Fanuc mill/turn postprocessor not outputting milling mode M code.

[Stevenl89]

I own a Dainichi F20BM lathe with Fanuc 16T control. The lathe has live tooling(not Y axis) and a sub spindle.

I have managed to get a postprocessor for the machine but there is still som problems. 

When I try to do a live tooling operation in Fusion 360 I cant get the code to ouput M35 (which is activate milling mode) on the machine before it starts with the live tooling operation. I have activated "live tool" in the tool library in Fusion 360.

It also seems like the code outputs a negative number for the C axis. Is this OK? 

Anyone who can help me with this? Please see attached files. 

Thanks! 

[Arun.rs]

Hi @Stevenl89 

Thanks for raising your concern via Forum.

Could you please share your model file so that I can have look into the same? 

File>Export>.F3d save the file and attach the file to this thread.

Regards

[Stevenl89]

Thank you so much for looking at it! File is attached 😊

[Arun.rs]

HI @Stevenl89 

I think you have wrongly assigned the C axis engagement codes. 

1. Got to 'function getCode' in post processor. Change as below,

case "ENABLE_C_AXIS":
    machineState.cAxisIsEngaged = true;
    return (spindle == SPINDLE_MAIN) ? 35 : 135;
  case "DISABLE_C_AXIS":
    machineState.cAxisIsEngaged = true;
    return (spindle == SPINDLE_MAIN) ? 34 : 134;

I am not sure about the lock codes, I have set M89 for Main and M189 for Sub spindle.

 case "LOCK_MULTI_AXIS":
    return (spindle == SPINDLE_MAIN) ? 89 : 189;
  case "UNLOCK_MULTI_AXIS":
    //return (spindle == SPINDLE_MAIN) ? 36 : 136;
  case "CLAMP_CHUCK":

2. Got to line number 1661 and remove the '//' from below code.

writeBlock(feedMode, gPlaneModal.format(plane), cAxisEngageModal.format(getCode("ENABLE_C_AXIS", getSpindle(PART))));

 

Save the file and test the NC code carefully.

For detail info about the post editing please refer the  FAQ link

Regards