G55 Problem - VF2

[JMFabrications]

Im having a strange issue with the WCS on my '02 VF2. Im doing a simple drill operation on these aluminum brackets we make, I have 2 vises setup on the table. I use G54 for the left vise and G55 for the right vise, I set the part zero for both WCS in the offset page but for some reason the machine wont use the Y offset in G55. It will use the X offset for G55 just fine, but defaults to the Y offset for G54 when it should use G55. I even tried setting the Y on G55 to 0 or some random number like -7.0000 and it still uses the G54 Y. Is there a parameter or setting im missing on the machine? Here is the code mastercam posted for me:

( T1 | 1/8 CENTERDRILL | H1 )
( T2 | 13/64 DRILL | H2 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T1 M6
N130 G0 G90 G54 X.3765 Y.25 S4966 M3
N140 G43 H1 Z.1
N150 M8
N160 G99 G81 Z-.05 R.1 F30.
N170 X4.5736
N180 G80
N190 G55 X.3765 Z.1
N200 G99 G81 Z-.05 R.1 F30.
N210 X4.5736
N220 G80
N230 M5
N240 G91 G28 Z0. M9
N250 M01
N260 T2 M6
N270 G0 G90 G54 X.3765 S6586 M3
N280 G43 H2 Z.1
N290 M8
N300 G99 G83 Z-1.35 R.1 Q.45 F40.
N310 X4.5736
N320 G80
N330 G55 X.3765 Z.1
N340 G99 G83 Z-1.35 R.1 Q.45 F40.
N350 X4.5736
N360 G80
N370 M5
N380 G91 G28 Z0. M9
N390 G28 X0. Y0.
N400 M30

Thanks,
Jim

[Geof]

You have this line; N190 G55 X.3765 Z.1

Try putting the actual Y coordinate in this line. Your last Y position was defined in G54 and the machine will not move Y again until it sees another Y command; just the the work coordinate from G54 to G55 will not move the Y without a Y command in G55.

[JMFabrications]

Wow I feel dumb! That worked.....Geof to my rescue!

Thanks again,
Jim