G92 And G54...G59

[jorgehrr]

Hi, please help me to understand -

I'm trying to understand programs in machines centers. (I work with lathes)

What is the difference, relation between G92(selection of coordinate system)
and G54...G59. Aren't they the same (distance from machine zero and part zero) Do I need a G92 every time I programmed a G54...G59???

Also, I see the H (high) offset in some machines is positive and in others is negative.

And finally what are the G codes they need to be in a safety block.

Thank you in advance

Jorge

[HuFlungDung]

When your machine boots up and homes itself, it establishes the machine coordinate system, and the origin of that coordinate system is typically set by parameter. The machine coordinate system is called G53 and it is the 'real coordinate system' upon which all the work shifts are based. The work shifts are your G54 to G59 and the coordinates associated with the work shifts are simple distances from the machine zero of the G53 machine coordinate system. You can always cancel a workshift by calling another workshift or making a move to a position in the machine coordinate system directly by calling a G00 G53 X.xxxx Z.zzzz

G92 has a lot more power than a workshift. It applies new values to the machine coordinate system axis, essentially moving the G53 origin somewhere else (this is a simplification, not exact but close enough to serve as a warning).

Thus, using a G92 supercedes all workshifts and will move them all, because the G92 represents new values assigned overtop the G53. Think of it as similar to reprogramming the axis displays to show values of your choice. Although in the background, the machine may maintain its own secret set of registers for the current position, what you see displayed will be fictitious axis values, but real enough to affect every program you run.

You cannot cancel a G92 because it is not a workshift. Rather, it was a renaming of the G53 axis positions, so to cancel the effect of calling a G92,you must return to a known position in the machine coordinate system, and then rename the axis back to what they 'should be'.

The danger of the G92 is that it is an immediate transposition of the coordinate system, and cannot be undone, and if a mid program restart is attempted with the machine out of position, and the control reads the G92 again, it will royally screw your tool positions from that point forth, because the G92 is applied always to the current position of the machine.

In lathe, you can and should return to home always, if you call a new G92 for each tool. Never restart the program from the current position after an abort. Staying with workshifts is the recommended safe way to operate nowadays. However, if you have to run an older control that has no workshift capability, then the above mentioned methods should keep you fairly safe.

[dlbnh]

Long and short of it is as follows: I'll use Fanuc as a reference here.
G54 - G59 are "work coordinates", commonly the values are taken from machine home or machine coordinate (G52) and used to refererence a part zero or shifts for subs or whole programs. In the case of a lathe, your "X" is commonly spindle center. "Z" anywhere.
G92 is an "incremental" shift in work coordinate, in that it will describe a new point of departure. For instance, you have G54 active and want to move your stock out from the spindle an nose extra 3" to try something like 3 parts in a row before stock feed without losing the initial G54 value.
Physically Go to "Z" +3.0" farter from the spindle with your "zero tool" and MDI or in the body of the program, call G92 Z0.0 -Done-
"Beware" if you call (machine reads)G54 - G59,G52,G53 etc. it will revert to that WCO so make sure there is only one work corodinate offset called before G92 is used and none after it. Get the drift?
Crash city if you make mistakes.

[JROM]

I never use G92.
G54 thru G59 are what I call fixture offsets, like if you have 3 or four vises on the table and want to jump around for different jobs. When the control sees a M30 at the end of the program it rewinds the program and resets all the default settings. Most of the time this resets the fixture offset to G54. So what I do is put the fixture offset (G54-G59) at the top of every tool path.
Then if I want to do a restart at a certain tool in the middle of the program I know the proper fixture offset is being used.

[jorgehrr]

Well....I wish I could say that I got it... but I think I will understand better when I do my first set up.

The fact that G92 does not need to be used like JROM mentions, confuse even more. It has to be an advantage or disadvantage when this code is in use and I hope I can figure out tomorrow when I run my program. ( just a couple of holes and a tap to start)

Thank you all for sharing your time.


Jorge

[cnc-king]

Originally Posted by JROM I never use G92. G54 thru G59 are what I call fixture offsets, like if you have 3 or four vises on the table and want to jump around for different jobs. When the control sees a M30 at the end of the program it rewinds the program and resets all the default settings. Most of the time this resets the fixture offset to G54. So what I do is put the fixture offset (G54-G59) at the top of every tool path. Then if I want to do a restart at a certain tool in the middle of the program I know the proper fixture offset is being used.

i have to agree with you G92 is bad news because it resets the machine position and 90% of the time a program reset and rewind will not reset it. I always use G10 to set my work offsets

[jorgehrr]

Thank you all for taking some of your time and share your knowledge.
I really appreciated it.

I'm getting there... If it wasn't for the operator that push the "clear" key and wipe out all my offsets.

Is going to be fun setting all the stuff back. I guess is a good learning curve.

Thanks again

Jorge