Official Luthiers Forum!
http://w-ww.luthiersforum.com/forum/

First pearl cut on CNC
http://w-ww.luthiersforum.com/forum/viewtopic.php?f=10101&t=56632		 Page 1 of 1
Author:  doncaparker [ Sun Jun 09, 2024 8:39 pm ]
Post subject:  First pearl cut on CNC
So, I pulled the trigger a few weeks ago on a used CNC router: A Stepcraft D840 (version 2) that I got for a pretty good price. It's not the best CNC machine, but it's not the worst, either, and it is a great fit for my available shop space and the relatively modest things I want to accomplish with it. I've been learning how to use it, mainly from the excellent Bob Mizek course available from Robbie O'Brien. The price of the course felt a bit steep before I pulled the trigger; it no longer feels expensive at all, compared to the putzing around I would have done without the guidance it provides. OLF mainstay Brad Combs has also been a wonderful resource (many, many thanks to Brad).

Other than the test projects I am cutting as part of the Bob Mizek course, today I was able to cut my first "real" test of something I intend to use on instruments. Check out the fit of this pearl inlay I plan to install on a batch of ukulele headstocks I am making for a "no experience necessary" building class I am leading in September at a religious retreat:

Attachment:
First pearl using CNC.jpg


Modest by the standards of many, but I feel great about not having to cut 10-12 of these suckers by hand!

I look forward to seeing what other drudgery I can avoid with this machine.
Author:  meddlingfool [ Sun Jun 09, 2024 9:13 pm ]
Post subject:  Re: First pearl cut on CNC
That’s what they’re for alright!
Author:  Marcus [ Sun Jun 09, 2024 9:23 pm ]
Post subject:  Re: First pearl cut on CNC
Well done. This machine will pay itself off in spades. Keep working at it, there is a lot to learn!
Author:  J De Rocher [ Sun Jun 09, 2024 9:54 pm ]
Post subject:  Re: First pearl cut on CNC
Did you cut both the pearl and the pocket with the CNC?
Author:  bcombs510 [ Sun Jun 09, 2024 10:03 pm ]
Post subject:  Re: First pearl cut on CNC
Nice work!


Sent from my iPhone using Tapatalk Pro
Author:  doncaparker [ Sun Jun 09, 2024 10:27 pm ]
Post subject:  Re: First pearl cut on CNC
J De Rocher wrote:
Did you cut both the pearl and the pocket with the CNC?


Yep! The pearl went fast, since it was just cutting profiles. The pocket took more time. In the future, I could save a bit of time by cutting the bulk of the pocket with a larger diameter cutter after defining the pocket with the small one, but for now, I am fine using just one cutter for both the pearl and the pocket.

I had some other work to do while the pocket was being cut, so the wait wasn’t so bad, and I avoided a tool change.
Author:  J De Rocher [ Sun Jun 09, 2024 10:45 pm ]
Post subject:  Re: First pearl cut on CNC
doncaparker wrote:
Yep! The pearl went fast, since it was just cutting profiles. The pocket took more time. In the future, I could save a bit of time by cutting the bulk of the pocket with a larger diameter cutter after defining the pocket with the small one, but for now, I am fine using just one cutter for both the pearl and the pocket.

I had some other work to do while the pocket was being cut, so the wait wasn’t so bad, and I avoided a tool change.


I asked because I'm wondering why the edges of the pocket are kind of ragged in some places. I've been gradually gravitating toward delving into CNC for some uses like this. I've seen the CNC results that Michael Colbert gets for inlays on his guitars and they are flawless. Because of that, if I make the jump I would be expecting and wanting to get flawless results especially since I do inlays into lighter colored woods at times. I want to be sure I end up getting a machine that can do that. So I'm wondering if the ragged edges I'm seeing are due to that particular CNC machine being not the best but not the worst or are due to something else. Maybe chip out of the wood?
Author:  doncaparker [ Sun Jun 09, 2024 11:23 pm ]
Post subject:  Re: First pearl cut on CNC
Well, keep in mind that this piece has not been glued in yet; it is just sitting in the pocket. And I didn’t sand down the rosewood before cutting the pocket, so the surface was not perfectly flat before I cut it. And I intentionally built in a few thousandths of gap between the pearl and the pocket that a person could make smaller and get a tighter fit. And this is literally my first pearl/pocket cut on any CNC. I was just seeing if I can accomplish the basics.

I am certain that a better machine would do a better job in general, but I don’t think I could draw any useful conclusions from this one test about whether my machine would be adequate for a specific level of desired precision for inlay work.
Author:  bcombs510 [ Mon Jun 10, 2024 1:24 am ]
Post subject:  First pearl cut on CNC
Since we’re talking about it … :)

I use the .024” version of these bits for the shell: https://www.precisebits.com/products/ca ... /shell.asp

And the .024” version of these bits for the pocket: https://www.precisebits.com/products/ca ... cutter.asp

The tool path approach is to cut the shell as a profile cut and then cut the pocket as a roughing pass with a larger cutter and then running an inside profile with the above .024” cutter. The important part here is it’s an inside profile not a pocket and it’s cut oversized by .003”.

For the roughing pass I use a 1/16 down cut end mill. It doesn’t have to be anything special. I use the ones from BQI because they are cheap - #2F062 - https://www.bqtool.com/square-end-mills.html

Don, I’m sure your machine can do this, will just take some testing on feeds and speeds. :)

The one that says Hubcap was done for Luke Baird and was so tight I was actually a little worried about the CA glue getting in there. :) These are all off the machine before glue up.

Image


Image

Image

Brad


Sent from my iPhone using Tapatalk Pro
Author:  doncaparker [ Mon Jun 10, 2024 8:16 am ]
Post subject:  Re: First pearl cut on CNC
Brad—

Getting (even more) geeky for a moment: when designing the inlay, do you filet all of the pearl “sharp points” to fit the size of your bit, or do you sometimes leave sharp points on the pearl and cut extra relief in the pocket to accommodate the sharp points? Mizek teaches the latter. With a dark background and matching filler, the extra pocket gaps at the sharp points disappear, and you get to have sharp corners on the pearl. The downside is that you are using filler, which can be avoided by making all the sharp points not as sharp so that the bit fits into every point. In any event, your inlays look awesome, and I appreciate the info and guidance (as always).
Author:  saltytri [ Mon Jun 10, 2024 8:50 am ]
Post subject:  Re: First pearl cut on CNC
.003" oversize for the pocket seems like it might be a bit too much. I do all my pockets with .001" and get a good slip fit with no visible gaps.
Author:  bcombs510 [ Mon Jun 10, 2024 9:14 am ]
Post subject:  Re: First pearl cut on CNC
Yeah, if you can go less definitely do. For example, my logo I don’t make the pocket oversized at all. The design of the logo helps with that.

I will also run the tool path twice which really helps for a good fit. Any amount of bit deflection in the first pass gets cleaned up in the second pass.

As for sharp corners, with the smaller cutters it doesn’t seem like I have to do anything special there? That being said, I haven’t done any multi piece inlay like that trout that Michael Colbert did a while back. Getting some info from him on process would be good because I believe he did it all on CNC.


Sent from my iPhone using Tapatalk Pro
Author:  bcombs510 [ Mon Jun 10, 2024 9:24 am ]
Post subject:  Re: First pearl cut on CNC
Don, also, since you’re using Vcarve - something that can help is using the allowance offset in a pocket or profile cut. You can use .001” or -.001” to shrink or enlarge the pocket / profile without having to change any vectors.

So try setting .001” like David recommends and then test fit the shell. If it is a nice fit, all good. If not, set the allowance to .0015” or .002” and try again. I don’t ever take the work off the table until I have the shell fitting well.


Sent from my iPhone using Tapatalk Pro
Author:  doncaparker [ Mon Jun 10, 2024 9:42 am ]
Post subject:  Re: First pearl cut on CNC
I’ll have to tinker with the offset feature. The way Mizek teaches it, you define the diameter of the bit as being a few thousandths less than the actual size of the bit. For instance, for a 0.023” diameter bit, define the bit as having only a 0.020” diameter. That gives an offset of 1/2 the difference on the pearl, and the other half in the pocket; in this instance, 0.0015” each. But I can see how the offset feature would be easier to dial in. This is one of those situations where I need to learn it the way the teacher teaches it, then I can move to something better as I improve overall.
Author:  bcombs510 [ Mon Jun 10, 2024 10:35 am ]
Post subject:  Re: First pearl cut on CNC
I hadn't heard of editing the tool database and setting the cutter smaller. It achieves the same purpose but I'm not sure I would do it that way.

I like having all the parameters in the crv file if possible. An edited tool would be in the crv but only for that instance and if you edited the tool again later, say during a different project, the crv is not automatically updated with those settings when you open it the next time.

I like to treat the crv as source code and I always build the g-code every time I run the project vs trying to keep existing run files around for long periods of time. If I'm going to run it several times over the course of a few days / week then that is one thing but if it has been a while since I've run the project I always go back and build from the "source". Just my weird way to approach it. :D
Author:  James Orr [ Mon Jun 10, 2024 11:19 am ]
Post subject:  Re: First pearl cut on CNC
Very cool!
Author:  ballbanjos [ Mon Jun 10, 2024 12:36 pm ]
Post subject:  Re: First pearl cut on CNC
Most of my inlay, I cut and rout by hand. But I did a "production run" of banjos a number of years back where I CNC'd the necks, fingerboards and peghead overlays (including inlay pockets) and the inlays themselves. I still did all of my engraving by hand. I used Rhino/MadCam to model and cut the necks, but used VCarve Pro for everything else.

Like Brad mentioned, I used the offset allowance in VCarve to cut the pockets. Another trick that I used mimics what I do when hand routing for inlays with sharp corners--I added tiny little vectors bisecting the sharp corners and routed a tiny line beyond the tips of stars, for instance. This makes up for the radius of the cutter and allows the inlays to go right in. The lines are short enough that they're invisible once you put the inlay in place.

In this picture, the tips of the stars and the two sharp points on the moon are done this way.

Dave
Author:  doncaparker [ Mon Jun 10, 2024 12:43 pm ]
Post subject:  Re: First pearl cut on CNC
Beautiful work, Dave! In the Bob Mizek course, he handles the sharp points by adding circles the same size as the bit at every sharp point, then moving the circles to just barely fit around the sharp points. This is for cutting the pocket, obviously. I used this on the two mountain peaks and the bottom right corner of the inlay shown in the original post. The rest of the corners were rounded (using the filet feature) to match the diameter of the bit.
Author:  bluescreek [ Tue Jun 11, 2024 10:34 am ]
Post subject:  Re: First pearl cut on CNC
I love precise bits I use .012 and .015
the have great support too
Author:  Ken Nagy [ Tue Jun 11, 2024 10:58 am ]
Post subject:  Re: First pearl cut on CNC
Coming from years of CNC work, ALL size changes, on lathes or mills was done with cutter comp. On mills it was with diameter changes to bring things to size. On lathes we would change x, or z, or do a pressure cut. Trying to hold +/- .001 or .0005 is as much an art as it is a science. Once set up, we could run +/-.001 all day on roughed out parts that were heat treated to 60 Rockwell or so (ceramic inserts). Drop the cutter comp with a new insert and check each part. Comp the next part a few tenths or so, and if it jumps again; change the insert and drop it back. You get to the point where you know you can get 4 parts on an edge. If you try to get more, your production will just go down, and you might even cut some too big, if you try to do a pressure cut with a new insert, and don't drop it down enough.

Milling out a pocket we would use a bigger end mill, and maybe, pick out, some smaller details, and then go with a finish cut.

For what you are doing; I don't think that you need separate rough and finish end mills. But a clear out cut, with a bigger diameter cutter comp, and then a finish pass, without the clear out, would work great. You might have to change the radius in the clear out pass, or you might have undercut problems.

I think that the outline is what you will see. Since your wood is darker, you can fill that, and all anyone will notice is the white pearl. Try it on what you have, and see how good, or bad it looks. Then see what it is like under varnish.

You can still play with the CNC, and tweak things. That's what they are made for. But a few thou clearance on an inlay doesn't sound like a problem.
Page 1 of 1 All times are UTC - 5 hours
Powered by phpBB® Forum Software © phpBB Group
http://www.phpbb.com/