Cut all the way to the edge

[dryphi]

Which is not the right way to machine it, of course.

What is the right way then?

[dryphi]

Looks like we purchased the ShopBot just in time to receive support still, so they're sending us the download for VCarve Pro v9.0, which is very nice of them.

[mtylerfl]

+++1

[adze_cnc]

Now you're suggesting that if I wanted to add radii or other finishing operations around the edges, then I would have to start with a bigger material size in VCarve than my actual source material.

Only if you insist on using an STL file and 3D finishing toolpaths for those edges. If you use fillets and chamfers that match the radii and angles of existing cutting tools then you can get by using "2D" operations and job setup X&Y dimensions to match your material.

For example, the "3D" model in the first attached image was cut using a straight bit, a round-over bit, and a 90-degree V bit using the vectors in the 2nd image---no STL file, no Rhino file, nothing just vectors.

Even though the chamfer face is wider than the cutting edge length of the V bit all it took was a bit of trigonometry to figure out the depth of cut needed to match faces.

Besides, nothing says you can't mix 2D and 3D operations for the same job. Use a 3D finishing path for the concave dish in one of your images and a 2D operation for the pocket it sits in, etc.

[LittleGreyMan]

Which is not the right way to machine it, of course.

What is the right way then?

Post an actual part you'd like to machine. As Steven also wrote (as previous posters), machining this part with 3D toolpath doesn't make sense. So what's the use of learning the wrong way to do it?

[BradyWatson]

Looks like we purchased the ShopBot just in time to receive support still....

Care to clarify?...Did you mean that you just barely made the cutoff for getting the free v9 upgrade? -or something else?

-B

[dryphi]

Did you mean that you just barely made the cutoff for getting the free v9 upgrade?

Correct.

[dryphi]

Post an actual part you'd like to machine.

Do you want the STL file?

EDIT: STL file couldn't be attached. ZIP file attached containing it. Happy to upload whatever you like.

[dryphi]

The download count keeps going up but nobody is responding, haha

[LittleGreyMan]

The download count keeps going up but nobody is responding, haha

Maybe some of us have to work from time to time.

Having several CAM systems, I would simply not use Aspire (or Vcarve) for this kind of parts. Of course it's possible but I'm curious to see solutions to machine it simply in Vcarve, without using a roundover bit as you mentioned you don't want to have a bit for each radius you may use.

[dryphi]

Having several CAM systems, I would simply not use Aspire (or Vcarve) for this kind of parts. Of course it's possible but I'm curious to see solutions to machine it simply in Vcarve, without using a roundover bit

Yes I realize this is unconventional and probably not what the program was meant to do but this happens to be all that I have unless we want to pay the machine shop an hourly rate. The idea is to use the SolidWorks - VCarve - ShopBot work process for relatively simple parts that we can manufacture ourselves, thus saving grant money for other things. This will be one of the first parts we make and I'm doing it as an "experiment" to learn the process. Eventually I'll be showing the ropes to grad students with no engineering knowledge.

Any roundover bit set in particular you might recommend? A Google search for "shopbot roundover bit" doesn't find much, and most of the roundover bits you find are for router tables. I'm slowly working on improving our inventory of bits and such but what we have currently is fairly limited. Because every grant purchase must be justified in terms of research goals it's not always possible to get everything you might want.

Moving on...

Here's what I'm thinking and it will require at least three separate STL files and VCarve files. But that's fine because we typically export them as individual toolpaths anyway. Timing or efficiency is not a concern for us.
1. Suppress all features on top except the spherical cut and machine that (from an STL).
2. Suppress the spherical cut to generate the STL for the top rounds. For this I would use something like a 10mm material thickness. It's necessary to set the virtual material size about a drill diameter bigger than the actual material size (y'all swear this isn't a work-around but really it is). When generating the toolpaths you also have to remember to check Use Offset for your XY Datum in the material setup - the 0,0 point I set on the ShopBot will be at the top left corner of the material whereas setting the virtual material larger will move the origin outside of the actual part boundaries. A couple screenshots are attached of this step.
3. Suppress all features on the top and bottom and generate the roundover toolpaths for the edges of the sides. This would be quite similar to #2. When machining this step I would just rotate the part in the vice to each of the four faces and repeat the job.
4. Add the text directly in VCarve using vectors. I imagine this will be easy. Haven't decided which bit to use yet, any suggestions?

What do you think?

As an aside, IMO steps 2 and 3 would be somewhat simpler if I could just tell VCarve that it's okay to machine beyond the material boundaries, but unfortunately that's not possible. The virtual environment is meant to represent reality as much as possible. However in this case in order to machine beyond the part edges I'm required to set a larger work piece in VCarve than my actual stock, to "trick" the program into doing what I want. That's the definition of a work-around. I will try to send the designers a "suggestion box" about this. Maybe I'm the only one, but for me at least this was a source of frustration.

[ger21]

You don't need to use Solidworks or .stl files at all for what you've shown. Learn to use the tools in V Carve Pro, like the moulding toolpath, which will give more efficient toolpaths, and better results.

[dryphi]

You don't need to use Solidworks or .stl files at all for what you've shown. Learn to use the tools in V Carve Pro, like the moulding toolpath, which will give more efficient toolpaths, and better results.

That's an idea... Watching the molding tutorial video now.
Sounds using native vectors instead of imported models is analogous to vector vs. raster artwork in illustration software. Whereas raster art is prone to pixellation when scaled up for instance, vector based illustrations are not.

Using native VCarve features then, wow would you suggest I generate the spherical cut? Clipart? Using other methods I'm concerned the result might not be perfectly spherical. We need that cut to be a portion of a perfect sphere because it's going to interface with a femoral head.

[LittleGreyMan]

It seems Gerry has been much more persuasive than previous posters!

If you don't have very specific reliefs, it's much better to use vectors and 2D cut, it will be much more efficient and you'll get a higher quality. Just have a look at your spherical shape and the tesselation issue with a stl.

If we forget the stl basis and go back to vectors, Vcarve will perfectly do the job.

First point, why is Vcarve supposed to machine only inside material boundaries? Just open a new project, draw a rectangle of the same size and generate a 2D profile toolpath outside the vector. Vcarve will calculate the toolpath without any issue. Now move your vector totally outside the material and re-calculate. It works too.

But you won't be able to preview cuts out of the material.

(I am using Aspire 8.5, but AFAIK, these features are the same in Vcarve)

If I understand correctly, you raw material will be at the final size of the surrounding box of your final part, right?

You plan using a vice. How will you ensure your part is in the right position for the first step and after rotating it?

After watching the moulding toolpath and profile toolpath videos, try doing it in Vcarve and post your file.

[ger21]

What does the spherical cut look like? You can probably do that as well with the moulding toolpath.