Siemens SINUMERIK 840D sl Function Manual page 607

;Machine contour section 2 with "CUTTER_2"tool
N200 T="CUTTER_2"
N210 WZW
N220 G0 X170 Y30 Z10 S3000 M3 D1
N230 Z-5
N240 G1 G64 G42 F500 X150 Y50
N250 Y150
N260 G2 J50 X100 Y200
N270 G1 X50
N280 Y50
N290 X150
N300 G0 G40 G60 X170 Y30
N310 Z100 D0
End of contour section 2
...
M30
PROC WZW
Tool change routine
N500 DEF INT TNR_AKTIV
N510 DEF INT TNR_VORWAHL
N520 TNR_AKTIV = $TC_MPP6[9998,1]
N530 GETSELT(TNR_VORWAHL)
;
;Execute tool change only if tool is not yet active
N540 IF TNR_AKTIV == TNR_VORWAHL GOTOF ENDE
N550 G0 G40 G60 G90 SUPA X450 Y300 Z300 D0
N560 M6
;
END: M17
PROC SUCHLAUF_ENDE SAVE
ASUB for calling the tool change routine after block search
N1000 DEF INT TNR_AKTIV
N1010 DEF INT TNR_VORWAHL
N1020 DEF INT TNR_SUCHLAUF
N1030 TNR_AKTIV = $TC_MPP6[9998,1]
N1040 TNR_SUCHLAUF = $P_TOOLNO
N1050 GETSELT(TNR_VORWAHL)
N1060 IF TNR_AKTIV ==TNR_SUCHLAUF GOTOF ASUP_ENDE
N1070 T = $TC_TP2[TNR_SUCHLAUF]
N1080 WZW
N1090 IF TNR_VORWAHL == TNR_SUCHLAUF GOTOF ASUP_ENDE
N1100 T = $TC_TP2[TNR_VORWAHL]
ASUP_ENDE:
N1110 M90
N1120 REPOSA
Basic logic functions: Mode group, channel, program operation, reset response (K1)
Function Manual, 11/2006, 6FC5397-0BP10-2BA0
; Preselect tool
; Call tool change routine
; Approach block for contour section 2
; Infeed
; Start point of contour
; Deselect radius compensation
; Deselect length correction
; Variable for active T number
; Variable for preselected T number
; Read T number of active tool
; Read T number of preselected tool
; Approach tool change position
; Execute tool change
; Variable for active T number
; Variable for preselected T number
; Variable for T number determined in search
; Read T number of active tool
; Read T number determined by search
; Read T number of preselected tool
; T selection by tool name
; Call tool change routine
; Restore T preselection by tool name
; Check-back signal to PLC
; ASUB end
Detailed description
2.5 Block search
49