Circles Not Circles

[epracefan@gmail.com]

I'm running G-code generated by Fusion 360 that's using adaptive clearing to create a pocket. The tool path is supposed to be circular, as indicated on the UCCNC screen, but the other photo is what is being cut. Do I have a setting wrong that might be causing this? I'm using the UCCNC post processor that was written by the Fusion 360 team.

This is the third time I've seen this. One instance I was cutting a pocket with some small round islands in the middle. The islands came out as irregular shapes. After that incident, I created a short program that cut a similar pocket in MDF with an island and it looked OK. I also saw a similar problem cutting a 3D profile that was supposed to be a 90 degree arc but the arc came out in two or three straight segments.

I'd appreciate any help you can provide.

Thanks
Ed

[cncdrive]

Looks like a CV tolerance setting issue.
With the UCCNC you can set the tolerances you allow on the path and if the software thinks that it can finish faster with an alternative path which is closer to the original path than the tolerances you defined and allowed then it will go on that path.

You can control the tolerances in the Configuration/General settings and on the left side there are the CV settings.
Especially take a closer look at the following settings:

- Linear error max.
- Corner error max.

These define how much in Units the software can go off the path in order to finish the path faster. (More description in the UCCNC manual.)
The higher you set these values the more it can go off the path.
For example the linear error max. is defined to 0.03 Units which is mostly fine for millimeter units as it is a pretty low value in millimeters, but may be high for some jobs if working in inches.
So, you may want to lower these if you want tighter path following, lower tolerances.

You may also define the tolerances with the G64 code (it sets the same parameters) and it's parameters are described in the UCCNC manual.
So, you could for example place a G64 in the beginning of your g-code file with the required CV parameters for the actual job and this way you do not have to remember what tolerances were the best for particular jobs. So, the next time you will run the same file it will have the CV tolerance settings.
Or if slower path execution is not an issue then you can set the CV tolerances low for all jobs and leave it like that all the time.

[epracefan@gmail.com]

Thank you very much for the prompt reply and solution to my problem. I did notice mention of those settings in the user's manual, but not knowing what I needed, decided to leave the default settings.

I changed both to .002" and was able to finish the part with no further problems. I'm really liking UCCNC with the 2017 screenset, much more than LinuxCNC which I've been using for a couple of years.

Thanks Again,
Ed