Fanuc 18T Lathes

[jorgehrr]

Hi every body.

Please I need to understand something.

I use G10 with machine centers, great tool... Never seen G10 in a Lathe, can someone please explain what is happening in this block:

G10P0Z0

This block is in the beginning of all programs in this used machine that we have, should I add the same block in new programs???? why????

Thank you in advance

Jorge

[stevo1]

I have never seen that or know of a reason of why you would need to program that at the beginning of the program. It does not even give a location of were to change using the “L” and with the “P” being set to 0 tells me that if it had to do with tool offset it would be tool 0 or if it were coordinates it would be the common coordinate but once again does no good if there is no “L”. I tried programming it in my 15series Fanuc and get a “Format Error”. I don’t know what that would be setting. My first guess would be that you don’t need it but I would check some of the programs maybe the macros to make sure that they were not setting a parameter to do something and wanted to make sure that it was cleared before running the program.

I have seen many weird styles of programming from people before me. A lot of times people don’t know what they need for a safe start at the beginning of a program so they cover all bases. Most of the time I can eliminate about 10 lines of start up and safe code that is not needed, confusing, and cluttered.

Stevo

[jorgehrr]

Thank you for replay,

Yeah...weird, I do not see an "L" an the "P" is set to zero.

I deleted the block of one of the programs and run the machine (dry run) it made the part with not problem.

I'm not sure If I want to stop using it.

Well, thank you again.

Cheers

Jorge

[stevo1]

I got curious and did some research in the books for the 18t. I noticed in the book about the G10 command that it appears that you might not have to have an “L” value. It appears that when using no “L” value and using P0 that it refers to your common offset. This code was probably used for a couple of reasons.

1. It was just a safe start code to make sure that nothing was put into the common coordinate before running the program.

2. Some time when programming or running the part the common was used shifting the work piece. Maybe take a look at some of his programs and see if maybe he was setting the common at some point.

What you could do is put a value in the common Z then MDI G10P0Z0 and see if it changes it to 0. If it does now you know what he was using it for. 10-1 it probably changes to 0. If that’s it and you don’t use the common coordinate then you can get rid of it. Sometimes it’s just years of habit to use certain codes at the beginning of a program.

Stevo

[jorgehrr]

Common offset??????

Please rephrase this. I do not know what a common offset is, I may know it as something else.

When you say add a value in the common "Z" I really do not know what you mean.

Thank you.

Jorge

[stevo1]

My apologize.

Ok your common offset is in the work coordinate page with G54-G59. You have used these before?? Press your “offset/settings” hard key then press the “work” softkey. The screen should look like the PDF I attached to this post. It will look a little different if it is a 18i-t control. You see how it has NO.00, NO.01, NO.02 ect. The NO.00 is your common work offset. This is applied to every move regardless of which work coordinate you use. I typically never use the common. The NO.() is how your G10 works. If you program G10L2P0(P0-P6) the L2 designates your work coordinate page the P0-6 will designate which coordinate to change. If it is P0 it changes the common, if P2 it changes G55ect.

So from here put a value in the common(NO.00) Z. Then MDI G10P0Z0. It should change the common Z to 0. If this is the case then it is as I stated in my previous post that it is not needed unless you are using the common work coordinate.

Hope this clears things up!
Stevo

[jorgehrr]

Great!!!!

That is it, you are right. It changed it back to Z0.

Man...Is good to understand what is going on.

Thank you for your help.

Regards.

Jorge

[stevo1]

No problem, anytime. Glad to help.

Stevo