A simple way to make inlays

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro
mmatarella
Posts: 15
Joined: Wed Jan 26, 2011 3:45 am

Re: A simple way to make inlays

Post by mmatarella »

A newbie playing catch up. :D

On the concern of the great depth cut on the male inlay in one pass, the .02 plus .02... Can I just zero out my z a bit higher than the actual material top, run the toolpath, then reset the z zero to the actual material surface and run it again? I just bought a Shark and it's a bit lighter duty than what many of you are using.

I did do a couple test inlays with the inlay toolpath in the V6 of V Carve already. But I see the advantges of greater detail in this method.

Thanks to all that came before me!
Mark

krtwood
Posts: 45
Joined: Wed Dec 16, 2009 9:38 pm

Re: A simple way to make inlays

Post by krtwood »

Finally had a chance to test this method out. Pretty amazing what it can do. Still experimenting on what values to use for small inlays in thin stock. I was testing out a couple sizes to see how small I could go with this graphic.
Attachments
inlay-after.jpg

MarkJohnston
Vectric Wizard
Posts: 820
Joined: Tue Jun 01, 2010 4:51 pm
Model of CNC Machine: CAMaster MC4848
Location: Prescott AZ

Re: A simple way to make inlays

Post by MarkJohnston »

That looks great, the detail is very clear. What size Vbits did you use?

I have been trying to get some pretty fine details but so far haven't achieved that fine of detail, plus when I sand it is sanding off the real fine detail even with the finest sand paper.

Thanks for posting, I have read everything on this post all 17 pages.

Mark

krtwood
Posts: 45
Joined: Wed Dec 16, 2009 9:38 pm

Re: A simple way to make inlays

Post by krtwood »

I used a 1/2" 60 degree 3 flute bit, and had my speeds really slow, I think 20 ipm. I did take pains when creating the vectors to try to eliminate sharp acute corners which I think is the biggest problem area. I have some other designs where I can't do that so I'll have to see how that goes. While I haven't done this technique before I have done v-carvings filled with inlace so I'm familiar with losing the fine areas when you sand it. I did end up running this through the drum sander a little more aggressively on the last pass than I intended and it still came out well though. I think it will help to seal the surface that gets the pocket before machining it so the glue doesn't soak into it. Then you only have to sand the inlay flush rather than deep enough to remove the glue in the surrounding area.

For this test the v-carve settings I used were just to cut the recommended settings in half (flat depth 0.15 on the female, start depth 0.1 and flat depth 0.1 on the male) but that results in cutting the male side a lot deeper than it needs to be on such a small piece. I plan to try start depth 0.1 and flat depth 0.5 next time. Some of the designs I'm doing need to be cut in some pretty hard woods like bloodwood so I want to minimize that cutting depth.

MarkJohnston
Vectric Wizard
Posts: 820
Joined: Tue Jun 01, 2010 4:51 pm
Model of CNC Machine: CAMaster MC4848
Location: Prescott AZ

Re: A simple way to make inlays

Post by MarkJohnston »

I need to try some more inlays. I also tried to smooth out some of the sharp angles on the designs by doing some node editing. I'm sure that my designs were way to aggressive for the inlay process but those were the ones I wanted. I will try a simpler design next time. I think that you are right about sealing the pocket before gluing the pieces, I will try that as well. I also ran the piece through the drum sander but I felt that was to aggressive.

Thanks for the additional advise.

Mark

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

Some of the really fine detail is lost because the woods themselves cannot be cut to such fine detail. They bend, shred and tear.

I wonder if the results could be improved by cutting the pocket 0.025" high, apply sanding sealer, let it dry while still on the machine and then cut the pocket to the final depth. Follow this with a similar approach to the inlay. The fine edges should be stronger and may cut cleaner. Super glue might work but it might also turn white when cut. Then again, the white might disappear with a coat of varnish.

Paul Z

PS Nice inlays!

krtwood
Posts: 45
Joined: Wed Dec 16, 2009 9:38 pm

Re: A simple way to make inlays

Post by krtwood »

The pocket isn't usually much of a problem, it's almost always the male side that has something break on small details that are across the grain. I have found that different woods work better than others. I was cutting a sun shape and in bubinga had failures twice, but the same machining worked fine in mahogany. Well at least it seems to, that one is complicated because there is a spear going through the sun so I had to first inlay the tip of the spear, then I'll do the sun, then the shaft of the spear. One of the more complicated ones I need to do even though the shapes are the simplest.

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

Check out Al's latest V Inlay work here:
http://www.vectric.com/forum/viewtopic.php?f=29&t=12211

User avatar
FixitMike
Vectric Wizard
Posts: 1652
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: A simple way to make inlays

Post by FixitMike »

A hint for those who want to use epoxy to glue in the inlay. If you heat the epoxy after mixing, it becomes quite liquid. I use a heat gun on low setting after spreading the epoxy on the wood. It just flows. Contrary to what one would expect, it doesn't cause it to set particularly faster.
Good judgement comes from experience.
Experience comes from bad judgement.

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

Thanks for the tip! I had no idea you could do that with epoxy. I just assumed it would set up quickly. I'm going to try it and I can think of a few other uses.

Thanks,

Paul Z

adamfritzsche
Posts: 3
Joined: Tue Jan 12, 2010 2:54 am

Re: A simple way to make inlays

Post by adamfritzsche »

I am inspired by how amazing some of these inlays look and am wanting to try my hand at it, but I have a few questions about how the final peice is finished. If I am using two different materials, each of which with their own stain/color, how is this tackled. Is the female portion prefished prior to even vcarving it? I would assume this would be the easiest way, but I am thinking that the prefinish could be damaged upon removal of the excess male portion. Any help in understanding the finishing techniques would be greatly appreciated.

User avatar
TimToo
Posts: 22
Joined: Sat Jul 16, 2011 11:37 pm
Model of CNC Machine: ShopBot

Re: A simple way to make inlays

Post by TimToo »

Paul & Damien,

Thanks for creating the great writeup and process!

I'm working through my first inlay now. I'm not smart enough to do something simple like the one-piece tree or the star shown in the examples. :lol: I'm starting with five woods being inlaid into a sixth wood. I've already figured out which pieces have to be done in what order (it's similar to creating embroidery designs which I do for my wife once in a while - have to consider what's "on top" of the other pieces so the end results looks right).

A little overlap between adjacent pieces should help me avoid misalignment problems. There's no reasonable way to do what I'm attempting without removing the pocket piece several times from the ShopBot table to slice off the excess bit that protrude after gluing in yet another inlay…

I'm hitting a bit of splintering, crumbling on fine details especially if there are multiple fine items in close proximity. So far, my 60 deg vbit cuts those cleaner than the 45 but I think my feed rate might need some slowing down as well.

For the male portions (the mirrored items that will be inlaid into the base material), it looks like I can minimize shredding of the fine details by artificially setting my z-origin 0.1 higher than it will ultimately be (essentially what mmatarella suggested but I figured it out on my own before seeing that post - d'oh). After cutting the full tool path, I move the bit to a clear area, drop it to -0.1 (absolute coords), and hit ZZ. I move Z up to 1 inch before cutting the same tool path a second time.

For one fragile wood I was working with (Vermillion I think), I bumped Z up 0.1 for the first pass, then down by .05 for a second pass, and then another .05 for a third pass.

I had significantly less tear out with that approach and my cut times are less than 5 minutes long, so repeating them once or twice is no big deal. I am hoping that as I dial in the proper feed rate, I can cut that to just two passes. I plan to trying raising it by only .05, cutting a little slower, then dropping it by that .05 and running the toolpath again.

I also figured out that if a piece has some tear out/splintering, there's enough slack in the process (using the defaults), that I can sneak in a cleanup pass by dropping Z .05 and rerunning my tool path (after having cut originally using the defaults in your document). My samples show there's an eighth of an inch of air gap below at the bottom of my inlay so there's enough room to be able to clean up some tear out by sneaking in an extra, very light, pass.

If I get my design to work, I plan to post a follow up of course.

Thanks again!

Tim S.

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

Tim,

Someone suggested using thin super glue to reinforce the wood before each cut. I haven't tried it but it seems like it would help a lot.

Before applying a finish, look across the surface of piece and see if a final coat of glue across the entire piece is needed to keep a consistant surface texture.

Paul Z

User avatar
TimToo
Posts: 22
Joined: Sat Jul 16, 2011 11:37 pm
Model of CNC Machine: ShopBot

Re: A simple way to make inlays

Post by TimToo »

Paul,

Thanks for the tip. I'll add it to the list of things I'll be trying this weekend. :lol:

I just finished a major edit of the original drawing to fix a number of problems I uncovered late Friday as I was working through the layers.

I need to get the inlays to sit deeper. I know how, I just need to adjust my work flow to make that happen. Along the way, I'll hopefully find at least one way to minimize the splitting (I'm pretty sure I can get past that with the info here and with what I've been tweaking as I go).

Not having a thickness sander makes cleaning up between wood changes a bigger time sink than it should be…the random orbit sander takes too long and tends to affect the piece I'm inlaying everything into (not a surprise given the sander is hand held).

I did try a thickness planer after having enough other problems that a bit of tear out really wouldn't matter. Naturally, it was going just fine until the very last (and fairly fine) pass. Though I suspect that bit of tearout was in part due to my inlays not going deep enough (and thus not having enough grip to survive the planer's evil influence).

The piece I'm working on is about the size of a sheet of standard paper, so getting good clamping pressure during glue up has been a problem. I need a better press (cauls and clamps just aren't cutting it). A pile of bricks just seems like the wrong way to beat that problem into submission but I might resort to it until I can cobble up something better.

Some of the problems I hit late Friday were my own fault. I had too much overlap between adjacent pieces being inlaid. Since they weren't going in very deep, they were easy to dislodge while v-carving for the adjacent/overlapping material. That's one of the things I fixed in the drawing tonight.

I was hurrying and used CA glue to hold pieces in…it's a proof of concept so it's not that important. I'll likely switch to polyurethane glue for the next attempt and see if that works better for me.

I definitely need to seal the background piece before cutting and gluing. That will prevent several problems I hit today. Sanding a big piece of inlaid walnut left dark brown, very fine, sanding dust embedded in the background material. Later, it all turned red when I sanded the inlaid vermillion flush. Sealing the pores in the background piece would've been smart (fortunately, this is just an experiment so my background isn't important right now - perfect place to make these mistakes and learn what else I should've seen coming).

It's been a very interesting challenge to try making it work for something fairly complex.

Tim S.

User avatar
TimToo
Posts: 22
Joined: Sat Jul 16, 2011 11:37 pm
Model of CNC Machine: ShopBot

Re: A simple way to make inlays

Post by TimToo »

Superglue didn't help…even when I was only cutting .025 deep (might've been .05 but either way, it was a light cut and still shredded).

I've made more changes to my drawing based on a bunch of trial and error. Heading back to the shop in a little while in hopes of finally getting it to work without splitting. If it doesn't work, I should be VERY close to having it sorted out…

Post Reply