So I am getting that Tool radius not less than arc radius with compensation error. I kept fiddling with lead in percentages, changed to smaller and smaller endmills just to see if that would fix it. It didn’t. I sent in a support ticket to Tormach to see if it was something with Path Pilot. Their support noted there was not an xy address before the I J resulting in an error. So is it something I can fix without manually editing every arc, and why is it doing that? Is it the Tormach post processor or is it SolidWorks?
snippet
Z1.35
G1 Z1.1875 F7.8625
G41 D06 X.3885 Y.5233 F23.5875
X.3793 Y.5149
G3 X.3752 Y.5062 I0.0084 J-0.0093
X.375 Y.5 I0.1248 J-0.0062 F31.45
I0.125 J0 
X.3752 Y.4938 I0.125 J0
You have to give us an initial X or Y point. Your code says it coming from Z to a compensated X or Y. You must have an initial point that is larger or equal to the radius of the tool being used. Then compensation is instated from that point to the initial cut point on your part. Post the half dozen lines before what you posted. If there is no code before than lack of an initial point to instate compensation from is your problem.
N40 ( Contour Mill15 )
M1
(1/8 EM CRB 2FL 1/2 LOC)
M6 T6 G43 H06
S4250 M3 M8
G55
G0 X.5 Y.5
Z2.375
Z1.35
G1 Z1.1875 F7.8625
G41 D06 X.3885 Y.5233 F23.5875
X.3793 Y.5149
G3 X.3752 Y.5062 I0.0084 J-0.0093
X.375 Y.5 I0.1248 J-0.0062 F31.45
I0.125 J0 
This is what the post processor produces; I think I will try to take out these lines
X.3752 Y.4938 I0.125 J0
X.3793 Y.4851 I0.0125 J0.00
You are only moving .023 in Y. You seem to be moving sufficiently in X. Try splitting the moves if possible . Instate G41 in only X since the move is more than .0625 if possible then move in Y on the next line.
The real problem is why does the post processor not do it’s job. So I will try to figure out what processor I downloaded and try the other one and see if it does a better job. Thanks
Post processors are never perfect. Many times you have to customize them yourself to get what you want. Other times so many hands have been editing them they are completely screwed up. Try the generic haas or fanuc compatible post processor and edit the beginning and ending of the post to match a pathpilot conversational program. You can also change to computer instead of control compensation. You will be locked into the size of tool used in the cad post at that point.
I use SW CAM with the goengineer postprocessor. The tool radius error occurs when on the NC tab in the CNC finish parameters CNC compensation and Toolpath center compensation are both enabled at the same time. For some reason it was the default setting for contour milling at least on my SW2021 install. If you set CNC compensation to off and repost you should get rid of the tool radius error.
You can configure the default settings in Technology Database → Mill → Strategies → Default Operation Parameters → Contour Mill → NC → CNC finish parameters.
That could be it, thank you for your input.