G54 command

[bfedger]

Can somebody enlighten me as to how the "G54" command will work when a "P" word with an"X" and "Y" coordinate are included in the same line. This programming is on a mori machinig center.
Thanks
bfedger

[beege]

What control is this?

G54.1 uses a "P" word to indicate which of 48 extra work offsets, similar to G54 thru G59. As far as I know, G54 by itself doesn't usually take a P. Of course it depends which control you are using.

[bfedger]

Thanks Beege,
I dont know what control series it is. To add more confusion ,I looked in the "offset",then "work" section of the work coordinates page. There I found 1 G54 work coordinate option and the G54.1 with extra settings up to 48. The confusion arises because in the program the comands a call out of"G54 P---".
not "G54.1 P-----".
Am I missing something?
The actual command looks like this: G54 L20 P----- .( Still not sure what "L" does in this format)


Thanks for your help
bfedger

[HuFlungDung]

This probably has something to do with G10, which is for programmed setting of offsets.

G10 L2 P1 X Z might be a sample command format.

What this does is takes those X and Z values and installs them into the G54 work offset table in your control, overwriting whatever was previously in there.

So instead of finding your G54 datum with an edgefinder or probe, you simply use G10 and some meaningful value to load the work offset. This typically has application where everything is known about the work fixture setup, for example, changing pallets on a large machine, but each pallet contains a different set of fixtures. It would be impractical to have a man standing around and rekeying in the work offsets all the time, so you write the changes into the program.

The variable L has certain definitions depending on which number follows it. For example, on my Mits control L2 is work offset register, L10 is tool offset register, and L11 is tool nose wear offset register. I've no idea whether this is standard across all cncs but once you understand what you're looking at, it's easier to find it in the book

The value written with "P" is an alias for a particular work offset or a tool number. Again, the manual may have a chart showing what the correspondence is.

[beege]

Let's see a whole section of code here. Maybe there's an extra hint hidden within.

[bfedger]

Hi Beege,
I'll see if I can get a hardcopy of the program
Thanks again
bfedger

[bfedger]

Thanks Hiflung
I'm in a situation where nobody in plant wants us to know too much (or so it seems)

[Doug_M]

I have been running a Mori machining center for the last 14 years . I do NOT claim to know it all but I have only seen 2 times that a P was used . The first is what HiFlung was describing . At the start of all my programs I have a G10 L2 P1 X? Y? Z ? This is just what HiFlung says . It automatically sets my work coordinates in the Work offset when it is read in the program . L2 P1 is G54, L2 P2 would be G55 and so on .If I use more than 1 offset . The only other instance I have of a P command is not used with an L and that is if I run a program that does multiple parts I will use a subprogram for each part and the command to calll that would be P122 or whatever the program is . At the end of the sub would be a M99 which sends it back to the main program where the offsets for the next piece would be read and then back to the subprogram to machine the next piece. I am not familiar with the L 20 command but like I said I definitely don't know it all . I have a Fanuc 6MB controller and I do have the book for it at work . I'll look in it and see if I can find anything more about this .

[CNCenforced]

Letter "L" also means the number of repetitions of your subprogram if your machine is using one.

[bfedger]

Thanks Doug M
That would be great if you could find the manuals. I'm not sure of the control series because the supervisor has them locked in his desk.
I dont know everything about cnc programming, but I can program as I have done some machining center programming and have more experience on lathes with FANUC controls. I can utilize work shifts and sub programming.
This "button pusher" attitude at work drives me crazy.
Thanks again
bfedger

[stevo1]

I think that pretty much every use of a P() used on a Fanuc control has been covered by everyone so far. For us to really know what it is used for we need to see the code. Can you post the program or the line of code?

I don’t even want to know why the supervisor has the manuals locked in his desk. These should be used by the programmers and maintenance crew. You should not need them to find out what model Fanuc it is. It should say it right on the front of the control. If you find out what model it is PM your email and I will get the manuals to you. If it is not on the front of the control I have a document attached that specifies the common areas to locate the model inside the cabinet.

One other thing missed on the P() value. This can also pertain to the dwell in a canned cycle. So you could have something like
G54G82X()Y()Z()R()P()

It is really tuff to speculate what the P is for because you have a weird combination in that line of code that doesn’t make much sense. If it were using the G10L()P()X()Y() then you would not need the G54 in that line. If it were using G54M98P()L() then there would be no reason to have a X() and Y() in that line.

Stevo


Moderator….HU. I could not attach the PDF for locating the model. I have been having problems doing this lately. The file is only 171k and the PDF is 500k max. It tries to upload the file and after about 1min it bombs out and gives the standard “internet explorer cannot display the webpage”. I have tired changing file names, zipping the file, copy/paste to word.doc ect. Nothing seems to work. Any idea's?

[psychomill]

OK..... back up the truck....

Are you confusing the programs with different Mori machines? Mori also uses another control besides FANUC.... and that's YASNAC.

Therefore, "G54P" would make sense. Since YASNAC doesn't use G54.1... It uses a P address for extended work offsets (P1 up to P27) for each "common". So you could be using offsets like G54P3... G56P16.... G58P2, etc, etc. The only weird deal would be the "L" in it and the fact you have G54.1 page (unless you're looking at different machines). However, to G10 on a YASNAC, you would then use both L and P much the same as a FANUC... except it's only "L2" (or Q2).... unless YASNAC has G54.1 now also??? very strange....