A simple way to make inlays

Post by **MZiegler** » Fri Dec 08, 2006 1:30 pm

Paul, thanks for sharing. This method could also can be machined with an end mill. While you would lose the advantage of having sharp corners, you still gain advantage with having all the items of the design layout, machined, aligned and glued at the same time. I was think of using this procedure for lettering. The advantage it would eliminate the trouble aligning and spacing all the individual letters. Mark

Post by **Paul Z** » Sat Dec 09, 2006 4:47 pm

Mark,

Great idea about lettering!

Since the inlay will have vertical sides and as little gap as possible, the alignment will have to be "spot on". If making the inlay releases stress in the material, it may shift the alignment enough to make installing the inlay difficult. If that happens, cut the strip of letters in half until they do fit.

Please show us your results (along with bit sizes and cut speeds).

Paul Z

Post by **MZiegler** » Sun Dec 10, 2006 1:29 pm

Paul, you got me! I have not made any lettering like this yet. Just thinking out loud. I was thinking that by cutting the lettering from the backside with a skin on it, it would be easy to glue it to another piece. Then you could sand or mill the skin off. I was thinking to do this without the pocket, so technically this would not be an inlay. Awhile ago I was try to make name plates and clock faces with raised lettering and was have lots of trouble in aligning and spacing the individual letters. You could rout pockets for the letterings and that would end that problem, but making pockets create new problems. So why not rout the letters as an unit and then glued them as unit too. On this clock face below the numbers were manually spaced and aligned and looks like it. The numbers on this clock was done by resawing. Maybe by doing the letters as a unit would be better. Mark

Post by **dmidkiff** » Sun Dec 10, 2006 2:35 pm

Tony and Maynard,

Thanks for the info, it worked like a charm.

Dave

Post by **MZiegler** » Wed Dec 13, 2006 11:35 pm

Thinking out loud here. Paul’s inlay method also might work for intarsia projects too. By repeat milling off, routing new pockets and gluing on new layers it would be 3D like an intarsia. The wood grain would run the same direction on each layer. I have not done or work out the details on this yet, just throwing the idea out there. Mark

Post by **Paul Z** » Fri Dec 15, 2006 1:26 pm

Mark,

One of the reasons for experimenting with very fast setting glues was to be able to do exactly as you describe but without having to wait a day for each step. I have experimented with super glue and accelerant (sp?) but there are issues. I'm going to try construction adhesive as well. Anyone else have a "sticky" idea?

Paul Z

Post by **Dave_W** » Sat Dec 23, 2006 4:39 pm

I seem to be having problems with the inlay settings described in the pdf. I'm running the demo so I haven't cut this out yet, but it seems like the inlay will bottom out before the sides contact each other.
I must be doing something wrong, but I can't figure out what it is.

Dave

Post by **Paul_n** » Sat Dec 23, 2006 4:50 pm

Dave.....

I have run into the same problem...

I think the answer is to use a larger diameter "V" bit.... but, I have not
tested as yet....

Let me know if that works for you....

Paul

Post by **Tony Mac** » Sat Dec 23, 2006 5:03 pm

Hello Dave,

Good to see you on the Forum.

The guys who have been working on this project (Paul Z, Paul N and Damian) have
recently spotted issue.

What you are seeing is the cutter not being large enough to machine to the required
depth, which leaves vertical walls that would be removed by a larger diameter cutter.

Using this approach the cutter must be large enough to machine to the Flat Depth + Start Depth

The image below tries to show what I mean with the Red triangle representing a small
cutter and the yellow showing how a larger cuter will remove move material.

I hope this makes sense and helps?

Tony

Post by **Dave_W** » Sat Dec 23, 2006 5:36 pm

Thanks for the quick reply. Could I get the same result by skimming the verticle walls down with an endmill pass? I'm not sure the laminate trimmer on my homemade CNC machine can handle a large bit.

Thanks,
Dave

Post by **dman** » Sat Dec 23, 2006 6:50 pm

Dave,
I'm not sure how deep you need the inlay to be but from looking at your image post the start depth of .2" seems a little too much. I generally make my inlays .2" deep for the pocket then set the start depth of .05" and cut depth of .2". This allows for the inlay to fit down inside the pocket and not reach the bottom of the pocket. Filling with glue to fill the void and allowing it to sit overnight to dry is critical to the process also. If you like, post the crv file and I will set it up and post the way I cut it out so you can see the settings.

Damian

Post by **Paul Z** » Sat Dec 23, 2006 7:25 pm

Guys,

I apologize for not being able to spend time on this, but I'm flat out until Monday.

Paul Z

Post by **Dave_W** » Sat Dec 23, 2006 8:10 pm

dman,

Here's a crv for the pocket and inlay. I'd like to be sure it works before I pull the trigger on the full version. I'm running the demo and can't cut the file. I'll see if I can tweak one of the included files to try it out. I'm planning on picking a .5" V-bit while doing some last minute shopping.
Thanks in advance for checking it out. Merry Christmas!

Dave

Post by **dman** » Sun Dec 24, 2006 7:43 am

Dave,
Since you have the trial version I am unable to open your crv files. I am going to post a crv of mine in hopes that you can open it. I will try to explain what I have done here.
1. For the pocket cut, I used a 1/2" 90 degree cutter with a flat depth of .2". I also used a 1/8" endmill to clear out the flat area in the bottom of the pocket. (You really don't need to use the endmill. It just makes the pocket cutting quicker).
2. For the inlay, I use the same 1/2" 90 degree cutter with a Start Depth of .05" and a Cut Depth of .2". This cut is made using the Profile Toolpath option not the Vcarve Toolpath. I believe both work the same I just prefer the Profile Toolpath. Usually the inlay material I use is .25" thick so the cutter will cut through the material when finished. I use double sided tape to hold the inlay material to the spoil board so the inlay when cut through will stay in place.

Once both are cut the inlay should sit down into the pocket but not bottom out. I fill the pocket area really well with glue and make sure all contacting surfaces of both the inlay and pocket get glue. I then clamp and let it sit flat overnight. The inlay won't look very pretty at this point. The inlay will be sitting above the intended board 1/8" or so. The next day, I put the piece back on the machine and mill down the inlay with a 3/4" cutter so it is very close the material I put it in to. This should be done in small increments (1/16" at a time) to avoid chipout. Once I have it close, I will just sand until it is perfect. This method seems to work well for me. It's late and I'm tired so if this doesn't make sense pleas ask and I will try to help however I can.

Damian

Post by **Paul Z** » Mon Dec 25, 2006 6:28 pm

A first look at the "W" problem seems to indicate that it may be a problem with the bit size. A "small" bit makes the problem show up and a "large" bit seems to make the problem go away. Since I have only done these inlays with large bits, that may be the reason that I didn't find the problem.

If one makes the inlay and pocket so that the thickness of the inlay (start depth + flat depth) is less than the cutting height (NOT width) of the bit in use, the process seems to work.

I'd appreciate if those who had problems would try thinner inlays to see if this gets rid of the problem (or send me your files and I'll try to check them). I can not read demo version files.

Paul Z

PS I think this may be why Damian's test case works and would like to hear his thoughts. He has the best set of inlays that I have seen using this method.