G92

[jybute]

Can anyone tell me what this is for?

[Geof]

Can anyone tell me what this is for?

Did you read the Haas manual?
" A G92 command effectively shifts all work coordinate systems so that the command position becomes the current position in the active work system."

I think this is correct:
It allows you to create extra work coordinate systems by creating values in a G92 register. These values are then added into all the positioning calculations that the machine does. Imagine that you are using G54 and your G54 coordinates are X-8.0 Y-6.0 and you move the machine to G54 X2.0 Y2.0; this means in the machine coordinate system you are at X-6.0 Y-4.0. Now you do the G92 command G92 X-4.0 Y-4.0; the machine does not move but a value is entered into the G92 register so that when you command the machine to go to G54 X-4.0 Y-4.0 it does not move because you have made your exisiting position this position. And if you now command G54 X2.0 Y2.0 (which is how you got to that position) you will move to a new position.

Are you confused? Do you know where the machine is going to go whenever you now give it a motion command. If your first answer was 'Yes' and your second answer was 'No' I think you are in the same shape as most people trying to sort out G92.

Anything that can be done with G92 can be done in a less confusing manner using G52 and I will be surprised if anyone advises you to try and understand and use G92.

[Ken_Shea]

You can find a ton of stuff on G92 just by doing a Google search.

Here is a link to an excellent explanation and example.

http://www.cncezpro.com/g92m.cfm

[HuFlungDung]

I agree with Geof that no one would recommend using G92 anymore, but who knows, there might be the odd valid use.

I like to keep the explanation as simple as possible: the G53 coordinate system is your machine's 'real coordinate system' that is established after it homes all the axis. When homing is completed, stored parameters set the G53 axis displays to certain values, lets say all zeros for that machine home position.

G92 is like a superficial renaming of the G53 coordinate system, kind of like 'programming the axis displays' to read whatever you want them to read. This is why it affects all the work offsets the same amount.

While it sounds handy, this can lead you to completely loose track of where machine home is, because you cannot cancel a G92 command, you can only issue a new one, and hopefully, if you have successfully returned to an accurate known position, then you can rename it correctly so that the axis displays once again correspond to distances from home in the G53 coordinate system.

That is how it used to be in the old cnc's anyway. The imminent danger was that if the control ever read a G92 command when it was not located at the start position of the program, you can imagine how it would assume the current position was the starting point and start machining whatever happened to be located in that area. Yikes! When using G92 and doing a program restart, you must positively move to the correct start point before that G92 is read, that was the rule.

On a modern machining center, you can likely recover position by homing all the axis again, and finding your way over to the G92 start position after the crash . Not fun, and I suspect that is why work offsets were created, because the machine coordinate system stays intact.

[turmite]

Hu at present I am that odd valid case. While I don't use what most would consider a commercial controller I do have to use G92 on may of my programs.

The thing that bothers me about it is that it is persistant and if you fail to cancel it with a G92.1 you are in deep voodoo!

Mike

[tobyaxis]

Can anyone tell me what this is for?

G92 is still widely used in shops in Large Aerospace Machine Shops in this area. Only reason is that the original programmers years ago programmed that way, and no one has time or they are too lazy to change them.

Also Fight Safety Certified Companies have to document all procedures in machining completely including programs for CNC's. If they reprogram a job or part they have to get that specific program authorized by the auditor along with all the processes after. Sounds stupid I agree, but when you go through the certification process and have a 40 million dollar contract companies tend to play by the rules for Flight Safety Parts.

Personally I have only used G92 once. The reason was that a customer wanted our shop to make his parts using his program and material. The customer was paying a lot so the boss didn't care. On the other hand if we programmed regular jobs with a G92 the boss may have blown his stack because he didn't want the programs written that way. The specific orders from the boss where G54-G59 and all programs where to be written in Absolute with no Sub-Programms. What a pain. The joke going around in that shop was "The next thing he will want us to do is to stop using Canned Cycles".

As long as that function is still available in Machine Tool Controls someone in the machining world will have a specific reason for using it.

[jybute]

Thanks, guys. I guess my real question was, whay woould anyuone want to use it? We use VGibbs, with several different post files, and we lost a pretty pricey part the other night, cause the wrong post was used. I have never had a problem with G92 when 3axis milling, but when rotary milling, or even rotary positioning, the issue has come up. We actually use a post that has in the title, "noG92". The post files are still a bit of a mystery to me also. Ive just learned wich side of the computer to sit on. But Im slowly bringing it together.

Thanks again guys.

[ajl6549]

We actually have a machine, 1978 Mazak V-12 with a 6m Fanuc control and as far as I know G92 is the only coordinate system we can use on it. What we do is determine how far from machine zero is our work zero, i.e. x-20. y-10. z-15 this would be from machine zero to wpc zero. Next, in the prog., the machine is sent home via G91 G28 X0 Y0 Z0. After homing the mach. the G92 line is used like this:

G91 G28 X0 Y0 Z0
G90 G92 X20. Y10. Z15.
T?M6
G90 G0 X0 Y0 (MOVE MACH TO WPC ZERO)
G43 H? Z1. (MOVE MACH TO Z1. USING TOOL LENGHT COMP.)
ETC.
ETC.
M30

Note that the axis is "set" at the distance from the work piece to the current position.

It's quite simple really, although primative!


A.J.L.

[jybute]

Here is an example of the problem.
N22 G0 X-.4 Y0. A228.277
N23 Z1.875
N24 G1 Z1.5425 F18.362
N25 M97 P237
N26 G0 X-.4 A228.277
N27 Z1.6825
N28 G1 Z1.35 F18.362
N29 M97 P237
-N30 G92 A-131.723

note the absolute "A" moves then the G92
After running the code in the m/c the "A" pos. is @20000.00 deg.
So when it starts to cut in the next op, it is in the wrong "A"pos.

[HuFlungDung]

Could it be a simple typo? Using a G91 incremental movement (which would produce an actual rotation, whereas G92 would not) would be reasonably common practice. Depends on the part, I guess, but the same rule would still apply: at some point the rotary must be returned to a known position in G53 (where you can safely branch out to work offsets), and it would be next to impossible except for homing it again.

If an actual program would be more conveniently run with a shift in A, then a new work offset should be called, with the appropriate A amount, all the other XYZ being copied from the original work offset.

[ajl6549]

Here is an example of the problem.
N22 G0 X-.4 Y0. A228.277
N23 Z1.875
N24 G1 Z1.5425 F18.362
N25 M97 P237
N26 G0 X-.4 A228.277
N27 Z1.6825
N28 G1 Z1.35 F18.362
N29 M97 P237
-N30 G92 A-131.723

If the above is read by the control it would have posistioned A axis at 228.277 in absolute, assume. The G92 command would then " set " A axis at -131.723. So in other words instead of being at A228.277 it would now be at A-131.723 but no axis movement would have occured

[jybute]

If the above is read by the control it would have posistioned A axis at 228.277 in absolute, assume. The G92 command would then " set " A axis at -131.723. So in other words instead of being at A228.277 it would now be at A-131.723 but no axis movement would have occured

It actually rotates the"A" in the sub. So when it comes out of the sub, its going to index to the wrong "A".