Is anyone doing this? Using the Amana #46280 as the Vbit in advanced Vcarve? I have seen videos of people using this to get tight inlays, but they are all using Vectric software. I cant get it set correctly in Carbide 3D.
I have not used a tapered bit for an Inlay. I have used the Frued 60 degree and the Groovee Jenny 60 Degree vee bits with good success. The key is on the male inlay to have a starting depth of .1 inches. The reason for this is it makes the male inlay slightly smaller than the female pocket. The reason this is important is with a slightly smaller inlay it seats deeper. The 60 degree would give you more surface area on the sides of the female pocket to get a good glue up.
Here is an example of varying start depth of the male plug.
Starting on the left the same image was carved (male plug) and you can see starting depth at .1" seats the plug much deeper than starting at the top of the material and the picture on the right shows that making the male plug deeper does not help because the inlay to the same size as the female pocket causing the male inlay to barely insert into the female pocket.
1 Like
You could but you would need to do some math & offset the profile by a little less than the radius of the cutter. I get really close to 0.015 for that cutter.
Offset the female profile 0.015 inside, and the male 0.015 outside. Use the same start & max depths that you would with a vee-bit.
This may not work with sharp corners. Your minimum radius, I think will be the radius of the cutter at the depth your are cutting plus the radius of the ball. So if you’re cutting 1" deep the radius of the cutter is really close to 0.125, and the radius of the ball is 0.016, so your minimum radius on your profile would be 0.141". Or the male will have larger radii in the deeper part of the inlay on corners.???
1 Like
My experience . . . struggled trying to get the right offsets to make a 46280 work in CC. Offsets necessary because the software doesn’t recognize the geometry of the tool accurately, so the actual tool length is shorter than the software measured length due to the missing ‘v’ on the point. Vectric has a specific tool type for tapered ball nose, so you get accurate cuts with no special offsetting required. Can make fairly detailed fine inlays. I find CC better for me on some projects, Vectric for others–good to have options.
I’m also increasingly convinced the other half of the secret is clamping pressure when gluing the inlay. I learned from others and have reverted to a shop press.
1 Like
Check out my reply here:
1 Like
This topic was automatically closed after 30 days. New replies are no longer allowed.