Best V bit for Inlays

[sm38240]

All,

I am currently using a 1/4" 60 degree V bit for inlays. I occasionally have tearout or chipping of the edges on my male parts. Often, these tearouts end up buried in the female part and cause no issues, but occasionally they do. Seems the harder the wood, the more prone it is to tear out. A recent piece of purpleheart was unusable due to the tear out. Is there a better bit profile or is this more of a function of my feeds and speeds?

Thanks!

Stan

[Adrian]

I find that v-bits with three cutting edges work better than those with two but a lot of it is down to feed rates etc. With the materials I cut I find it easier to get into the sweet spot with thee cutting edges. Bear in mind that with a v-carve toolpath there are so many short segments and z-movement that the machine will not be physically capable of moving at higher rates so the actual rate may be far below the programmed one. That means that the RPM can often be far too high.

[scottp55]

Hi Stan,
WAS encountering somewhat similar problems, but to a lesser extant, as I went opposite of Adrian, and used half round 60 degree (.005"flat)Engraving bit from Onsrud(#37-01) as there is no spiral to grab wood, and because of tiny flat the nooks and crannies came virtually flat faster with less or no cleanup required.
With only 1 flute, I could crank my spindle close to or at max rpm(18K).

One thing that most often gave me better results was to reverse the toolpath order to cut the VCarve portion FIRST while it had support of the rest of the wood, THEN large tool for waste.
Lowering my Plunge speed until it sounded good and gave good results worked very well.

And in this Tree example.....Zeroing as normal, then moving my spindle up(say to Start Depth) and rezero'ing Z, and running the VCarve path, THEN lowering and re-zeroing to original Z-Zero,
worked nicely as well.

Haven't done one in 2 years, but may try a very small one with Fine details soon in a slice of Pin Cherry burl, and may order a 45 degree of the same bit, OR go directly to a 30degree Engraving,
so that fine details survive the inevitable sanding on the Tiny details.
Just mentioning;
scott

[Darryl Kerney]

Hi Stan,
WAS encountering somewhat similar problems, but to a lesser extant, as I went opposite of Adrian, and used half round 60 degree (.005"flat)Engraving bit from Onsrud(#37-01) as there is no spiral to grab wood, and because of tiny flat the nooks and crannies came virtually flat faster with less or no cleanup required.
With only 1 flute, I could crank my spindle close to or at max rpm(18K).

One thing that most often gave me better results was to reverse the toolpath order to cut the VCarve portion FIRST while it had support of the rest of the wood, THEN large tool for waste.
Lowering my Plunge speed until it sounded good and gave good results worked very well.

And in this Tree example.....Zeroing as normal, then moving my spindle up(say to Start Depth) and rezero'ing Z, and running the VCarve path, THEN lowering and re-zeroing to original Z-Zero,
worked nicely as well.

Haven't done one in 2 years, but may try a very small one with Fine details soon in a slice of Pin Cherry burl, and may order a 45 degree of the same bit, OR go directly to a 30degree Engraving,
so that fine details survive the inevitable sanding on the Tiny details.
Just mentioning;
scott

Hi scottp55 !
almost a year later but i found this thread while searching for opinions on using a 30deg bit for vcarve inlay.
running the vcarve before the clearance does seem like a good idea, we tried it on our 2nd attempt at this, won't know for sure till monday when we slice it...
but, the real issue for us is pass depth on the first pass going down to start depth + flat depth, so,
i like your idea of using 2 different Z zero points, that's an alternate way of doing what i was trying to figure today actually.
to prevent the too deep first pass because of the start + flat depth that is too much for some bits i think i've found a solution...
first calculate a pocket path on the male part to outer boundary equal to the start depth, then calculate the vcarve, with clearance tool if needed, with the start depth + flat depth, the pocket path will have taken it down to the start depth, then, calculate a quick engrave path only on the inlay design also down to the start depth, then run vcarve clearance path, then QE path, then vcarve path last.
so for example, with 1/4" bit, pocket path then the vcarve clearance path , then with a v-bit the QE path then vcarve part 2 path.
I HAVEN'T tried it yet but using the numbers i am it seems like it will work, i get the most amount of inlay material to work with trying a 30deg bit in simulation and 0.4" as the total depth, with the male part split 0.2' start + 0.2" flat depth.
it seems to me your re-zeroing is meant to achieve the same thing, so far i've been finding it to be a source of trouble, trying to get the z zero perfect with bit changes, so much to learn with all this but i am really enjoying it when nit works and not so much when is doesn't haha !

[mfirlott]

For myself...my journey to better success came with...

1) I now use a 30 degree v-bit with a 0.005" flat tip.

2) I found that doing inlays into cutting boards with face or edge grain had lots of breakage depending if the bit travelled with or across the wood grain. When I make end grain cutting boards I have much less breakage as all the grain is vertical. So much of my inlay work has now been into end grain.

3) As mentioned by Scott...for the male component...I do the v-carve first then the clearance. Lots of success with this as the thinner pieces have support.

4) I do manage the pass depths but I also do the male inlay in two separate toolpaths. My Female depth is 0.33" and I set the pass depth of the v-bit and clearance bits to 0.07". This means about 5 passes for the cutting of the female. My Male total depth (or height) is 0.30". The pass depths are set same as for the female at 0.07" BUT I run 2 toolpaths. The first toolpath is start depth = 0.0" with a flat depth of 0.15". The second toolpath is start depth = 0.15" with a flat depth = 0.15". This produces a total height for the male of 0.30" which fits into the female depth of 0.33".

5) After all of this I sometimes still saw a poor fit of the male into the female. No breakage but just a poor fit with air gaps. I noticed that in several cases it was my glue-up that was the culprit of the bad fit. The male inlay had air gaps but always only on one side of the board and that's when I realized that I was not applying even pressure when clamping all the sides. I've since purchased a cheap hydraulic press and now with #1 to #5 in play above, the even pressure provided by the press produces a very nice and tight fit with no air gaps.

[Tom M]

Thanks for the tips. When doing the male side, Do you run a clearing pass after the first Vcarve toolpath or do both Vcarve toolpaths then a clearing?

[PRO4824]

Well, I'm gonna have to bookmark this thread. Lots of good info.

[Aussie]

Hi Stan,
WAS encountering somewhat similar problems, but to a lesser extant, as I went opposite of Adrian, and used half round 60 degree (.005"flat)Engraving bit from Onsrud(#37-01) as there is no spiral to grab wood, and because of tiny flat the nooks and crannies came virtually flat faster with less or no cleanup required.
With only 1 flute, I could crank my spindle close to or at max rpm(18K).

One thing that most often gave me better results was to reverse the toolpath order to cut the VCarve portion FIRST while it had support of the rest of the wood, THEN large tool for waste.
Lowering my Plunge speed until it sounded good and gave good results worked very well.

And in this Tree example.....Zeroing as normal, then moving my spindle up(say to Start Depth) and rezero'ing Z, and running the VCarve path, THEN lowering and re-zeroing to original Z-Zero,
worked nicely as well.

Haven't done one in 2 years, but may try a very small one with Fine details soon in a slice of Pin Cherry burl, and may order a 45 degree of the same bit, OR go directly to a 30degree Engraving,
so that fine details survive the inevitable sanding on the Tiny details.
Just mentioning;
scott

Hi Scott,

That image would be great as a v carve resin fill.... always looking for a challenge... blending haven’t tried that yet....now on my to do list.
Ron

[Aussie]

My go to is a 30 deg 2 flute... no major issues for me with cutting the inlay.