must be commanded only. Example: P1. Cannot be commanded. Command P1 S499.5 P11 cannot be commanded. Command S499 P11 or S500 P11 In...

  • Page 14

    8 3.7 Suppression of Leading or trailing Zero Data format on older NC systems (prior to around 1982) used to require a fixed number of digits for NC-words. Systems manufactured after around 1982 do not require this type of format any longer. It is not necessary to place a zero in front or at ...

  • Page 15

    9 3.9 Optional Block Skip Character, “/ “Slash Placing a slash “/” at the beginning of a block allows optional skipping (not executing) of the commands specified on that block. A switch located on the operation panel controls the skip function. Switch ON = skips the block, switch OFF ...

  • Page 16

    10 For example: Once G98 has been commanded the inches per minute feed mode remains active in every block. It’s not necessary to repeat the command. The G99 command cancels the G98-mode. Once a specific feed rate has been commanded it remains active until replaced with a different feed rat...

  • Page 17

    11 3.11 Spindle Command A numerical value following the address “S” sets the spindle speed. There are two different types of spindle control modes available. The spindle control mode is set by these G-codes: G96 = Constant surface speed control mode G97 = RPM control mode The command: G...

  • Page 18

    12 The G50 S-command is valid only during G96-mode. “G50 S1200 P11” does not override a “G97 S2000 P11” -command. The G50 S-command is modal. 3.12 Tool Command A tool command consists of the Address “T” followed by a number ranging from 0 to around 1232. The upper limit of the ran...

  • Page 19

    13 NO. offset # X X axis offset Z Z axis offset R Tool nose radius T Tool nose vector 01 1.75 -.025 .0312 3 02 Tool offsets are important for size control of the part to be machined. After a part has been machined and inspected for dimensional accuracy, any size correction that might be nee...

  • Page 20

    14 4 Tool Nose Radius Compensation Most carbide turning tool inserts employ a tool nose radius at the tool tip for the purpose of increasing tool life. Standard radii range from 1/64" up to 3/32" in 1/64th increments, typically. In some cases, radius- grooving tools are used for mach...

  • Page 21

    15 G41 = Tool nose radius compensation – left G42 = Tool nose radius compensation - right Geometry of a tool path that has been programmed using the actual part dimensions can be produced correctly when the automatic tool nose radius compensation function is applied. Rules to apply in the u...

  • Page 22

    16 4.2 Tool Nose Radius Compensation Data Tool nose radius compensation is stored in the tool-offset tables under the columns “R” and “T”. The tool offset that stores the TNR COMP data for the tool in use must be activated by the tool command, otherwise no compensation is possible. Tool...

  • Page 23

    17 G-codes activate various types of control functions or set modes of operation. G-codes are subdivided into groups or families, by function- type as shown in the table, below. Special Notes on G-Codes The following G-codes are active upon initial power-up of the control: G0, G18, G22, G40, ...

  • Page 24

    18 5.1 G-Code List (G-code system A, partial listing) G Code Group Modal Function G00 01 Yes Rapid traverse G01 01 Yes Linear interpolation G02 01 Yes CW Circular interpolation G03 01 Yes CCW Circular Interpolation G04 00 No Dwell G10 00 Yes Data Setting G11 00 Yes Data Setting cancel G17 16 Ye...

  • Page 25

    19 6 Miscellaneous Functions, “ M “-codes Please note that M-codes may vary from one machine tool builder to another. Most of the M-codes shown on the list shown below are generally valid for PUMA Turning Centers only. M0 through M9 may apply for other brands of turning centers, as well. O...

  • Page 26

    20 M-Code Description Spec. M51 Bar Feeder Command 2 OptionM52 Splash Guard Door Open OptionM53 Splash Guard Door Close OptionM54 Parts Count OptionM58 Steady Rest Clamp OptionM59 Steady Rest Unclamp OptionM61 Switching Low Speed M62 Switching High Speed M66 Main CHUCKING LOW PRESSURE ...

  • Page 27

    21 7 Coordinate Systems 7.1 Basic Coordinate System Shown below is a standard two-dimensional coordinate system where the X-axis runs in horizontal direction and the Y-axis in vertical direction. X is the first and Y is the second axis in the basic coordinate system. In NC-lathe programming a ...

  • Page 28

    22 The sketch below shows the standard two-axis NC-lathe-coordinate system in a two-dimensional view in which the X-axis runs vertically and the Z-axis horizontally. The point X0, Z0 is called the ORIGIN or ZERO-POINT of the coordinate system. X-axis coordinates represent diameters on a part. ...

  • Page 29

    23 7.3 Machine Coordinate System The origin or zero point of the machine coordinate system is normally located at the intersection of the main-spindle center axis (X0) and the spindle flange face (Z0). This point serves as a “hard” reference for calibration of the turret “HOME-position”....

  • Page 30

    24 7.4 Work Coordinate System The ORIGIN of the coordinate system used for programming is established at a specific point on the part to be machined. This is called the WORK ZERO POINT. The coordinate system used in a NC-program is called the WORK COORDINATE SYSTEM. The X-axis work zero point...

  • Page 31

    25 7.5 Work Offsets & Work Coordinate Systems Older NC-lathes are equipped with a single work offset register, known as the “WORK SHIFT”. The work-offset distance is entered into the work shift register. This will set the origin of the “Work Coordinate System” or the program zero...

  • Page 32

    26 7.6 Work Coordinate System Grid The sketch below shows a coordinate system grid that is applicable for a turning center equipped with a turret. The turret is located on the “top right hand side” of the spindle, or on the opposite side of the spindle center as seen from the operator. On t...

  • Page 33

    27 7.7 Absolute Coordinate Command A distance measured from the zero point to any point in the coordinate system is called an ABSOLUTE Dimension. Once the work zero point has been established the coordinates used for programming are referenced to that point. For programming of the tool path tha...

  • Page 34

    28 An incremental dimension is a distance measured from a point in a coordinate system to another point. Dimensioning found on a shop drawing is not always convenient for use in NC-programming. When absolute coordinate commands (X, Z,) are used all dimensions need to be referenced to the origin...

  • Page 35

    29 7.9 Absolute & Incremental Command in same Block Absolute & incremental coordinates can be specified together in the same block. For example: X3.395 W-3.0 Or: U1.625 Z-3.459 8 Positioning 8.1 G0 – Positioning in the Work Coordinate System Format G0 X (U) Z (W) Rapid traverse-m...

  • Page 36

    30 As illustrated in the sketch, positioning is not necessarily done in a straight line from point A to point B. Positioning speed of both axis servos is about the same. In this case the travel distance along the X-axis is shorter than along Z. X arrives at the destination before Z. In order to...

  • Page 37

    31 9 Interpolation Function 9.1 G1 - Linear Interpolation Format = G1 X (U) Z (W) F - This commands a linear move at a feed rate. Linear interpolation means that both axes, X and Z will arrive at the commanded point at the same time. The tool path as shown above is accomplished by linear inte...

  • Page 38

    32 9.2 G2 - Circular Interpolation Clockwise Format = G2 X (U) Z (W) R_ F_ -Circular move (CW) at a commanded feed rate. Start-point of arc: X1.0 Z0 Circular interpolation command: G2 X5.0 Z-2.0 R2.0 F0.005 Or: G2 U4.0 W-2.0 R2.0 F0.005 9.3 G3 - Circular interpolation Counter Clockwis...

  • Page 39

    33 For circular interpolation in general, please note the following: Feed rate must be commanded or a feed rate must be active (modal) when G2 or G3 is commanded. G2 and G3 are modal. Circular interpolation starts from the current position of the tool. The commanded position in the G2 or G...

  • Page 40

    34 9.4 Circular Interpolation using arc center point specification Format: G3 X (U) Z (W) I_ K_ F_ Arc shown in the sketch: Start-point of arc: X5.0 Z0 G3 X6.0 Z-4.0 I-1.75 K-2.25 F0.005 Notes: “I” and “K” specify the location of the arc-center relative to the start point of the ar...

  • Page 41

    35 9.5 Chamfering & Corner Rounding Function (using Addresses “C” , “R” ) A 45-degree chamfer or a 90-degree arc can be produced when a surface parallel to X and an adjacent surface parallel to Z is machined in two consecutive blocks during G1-mode. The ch...

  • Page 42

    36 9.6 Chamfering Function (using Addresses “ I ”, “K”) A chamfering function similar to the function described in the previous chapter is available, using the addresses “I” or “K”. A 45-degree chamfer can be produced when a surface parallel to X and an adjacent surface parallel...

  • Page 43

    37 9.7 Thread Cutting Function (G32) The G32-command is used for various types of thread cutting applications. This thread cutting function works similar to the linear interpolation function, G1, except that in G32-mode the rotation angle of the main spindle and the starting of the feed motion a...

  • Page 44

    38 In the block with the G32-command the feed rate “F” specifies the Lead of the thread in inches per revolution. “Inch-Standard” threads are normally specified by thread size and by the Pitch of the thread. Pitch, meaning the number of threads per inch, abbreviated “TPI”. For a th...

  • Page 45

    39 Programming of a thread requires some machining skills and experience. The following important factors must be considered when programming a thread: Type of material to be cut Thread shape or form Thread lead and thread height Mechanical strength of the work-piece Selection of the cut...

  • Page 46

    40 Leading edge cutting Leading edge cutting means that after the first pass only the left edge of the tool does the cutting. This is accomplished by shifting the Z-axis start position of the tool toward the thread with every pass. For V-shaped thread forms the leading edge cutting method work...

  • Page 47

    41 9.8 Tapping In theory, the G32 thread-cutting function can be applied for tapping when the optional canned cycles for tapping (G84 and M29-rigid tapping option covered in a different section in this manual) are not available. When using the G32 function for tapping a floating tap holder is ...

  • Page 48

    42 See point “B” shown in the sketch below. Subsequently the move to the reference point is done in rapid traverse mode. Caution must be used with the G28 X__ Z__ (absolute command). The point X, Z, as specified must be clear of the work piece. 10.2 G30 - 2nd Reference Point Return (Rapid ...

  • Page 49

    43 Caution must be used with the G28 X__ Z__ (absolute command). The specified point X, Z, must be clear of the work piece, without fail. 11 Standard Program Format O1234; LETTER O FOLLOWED BY A 4 DIGIT PROGRAM NUMBER G50 S-----; SETS A MAXIMUM ALLOWABLE CHUCK RPM IN G96 MODE N100 T0101 ...

  • Page 50

    44 M4 P11= SPINDLE REVERSE G00 X_____ Z_____ G41/42; RAPID UP TO PART AND ADD CUTTER COMP. ------------------------------------------------------------------- MACHINING INSTRUCTIONS ------------------------------------------------------------------- G00 G40 X_____ Z_____ ; RAPID BACK TO TH...

  • Page 51

    45 12 Sub Programs Programs can be created for various types of operations or routines that can be used repetitively. For example: Sub programs for operations such as bar pulling or bar feeding, repetitive grooving, contouring or hole drilling routines, etc. can be stored in the NC-memory. When...

  • Page 52

    46 12.2 Sub program Repetition When a routine needs to be repeated several times consecutively, the letter “L” specifies the repetitive count. When L is omitted, the sub program is executed once only. For example: M98 P1234 L5 (L5= Repeat program # 1234, 5 times) Some older controls such a...

  • Page 53

    47 13 Simple Canned Cycles for turning (G90) The G90 canned cycles perform a box pattern consisting of in-feed, retract and returning the tool back to the initial start position by specifying one block of information only. 13.1 G90 Canned Turning and Boring G90 is a straight box turning cycl...

  • Page 54

    48 Notes on using G90 canned cycles for turning and boring O. D. Turning I.D. Turning Positioning, G00 to start point X axis .2" larger than stock diameter X axis .2" smaller than bore diameter Z axis in front of Work piece by .1000" G90 turnin...

  • Page 55

    49 It is possible to use the G90 command and vary your endpoint of the Z-axis. The cycle time can be reduced by commanding a G0 with the X axis .05 larger than the cutting diameter. This will let the tool rapid back to its starting position in Z. G0 X4.1 Z.1 G90 X3.8 Z-1.4...

  • Page 56

    50 G0 X3.85 ───────────────┐ G90 X3.6 Z-1.4 F.015 │ G0 X3.65 ───────────────┤ G90 X3.4 Z-1.4 F.015 ├────────── Here the X axis is commanded to a G0 X3.45 ───────────────┤...

  • Page 57

    51 13.2 G90 Canned Cycles for Taper Turning and Boring Taper cutting can be specified using the G90 cycle by the following syntax: G90 X__ (or U) Z___ (or W) R___ F___; In the above example the new variable is R, this is used to specify the direction and amount of taper, the taper is specif...

  • Page 58

    52 13.3 G94 Canned Facing G94 is a box turning cycle that will permit the programmer to execute facing cuts on the part. The syntax is as follows: G94 X(U) Z(W) F X X coordinate of order point relative to X0 (U) Incremental dimension of order point relative to the start position on X ...

  • Page 59

    53 Notes on using G94 facing Positioning - G0 To Start Point X axis, approximately .2" larger than the work piece Z axis, approximately .1" in front of the work piece Facing cycle, G94 Order point at smaller diameter than at start point

  • Page 60

    54 13.4 G94 Canned Cycles for Facing on a Taper The G94 can be programmed to execute a taper cutting action, the syntax for doing this is as follows: G94 X(U) Z(W) R F In the above example the new variable is R, this is used to specify the direction and amount of taper, the taper is specifie...

  • Page 61

    55 14 Multiple Repetitive Cycles Multiple repetitive cycles allow the programmer to write programs for complex shapes while keeping the number of program lines down to the absolute minimum. The programmer will typically write a line that contains various cutting parameters and after that will w...

  • Page 62

    56 14.2 G71 Turning – Boring Roughing Cycle G71 permits the rough machining of a contour along the Z-axis from a solid blank of material leaving a allowance of stock on the X & Z-axis to be finish machined afterwards. The syntax is as follows: G71 U R G71 P Q U W F U = the depth of cut...

  • Page 63

    57 Tool path of G71 Cycle 1) Rapid from start point of tool towards the diameter specified in P by the stated depth of cut. 2) Feed parallel to the spindle axis to a point in the programmed contour minus the value W. 3) Retract the tool at a 45-degree angle to clear the tool out of the cut, th...

  • Page 64

    58 Notes on using G71 turning - boring OD Turning ID Boring Rapid Positioning G00 X axis to the largest diameter to be turned X axis to the smallest diameter to be turned Z axis .1" in front of Work piece Z0 Z axis .1" in front of Work piece Z0 First Line Of Contour Description Ra...

  • Page 65

    59

  • Page 66

    60 14.3 G72 Facing G72 permits the rough machining of a contour along the X-axis from a solid blank of material leaving a allowance of stock on the X & Z-axis to be finish machined afterwards. The syntax is as follows: G72 W R G72 P Q U W F W = the depth of cut for each roughing pass, th...

  • Page 67

    61 Tool path of G72 Cycle 1) Rapid from start point of tool towards the diameter specified by “R” stated depth of cut. 2) Feed perpendicular to the spindle centerline to a point in the programmed contour minus the value W. 3) Retract the tool at a 45-degree angle to clear the tool out of the...

  • Page 68

    62 Notes on using G72 turning - boring OD Turning ID Boring Rapid Positioning G00 X axis approximately .2" larger than the stock diameter X axis approximately .2" smaller than the stock diameter Z axis .1" in front of Work piece Z0 Z axis .1" in front of Work piece Z0 Fir...

  • Page 69

    63

  • Page 70

    64 14.4 G73 Turning - Boring, Pattern Repeating The G73 cycle permits the removal of stock in a fixed pattern cycle leaving a specified amount of stock for a finish pass. This is most often used with a casting or forging. The contour will be generated in a number of passes determined by the pro...

  • Page 71

    65 Tool path of G73 Cycle OD Turning ID Boring Rapid Positioning G00 X-axis to the largest diameter to be turned X-axis to the smallest diameter to be turned Z-axis .1" in front of Work piece Z0 Z-axis .1" in front of Work piece Z0 First Line Of Contour Description Rapid move in X to ...

  • Page 72

    66 14.5

  • Page 73

    67 G74 Peck Drilling & Face Grooving (trepanning) On The Z Axis The G74 command can be used both as a peck drilling cycle (to break chips) and as a face grooving cycle (to "pocket out" a groove area larger than the groove tool). The syntax for peck drilling is as follows: G74 R ...

  • Page 74

    68 The syntax for G74 trepanning is as follows: G74 R G74 X Z P R (first line) = retraction amount after each peck, no decimal, this setting will over ride parameter #5139 X = final diameter (note 1) Z = depth of groove P = step over amount, no decimal point Q = depth of each peck, n...

  • Page 75

    69 Example #2 G0 X3.5 Z.1 G74 2.3 Z-.5 P3000 Q1000 G0 G40 X(. Z5. T900 M1

  • Page 76

    70 14.6 G75 Peck Grooving on the X Axis The G75 command can be used both as a peck drilling cycle (to break chips) and as a face grooving cycle (to "pocket out" a groove area larger than the groove tool). The syntax for peck grooving is as follows: G75 X Z P Q F X = bottom of groo...

  • Page 77

    71 Example #2 G00 X2.9 Z-.625 G75 X2.2 Z-2.175 P.1 Q.45 F.002 (note 1) G0 G40 X7. Z6. T900 M1 Note 1: Z-.625 = .5 + .125

  • Page 78

    72 15 Thread Cutting Cycles By programming a single point tool to feed axially over the same point again and again a thread will be cut. Three thread cutting cycles are provided: G32, G92 and G76. When these are used, each tool path will start out at the same point. Threading must be done in G9...

  • Page 79

    73 15.2 Imperfect Thread Calculation When threading it is important to take into consideration the distance needed for the acceleration and deceleration of the cutting tool while it is in the work piece. The cutting tool should be positioned far enough in front of the start of the thread to a...

  • Page 80

    74 15.3 G76 Thread Cutting, Multiple Repetitive The G76 command is a two-line call out the same as all multiple repetitive cycles. However by setting certain parameters you can eliminate the first line. However the program will then not dictate these values the parameters will. If you need to...

  • Page 81

    75 The correct syntax for the second line is as follows: G76 X Z P Q F X = for OD threads, the minor diameter, for ID threads, the major diameter. Z = the endpoint of the thread in the Z-axis. P = height of a complete thread, radial, no decimal point (note 1) Q = depth of first cutting pass, n...

  • Page 82

    76 Tool-path of G76 cycle, OD thread: 1- Rapid to major diameter, minus 2*D 2- Thread to Z axis dimension, first pass 3- Rapid out to start point diameter 4- Rapid to start point Z 5- Rapid to diameter for second pass 6- Thread to Z-axis dimension. 7- Sequence is repeated until thread reache...

  • Page 83

    77 Example of two line G76 Thread = 2 – 18 Pitch = .0555 Major Diameter = 2.0 Number of Finish Passes = 3 Minor Diameter = 1.9302 Chamfer Amount = 0 (pull straight out) Radial Height of Thread = .0349 G0 X2.1 Z.2 rapid to clear stock G76 P030060 G76 X1.903 Z-.8 P349 Q120 F.0555 G0 X9. X5. ...

  • Page 84

    78 15.4 G76 Thread Cutting, Multiple Repetitive, Taper By adding address R to the standard G76 line along with a numerical value taper threads can be generated. G76 X Z R P Q F R = is the difference in diameter from the Start point of the tool at the beginning of the tapered thread to the end ...

  • Page 85

    79 15.5 G76 – THREADING CYCLE – TWO LINE FORMAT (FS 0,16,18,21T,31i,32i, -FORMAT) (Applicable with Fanuc Controls, T series, systems 0,16,18,21,31i,32i. Also: Mitsubishi 500L, 50, 64) FIRST COMMAND LINE: G76 P021060 Q05 R10 (See detailed explanation, below) P 02 10 60 Specify “P”, foll...

  • Page 86

    80 1.) Upon execution of the G76-cycle all data contained on the first G76-command line is automatically stored in the parameter tables. 2.) Values for “P” and “Q” to be specified without decimal point for all Fanuc Controls. For example: 0.0001”=1, 0.001”=10 0.01”=100 0.1...

  • Page 87

    81

  • Page 88

    82 G76 – THREADING CYCLE - SINGLE LINE FORMAT - (FS 15T-FORMAT) (Applicable with Fanuc Controls, T series, systems 10, 11, 12 AND 15T) This format can also be used with Fanuc Controls, T series, system 0, 16,18,21 and 30 series, when the tape format setting option is available. I this case, pl...

  • Page 89

    83 15.6 Programming Examples, using the G76-Thread Cutting Cycle Example 1: Cutting a 1”-10 UNS -external thread: Action Program 1. Enter modal commands G0 G18 G40 G97 G99 2. Enter the tool and tool offset command T0101 3. Enter the Spindle command (Always use G97, NEVER G96) G97 S100 M3 (M...

  • Page 90

    84 Example 2: Cutting a 1”-10 UNS -internal thread: Action Program 1. Enter modal commands G0 G18 G40 G97 G99 2. Enter the tool and tool offset command T0101 3. Enter the Spindle command (Always use G97, NEVER G96) G97 S100 M3 (M4)P11 4. Turn ON the coolant M8 5. Move the tool to the start p...

  • Page 91

    85 15.7 G76 Thread Cutting, Multiple Repetitive, Multi Start Multiple start threads are possible in the G76 mode, you have to shift the starting point for the extra threads by 1/n of the pitch. Example Cut 5" - 4TPI, 3 start G0 X5.1 Z.15 rapid to start of thread G76 X4.9633 Z-1.4 P1534 ...

  • Page 92

    86 15.8 G92 Thread Cutting The G92 command will drive the cutting tool in a "box" pattern. Straight threads can be cut using the following command: G92 X Z F Q X = the diameter that you are cutting the pass at Z = the endpoint of the threading pass F = the feed rate (pitch) of ...

  • Page 93

    87 Notes on using G92 threading cycle Rapid move to start point OD Threading ID Threading X axis approx. .1" larger than major thread diameter X axis approx. .1" smaller than minor thread diameter Z axis, in front of thread by at least 2 threads G92 Threading Cycle Order point is smal...

  • Page 94

    88 15.9 G92 Thread Cutting, Taper By adding address R to the standard G92 line along with a numerical value taper threads can be generated. G92 X Z R F R = is the deference in diameter from the beginning of the tapered thread to the end of the tapered thread. This is expressed radial. The valu...

  • Page 95

    89 16 Canned Cycles for hole machining (G80 Series) Canned cycles for hole machining are optional equipment. Most of the older FANUC controls are not equipped with this option. On a 2-axis turning center, the following canned cycles can be used: 1. G83 (Z-axis Peck Drilling Cycle) 2. G84 (Z-...

  • Page 96

    90 EXAMPLE 1: G83 (Z-axis Peck Drilling Cycle) Program Text Explanation O4513(DRILL DIA .3125 x .75 DEEP) T0303 Get tool #3 and offset #3 G97S750 M3 P11 Spindle speed 750 RPM, CW G0 Z0.15 M8 Tool approach & Coolant ON X0 Tool at center of spindle G99G83 Z-.750 Q2500 F0.005 Peck drilling 0...

  • Page 97

    91 G87 X-axis Peck Drilling Cycle with Live Tools FORMAT: G87 X___ Q___ F___ P___ X = End position at depth of hole (X-Diameter) Q = Peck distance, number without decimal point F = Feed rate P = Dwell time at bottom of hole, in milliseconds, without decimal point NOTES: 1. Position the too...

  • Page 98

    92 17 Miscellaneous Settings 17.1 Instructions for Setting the Work-Zero Point on Lathes with Fanuc 18T 21T, Or 30 Series Controls. Every CNC-lathe has one basic coordinate system that remains fixed and cannot be changed. This is known as the “Machine Coordinate System”. The origin or zero po...

  • Page 99

    93 Depending upon programming method applied the work zero point “Z0” may be located at an arbitrary point along the z-axis of a work-piece, while “X0” is always located at the center axis of the spindle. Thus, the X-register for all work offsets must always remain zero. The work zero ...

  • Page 100

    94 17.2 Work-offset setting procedure for lathes equipped with Q-setter. 1. Every tool attached to the turret must be touched-off at first, using the automatic tool setter (Q-setter), before setting the work zero point. 2. The raw material for the work-piece to be machined is placed into the ch...

  • Page 101

    95 completed press the “OFFSET”-key, then the software-key “WORK”. Now the screen as shown on page 1 above will appear. 7. Move the yellow cursor onto the Z-data field on the “G54” -work offset. Press the “Tool Measure-Key” on the operation panel for two seconds. 8. Now, key-in ...

  • Page 102

    96 17.5 Changing Parameters on 16/18TC and 30 Series Controls 1- Select mode push button for MDI 2- Set program protect key to OFF 3- Press <OFFSET /SETTING> key on panel until <SETTING HANDY> screen is displayed 4- At Parameter Write Enable, key in <1> and press <input>....

  • Page 103

    97 18 Operator's Control Panel The machine is controlled by the various keys and switches located on the operation panel. MODE PUSHBUTTON SWITCHES - Use this to select the desired operating mode Edit Mode - Edit mode is used to enter a new program into memory whether by keyboard or downloadi...

  • Page 104

    98 a relatively slow speed as set by parameter #1421. F25 will move at 25% speed, F50 will move at 50% speed and F100 will enable 100% of the rapid feed rate as set by parameter #1420. Feed rate Override Dial - While the machine is in operation, you may alter the current programmed feed rate. Yo...

  • Page 105

    99 The feed override switch controls feed velocity in dry run mode. Use DRY RUN for tool path verification only, without actually machining a part. <Tool Measure> - Press this first when setting Tool Offsets and the Work shift Zero (see sections 14 & 15). Coolant Pushbutton - Allows ...

  • Page 106

    100 NC Programming for Turning Centers For 30 Series Control single path machines Equipped with Live Tools & C- Axis

  • Page 107

    101 ROTARY AXIS FUNCTIONS When machining with live tools a rotary-axis allows angular positioning of the work piece between zero and 360 degrees. The CNC system converts one of the lathe spindles into a rotary axis. C - Axis PUMA Turing centers equipped with a turret and driven tools normally ...

  • Page 108

    102 Front view of Lynx 220LM Feed Rate Calculation for the Rotary Axis The feed rate for a rotary-axis is specified in units of angular velocity, either in degrees per minute or in degrees per tool revolution. To convert the tangential feed rate on the circumference of a circle that is def...

  • Page 109

    103 Feed Rate Calculation for Linear Interpolation with Rotary Axis Caution concerning the feed rate must be applied when linear interpolation between the rotary axis and the Z-axis is done. The tangential feed rate along the tool path becomes high when the arc length of the rotary axis move is ...

  • Page 110

    104 SPINDLE MODE AND ROTARY AXIS MODE COMMANDS For PUMA Lathes, equipped with a C-axis, the program commands as shown below apply. Commands are shown for turning mode and for live tool mode, separately. Main Spindle Mode (C-Axis Disconnected) For turning operations on the main spindle, the comma...

  • Page 111

    105 Command Remarks M05 P12 Live tool spindle rotation-stop command . G0 G40 G80 Use these G-codes at the beginning of any program segment where “Canned cycles” G81through G88 or cutter compensation G41, G42 is used. M90 C-axis unclamp-command. Use at the beginning of any program segment whe...

  • Page 112

    106 ANGULAR POSITIONING FUNCTION FOR SPINDLES Angular positioning function for spindles can be utilized for machining with live tools. Angular positioning is applied typically on the sub spindle for the PUMA MS-series turning centers. Spindle orientation When the spindle orientation option is p...

  • Page 113

    107 Once commanded, the spindle is held in position under power by the spindle motor. The M3, M4 or M5-command cancels spindle positioning. System parameter 4077 S-1 sets the reference angle for the main spindle.

  • Page 114

    108 DRILLING AND TAPPING WITH LIVE TOOLS ON THE C-AXIS Canned cycles for hole machining with the C and Z-axis Z-axis peck drilling, C-axis positioning G83 C___Z___Q___ P___F___ Z-axis tapping G84 C___Z___F___ Notes: C = C-axis position, X = X-end position, (diameter), Q = peck distance ...

  • Page 115

    109 G0C0Z.5 X1.5 M8 X1.5 M8 Z.1 Z.1 G97S1000M29P12 G83C0Z-.45.Q1250F.005M89 G84C0Z-.35F.05M89 C90.Q1250M89 C90. M89 C180.Q1250M89 C180. M89 C270.Q1250M89 C270.M89 G0G80Z.5M90 G0G80Z.5M90 X8.Z4.M5P12 X8.Z4.M5P12 M1 M1

  • Page 116

    110 Canned cycles for hole machining with the C and X-axis X-axis peck drilling, C-axis positioning G87 C___X___Q___ P___F___ X-axis tapping G88 C___X___F___ Notes: C = C-axis position, Z = Z-end position, Q = peck distance (No decimal point allowed with the Q. Repeat Q on each subsequent l...

  • Page 117

    111 POLAR COORDINATE INTERPOLATION FUNCTION G12.1 On a Turning Center that is equipped with a C-axis (rotary axis), interpolation between the linear axis “X” and the rotary axis “C” is possible by use of the G12.1-function. This function simplifies programming of shapes to be machined ...

  • Page 118

    112 Layout of the X-C coordinate system plane • The diagram above shows the X-C coordinate system plane as viewed when looking at the front face of the main spindle. • The address “X” defines a point by the distance from origin horizontally on diameter (Positive or negative value)....

  • Page 119

    113 • Positioning command “G0” cannot be used in G12.1-mode. Positioning is done in G1- mode, using a feed rate of around 30” to 60” per minute, depending on application. • Feed command In the G12.1-mode the feed velocity can be specified either by units of linear distance per minu...

  • Page 120

    114 Command for arc of less than 360°: (G2 or G3) X_ C_ I_ J_ Command used for full circle: (G2 or G3) I_ or: J_ • Cutter compensation function In polar coordinate interpolation the cutter compensation function should always be used, regardless of programming method. Size control on a...

  • Page 121

    115 Tool offset data, including the “R” and “T”-data are activated by the tool offset command. (The “D”-command, such as used in machining center programming cannot be used). • Adjusting the part size Suppose that an external hexagon shape was machined over-size by 0.005” (measu...

  • Page 122

    116 Programming example The figure above left shows two flat surfaces to be machined on the front face of a 1.25” diameter part. A clearance diameter of 1.300” that intersects with both of the flats has been added to the figure on the right. The coordinates (X 1.0, C0.4153) located at the...

  • Page 123

    117 Deciding the machining method The milling operation on this part can be programmed in various different ways. Examples for three different programming methods A, B and C are shown. Programming Method “A” The figure on right shows programming of the tool center-path. The cutter to be use...

  • Page 124

    118 G12.1 Polar coordinate interpolation ON G1 G98 C.5339 F60. C-axis position at the first point of the contour shape, use IPM - feed mode, if desired (Note: the C-command at this time represents a linear dimension – not degrees) G1 G41 X1.75F7. (1) Cutter comp ON X-axis position at the firs...

  • Page 125

    119 Preparing the machining program for methods “B” and “C” “Climb Cutting” is done in both cases. Hence the cutting start point coordinates in both cases are at X1.0 C0.4153. The automatic cutter compensation function G41 is applied. The cutting start point is located on the top rig...

  • Page 126

    120 CYLINDRICAL INTERPOLATION Principle of Operation The cylindrical interpolation function “G7.1” allows circular interpolation between the Z-axis and a rotary axis. Programming is done using Cartesian coordinates for the Z-axis and degrees of rotation for the rotary axis. Arc specification...

  • Page 127

    121 C º = L / R x 57.29578° • Z-coordinates specify absolute dimensions parallel to the length of the cylinder. The letter “W” can be used for incremental specification along the Z-axis. • C- axis rotation is specified as an absolute angle in degrees. The letter “H” for increment...

  • Page 128

    122 C º = L / D x 114.59156° When diameter “D” is used to define the circle, use this formula: 114.59156° = two radians. Cylindrical Interpolation Example The letters “J and R” to be engraved around the OD of a 2.9”-diameter part, using cylindrical interpolation-function G7.1 A 1/3...

  • Page 129

    123 Converting linear coordinates to degrees of rotation For the sample part at hand the factor for converting linear units into degrees is calculated as follows: 1 / 2.9 x 114.59156 = 39.514331º per 1” of linear distance The table below shows the start-points and end-points for the letter...

x