Jerky tool path generation (why?)

[fritter63]

HI all, I'm trying to understand why one of my toolspaths runs (or rather, is generated to be) jerky when on the machine.

See attached picture. Here I have selected an oval shaped pocket and a 1/4" bit. The pocket is about 1/2" wide. The resulting g-code will

first cut the larger diameter in a couterclockwise motion which is very fast and smooth, then it will cut the inside dimension with a couterclockwise motion which is slow and jerky. It is steping along the arcs one little bit at a time with pauses in between. 

It's not clear to me why this is. If you look at the g-code (attached), you can see that indeed the counterclockwise path issues a G3 up front, then just a bunch of x/y coords. The jerky clockwise pattern has alternating G2 and G1 commands. What is the reason for this? Can't it run counterclockwise the same as clockwise? Is this to due climb cut vs normal cut direction concerns?

I have seen This Thread, but I don't think this is related.

Also, here is a video showing the machine in operation. It is timestamped to just before the first counter-clockwise cut, so you can see that and then see the jerky part aferwards:

https://youtu.be/rtOwYWi6ZoU?t=33

Thanks.

[HughesTooling]

Can you attache the f3d file. Are you using a 2d op, the offset from a ellipse will be a spline and I think that's causing the problem, you'll probably find you get a better toolpath from 3d contour with smoothing enabled. I'm guessing the smooth toolpath is from the ellipse and the jerky toolpath is the offset.

Mark

[HughesTooling · Accepted solution]

After rereading you post again I see what's going on. When the toolpath is an offset to the outside the op does corner rounding and adds a rad at the end of every short line, the same rad as the cutter.

Here's an example with no smoothing using the setup below.

This generates over 700 lines.

If you enable smoothing, set the tolerance to 0.001 and smoothing to 0.01, ignore the warning message.

You get 32 lines.

Mark

[fritter63]

Thanks @HughesTooling

How did you get that display that shows the gcode as "linear", etc? Is that in F360 or is that another app?

[HughesTooling]

Expand the op, the bottom node is the toolpath, right click and select view.

Mark