Is G92 Evil Or Should I Learn To Use It

[eliot15]

I apologize for not having the actual code to post.

Buddy o' mine was tearing his hair out on a program today that was doing a helical interpolation (I think) with like L49 (49 repetitions of a sub routine).

I'm pretty sure the sub routine had a G92 in it. (again, I apologize for not having the actual code).

So he'd reset the program, and execute the line:

G43 Z1. H2

but the tool would plunge to the last iteration of the sub program the control seemed to know about (or at least thats how it appeared to us). The tool wouldn't recognize Z1. It just kept going, and going, and going..... to like Z-3.000

I kept telling him, "DUDE, either your tool isn't touched off right, or your Z0. isn't picked up right!!!!" And he said, "DUDE, no way!!!". So we checked both, and both were right!!!!

So I went into MDI mode and brought his tool down to Z1. All was well. I guess I reset some modal values when I did that, but whats up with this G92 stuff?????

I'm SURE this was a G92 related problem, but I've never used G92 'cause I hear its evil.

Is it?????? What does it do????

[Geof]

It is EVIL buahahahahaha

I have never used G92 but I read up on it when I started using G52. They are similar in some ways but very different in others and it is the difference I didn't like.

Here is my understanding of it.

With G92, no matter what Work Zero you are using, the location of the tool at the time you command G92 becomes the Work Zero location. Which sounds fine and is fine for the first time you command G92. For instance if you have G54 as the active Work Zero and it is located at X-4. Y-4. you can move to X-1. Y-1. and command G92. Now your work zero is at X-5. Y-5. and if you repeat the move and command you gradually walk off the table. And if you want to get back to the original Work Zero location you need to know where it is within the, now shifted, Work Zero you are working in.

I got the feeling I didn't know where I was when I started thinking about how to program multiple locations using G92. With G52 you explicitly define where an extra Work Zero is located, but you do not move the original Work Zero. Using a similar example to that above with G54 at X-4. Y-4. the command G52 X-1. Y-1. tells the machine to use the position X-5. Y-5. as the Work Zero and G52 X0. Y0. tells it to go back to the original X-4. Y-4. I found this easier to visualize when planning a program with multiple locations and multiple subroutines.

In actual fact the way the machine controller handles G52 is that it always adds the G52 coordinates to the active Work Zero coordinate. But if the value(s) in the G52 register are zero nothing is added.

I hope this helps rather than confuses. I am good at both.

[HuFlungDung]

I think of G92 as a shift of the G53 machine coordinate system. And since G53 underlies all the other work offsets, a G92 command will cause a proportionate shift of all work offsets.

There is no effective way to cancel a G92 offset except to make a movement to a known position in the G53 machine coordinate system. Typically, this would be machine home. So you'd make a movement to machine home, and command G92 X0 Y0 Z0 at that position and it is effectively cancelled.

If you happen to run a Haas, it has G92 way down at the bottom of the list of work offsets. Every new G92 command has a cumulative effect, and if you go into the work offset register, you can view the accumulated G92 values. In the Haas, you can cancel the current G92 by entering all zeros into the G92 register.

It is valuable to know how to use G92...not so much for 3 axis work, but you can do some miracles saving time on multi-turn 4th axis work.

For repeats in a subroutine, you must be very careful to know exactly where you have the tool positioned at the moment the G92 is commanded, simply for the reason that the new G92 command will add its new values to the existing accumulated G92 values.

Starting over with G92 at the beginning of the program basically requires a return to machine home, with a command to set G92 X0 Y0 (you can leave any axis out if you are not making any adjustments in said axis) while at home position. Then you can proceed into the subroutine and use the G92 in an accumulative fashion again.

[eliot15]

Wow. Thats scary. Remind me to never use G92.

Odd, though, that hitting RESET didn't seem to cancel the controls knowledge of its last commanded G92 location (if thats what was actually happening, though that sounds kinda' plausible, based on your not confusing explanation).

The tool kept running to that location (the Z depth at like iteration number 39 of the sub program) even after hitting RESET. Weird.

Only way I could get the machine to behave like the machine I love and know again was to call it a *$*^#*&@, and then execute another G54 in MDI mode.

Thanks for the reply.

[eliot15]

And thanks HuFlungDung (which is really fun to say). Didn't see your post 'till after my last one.

Oh, and "First you get good, then you get fast, then you get grouchy" has become a bit of a mantra
at work. Just rattled it off one day, but it really caught on....