Faceted edge rounded over

[ekparsons]

Hi,

I am 3D carving a part that has facets and the customer wants sharp straight edges. The edges are getting rounded over. The tool path is 3D finishing with a 1/8” tapered ball head running a 10% step over. I’ve changed the CV setting in Mach3 to stop on angles > 270, from 89 and 179 but don’t see any improvement. I am using machinist wax, which can hold a tight corner.

The angle is over 180 deg, with the outside facets in -45 deg on both sides, towards the center it slopes more gently ~15 deg downward from three faces. It appear dimensionally correct for the most part. The part is well secured.

I just need to get one right, if it takes more time that is ok because it will be used to make a mold.

I have a bunch of different bits and I am looking for things to try.

[highpockets]

Picture/s would help....

[ekparsons]

Oops, sorry

[ekparsons]

Also the shape was created in Rhino and imported.

[adze_cnc]

Also the shape was created in Rhino and imported.

As a native .3DM Rhino file or as a .STL file?

Is the "top" flat? If so you could mill that plane with an end-mill. Then mill the 45 planes with a 90 degree v-bit and the 15 degree planes with a 150 deg v-bit (if such a bit exists). You'd have do some trigonometry and layout out a bunch of vectors but it could be done.

The long 45-degree chamfers in the image were done with a 90-degree v-bit that had a cutting edge too short. It was done in two passes at two different depths with two separate vectors.

[ekparsons]

No, unfortunately it is not flat, this is what the model is supposed to look like from the preview JPEG.

[ekparsons]

The straight outline is a profile cut. I have tried x raster. I have cutting MDF, expanded PVC and machinist wax.

[ger21]

Set Stop CV on angles to 10°, and see if that works.
With Mach3, the higher the acceleration, the more precise your 3D parts will be.

[ekparsons]

The file was imported direct from a .3dm file. I will try 10 deg angle tomorrow, thanks to all for the help.

[TReischl]

Instead of fiddling around ad nauseam with CV settings etc, I would treat each one of those facets as an individual milling operation. Extend the facet beyond the intersections with the other facets. This will result in sharp intersections. Probably not even much slower. Think of it as three jobs.

If you insist on fiddling with control settings, you might try turning on exact stop aka "in position" on the control. Controls have a tolerance zone that allows the next move to begin before the current one is complete. I do not recommend this method since it usually results in tool marks.

[ger21]

The only CV setting that really makes a difference is the CV Angle setting.
I'd turn off all the other CV settings.

Mach3's CV mode is not the best when you need very precise 3D toolpaths and sharp corners. Mainly because Mach3 has no settings to specify deviation from the toolpath, so you'll almost always see rounding in some areas, unless you cut slower than you'd probably like.