Inlay Help

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro
Post Reply
Bigjay
Posts: 7
Joined: Mon Jul 12, 2021 8:49 pm
Model of CNC Machine: Mill Right Mega V

Inlay Help

Post by Bigjay »

I am just starting out with CNC work and have attempted some inlays but with no success. I have included pictures of what is happening and hopefully this is a simple fix. I have my pocket flat depth set at .3" and the inlay start depth of .2" and flat depth of .1" as this is what I have found to work well in a lot of tutorials. I am using a 90 degree V-bit with 3/8" diameter and 7/16" cutting height as well as a 1/4" end for my clearance tool. What is happening is that the plug or inlay piece has straight sides for approximately .1" before it gets to the v groove which does not allow for proper fit up.
Inlay.jpg
Pocket.jpg

User avatar
Adrian
Vectric Archimage
Posts: 14504
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Inlay Help

Post by Adrian »

I don't do those types of inlays personally but I doubt they will work with a clearance tool due to the way they use a start depth. When the original method was published the v-carve toolpath didn't support clearance tools.

User avatar
adze_cnc
Vectric Wizard
Posts: 4303
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Inlay Help

Post by adze_cnc »

When you preview the toolpaths for the plug in VCarve do you see the same "straight sides for approximately .1 inch before it gets to the v groove"?

i.e. if the preview looks correct and the cut doesn't then it's not the toolpaths but how the Z height is set between tool changes.

Bigjay
Posts: 7
Joined: Mon Jul 12, 2021 8:49 pm
Model of CNC Machine: Mill Right Mega V

Re: Inlay Help

Post by Bigjay »

The straight edge is there on the preview. I think I may have been just going too deep for that bit as i have since changed the pocket flat depth to .2" and the inlay start depth at .15 and the flat depth to .05 and it seems to work fine.

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: Inlay Help

Post by FixitMike »

A 3/8" diameter 90 degree V bit has a side height of only .1875". If you attempt to make a deeper cut (Which is what the first pass on the male will be, since it assumes everything above the start depth is air for determining the depth of the first cut) everything above the cutting edge "corner" will be a straight up and down side.
You need a larger diameter diameter V bit so the side height is at least equal to the start depth plus the tool pass depth (or flat depth if it is less than the tool pass depth) since that will be the depth of the first pass on the male part.
The other solution is to run multiple toolpaths, starting with a start depth of zero, then incrementing the start depth by the cutting depth (or a little less) until you get to the desired starting depth.

If you use the multiple toolpath method, you can ignore the flat end mill cleanup toolpaths until the last toolpath to save time.

Adrian: Using a flat end mill for cleanup does not cause any problems with the Zank inlay. It just means that the cleaned up areas will not have any "peaks" caused by stepover of the V bit point.
Good judgement comes from experience.
Experience comes from bad judgement.

User avatar
Adrian
Vectric Archimage
Posts: 14504
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Inlay Help

Post by Adrian »

FixitMike wrote:
Tue Jul 13, 2021 8:04 pm
Adrian: Using a flat end mill for cleanup does not cause any problems with the Zank inlay. It just means that the cleaned up areas will not have any "peaks" caused by stepover of the V bit point.
Thanks. I wasn't sure if it would work properly as it uses the start depth in a way it was never designed for so my initial thought would be that a straight/v-bit combo might end up with a straight sided cut as the material shouldn't be there.

Post Reply