MecSoft Corporation

I'm having trouble trying to figure out how to set up the milling of the teeth on this Hirth connector.

The photo shows an original STL file that really wasn't that good. So I created the drawing from scratch with the idea of using a 60 degree V mill for the teeth. The 3D printed STL file came out really nicely and even locks well to a companion part. I'd like to make it from metal so now the CAM part.

I think I have the profiles done but really can't get a handle on how to select and create the teeth which are actually beveled so it's likely a 3D not 2D operation. The V bit tool is 6mm and has an angle of 60 degrees. The ones I bought have a sharp edge. I can live with that.

Any suggestions on how to fix this?

I've been able to use the Engraving method with the 60 degree V bit (30 degree from centerline) and done a dry run on the mill. However to do that I had to first export the file as a STP file and then load it back into AlibreCAD and then start AlibreCAM. Loading it with VisualCAM had the same results as AlibreCAM. The difference is shown in the pictures.

I sent a copy of the STP file to my friend who plays with Fusion360. He quickly whipped it out using what Fusion called Radial. He also surfaced the flat area and the center hole so the G-Code included that. But the interesting part is shown in the LinuxCNC image. I'll add the STP file in another posting.

So how is this done in VisualCAM? I've tried all the variations in both the 2D and 3D milling tabs and it's all really messy.

And here's the STP file if someone wants to try it with VisualCAM.

You can use 3 axis Radial Machining in VisualCADCAM to program the teeth.

So it's as simple as just setting an inner and outer containment ring and then using radial machining. Thanks. I've been playing with that a bit but there is another problem that setting various parameters doesn't seem to 'adjust'.

The issue is that the very first pass plunges to the bottom and then takes the deepest pass and then the next few are redundant. The tool path needs to enter at the highest Z rather than the lowest Z. Then each of the first passes subsequently goes lower. After that it's fine.

I tried putting the containment circles at different heights but that didn't work either.

Also if I want the tool bit to go a bit further to the middle and further past the teeth I can specify different ring sizes but then the path direction changes too. Any way to make it do a bit of over-travel past the actual surfaces.

As Radial Machining is a finishing operation, the toolpath is generated to the part geometry.
You can use Z containment, and specify Step-down Z cuts to program this in multiple Z levels (like a roughing operation). This is available under Z containment tab.
Alternatively you can program a Horizontal roughing toolpath before a finishing operation.

To extend the toolpath past the edge on both sides, you can set Cut Connections to Linear, specify a length and angle =0. Cut Connections is located under Entry/Exit tab.

Cool. I wonder why I couldn't figure that out. I did try things but not the Z levels. Nor did I try the cut connections.
Now is there a way so the first cut starts at the highest Z level rather than the lowest?

I tried connections and that worked great. However the Z levels is a non-starter. Total waste of machine time. What's needed is the ability to declare where the cut starts. By default it's at the bottom of the tooth rather than at the top. Which seems kind of odd. I'll try a roughing operation and see what it does.