1. Manuals
  2. Brands
  3. Brother Manuals
  4. Printer
  5. TC-32B
  6. Manual

Brother TC-32B Manual

Hide thumbs
Table of Contents

Advertisement

Quick Links

Download this manual
TC-32B
Title
TC-32B
NC PROGRAMMING
MANUAL
Please read this manual carefully before starting operation.
1
2003/4/21
eTCOMNCPRT1.doc

Advertisement

Table of Contents
loading

Related Manuals for Brother TC-32B

Summary of Contents for Brother TC-32B

  • Page 1 TC-32B Title TC-32B NC PROGRAMMING MANUAL Please read this manual carefully before starting operation. 2003/4/21 eTCOMNCPRT1.doc...
  • Page 2 TC-32B Title This manual describes the NC-Programming of the TC-32B. The tapping centre is able to perform drilling, tapping, and facing. We shall not bear any responsibility for accidents caused by user's special handling or handling deviating from the generally recognized safe operation.
  • Page 3 The contents of this Manual are subject to change without notice. This manual are complied with utmost care. If you encounter any question or doubt, please contact your local dealer. © Copyrigt 2004 BROTHER INDUSTRIES,LTD. Machinery & Solution Company. Machine Tools Field. ALL RIGHTS RESERVED. 2003/4/21...
  • Page 4 TC-32B Title HOW TO USE THE MANUAL This Instruction Manual consists of the following elements: General description Is an outline of the description given in the section. Alarm Is a alert given against a danger which may cause serious damage or death to human being or may damage the machine.

  • Page 5: Table Of Contents

    TC-32B Contents Chapter 1 Program Composition-------------------------------- 1-1 Types and composition of program ------------------------------------1-2 Composition of block -------------------------------------------------------1-2 Composition of word --------------------------------------------------------1-3 Numerical values ----------------------------------------------------------1-3 Sequence number ---------------------------------------------------------------1-4 Optional block skip -------------------------------------------------------------1-4 Control out/in function---------------------------------------------------------1-4 Coordinate Command -------------------------------- 2-1 Chapter 2...
  • Page 6 TC-32B Contents 3.27 Peck drilling cycle (G183) ----------------------------------------------------3-55 3.28 Local coordinate system function (G52) --------------------------------3-56 3.29 Single direction positioning function(G60)-----------------------------3-57 3.30 G code priority--------------------------------------------------------------------3-58 Preparation Function (tool offset function) ---- 4-1 Chapter 4 Tool Dia Offset(G40,G41,G42) -----------------------------------------------4-2 4.1.1 Tool dia offset function ------------------------------------------------------------------------- 4-2 4.1.1.1...
  • Page 7 TC-32B Contents 5.4.12 End mill tap cycle (G177) -------------------------------------------------------------------- 5-21 5.4.13 End mill tap cycle (G178) -------------------------------------------------------------------- 5-22 5.4.14 Double drilling cycle (G181,G182) --------------------------------------------------------- 5-23 5.4.15 Double boring cycle (G185,G189) ---------------------------------------------------------- 5-24 5.4.16 Double boring cycle (G186)------------------------------------------------------------------ 5-25 5.4.17 Canned cycle of reducing step --------------------------------------------------------------- 5-26 5.4.18...
  • Page 8 TC-32B Contents Chapter 9 High Accuracy Mode A--------------------------------- 9-1 Outline -------------------------------------------------------------------------------9-2 Usage --------------------------------------------------------------------------------9-3 9.2.1 User parameter setting ------------------------------------------------------------------------ 9-3 9.2.2 User parameter description ------------------------------------------------------------------- 9-4 9.2.3 Usage in a program ---------------------------------------------------------------------------- 9-5 9.2.4 Conditions available --------------------------------------------------------------------------- 9-6 9.2.5 Conditions where high accuracy mode A is released ------------------------------------ 9-6 Restrictions------------------------------------------------------------------------9-7 9.3.1...
  • Page 9 TC-32B Contents Chapter 13 Option------------------------------------------------------ 13-1 13.1 Programming precautions when using rotation axis (index table) -----------------------------------------------------------------------13-2 2004/01/19 eTCOMNCPRC.doc...
  • Page 10 TC-32B Contents (This page is a blank.) 2004/01/23 eTCOMNCPRC.doc...
  • Page 11 TC-32B Quick index Chpt. 1 PROGRAM COMPOSITION Chpt. 2 COORDINATE COMMAND Chpt. 3 PREPARATION FUNCTION PREPARATION FUNCTION Chpt. 4 (TOOL OFFSET FUNCTION) Chpt. 5 PREPARATION FUNCTION (CANNED CYCLE) PREPARATION FUNCTION Chpt. 6 (COORDINATE CALCULATION)) Chpt. 7 MACRO Chpt. 8 AUTOMATIC WORK MEASUREMENT Chpt.
  • Page 12 Quick index TC-32B (This page is a blank.) 2003/04/14 TCOMCOOP8-2...

  • Page 13: Chapter 1 Program Composition

    TC-32B Chapter 1 Program Composition CHAPTER 1 PROGRAM COMPOSITION 1.1 Types and composition of program 1.2 Composition of block 1.3 Composition of word 1.4 Numerical values 1.5 Sequence number 1.6 Optional block skip 1.7 Control out/in function 1 - 1 2004/01/22 eTCOMNCPR1-1.doc...

  • Page 14: Types And Composition Of Program

    Chapter 1 Program Composition TC-32B Types and Composition of Program The program is divided into the main program and the subprogram. (1) Main program The main program is for machining one workpiece. While the main program is in use, a subprogram can be called to use the program more efficiently.

  • Page 15: Composition Of Word

    TC-32B Chapter 1 Program Composition Compositiom of Word A word is composed of an address and some digit of figures as shown below. (Algebraic sign + or - may added before a numerical value.) -1000 Address numerical value Word (Note 1) The address uses one of the alphabetical letters.

  • Page 16: Sequence Number

    Chapter 1 Program Composition TC-32B Sequence Number A sequence number (1~99999) can be used following the address N for each block. Command format N *****; A sequence number is used following the address N. A sequence number can be specified with up to 5-digit number.

  • Page 17: Chapter 2 Coordinate Command

    TC-32B Chapter2 Coordinate Command CHAPTER 2 COORDINATE COMMAND 2.1 Coordinate system and coordinate value 2.2 Machine zero point and machine coordinate system 2.3 Working coordinate system 2 - 1 2004/01/22 eTCOMNCPR2-1.doc...

  • Page 18: Coordinate System And Coordinate Value

    Chapter2 Coordinate Command TC-32B Coordinate system and coordinate value Coordinate values should be set in one coordinate system to specify a tool movement. There are two types of coordinate systems. (i) Machine coordinate system (ii) Working coordinate system The coordinate values are expressed by each component of the program axes (X, Y and Z for this unit).

  • Page 19: Machine Zero Point And Machine Coordinate System

    TC-32B Chapter2 Coordinate Command Machine Zero Point and Machine Coordinate System (1) Machine zero point The machine zero point is the reference point on the machine. (2) Machine coordinate system The coordinate systen with the machine zero point as its reference point is called the machine coordinate system.
  • Page 20 Chapter2 Coordinate Command TC-32B ( This page is a blank.) 2 - 4 2004/01/22 eTCOMNCPR2-1.doc...

  • Page 21: Chapter 3 Preparation Function

    TC-32B Chapter 3 Preparation Function CHAPTER 3 PREPARATION FUNCTION Outline of G code Positioning (G00) Linear interpolation (G01) Circular/helical interpolation (G02, G03) Circle cutting (G12, G13) Plane selection (G17, G18, G19) Dwell (G04) Exact stop check (G09, G61, G64) Programmable data input (G10) 3.10...
  • Page 22 Chapter 3 Preparation Function TC-32B 3.27 Peck drilling cycle (G183) 3.28 Local coordinate system function (G52) 3.29 Single direction positioning function (G60) 3.30 G code priority 3 - 2 2004/01/22 eTCOMNCPR3.doc...

  • Page 23: Outline Of G Code

    TC-32B Chapter 3 Preparation Function Outline of G code Within 3-digit number following the address G determines the meaning of the command of the block concerned. The G codes are divided into the following two types. Type Meaning The G code is effective until another G code in the Modal same group is commanded.
  • Page 24 Chapter 3 Preparation Function TC-32B Group G cord Contents Modal G00* Positioning Linear interpolation Circular/ helical interpolation (CW) Circular / helical interpolation (CCW) Modal G102 XZ Circular interpolation (CW) G103 XZ Circular interpolation (CCW) G202 YZ Circular interpolation (CW) G203...
  • Page 25 TC-32B Chapter 3 Preparation Function Group G cord Contents Modal Tool length offset + Tool length offset - Modal G49* Tool length offset cancel G50* Scaling cancel Modal Scaling G50.1 Mirror image cancel Modal G51.1 Mirror image Local coordinate system...
  • Page 26 Chapter 3 Preparation Function TC-32B Group G cord Contents Modal G90* Absolute command Modal Incremental command Working coordinate system setting One-shot Feed rate per minute G98* Return to the initial point level Modal Return to the R point level Canned cycle (High-speed peck drilling cycle)
  • Page 27 TC-32B Chapter 3 Preparation Function Group G cord Contents Modal G173 Canned cycle (High-speed peck drilling cycle) One-shot G177 Canned cycle (End mill tap cycle) Modal G178 Canned cycle (End mill tap cycle) G181 Canned cycle (Double drilling cycle) Modal...
  • Page 28 Chapter 3 Preparation Function TC-32B Group G cord Contents Modal G120 Positioning to the measuring point One-shot G121 Automatic measurement Corner (Boss) G122 Automatic measurement Parallel (Groove) G123 Automatic measurement Parallel (Boss) G124 Automatic measurement Circle center (Hole, 3 points)

  • Page 29: Positioning (G00)

    TC-32B Chapter 3 Preparation Function Positioning (G00) A tool moves from its current position to the end point at the rapid traverse rate in each axis direction independently. Therefore, a tool path is not always a linear line. Command format X_Y_Z_A_B_C_ ;...

  • Page 30: Linear Interpolation (G01)

    Chapter 3 Preparation Function TC-32B Linear interpolation (G01) Linear interpolation moves a tool linearly from the current position to the target position at the specified feedrate. Command format X_Y_F_ ; Up to X,Y,X and one additional axis can be controlled simultaneously.

  • Page 31: Chamfering To Desired Angle And Cornering C

    TC-32B Chapter 3 Preparation Function (Note2) α β The example below shows linear interpolation of linear axis and rotation axis α β When "G01 G91 X Ff ;" is programmed: α +β Time taken for B-axis movement: β Feedrate along B axis: α...
  • Page 32 Chapter 3 Preparation Function TC-32B When the chamfering amount is longer than the chamfering command block and feeding quantity of the subsequent block, set extended point from each blocks as "chamfer start point" and "chamfer end point". Example.1: Liner cutting eNCPR3.04.ai...
  • Page 33 TC-32B Chapter 3 Preparation Function Corner-R end poin Virtual corner Corner-R start point intersection The cornering command block and the subsequent block must contain the interpolation command (G01-G03). When the subsequent block does not contain an interpolation or movement command, an alarm will occur.

  • Page 34: Circular/Helical Interpolation (G02, G03)

    Chapter 3 Preparation Function TC-32B Circular/Helical Interpolation (G02, G03) 3.4.1 Circular interpolation Circular interpolation moves a tool along a circular arc from the current position to the end point at the specified feedrate. 3.4.1.1 Circular interpolation X-Y plane G17G02 X_ Y_...

  • Page 35: Xz Circular Interpolation

    TC-32B Chapter 3 Preparation Function 3.4.1.2 XZ Circular interpolation G102 X_ Y_ I_ J Command format G103 The commands are given in the following format: G 102 Clockwise (CW). Rotation direction G103 Counterclockwise (CCW). G90 mode End point in the working coordinate system.
  • Page 36 Chapter 3 Preparation Function TC-32B 3.4.1.3 XZ Circular interpolation G202 X_ Y_ I_ J Command format G203 The commands are given in the following format: G202 Clockwise (CW). Rotation direction G203 Counterclockwise (CCW). G90 mode End point in the working coordinate system.
  • Page 37 TC-32B Chapter 3 Preparation Function The end point of the circular arc takes either the absolute value or the incremental value according to G90 or G91. The incremental value commands the distance from the circular arc start point to the end point.
  • Page 38 Chapter 3 Preparation Function TC-32B eNCPR3.10.ai Absolute command; G03X-60. Y-10. I-50. J-20. F1000 ; Incremental command; G03X-30. Y30. I-50. J-20. F1000 ; eNCPR3.11.ai (1) G02X-70. Y-50. R25. F1000 ; (2) G02X-70. Y-50. R-25. F1000 ; (Note 1) When either I, J or K is omitted, it is regarded zero.
  • Page 39 TC-32B Chapter 3 Preparation Function Transition of radius eNCPR3.15.ai eNCPR3.14.ai (Note 6) If the ending radius is extremely larger than that of the starting radius, an alarm will occur. (Note 7) The G36~G39 codes cannot be commanded in the circular arc mode.

  • Page 40: Helical Interpolation

    Chapter 3 Preparation Function TC-32B 3.4.2 Helical interpolation Putting the other than selected plane axis command in the circular arc block permits a helical cutting. Command format X-Y plane: G17G02 X_Y_Z_ I_ J_ G17G03 X_Y_Z_ I_ J_ Z-Y plane: G18G02 Z_X_Y_...

  • Page 41: Spiral Interpolation (G02, G03)

    TC-32B Chapter 3 Preparation Function 3.4.3 Spiral interpolation (G02, G03) An increment or decrement per rotation is specified for the circular interpolation command to perform spiral interpolation. Command format X-Y plane: {G17}G02X_Y_I_J_Q_L_F_; {G17}G03X_Y_I_J_Q_L_F_; Z-Y plane: {G18}G02Z_X_K_I_Q_L_F_; {G18}G03Z_X_K_I_Q_L_F_; Y-Z plane: {G19}G02Y_Z_J_K_Q_L_F_;...
  • Page 42 Chapter 3 Preparation Function TC-32B Cutter compensation can be performed only in offset mode. An alarm will occur when this is attempted in startup or cancel mode. The setting for [Cutter compensation] is applied relative to the start point and target point specified in the program during cutter compensation.

  • Page 43: Conical Interpolation (G02, G03)

    TC-32B Chapter 3 Preparation Function 3.4.4 Conical interpolation (G02, G03) The travel command of another axis in addition to the spiral interpolation command is added and an increment and decrement is specified for that axis per spiral rotation to perform conical interpolation.
  • Page 44 Chapter 3 Preparation Function TC-32B 25.0 25.0 (0,37.5,62.5) 25.0 25.0 100.0 - 100 Example of program Start point (0.,100.,0.) End point (0.,-37.5,62.5) Distance to the center (0.,-100.) Increment/decrement in radius -25. Increment/decrement in height No. of rotations Example of program Start point (0.,100.,0.)
  • Page 45 TC-32B Chapter 3 Preparation Function Cutter compensation can be performed only in offset mode. An alarm will occur when this is attempted in startup or cancel mode. The setting for [Cutter compensation] is applied to the selected plane during cutter compensation, relative to the start point and target point specified in the program.

  • Page 46: Cutter Compensation Procedure For Spiral Interpolation And Conical Interpolation (G02, G03)

    Chapter 3 Preparation Function TC-32B 3.4.5 Cutter compensation procedure for spiral interpolation and conical interpolation (G02, G03) Assuming a virtual circle with the center of the spiral interpolation as the center for the start point and end point of the block, cutter compensation is performed for the virtual circle and then spiral interpolation is performed based on the result of cutter compensation.

  • Page 47: Circle Cutting (G12, G13)

    TC-32B Chapter 3 Preparation Function Circle Cutting (G12, G13) Starting from the center of the circle, the tool cuts the inner side of the circle and returns to the center of the circle. Command format G12I_D_F_; G13I_D_F_; Clockwise cutting direction...

  • Page 48: Plane Selection (G17, G18, G19)

    Chapter 3 Preparation Function TC-32B An alarm will occur when command "D" is omitted. An alarm will occur when the product of the radius (command "I") minus compensation is zero (0) or a negative value. An alarm will occur when the circle cutting command (G12, G13) is specified together with the cutter compensation command (G40, G41, G42) (startup or cancel mode).

  • Page 49: Dwell (G04)

    TC-32B Chapter 3 Preparation Function Dwell (G04) Upon completion of the previous block and in-position check, some time elapses before executing the next block. Command format P,X : Dwelling time (sec) Exact Stop Check (G09, G61, G64) Since acceleration and deceleration is applied independently to each axis, the actual tool path comes inside the programmed path if each axis speed changes greatly between the former block and the new block in the cutting feed.
  • Page 50 Chapter 3 Preparation Function TC-32B (Note 2) Old block Cutting feed No traveling New block × × × Positioning × × Cutting feed × × × No traveling Cutting mode × Exact stop check mode When the old block is clamped while the additional axis is traveling, exact stop check is executed.

  • Page 51: Programmable Data Input (G10)

    TC-32B Chapter 3 Preparation Function Programmable Data Input (G10) (1) Input of working zero position Command format G10L2Pn X_ Y_ Z_ A_ B_ C_ When the G90 mode (absolute command) is selected, the commanded offset amount becomes newly effective. When the G91 mode (incremental command) is selected, the commanded offset amount is added to the currently set offset amount to become a renewed offset amount.
  • Page 52 Chapter 3 Preparation Function TC-32B (3) Input of tool fine offset value When tool length /Tool diameter compensation command is issued using the program, the data of the fine offset number corresponding to the commanded offset number is automatically reflected in operation.
  • Page 53 TC-32B Chapter 3 Preparation Function Measurement result New working zero point Old working zero point eNCPR3.16.ai (5) Input of tool life. Command format G10L97 P_ Q_ R_ W_ Tool No. Life category Non counting Time (Minutes) Count of hole machining (Hole)

  • Page 54: Soft Limit

    Chapter 3 Preparation Function TC-32B 3.10 Soft Limit The allowable area of the tool motions can be specified in the following three ways. (1) Stroke setting by the parameter 2 (2) Stroke limit setting by the parameter 1 (3) Programmable stroke limit setting by the G22 code 3.10.1...

  • Page 55: Programmable Stroke Limit (G22)

    TC-32B Chapter 3 Preparation Function 3.10.3 Programmable stroke limit (G22) The allowable area of the tool motions is commanded by the program. Command format G22 X_Y_Z_I_J_K_ ; Programmable stroke limit on + direction of X axis. Programmable stroke limit on + direction of Y axis.

  • Page 56: Return To The Reference Point (G28)

    Chapter 3 Preparation Function TC-32B 3.11 Return to the Reference Point (G28) Command format G28X_Y_Z_A_B_C_; This command provides an automatic return to the reference point through an intermediate point for commanded axes. Positioning to the reference point is made through an intermediate point as specified by X_Y_Z_A_B_C_.

  • Page 57: Return From The Reference Point(G29)

    TC-32B Chapter 3 Preparation Function 3.12 Return from the Reference Point (G29) Command format G29X_Y_Z_A_B_C_; This command provides positioning to the commanded position through an intermediate point for commanded axes. At an incremental command, an incremental distance from the intermediate point must be commanded.

  • Page 58: Selection Of Working Coordinate System (G54~G59)

    Chapter 3 Preparation Function TC-32B 3.15 Selection of working coordinate system (G54~G59) When 6 sets of the coordinate systems for each workpiece are set in the data previously, necessary coordinates system can be selected by commanding the G54 through G59 codes.

  • Page 59: Scaling (G50, G51)

    TC-32B Chapter 3 Preparation Function 3.17 Scaling (G50, G51) The programmed shape can be enlarged or reduced by the desired scaling factor. Scaling is possible using the same ratio for all axes or a different ratio for each axis. Scaling using the same ratio for all axes Command format G51X_Y_Z_P_;...
  • Page 60 Chapter 3 Preparation Function TC-32B Example of scaling using the same ratio for all axes Scaling using the same ratio for all axes Scaling center ’ P1P2P3P4 → P1’P2’P3’P4’ ’ Y-axis Scaling using a different ratio for each Machining axis...
  • Page 61 TC-32B Chapter 3 Preparation Function Precautions for use of scaling function: (Note 1) When scaling is invalid Tool offset set for [Cutter compensation] and [Tool length offset] is not subject to scaling. Additional axes are not subject to scaling. An alarm will occur when coordinate transformation (rotational transformation, scaling, programmable mirror image) is performed while the additional axis is selected by the plane selection command (G17, 18, 19).
  • Page 62 Chapter 3 Preparation Function TC-32B Program example of mirror image using scaling function When a negative number is specified for the scaling factor, programmable mirror image is applied. When a negative value is specified for the scaling factor and there is only one scaling axis, CW and CCW of circular travel will be reversed.

  • Page 63: Programmable Mirror Image (G50.1, G51.1)

    TC-32B Chapter 3 Preparation Function 3.18 Programmable Mirror Image (G50.1, G51.1) Mirror image is applied to the program commands for the axes specified in the program. Mirror image Command format G51.1X_Y_Z_; Mirror image cancel Command format G50.1X_Y_Z_; Mirror image setting can be applied simultaneously for the 1st to 3rd axes.
  • Page 64 Chapter 3 Preparation Function TC-32B Precautions for use of programmable mirror image: (Note 1) When programmable mirror image is invalid Mirror image is not applied to the positioning direction for single direction positioning (G60). Tool length offset is not subject to mirror image setting compensation.
  • Page 65 TC-32B Chapter 3 Preparation Function Coordinates are calculated according to the following sequence: mirror, scaling, and then rotational transformation. Accordingly, set these in this order in a program. Set these in the reverse order to cancel previous settings. An alarm will occur when the specified sequence is not followed.

  • Page 66: Rotational Transformation Function (G68,G69)

    Chapter 3 Preparation Function TC-32B 3.19 Rotational Transformation Function (G68, G69) The shape specified in the program is rotated. Rotational transformation Command format G68α_β_R_; Rotational transformation cancel Command format G69; αβ Rotation center coordinates Rotation angle (based on CCW) After rotation...
  • Page 67 TC-32B Chapter 3 Preparation Function An alarm will occur when any reference position return related command (G27, G28, G29, G30) is used during rotational transformation. An alarm will occur when ccommand (G52 or G92) during rotational transformation. An alarm will occur when any automatic workpiece measurement command (G131, G132, G120 to G129) is used during rotational transformation.

  • Page 68: Coordinate Rotation Using Measured Results(G168)

    Chapter 3 Preparation Function TC-32B 3.20 Coordinate rotation using measured results (G168) Command format G168 X_Y_Q_; X,Y : Rotation center coordinate value. Selects the desired measured result by setting "1" to "4". When the selection is omitted, the setting is considered to be "1".
  • Page 69 TC-32B Chapter 3 Preparation Function (3) When additional axis is commanded 1. Absolute command (e.g., B axis) • When B STROKE of user parameter is set to 1: YES, the B axis rotates to the commanded angle. • When B STROKE of user parameter is set to 0: NO, the B axis rotates in the direction closer to the commanded angle.

  • Page 70: Change Of Workpiece Coordinate System(G92)

    Chapter 3 Preparation Function TC-32B 3.22 Change of workpiece coordinate system (G92) Change of workpiece zero position can be commanded as follows: Command format G92X_Y_Z_A_B_C_; This command shifts the zero position in the working coordinate system so that the current tool position becomes to the commanded coordinate values.
  • Page 71 TC-32B Chapter 3 Preparation Function New G55 New G54 working zero position working zero position Old G55 working zero position Old G54 working zero position eNCPR3.22.ai In the above figures, G92 is commanded in the coordinate system of G54. When the working zero position of G54 shifts, the other working zero positions of G55 through G59 also shift the same amount as G54.

  • Page 72: Skip Function (G31,G131,G132)

    Chapter 3 Preparation Function TC-32B Spindle end face Tool top point The target value in the program becomes the same as commanded by G92. (Note 6) When the additional axis is commanded while an optional additional axis is not installed, an alarm will occur.

  • Page 73: Continuous Skip Function (G31)

    TC-32B Chapter 3 Preparation Function 3.24 Continuous skip function (G31) The tool moves linearly (linear interpolation) at the specified feedrate from the current position to the target position. If the detection signal turns ON in the meantime, the coordinate value when the detective signal turns ON is stored in the system variables(#5061~#5063) of custom macro.

  • Page 74: High Speed Peck Drilling Cycle (G173)

    Chapter 3 Preparation Function TC-32B 3.26 High speed peck drilling cycle (G173) Command format G173 X _ Y _ Z _ R _ Q _ F _ ; R point Z point rapid feed cutting feed eNCPR5.19.ai 3 - 54 2004/01/22 eTCOMNCPR3.doc...

  • Page 75: Peck Drilling Cycle (G183)

    TC-32B Chapter 3 Preparation Function 3.27 Peck drilling cycle (G183) Command format G183 X _ Y _ Z _ R _ Q _ F _ ; This is cycle where return operation is removed from G83. R point Z point...

  • Page 76: Local Coordinate System Function (G52)

    Chapter 3 Preparation Function TC-32B 3.28 Local coordinate system function (G52) Command format G52 X_ Y_ Z_ A_ B_ C_ ; X, Y, Z, A, B, C: Amount of shift from workpiece coordinate zero point Operation will be the same regardless of G90 or G91.

  • Page 77: Single Direction Positioning Function(G60)

    TC-32B Chapter 3 Preparation Function 3.29 Single direction positioning function (G60) G60 X_Y_Z_A_B_C_ Command format X, Y, Z, A, B, C: Command value of the axis for which single direction positioning is performed. Coordinate of end point for G90 and travel amount for G91...

  • Page 78: G Code Priority

    Chapter 3 Preparation Function TC-32B 3.30 G code priority Executed correctly. Error The last G command is effective. One-shot is executed and the modal is updated. One-shot is executed and the modal is updated, but an error occurs when circle arc is commanded.
  • Page 79 TC-32B Chapter 3 Preparation Function Command the same block (Model-Model) 3 - 59 2004/01/22 eTCOMNCPR3.doc...
  • Page 80 Chapter 3 Preparation Function TC-32B Command the same block (Model-One-shot) 3 - 60 2004/01/22 eTCOMNCPR3.doc...
  • Page 81 TC-32B Chapter 3 Preparation Function Command the same block (One-shot -One-shot) 3 - 61 2004/01/22 eTCOMNCPR3.doc...
  • Page 82 Chapter 3 Preparation Function TC-32B Command during Model G17 G18 G22 G23 G40 G41 G49 G50 G51 G50.1 G51.1 G54 G54.1 G61 G66 G67 G68 G69 G73 G80 G90 G94 G98 G177 G168 G0,G1 G2,G3 G18,G19 G41,G42 G43,G44 G50.1 G51.1 G54.1...
  • Page 83 TC-32B Chapter4 Preparation function (Tool offset function) CHAPTER 4 PREPARATOION FUNCTION (TOOL OFFSET FUNCTION) 4.1 Tool dia offset (G40, G41, G42) 4.2 Tool length offset (G43, G44, G49) 4 - 1 2004/01/22 eTCOMNCPR4.doc...

  • Page 84: Tool Dia Offset(G40,G41,G42)

    Chapter4 Preparation function (Tool offset function) TC-32B Tool dia offset (G40, G41, G42) 4.1.1 Tool dia offset function Programming is done according to the actual workpiece form, but this function enables the tool to move along the path with an offset from actual workpiece form, which is equivalent to the used tool radius.

  • Page 85: Cancel Mode

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.2 Cancel mode The system enters the cancel mode right after the power is turned ON or the [RESET] key is pressed. In the cancel mode, the path of the tool center coincides with the programmed path.

  • Page 86: Start-Up

    Chapter4 Preparation function (Tool offset function) TC-32B 4.1.3 Start-up When a block which satisfies all the following conditions is executed in the cancel mode, the system enters the offset mode. The control in this operation is called the start-up. a) G41 or G42 is commanded.

  • Page 87: Outside Cutting (90° ≤ Θ < 180°)

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.3.2 Outside cutting (a)Type 1 : Linear - Linear Type 1 : Linear - Arc (b)Type 2 : Linear - Linear Type 2 : Linear - Arc (Note 1) Type 1 and 2 can be selected in parameter 1 for start-up and cancel motions.
  • Page 88 Chapter4 Preparation function (Tool offset function) TC-32B Outside cutting ( θ < 90°) 4.1.3.3 (a)Type 1 : Linear - Linear Type 1 : Linear - Arc (b)Type 2 : Linear - Linear Type 2 : Linear - Arc (Note 1) Type 1 and 2 can be selected in parameter 1 for start-up and cancel motions.

  • Page 89: Offset Mode

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.4 Offset mode A tool movement command in the offset mode includes a positioning, a linear interpolation, a circular interpolation and a helical interpolation. 4.1.4.1 Inside cutting Linear - Linear Arc - Linear Linear - Arc Arc –...
  • Page 90 Chapter4 Preparation function (Tool offset function) TC-32B α < (Note 1) When going around at a narrow angle (there is ˚) no cross point of 2 perpendicular lines from programme lines, so that tool center path will be exceptionally as follows;...

  • Page 91: Outside Cutting (90°≤Θ<180°)

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.4.2 Outside cutting (90°≤θ<180°) Linear - Linear Linear - Arc Arc - Linear Arc - Arc 4 - 9 2004/01/22 eTCOMNCPR4.doc...

  • Page 92: Outside Cutting (Θ < 90°)

    Chapter4 Preparation function (Tool offset function) TC-32B (Note 1) When 179˚ <θ<180˚, tool center path will be as follows; Linear -Linear It will be processed in the same procedure as above in case of Arc - Linear, Linear - Arc and Arc - Arc.

  • Page 93: Exceptional Case

    TC-32B Chapter4 Preparation function (Tool offset function) Linear - Arc Arc - Arc 4.1.4.4 Exceptional case There is no cross point at inside cutting. Alarmed stop As above figure shows, the cross point of the arcs is present if the offset value is small, but it may be disappear if the offset value becomes large.

  • Page 94: Offset Cancel

    Chapter4 Preparation function (Tool offset function) TC-32B 4.1.5 Offset cancel When the command satisfying all the conditions as shown below is executed in the offset mode, the offset cancel mode becomes effective. The tool motion in this status is called an offset cancel.
  • Page 95 TC-32B Chapter4 Preparation function (Tool offset function) Type 1:Arc-Linear Type 2:Arc-Linear Type 2:Linear-Linear (Note 1) Type 1 and 2 can be selected in parameter 1 for start-up and cancel motions. ≤ < (Note 2) If the angle is close to 180˚(79˚...

  • Page 96: Outside Cutting (Θ < 90°)

    Chapter4 Preparation function (Tool offset function) TC-32B Outside cutting （θ < 90˚） 4.1.5.3 Type 1:Linear-Linear Type 1:Arc-Linear Type 2:Linear-Linear Type 2:Arc-Linear 4 - 14 2004/01/22 eTCOMNCPR4.doc...

  • Page 97: G40 Single Command

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.6 G40 single command When G40 is specified independently, the tool moves to the position offset perpendicularly in the preceding block and stops. Linear – Linear G41 X_Y_D_; G40 ; Arc – Linear G41 X_Y_D_;...

  • Page 98: Change Of Offset Direction In Offset Mode

    Chapter4 Preparation function (Tool offset function) TC-32B 4.1.7 Change of offset direction in offset mode By commanding G41 or G42, or converting the algebraic sign (+, -) of the offset amount, the offset direction can be changed even in the offset mode.

  • Page 99: Change Of Offset Direction In Offset Mode

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.8 Change of offset direction in offset mode 4.1.8.1 When there is a cross point Linear - Linear Linear - Arc Arc - Linear Arc - Arc 4 - 17 2004/01/22 eTCOMNCPR4.doc...

  • Page 100: When There Is No Cross Point

    Chapter4 Preparation function (Tool offset function) TC-32B 4.1.8.2 When there is no cross point Linear – Linear Linear – Arc Arc – Linear Center 4 - 18 2004/01/22 eTCOMNCPR4.doc...

  • Page 101: When Offset Path Becomes More Than A Circle

    TC-32B Chapter4 Preparation function (Tool offset function) Arc – Arc Center Center 4.1.8.3 When offset path becomes more than a circle By changing offset direction offset path becomes more than a circle, but actual offset path is short cutted as shown below.

  • Page 102: G Cord Command For Tool Dia Offset In Offset Mode

    Chapter4 Preparation function (Tool offset function) TC-32B 4.1.9 G code command for tool dia offset in offset mode Linear - Linear Linear - Arc Arc - Linear Arc - Arc 4 - 20 2004/01/22 eTCOMNCPR4.doc...

  • Page 103: Notes On Tool Dia Offset

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.10 Notes on tool dia offset (1) Command of tool dia offset amount The offset amount is commanded by the number of the D command. When G41 or G42 is commanded, the offset amount is commanded in the same block.
  • Page 104 Chapter4 Preparation function (Tool offset function) TC-32B (5) Cutting insufficient This problem occurs in the case of a program containing a step smaller than the tool radius. Cutting insufficient 4 - 22 2004/01/22 eTCOMNCPR4.doc...
  • Page 105 TC-32B Chapter4 Preparation function (Tool offset function) (6) Corner movement When cutting the outer side, the tool moves around the corner from different angles.The movement mode and the feedrate up to the single block stop point are as specified in the current block.
  • Page 106 Chapter4 Preparation function (Tool offset function) TC-32B The original movement in the above figure are: P0-P1-P2 Linear movement P2-P3 Linear movement The tool moves once around the circular arc afterwards with P3 as the target. If this small movement function is used, the movement from P2 to P3 is ignored and...
  • Page 107 TC-32B Chapter4 Preparation function (Tool offset function) (7) Block without movement When the command without any X/Y movement is given for more than 3 blocks during the tool dia offset mode, the movement is as shown below and overcutting or undercutting occurs.
  • Page 108 Chapter4 Preparation function (Tool offset function) TC-32B (8) Tool movement in case of tool dia offset amount zero a) Start-up When G41 or G42 is commanded in the cancel mode, the offset mode becomes effective but the start-up motion is not available as the offset amount is zero.
  • Page 109 TC-32B Chapter4 Preparation function (Tool offset function) (9) Exceptional case or alarm-generating command 1.Command to produce the vertical vector G10 : Programmable data input G52 : Local coordinate system G92 : Coordinate system setting #3000:Alarm display #3006: Message display & stop When the above command is given, the tool moves to the point which is offset as much as the tool dia as specified by the last X/Y movement command.
  • Page 110 Chapter4 Preparation function (Tool offset function) TC-32B (11) Manual intervention When moving the tool by manual operation in the offset mode and starting the memory operation again, the corrected offset path starts from two blocks ahead. 04L68.ai When moving the tool by manual operation after it stopped at the block end point P2, the tool movs from P2' to P3, then follows the corrected offset path after P3.

  • Page 111: Override Function Related To Tool Dia Offset

    TC-32B Chapter4 Preparation function (Tool offset function) 4.1.11 Override function related to tool dia offset 4.1.11.1 Automatic corner override When the blocks before and after the inner corner satisfy the following conditions, an automatic override is applied to reduce the load on the tool.

  • Page 112: Override Of The Inside Circular Cutting

    Chapter4 Preparation function (Tool offset function) TC-32B 4.1.11.2 Override of the inside circular cutting When cutting along the circular arc whitch is offset inside during the offset mode, the actual feedrate is calculated by multiplying the commanded feedrate by Rc/Rp.

  • Page 113: Tool Length Offset (G43,G44,G49)

    TC-32B Chapter4 Preparation function (Tool offset function) Tool Length Offset (G43, G44, G49) This function corrects the tool position so that the tool nose comes to the programmed position. In either the absolute command or the incremental command, the end point in the programmed Z-axis move command is offset as specified by H code to become the actual end point.
  • Page 114 Chapter4 Preparation function (Tool offset function) TC-32B (This page is a blank.) 4 - 32 2004/01/22 eTCOMNCPR4.doc...

  • Page 115: Chapter 5 Preparation Function (Canned Cycle)

    TC-32B Chapter 5 Preparation function (canned cycle) CHAPTER 5 PREPARATION FUNCTION (CANNED CYCLE) 5.1 List of canned cycle function 5.2 Basic motions in canned cycle 5.3 General description of canned cycle 5.4 Details of canned cycle 5.5 Canned cycle for tool change (non-stop ATC)(G100)

  • Page 116: List Of Canned Cycle Function

    Chapter 5 Preparation function (canned cycle) TC-32B CANNED CYCLE For repetitive machining, a series of paths that is usually specified in a few blocks can be specified in one block. List of Canned Cycle Function Table 5-1 List of canned cycle function...

  • Page 117: Basic Motions In Canned Cycle

    TC-32B Chapter 5 Preparation function (canned cycle) Basic Motions in Canned Cycle In general, the canned cycle is composed of the following six motions. Motion 1 : Positioning (at rapid feed) to the drilling position (X/Y) Motion 2 : Positioning to R point (at rapid feed)

  • Page 118: General Description Of Canned Cycle

    Chapter 5 Preparation function (canned cycle) TC-32B General description of canned cycle 5.3.1 Command related to canned cycle motions Absolute command (1) Data format Incremental command Initial point level return (2) Return level R point level return (3) Drilling mode...

  • Page 119: Types Of Return Point (G98,G99)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.3.3 Types of return point (G98, G99) There are two types of return points - initial point level return (G98) and R point level return (G99) - when the canned cycle motions are finished.

  • Page 120: Machining Data Of Canned Cycle

    Chapter 5 Preparation function (canned cycle) TC-32B 5.3.5 Machining data of canned cycle Command format G * * X _ Y _ Z _ R _ Q _ P _ F _ S _ K _ ; G code Position data...

  • Page 121: Repeat Number Of Canned Cycle

    TC-32B Chapter 5 Preparation function (canned cycle) 5.3.6 Repeat number of canned cycle When drilling at an equal interval is repeated in the same canned cycle, use the address K and specify the repeat number. The command range of K is 0 - 9999.

  • Page 122: Details Of Canned Cycle

    Chapter 5 Preparation function (canned cycle) TC-32B Details of canned cycle 5.4.1 High-speed peck drilling cycle (G73) Command format X _ Y _ Z _ R _ P _ Q _ F _ ; Return point R point Z point...

  • Page 123: Reverse Tapping Cycle (G74)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.2 Reverse tapping cycle (G74) Command format X _ Y _ Z _ R _ P _ F _ S _ ; Return point R point Rapid feed Cutting feed Spindle CW Z point Spindle CCW eNCPR5.06.ai...

  • Page 124: Fine Boring Cycle (G76)

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.3 Fine boring cycle (G76) Command format X _ Y _ Z _ R _ Q _ P _ F _ S _V _; Return point R point Spindle stop Z point Rapid feed...

  • Page 125: Tapping Cycle (G77)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.4 Tapping cycle (G77) Command format X _ Y _ Z _ R _ Q _ S _ ; Return R point Spindle stop Z point rapid feed cutting feed spindle CW spindle CCW eNCPR5.08.ai...

  • Page 126: Reverse Tapping Cycle (Synchro Mode) (G78)

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.5 Reverse tapping cycle (synchro mode) (G78) Command format X _ Y _ Z _ R _ Q _ S _ ; Return R point Spindle stop Z point rapid feed cutting feed...

  • Page 127: Drilling Cycle (G81,G82)

    TC-32B Chapter 5 Preparation function (canned cycle) • Tapping high-speed return The spindle speed at a return of synchro tapping (G77 or G78) is variable. Command format X _ Y _ Z _ R _ Q _ S _ L _ ;...
  • Page 128 Chapter 5 Preparation function (canned cycle) TC-32B High speed cycle Feed speed at start and end of drilling cycle (G81 or G82) is variable. Command format X _ Y _ Z _ R _ W _ V _ F _ E _ L _ P _;...

  • Page 129: Peck Drilling Cycle (G83)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.7 Peck drilling cycle (G83) Command format G83 X _ Y _ Z _ R _ P _ Q _ F _ ; Return point R point Z point Dwelling for P sec...

  • Page 130: Tapping Cycle (G84)

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.8 Tapping cycle (G84) Command format G84 X _ Y _ Z _ R _ P _ F _ S _ ; Return R point Spindle stop Z point rapid feed cutting feed...

  • Page 131: Boring Cycle (G85,G89)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.9 Boring cycle (G85, G89) Command format X _ Y _ Z _ R_ P_ F_ ; Return R point Spindle stop Z point rapid feed cutting feed spindle CW spindle CCW eNCPR5.14.ai High speed cycle Free speed at return of boring cycle (G85 or G89) is variable.

  • Page 132: Boring Cycle (G86)

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.10 Boring cycle (G86) Command format X _ Y _ Z _ R _ P _ F _ S_ Q_; Return point R point Rapid feed Cutting feed Z point Spindle CW Spindle stop...
  • Page 133 TC-32B Chapter 5 Preparation function (canned cycle) High speed cycle Feed speed at start and end of boring cycle (G86) is variable. Command format X _ Y _ Z _ R _ W _ V _ F _ E _ L _ P_ Q_ ;...

  • Page 134: Back Boring Cycle (G87)

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.11 Back boring cycle (G87) Command format X _ Y _ Z _ R _ Q _ P _ F _ S_ V_ ; Single block stop Spindle orientation specified by V Z point...

  • Page 135: End Mill Tap Cycle (G177)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.12 End mill tap cycle (G177) Command format G177 X _ Y _ Z _ R _ S_ L _ Q _E _ ; Feeding speed changeover point. Distance from point "R", regardless of absolute mode (G90) or incremental mode (G91).

  • Page 136: End Mill Tap Cycle (G178)

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.13 End mill tap cycle (G178) Command format G178 X _ Y _ Z _ R _ S_ L _ Q _E _ ; Q : Feeding speed changeover point. Distance from point "R", regardless of absolute mode (G90) or incremental mode (G91).

  • Page 137: Double Drilling Cycle (G181,G182)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.14 Double drilling cycle (G181,G182) G181 Command format X _ Y _ Z _ R _ I _ J _ W _ V _ F _ E _ L _P_ ; G182 Double rapid feed start point (follow G90/G91) Distance from point "R"...

  • Page 138: Double Boring Cycle (G185,G189)

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.15 Double boring cycle (G185,G189) G185 Command format X _ Y _ Z _ R _ I _ J _ F _ E _ P _ ; G189 Double rapid feed start point (follow G90/G91) Distance from point "R"...

  • Page 139: Double Boring Cycle (G186)

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.16 Double boring cycle (G186) Command format G186 X _ Y _ Z _ R _ I _ J _ W _ V _ F _ E _ L _ P _ Q _ S _ ;...

  • Page 140: Canned Cycle Of Reducing Step

    Chapter 5 Preparation function (canned cycle) TC-32B 5.4.17 Canned cycle of reducing step For G73, G77, G78, G83, G173 and G183 fixed cycles, reducing step is available which reduces the cutting feed depth gradually. (1) High-speed peck drilling cycle (G73) (Reducing step)
  • Page 141 TC-32B Chapter 5 Preparation function (canned cycle) (2) Peck drilling cycle (G83) (Reducing step) Command format X _ Y _ Z _ R _ P _ W _ V _ F _ W : 1st cutting feed V : Minimum cutting feed...
  • Page 142 Chapter 5 Preparation function (canned cycle) TC-32B (3) Tapping cycle (synchro mode)(G77) (Reducing step) Command format X _ Y _ Z _ R _ W _ V _ S; 1st cutting feed Minimum cutting feed Return point Spindle stop R point...
  • Page 143 TC-32B Chapter 5 Preparation function (canned cycle) (4) Reverse tapping cycle (synchro mode)(G78) (Reducing step) Command format X _ Y _ Z _ R_ W _ V _ S _ 1st cutting feed Minimum cutting feed Return point Spindle stop...
  • Page 144 Chapter 5 Preparation function (canned cycle) TC-32B (5) High-speed peck drilling cycle (G173) (Reducing step) Command format G173 X _ Y _ Z _ R _ W _ V _ F _ W : 1st cutting feed V : Minimum cutting feed...
  • Page 145 TC-32B Chapter 5 Preparation function (canned cycle) (6) Peck drilling cycle (G183) (Reducing step) Command format G183 X _ Y _ Z _ R _ W _ V _ F _ 1st cutting feed Minimum cutting feed R point 2nd cutting feed...

  • Page 146: Canned Cycle Cancel (G80)

    Chapter 5 Preparation function (canned cycle) TC-32B (7) For G73, G83, G173 and G183 fixed cycles, the cutting feed after the second time will be as below. Cutting feed depth = Coefficient × 1st cutting feed (W) Time of cutting Coefficient 0.825 0.675...

  • Page 147: Notes On Canned Cycle

    TC-32B Chapter 5 Preparation function (canned cycle) 5.4.19 Notes on canned cycle (1) When commanding the canned cycle (G73, G81 to G83, G85, G89, G173,G181 to G183, G185, G189) which does not control the spindle rotation, the spindle should be rotated in advance by the M code.

  • Page 148: Canned Cycle For Tool Change (Non-Stop Atc)(G100)

    Chapter 5 Preparation function (canned cycle) TC-32B Canned cycle for tool change (non-stop ATC) (G100) (1) When TC-32B. Command format G100 T _ X _ Y _ Z _ R _ A _ B _ L _ ; (3) (4)
  • Page 149 TC-32B Chapter 5 Preparation function (canned cycle) Operations (1) Tool moves to the Z-axis point "R" while performing 0-degree spindle orientation. When "T" is commanded, magazine swivels. (2) Tool movement to theZ-axis ATC origin, to the X axis origin point and to Y axis ATC position, A, B axes movement to the the commanded value and also maga zine cover opening occur simultaneously.
  • Page 150 Chapter 5 Preparation function (canned cycle) TC-32B • When point "R" command position (5) is lower than Z axis command position (7), tool moves to Z-axis commanded position, and operation (7) is not performed. Tool change motion Tool change motion differs depending on tool type set on [MAGAZINE TOOL] screen.
  • Page 151 TC-32B Chapter 5 Preparation function (canned cycle) Next tool preparation Next tool preparation is performed after the arm has swiveled or the pot has risen after the arm swivels in the ATC sequence. When ATC is not performed, only next tool preparation is performed.
  • Page 152 Chapter 5 Preparation function (canned cycle) TC-32B (This page is a blank.) 5 - 38 2004/01/22 eTCOMNCPR5-1.doc...

  • Page 153: Preparation Function (Coordinate Calculation)

    TC-32B Chapter6 Preparation function (coordinate calculation) CHAPTER 6 PREPARATION FUNCTION (COORDINATE CALCULATION) 6.1 List of coordinate calculation function 6.2 Coordinate calculation parameter 6.3 Details of coordinate calculation function 6.4 Usage of coordinate calculation function 6 - 1 2004/01/22 eTCOMNCPR6-1.doc...

  • Page 154: List Of Coordinate Calculation Function

    Chapter6 Preparation function (coordinate calculation) TC-32B Coordinate calculation function This function is for calculating the point group coordinates in one block. Point groups are such as on a linear line, on a grid and on a circular arc. By combining such functions as the canned cycle etc., drilling at each point group is available by one command.

  • Page 155: Details Of Coordinate Calculation Function

    TC-32B Chapter6 Preparation function (coordinate calculation) Relation of each calculation function and parameter is as shown below. Parameter Function G code ● ● ● ● Bolt hole circle Linear(angle) ● ● Linear(X,Y) ● ● ● ● ● Grid ● : Be sure to specify. Otherwise, alarm occurs.

  • Page 156: Linear (Angle)

    Chapter6 Preparation function (coordinate calculation) TC-32B 6.3.2 Linear (angle) With the reference point at the commanded coordinate, the coordinate values along the linear line at the angle (θ°) formed by the X axis are calculated. Command format G37 X_ Y_ I_ J_ K_...

  • Page 157: Grid

    TC-32B Chapter6 Preparation function (coordinate calculation) (Ex.) G38 X0 Y0 I20 J15 K4 ; eNCPR6.02.ai (Note 1) When K is omitted, it is regarded as 1. (Note 2) The reference point becomes the first machining point. 6.3.4 Grid With the reference point at the commanded coordinate, the coordinate values of the grid...

  • Page 158: Usage Of Coordinate Calculation Function

    Chapter6 Preparation function (coordinate calculation) TC-32B (Ex.) G39 X0 Y0 I20 J25 K4 P3 Q30 ; eNCPR6.03.ai (Note 1) The reference point becomes the first machining point. (Note 2) The coordinate is calulated in the X direction from the reference point.

  • Page 159: Chapter 7 Macro

    TC-32B Chapter 7 Macro CHAPTER 7 MACRO 7.1 What is a Macro? 7.2 Variable Function 7.3 Calculation Function 7.4 Control Function 7.5 Call Function 7 - 1 2004/01/22 eTCOMNCPR7-1.doc...

  • Page 160: What Is A Macro

    Chapter 7 Macro TC-32B What is a Macro? A “macro” has four main functions: variable function, calculation function, control function (condition branch), and call function (performs the same operation repeatedly). Using these macro functions allows you to create original canned cycles or more flexible programs.

  • Page 161: Variable Function

    TC-32B Chapter 7 Macro eNCPR7.01.ai Variable Function 7.2.1 Outline of variable function For normal programs, commands are given by directly designating a numerical value (e.g. G90, X200). Using the macro’s variable function allows you to use the value stored in the variable for G and X commands.

  • Page 162: Undefined Variable

    Chapter 7 Macro TC-32B [Example 2] #100 = #[100+10] This formula specifies that the value stored in variable #110 is written to #100. [Example 3] When #1 = 9, #9 = 20, and #20 = 30, #5 = # [# [#1]] is equal to #5 = 30.

  • Page 163: Types Of Variables

    TC-32B Chapter 7 Macro 7.2.4 Types of variables There are two types of variables: Local variable (#1 ~ #26) Common variable (#100 ~ #199, #500 ~ #599) Local variables are provided for each call level of the macro program. When a macro program is called, the local variables of the called macro level are stored, and a new local variable area is created for the called macro program.

  • Page 164: Variable Display And Setting

    Chapter 7 Macro TC-32B 7.2.5 Variable display and setting Variables are displayed and manually set on the data bank screen. Press the [3] and [ENT] keys at the data bank menu screen, or shift the cursor to the menu No.3 and press the [ENT] key.

  • Page 165: System Variable

    TC-32B Chapter 7 Macro 7.2.6 System variable Interface input/output signal Signal input #1000 ~#1015 Signal output #1100 ~ #1115 Signal batch reading (16 bits) #1032 Signal batch writing (16 bits) #1132 [Example of use] A signal is output from the program to external output port 103.
  • Page 166 Chapter 7 Macro TC-32B Alarm indication #3000 = n (ALARM MESSAGE) Alarm number 9000 + n (n: 0 ~200) occurs, and the alarm message in the brackets (the first 20 characters, reset by the [RESET] key) is displayed. Only alphanumerical characters are used in the brackets and registered in the alarm log.
  • Page 167 TC-32B Chapter 7 Macro Mirror image Mirror images of each axis Numerical value is converted from binary number to decimal number. Mirror image #3007 0: INVALID bit 0: X axis 1:VALID bit 0: Y axis bit 0: Z axis Modal information The called modal information can be read.
  • Page 168 Chapter 7 Macro TC-32B Current position Read while Contents Coordinate System Tool offset traveling #5001~ End point Workpiece coordinate Not included Possible #5008 coordinate system #5021~ Current Machine coordinate Included Not possible #5028 position system #5041~ Current Workpiece coordinate Included...
  • Page 169 TC-32B Chapter 7 Macro Workpiece counter Read setting value of the workpiece counter screen and write. #3801 Workpiece counter 1 count number #3802 Workpiece counter 1 present #3803 Workpiece counter 1 finish #3804 Workpiece counter 1 finish announcement #3811 Workpiece counter 2 count number...

  • Page 170: Calculation Function

    Chapter 7 Macro TC-32B Calculation Function 7.3.1 Calculation type Calculations such as those below are possible for variables and numerical values. [Supplementary explanation] • Numerical values are entered for i, j, and k of #i, #j, and #k (e.g. #10), indicating they are macro variables.

  • Page 171: Precautions For Calculation

    TC-32B Chapter 7 Macro 7.3.3 Precautions for calculation (Note 1) Formula The right side of the equation can be connected using a constant, variable, function, or operator. When using a constant, any value without a decimal point is regarded as having a decimal point at its end.

  • Page 172: Control Function

    Chapter 7 Macro TC-32B Control Function The control function allows you to change the flow of the program in the middle of the program by designating certain conditions. The control function has the following three types: GOTO statement (Unconditional branch)

  • Page 173: While Statement (Repetition)

    TC-32B Chapter 7 Macro [Example] (1) IF[#100 EQ 50] GOTO 123; (2) IF[#101 GT 102] GOTO 123; (3) GOTO 124; N123; N124; At (1) above, If variable #100 is 50, the program skips to (4), where the sequence number is 123.

  • Page 174: Precautions For Control Function

    Chapter 7 Macro TC-32B (Note1) The range of numerical values that can be used in the conditional expression is -2147483647 to 2147483647. If a value not within this range is used, an alarm will occur. Condition satisfied Condition not satisfied Processing END m;...
  • Page 175 TC-32B Chapter 7 Macro (Note 2) DOm ~ ENDm should not be overlapped in the WHILE statement. WHILE [#100 LT 10]DO 1; WHILE [#101 EQ 50]DO 2; END 1; END 2; WHILE [ ” 100 LT 10 ] DO 1;...

  • Page 176: Call Function

    Chapter 7 Macro TC-32B (Note 5) IF statement and WHILE statement IF ~ GOTO within WHILE ~ END cannot be branched to a section outside WHILE ~ END. WHILE [#101 EQ 0] DO 1; IF[#101 EQ 10]GOTO 123; END 1;...

  • Page 177: Simple Call Function

    TC-32B Chapter 7 Macro 7.5.1 Simple call function G65 is generally used to call a macro program. Command format G65 P_L_(Argument); Macro program number to be called Number of calls to be repeated (up to 9999) If “L” is omitted, “1”is automatically selected.

  • Page 178: Modal Call Function

    Chapter 7 Macro TC-32B 7.5.2 Modal call function When a macro program is automatically called each time an axis movement command is given once registered, it is called a “modal call function”. Use G66 to register a modal call and G67 to cancel registration. When a modal call is registered, the macro program is executed after each axis movement.

  • Page 179: Macro Call Argument

    TC-32B Chapter 7 Macro 7.5.3 Macro call argument Argument(s) must be declared when it is necessary to pass local variables to the macro. Format 1 Augments can be declared for all addresses, excluding G, L, N, O, and P. Addresses...
  • Page 180 Chapter 7 Macro TC-32B Format 2 A, B, and C, and repeating I, J, K can be designated.  Addresses with Macro Nth repeat argument variables specified (Note 1) Addresses that do not require setting can be omitted. (Note 2) Local variables corresponding to non-designated addresses are null.

  • Page 181: Difference Between G65 And M98

    TC-32B Chapter 7 Macro 7.5.4 Difference between G65 and M98 Arguments can be designated for G65, but cannot be designated for M98. Local variables are available for G65 depending on the depth of nesting, but are not available for M98.

  • Page 182: Multiple Nesting Call

    Chapter 7 Macro TC-32B 7.5.5 Multiple nesting call Macro calling depth of nesting is up to 4 -fold. Local variables (#1 ~ #26)are provided for each macro level. When macro is called by G65, local variable of called macro level is stored once, and new local variable of called macro program is prepared.

  • Page 183: Chapter 8 Automatic Work Measurement

    TC-32B Chapter 8 Automatic work measurement CHAPTER 8 AUTOMATIC WORK MEASUREMENT 8.1 Before automatic work measurement 8.2 Setting of data on automatic work measurement 8.3 Operation of automatic work measurement 8.4 Display of the measured results 8.5 Lock key operations...
  • Page 184 Chapter 8 Automatic work measurement TC-32B Automatic Work Measurement Automatic work measuring functions 1. G121 -- X and Y coordinates of a corner eNCPR9.01.ai 2. G129 -- X and Y coordinates of a groove eNCPR9.02.ai 3. G122 -- X and Y coordinates of the axis of parallel groove eNCPR9.03.ai...
  • Page 185 TC-32B Chapter 8 Automatic work measurement 5. G124,G126 -- X and Y coordinates of the center of a hole eNCPR9.05.ai 6. G125,G127 -- X and Y coordinates of the center of a boss 7. G128 -- Z coordinate of the top surface of a workpiece...

  • Page 186: Before Automatic Work Measurement

    Chapter 8 Automatic work measurement TC-32B Before Automatic Work Measurement Set the necessary parameters of User Parameter 7 (ZERO MEASUREMENT). Unless the parameters are set correctly, the probe may be damaged. Setting of Data on Automatic Work Measurement User Parameter...
  • Page 187 TC-32B Chapter 8 Automatic work measurement Item Description MEASURING MOTION (0:TYPE1) 1) It is checked that the detection signal is off. (0:TYPE1 1:TYPE2) 2) The probe moves in the specified axis direction at the speed preset to MEASURING SPEED 1.
  • Page 188 Chapter 8 Automatic work measurement TC-32B Item Description MEASURING SPEED 1 Sets the first measuring speed for MEASURING MOTION(TYPE1). *Relief amount of probe = L (mm) *SKIP FEED TIME CONSTANT 1 = t (msec) *MEASURING SPEED 1 = F1 (mm/min) *Delay in control system = td (msec) = 12 (msec) （(F1×td)÷(60×1000)）...
  • Page 189 TC-32B Chapter 8 Automatic work measurement Item Description MEASURING TRAVEL LMT Sets the amount of overtravel when the measuring skip has exceeded DISTANCE the estimated value(program command value). Setting range: 0.000~99.999 mm 0.0000~9.9999 inch MEASUREMENT TOLERANCE 1 When the difference between the measured value and the estimated value (program command value) has exceeded the preset value, MEASD VAL ERR LRG(1) will occur.
  • Page 190 Chapter 8 Automatic work measurement TC-32B (Note) The setting values of MEASURING SPEED, RETURN DISTANCE AFT MEASURNG and so on differ according to the probe mounted. Consult the probe maker and set the values. During automatic work measurement, the speed that the probe moves to the measurement start point or returns from the measured point conforms to the modal of G00 and G01.

  • Page 191: Operation Of Automatic Work Measurement

    TC-32B Chapter 8 Automatic work measurement Operation of Automatic Work Measurement 8.3.1 Corner Command format Boss G121 X_ Y_ I_ J_ K_L_D_Z_ R_Q_ Groove G129 X_Y_ I_ J_ K_ L_D_Z_R_Q_ ; 8 - 9 2004/01/30 eTCOMNCPR8-1.doc...
  • Page 192 Chapter 8 Automatic work measurement TC-32B ...Estimated corner value I ,K ...X-axis position when measuring in the Y direction, offset value from (X, Y) J ,L ...Y-axis position when measuring in the Y direction, offset value from (X, Y) ...Tool offset number ...Z coordinate during measurement...
  • Page 193 TC-32B Chapter 8 Automatic work measurement Measurment pattern The spindle is oriented. The probe moves to the first measurement start point of the X and Y axes. The probe moves to the Z axis measurement height. The first measurement is carried out (Position "J").
  • Page 194 Chapter 8 Automatic work measurement TC-32B d) I<0, J<0 1ST... spindle180°, in the -X directi 2ND... spindle180°, in the-Y directio eNCPR9.14.ai Measurement pattern The spindle is oriented. The probe moves to the first measurement start point of the X and Y axes.

  • Page 195: Parallel

    TC-32B Chapter 8 Automatic work measurement c) I<0, J<0 1ST ... spindle 0° , in the +X direction 2ND... spindle 180° , in the -Y directi eNCPR9.17.ai d) I>0 , J>0 1ST ... spindle 0° , in the +X directi 2ND...
  • Page 196 Chapter 8 Automatic work measurement TC-32B Tool offset number Z coordinate during measurement Z coordinate of return point when the Z axis has traveled from one measurement point to the other measurement point or when the movement has completed. Register No. that stores the measured results ("1" when omitted)
  • Page 197 TC-32B Chapter 8 Automatic work measurement Boss Measurement pattern Spindle orientation 180°. The probe moves to the first measurement start point of the X and Y axes. The probe moves to the Z axis measurement height. The first measurement is carried out.

  • Page 198: Circle

    Chapter 8 Automatic work measurement TC-32B 8.3.3 Circle The circle center is calculated by measuring three points. hole G124 X_ Y_ I_ D_Z_ R_Q_ Command format boss G125 X_ Y_ I_ D_ Z_ R_Q_ The circle center is calcutaled by measuring four points.
  • Page 199 TC-32B Chapter 8 Automatic work measurement Measurment pattern Hole ... Three-point measurement 1. Spindle orientation 0゜. The probe moves to the first measurement start point of the X and Y axes. 2. The probe moves to the Z axis measurement height.
  • Page 200 Chapter 8 Automatic work measurement TC-32B eNCPR9.26.ai Hole ... Four-point measurement 1. Spindle orientation 0゜. The probe moves to the first measurement start point of the X and Y axes. 2. The probe moves to the Z axis measurement height.
  • Page 201 TC-32B Chapter 8 Automatic work measurement Boss ... Four-point measurement 1. Spindle orientation 180゜. The probe moves to the first measurement start point of the X and Y axes. 2. The probe moves to the Z axis measurement height. 3. The first measurement is carried out (in the -X direction ).

  • Page 202: Z Level

    Chapter 8 Automatic work measurement TC-32B 8.3.4 Z LEVEL Command format G128 X_ Y_ Z_Q_ X and Y coordinates of measuring point Z coordinate of measuring start point Register No. that stores the measured results ("1" when omitted) eNCPR9.29.ai Measurment pattern Spindle orientation 0°.

  • Page 203: Handling Of Measured Results

    TC-32B Chapter 8 Automatic work measurement measyrement position eNCPR9.30.ai G120 Xa Yb Zc When [G120 Xa, Yb, and Zc] is commanded, the probe moves to point P. When the measurement data does not exist, NO MEASRUING DATA alarm will occur.
  • Page 204 Chapter 8 Automatic work measurement TC-32B When you continue to another measurement, previous measurement results are displayed. T07005u2.bmp 8.4.2 Reflection of measured results on workpiece coordinate system The measured results are reflected in the workpiece coordinate system. Command format G10 L99...
  • Page 205 TC-32B Chapter 8 Automatic work measurement machine coordinat system -120 The working coordinate data G55 is changed to X = -40.000 and Y = -80.000. 8 - 23 2004/01/30 eTCOMNCPR8-1.doc...

  • Page 206: Lock Key Operations

    Chapter 8 Automatic work measurement TC-32B Lock key operations DRY RUN The probe moves to the measurement start point, but measurement is not carried out. Measurement data is not transferred, either. MACHINE LOCK Axes are not moved. The coordinate value on the<POSITION> screen varies.

  • Page 207: Chapter 9 High Accuracy Mode A

    TC-32B Chapter 9 High Accuracy Mode A CHAPTER 9 HIGH ACCURACY MODE A Outline Usage Restrictions Effective Functions 9 - 1 2004/01/22 eT32BNCPR.9.doc...

  • Page 208: 9.1 Outline

    Chapter 9 High Accuracy Mode A TC-32B 9.1 Outline High accuracy mode A is a function for highly accurate machining at high speed. It is ideal for contouring and 3D workpiece machining. This function enables you to machine workpieces at high speed yet maintain accuracy.

  • Page 209: Usage

    TC-32B Chapter 9 High Accuracy Mode A Usage 9.2.1 User parameter setting High accuracy mode A has three deceleration functions. Adjusting the settings for user parameters (Corner deceleration override, Arc deceleration override, Curve approximation deceleration override) alters the shape accuracy. In addition to this, up to three patterns (levels 1 to 3) can be set for parameters, and these can be changed in the NC program.

  • Page 210: User Parameter Description

    Chapter 9 High Accuracy Mode A TC-32B 9.2.2 User parameter description Parameter name Descriptions Setting range (%) Corner deceleration Set the automatic corner deceleration override for level 1 override 1 (M260) in high accuracy mode A. When 100 is set, automatic corner deceleration is performed using the machine’s unique deceleration rate.

  • Page 211: Usage In A Program

    TC-32B Chapter 9 High Accuracy Mode A 9.2.3 Usage in a program Use the following M codes to use high accuracy mode A. M260：High accuracy mode A (level 1) on M261：High accuracy mode A (level 2) on M262：High accuracy mode A (level 3) on M269：High accuracy mode A off...

  • Page 212: Conditions Available

    Chapter 9 High Accuracy Mode A TC-32B 9.2.4 Conditions available G code modal conditions must be as below to use high accuracy mode A. The conditions below are current when the power is turned on. G64：Cutting mode G67：Macro cancel G80：Canned cycle cancel See the Instruction Manual for check method of G code modal conditions.

  • Page 213: Restrictions

    TC-32B Chapter 9 High Accuracy Mode A Restrictions 9.3.1 Functions available Functions that can be used while high accuracy mode A is on are given below. 1. All M codes 2. C codes in the table below. G code Function...

  • Page 214: Effective Functions

    Chapter 9 High Accuracy Mode A TC-32B Effective Functions The functions below are available while high accuracy mode A is on. (1) Automatic corner deceleration function (2) Automatic arc deceleration function (3) Automatic curve approximation deceleration function 9.4.1 Automatic corner deceleration function When machining a corner, the actual tool path gradually deviates from the program path as the tool approaches the corner.

  • Page 215: Automatic Arc Deceleration Function

    TC-32B Chapter 9 High Accuracy Mode A 9.4.2 Automatic arc deceleration function When performing circular interpolation, a radial error in the actual tool path occurs relative to the specified circular arc, and the arc radius decreases. In addition to this, the error becomes larger as the feed rate increases.

  • Page 216: Automatic Curve Approximation Deceleration

    Chapter 9 High Accuracy Mode A TC-32B 9.4.3 Automatic curve approximation deceleration This function automatically decelerates the curve approximation block feed rate according to the curve approximation deceleration override setting so that the shape accuracy for the curve approximation block (curve composed of minute blocks) specified by the NC program is maintained.

  • Page 217: Chapter 10 Subprogram Function

    TC-32B Chapter10 Subprogram function CHAPTER 10 SUBPROGRAM FUNCTION 10.1 Making Subprogram 10.2 Simple Call 10.3 Return No. Designation from Sub Program 10 - 1 2004/01/16 eTCOMNCPR10-1.doc...
  • Page 218 Chapter10 Subprogram function TC-32B Function of Subprogram When a program contains fixed sequences or frequently repeated patterns, these sequences or patterns may be entered into the memory as a subprogram. The subprogram can be called out in the memory operation mode.
  • Page 219 TC-32B Chapter10 Subprogram function Special uses of M99 If the M99 command is executed in the main program, the control returns to the start of main program. When optional block skip is off; When optional block skip is on /N0100 M99;...

  • Page 220: Command By Sub Program

    Chapter10 Subprogram function TC-32B 10.3 Return No. Designation from Program Command format M99 P_ ; 10.3.1 Command by sub program (Program execution sequence ) When the command is executed, the program returns the commanded sequence No.of the parent program. The sequence No is serched from the top of the program,and the program returns to the block initially found.

  • Page 221: Chapter 11 Feed Function

    TC-32B Chapter11 Feed function CHAPTER 11 FEED FUNCTION 11 - 1 2004/01/22 eTCOMNCPR11-1.doc...
  • Page 222 Chapter11 Feed function TC-32B Feed Function Feedrate is specified by the number following address F. (1) Command range Metric system : 1~999999 mm/min 1~999999゜/min Inch system : 0.1~99999.9 inch/min 0.1~99999.9゜/min (2) Clamp If the axis movement at a higher feedrate than the values specified by the machine parameter, an alarm is generated.

  • Page 223: Chapter 12 S,T,M Function

    TC-32B Chapter12 S,T,M function CHAPTER 12 S,T,M FUNCTION 12. 1 S Function 12. 2 T Function 12. 3 M Function 12 - 1 2004/01/22 eTCOMNCPR12.doc...

  • Page 224: S Function

    Chapter12 S,T,M function TC-32B S,T,M Function By commanding the following functions, machine motions other than the axis movements are available. : Spindle speed command : Tool magazine number command : ON/OFF command of various solenoids of the machine 12.1 S Function The S code is used for specifying the spindle speed.

  • Page 225: M Function

    TC-32B Chapter12 S,T,M function 12.3 M Function The M codes are used for commanding ON/OFF of various solenoids of the machine. It is commanded by address M and a following within 3-digit number. When the M command is in the same block as that of the axis movement, the motion is devided following three types.
  • Page 226 Chapter12 S,T,M function TC-32B List of M code (2) Operation Modal/ Group M code Content order vs. one-shot axis feec M400 M400 ON (Chip shower On) simultaneous modal M401* M400 OFF (Chip shower Off) M402 M402 ON simultaneous modal M403*...
  • Page 227 TC-32B Chapter12 S,T,M function List of M code (3) Operation Modal/ Group M code Content order vs. one-shot axis feed M120 TOUCH signal check after one-shot M121 TOUCH signal check after one-shot Tool breakage detection M200 after one-shot (with return motion)
  • Page 228 Chapter12 S,T,M function TC-32B List of M code (4) Operation Modal/ Group M code Content order vs. one-shot axis feed M440 Unclamping B axis modal M441* Clamping B axis M442 Unclamping A axis modal M443* Clamping A axis One-shot output (Proceeds to the...

  • Page 229: Program Stop (M00)

    TC-32B Chapter12 S,T,M function 12.3.1 Program stop (M00) The spindle stops after the commanded motions in a block are all finished. The coolant pump is turned OFF at this time. Next sequence is started by pressing the START switch. (Note) When the spindle should be rotated in the blocks after the M00 command, command M03 or M04.

  • Page 230: Tool Change (M06)

    Chapter12 S,T,M function TC-32B 12.3.6 Tool change (M06) (1) When TC-32B Command format T _ X _ Y _ Z _ R _ A _ B _ L _ ; (3)(4) ATC position R Point Single block stop po eNCPR13.03.ai...
  • Page 231 TC-32B Chapter12 S,T,M function Operations Tool moves to the Z-axis point "R" while performing 0-degree spindle orientation. When "T" is commanded, magazine swivels. Tool movement to theZ-axis ATC origin, to the X axis origin point and to Y axis ATC position, A, B axes movement to the the commanded value and also maga zine cover opening occur simultaneously.
  • Page 232 Chapter12 S,T,M function TC-32B Tool change motion Tool change motion differs depending on tool type set on [MAGAZINE TOOL] screen. (When large tool is not set on [MAGAZINE TOOL]) The following sequence is performed: Pot raises. Magazine swivels. Pot lowers.
  • Page 233 TC-32B Chapter12 S,T,M function Next tool preparation Next tool preparation is performed after the arm has swiveled or the pot has risen after the arm swivels in the ATC sequence. When ATC is not performed, only next tool preparation is performed.

  • Page 234: Workpiece Counter Specification (M211~M214)

    Chapter12 S,T,M function TC-32B 12.3.7 Workpiece counter specification (M211~M214) When M211~M214 are specified to the counter 1~4 respectively, and M211 ~ M214 are commanded in the memory operation, the commanded counter counts up by specified step at the execution of M02 or M30.

  • Page 235: Tap Time Constant Selection (M241 To 250)

    TC-32B Chapter12 S,T,M function 12.3.12 Tap time constant selection (M241 to 250) When the M251 command is given, tap time stay constant when tapping of Z-axis speed . When the M251 command is given, tap acceleration stay constant when tapping of Z-axis speed.

  • Page 236: Waiting Until Response Is Given (M460 To M469)

    Chapter12 S,T,M function TC-32B 12.3.18 Waiting until response is given (M460 to M469) For example M460 command waits until M460 signal turns on. M461 command waits until M460 signal turns off M462 command waits until M462 signal turns on. M463 command waits until M462 signal turns off.
  • Page 237 TC-32B Chapter13 Option CHAPTER 13 OPTION 13.1 Programming Precautions When Using Rotation Axis (index table) 13 - 1 2004/01/22 eTCOMNCPR13-1.doc...
  • Page 238 Chapter13 Option TC-32B 13.1 Programming Precautions When Using Rotation Axis (index table) When using the QT table on the TC-31A, 32A, and R2A with the rotation axis installed, be sure to place the rotation axis positioning command before the cutting command in the program file.
  • Page 239 eT32BNCPROKU...
  • Page 240 6A3468001 0401(1) eT32BNCPROKU...

Table of Contents