I need more work offsets! (Fanuc control)

[Bucky Cornstarch]

Hi,

I run 3 double throw vises on my VMCs, with each throw of the vise using a different work offset. So far it has worked beautifully: six work offsets, six vise holdings.

 

I've recently come to the conclusion that if I could add just one single throw vise to each machine to handle some 2nd op work, I could significantly increase my production. I've got room on the tables, and some 4 in Kurts laying around.

 

Problem is, I am out of available work offsets! I'm running Fanuc O-M controllers on each machine, and Mcam V9.x. Am I out of luck here? Am I limited to just the six work offsets? Is there anything I can do with Mastercam to help?Each vise station is running a different operation on a part, or a different part all together, so using subroutines seems to be out.

 

Help, all I need is one more lousy work offset!

 

Thanks,

Jim

[Guest]

No, if you have G54 thru G59 then that's it

 

Can you run two operations on 1 work offset.

 

If you know the distance of the XY zero between 2 parts you could set your geometry at that location and then link the 2 different programs to 1 work shift.

 

Dicey but it'll work

[TC]

I have the Fanuc 18i control and I have 48 more offsets when I use G54.1 P1-48. Don't know about the O-M control, but its worth a shot...

[Tim Simmermon]

I believe our Haas has some extra work offsets in the G100's. I'm not positive, though. Not sure if that is specific to the Haas control or not. Check your manual if you haven't done so already.

[DavidB]

MAin program

G90 G10 L2 P1 X Y Z B Sets the offset.

M198 call program

G90 G10 L2 P1 X Y Z B Sets the offset.

M198 call program

Repeat as many times as you want.

 

This way your unlimited of working offsets.

 

HTH

[heavychevy2155]

can you use g54.1 p## I have used fanuc controls with this setup.

[Bruce Caulley]

Here is the trick.

 

We leave all of our G54-G59 data blank. Each job has a datum programme i.e 5001 is 1st datum point 5002 is second etc etc

 

5001 would just be something like G92 x y z

 

This way we can have as many offsets as we want and if you combine this method with quick change doweled fixturing the next time you run the job all you need to do is empty the programmes in the control, load all the programmes necessary for the new job and away we go. We run all of our programmes as subs so the first sub called in the main programme will be the datum programme. You don't need to run this way of course, you could just use a g92 at the beginning of the programme.

 

HTH

Bruce

[crazy^millman]

Or you can call Fanuc and have them added it cost $500 for our machine about a month ago.

 

HTH

[DC Gorn]

+1 With what DavidB posted. Its so easy and operators pick up on it quick. We use it all the time on mills and laths.

[Guest CNC Apps Guy 1]

+1 more to David. I ALWAYS put G10 fixture offsets in my programs. The offsets are always getting written and overwritten.

 

So your line (At the head of your program) looks like this;

( G54)

G90 G10 L2 P1 X00.0000 Y00.0000 Z00.000 B000.000

( G55)

G90 G10 L2 P2 X00.0000 Y00.0000 Z00.000 B000.000

( G56)

G90 G10 L2 P3 X00.0000 Y00.0000 Z00.000 B000.000

( G56)

G90 G10 L2 P4 X00.0000 Y00.0000 Z00.000 B000.000

( G57)

G90 G10 L2 P5 X00.0000 Y00.0000 Z00.000 B000.000

( G58)

G90 G10 L2 P6 X00.0000 Y00.0000 Z00.000 B000.000

( G59)

G90 G10 L2 P7 X00.0000 Y00.0000 Z00.000 B000.000

G11

 

Infinite number of offsets. :-)

[Psychomill]

James....

 

quote:

---

( G54)

G90 G10 L2 P1 X00.0000 Y00.0000 Z00.000 B000.000

( G55)

G90 G10 L2 P2 X00.0000 Y00.0000 Z00.000 B000.000

( G56)

G90 G10 L2 P3 X00.0000 Y00.0000 Z00.000 B000.000

( G56)

G90 G10 L2 P4 X00.0000 Y00.0000 Z00.000 B000.000

( G57)

G90 G10 L2 P5 X00.0000 Y00.0000 Z00.000 B000.000

( G58)

G90 G10 L2 P6 X00.0000 Y00.0000 Z00.000 B000.000

( G59)

G90 G10 L2 P7 X00.0000 Y00.0000 Z00.000 B000.000

G11

 

---

should be:

 

( G54)

G90 G10 L2 P1 X00.0000 Y00.0000 Z00.000 B000.000

( G55)

G90 G10 L2 P2 X00.0000 Y00.0000 Z00.000 B000.000

( G56)

G90 G10 L2 P3 X00.0000 Y00.0000 Z00.000 B000.000

( G57)

G90 G10 L2 P4 X00.0000 Y00.0000 Z00.000 B000.000

( G58)

G90 G10 L2 P5 X00.0000 Y00.0000 Z00.000 B000.000

( G59)

G90 G10 L2 P6 X00.0000 Y00.0000 Z00.000 B000.000

G11

 

 

Must still be early eh?!!

[Guest CNC Apps Guy 1]

Yeah, and I did not get to bed until about 2:00am and got back up @ 5:30am.

 

I'm beginning to wonder if I should go back to work for a company. These long hours are getting harsh and I'm not liking it much.

[Bucky Cornstarch]

Thanks for the responses. Here's where it gets a bit complicated: I've got hundreds of programs already written, which have been manualy edited to combine g54, g55, g56, etc. The process is this: Call the first tool, let's call it a face mill. Use the face mill on all operations (work offsets) that require that tool. Next, call up the next tool, say, a 1/2" roughing EM. Use that tool on all operations that need that tool. Repeat until all tools have done their thing, usually between 12-20 tools per job.

 

What I'm looking to do is a second op type thing on the machine, using a single 4 inch vise that only needs one offset, while still using G54-g59. An example would be a part that has a 1/4" hole drilled in it on the manual mill as a fourth op. Problem is, I already use a 1/4" drill on the CNC, and if I had one more fixture offset, I could do the 4th op on the CNC.

 

Many of you are probably wondering why go to the trouble, why not just do the 4th op manually? Well, I've done some analysis, and there are several parts we make that could be integreted into other jobs, litterally saving us hundreds of machine hours per year. If I have to, I'll bite the bullet and have the extra offsets added by Fanuc (one machine already has them), but I'd like to know if there is another way.

 

BTW, I'd upload a sample program, but I can't seem to access the FTP site. I could email a copy if anybody would like to see an example.

 

Thanks again,

Jim

[Roger Peterson]

Does your controller support G52 work coordinate shift?

 

G90 G54 X0.0 Y0.0 Z0.0

G52 X10.0 Y0.0 Z-2.5

Gcode to run part

G52 X0.0 Y0.0 Z0.0

 

the G52 value would equal the distance from G54 X0 Y0 to the zero point on your second op vise.

 

 

HTH

[Bucky Cornstarch]

That may be the way I end up doing things. I was hoping to keep the machine operator out of my programs, (don't ask) but that may be my only alternative.

 

Thanks,

Jim

[Roger Peterson]

Personally I don't like using G52's, or G10's (the way the other guys mentioned). Not because it doesn't work but it can get a bit hairy on mid-program restarts (found this out the hard way several years ago) with the wrong operator. I love G10's, but I like to define them once at the top of the file.

 

500 bucks for additional offsets isn't much compared to getting a spindle bearing replaced if something really bad happened.

 

Take into consideration the quality of operators you have when you make your decision.

[specv]

Does the control have macros? If it does you could use them to do the same thing. I have written programs for 6 parts using 1 fixture offset, and macros to shift the locations of the other parts.