fanuc parameter# for current work offset?

[Jeremy Herron@DBS Solutions™]

Does anyone know the parameter number on a fanuc for the current work offset when using G54-G59? For instance if you are using G54.1 P1-P300 it is #4130. I am writing a macro to probe a part, set any work offset desired, and populate the WSEC table and this variable is all I missing.

 

TIA.

[GnoGueyJose]

This is our usual starter for setting up WSEC on our MAM72's;

 

%

O7777(BLOCK CHECK & WSEC UPDATE)

 

(SET G59)

#5321=-14.966

#5322=-17.665

#5323=-17.635

#5324=0

#5325=0

G0G90G59

 

(PROGRAM USES G54 PART LOCATED AT CENTER OF ROTATION)

 

T1M6

 

#181=0 (X SHIFT FROM CENTER OF ROT)

#182=0 (Y SHIFT FROM CENTER OF ROT)

 

#191=17. (SET X STOCK SIZE)

#192=3.25 (SET Y STOCK SIZE)

#193=6. (SET Z STOCK SIZE)

 

#159=.05 (X POS. TOLERANCE)

#160=.01 (Y POS. TOLERANCE)

 

#161=.125 (X + TOLERANCE)

#162=.125 (Y + TOLERANCE)

#163=.125 (Z + TOLERANCE)

 

#171=0 (X - TOLERANCE)

#172=0 (Y - TOLERANCE)

#173=0 (Z - TOLERANCE)

 

(H FOR SIZE TOL)

(M FOR TRUE POS TOL)

G43H#517Z12.75

G65P9832(PROBE ON)

 

G65P9810X#181Y#182F200. (X Y SAFETY MOVE TO APROX BLOCK CENTER)

 

G65P9810Z[1.+#193]F200. (Z SAFETY MOVE 1 INCH APPROX ABOVE BLOCK)

 

(Z MEASURE WITH Z TOLERANCE CHECK BELOW)

G65P9811Z[#193]

IF[#142GE#163]GOTO3003

IF[#142LE#173]GOTO3013

#157=#142(Z POSITION ERROR)

 

(X MEASURE AT Z-.5 POSITION WITH TOLERANCE CHECK IN X SIZE & POS BELOW)

G65P9812X#191Z[#193-.5]

IF[#143GE#161]GOTO3001

IF[#143LE#171]GOTO3011

IF[#140GE#159]GOTO3021

#155=#140(X POSITION ERROR)

 

(Y MEASURE AT Z-.5 POSITION WITH TOLERANCE CHECK IN X SIZE & POS BELOW)

G65P9812Y#192Z[#193-.5]

IF[#143GE#162]GOTO3002

IF[#143LE#172]GOTO3012

IF[#141GE#160]GOTO3022

#156=#141(Y POSITION ERROR)

 

(-)

(UPDATE WSEC)

IF[ABS[#155]GT.054]GOTO155

#26010=#155(X ERROR TO WSEC OFFSET 1)

N155

IF[ABS[#156]GT.054]GOTO156

#26011=#156(Y ERROR TO WSEC OFFSET 1)

N156

IF[ABS[#157]GT.054]GOTO157

#26012=#157(Z ERROR TO WSEC OFFSET 1)

N157

(-)

 

 

(-)

G65P9833(PROBE OFF)

(-)

G53Z0

G49

G90

M99

 

 

N3001(X + ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=11(X OVERSIZE)

 

N3011(X - ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=12(X UNDERSIZE)

 

N3021(X - ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=13(X OUT OF POSITION)

 

 

N3002(Y + ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=21(Y OVERSIZE)

 

N3012(Y - ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=22(Y UNDERSIZE)

 

N3022(Y - ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=23(Y OUT OF POSITION)

 

 

N3003(Z + ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=31(Z OVERSIZE)

 

N3013(Z - ALARM)

(-)

G65P9833(PROBE OFF)

(-)

G28G91Z0

#3000=32(Z UNDERSIZE)

 

%

 

Hope you can get something useful from this.

[Jeremy Herron@DBS Solutions™]

Thanks. I have all that worked out. I program the probing of the part for each specific part in mastercam and sets wahtever work offset I want and then my macro does the math to determine the difference fro C.O.R and populates whathever g54.4 p# I want. Sets my center of rotation work offset (just in case an operator erases or changes it), and then double checks all the math and alarms if something is wrong. What I need is the parameter # for whether I am using G54, 55, 56... 59. On a Mazak it is #4012, and if it is a G54.1 p1-p300 it is #4130. #4130 is the same on a fanuc, #4012 is not.

[Jeremy Herron@DBS Solutions™]

I found it. It is #4014 if anyone is interested.

[GoetzInd]

Its 4014

edit:oops Im late