Feed rate drops at dogbone

[logicspeaks]

Greetings,

I'm currently a CNC operator who uses this software at our shop daily. I found an issue I can't quite resolve and seems to be somewhat unpredictable.

The problem:

At times (not always) when I add dog-bones to our parts for routing my feed rate drops drastically prior to the dog-bone radius and then resumes like normal after routing that radius. The scenario is like this: I'm feeding at 800 IPM when suddenly my machines feed rate drops to 20 IPM until it finishes the dog-bone radius. Meanwhile the RPM stays at 18000 so its basically burning my end-mill during that 5-7 seconds. This happens whether I have multiple passes or single passes.

Additionally, this doesn't happen on every dog-bone radius. It seems rather random. The polylines appear to be completely clean and there are no extra points to speak of. This happens whether have an imported file from Rhino or whether I draw in manually within the V-carve Pro software.

Finally, if I were to delete my path and redo the toolpath within V-carve it still does the same thing. If I change it from a single pass to 2 passes, it changes which dog-bone it happens on but it never quits. Resetting my machine also doesn't change anything. Re-importing a new file doesn't change anything and redrawing the file doesn't change anything and redoing the dog-bone doesn't change anything. Additionally, I have had a copy of the drawing within V-carve (say I'm cutting 3 pieces) where only 2 of those pieces keep doing it and if I delete those two and copy from the first one without issue - it still has the problem.

Now I know that it is very possible that its something to do with maybe the config file for Shop Sabre or something with the way its electronics is interpreting the data. The gcode seems okay as far as I can tell. Nothing weird. Again, this appears to be random - nothing I predictable about it. I cannot recreate this issue.

I have searched through the forum and couldn't find anyone with this issue. If anyone has run into this please let me know. Id really appreciate it!

[Adrian]

It might be arc processing. You could test that by using a post processor without ARC in the name so no arc commands are generated or using the Fit Curves to Vector tools to convert any arcs to beziers.

If it's not that it might be the acceleration/deceleration settings for tight curves in the control software. My machine used to have issues with tight curves as the default config file supplied was meant for cutting large cabinet pieces. Once I tuned it for the smaller, tighter pieces I typically cut it was a different machine

[logicspeaks]

Thanks for the reply Adrian,

I'll try your suggestions but this still doesn't really make sense because I run hundreds of parts where I make dog-bones and in most cases (like 90% or greater) I never have this issue. Its as if it appears out of nowhere. But I won't know until I try your suggestions.

[tomgardiner]

My theory is that the dogbone fillets are of different radii. When the radius of the dogbone is very close to the radius of the cutter then the control software calculates a very small radius arc and the deceleration is large. If you draw the dogbones with a larger radius offset then the arc will be larger and the deceleration will be smaller. Even a few thousandths makes a big difference with my controller.
You can test this by cutting a rectangle with different dogbones at each corner.

[IslaWW]

Depending on the controller, your issue can be improved by adjusting the arc feed and centripetal settings.

That said, small radii on an 800 ipm line feed are going to be problematic unless you have lots of torque