Simple Task Got Me Stumped

[Burkhardt]

I thought I know my way around Vcarve, DeskProto and 3D-Cut quite well but I ran into a problem today.

I have a simple rectangular board (happens to be about 7" x 5" ) and I want to bevel the top edges. I know I could just use a roundover bit and cut around the perimeter to do that in a few seconds. But that would limit me to the radius of the bit (I have only 1/4" radius). So I thought it should be really easy to do that with a ballnose bit and rather small stepover.

I want a bevel radius of 0.2" and a stepover of 0.01", that means I would have to go around the 4 edges about 32 times. With a total edge length of 24" and a feed rate of 120ipm that should only take 6 or 7 minutes theoretically.

I could not find a way to do this in 2.5D Vcarve at all (I know it is not intended for this purpose). But when I load the 3-d model into 3D-Cut or DeskProto all the strategies I tried lead to machine times of over an hour, sometimes much more. 3D-cut is especially bad because it has only linear finish cut strategies which try to machine the entire board surface which is stupid. DeskProto has a waterline toolpath strategy that should help but it takes forever to calculate and sometimes crashes.

It may be that Aspire can do that but unfortunately I don't have this software. I am almost tempted to hand write the g-code for this purpose.

This is such an elementary task, there should be a simple way to do this. Any idea?

[adrianm]

To do it in VCarve you would need to create multiple toolpaths with each one having an offset and start/cut depth on from the previous one.

Bit tedious to create but should cut pretty quickly once it's done.

[jerry_stanek]

why not do in vcarve pro with a two rail sweep.

[adrianm]

The two rail sweep is in Aspire not in Vcarve.

[Brady Watson]

why not do in vcarve pro with a two rail sweep.

You can't do a 2-rail sweep in VCP. Aspire only in the Vectric family.

It is possible to create a 3D model in another software package that has the radius you need. Then generate the toolpaths in Cut3D. You then save the Cut3D file. You can then import it into VCP and register it to the rest of your 2D project.

You can do it using the SB3, using the Extruder utility - but it will not be as efficient as a CAM-generated file.

-B

[adrianm]

I haven't used it myself but I've seen some impressive things done with Paul's FlutePlus gadget. Should be able to do this with it but it will probably still take a while due to the type of machining.

http://paulrowntree.weebly.com/gadgets.html

[Ger21]

As Adrian says, create your 32 offset vectors, and assign the appropriate depth to each toolpath.

I've done this sort of things many times over the years. It would be nice if V Carve Pro (or Aspire) could use the Z value of imported vectors as the depth of cut.
I've written autocad macros to automatically offset and set the correct Z depth of polylines, and used a CAM program that could use the Z depths for the toolpaths (CadCode). Once the macro was written, this would become a 2 click operation.

With Aspire, you could import your model, and set machining boundaries to just route the edge. This would be much faster than Cut3D.

Unfortunately, with the tools you have, I'd vote for the 32 offsets.

If you go through the effort of setting up 32 layers, and making toolpath templates, then saving the file as a template, it will be much less painful the next time you want to do this.

[myxpykalix]

In the end i think it will be easier to just go buy a bigger roundover bit, however maybe you could send your model to someone who has aspire and let them make some toolpaths for you?

[adrianm]

It would be nice if V Carve Pro (or Aspire) could use the Z value of imported vectors as the depth of cut.

I haven't made use of it myself so not sure if it's the same thing but there is an option on the vector selector part of the toolpath to set the cut depth from imported vectors.

[Burkhardt]

Thanks for all the recommendations. I can't believe that is not a standard function. After all a vcarve chamfer may do it sometimes but a rounded bevel is such a common feature. Maybe I should write to Paul Rowntree as a suggestion since he seems to be really good at Vectric gadgets. I tried to understand if the flute+ gadget could be used but not sure about that.

Anyway, for my project I will probably make a little program to create g-code for bevels on rectangular plates. May not be much more work than parameterizing dozens of tool paths by hand and could be useful for other projects in the future.