Whew. I was beginning to think it was just me. 
What was the tool set for?  It's hard to tell.
I just noticed on yours that it also rounds the corner at the top left before it goes on to the lead out. I don't think it should be doing that either. Should probably be hanging a hard right there.
I also notice that when you set the tool to say .125 it rounds both top and bottom left side corners even though it does stop the X creeping as it climbs. Seems maybe it's not paying attention to exact stop?

Sage

Sage , the radiused tool path is normal... to go around a sharp corner without the cutter leaving the profile. I saw that illustrated with the triangles in the manual.
I'll keep watching.
Thanks,
RC

Here is a clip from the manual.

"For Mach2 to work, the tool path must be
such that the tool stays in contact with the edge of the part geometry, as shown on the left
side of figure 10.1. If a path of the sort shown on the right of figure 10.1 is used, in which
the tool does not stay in contact with the part geometry all the time, the interpreter will not
be able to compensate properly when undersized tools are used."

D1  .025" is bad.
Anything .030' and over is good.
Probably should stick to the more conventional method mentioned earlier by Ger.
Either use 2 offsets, OR use 2 D's and comp.
RC

Interesting comment from the manual. (Noticed figure number is wrong - another one for the list).
Especially the point about small tools being a problem. Also the fact that it is not rounding some corners (bottom left) and is therefore not following it's own rules is perplexing.
I think it's one for the programmer(s). Hopefully they get wind of it.

You are correct about sticking to what works.  I'd like to stick with one tool path and two offet numbers. I beleive there is way to use G-code to change the values in the tool table. Perhaps G41 P0.###
Is that it?
Tat way I can call the same subroutine twice and keep the code compact.

Sage

I noticed the fig. # also.
The only time it doesn't round the lower left corner is when the path goofs up (.025" or less). Otherwise, it's rounded.
Not familiar with changing the table with code, but you could easily call a different tool. D1=.125, D2=.145  or whatever to create the desired offset.

Just like Ger said in reply #34.

Good luck Sage,
RC

You can't change the tool table with g-code. You can however, use P to specify the tool radius used for comp. So, you can use:

G41 P0.165

for roughing, and:

G41 D1

for finishing, and use T1 for both without changing tools.

As for the manual, the comp section was originally copied from the EMC manual. (pictures and all)

And I get the same error as the posted pics as well.

Ok, thanks for the tip. I'll be using it big time in my re-write of the part G-code.

So, case closed I guess unless Graham maintains his is working ok. Then I'd be interested to figure out why.

Can someone make sure this is put on "the list"?

I'm assuming the programmer will have more insight as to why the small cutters screw up.

It is a pretty small part and a small cutter. Maybe the math is buried in the decimal places and falls apart.

I'll just add it to my list of things to watch out for.

Thanks everyone.

Sage

This is an old program I ran on my mill. I don't use cutter comp on the mill as the cam calculates for the tool offset.
But to try and better understand where and how cutter comp was goofing up I started trying as many programs as I could.
The picture below is an interesting example of how the arc in the profile should have been trimmed to stay within the starting area.
The profile should never cross its self. Although there is times when you may want to cross a profile like in a figure eight it should not be possible to do so using left or right cutter comp.
It should only recreate offset periphery geometries for the first area that can be painted "Flooded" with a brush "Tool" the size of the current active tool.
The specification of the G4* offset word would determine in witch bounds of the area to fill.
A determination of open ended and area type geometries would need to be determined.
Geometry specifying a G4* word and which does not intersect itself would be considered open ended.
Geometry intersecting itself without the G4* word would be a center line tool path no offset needed.
Geometry intersecting itself with the G4* word would need to be "Flooded" like stated above.

If we can get that working in the X Y plane then maybe we can move on two all three. 


 
       
     

Hi Guys

after much experimenting I now have the same fault as you do, the difference was I was running Mach in Metric and entering metric values e.g. .02mm , running it in inches gives the same fault.

I am in contact with Brian about this, so we will see what he has to say.

Graham