Repeat g-code with y offset

[cncwhiz]

E-Stop,
The line that should be before the "G10's" should contain the "G90" as well as all the other g codes to cancel drilling, cut comp etc. I also like to use a "G49" to make sure that the "G10's" don't double load the work offsets. The "G49" is a pretty important command in this line, however there can be times in setup that if it is read after a tool offset it can result in the tool moving to the "0" offset position. I personally do not put the "G90" in my "G10" line and have my posts built to not output it. I do make sure that it gets called before and after the "G10" lines. I have places in my programs where I use "G91" but I always make sure that the next line has "G90" even if it is a forth axis index move. I agree with the statement about the operators I have built macro's and all kinds of insurance into my programs too keep operators from having problems, but they still from time to time find a way to get in trouble.

[rob2424]

is the G10 supported in cnc zeus?

[tpaulson]

Originally Posted by rob2424 is the G10 supported in cnc zeus?

That appears to be the problem. According to CNCZeus support, currently G10 is Not supported.

I guess I will just have to generate the code for each box instead of doing a subprogram. Not a big deal, I just figured there was any easy way to repeat the code with offsets. Which there is, but CNCZeus doesn't support it. I will probably look at using Mach2 sometime in the future, but CNCZeus works well for now.

Thanks again
Tim

[Swami]

You can still subroutine. Just write the subroutine with all G91 codes. When the subroutine is over, move to a new absolute location (G90) and fire the subroutine again, as often as needed. Does that make sense? You just keep using G90s to get the cutter in your "start" position.

Swami

[tpaulson]

Swami
I am very new to G code, but I think I understand. The problem is that the software I usually use to create the g-code from dxf doesn't appear to have the ability to generate incremental programming. DeskCNC is the only software I currently have access to that can create pockets.
Is there other software available inexpensive or free that will generate relative g-code for pockets?

Thanks
Tim

[cncwhiz]

If this is an older fanuc controller 11 or 15, I can give you the option code to turn on the option. think that it is 9102 bit O.

[Swami]

Oh! No incremental...I understand why you needed to do it with G10 then now....

I dont know of a program that will generate the pocket using G91, but you could manually edit the code most likey.

Assume your machine is at 0,0 (or something else convenient). Program your first pocket You should be able to take that code and just append G91 (or remove G90) codes from what was produced. When you could make that modified code into a subroutine (by putting O1000 to start the block and M99 to end it) Now you should have a block of code that will work from whatever startingpoint you are at prior to calling it.

Example:
G0 G90 X0 Y0
M98P1000

G0 G90 X7 Y0
M981000

Hopefully that can help you out.

I was wondering, if you have a DXF to code generator, why not DXF all the pockets you want to make and let the program write the whole thing? Sheetcam would be very good for that. www.sheetcam.com

Good Luck,
Swami

[tpaulson]

Swami
Thanks for your help.

Originally Posted by Swami I was wondering, if you have a DXF to code generator, why not DXF all the pockets you want to make and let the program write the whole thing? Sheetcam would be very good for that. www.sheetcam.com

I ended up letting the software generate all of the pockets like you mentioned.

The main reasons why I was trying subroutines was:
1. To allow for quick changes of pocket size. Just make the change on one pocket location in the DXF instead of 5.
2. The subroutine method would also complete an entire box before moving to the next box. Having the g-code generater create all pockets, creates code to make the first pocket on all 5 boxes before creating the second pocket on the first box. This is a waste of time if I only need to make one box instead of all 5.
3. Easily change the number of boxes to be machined in a run

Tim