Drilling Post Problem

[Anonymous]

Hey all,

I tried to do a drilling operation the other day but it did not work as expected on the machine. The toolpath looked correct and the simulation also appeared correct. But when the machine went to drill the holes, it only drill the first one. It proceeded to the location of the second hole and then to the third and fourth, but it did not go down to drill out the holes.

I use a post processor for the Shopsabre originally from @skidsolo which is attached.

I've recreated my problem with a simplified model:

G90
S16000
M3
G4 X4
G0 X101.600 Y25.400 Z40.400
G0 Z30.400
G81 X101.600 Y25.400 Z0.000 R30.400 F1355 #first hole drills
G0 X25.400 #no indication of Z command for second hole
G0 Y101.600 #third hole
G0 X101.600 #fourth hole
G80
G0 Z40.400
M5
G53 Z
G53 Z
X0Y0

[LibertyMachine]

If I give you a suggestion, any chance you could test it out?

Manually remove the G0 from the beginning of the lines for the last 3 holes

Fanuc doesn't like having the G0 there and it will just ignore the G81 command

Quick edit and sidenote: I don't think I've ever seen a shorter post processor...

[Anonymous]

@LibertyMachine

Thanks for the suggestion. I ran the modified G-code today and it worked. Now how do I fix the post processor so that there is no G0?

[LibertyMachine · Accepted solution]

I took a quick stab at it, and it should work. However, there is an annoying space where the G0 was and I don't know if that's going to cause you any grief.

Let me know and if it is an issue, I will do some more digging and learn how to make that go away.

[Anonymous]

Your post processor worked. One question I have is if the change you made was specifically for drill operations. I'm hoping that fixing this problem won't create problems for other operation types, or when operations are one after the other in a post.

[LibertyMachine]

Your Post Processor is configured to utilize only one type of drilling cycle, the G81 cycle. This is a drill to depth and rapid out. Any other cycle will result in long hand code.

The section of code that I edited only controlled the output of a G0 on subsequent drilled holes, no other motion. You "should" be good to go.

But as always, test test test