I tried cutting a circle design today with the center at 0,0 in v carve.
The cnc was also zero at center on the material.
It was drawn in Autocad 2000 with a center at 0,0 then brought into v carve.
My cnc is a Techo Isle, it started cutting the cirlce half of the width of material off.
What am I missing? I usally use the bottom left corner as my start and this was the first time I tried to use center.
Thanks for any help. Glenn

Glenn,
Check this .

I had the same problem with my Techno. I posted the problem on the CNCZone Techno section along with the code and someone posted some modified code that worked. As near as I can figure, I modified the Techno post processor to eliminate the M6 command and mistakenly grabbed some extra. I recalled my archived, unmodified PP and very carefully removed only the M6 and have not had another problem.

If you have modified you PP then you might look there. It seemed to only affect circles and ovals.

Keep us posted if you find another reason.

Joe

Thanks a bunch! Ill try that tonight and let you know.

Thanks, That fixed the problem. Removed the M6 command at all tool changes in the post and it started in the correct location.

Glad I could help. The M6 command is used with an ATC, which I don't have. Most of the time it wouldn't give me any trouble except when I would try to use a 1/32" bit in which case it would error out and shut down the interface. Since mine is an old machine my proximity switches don't work so I would lose my x,y zero and my work would be ruined. The PP I use is the ATC arc (inch) because (I believe) it is the only option with "arc".

Anyhow...glad it worked for you.

Joe

Oh man, it didnt work with a tool change !!

It worked with one tool. I then ran a program with two tools, it stopped for the tool change for a few seconds, then the spindle turned back on and it started to go to rout the rest of the program.

I went back to the original pp with the M6 and it starts the circle design half off again.

Im back to using the bottom right corner for now, but would like to get it working on the center 0,0 in a circle. I have some designs i want to rout the hanger in the back and cut the circle, then flip in a jig to do the v carving.

I do some searching again !!

Thanks, Glenn

Cant sleep now, running G code in my head!

I compared your modified and orginal codes from the cnczone and found the difference is in the header.

Our Techno PP looks like this with a G90 and G92 code.
"%"
"o0000"
"G90"
"G92X0Y0"
"T[T]M6"
""
"M3 [S]"
"G0[ZH]"
+"G0[XH][YH]"

The modified code has no G92
%
o0000
G90G0X0Y0
T5M6

I ran a circle with a tool change with only the G90 and it goes to X-Y zero then to the correct start point and cuts fine, got to the tool change and worked fine also.

I remember that the G90 and 92 were absolute and incremental codes I think. Not sure how it works, but it seems to fix the issue.

Im going to copy my PP and and change the header and save it as a new one for center zero pt.

I have not tried it with center to a square yet to see if that will change.

Both files looked good on the vectric preview and the Techno preview, but cut wrong with the G92 in the header.

Thanks again for your help and links. I will post pics when ever I get around to cutting the stuff !!

Glenn

If I remember correctly, a G92 is used to reset the x y coordinates in the code. I have used it in the past to move to a new location and reset the x0y0 then rewind and run a new part. It saves having to manually do the 0,0 reset in Mach3.

Russ

I tried cutting to the left side of an open line today and it did the same thing. Starts in the wrong location.

Revised the header to remove the G92 and x,y 0 and it ran the open vectors fine.

%
o0000
G90
T5M6

Sent an email to Techno today. Let you know what I find out.
Thanks, Glenn