Missing H and G54....G59 offsets

[jorgehrr]

I need help.

How can I find the program zero to be able to run my programs if I do not have my G54....G59 offsets anymore (got deleted by accident).

I have the programs, the fixtures but all the offsets are gone.

Any way to calculate those numbers back, fixtures are old and do not have any reference.

It has to be a way...please help me.

Also, is there a parameter number to lock these offsets so they can not be deleted?????

Thank you guys I know I'm going to get answers in here

Jorge

[HuFlungDung]

The work offsets are usually based on some sort of a datum (reference point) on the fixture or the part. I would think it most unusual that you would never have to change these work offsets on a regular basis. You must have some kick ass discipline in your shop

There must be some feature on the part or the fixture that you can reference to. Its difficult to say exactly what you would use, but, say for example, you run an old program and allow the program to run to position the tool beside a known edge or over a hole. Stop the program at that point, zero your operator displays, and using an edge finder, determine the distance that you have to move the machine to get the tool into correct position in X and Y. The values you get on the operator display should be the correct values for the current active work offset (sign of the values may be inverted, but that should be pretty obvious when you rerun the program and the machine goes way way off position).

The "H" offset is your tool length offsets and is not related to the work offsets in X and Y. However, there could be a Z component of the work offset, however, if your habit is to set the tools off the top of the part then the Z value for each work offset would normally be zero.

[cutsall]

I have seen an instance where the part zero remained constant from fixture to fixture but it was a confusing situation to say the least. The fixtures were referenced on the table at a pre-determined position and the program positions were referenced from a point not related to the part i.e. bottom left, top right, centerline datum, or even a postion related to the part geometry. It was almost impossible to look at a part print and a program and correlate the numbers. If you know the location of the fixture on the table and a feature of the part such as a drill hole or part edge you should be able to re-establish g54....g59 offsets by determining the x,y locations from the program. Example if it is X-15.0000" Y-5.0000" to a known location from machine home but the program calls for X-10.0000" Y0.0000" then you may assume that the G offset for that feature is X-5.0000" Y-5.0000". The same may hold true for H offsets in your case if you are using dedicated preset tool lengths. The only way to be sure is to post a copy of your program and its part print on the forum and let us take a look. You may want to add a G10 L2 P1 X.... Y....possibly Z.... to the start of your programs to automatically write your offsets to the control thereby eliminating the problem you currently have. P1=G54 P2=G55 P3=G56 etc. If I have mispoken I am sure Hu-Flung or someone else on the forum will set you and I straight pretty quick. I have been in machine tool thirty years and thought I was pretty savvy but the knowledge base on this forum is awesome. I wish I had the opportunity to work with some of these guys.

[Geof]

Can you get hold of a part that was machined in the fixture? With a part you could dial into some feature; a bore, a corner, a step, anything you could get an X, Y position for in machine coordinates then look at the program to find the program coordinates for this feature and get the work offset from the difference.

[jorgehrr]

Thank you all

Cutsall -I agree 100% with your comment about the people in these forums, GREAT place to learn from the best.

Here is what I did

I set up a job an and I worked with a part that was already machined, using a drill operation I brought the drill right to the hole already done I copy the numbers of machine position subtract or add (I do not remember witch one worked) the first G00 moved in X and Y and use them in my G54...It worked a few adjustments and I was ready to go. Al the others operations where in place after I got my drill in place.

H offsets are positive numbers and set in the bench (not a problem).

It took me all afternoon but I got the job running.

Thank you for your time and input.

Jorge