Slow feed rates on curves, fast feed rates on straight routes

[Heritage820]

Hi there, I am sure this subject has been discussed somewhere in previous posts, but I can't seem to figure out why my machine cuts really slow on curves and fast and jerky on straight routes. This is what my tool parameters look like-

[Tailmaker]

Probably the acceleration settings of your machine.
I don't think the Vectric software has anything to do with it.
Check the g-code and you may find there is no specific command to change the feed rate in curves.

[Rcnewcomb]

Acceleration and deceleration is handled by the machine's control software, not by the Vectric software.

[adze_cnc]

My initial thoughts are that the vectors making up the shapes have an excessive amount of control points.

[sharkcutup]

Curves are synonymous for having many nodes if they are not bezeir curves. Having a lot of nodes with slow the speed rate.

Sharkcutup

[Heritage820]

My initial thoughts are that the vectors making up the shapes have an excessive amount of control points.

I like where you are going here. I know my control software is not messing with the feed rate because when I cut curved pieces using other software to generate the code, I have no problems and the feed rate is the same on curved and straight cuts.

[Heritage820]

Looking at my vectors and the curves are bezier, anything look out of the ordinary here??

[adze_cnc]

My next thought was: when saving from VCarve what post-processor are you using?

My version 9.519 shows three Morbidelli post-processors:

1. Morbidelli 336 NBR Arcs(inch)(*.xxl)
2. Morbidelli Xilog Plus Arcs(mm) (*.xxl)
3. Morbidelli Xilog Plus (mm) (*.xxl)

[Heritage820]

I have the same version of VCarve that you do, however, I only have this option for post processor- "Morbidelli Xilog Plus (mm)(*xxl.)"

[Heritage820]

I went ahead and added the other options for my post processor, so now I have all three. Going to try the one with "arcs" in the name today. Thanks!

[Tailmaker]

The "arcs" pp will only help with circles and circular arcs, not with the free-form curves.
You could look into the g-code for a representative piece of tool path and see if that has many more lines than you have control points.

[Mark]

Hello,
Once you are using an ARC post processor, you can convert any non-arc geometry within your design into arcs,
using the "Fit Curves to vectors" tool (using the "Circular Arcs" option).

I hope that this helps.
Cheers,

Mark.

[kstrauss]

I don't know anything about your control software but, assuming that you have the option, you may have "exact stop mode" (G64) enabled.
See https://linuxcnc.org/docs/2.6/html/comm ... cepts.html for more than you probably want to know.

Another possibility is that you have many short segments and your control software cannot process them fast enough to maintain full speed.