Pockets for inlays with sharp points?

[rsnewmanRFVUW]

I'm new to cnc, cutting pearl inlays and pockets for banjos  I've just cut a 5 point star, and cutting the pocket with a .020" endmill.  

The cutter is unable to get all the way into the sharp point, so I have to create a new drawing, adding a little .020 box at the end of each point.  See the jpeg attached below.

I'm wondering if there's a way I can accomplish this with the software?  Can I get a toolpath to cut outside the lines only where it's necessary to cut to the end of the pocket?

[paul.clauss]

Hi @rsnewmanRFVUW

Thanks for posting! It looks like you are having difficulties machining to a sharp point in your star model.

What toolpath are you using? Most 3D toolpaths work with a machining boundary selection, which requires you to set the tool condition to either tool center inside, on, or outside the boundary. For your purpose, I would imagine that you are using the "Tool Inside Boundary," which will cut the star points short before the end. They will, however, give the sharpest point possible with your tool. 

Unfortunately, you cannot vary the boundary conditions of a single chain defining a machining boundary in Fusion 360. Using the sketch geometry may help you get the results you are looking for, but this will create a straight section at the end of the star arms rather than a sharp point. I would instead cut the points slightly short and keep the tool inside the machining boundary, as this may give a more consistent surface finish and profile.

Hopefully this helps! Please let me know if you have any other questions. Also, as the amount of material that will be removed depends on the dimensions of your star model in relation to your tool dimensions, feel free to provide the dimensions for the star (or the Fusion design you are working with) and I am happy to walk through how I would approach this pocketing toolpath in your model.

[rsnewmanRFVUW]

Thanks for the reply Paul.

I start with a 2D pocket, using a 1/16" bit, followed by a rest cut pocket with a .020" mill.  The little rectangle at the point is .020 wide.  Then I do contour cuts with the .020" mill, taking .001" per cut till the inlay just fits in.  In practice it works just fine, the glue fills in the gaps and is virtually invisible.  WAY better than when I did it manually with a dremel

I've ordered a .012" end mill to sharpen up the inside corners in the pearl stars.  I could make the rectangles .012 wide and use that for smaller gaps,, but I really don't think it's necessary.

Sounds like there is no way to avoid having to sketch those little clearance rectangles at the ends of the points.  It's not really that difficult or time consuming, but as I get more comfortable with Fusion, I'm very interested in what it's capabilities are.. 

The star is 1" across the points, and 050" thick.  I am very interested to learn how you would approach this, if it's not too much trouble for you.

Thanks again

Richard

[paul.clauss]

Hi @rsnewmanRFVUW

Thanks for the response! I kind of missed that you need to inlay the stars into the holes - that is my mistake!

In that case, I like the process you have. While having to repeat the contour cuts is time consuming, it will give the best fit for the inlay, as you will be able to test the fit and continue removing only as much material as necessary. My only recommendation would be to keep track of the number of 0.001" contour cuts you need, and then simply offsetting the model contours by that much if it is consistent (to oversize the model for CAM and avoid having to repeat the contour cuts).

I think that the only real way to avoid the rectangles, for this cut, is to oversize the profile being cut. This will allow the points of the star to fit in more easily, but may make the overall fit slightly worse (as the entire star will be slightly larger). I would recommend trying both techniques and seeing which works better for you!

Please let me know if you have any questions - I'm happy to help!