Is there a way to generate toolpaths for the grooves in CC pro? I know I could model them, and hit 3d finish. I’m just looking for advice on recreating something similar.
Thank you.
Save for in V carving, Textures, or 3D, Carbide Create only does toolpaths with flat bottoms.
I do not know of a CAM tool which will allow one to select geometry and cut it at an angle.
Because of this, I’ve been working on a system which allows full control of the tool by writing out G-code, but it’s a programmatic system, and only suited to projects which can be defined mathematically.
1 Like
In most cases, it would be great if you could define the depth of cut based off the 3d geometry instead of the stock thickness. Say 1/8” doc with .125 ball endmill and no offset on the desired vector.
Will vcarve follow the 3d geometry? If so could I just use a ball endmill instead of a vbit?
It can be done. I used the red rectangle to model the curved grip. Then the green squares to subtract the ends. I used the large blue rectangle and the edge of the grip to machine away the outside material just for show. The slightly larger rectangle around the grip edge is the boundary for the 3D finish pass to get the curved top. Then the 5 spokes are obviously the boundaries for the 3D groove paths.
Each groove path is separate, and you have to match the toolpath angle to the groove angle.
I disabled the groove components to machine the top of the grip. Then enabled them & machined the grooves.
Lucas_Carroll_Pistol_Grip.c2d (468 KB)
And yes, a “curve drive” 3D path with a depth offset would be really handy.
4 Likes
Thank you Tod. I have done similar setups this way, I am more concerned with the finish. With straight lines one could adjust the angle of the finish pass to correspond to the groove. As far as trying to follow a spline, I am hitting a brick wall.
No way I know of to follow a curve & a 3D contour in CC. But even if I had cut all those grooves at 0°, it would still cut it, just would probably need some hand cleanup.
3 Likes
I love CC, I just wish we had a few more toolpath options. Radial finishing would be great too.
I did work up a file for radial finishing:
It was done in OpenSCAD Graph Editor, requires the Python-enabled version of OpenSCAD, and the installation of my gcodepreview library, which arguably makes just doing it in Carbide Create using the Radial Array tool much more expedient — I did that in a current project, will post the file this evening.
1 Like
Awesome, now you’re going to have to explain this to me like I have absolutely zero clue what you’re talking about, lol!
Ok I understand. I was speaking in regards to 3D finishing.
I’m going to link a YouTube video, I know absolutely nothing about programming but this looked very interesting.
1 Like
I do this for holes. Use a tool a bit smaller than the hole & “Hole Mill” it, rather than drilling.
Here’s the sample part from the video, scaled down to use a 1/4" tool…
Some things to note. You have to adjust the ramp angle based on the size of the feature being cut.
Larger features require a smaller ramp angle to get roughly the same depth per cut.
CC likes to conventional mill. Notice in the video he’s climb milling. (<— Another shameless plug for climb cutting 
)
Ramping in CC starts right on the part surface. If you want a little bit of lead in, make the toolpaths a little bit deeper, and offset your Z zero on the machine by that same amount. i.e. Your pockets are 0.500 deep, so I program them to 0.520, and when I set my zero I touch off to the top of part & enter -0.020 in the Z register.
I set my depth of cut in the file to 0.490. This forces a rough/finish strategy. The tool will ramp down to 0.490, make a flat cut at that depth, then ramp down to 0.500 & make another finish pass.
high_feed_ramping.c2d (224 KB)
3 Likes
I take a similar approach. I generally cut phenolics, so assume I want a pocket .20” deep. I will turn on ramping and put my start depth at .19”. I don’t think this would work with aluminum but it works fairly well with phenolics and hard woods. I also crank up the plunge rate so it’s a fairly quick operation.
This topic was automatically closed after 30 days. New replies are no longer allowed.