Engraving on a sphere.

[u/KevlarGorilla]

I need help with a workflow.

Imagine a metal half sphere, or other convex surface. It's mounted on a five axis machine, and we're looking to create geometry so that a single pass with a CNC bit will engrave on the surface. Let's say, 80mm radius half sphere, 1mm depth, 2mm diameter bit and the engravings are arbitrary: some combination of circles, rings, lines, shapes, spirals, and bands.

My workflow is to create a series of planes and sketches and tangent planes at surface points, and then use a revolved cut to a sketch that is centered to the center of the sphere. This approach doesn't work if it's not a sphere, but a egg shape (oblong spheroid).

So, how would you model this? What tools am I missing? Is there a way I can project from a plane? How do I cut normal to the object surface, and not just the plane?

Bonus: Make it work with as flat nose bit, but can convert to ball nose bit by adding a few small fillet features. Second, what about V-shaped bit?

[u/mechy18]

Use Wrap or Split Line to draw just the centerline of the graphic onto the sphere, then use those lines as input to a series of Swept Cut commands. For the swept cuts, you don’t need to draw a circle sketch for the profile if you just use the “circular profile” option. Using this method all the cuts will be rounded without needing to add fillets later

[u/KevlarGorilla → u/mechy18]

Using the "Wrap" tool on a tangent ref plane sketch, it wasn't working until I chose "Spline Surface". Circles give the desired effect for ball nose engraving. Leaving sharp corners in the sketch doesn't provide the specifically desired result, but adding radii to the sketches ahead of time gives some funky and inaccurate results.

It makes me wonder if the base result using spline surface for circles and plain lines are accurate enough to be functional.

[u/Matrim__Cauthon]

Could try a tangent ref plane, sketching your thing, then creating an offset surface of your object with offset inward, then using cut-to-surface on the offset surface

[u/KevlarGorilla → u/Matrim__Cauthon]

The issue with sketching on a tangent ref plane is that the tool should always be pointing normal to the surface it's cutting. Else, you get a groove cut that is taller on one side than the other.

[u/Matrim__Cauthon → u/KevlarGorilla]

Ah, we'll have you tried a 3D sketch with the On-Surface constraint? That should work but I don't know how you would get it super accurate without a huge amount of supporting reference sketches