New problem with G3 commands

I have an Acu-rite controller I have used for years with no issues, generating G-code with HSMWorks in Solidworks. Now all of the sudden I am getting errors when I load programs that highlight a line with the error "Circle incorrectly programmed". I contacted Acu-rite and they pointed out the error in the code. This is the code generated by HSMworks that throws the error at line N390:

N380 G3 Y-0.5617 Z-0.0693 I0 J0.0313
N385 G1 X-0.9681 Z-0.0734
N390 G3 Y-0.6243 Z-0.0768 I0 J-0.0312
N395 G1 X-0.85 Z-0.0809
N400 G3 Y-0.5617 Z-0.0844 I0 J0.0313
N405 G1 X-0.9681 Z-0.0885
N410 G3 Y-0.6243 Z-0.0919 I0 J-0.0312

Here is the corrected G-code that doesn't throw an error:

N380 G3 Y-0.5617 Z-0.0693 I0 J0.0313
N385 G1 X-0.9681 Z-0.0734
N390 G3 Y-0.6243 Z-0.0768 I0 J-0.0313
N395 G1 X-0.85 Z-0.0809
N400 G3 Y-0.5617 Z-0.0844 I0 J0.0313
N405 G1 X-0.9681 Z-0.0885
N410 G3 Y-0.6243 Z-0.0919 I0 J-0.0313

Is this a rounding error in Solidworks? Is it a problem with the post processor? Anyone have any idea what the fix might be for this?

Thank you,

Jeff

If anyone cares I believe I figured this out so I'll post the answer in the unlikely event it can help someone. It turns out its a rounding error in the CAM software (I think). This slot had a radius of .28175. It was rounding the negative J values one way and the positive values the other way. When I do any radius that only goes to 4 digits the problem disappears. Why it does that I can't say, but the proof is in the pudding. I can deal with 4 digit radii.

Try changing the post processor to use 5 digits. I did that to remove errors using compensation on my milltronics mill. Letting your controller do the rounding may help.