[thompson_chop]

Just got v11 and trying to do some tests, but having some problems with cutter comp as output by the post processor. I have a Dynapath Delta 10 controller. Following is a simple file straight from the post processor for that controller. Just a square with a circle in the middle.

The program seems to run fine until line 185, which is g41 cutter comp left. This controller excepts G40, 41 and 42. But I get an error with g41 in this program.

I run the same program with the offset to none, g40 and the program ran all the way through.

So I'm not sure if it's looking for something before line 185? I also noticed that the post is adding several g codes to the first line, which my manual says there can only be one g command per line.

Can anyone help with this issue?

%
N5G70G40G17G90G80
N15T1M06
N25S1225M03
N35G00X0.0Y0.0F5.0
N45Z1.969
N55X0.75Y0.0
N65Z0.125
N75G01Z-0.5
N85G03I0.0J0.0
N95G01X0.375Y0.0
N105G03I0.0J0.0
N115G01X0.188Y0.0
N125G03I0.0J0.0
N135G00Z1.969
N145S1225
N155X-2.006Y2.257
N165Z0.125
N175G01Z-0.5
N185G41X1.992Y2.257D1
N195G02X2.242Y2.007I1.992J2.007
N205G01X2.242Y-2.007
N215G02X1.992Y-2.257I1.992J-2.007
N225G01X-2.006Y-2.257
N235G02X-2.256Y-2.007I-2.006J-2.007
N245G01X-2.256Y2.007
N255G02X-2.006Y2.257I-2.006J2.007
N265G40G00Z1.969
N275M30

[tjb1]

N5 is a safe start line, it cancels most and you need a linear move after activating cutter comp before it will take effect so either add another line before the G02 or move the G41 command to a new line before N185 and then change 185 to a G01. Your control should take multiple G codes on a line, most I am familiar with wont take more than one M code.

Try moving G41 to N180 and change G41 on 185 to G01, if that doesnt work you will need to put G41 on N155.

[thompson_chop]

I agree, N5 looks suspect. This was the code generated straight for the post processor. Also noticed on that line there is a g40, no comp and is also modal. According to the manual I have for this controller, it cancels out any proceeding g41 or 42. Does this sound correct?

Just looking for a way to output clean code from Dolphin without modification, or am I asking to much? Will this be a case that I'll have to modify every code that comes out of Dolphin?:devious:

[tjb1]

Yes N5 is a common line, it is used to cancel anything that may not have been canceled before...cutter comp G40, drill cycles G80, etc...

You can edit a post processor to make it output the correct code. There may be one available already.

Are you sure your control wont accept multiple G codes per line and it wasn't talking about M codes.

[thompson_chop]

You're correct, I can have multiple G codes per line, but only one M code per line.

Forgive me, I'm still trying to get use to this whole CAM software thing. Normally, programming at the machine, I can only enter one G per event and each event is a line.

Also, your suggestion worked on changing g41 to g01. And moving g41 back one line. Thanks for your help