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

Re: A simple way to make inlays

Postby llwood » Thu Jun 19, 2014 4:26 pm

BrianM wrote:This is because you have told the software that the second toolpath starts at Z -0.19 so the 2d preview shows what the toolpath would machine assuming that the material is starting at Z -0.19.

This is the intended behavior as many jobs involve pocketing out an area and then machining in the base of the pocketed area. If you imagine v-carving text in the base of a pocket, showing the outline of the v-carving at the surface level would be completely useless.


Brian, this makes sense. Thanks for your explanation and helping me to understand that this is intended behavior.

--Andy
User avatar
llwood
Vectric Wizard
 
Posts: 385
Joined: Sun Nov 18, 2012 5:07 pm
Location: Dillsburg, PA
Model of CNC Machine: Legacy Maverick

Re: A simple way to make inlays

Postby llwood » Sun Jul 06, 2014 4:52 am

I read the document "VCarve Inlay Description and Procedure" by Paul Zank and Damien Durrant. I first want to say thank you for producing this description that has helped so many, including me, understand how to do this. There is also a lot of good discussion on this thread, and I've read it all. Now that we have some experience with an inlay project, I still have a question.

The document suggests the following depths as a starting point:
Inlay Flat Depth = 0.2”
Inlay Start Depth = 0.1”
Inlay Pocket Flat Depth = 0.3”

According to my calculations, using an inlay start depth of 0.1" means that the smallest part of the inlay would be sized 0.115" larger than the pocket. This means that if a part of the inlay art work is smaller than 0.115" across (almost an eight of an inch), the inlay won't fit in the pocket. We wanted to do a project where some of the of the inlay regions were only 0.05" across, and when we used those dimensions, the 2 pieces wouldn't fit together. By trial and error, I found that using:
Inlay Flat Depth = 0.04”
Inlay Start Depth = 0.16”
Inlay Pocket Flat Depth = 0.2”
worked to have the pieces fit together and retain the small lines. In this case, the 2 pieces fit almost completely tight together. I just posted the pictures of this project on the gallery at the following link. Some of the outline lines are very thin, and these settings seem to work to have them all show up.
viewtopic.php?f=5&t=20152

But some of the pictures in this thread, particularly those of trees, are also very intricate. Some of the trees have very narrow branches. Did you use an inlay flat and start depth of 0.2 and 0.1", respectively, or did you also adjust those values? Of course the dimensions mentioned in the document are just a starting point which will need to be customized for each project, but it would be great to have a discussion of how to set these values for different projects. We sure junked a lot of wood in the process.

Thanks,
--Andy
User avatar
llwood
Vectric Wizard
 
Posts: 385
Joined: Sun Nov 18, 2012 5:07 pm
Location: Dillsburg, PA
Model of CNC Machine: Legacy Maverick

Re: A simple way to make inlays

Postby kaetamer » Tue Jul 08, 2014 4:05 pm

Don't you mean Start Depth of .04 and Flat Depth of .16?
kaetamer
Vectric Apprentice
 
Posts: 28
Joined: Mon May 12, 2014 3:10 pm
Model of CNC Machine: CNCRP Pro 4824

Re: A simple way to make inlays

Postby llwood » Tue Jul 08, 2014 6:42 pm

Yoga block inlay settings screen capture.jpg
No, actually I did mean Start depth of 0.16 and Flat depth of 0.04 (see screen capture), and I remember having some reasoning for these values when I came up with them, but to be honest, I don't remember what it was at this point. All I know is that it works, meaning the inlay fits and gives the results I was looking for after finishing.

--Andy
User avatar
llwood
Vectric Wizard
 
Posts: 385
Joined: Sun Nov 18, 2012 5:07 pm
Location: Dillsburg, PA
Model of CNC Machine: Legacy Maverick

Re: A simple way to make inlays

Postby kaetamer » Tue Jul 08, 2014 10:53 pm

Right, I stand corrected.

I previewed each iteration of start and flat depths reversed and it does seem to make a difference. Perhaps someone could chime in on the mechanics of start and flat depth and whether there are rules regarding start and flat depths as a function of inlay width/depth.

I too have wasted a good deal of maple and walnut trying to get tight fitment; I can get close but my results seem to vary randomly.

Help?
kaetamer
Vectric Apprentice
 
Posts: 28
Joined: Mon May 12, 2014 3:10 pm
Model of CNC Machine: CNCRP Pro 4824

Re: A simple way to make inlays

Postby llwood » Wed Jul 09, 2014 6:49 am

Inlay schematic.jpg
After some thought, I remember how I arrived at those values for Inlay Start Depth and Flat Depth. I drew up a schematic to illustrate it. I created the schematic in VCarve Pro, so I attached both a jpg file of a screen capture and well as the .vcp.

I first wanted to see what would cause the inlay and picket to fit together perfectly, with no glue gap. It turns out that if the Inlay Start Depth is the same as the Pocket Flat Depth, the pieces will fit together perfectly. Reducing the Inlay Start Depth and having an Inlay Flat Depth will make the inlay piece larger, thereby forming a glue gap. I kept it so that the Inlay Start Depth plus the Inlay Flat Depth equals the Pocket Flat Depth, but I don't know if this is necessary. In this case, the glue gap is the same as the Inlay Flat Depth. If you are using a 60 degree vbit, the inlay will be larger than the pocket by an amount that is 1.155 times the Inlay Flat Depth (0.577 times it on each side). If the thinnest segment of the artwork is not 1.155 times the Inlay Flat Depth in width, then the pieces won't fit together properly.

For example, if the Inlay Flat Depth is 0.04, the thinnest part of the inlay artwork should be 0.0462, but I'll round this up to 0.05. If you don't have very thin lines in the artwork, you can use a larger Inlay Flat Depth.

This has worked pretty consistently for us.

--Andy
Attachments
Inlay Schematic.crv
(575.5 KiB) Downloaded 310 times
User avatar
llwood
Vectric Wizard
 
Posts: 385
Joined: Sun Nov 18, 2012 5:07 pm
Location: Dillsburg, PA
Model of CNC Machine: Legacy Maverick

Re: A simple way to make inlays

Postby FixitMike » Wed Jul 09, 2014 6:57 am

For the female part:
The flat depth controls the maximum depth that the V-bit will cut. The deeper it is, the thicker the male inlay should be. .150" has worked for me. If the inlay has wide places, a deeper depth could be used. For narrow lines, the V-bit will only cut deep enough so the cut is the width of the line, regardless of what the flat depth is.
The start depth is usually set to zero, or a small value (like .005") if you think you are going to end up sanding off some of the surface of the part.

For the male part:
The flat depth sets the size of the empty space between the two pieces after they are glued together. I use .125". If there are narrow spaces between the parts of the of the inlay, the actual space may be less at that location.
The start depth controls how far the male part will stick into the female part. It has to be less than the flat depth of the female part. The difference has to be enough to allow for the ridges that remain when the V-bit cuts the flats in the female part plus just enough for excess glue. I use a .030" difference. i.e. .120" for a female flat depth of .150".

Some hints that you may find helpful.
Sand off the tips of the sharp high spots in the male part so it can go all the way into the female part, except don't sand the areas that will be fine lines in the finished parts.
Clean out the bottoms of V lines in the female parts with a sharp tool I use a dental pick.
Be very sure that the V-bit angle is correct.
Good judgement comes from experience.
Experience comes from bad judgement.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1531
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (extensively modified)

Re: A simple way to make inlays

Postby llwood » Fri Jul 11, 2014 12:16 am

Inlay schematic2.jpg
In an earlier post, I said "If the thinnest segment of the artwork is not 1.155 times the Inlay Flat Depth in width, then the pieces won't fit together properly." I'm now certain this is WRONG! I put together another schematic (attached) this one diagramming how narrow segments in the artwork are handled. It doesn't appear that any amount of narrowness in the artwork will cause the pieces to not fit together, but the narrower the artwork, the more likely the segment will be removed while cutting/sanding away the backing.

I'm certainly not always right, but I can admit my mistakes!
--Andy
Attachments
Inlay Schematic2.crv
(697 KiB) Downloaded 305 times
User avatar
llwood
Vectric Wizard
 
Posts: 385
Joined: Sun Nov 18, 2012 5:07 pm
Location: Dillsburg, PA
Model of CNC Machine: Legacy Maverick

Re: A simple way to make inlays

Postby Paul Z » Wed Mar 25, 2015 6:54 pm

This is a link to a beautiful, very large V Inlay project elsewhere in the forum. viewtopic.php?f=29&t=22080
Paul Z
Vectric Wizard
 
Posts: 516
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Re: A simple way to make inlays

Postby Paul Z » Sat Jul 04, 2015 5:57 pm

Here's a link to the use of 30 degree bits used for V Inlays.

viewtopic.php?f=28&t=22774
Paul Z
Vectric Wizard
 
Posts: 516
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Can't Figure This One Out

Postby Greg J » Mon Mar 21, 2016 1:12 am

I've made beautiful inlays in the past with the V-bit method. Works wonderful!!!

Now I'm trying to make an end grain cutting block with inlay and having all kinds of problems. Everything I try leaves gaps between the base material and the inlay material.


the bit is a Amana Tools 45 degree V-bit, 1/2" shank. It actually measured 52.1 degrees. Still have gaps.

Attached are the 3 V-Carve files. I separated into 3 files to reduce file size.
Elk Inlay 1 has a start depth of 0.100" and a Flat Depth of 0.001". There is a clearing tool path using a 1/4" end mill.
Elk Inlay 2 has a start depth of 0.200" and a flat Depth of 0.001".
Elk Inlay 3 has a start depth of 0.200" and a flat Depth of 0.100".
In my file I safe all 3 files together to make one 1/4" End Mill file and one 52.1 Degree V-bit file.

I didn't include the Pocket file (female part) since that is just a Flat Depth of 0.300".

Any help/suggestions are greatly appreciated. I'm making this cutting block for a fund raiser and I don't want to disappoint this very cool lady who I said I'd would make this for.
Attachments
Elk Inlay.png
Vectric Form Elk 1.crv
(1.13 MiB) Downloaded 190 times
Vectric Form Elk 2.crv
(1.11 MiB) Downloaded 200 times
Vectric Form Elk 3.crv
(1.09 MiB) Downloaded 185 times
Greg J
 
Posts: 8
Joined: Sun Nov 21, 2010 4:24 pm
Location: New Mexico, USA
Model of CNC Machine: MechMate #13 -It's a workhorse, LOVE IT!

Re: A simple way to make inlays

Postby Mobius » Wed Mar 23, 2016 1:54 am

I didn't look at the files, but as you have said you were successful before I imagine they are fine. What it looks like to me is the male piece of wood is moving as it is being cut, changing the shape slightly.
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Mobius
Vectric Wizard
 
Posts: 401
Joined: Wed Jul 09, 2014 1:19 am
Location: Drumheller, Alberta, Canada
Model of CNC Machine: CRP Pro 4848 Custom Build

Re: A simple way to make inlays

Postby Greg J » Wed Mar 23, 2016 4:43 am

Thanks for the help Mobius,

I tried changing the V-bit angle from 52.1 to 46 degrees. Made a straight line cut for about 2 inches with the bit. Made a 90 degree cut to the straight line cut and physically measured the angle with a protractor. Closer to 46 degrees than 52. Anyways, made another inlay last night and glued up. Tonight I surfaced off the top and still major gaps.

It's really looking like the female pocket is too deep or the male inlay is too shallow.

tomorrow night I will make another inlay, wait 24 hours for glue to set (the hardest part :) ) and see what the results are.

It was so easy before. Don't know why all the troubles this go around. Oh well, I bet I learn something. Hate it when that happens :D
Greg J
 
Posts: 8
Joined: Sun Nov 21, 2010 4:24 pm
Location: New Mexico, USA
Model of CNC Machine: MechMate #13 -It's a workhorse, LOVE IT!

Re: A simple way to make inlays

Postby scottp55 » Wed Mar 23, 2016 12:36 pm

Just me, but if the female was .3, then for the male I would have a start depth of .15" and a flat depth of .15" like in the hummingbird tutorial.
And only 1 file for the male.
scott
scott
User avatar
scottp55
Vectric Wizard
 
Posts: 3007
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP9.5

Re: A simple way to make inlays

Postby Greg J » Wed Mar 23, 2016 1:15 pm

Thanks scottp55,

I uploaded 3 files here due to size constraints (can only upload 2Megs, etc). It's the vectors that make it so large. I only have one cut file for the male part.

I agree with what your saying and that's what the next test will be. Female will be .300" and Male will be .150" start and .150" flat.

Since its for a cutting block, I was trying to make the inlay as thick as possible.

Dang day job is getting in the way. Think I'll take a vacation day tomorrow and work on this. Much more fun, rewarding, relaxing, good for the head. Ah, but I'm not telling you people anything :D
Greg J
 
Posts: 8
Joined: Sun Nov 21, 2010 4:24 pm
Location: New Mexico, USA
Model of CNC Machine: MechMate #13 -It's a workhorse, LOVE IT!

PreviousNext

Return to VCarve - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 6 guests