[angelw]

I have my cam program to add 20 to the diameter offset like your saying. But as far as the compensation value I usually leave that set at zero and than if I need to increase or decrease I will put in a small +or- value. I don't know if that is the proper way of doing things but it is the way I have been doing it on my haas and milltronics machines and seems to work well. 99% of the time I am using my cam system for programing. I will make adjustments in that so I don't have to remember compensation numbers. So maybe that way won't work on this machine?

Thanks
Jake

Hi Jake,
No, this is the only Tool Offset Registry you have on your machine. The Only other Offset Registry you have is for Workshift (G54 to G59)

I don't understand what you mean by "I have my cam program to add 20 to the diameter offset", because the Example Code in your opening Post shows the same Offset Number for both your Tool Length and Tool Radius Offsets. For T09 you have H09 for Length and D09 for Radius Offsets. This would work if you had separate offsets for Tool Radius, but your control is not equipped in this way. If the Offset value of -7.014, shown in the attached picture in your last Post, is the Tool Length Offset used in the Example Program, then this value would also have been called up for the Tool Radius Offset via D09. The minus value in a Tool Radius Offset actually inverts G41 and G42, meaning that G41 works like G42 and vice versa when a minus value is used. This, and because you have no Circular Interpolation command in the program is the reason why an interference error was not raised by the control.

If what you mean, is that you have the CAM software, compensate for the Tool Radius in the program, then you still need to be calling a different Offset Number for Tool Radius than the Offset being used for Tool Length in your program. Change your program to use D59 (for tool T09) and register a Zero value in Offset Number 59 (if the CAM software is compensating for the Tool Radius in the program) and your program should run. You will still have issues applying and cancelling the Tool Radius Offsets in way in which you show it being done in your example program. You may get away with it when the Tool Radius Offset value is Zero, but its not good programming form.

Regards,

Bill