brother TC-32B Programming Manual
TC-32B Title
TC-32B
NC PROGRAMMING
MANUAL
Please read this manual carefully before starting operation.
2003/4/21 1 eTCOMNCPRT1.doc
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.
1
The relation between the manuals is as follows.
- OPERATION MANUAL
This manual describes the operations of the machine.
- INSTALLATION MANUAL
This manual describes the installation of the machine.
- PROGRAMMING MANUAL
This manual describes the programming of the machine.
Keep this manual for future reference.
Please include this manual when reselling this product.
When this manual or labels are lost or damaged, please replace them (charged) from your nearest
agency.
This manual is printed by using paper obtained from farmed trees.
2003/3/20 2 eTCOMNCPRT1.doc
TC-32B Title
INTRODUCTION
Congratulations on your purchase of the Brother CNC
tapping center. Correct usage of the machine is of most importance to assure the
expected machine capabilities and functions as well as operator's safety. Read this
Manual thoroughly before starting operation.
* All rights reserved: No part of this manual may be reproduced, stored in a retrieval system,
or transmitted in any form without prior permission of the manufacturer.
* 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 3 eTCOMNCPRT1.doc
1
y
TC-32B Title
HOW TO USE THE MANUAL
This Instruction Manual consists of the following elements:
(1) General description Is an outline of the description given in the section.
(2) Alarm Is a alert given against a danger which may cause serious
damage or death to human being or may damage the machine.
The hazards are explained in this order:
degree of danger,
subject of danger,
expected damage,
preventive measure,
(3) Operation procedure Is a procedure of activating a function.
(4) Screen Is given to describe important points of a procedure given.
NOTE: This screen is only a representation of the information
displayed on the actual screen and therefore differs
somewhat from the actual screen
layout and screen fonts.
(5) Illustration Is a sketch, figure, view, etc. indicating dimensions, position or zone, given
in the points where it is necessary to provide complementary information to the text
description.
(2) Alarm
(3) Operation procedure
WARNING
Dropping a heavy object onto
your foot may fracture your foot
bones.
When lifting heavy objects,
wear safet
shoes.
(1) General description
1.3.1Before starting operation
Before starting operation careful to read bellow.
(1)Tu rn off the main pow er break er hand le on
the contro l box doo r. Never touch t he primar y side
power source or the terminal of the main power
breaker, as these have high voltage applied.
(2)Put up a signboard w hich says ' Under Mainte nance
(3)Never allow people to approach the mach ine,
particularly moving areas.
(4)Do not place any unnecessary object around the
machine.
(5)Wear a helmet and safety shoes.
1 - 2
(5) Illustration
2003/3/20 4 eTCOMNCPRT1.doc
1 - 3
(4) Screen
TC-32B Contents
Chapter 1 Program Composition-------------------------------- 1-1
1.1 Types and composition of program ------------------------------------1-2
1.2 Composition of block -------------------------------------------------------1-2
1.3 Composition of word --------------------------------------------------------1-3
1.4 Numerical values ----------------------------------------------------------1-3
1.5 Sequence number ---------------------------------------------------------------1-4
1.6 Optional block skip -------------------------------------------------------------1-4
1.7 Control out/in function---------------------------------------------------------1-4
Chapter 2 Coordinate Command -------------------------------- 2-1
2.1 Coordinate system and coordinate value -------------------------------2-2
2.2 Machine zero point and machine coordinate system ---------------2-3
2.3 Working coordinate system--------------------------------------------------2-3
Chapter 3 Preparation Function --------------------------------- 3-1
3.1 Outline of G code ----------------------------------------------------------------3-2
3.2 Positioning (G00) ------------------------------------------------------------3-9
3.3 Linear interpolation (G01) ----------------------------------------------------3-10
3.3.1 Chamfering to desired angle and cornering C ----------------------------------------------3-11
3.4 Circular/helical interpolation (G02, G03) --------------------------------3-14
3.4.1 Circular interpolation --------------------------------------------------------------------------- 3-14
3.4.1.1 Circular interpolation ---------------------------------------------------------------------- 3-14
3.4.1.2 XZ Circular interpolation ----------------------------------------------------------------- 3-15
3.4.1.3 YZ Circular interpolation ----------------------------------------------------------------- 3-16
3.4.2 Helical interpolation----------------------------------------------------------------------------- 3-20
3.4.3 Spiral interpolation (G02, G03) --------------------------------------------------------------- 3-21
3.4.4 Conical interpolation (G02, G03) -------------------------------------------------------------3-23
3.4.5 Cutter compensation procedure for spiral interpolation and conical interpolation
(G02, G03) ---------------------------------------------------------------------------------------- 3-26
3.5 Circle Cutting (G12, G13) -----------------------------------------------------3-27
3.6 Plane Selection (G17, G18, G19) -------------------------------------------3-28
3.7 Dwell (G04)-------------------------------------------------------------------------3-29
3.8 Exact stop check (G09, G61, G64) -----------------------------------------3-29
3.9 Programmable data input (G10) --------------------------------------------3-31
3.10 Soft limit ----------------------------------------------------------------------------3-34
3.10.1 Stroke --------------------------------------------------------------------------------------------3-34
3.10.2 Stroke limit --------------------------------------------------------------------------------------3-34
3.10.3 Programmable stroke limit (G22) ----------------------------------------------------------- 3-35
3.11 Return to the reference point (G28) ---------------------------------------3-36
3.12 Return from the reference point(G29) ------------------------------------3-37
3.13 Return to the 2nd/3rd/4th reference point (G30)----------------------3-37
3.14 Selection of machine coordinate system (G53)-----------------------3-37
3.15 Selection of working coordinate system (G54~G59)----------------3-38
3.16 Additional working coordinate system selection (G54.1) ---------3-38
3.17 Scaling (G50, G51) --------------------------------------------------------------3-39
3.18 Programmable Mirror Image (G50.1, G51.1)----------------------------3-43
3.19 Rotational transformation function (G68,G69) ------------------------3-46
3.20 Coordinate rotation using measured results(G168)-----------------3-48
3.21 Absolute command and incremental command (G90, G91)------3-48
3.22 Change of workpiece coordinate system(G92) -----------------------3-50
3.23 Skip function (G31,G131,G132)---------------------------------------------3-52
3.24 Continuous skip function (G31) --------------------------------------------3-53
3.25 Change of tap twisting direction(G133,G134) -------------------------3-53
3.26 High speed peck drilling cycle (G173)) ----------------------------------3-54
2004/01/19 1 eTCOMNCPRC.doc
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
Chapter 4 Preparation Function (tool offset function) ---- 4-1
4.1 Tool Dia Offset(G40,G41,G42) -----------------------------------------------4-2
4.1.1 Tool dia offset function -------------------------------------------------------------------------4-2
4.1.1.1 Tool dia fine compensation ---------------------------------------------------------------4-2
4.1.2 Cancel Mode ------------------------------------------------------------------------------------- 4-3
4.1.3 Start -up ------------------------------------------------------------------------------------------- 4-4
4.1.3.1 Inside cutting -------------------------------------------------------------------------------4-4
4.1.3.2 Outside cutting (90° ≤ θ < 180°)--------------------------------------------------------- 4-5
4.1.3.3 Outside cutting (θ < 90°) ------------------------------------------------------------------ 4-6
4.1.4 Offset Mode -------------------------------------------------------------------------------------4-7
4.1.4.1 Inside cutting (180° ≤ θ) ------------------------------------------------------------------ 4-7
4.1.4.2 Outside cutting (90° ≤ θ < 180°)--------------------------------------------------------- 4-9
4.1.4.3 Outside cutting (θ < 90°) ------------------------------------------------------------------ 4-10
4.1.4.4 Exceptional case ----------------------------------------------------------------------------4-11
4.1.5 Offset Cancel ------------------------------------------------------------------------------------- 4-12
4.1.5.1 Inside cutting (180° ≤ θ) ------------------------------------------------------------------ 4-12
4.1.5.2 Outside cutting (90° ≤ θ < 180°)--------------------------------------------------------- 4-12
4.1.5.3 Outside cutting (θ < 90°) ------------------------------------------------------------------ 4-14
4.1.6 G40 single command ---------------------------------------------------------------------------- 4-15
4.1.7 Change of offset direction in offset mode --------------------------------------------------- 4-16
4.1.8 Change of offset direction in offset mode -------------------------------------------------- 4-17
4.1.8.1 When there is a cross point -------------------------------------------------------------- 4-17
4.1.8.2 When there is no cross point ------------------------------------------------------------- 4-18
4.1.8.3 When offset path becomes more than a circle -----------------------------------------4-19
4.1.9 G cord command for tool dia offset in offset mode ----------------------------------------4-20
4.1.10 Notes on tool dia offset ------------------------------------------------------------------------- 4-21
4.1.11 Override function related to tool dia offset -------------------------------------------------- 4-29
4.1.11.1 Automatic corner override -------------------------------------------------------------- 4-29
4.1.11.2 Override of the inside circular cutting------------------------------------------------- 4-30
4.2 Tool length offset (G43,G44,G49) -----------------------------------4-31
4.2.1 Tool length fine offset -------------------------------------------------------------------------- 4-31
Chapter 5 Preparation Function (canned cycle) ------------ 5-1
5.1 List of canned cycle function -----------------------------------------------5-2
5.2 Basic motions in canned cycle ---------------------------------------------5-3
5.3 General description of canned cycle ------------------------------------5-4
5.3.1 Command related to canned cycle motions ------------------------------------------------5-4
5.3.2 Setting of data in absolute / incremental command -------------------------------------- 5-4
5.3.3 Types of return point (G98,G99) ------------------------------------------------------------ 5-5
5.3.4 Canned cycle motion conditions------------------------------------------------------------- 5-5
5.3.5 Machining data of canned cycle ------------------------------------------------------------- 5-6
5.3.6 Repeat number of canned cycle-------------------------------------------------------------- 5-7
5.4 Details of Canned Cycle-------------------------------------------------------5-8
5.4.1 High-speed peck drilling cycle (G73) ------------------------------------------------------5-8
5.4.2 Reverse tapping cycle (G74) ----------------------------------------------------------------- 5-9
5.4.3 Fine boring cycle (G76) -----------------------------------------------------------------------5-10
5.4.4 Tapping cycle (G77) ---------------------------------------------------------------------------5-11
5.4.5 Reverse tapping cycle (Synchro mode) (G78) -------------------------------------------- 5-12
5.4.6 Drilling cycle (G81,G82) --------------------------------------------------------------------- 5-13
5.4.7 Peck drilling cycle (G83) --------------------------------------------------------------------- 5-15
5.4.8 Tapping cycle (G84) ---------------------------------------------------------------------------5-16
5.4.9 Boring cycle (G85,G89) ---------------------------------------------------------------------- 5-17
5.4.10 Boring cycle (G86)----------------------------------------------------------------------------- 5-18
5.4.11 Back boring cycle (G87) ----------------------------------------------------------------------5-20
2004/01/23 2 eTCOMNCPRC.doc
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 Canned cycle cancel (G80) ------------------------------------------------------------------- 5-32
5.4.19 Notes on canned cycle ------------------------------------------------------------------------ 5-33
5.5 Canned cycle for tool change (non-stop ATC)(G100)---------------5-34
Chapter 6 Preparation Function (coordinate calculation) 6-1
6.1 List of coordinate calculation function ----------------------------------6-2
6.2 Coordinate calculation parameter -----------------------------------------6-2
6.3 Details of coordinate calculation function ------------------------------6-3
6.3.1 Bolt hole circle --------------------------------------------------------------------------------- 6-3
6.3.2 Linear (Angle) ---------------------------------------------------------------------------------- 6-4
6.3.3 Linear (X,Y) ------------------------------------------------------------------------------------ 6-4
6.3.4 Grid -------------------------------------------------------------------------------------------- 6-5
6.4 Usage of coordinate calculation function-------------------------------6-6
Chapter 7 Macro------------------------------------------------------- 7-1
7.1 What is a Macro? ----------------------------------------------------------------7-2
7.2 Variable Function ----------------------------------------------------------------7-3
7.2.1 Outline of variable function ------------------------------------------------------------------ 7-3
7.2.2 Expression of variable -------------------------------------------------------------------------7-3
7.2.3 Undefined variable -----------------------------------------------------------------------------7-4
7.2.4 Types of variables ------------------------------------------------------------------------------7-5
7.2.5 Variable display and setting ------------------------------------------------------------------ 7-6
7.2.6 System variable ---------------------------------------------------------------------------------7-7
7.3 Calculation Function ---------------------------------------------------------7-12
7.3.1 Calculation type -------------------------------------------------------------------------------- 7-12
7.3.2 Calculation order ------------------------------------------------------------------------------- 7-12
7.3.3 Precautions for calculation ------------------------------------------------------------------- 7-13
7.4 Control Function---------------------------------------------------------------7-14
7.4.1 GOTO statement (unconditional branch)------------------------------------------------ 7-14
7.4.2 IF statement (conditional branch) ----------------------------------------------------------- 7-14
7.4.3 WHILE statement (repetition) ---------------------------------------------------------------7-15
7.4.4 Precautions for control function------------------------------------------------------------- 7-16
7.5 Call Function --------------------------------------------------------------------7-18
7.5.1 Simple call function --------------------------------------------------------------------------- 7-19
7.5.2 Modal call function---------------------------------------------------------------------------- 7-20
7.5.3 Macro call argument -------------------------------------------------------------------------- 7-21
7.5.4 Difference between G65 and M98 ----------------------------------------------------------7-23
7.5.5 Multiple nesting call--------------------------------------------------------------------------- 7-24
Chapter 8 Automatic work measurement--------------------- 8-1
8.1 Before automatic work measurement ------------------------------------8-4
8.2 Setting of data on automatic work measurement --------------------8-4
8.3 Operation of automatic work measurement----------------------------8-9
8.3.1 Corner --------------------------------------------------------------------------------------------8-9
8.3.2 Parallel ------------------------------------------------------------------------------------------- 8-13
8.3.3 Circle ---------------------------------------------------------------------------------------------8-16
8.3.4 Z level --------------------------------------------------------------------------------------------8-20
8.3.5 Positioning to the measurement position ---------------------------------------------------8-20
8.4 Handling of measured results-----------------------------------------------8-21
8.4.1 Display of the measured results-------------------------------------------------------------- 8-21
8.4.2 Reflection of measured results on the workpiece coordinate system------------------ 8-22
8.5 Lock key operations ------------------------------------------------------------8-24
2004/01/19 3 eTCOMNCPRC.doc
TC-32B Contents
Chapter 9 High Accuracy Mode A--------------------------------- 9-1
9.1 Outline -------------------------------------------------------------------------------9-2
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
9.3 Restrictions ------------------------------------------------------------------------9-7
9.3.1 Functions available ---------------------------------------------------------------------------- 9-7
9.3.2 Additional axis travel command -------------------------------------------------------------9-7
9.4 Effective Functions -------------------------------------------------------------9-8
9.4.1 Automatic corner deceleration function ----------------------------------------------------9-8
9.4.2 Automatic arc deceleration function ------------------------------------------------------- 9-9
9.4.3 Automatic curve approximation deceleration --------------------------------------------- 9-10
Chapter 10 Subprogram function --------------------------------- 10-1
10.1 Making subprogram ------------------------------------------------------------10-2
10.2 Simple call ----------------------------------------------------------------------10-3
10.3 Return No. designation from sub program-----------------------------10-4
10.3.1 Command by sub program-------------------------------------------------------------------- 10-4
10.3.2 Command by main program------------------------------------------------------------------ 10-4
Chapter 11 Feed function-------------------------------------------- 11-1
Chapter 12 S,T,M function------------------------------------------- 12-1
12.1 S function --------------------------------------------------------------------------12-2
12.2 T function --------------------------------------------------------------------------12-2
12.2.1 Commanded by tool No. ---------------------------------------------------------------------- 12-2
12.2.2 Commanding by pot No. (magazine No.) --------------------------------------------------12-2
12.2.3 Commanded by group No.-------------------------------------------------------------------- 12-2
12.3 M function--------------------------------------------------------------------------12-3
12.3.1 Program stop (M00) --------------------------------------------------------------------------- 12-7
12.3.2 Optional stop (M01) --------------------------------------------------------------------------- 12-7
12.3.3 End of program (M02, M30) -----------------------------------------------------------------12-7
12.3.4 Commands on the spindle (M03, M04, M05, M19, M111) ----------------------------- 12-7
12.3.4.1 Spindle orientation to desired angle (M19) --------------------------------------- 12-7
12.3.5 M signal level output (M400~M409)------------------------------------------------------- 12-7
12.3.6 Tool change (M06)----------------------------------------------------------------------------- 12-8
12.3.7 Workpiece counter specification (M211~M214) -----------------------------------------12-12
12.3.8 Workpiece counter cancel (M221~M224) -------------------------------------------------12-12
12.3.8.1 Tool life counter ----------------------------------------------------------------------- 12-12
12.3.9 Automatic corner deceleration (M232, M233) ------------------------------------------ 12-12
12.3.10 Tool breakage detection (M120 and M121)----------------------------------------------12-12
12.3.11 Tool breakage detection (M200 and M201)---------------------------------------------- 12-12
12.3.12 Tap time constant selection (M241 to 250) ---------------------------------------------- 12-13
12.3.13 Pallet related M codes (M410, M411, M430, and M431) ----------------------------- 12-13
12.3.14 Unclamping and clamping C axis (M430 and M431)---------------------------------- 12-13
12.3.15 Unclamping and clamping B axis (M440 and M441) ----------------------------------12-13
12.3.16 Unclamping and clamping A axis (M442 and M443) ---------------------------------- 12-13
12.3.17 One-shot output (M450, M451, M455, and M456)------------------------------------- 12-13
12.3.18 Waiting until response is given (M460 to M469) ---------------------------------------12-14
12.3.19 Magazine rotate speed (M435 to M437)-------------------------------------------------- 12-14
12.3.20 Magazine rotate to tool setting position (M501 to M599) ----------------------------- 12-14
12.3.21 Positioning finished check distance (M270 to M279)---------------------------------- 12-14
2004/01/23 4 eTCOMNCPRC.doc
TC-32B Contents
Chapter 13 Option------------------------------------------------------ 13-1
13.1 Programming precautions when using rotation axis
(index table) -----------------------------------------------------------------------13-2
2004/01/19 5 eTCOMNCPRC.doc
TC-32B Contents
(This page is a blank.)
2004/01/23 6 eTCOMNCPRC.doc
TC-32B Quick index
Chpt. 1 PROGRAM COMPOSITION
Chpt. 2 COORDINATE COMMAND
Chpt. 3 PREPARATION FUNCTION
PREPARATION FUNCTION
Chpt. 4
Chpt. 5 PREPARATION FUNCTION (CANNED CYCLE)
Chpt. 6
Chpt. 7 MACRO
Chpt. 8 AUTOMATIC WORK MEASUREMENT
(TOOL OFFSET FUNCTION)
PREPARATION FUNCTION
(COORDINATE CALCULATION))
1
2
3
4
5
6
7
8
8
Chpt. 9 HIGH ACCURACY MODE
Chpt.10 SUBPROGRAM FUNCTION
Chpt.11 FEED FUNCTION
Chpt.12 S, T, M FUNCTION
Chpt.13 OPTION
9
10
11
12
13
2004/01/16 1 eTCOMPRIN.doc
Quick index TC-32B
(This page is a blank.)
2003/04/14 2 TCOMCOOP8-2
TC-32B Chapter 1 Program Composition
CHAPTER 1
PROGRAM COMPOSITION
1
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
2004/01/22 1 - 1 eTCOMNCPR1-1.doc
1
Chapter 1 Program Composition TC-32B
1.1 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.
Command M02 (or M30) to finish the main program.
Main program
N0001 G92X100;
N0002 G00Z30
:
:
:
M02;
(2) Subprogram
A subprogram is used by calling it from the main program or other subprograms.
Command M99 to finish the subprogram.
Subprogram
N0100 G91X10;
:
:
:
M99;
1.2 Composition of Block
The program is composed of several commands. One command is called a block. A block is
composed of one or more words. One block is discriminated from another block by an end of
block code (EOB).
This manual expresses the end of block code by the symbol ";".
⋅⋅⋅
;
N0001 G92X100
Block
;
⋅⋅⋅
;
M02
Block
;
(Note 1) The end of block code
ISO code : [LF] 0A(hexadecimal)
EIA code : [CR] 80(hexadecimal)
(Note 2) One block has maximum 128 characters.
2004/01/22 1 - 2 eTCOMNCPR1-1.doc
TC-32B Chapter 1 Program Composition
1.3 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.)
Address numerical value
(Note 1) The address uses one of the alphabetical letters.
(Note 2) The address "O" can not be used except for comments.
1.4 Numerical Values
(1) Decimal point programming
Numerical values can be input in the following two ways and set by the user
parameter (Switch 1).
Command type 1 (Standard)
Programmed command Commanded axis Actual amount (mm) Actual amount (inch)
1
Rotation axis 1 deg 1 deg
X
Feed axis 1mm 1 inch
-1000
1
1.
Command type 2 (Minimum)
Programmed command Commanded axis Actual amount (mm) Actual amount (inch)
1
1.
(Note) User parameter : Refer to Instruction manual.
Rotation axis 1 mm 1 inch
Rotation axis 1 deg 1 deg
Feed axis 0.001 mm 0.0001 inch
Rotation axis 0.001 deg 0.001 deg
Rotation axis 1 mm 1 inch
Rotation axis 1 deg 1 deg
(2) Programmable range of address
The maximum number of digits is 9.
The digits less than the minimum range are ignored.
2004/01/22 1 - 3 eTCOMNCPR1-1.doc
1
Chapter 1 Program Composition TC-32B
1.5 Sequence Number
A sequence number (1~99999) can be used following the address N for each block.
Command format N *****;
i) A sequence number is used following the address N.
ii) A sequence number can be specified with up to 5-digit number.
(Note 1) The sequence number "N0" should not be used.
(Note 2) It is used at the head of a block.
Ex.) N0100 G90X100;
When a block has a slash (/) code at the head of block (the optional block skip is
commanded), a sequence number can be used either before or after it.
Ex.) N0100/ G90X100; or /N0100 G90X100;
(Note 3)
The order of sequence numbers is arbitary and need not be consecutive.
(Note 4)
The sequence number is recognized as numerical values. Therefore such numerical
values as 0001, 001, 01 and 1 are regarded as the same number.
1.6 Optional Block Skip
When a block has a slash (/) code at the start and [BLOCK SKIP] key on the operation panel is
turned ON, all information in the block with the slash code is ignored during the automatic
operation.
If the [BLOCK SKIP] key is OFF, information in the block with the slash code is effective.
That is, the block with a slash code can selectively be skipped.
..... ; / N0100 G00X100 ..... ; N0101 .....
Ignore these words
(Note 1)
A slash (/) code must be put at the start of a block. If it is placed elsewhere in the
block, an alarm is generated.
This code can be also put right after a sequence number.
(Note 2)
In the single block mode during automatic operation, when the [BLOCK SKIP] key is
ON the operation does not stop at a block with a slash code, but stops at the next
block.
1.7 Control Out/In Function
For a easier look at the program, comments can be inserted in the program.
The comment is discriminated from operation by "(" and ")" at the start and the end.
( ............. )
(Ex.) N1000 G00X200 (PRO-1);
(Note)
A comment including the control out and in codes should not be longer than one
block.
2004/01/22 1 - 4 eTCOMNCPR1-1.doc
TC-32B Chapter2 Coordinate Command
CHAPTER 2
COORDINATE COMMAND
2
2.1 Coordinate system and coordinate value
2.2 Machine zero point and machine coordinate system
2.3 Working coordinate system
2004/01/22 2 - 1 eTCOMNCPR2-1.doc
Chapter2 Coordinate Command TC-32B
5
2.1 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).
2
15
Z
Y
Tool target position:
CommandedX20.Y10.Z1
10
X
0
20
eNCPR2.01.ai
2004/01/22 2 - 2 eTCOMNCPR2-1.doc
TC-32B Chapter2 Coordinate Command
2.2 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. Each machine has its own coordinate system.
Machine zero point
X axis stroke
-X
Y axis
stroke
Table
(0,0,0)
2
2.3 Working Coordinate System
The working coordinate system is used to specify a tool motion for each workpiece.
A coordinate system previously set in the "Data Bank" is once selected, programming afterward
can be easily done by specifying that coordinate system.
Each coordinate system is set by using an offset amount from the machine zero point to the
working zero position.
(Note) Data Bank : Refer to Instruction manual.
-Y
eNCPR2.02.ai
2004/01/22 2 - 3 eTCOMNCPR2-1.doc
2
Chapter2 Coordinate Command TC-32B
( This page is a blank.)
2004/01/22 2 - 4 eTCOMNCPR2-1.doc
TC-32B Chapter 3 Preparation Function
CHAPTER 3
PREPARATION FUNCTION
3.1 Outline of G code
3.2 Positioning (G00)
3.3 Linear interpolation (G01)
3.4 Circular/helical interpolation (G02, G03)
3.5 Circle cutting (G12, G13)
3.6 Plane selection (G17, G18, G19)
3.7 Dwell (G04)
3.8 Exact stop check (G09, G61, G64)
3.9 Programmable data input (G10)
3.10 Soft limit
3.11 Return to the reference point (G28)
3.12 Return from the reference point (G29)
3.13 Return to the 2nd/3rd/4th reference point (G30)
3.14 Selection of machine coordinate system (G53)
3.15 Selection of working coordinate system (G54~G59)
3.16 Additional working coordinate system selection
(G54.1)
3.17 Scaling (G50, G51)
3.18 Programmable mirror image (G50.1, G51.1)
3.19 Coordinate rotation function (G68, G69)
3.20 Coordinate rotation using measured results (G168)
3.21 Absolute command and incremental command
(G90, G91)
3.22 Change of working coordinate system (G92)
3.23 Skip function (G31, G131, G132)
3.24 Continuous skip function (G31)
3.25 Change of tap twisting direction (G133, G134)
3.26 High speed peck drilling cycle (G173)
3
2004/01/22 3 - 1 eTCOMNCPR3.doc
3
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
2004/01/22 3 - 2 eTCOMNCPR3.doc
TC-32B Chapter 3 Preparation Function
3.1 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
Modal
One-shot
The G code is effective until another G code in the
same group is commanded.
The G code is effective only at the block in which it is
specified.
3
2004/01/22 3 - 3 eTCOMNCPR3.doc
Chapter 3 Preparation Function TC-32B
Group G cord Contents Modal
G00* Positioning
G01 Linear interpolation
G02 Circular/ helical interpolation (CW)
G03 Circular / helical interpolation (CCW)
Modal
G102 XZ Circular interpolation (CW)
G103 XZ Circular interpolation (CCW)
3
G202 YZ Circular interpolation (CW)
G203 YZ Circular interpolation (CCW)
G04 Dwell One-shot
G09 Exact stop check One-shot
G10 Programmable data input One-shot
G13 Circular cutting CCW One-shot
G17* XY plane selection
G18 YZ plane selection
G19 ZX plane selection
G22* Programmable stroke limit on
G23 Programmable stroke limit cancel
G28 Return to the reference point
G29 Return from the reference point
G30 Return to the 2nd /3rd/4th reference point
G31 Skip function One-shot
Modal
Modal
One-shot
G36 Coordinate calculation function (Bolt hole circle)
G37 Coordinate calculation function (Line-angle)
One-shot
G38 Coordinate calculation function (Line-angle)
G39 Coordinate calculation function (Grid)
G40* Tool dia offset cancel
G41 Tool dia offset left
G42 Tool dia offset right
The G codes with * mark indicates the modal status when the power is turned ON.
(Note1) Details of coordinate calculation functions are described in " Chapter 6 ".
(Note2) Details of tool dia offset are described in " Chapter 4 ".
2004/01/22 3 - 4 eTCOMNCPR3.doc
Modal
TC-32B Chapter 3 Preparation Function
Group G cord Contents Modal
G43 Tool length offset +
G44 Tool length offset -
G49* Tool length offset cancel
G50* Scaling cancel
G51 Scaling
G50.1 Mirror image cancel
G51.1 Mirror image
G52 Local coordinate system
G53 Machine coordinate system selection
G54* Working coordinate system selection 1
G55 Working coordinate system selection 2
G56 Working coordinate system selection 3
G57 Working coordinate system selection 4
G58 Working coordinate system selection 5
G59 Working coordinate system selection 6
G54.1 Extended working coordinate system selection
Modal
Modal
Modal
3
One-shot
Modal
G60 Single direction positioning One-shot
G61 Exact stop mode
Modal
G64* Cutting mode
G65 Macro call One-shot
G66 Macro modal call
Modal
G67* Cancel macro modal call
G68 Coordinate rotation function
G69* Coordinate rotation function cancel
G168 Coordinate rotation using measured results
Modal
2004/01/22 3 - 5 eTCOMNCPR3.doc
3
Chapter 3 Preparation Function TC-32B
Group G cord Contents Modal
G90* Absolute command
Modal
G91 Incremental command
G92 Working coordinate system setting One-shot
G94 Feed rate per minute
G98* Return to the initial point level
Modal
G99 Return to the R point level
G73 Canned cycle (High-speed peck drilling cycle)
G74 Canned cycle (Reverse tapping cycle)
G76 Canned cycle (Fine boring cycle)
G77 Canned cycle (Tapping cycle, synchro mode)
G78
G80* Canned cycle cancel
Canned cycle (Reverse tapping cycle, synchro
mode)
G81 Canned cycle (Drill, spot drilling cycle)
G82 Canned cycle (Drill, spot drilling cycle)
G83 Canned cycle (Peck drilling cycle)
G84 Canned cycle (Tapping cycle)
G85 Canned cycle (Boring cycle)
G86 Canned cycle (Boring cycle)
G87 Canned cycle (Back boring cycle)
G89 Canned cycle (Boring cycle)
Modal
2004/01/22 3 - 6 eTCOMNCPR3.doc
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
G182 Canned cycle (Double drilling cycle)
G183 Canned cycle cancel (Peck drilling cycle) One-shot
G185 Canned cycle (Double boring cycle)
G186 Canned cycle (Double boring cycle)
G189 Canned cycle (Double drilling cycle)
G100 Non-stop automatic tool change One-shot
Modal
3
2004/01/22 3 - 7 eTCOMNCPR3.doc
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)
3
G125 Automatic measurement Circle center (Boss, 3 points)
G126 Automatic measurement Circle center (Hole, 4 points)
G127 Automatic measurement Circle center (Boss, 4 points)
G128 Automatic measurement Z-axis height
G129 Automatic measurement Corner (Groove)
G31 Measurement feed
G131 Measurement feed
G132 Measurement feed
G133 Changeover of tap twisting direction (CW)
G134 Changeover of tap twisting direction (CCW)
(Note)
Commands G120 to G129 are described in detail in " Option, Automatic
Measurement " in the instruction manual.
One-shot
One-shot
One-shot
2004/01/22 3 - 8 eTCOMNCPR3.doc
TC-32B Chapter 3 Preparation Function
3.2 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 G00 X_Y_Z_A_B_C_ ;
When the additional axis is commanded and the optional additional axis is not installed, an alarm
will occur.
In the positioning mode actuated by the G00 code, the execution proceeds to the next block after
confirming the in-position check. (Note 1)
3
eNCPR3.01.ai
(Note 1)
In-position check is to confirm that the machine detecting position is within the
specified range around the target (end) point.
(This range is set by the machine parameter for each axis.)
(Note 2)
The rapid traverse rate is set by the machine parameter for each axis.
Accordingly, rapid traverse rate cannot be specified by the F command.
2004/01/22 3 - 9 eTCOMNCPR3.doc
Chapter 3 Preparation Function TC-32B
3.3 Linear interpolation (G01)
Linear interpolation moves a tool linearly from the current position to the target position at the
specified feedrate.
Command format G01 X_Y_F_ ;
Up to X,Y,X and one additional axis can be controlled simultaneously.
When the additional axis is commanded and the optional additional axis is not installed, an alarm
will occur.
3
The feedrate is commanded by the address F. Once the feedrate is commanded, it is effective until
another value is specified.
When the X, Y, and Z axes are commanded, the feedrate is determined by the value entered to mm
/ min.
When the additional axis is commanded, the feedrate is determined by the value entered to ｰ
/min.
End
point
Start
point
eNCPR3.2.ai
(Note 1) Feedrate along each axis is as follows:
When "G01 G91 X
Feedrate along X axis: Fx＝ ─── • f
L
β
Feedrate along Y axis: Fy＝ ─── • f
L
( L =
2004/01/22 3 - 10 eTCOMNCPR3.doc
α2 + β2 )
α Yβ Ff ;" is programmed:
α
Loading...