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

A simple way to make inlays

Postby Paul Z » Wed Sep 06, 2006 8:57 pm

For full details on how to design and machine V-Inlays read the attached PDF document.

The steps listed below were Paul's original thoughts on a generic procedure for cutting
inlays, but he later found they are not always correct.

**********************************************************************************

I have wanted to make some inlays with my shopbot but there were two issues:
1. the artwork has to be revised to accommodate the bit size and that would require a fair amount of CAD work for each inlay
2. the resulting inlay would have rounded edges.

I remembered that people who do intarsia will often angle their blade and rotate the piece as they cut to make up for the thickness of the blade. The resulting pieces fit perfectly even though they fit on a bevel. Could one achieve a similar effect using v bits?

It came to me that I might already have the necessary tools, both hardware and software (V Carve). Here is the process that I used:

1. This test was done with a 90 degree bit (‘cuz that’s what was in the router and I was too lazy to change it. A 60 degree bit might have produced better results.)
2. Pick a graphic. I used inkscape (free on the web) to generate an outline of the graphic. (One could also start from a DXF file or even make the design in V Carve.)
3. Start V Carve and import the path file.
4. Check for open or duplicate vectors and correct them if necessary.
5. Copy the path; paste it; and, using the mirror function, flip it horizontally.
6. Move it to the right to get it away from the original path.

(Top figure)

7. Now decide how deep you want the inlay to be. Keep it relatively deep to make the inlay piece less fragile. For this example, let’s use 0.2 inches.
8. Create a V Carve tool path with the original path (the one on the left) using a flat depth of 0.2 inches. This will be used to create the pocket for the inlay.
9. Now create profile tool path 0.2 inch deep on the flipped path (the one on the right) using the Machine Vectors “ON” option and no tabs. This will be used to create the inlay itself.

(Middle Figure)

10. Cut the pocket into your base material.
11. Cut the inlay into material that is thicker than the cut depth.
12. Sand the back of the inlay until the inlay falls away from the rest of the material.
13. Glue inlay into the pocket.

Here are the pocket and the inlay and below that is the inlay in the pocket.

(Bottom Figure)

The inlay rides a little high because I haven’t cleaned off some “fuzzies” from the cutting. When I press the inlay down, it fits almost perfectly.

I am working on a slight modification to the process of cutting the inlay to make it thicker than the pocket. This would allow cutting the inlay with tabs and eliminate the process of sanding until the part becomes free. The inlay will be higher than the pocket when installed but it can then be sanded flush.

The result of this method is that graphics (many? most?) can be used without alteration and that the inlay can have sharp points. I hope some of you find this useful and please let us see anything you might create.



Paul Z
Attachments
pocket and inlay.jpg
two paths formatted.JPG
two paths.JPG
inlay layout.jpg
Bird.jpg
VCarve_Inlay_Description_and_Procedure.pdf
PDF document describing the V-Inlay procedure
(1.09 MiB) Downloaded 7916 times
Paul Z
Vectric Wizard
 
Posts: 503
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Postby dighsx » Wed Sep 06, 2006 9:19 pm

Very cool Paul! I've played around with this a bit and have found that when cutting the pocket toolpath if you zero the cutter just a hair above the piece you get a tighter fit.

Again great job and thanks for sharing your method. This really makes inlays a lot easier do. And quicker too!
Take it easy.
Jay (www.cncjay.com)
User avatar
dighsx
Vectric Wizard
 
Posts: 941
Joined: Tue Nov 01, 2005 12:36 am
Location: Royal Oak, Michigan USA

Postby CRFultz » Thu Sep 07, 2006 10:08 am

Nice work Paul!....I'll give it a shot.
Have you tried cutting your inlay piece from the back?
I use a 30 degree v bit and cut the inlay that has been flipped upside down.
For thin veneer type inlays it seems to work ok.
For scroll saw inlays I tilt apx 3 degrees per 1/2" and tape the the pieces together and try to keep the piece cutting with the angle facing inward the top will fall into the bottom.
That is where i thought of getting the angles needed for the machine to cut out.
Anyway your ideal sounds like it would be easier, I'll try it on my next inlay project, thanks!

Chuck
CRFultz
Vectric Wizard
 
Posts: 1150
Joined: Tue Mar 28, 2006 4:21 pm
Location: Longview, Texas

Postby Paul Z » Sat Sep 09, 2006 3:46 pm

I forgot to mention that since one uses "normal" size bits, the cutting speeds are much faster than when one uses small bits. In this test case I used a 1 1/4" V bit and an 1/4" end mill. Both were run at 1.5"/sec. With a 40% overlap the end mill cut the bottom of the pocket very quickly. Had the pocket been smaller, I would have just used the V bit with a 1/32" step over.

Paul Z
Paul Z
Vectric Wizard
 
Posts: 503
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Postby Paul Z » Fri Sep 22, 2006 4:21 pm

Here are the modifications of the previously posted procedure. The modified procedure insures a better fit of inlay to pocket by accommodating the inevitable inaccuracies caused by both the machine and the materials.

Note that the inlay is upside down in the diagram as compared to when it is cut. Also note that all cut depths are measured from the top of the materials.

Both the pocket and the inlay are V Carved. The flat pocket depth should be a little deeper than the inlay start depth to make sure that the angled sides contact before the flat portions of the pocket and inlay contact. The inlay flat depth provides that extra margin should the pocket be a little larger than intended or the inlay be a little smaller than intended.

If the overall project is complex, one could cut matching numbers in the inlay and pockets to identify what part goes where.

By the way, I have cut all of the pockets for a project at one time and then cut all of the petals of a flower as a single inlay. This does make the wood grain go in just one direction; however, it can speed up the process quite a bit.
Paul Z
Vectric Wizard
 
Posts: 503
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

A fish inlay

Postby Paul Z » Mon Sep 25, 2006 11:49 am

Here is a fish inlay using the modified procedure. The edges meet almost perfectly.
Paul Z
Vectric Wizard
 
Posts: 503
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Postby CRFultz » Mon Sep 25, 2006 1:00 pm

Paul, you have that inlay procedure nailed....excellent work..!! :D

Chuck
CRFultz
Vectric Wizard
 
Posts: 1150
Joined: Tue Mar 28, 2006 4:21 pm
Location: Longview, Texas

Postby dman » Mon Sep 25, 2006 10:28 pm

Hi Paul,
First off I'd like to say what a great way to make inlays you have come up with. I do have several questions though. If you make a pocket and vcarve of .2", do you make the inlay piece by using profile machine vectors "on" or "outside"? I tried several with the "on" approach with a starting depth of .18" and the inlay fit loose. When I did it with it on the "outside" I get the results like your modified procedure shows. The inlay is higher up and contacts the sides before fitting all the way into the pocket. I haven't got to sand the piece as I had to leave for work before the glue set so I will know better tomorrow. Just wondering if I did something wrong. Thanks again for showing this very useful way to use vcarve.
Damian
User avatar
dman
Vectric Craftsman
 
Posts: 180
Joined: Wed Mar 01, 2006 6:52 am
Location: Weirton,WV USA

Postby dman » Tue Sep 26, 2006 6:06 am

OK, I couldn't wait till morning to see the results. :D From what I can see, other than a small chip at the lower right on the "A" inlay it fits perfect. I am going to test it on a few other things to get the procedure down but it looks like it works very well. Thanks again Paul for showing me the way!
Damian
Attachments
Router 186.jpg
User avatar
dman
Vectric Craftsman
 
Posts: 180
Joined: Wed Mar 01, 2006 6:52 am
Location: Weirton,WV USA

Postby Paul Z » Tue Sep 26, 2006 2:17 pm

Glad to hear (and see) that you were able to use the inlay method. The modification of the original method means that both the pocket and the inlay are V Carved without any offsets. Note that a profile cut is the same as a v carve with a start depth of zero. The only problem using the profile cut is that it doesn't leave any margin for machine or material errors.

I also broke off a piece of the fish inlay (the tip of the dorsal fin) because I didn't wait for the glue to dry.

Do you have any ideas what this method should be named?
Paul Z
Vectric Wizard
 
Posts: 503
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Postby Paul Z » Wed Sep 27, 2006 12:20 pm

I ran a simple test and proved to myself that my last post was in error. The profile with a start depth of zero does NOT produce the same cut as a v carve. I think both parts MUST be V Carved. This MAY account for dmans issue with a sharp inside corner. The fish inlay has many sharp inside corners and they all seemed to work. I'll run some more tests when I get time.

Very sorry for the bad info.

Paul Z
Paul Z
Vectric Wizard
 
Posts: 503
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Postby dman » Wed Sep 27, 2006 5:18 pm

I also deleted my last post as I was not able to repeat the process. :(

However, in the below example, I have tried yet another method that is similar to Paul's and had some great results. Before posting the method I am going to try it on several other shapes and see if it can be repeated. I think this method is close. This inlay came out about as perfect as I think they can with some very sharp clean edges and a beautiful fit overall. The colored MDF from Great Lakes makes it look very nice as well.

Damian
Attachments
Router 189.jpg
User avatar
dman
Vectric Craftsman
 
Posts: 180
Joined: Wed Mar 01, 2006 6:52 am
Location: Weirton,WV USA

Postby MZiegler » Thu Sep 28, 2006 5:03 am

I ran a simple test and proved to myself that my last post was in error. The profile with a start depth of zero does NOT produce the same cut as a v carve. I think both parts MUST be V Carved. This MAY account for dmans issue with a sharp inside corner.

Paul, both the pocket and the inlay do not need to be v carved. The inlay can be cut by the 2D profile toolpath with the sharp internal corners (3d) option selected. Mark
MZiegler
Vectric Apprentice
 
Posts: 51
Joined: Mon Feb 20, 2006 3:06 pm

Postby dman » Thu Sep 28, 2006 7:14 am

OK here's how I made these inlays.

I have the original picture/text vectors I want to inlay. Use the standard vcarve toolpath with a flat depth of .08" - I used a 60 deg vbit and a .125 endmill for this. This is the pocket cut that the inlay will fit into.

Now I make a mirror copy of the original vector and do not resize or offset it in any way.
I then select the profile toolpath and use a 60 deg vbit. I choose to follow the vectors on an "outside" toolpath with a start depth of .04" and cut depth of .2" (I am using .25" material for the inlay). By selecting the "outside" toolpath the options of sharp outside and inside corners is available. I have both checked. Once this is cut, I sand or use a knife to release the inlay from the waste material.

Now the inlay when flipped over into the pocket will fit down into the pocket but not bottom out on the flat depth until after all the sides of the inlay contact the sides of the pocket and I have sharp corners where I need them. When glued and clamped it gives a very tight fit.

Since I used .25" material, I have a good bit sticking up above the pocket. I just put the piece back on the router and used .75" router bit to level the inlay so it is very close to the pocket material and then sand it until it is flush.

I think what happens with this method is that since the start depth on the profile toolpath is .04" it gives a slight offset to the inlay and allows it to sit down inside the pocket. The inside corners on the inlay end up not being sharp for the first .04" but this in on the bottom when assembled so it is not seen. So far on the two I have tried it has worked very well and is easy to setup.

Damian
Attachments
Router 193.jpg
User avatar
dman
Vectric Craftsman
 
Posts: 180
Joined: Wed Mar 01, 2006 6:52 am
Location: Weirton,WV USA

Postby Wemme » Thu Sep 28, 2006 10:00 am

Wow These inlays look Great!
any one mind posting the crv files for testing?
Cheers
Bart
User avatar
Wemme
Vectric Wizard
 
Posts: 506
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Next

Return to VCarve - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 5 guests