Setting Z axis with G92 work shift

[venomgrrrl]

Have my X, Y's s set...and all my tools measured...can anyone tell me how to set my Z axis (do i have to do so with every tool?)

I noticed in the programs in my m/c from previous owner all state a Z0.0 in there G92 line!

Im new to this old skool style of programming..any advice is welcome advice
Thanx

[HuFlungDung]

I sent you this as a PM, but I thought I might post it here, in case other users might have some additional insight

Obviously, this G92 system makes it awkward to reuse a set of tools on a new job where the top of the job zero is different. But its not impossible. All you need is to implement a system: beginning with the spindle up at home, set the tools to the top of a reasonably high guage, like a 6" or 8" gauge block sitting on the table. Pick a guage height that is typically higher than any part you are likely to fixture.

This will give you a set of raw length figures to put in your tool length offset table. This has nothing to do with workshift, BTW.

Now, to set the G92Z, you take any tool, touch it to the top of the part. Zero your operator axis display (if you can, this makes it easier to measure), and jog up to the top of the guage block. This should give you a positive Z value, which becomes your Z G92, so write it down.

Now, return the machine to home (spindle up) and modify the G92 Z that you will use in your program to the same value as you just measured.

In operation, with slow rapids first!! when you execute a tool length offset, you should see the toolpoint come down to the height of the guage block. The absolute display will not show any change, it will still be holding the G92 Z value, which if correctly measured and entered, will be the exact distance from the top of the job.

Your next programmed move can be your typical G00 Z1.0 which will bring the tool down to the rapid plane and you can then execute the program normally. Program with the top of the part as being Z0.

Let me know what you see in real life when you try this out. My experience was not with an old Fanuc, but with an old Bandit, but I'm reasonably sure that this phase of operation will be similar. It is possible, of course, that FANUC might invert a direction sign for offsets or something.

[Ozemale6t9]

The way I would do it, is set a tool to be used as a datum tool for every job (eg. tool 1). Set the tool offset for that tool to 0 (eg. offset 1), MDI G43 H1 (or whatever offset you chose) and then set the Z value of your work offset (eg. G54), using that datum tool, the same as for setting X&Y. I usually set the top of the job as Z zero. Also zero the Z value of your relative position display at this time. After this, you simply bring each of the other tools down to touch your Z datum position, read off the Z relative position, and enter that into the offset for that tool.

Then in your program, after you have done the tool change, you put a line such as:

G0 G43 Z100.0 H2 (calls offset #2 and rapids to 100mm above the job)

and the rest of your Z positions are simply negative values from the top of the job.

[venomgrrrl]

This would be typiucally what i would usally do BUT my m/c is not reading any G54's ect...I am currently trying Huflungs idea and cant wait to post what happens

[venomgrrrl]

Ok ... Using the "gauge block set-up" here is what I did:
I chose a Gauge that was 13" as the top of my piece is 8"
I home all axis
Touch top of my piece w T1, Zero on "relitave" screen
Jog to top of 13" gauge...readout is +5.794
I imput this into my G92 Z line (wich read out as 0)
When i ran it made no attemt to stop @ 1.5" abouve (wich is where it is prgmd to stop)
sO it prob would have tried to rapid thru piece LOL...it didnt though (quick like rabbit..I AM)
I tried using the Negitive version of this number, +Z O.T.

What i am to understand is that G92 is reading all co-ords from home post. So i am going to try (again) to get a readout from home and put this into program...pain in ass cuz if it works i will need to do for every tool...every time >.<

ps I freakin love this place!

[venomgrrrl]

OKiee- now what ive tried:

In Offsets pg there is a "00" this is my workshift offset (01=G54 02=G55ect)

I home my axis Z0, in relitive pg. I set Zero, jogged dwn to piece, got a readout of 11.394. I imput this into my 00 z (Z=11.394) My G92 line was still reading a Z0.

It stopped tool 6" above piece, rpd dwn 1.5" to end up at 4" above work (1.5" is my ref above piece.

I ran these steps again with a -11.394 and came up w exactly same results therefore the 00 workshift page does not register or i am not putting in right #

I tried imputing this value directly into the G92 line...as a positive value it would have rapid into piece, as a negitive it O.T. the Z+

So i am going to try now to deduct 6" of of my (Z home to piece value), imout into "00" shift pg. and see if that does not work. If this is the case i would have to deduct a variable # from every Z value.. should be interesting

[venomgrrrl]

And so on....
I have deducted the 6" from my Z value (in pure desperation...ill try anything)
In the workshift pg (00) i still end up 6" above piece, so this pg is usless,
Tried directly in prgm. as a positive value it would go thru piece, as negitive it O.T +Z.
*whew* this is getting trying

[venomgrrrl]

Problem resolved...
Huflundung is a genius...was exactly right in operation instructions, i just executed it poorly.
All my H (tooling) Had been put in program in accordance to block#'s ex N1=H1 even if it was tool 16 (N5 T18 would read H5) thus pulling offsets from wrong tools.
And so 1 more bug squashed...lol

Thanx for all the help everbody

[HuFlungDung]

Glad to hear you got it.

Now be really careful (ie., paranoid) about returning the axis to home before the machine re-reads a programmed G92, and you will steer clear of most all of the bad luck associated with the dread G92. Did I say this before? It bears repeating

[Geof]

I have followed this thread because G92 totally confuses me and I wanted to get hints. When I moved to CNC the way things worked out I started using Haas. And I am soooo glad....setting tool offsets means bringing the tool down to then part and pushing TOOL OFSET MESUR. That is within my limited capability.

[HuFlungDung]

Geof,
As I became familiar with the use of G92 on old cnc's through trial and error, I think I came to better understand why G92 behaves as it does only after using a modern cnc.

I believe it is a matter of how many 'levels' of axis position registers the cnc can maintain. The old slow cnc's only had perhaps two such levels, the machine coordinate system and the tool length offset register for the Z axis, and the radius offsets for X and Y. The old Bandits did not even have a name for the machine coordinate system (G53) but it was still there

When the cnc was powered up, it knew nothing except to assume that all axis positions were all zero. In the most simplistic cnc, you could power up, jog around to find a part datum, then power down and reboot just to get the axis registers to show all zeroes again.

So the power of the G92 command was to eliminate the necessity to power off the cnc to reset the axis registers. However, its effects worked directly on the machine coordinate system registers, ie., you were altering the very lowest level of positional status that the computer had. This is why the G92 was clumsy and dangerous, because there was no way to call up an even lower level of position registers.....nothing 'keeping track' of where the coordinate system was shifting. Multiple G92 calls are like incremental positioning of the machine coordinate system!

So return to home commands were devised to serve as a sort of last resort to get the machine to run back to some physical switches, with known position assumed to be machine zero. At least with the return to home switch, the G92's would only have one such incremental effect of repositioning of the coordinate system, after which it would be checked by return to home where it was ready to reassign a new G92 for a move to a new datum.

So because the G92 fiddles with the machine coordinate system, this is why G92 affects all the work offsets by the same amount, at least this is how I interpret the info on operation of a couple of modern cnc's that I have run. I believe that the modern cnc maintains its G53 coordinate system unchanged at the lowest level, even if a G92 is called, because it is possible to recover position at any time with a G53 command. However, the legacy effects of G92 coordinate system shift are still with us, that danger is that the G92 command has such an immediate effect such that "right here right now, this is new absolute position of the machine" regardless of where it is and this poses the same danger as a loose cannon on deck

[Geof]

Hu; Why did you not put this explanation up a couple of years ago? I had already worked out much of what you write but you filled in some holes. It is a legacy thing really and is redundant in a machine that can have a couple of hundred work zeroes and a similar number of tool offsets. Not to mention G52 which is I think safer to use than G92.