I've been dealing with this for a long time now. It's mostly a problem on larger pieces only because it's more noticeable. It happens on everything.

This was cut with a horizontal strategy with a .010" step over. The Intol and Outol are .001" and the piece is 15" in diam. The cut direction is mixed.

The piece has been primed and I sanded through to the base material so the ridges and valleys would show up.

Here is a wide shot. One think to look at is how symmetrical the chop is as it leads around the bell and the goes straight as the wall of the pattern goes straight. also notice how there is no chop where the axis is running nearly parallel.



Here's a closeup



I'm really getting tired of sanding this crap!!!

Derek

What kind of cam program are you using.

And what is the precision of the line used to do circle machining.(see next line)

Is your Cam software output line instead of I and J code.

I have seen this with Cam software where the precision was set for roughing machining. You have to change it for finishing.

Maybe I'm complety wrong.

Jeff

 

Backlash is not likely to cause such regularly-spaced defects.  Far more likely it's a problem with the G-code - instead of outputting an arc, it's outputting short straight-line segments, which your machine is faithfully reproducing.  Can you post a small sample of the G-code?

Regards,
Ray L.

You guys may be on to something.
Here is a patch of code

N28 G01 X10.968 Y4.755
N29 G01 X11.061 Y4.777
N30 G01 X11.101 Y4.787
N31 G01 X11.234 Y4.822
N32 G01 X11.368 Y4.861
N33 G01 X11.474 Y4.895
N34 G01 X11.501 Y4.904
N35 G01 X11.608 Y4.942
N36 G01 X11.714 Y4.982
N37 G01 X11.768 Y5.003


And here is a screen capture of the code plotted against the tool path.


The larger segments are .140" long. Yikes that's a pretty long straight run.

Derek

Yup, not good G-code.  Those should all be G02s or G03s, to cut real arcs.  What CAD/CAM are you using the generate that code?  It could be the CAD is drawing it that way, and the CAM will just follow the CAD.  Or, it could be an "optimization" in the CAM.

Regards,
Ray L.

Hi Derek,

Perhaps a silly question but are you certain that your spindle / cutters are running concentric ?.

Tweakie.

It is sometimes a option in the post processor of the CAM program.   Try posts for other machines to make sure it is capable of G2 and G3.

usually you want G2 G3 with incremental I and J


If not just edit the code by hand on simple things like that..


G0G90X2.Y0
G2I-2.F15.


Will send the cutter on a 4 inch (centerline) cut at 15 inches a minute

change to G3 if you want it to go CCW