Gang lathe need X before Z in post

[marc7X3XJ]

Ok, I have gotten decent code out of the CNC NEW PP now as far as direction of tool approach goes but now I am having a little issue with tool change commands. I just dragged an expensive carbide drill across the face of a test part. After the drill operation it retracted to the safe plane but on the next tool call the Z move was first and for some reason the boring operation was starting about .002" into the part instead of at the safe plane. I need to look at the file and try to figure that out but seeing how it is a gang lathe I think that the PP should write the X move before the Z move on tool changes because all the tools should be at the safe plane retract from the prior operation. Can someone help me figure this out or is there a very specific reason why it is not done this way?

Also the programs written by the PP are ending in a M15 and not an M30 so some help on that would be great too.

Thank you,
Marc

[daniel_lyall]

You need to add the post you are using and what machine and control?

[marc7X3XJ]

The control is a GSK 980TDc and I am attaching the post now.

Thank you,
Marc

[marc7X3XJ]

I figured out how to reverse the X-axis and Z-Axis output using Visual Studio Code so now the only small issue that I am having is that there is no M30 generated at the end of the program. It is not a big deal to add that but it certainly would be more convenient if it was generated from the PP. 

I am attaching the revised PP (original PP is posted above) and the code generated from each in case this can help anyone else using a CNCNEW machine. Please be sure to check the PP thoroughly on your own because I am new to this and will not take responsibility for any problems that arise from the revised PP usage.

Does anyone know how to get the M30 to generate automatically?

Marc

[daniel_lyall]

If the M15 is not meant to be there and is in the spot where M30 should be change the 15 to 30.

[marc7X3XJ]

It looks like the PP puts in the G15 at the end of each operation. I am looking at the end of the cps file and I do not know enough about them to add or modify where to put a M30  when I program ends.

[daniel_lyall]

Does the M15 need to be there and do you use a C axis? 

it is on line 253

 case "ENABLE_C_AXIS":

    machineState.cAxisIsEngaged = true;

    return (spindle == SPINDLE_MAIN) ? 14 : 14;

  case "DISABLE_C_AXIS":

    machineState.cAxisIsEngaged = false;

    return (spindle == SPINDLE_MAIN) ? 15 : 15;

[marc7X3XJ]

The machine does have live radial tools but I am not using them on this part. The M15 is doing no harm here. Not having the M30 is is the real issue that slows me down a little if I forget to manually add it.

I have searched my Haas PP for "30" and there are only two instances and only one of those appears to be related to mFormat at the end of the PP. I have copied and pasted the following line after the (COMMAND_END) ;  in my CNC New PP

writeBlock(mFormat.format(30));

This seems to be working but please let me know if there is a better way to accomplish this or if I did it correctly. I will include my new complete PP if anyone want to check it out.

Thank you,
Marc

Marc

[daniel_lyall]

That is what I was going to suggest you do.

[marc7X3XJ]

I figured it had to be something simple but I was worried that I could screw the whole thing up without the help of a pro. 

Marc

[daniel_lyall]

I am definitely not a pro, I have just been doing it long enough to know what goes where.