Deep Vcarve Inlay

This forum is for general discussion regarding VCarve Pro
Post Reply
KWiK
Vectric Craftsman
Posts: 133
Joined: Tue May 27, 2014 3:03 am
Model of CNC Machine: ShopSabre

Deep Vcarve Inlay

Post by KWiK »

I am trying to make a deep inlay using a 1/8" 30º V bit. Unfortunately I cut the pockets before I worked on the Inlay Cuts. Anyhow I am trying to do a Start Depth of .325 (I do multiple cuts to get there) and a Flat Depth of .075. I keep trying different setting but this is always the result
star1.JPG
I presume it is because the height of the cutting edge is .233. I changed the tool to a .25 30º v bit and I end up with a much better result
star2.JPG
Unfortunately I don't own a .25 30º bit. Anyone have any ideas on how to accomplish it with the smaller bit?

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: Deep Vcarve Inlay

Post by mtylerfl »

Ok. So you cut the pocket in the material already. Couldn't you just set your Z-zero from the top surface of the pocket and avoid trying to create the "deep inlays"? Just setup your inlays for material equal to the pocket surface-to-bottom dimension as your material thickness.

I may be a little foggy on the situation you find yourself in, so feel free to correct me!
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Deep Vcarve Inlay

Post by FixitMike »

What is the V bit pass depth? It should be less than the height of the tool. Try a .125 pass depth.

From Help--Help Contents:
"Multiple z level passes will be automatically calculated where the tool needs to cut deeper than its Pass Depth specified in the Tool Database."
Good judgement comes from experience.
Experience comes from bad judgement.

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Deep Vcarve Inlay

Post by FixitMike »

That is what happens when the start depth is greater than the cutting height of the V bit.

I believe you can work around this by offsetting the star inwards (sharp offset corners) and changing the start depth accordingly.
As I calculate it, if you use a start depth of .2, a flat depth of .2, and a star vector that is offset inwards .0335" it should work with a 1/8 dia. 30 degree bit.

Reducing the start depth by .125 to .325-.125=.200 means that the offset for the Vcarved star will be .125 x tan(30/2) = .0335. The flat depth is increased by the same .125 to maintain the total cut depth of .400.

Note that this fix works only for designs with straight lines. It won't work for more complex design that includes curved vectors.
Good judgement comes from experience.
Experience comes from bad judgement.

KWiK
Vectric Craftsman
Posts: 133
Joined: Tue May 27, 2014 3:03 am
Model of CNC Machine: ShopSabre

Re: Deep Vcarve Inlay

Post by KWiK »

Thanks all for the replies. I did work on it some more and basically came up with the same thing as FixitMike. I am horrible with math, but can run 3D cad. I made a 3d Model of the star, then drew a line across it looking at it from the side, at a depth less than the cut height of the tool. I then measured the length of the line, and scaled a copy of the stars to that diameter. Preview appears to work, but I have not yet tried it.

This is a all end grain cutting board, so I like to make the inlays as deep as possible.

Post Reply