Cutting Alalam (abalone sheets) Inlay with ShopBot

[austin0949]

I am hoping to be able to cut Abalam (abalone sheets) inlays for our guitar fingerboard inlays on my benchtop alpha shopbot. I have a good dust collector and would be wearing a respirator. Any other suggestions technical (bits, adapters, speed, etc) or safety issues on how to make this work? The Abalam sheets are .050 thick. Thank you

[supertigre]

Austin;

I have not been able to cut Abalam or MOP with my ShopBot but with my laser I can cut and engrave both.

[trakwebster]

Guy,

I what way did the cutting fail?

Is your laser mounted on the shopbot, or is this some other kind of machine?

[supertigre]

Arthur;

There were several problems with cutting the shell with the router.

The shell is brittle and I could not find a good way of mounting it that allowed me to machine it without breaking it while removing it from the holding board.

Delicate detail (star points, etc.) break off, the shell chips, etc. etc. when routing. And it is impossable to cut sharp inside corners. I did not try to engrave it but there is no way the router could match the resolution of the laser.

The laser is a zero force machine, a light spray of PhotoMount (a low tack temporary adhesive) is more than enough to hold it in place. Cutting shell is a pain with the laser too, but with time and patience it is (just) possable to achieve a satisfactory result.

The laser is another machine (Universal Laser Systems 40W).

[trakwebster]

Rats!

I, too, had some hopes of using the bot to cut some mother of pearl and abalone shell. Doesn't sound so hopeful.

[supertigre]

WARNING! Shameless self promoting plug follows!

Austin / Arthur;

For a few shekels and a half pound of flesh (i.e. wholesale to a fellow 'Botter)...

I can do it for you. :o)

Send email for details.

[handh]

You can glue the sheets to a substrate with a water soluable wood glue. After cutting out the sheet place the cutouts in water and let set overnight. They will come apart. Hope this helps.

[watswood]

As Guy said, it is tricky, but it can be done with the shopbot. Here is a picture of some diamond shaped inlays (.65" x .375" with a radius of .0156" on the points) which I recently cut out of .03" abalam:


8695

I used a .0469" end mill in one pass at .2 ips. The material was 'double stick taped' to a flat waste board. I tried several different varieties of double stick tape and only one type worked well. It's a paper tape similar in properties to plain old masking tape. You can tear it with your fingers easily and it's firm, thin, and sticky (but not 'too' sticky). Here is one source for it: http://www1.mscdirect.com/CGI/NNSRIT?PMAKA=00324707

The parts are cut all the way through and then carefully removed with a thin putty knife. Some of the shell dust may stick to the part, but will come off with a light stroke of a sanding pad. I've also used this method for cutting shell veneer as thin as .006" and shell slabs .06" thick with no chipout or broken parts. The veneer however is first epoxied to a dark wood veneer substrate to give a final thickness of about .035". This makes it easy to work with. For larger inlays I will use a larger bit such as a 1/16" or 3/32", but with these bits I prefer a downcut.

If anyone is interested in a source for abalam and veneer that is reasonably priced, check out http://www.rescuepearl.com/
She has alot of partial sheets that are about half the normal cost.
If you can find this guy: http://wellsguitars.com/Articles/Asia_2005/Asia_2005-Pages/Image9.html
then you can get it real cheap, but you have to order $1000 or more.

If your inlays are 'real' delicate, hire Guy.

Eugene

[supertigre]

Here is a sample of a MOP Star I cut and engraved for a client. The recess was also done on the laser.


8696

[knoxdude]

I'm looking to do the same thing with my 'Bot. A friend of mine has had great success using a 0.020" four flute end mill from MSC in his router, and taking light cuts with a slow feed rate. I'm looking into an air driven tool with a higher RPM. Harbor Freight has a small air driven d1e grinder with a 1/8" collet for $20. It runs at 56,000 rpm. I'd like to find a 1/16" collet for it so I could use dental burrs. Carbide dental burrs are about $1.50 each and the smaller straight bits are about 0.033" (1/8" shank). MSC has end mills down to 0.005". A lot of folks are cutting abalone and pearl (the latter is much harder than most abalone, I know, I've cut my share by hand!) and I see no reason the ShopBot can't do it just as well. If I'm not mistaken, seems as though I've heard of folks using hot hide glue to glue the shell to a substrate so it can be soaked off in warm water after the cut.

You won't ever get sharp inside corners with a rotary cutter, but it's an easy thing to go back and hit those corners by hand with a jewlers saw.

Also, on more fragile cuts, try cutting in a couple of passes, and leaving a "web" of shell about 1/3 the thickness of your material on the back side to support the more delicate areas. If you'll click on my profile, you'll see a mandolin peghead. Tom Ellis cut my name for me and while you can't see it here, there are several webs connecting some of the more fragile letters. Hope some of this helps. I hope to be cutting pearl on my ShopBot in a couple of weeks.

I'm curious how the laser works. I've heard it could be done, but have no idea what size laser is needed.

Thanks,
Lynn

[dingwall]

Lynn, a handheld air tool will not have enough torque to cut pearl, but it would engrave it fine. I've gone the Air Turbine route and come to the conclusion that it doesn't make much sense to use a $700 turbine and run a 5 hp compressor flat-out to drive a .025" bit.

Guy, that looks great! How did you hold the angled headstock in your machine?

[knoxdude]

Well, I've wondered about the torque on these air driven cutters. Sheldon, have you tried one and found it to be too low in torque? Are you just using a router now or a spindle head? The turbine I was looking at uses only 2 cfm... not much of a load for a compressor. I'm thinking about cutting it in two or three passes and not trying to hog it out all at once. If I'm not mistaken, Tom Ellis uses air driven cutters on his machines, and that's all he does is cut shell. I'm trying to call Don MacRostie and see what he uses. I think he's using a ShopBot to cut pearl.

[supertigre]

Lynn;

It doesn't take a very big or powerful laser to cut and engrave shell. The problem is to get the power levels, feeds, and finese in line as getting one of them off by even a little will spoil the cut. Shell turns into chalk when you hit it with a laser, too much power or too slow a feed and the cut line is too wide, too little power or too fast a feed and you cannot go back and redo the cut through the layer of chalk now sitting in the grove, trying to recut through the chalk will make the grove wider not deeper and it is extreemly difficult to clean the chalk out of the grove and not move the piece.

Sheldon;

The pegboard face is a seperate piece of 3/16" Macassar Ebony, no angle involved.

I must have been using the wrong tape and cutter. I don't think I could use cutters that fine with the runout on the PC router either.

[mziegler]

Guy and Lynn, many people have said that it impossible to cut sharp inside corners with round bit, but that not true, it can be done. I have no experience with abalam, so would I don’t know if it that practicable to do in that material. The technique does work best in thin materials.

Jeffrey, that is a new hold down method to me. Water released the parts and then them they float away! Well, maybe shell wouldn‘t float away. Thinking outside of the box here.

Air Turbine Tools has many models of air turbines for a wide range of materials.( www.airturbinetools.com (http://www.airturbinetools.com) ) Saw the information at Midwest Shopbot camp.
Mark

[knoxdude]

Eugene, did you just use your router to cut the diamonds? I'm thinking real serious about a 60 to 70k air turbine. Don MacRostie is using that for Abalam and pearl. The investment is not that much, so it's worth a try.

Lynn

[watswood]

Lynn, I used a spindle at 18k rpm. Before the spindle I used to use a Bosch 2hP router at 24k rpm, and pre shopbot I used a trim router running at 30k rpm. I have no experience with air turbines, but I would wonder how long bits might last at 70k?

[knoxdude]

Don says the bits last a long time. His air turbine is an inexpensive unit from Harbor Freight. All they have now is 56k rpm. I did an internet search last night and the 70k are impossible to find. But, the 56k is on sale for $15 at Harbor Freight. Might be worth a try. Never thought about a trim router. That's a good idea.

Lynn

[jim_ludi]

Lynn, you might want to look at this air turbine http://www.turbocarver.com/. I tried it at a woodworking show and found it to be a cutting demon (hand held). According to TurboCarver - "It's ideal for egg carvers, gourd carvers, glass artists, model makers, wood carvers, scrimshaw artists, metal workers, or anyone wishing to do precision carving, etching, or engraving in materials ranging from egg shell to hardened steel and gemstones."

It seemed to me that the compressed air requirement were fairly low. They also offer a water mist system. Should be real easy to mount to the Bot too.

Also, according to recent posts on the forum, it's possible to cut pockets with sharp corners using a vee bit and VCarve Pro http://www.talkshopbot.com/forum/messages/2/14775.html, http://www.vectric.com/.

[dingwall]

Hi Lynn,

I used an airturbine tools unit. It was a beautiful tool, but used all 14 cfm my compressor could put out, which meant my compressor was running constantly - not good. A 30 cfm compressor would have been fine.

I own 3 PC routers. They all have too much runnout for small bits. I replaced one with a Bosch 2hp unit. It's measured runnout is very good and is reasonably quiet. I replaced the main router with a Milwaukee. It's runnout is very minimal too and works great with small inlay bits.

I have one of those 54K air hand pieces. It seems a little too light duty and might be prone to chatter YMMV. I'd be interested in finding out what brand/model Tom's using. Don's a genius, he can make anything do just about anything.

When I switched from 65K rpm air to 23K rpm Bosch I expected to have to lower my feed rates by an equivalent amount, but I only had to lower them to maybe 60% of the previous rate. For me a feed rate of 2mm/sec with a ramp of 1.5mm/sec works really well on Abalam and solid pearl. This is for one full depth roughing and one full depth finishing pass.

[knoxdude]

Sheldon, Don said he used an $89 air driven micro die grinder from Harbor Frieght running 70k rpm. I think his reasoning was that it might have less runout than the 56k rpm unit. He gets great results with it. Harbor Freight doesn't list a 70k in their catalog any more, but the 56k is on sale for $15. At that price, I think I'll try it. If it doesn't work, there's not big loss. It doesn't take much torque to spin a 0.020" bit! By the way, when my PC router gave up the ghost, I bought a Milwaukee. I agree, it's a better router. At least for my use. I got the PC rebuilt, but plan to only use it for back-up. I may buy a laminate trimmer for cutting the pocket in the peghead veneers so I don't have to listen to the 3.5 hp router scream! I can see it now, I'm going to be working on a mounting system so I can switch between three different tools. I think a laminate trimmer and the air turbine could be mounted together. (Only using one at a time.) That would be a big time saver.

I've seen the turbo carver, but have about abandoned the idea of dental bits as it seems these small end mills have a good life and actually come in smaller sizes than the dental burrs. Anyone seen an 1/8" to 1/16" shank adapter?

Lynn

[les_linton]

Mark,

Although I understand what you are saying, I believe that cutting a "sharp" corner with a round tool is all in perspective.

The radius will always be there, but the goal is to not let the eye know it.

I talked to the folks at Precise Bits about this when I was quoting a project where the customer wanted "sharp" indide corners on some pretty small parts like what is being discussed here.

I have yet to try this (didn't get the job) but their method was to drill the corners using an .020 drill. Then cut your pocket using an appropritate size end mill and then route the final edge with a .0625 end mill.

The radius of the corner is only .010 and I think that you would be hard pressed to "see" that it wasn't sharp.

Lynn, your show is great...

Les

[watswood]

Lynn,
Here is a source for 1/8", I'll keep looking for 1/6": http://www.mlcswoodworking.com/shopsite_sc/store/html/smarthtml/pages/adapbush.html

[knoxdude]

Thanks Eugene. A fellow ShopBotter in Chattanooga turned me on to some 1/4" OD x 1/8" ID reducers from MSC. I think they are made for a die grinder and are the best reducers I've seen. I got a couple. They are $6 or $7 each, but worth it. Unfortuatly, they don't have one for 1/16" ID. Still would like a 1/8"OD to 1/16". Let know if you find anything.

Thanks a lot!
Lynn

[watswood]

I found one, but it's pricey. Scroll down this page a bit:
http://turtlefeathers.com/text/optima/optima-main.html

[dingwall]

You should be able to find all the cutters you need in 1/8" shank.

[trakwebster]

MLSC has a good deal on reducers. They're $4 each and you can get free shipping. I used one today to cut thin slots with an 0.023" carbide bit from RobbJack, and it seemed to do a good job. The shank is 1/8" and with the reducer I ran it in a 1/2" collet.

The bit spun fast and true. I was working in poplar, and took off only 0.012 per pass, but it seems to have worked fine.

It was running in a Makita router, at about 23,000 rpm, and moving about 1.5 ips in X&Y.

I liked it so I've bought some more of these reducers, so that I can just allocate them to the small bits. At $4 each, why not?

[knoxdude]

Arthur... do the MLSC reducers just have one cut up the side? I bought some from them before and found it real difficult to get bits in and out of them. The ones i got from MSC are made more like a router collet, with four cuts.

Lynn

[trakwebster]

I think that maybe they do only have one cut. I've not had much difficulty with them in that regard.

But maybe I will!

[mziegler]

Les, here a preview image from Vcarve Pro showing sharp inside corners on this box joint done by a round bit. The material is ¼ inch thick and the box joints are ¼ inch deep. Far as I know the Vcarve Pro preview screen is very accurate. Since I am no good at explain things and it is easier to show how it was done, I will post the CVR file over at the Vectric Forum site.
Drilling the sharp inside corner is my prefer method do this. As Les mention above, drill first and rout second. A 1/8 drill point router bit with a ¼ rout bit is a good combination for ½ ,¾ inch material. Then take a block or clamp the mating part to pressed or crushed the remaining wood. Mark


8697

[jim_ludi]

Lynn, I haven't found any updates to your posts on inlay setups. Have you been able to rig something up that's workable for inlay? What worked and what didn't?

[patricktoomey]

Jim, check out this post on the VCarve forum...

http://www.forum.vectric.com/viewtopic.php?t=564&postdays=0&postorder=asc&start =0

Paul Z came up with it and I have been using this method since he posted it. The results are incredible and it's easy to do. From page one you can see the examples but the technique has become more refined. Go to page 4 and look about 2/3rds of the way down the page for a link to a PDF document with detailed instructions and examples. It uses V bits to create sharp cornered inlays that mate up perfectly without worrying about material thickness variances.