Table of Contents
Advertisement
With FN20: WAIT FOR you can delay execution of the NC program until the
entered condition is fulfilled. These conditions can be comparisons of a PLC
variable with a constant (See "PLC Programming" on page 7 – 3).
With FN17: SYSWRITE ID420 NR0 IDX0 = 0, all coordinate transformations (e.g.
cycles 7, 8, 10, 11, 19) performed in the tool-change program become globally
effective. Without this block, they remain locally effective (only in the tool-
change program).
To ensure that during a block scan the tool-change program is not run until the
end of the scan, you must enter the instruction NCMACRO=TC in the
MGROUPS.SYS file. (See "Returning to the Contour" on page 6 – 294). If no
NC program is specified in the NCMACRO.SYS file, the TOOL CALL is
executed as before.
For test purposes, the tool-change program can be called from the TNC
partition. In this case, the program call is handled as PGM CALL, i.e. defined
values such as Q parameters and feed rate remain globally effective.
If the tool-change program is called from the PLC partition, the tool-change
program is handled as cycle call, i.e. defined values remain only locally
effective.
0 BEGIN PGM TCALL MM
1 M112 T4 ; INSERT ROUNDING TO POSITION CONTINUOUSLY
2 FN18: SYSREAD Q1 = ID60 NR1 IDXO ; TOOL NUMBER
3 FN18: SYSREAD Q2 = ID60 NR2 IDXO ; TOOL AXIS
4 FN18: SYSREAD Q3 = ID60 NR3 IDXO ; SPEED
5 FN18: SYSREAD Q4 = ID60 NR4 IDXO ; OVERSIZE IN TOOL LENGTH DL
6 FN18: SYSREAD Q5 = ID60 NR5 IDXO ; OVERSIZE IN TOOL RADIUS DR
7 FN19: PLC=+Q / +0 ; INFO FOR PLC FOR PRE-POSITIONING THE MAGAZINE
8 LBL 5 ; CHECK WHETHER TOOL IS ALREADY IN THE SPINDLE
9 FN 18: SYSREAD Q18 = ID2000 NR60 IDX2301; READ BYTE 2301
10 FN 9: IF +Q18 EQU +0 GOTO LBL 5 ; BYTE2301=0: WAIT FOR PLC
11 FN 11: IF +Q18 GT +1 GOTO LBL 3 ; BYTE2301=2: TOOL IS ALREADY
12 ; IN THE SPINDLE
13 FN 18: SYSREAD Q10 = ID1000 NR4210 IDX0 ; CHANGE POSITION IN AXIS X
14 FN 18: SYSREAD Q11 = ID1000 NR4210 IDX2; CHANGE POSITION 1 IN AXIS Y
15 FN 18: SYSREAD Q12 = ID1000 NR4210 IDX5; CHANGE POSITION IN AXIS Z
16 FN 18: SYSREAD Q15 = ID1000 NR4210 IDX3; CHANGE POSITION IN AXIS Y
17 L X+Q10 Y+Q11 Z+Q12 R0 F MAX M91 ; MOVE TO TOOL CHANGE POSITION
18 LBL 4 ; BYTE2300=1: SPINDLE AND MAGAZINE IN POSITION ?
19 FN18: SYSREAD Q18 = ID2000 NR60 IDX2300
20 FN10: IF +Q18 NE +1 GOTO LBL 4
21 L Y+Q15 R0 F MAX M91 ; TOOL IN CHANGER
22 L Y+Q11 M71 ; CLAMP THE TOOL AND RETURN TO THE CHANGE POSITION
23 LBL 3
24 TOOL CALL Q1 Z SQ3 DL+Q4 DR+Q5 ; TOOL CALL WITH T STROBE
25 M113 ; CANCEL M112
26 END PGM TCALL MM
6 – 422
HEIDENHAIN Technical Manual TNC 426, TNC 430
Advertisement
Table of Contents
