What's the deal with so many offsets ?

[mannster]

I hate to bug you guys with what is probably a silly question. I have been handcoding and turning parts on a SL-10 and everything has been going fine.
The only offset I ever change is the G54 to set the origin on the face of my part.
Sooo...
What are all the other offsets used for ? I dont know why they are necessary really. The SL-10 boasts over a hundred offsets, and I just don't get why.

(I am specifically referring to the G offsets, G52, G54 etc. etc.)

[HuFlungDung]

I've used up to 8 at a time thus far Very handy if you've got lots of vises on the table of a mill.

But for lathe, I can imagine that some guys might have a series of parts that they run over and over. If the parts have a different chucked length, then they need a different work offset for each program. Some of us might just go in and modify the G54 for each job, but you don't have to. You can set up a "permanent list" of offsets, and dedicate them to particular programs which work at that part length, and if the program calls the corresponding work offset, then you never have to edit the offset table at the machine. It could be more trouble free in well controlled circumstances, than forgetting to recheck the G54 after loading in a new program.

[Geof]

If you are doing bar work where your bar is large enough and your part small enough that you can machine and part off several pieces before advancing the bar the multiple offset are useful. You write the program for one part and make it a subroutine. Set G54 for the first part furthest away from the chuck, go to the subroutine and finish and part this one off, return to the main program and set G55 which is the part length plus parting allowance closer to the chuck and go to the subroutine again and finish and part off the second piece, back to the main program and set G56 which is two part lengths closer to the chuck then back to the subroutine to finish the third part. If there are only three parts now set G54 and go through the bar feed loop. This saves a lot of time particularly on our old HL1 which has an air opening chuck so the spindle has to be stopped for feeding the bar. Even on our SL10s with bar feeders that operate with the spindle running you save many seconds per part.

If my explanation is not clear enough I can attach a program with comments and you can view it on your graphics.

I will admit I don't see the need for a hundred offsets on the lathe and I think that is just an artifact of the Haas software which seems to have the same core code for both lathe and mill. As Hu said multiple offsets on the mill are very useful; I think the largest number we use in a single program is 32.

[miljnor]

I use 2 offsets min on almost every program. g54 is the front side of a 2 sided part and g55 is the back side of a 2 sided part. this keeps you from having to program your second side like it was .0xx shorter becuase you machined off some of the first side. (this is how they were doing it in the first shop I ever worked! what a PITA! )

Some times on realy odd parts you will have to flip the part in the chuck more than once to get the job done.

Your obviously new at this, give it time youll soon be thinking of realy creative ways to use the other offsets. He!! you'll even be outsmarting yourself soon!

[mannster]

Thanks guys !

I get the general idea now. I guess it depends on the type of work you generally have to do.
I understand Geof's concept. I do not trust our parts catcher to work properly so generally I write a program for one part, part it off and then manual adjust the G54 the appropriate negative distance to start the next part.
and yes, I am kinda new to this but I had to get good FAST!!! so I can make the parts we need one way or another.

Now, I am still curious about the G52. I havent had to adjust it, and the manuals dont get into specifics about it. I know it has something to do with the local coordinate system, but why would I ever need to change it ?

Thanks in advance !

[HuFlungDung]

G52 is simply your operator position display, I believe. You can zero an axis at any time (in mdi) and proceed to make a measured relative move or whatever you like. Depending how you perform your tool offset measurements, it can be handy for that.

However, zeroing the operator display does not affect the correctness of the absolute positions called by your program when you go into automatic mode. G90 absolute coordinates reference to the machine home, which is established as the G53 machine coordinate system on startup.

There is one exception, but it hearkens back to the "old way" of doing things. That would be the use of a G50 (on lathes) or G92 (on mills) which superimposes an imaginary coordinate system shift on top of the G53 coordinate system, and affects everything, including the work offsets. Maybe that's more than you wanted to know

[Geof]

It think it would be possible to do the multiple parts per bar advance using G52 rather than the way we do it with G55, 56 etc. To use G52 after the first part you would have the command G52 X0. Z-(part length plus parting allowance) and after this command the machine uses that point, which is itself defined in G54, as the work coordinate system. Then you have to cancel the G52 to go back to G54. I seem to recall I tried this and found that under some conditions such as stopping partway through a program the G52 remained active. This was a while ago when I was teaching myself G code programming and I think now if I had put a line G52 X0. Y0. at the top of the program it would have been okay.

G52 is very useful in the mill when you are doing multiple parts in a fixture because you can have a reference hole to set G54 then all your individual part work coordinates are located using G52 Xn.nnnn Yn.nnnn for the different positions in the fixture.

Comment:
Hu posted while I was typing and I don't think he is quite complete in describing G52; it is a real work coordinate system but it is defined within your active work coordinate system. And I don't think it matters which work coordinate system you are using; for instance the default on a Haas is G54 so if you do not specify anything else that is the system you are working in and your G52 Xn.nnnn Yn.nnnn locates the G52 at the point n.nnnn, n.nnnn in G54. However if you command G55 as a different work coordinate system and do the G52 command the G52 position is in G55.

[Geof]

....manual adjust the G54 the appropriate negative distance to start the next part.....

Do you use a stop in the turret with an automatic bar advance?? If the answer is yes your procedure can have a high risk associated with it. If you bring the stop forward without having changed all your negatives back you may finish up stopping the chuck. Unfortunately I speak from experience; one time my guy missed a G54 at the beginning of the stop/bar advance loop. The result was the stop went in about 1/2 an inch past the jaws on a chuck spinning at 1000 rpm. The bang was quite impressive, it took a few minutes to make up a new stop to replace the one that was sheared off and a day and a half to realign the machine.

[HuFlungDung]

Geof,
You could be right, I've never read anything on the use of the G52 either, so I just assumed

I still don't quite follow the usage of it from your example. Obviously, there must be a datum set for the G52, so how is that done within an existing work offset? Is it like an offset within an offset? Sounds like a good way to get lost

[Geof]

Hu;
I assume you mean the mill example. It is an offset within an offset and the datum for the G52 offset is the coordinate set in the G52 Xn.nnnn Yn.nnnn command. It is a good way to get lost because on Haas machines you have to actively cancel it with the command G52 X0. Y0.

It is a bit foggy in my memory but I seem to recall the first time I played with G52 about four or five years ago I did not clue in to the active cancel; it is not explicitly mentioned in the Haas mill manual in the section "G52 Set Local Coordinate System Haas". The result was every time the program ran the G52 command added onto itself from the previous cycle so I kept getting overtravel alarms.

You run Haas machines? I can dig out the program that uses G52 and send you a copy and you can view it in graphics.

[HuFlungDung]

Thanks Geof,
I did some web searching and found a good example here on how to use the G52:
http://www.mmsonline.com/articles/0100cnc.html

So it is a convenient method of programming a subroutine in absolute coordinates, then calling up the subroutine from various points in the current work coordinate system. I guess I never found it that difficult to program a sub in incremental, but maybe I'll have to "get modern"

[Geof]

That is a very good write up; one to print for my files. The funny thing is though for something as simple as a hole it is a toss up whether I would position myself with coordinates and use incremental or use G54,55,56,57.

I realised we are guilty of hijacking Mannster's thread; Ooops, sorry.