Using G10 to set work offsets and Z offsets

I need some help with using the G10. I would like to use this code to set all of my Z- offsets on my production jobs. we have a toolsetting machine that we set our tools to, and we now write the offsets down on a set-up sheet so that the operator just has to type them in. we have experienced some problems with bad numbers being put in the control and the machine crashing with proven numbers. because the number was typed in wrong.So how do I use this code to set these numbers automaticly with a program? I would like to also use to set my work cord's also.
Dan

wrong idea.
although you can use G10 for this it makes little sense.
instead, type up all of your offsets and dump them into the offset page the same way you transfer programs.
using g10 in the program is meant for coordinates (like fixture offsets) that will always be the same (or close) every time you run the job.
the idea is to keep operators out of the program.

Is your toolsetter able to print or copy to a floppy, or maybe save the data to a file and dump into the machine?

pi,
why does it make little sence. we want to try to eliminate the operator's loading offset's except through a DNC along with the program.
the tool setter is a manual one that has a comparator screen. we proved that we can set tools to .0005 in length.we want the operator's to load the offset's in just like they would a program. the only time they would need to set offset's by hand is when it is a new job. what I need to know is how to write this in a program to setZ- offsets and tool radius offsets along with G54-58 work cord's. ?

[ QUOtype up all of your offsets and dump them into the offset page the same way you transfer programs.

When reading your reply again how do we dump offsets in the offset page. is there a different code other than G10 to do this?

It depends on your control somewhat. You can create a G10 program to load all of this in your control, including offsets, comps, tool data etc.

For Fanuc, mazak and related it goes something like this:

G10L2P(?)XYZB = L2 is for offsets. "P" controls the work number (P1=G54, P2=G55, P3=G56 etc.)
G10L20P(?)XYZB = L20 is for extended offsets. "P" controls P1, P2, P3, P4, etc.
G10L10P(?)R(?) = L10 is tool length. "P" is tool number, "R" is the value.
G10L11P(?)R(?) = L11 is length 'wear' if you have it the option. "P" is tool number, "R" is the value.
G10L12P(?)R(?) = L12 is geometry (tool radius or cutter comp if you use it here), "P" is comp number, "R" is the value.
G10L13P(?)R(?) = L13 is geometry 'wear' (cutter comp), "P" is the comp number, "R" is the value.

If you have a Yasnac, your workoffsets might be like: G10L2P1J(?)

On many controls you can load the tool info, data, workoffsets, parameters, whatever seperately and directly to the related pages without the operator having to cycle it.

HTH....

Depending on the control, there are different ways to do it. Loading them via the G10 route is probably the easiest but DON'T MAKE IT PART OF THE PROGRAM.

Putting the fixture offsets in the program is fine because they should be the same ( or very close ) each time the job is set up. The tool offsets will be different everytime the job is set-up. Therefore you have to edit the program everytime. Or worse yet, the operator will be editing. Even when a tool breaks or is changed out for any reason, the program will need edited.

So create another program that contains nothing but the tool data. Load it in and delete it from the control. If just one tool is replaced, that data will have to be entered manually. The goal is to only have one person (the programmer) responsible for the contents of the program.

That said, there are a couple of top notch operators in most shops that can be trusted to make edits, but not the McOperators. Even the trusted ones, I don't allow them to upload a program back to the main system. Anything saved from the shop floor goes into a "TEMP" folder. Then I do a comparison between the original and the modified files and make the final decision.

+1 E-stop...

Do the same thing here. Should've clarified that a little. We use memory sticks (where available) for the tools. Programs go through the normal channels. Work offsets are in the program since all of our setups are on a grid or repeatable fixtures. For the older machines, the tool data is seperate (has its own program to load offsets then deleted). Some of our machines are also networked to the presetters and the data can be uploaded to the control directly from the setter.

try this:
punch all offsets to the pc. look at the code.
that is what they need to look like to reload them.

Hey PSYCOMILL, E-STOP,
Thanks for the info on the G10. Now how would you write the program from the start using: TOOL1 H1 Z-10.5" offset D101 .500"r. for comp. this for setting a 1.0" e-mill on top of a fixture the difference between the fixture and the part in Z will be put in the G54 Z setting on the work cord. page. all of our tooling fixtures, vices, ect. are mounted to the table with tapered locking pins (not sure of correct name)that have a male on the table and a female mounted to the fixture this system always repete's to within tenths if every thing is kept clean. the only variable in Z hight is the part itself. this is why we are trying to get this G10 thing working.

Once again I'll say thats its not a good idea to have the tool offset info part of the running program. That said, heres how you write the code for the tool as you described.

You haven't mentioned the control or machine you have, but I'll assume Fanuc (and related) here.

TOOL1 H1 Z-10.5" offset D101 .500"r. for comp.

Click to expand...

G90G10L10P1R-10.5 (L10 for length, P is the tool number, R is the value)

G90G10L11P101R.5 (L11 for comp, P is the comp number, R is the value)

This is for standard boards. Some boards are slightly different. Geometry for comp might be L12 or even L13. Try the codes in MDI to see where it puts it or output the tool offsets in you control to see the 'L' numbers. Tool comp has three levels, comp A, comp B, and comp C.

Pysycomill,
Thanks that helps clear this up. I will make the G10 program seperate from the main program for peace of mind. what's one more keystroke on the DNC! sure beats setting them for the second time by hand