[GITRDUN]

My VF-1 only has a few offsets still not used. We run the same part programs over and over without having to change out vise jaws etc. etc. The operator only needs to know how to change the part program to run any of our parts. This makes it much easier to train new employee and reduces crashes and set up errors due to operator error. The only problem is if we add a few more programs we are going to be out of tool offsets and work coordinate offsets in the machine. I think you can load offsets with a program but ive never used this feature and have no idea how to do it or what problems it might cause. Im just wanting to know how everyone else is solving this dilema. This is an age old problem but ive never actually ran out of offsets on a machine before.
Also we use the same tools on numerous different parts which creates a problem when its time to offset the tool length, one tool might have 8 different offsets asigned to it throughout all the programs.

[WITOMCIO]

In my HAAS i just turn parameter 156 on.
Use it all the time with no problems

[a1cadcam]

use a tool preset block and set each wcs XYZ in each program with a G10...
tool lengths and fixture offsets can be set and changed using G10 in the program.

[Geof]

I suggest you read the Manual about G52.

G52 allows you to define a second work zero within an existing work zero.

For instance you can use G54 to locate the corner of the fixed vise jaw then within the programs that use that vise you use G52 to locate the work zero for the part. You might have a 4" square block centered in a jaw 6" wide and want to put the work zero at the center of the block. From the corner of the jaw you want to move X-3.0 and Y-2.0 so at the top of your program you have the command:

G54 (Not really needed because it is the default but you could use any Gnn)
G52 X-3.0 Y-2.0

Now the program uses that point as the work zero.

At the end just before the M30 you put:

G52 X0.0 Y0.0
M30

You can do the same thing for the Tool Length Offsets. Take all you tool offsets using a gauge block on the vise; I say do this so they will be above the highest part that is machined. This sets them all at a known position.

Now you can include a Z coordinate in the G52; this is the distance from the top of the gauge block to the place you want to have as Z zero on the part; for instance if this is 2.5" then the command is:

G52 Z-2.5

The reason I say put the gauge block to have the offsets above the part is for safety. If the G52 command needs a negative and you accidently use a positive number everything is fine because your tool just goes way too high. If you position things so the Z has to be positive and you by mistake put in a negative everything goes way too low and your bury a tool into the part or vise.

Again at the program end you command G52 Z0.0

You can zero or change the G52 anywhere in the program.

Incidentally also check whether you are running Haas Mode or Fanuc mode; they differ in the way they cancel G52 with M30 or RESET.

There are others ways to get more work offsets by using the G10 command to enter new values for G54, 55 etc but I think G52 is more versatile and also means you can leave the others alone so you know where you are. Especially if you stop a program part way through you might not know what is in G54, 55 etc.

[R1_pilot]

Just put this at the top of your programs:

G10 G90 L2 P1 X#.### Y#.### Z#.###

where # are the actual offset numbers. And P1 = G54, P2 = G55, P3 = G56 and so on.

Just make sure your P and your Gs match.

If you have extended work offsets, you can also use L20 but I am sure you do not.

When I program they usually are big negative numbers, ie:

G10 G90 L2 P1 X-12.2122 Y-5.1242 Z-15.2456

Hope this helps.

[GITRDUN]

I knew G52 was a sort of universal coordinate but wasnt aware of how to use it correctly. I think ill play with that one as soon as i have a day or two to reprogram everything.
What happens if you start in mid program or something? Is it still going to pick up the coordinates correctly using the G52?

[GAS]

Because your fixture never moves all you would have to do is use a tool presetter and record the length of the tools in the holders for every job and add that to your set-up sheet. Then you can turn on setting #156 (SAVE OFFSETS WITH PROGRAM) then when you save a program to a floppy or a USB disk all of the machine offsets will be saved with the program. Now when that job comes back around all you have to do is reload the saved program and the control will ask you if you want to load the offsets with the program. It is that simple, now have the tool crib preset the tools on a cart with the set-up sheet and the program. All your operator has to do is to put the tools in the machine in the order in your program, load the program, put the material in the vise and push cycle start.
We have set-up many machining centers exactly the same way. We pinned the Vise to the table so if it was removed it could be placed back exactly where it was possitioned last. This way all of our saved programs would not have to be changed in case the vise was moved. Then we preset all of our tools just incase one of them broke we could replace it with out having to guess at the length. If you record all of the information about the set-up then you can cut your set-up times to practly nothing.

Regards GAS

[Geof]

I knew G52 was a sort of universal coordinate but wasnt aware of how to use it correctly. I think ill play with that one as soon as i have a day or two to reprogram everything.
What happens if you start in mid program or something? Is it still going to pick up the coordinates correctly using the G52?

Yes provided you have RESTART turned on in the Settings. The Haas Restart scans the program ti get all the offsets correctly applied.

Also if you choose your restart point correctly you can make sure it is just ahead of the G52 command.

[GAS]

What does Program Restart have to do with saving tool offsets with programs? Or reloading them back in the control with the saved program. Please explaine.

The offsets are loaded indapendantly of the program. Program Restart has no effect on tool offsets. Now if you want to start in the middle of a tool path Program Restart could be bennafical.

GAS

[GITRDUN]

I understand the loading offsets with the program. (knew it could be done just didnt know how, thanks for shedding light on that for me)
While im on the subject does anyone know of a way to simplify my problem of numerous tool offsets for the same tool? We use tool 4 in almost every program but have to give it a different length offset for each part program. This is a mess when you replace a broken or dull tool and have to offset all of them that relate to that tool. This is also the reason that all tool offsets are almost used up.
I apreciate everyone taking the time to share what im sure is mostly common knowledge. Ive been programming for 12 years in a job shop. So there was never a need to store anything other your program for future reference. Most jobs were bid on and ran maybe once or twice.

[GAS]

Here is one solution to that problem. Set all of the tools to the top of the table. Now measure the distance from the top of the table to the top of your part "Z zero" and enter that value in the G54 work offset in the Z colume. Now tool 4 can use offset 4.

Regards GAS

[Geof]

.... While im on the subject does anyone know of a way to simplify my problem of numerous tool offsets for the same tool? We use tool 4 in almost every program but have to give it a different length offset for each part program.....

Yes, I told you, it can be done using G52.

You set all the tools to a raised reference point then for each program and part you put the Z difference between the reference point and the part Z zero location in as the G52 Z coordinate.

You keep to the same reference point all the time and the Z coordinate in the G52 never changes.

When you replace a tool it is set to the reference point just the same as the previous tool.

Read my other post through again particularly the bit about setting tool offsets to a gauge block higher than any part. Never set tool offsets to the table because then your Z shift is positive and as I point out you are setting yourself up for a crash if you put in a negative value by mistake.

[Geof]

What does Program Restart have to do with saving tool offsets with programs? Or reloading them back in the control with the saved program. Please explaine.....
GAS

The Restart question was with regards to G52 and had nothing to do with saving or reloading offsets.

[big_mak]

To solve the tool offset issue, it would be easiest to use a common point, like the table. If you have a presetter, you would use the tool gage length as your offset. Thus your tool length would be a positive number. This is a convention used when you have tool measuring probes, or offline presetters and such, and is a reliable means of checking your lengths, as the tool comes into the spindle, before it runs down to the part, you can use a tape measure, or Rule to double check the offset.

If you did this, you could make a dummy tool, as a quazi part probe, and use this to figure out your Z offsets for each work offsets. Take the work offset you measured, and subtract the offset length of your dummy tool!!!!

In some Yasnac Controls this is built in, how you handle your part and tool setup!!!!

[Geof]

To solve the tool offset issue, it would be easiest to use a common point, like the table......

Ignore all these people who tell you to use the table . Do it my way it is safer.

[big_mak]

Safest way geof, is to use a renishaw tool setter!!!!! then with the work probe, you are laughing!!!!!!!

[Geof]

Safest way geof, is to use a renishaw tool setter!!!!! then with the work probe, you are laughing!!!!!!!

Wait until you have employees who try to bore a hole in the table using the probe . Then you might rethink the ratio between time and money saved and money spent on new probes.

[big_mak]

I don't usually have this problem as I am THE man! Doing it all. and the probe is always the same tool, so as last night, I have yet to call it up to cut metal.

I've used it in process to measure bores and update D-Comp with great sucess!

[chuy]

I agree with R-1 pilot since your running a haas...It will read either fanuc or a yasnac program...nice feature with the Haas....I've seen the use of the g52 as well...but with the g52 I've seen alot more crashes by inexperienced operators...G10 is the the safer option well it's pretty brain dead...and that's
I believe what your looking for..,but either will work just depends on the operator... and your preference.

[GITRDUN]

Yes, I told you, it can be done using G52.

Sorry, im a little slow to comprehend sometimes. I just didnt quite catch everything you were trying to explain at first. That will certainly solve all my problems, thanks for the detailed explanations.
I think i will try the G52 instead of the G10. It sounds pretty straight forward and shouldnt take much time to change all the programs. Im not quite seeing the differences between the G52 and G10. The Haas manual is not to detailed in this area as far as i can tell. However they are much better than many of our old Japanese machine manuals i must say. They lose half the meaning in translation.