sometimes posts g55 when g54 is programmed

[rob.b]

Hi guys, currently running X6 and have had no dramas up until recently when once the program had been sent it would change to g55 by itself even though the settings and post says g54, our post is perfect haven't changed anything on it.

if anyone has any idea what might cause this and how to fix it would be much appreciated.

Regards

Robbie

[Colin Gilchrist]

The post reads values from the NCI file to generate Work Offset output. There is a mechanism built into Mastercam that will "auto-increment" the work offset number, whenever Mastercam senses a change in the orientation of your Tool Plane.

 

The easiest way to correct the problem is to go into the Planes Manager and set the Work Offset number to '0'. When Mastercam prompts you, choose the option to update the existing planes being used.

 

A setting of '-1' in the work offset data entry field is never a good idea. It will auto-magically screw you when you aren't paying attention...

[ahaslam]

 If you have two tools set with the same work plane (or even the same tool with different operations) but different tool plane mastercam will post out a G55 when the T-Plane changes. Select all your tool paths that use the same plane then right click and use the feature "Edit Common Parameters." Select planes then select your working plane. Doing this will force all your tool paths onto the same plane.

[rob.b]

sweet thanks for your help I will definitely try those tips.