| Official Luthiers Forum! http://mowrystrings.luthiersforum.com/forum/ |
|
| Fret slotting http://mowrystrings.luthiersforum.com/forum/viewtopic.php?f=10106&t=13485 |
Page 1 of 2 |
| Author: | Steve Spodaryk [ Sun Sep 02, 2007 6:11 am ] |
| Post subject: | |
Great to see some activity here lately. I've been doing some fret slotting in ebony and rosewood and I'm also writing a short article about the process with RM Mottola. I just wanted to see if anyone else was slotting, and whether they'd be willing to share info about feed rates, etc. My machine is a sturdy DIY machine with a heavy aluminum frame and a 2.25 HP PC 892 on it. Steppers, ballscrews, linear rails, vacuum holding for parts. Based on the Onsrud datasheets and the RobbJack Calculator, I've been working in the feed rate range of 12-25 IPM, taking about .015"-.020" depth of cut, with a .023" endmill spinning at 23K RPM. This gives a chip load/tooth of about .0006" at the higher speeds. No problems at these speeds. I've seen references to taking full depth (.080"+) cuts at equivalent speeds (25 IPM), but I'm nervous to try this and the forumlas don't seem to support this kind of aggressive work with a small cutter. Any thoughts or practical numbers for me to work with before I start breaking bits? Thanks, Steve |
|
| Author: | Don Williams [ Sun Sep 02, 2007 6:17 am ] |
| Post subject: | |
Hi Steve, Nice to see you here. John Watkins has had considerable success slotting fretboards in the past. Perhaps you can coax him into helping you out. As many can tell you (and I think you know) John came up with the idea of slots that have the same arch as the fretboard, leaving more meat in the middle for a stiffer and more stable fretboard. |
|
| Author: | Sprockett [ Sun Sep 02, 2007 6:52 am ] |
| Post subject: | |
Steve I use the .020 and .023 bits for inlay and for fretting, what helps the most I've found is to take shallow passes. There's a trade off on how long something like this takes, I keep my IPM pretty low (down in the 8 -14 range). The big trick John taught me was to try and keep the slot clear so the bit does not overheat, I run a huge dust collection system and have a full dust shield built into my CNC machine to help as much as it can. Regardless... I still break them more than I would like, I think it just comes with the territory :) -Paul- |
|
| Author: | Parser [ Sun Sep 02, 2007 8:33 am ] |
| Post subject: | |
I think if you are running in the 12 to 25 ipm range you are doing well. Those are tiny bits and it is very easy to abuse them. I usually run on the low side of that range just to stay on the safe side. I also cut my slots along a radius. I don't have enough depth of cut on these tiny little end mills to do anything but that! |
|
| Author: | Bob Garrish [ Sun Sep 02, 2007 10:44 am ] |
| Post subject: | |
The feeds and speeds at precisebits.com work pretty well. I use those and add a little speed until the bit sounds wrong. John was the first to offer boards slotted like that commercially, but others have been using similar construction for a long time. I'm pretty sure Thorn guitars was the first, although other makers have independently come across the idea (Kevin Ryan did, without knowing who John or Thorn are). |
|
| Author: | Steve Spodaryk [ Sun Sep 02, 2007 12:04 pm ] |
| Post subject: | |
Thanks, this is helpful. I'm also cutting these slots at a radius that matches the fingerboard. I think I first saw this done at least 3-4 years ago, but didn't know who to attribute it to. It does make for a stiffer fingerboard. The feed rate/chip load formulas seem to indicate that 25 IPM is about it for a 23K RPM router. PreciseBits states that you can take a full depth (.100") cut at 25 IPM at 40K RPM. This is a 3 flute cutter with some improved geometry for the task at hand - so that seems reasonable as well. For the time being, I'll stick with my lighter passes and 25 IPM (or under) feed rates for fingerboards. For pearl, I'm going about 6-10 IPM. Maybe I'll try a few bits from PreciseBits and see if I can't push them a little harder. Climb cut (clockwise) or not? I tend to climb cut almost everything (a lot less blowout), but wonder if that might make a difference as well. Steve |
|
| Author: | Bob Garrish [ Sun Sep 02, 2007 1:19 pm ] |
| Post subject: | |
There's no such thing as a climb cut when you're slot milling. There's no 'inside' and 'outside' to a slot. You'll want to make sure you use the right column for your feed rates on the PreciseBits site. The feed you stated (25IPM) is for Walnut. The feed for ebony is just over 7... As a general rule climb cuts are the way to go so long as your setup is rigid. They help finish a lot in metal, and they help chipout a lot in wood. |
|
| Author: | Rick Turner [ Sun Sep 02, 2007 1:38 pm ] |
| Post subject: | |
I made a templet-guided fret saw at Alembic about 30 years ago that cut a constant depth slot on any radius fingerboard. I had a pair of guides concentric with the blade on a chop-saw-like setup with a custom blade on an arbor mounted to a floating pivoted head and the fingerboards were mounted to a table on drawer slides for the sawing motion. It could do three fingerboards at a time, one slot at a time. Now we've got the Techno, and fret slotting is one of our next operations, so thanks, guys! |
|
| Author: | Steve Spodaryk [ Sun Sep 02, 2007 2:39 pm ] |
| Post subject: | |
Bob, are you taking a full pass - or multiple shallow passes? With your extra spindle speed and overall machine rigidity, I'm just curious if anyone is doing this. Rick, I'll be eager to hear about your experiences with the machine. The CNC with endmill approach may not match a circular saw blade for speed, but it opens up a lot of interesting options for slotting. Steve |
|
| Author: | Jim Watts [ Sun Sep 02, 2007 2:51 pm ] |
| Post subject: | |
You know I started to type a long drawn out answer on hp, rigidy, material, spindle run out, cutter dia. etc... It all plays in, then deleted it as it probably doesn't apply as it was coming from a metal world. But I will add this; I would use a 4 flute bit for rigidity sake. I also would use a slightly under size bit and climb cut a profile, not cut a slot, you'll get a more accurate slot and you can tweak it in with cutter comp. I also would probably not take more than about 1.5 times the diameter of the cutter just help with clearing the slot of chips. It's been over 10 years since I've done this (on a fadal) and haven't tried it with my hobby machine yet, but have high hopes and will try it soon on it. |
|
| Author: | Steve Spodaryk [ Mon Sep 03, 2007 1:07 am ] |
| Post subject: | |
Jim, if you have the time to give us some metalworking info, I'm sure it would have some application here. Fret slots don't require a lot of horsepower, but rigidity and runout are certainly issues. Especially if you don't like breaking bits! I've been using 1/32" 4 flute bits in pearl and for general inlay work, and they do work very well. The PreciseBits "fret mills" come with a 3 flute geometry, which may also provide some extra rigidity. I am going to try these. I considered using a .020" mill and routing a profile to a width of .023" or .024". That seems like a reasonable approach, but slower. My .023" endmill is producing slots around .024" in width, so there is a little bit of positional inaccuracy or runout at work. Not suprising with a regular wood router and rolled ballscrews. Even so, I think the accuracy is pretty amazing and this is a good slot width for most fretwire and I am very happy with the results. I wouldn't expect most benchtop machines to do any better with such small mills and taking 4-6 light passes to cut the slot. To clear dust I plan to install a small blower near the cutter, and make a small "brush" style enclosure to focus more airflow from my dust collector. Steve |
|
| Author: | John Watkins [ Mon Sep 03, 2007 1:29 am ] |
| Post subject: | |
I agree that pocketing with a smaller cutter will produce more accurate slots, but I think it's overkill in this application. Bridge saddle slots are a great example of when to do that. As long as my .023" shim will fit into a fret slot and my .026" shim will not, I'm happy. Dust collection alone will not clear the packed in dust. You need as much air as you can get right on the cutter, like this. 
|
|
| Author: | Parser [ Mon Sep 03, 2007 2:06 am ] |
| Post subject: | |
Another trick that you guys probably know about is to not route all the way thru the edge of the fingerboard. This hides the fret tang and doesn't require binding (you have to trim the fret tangs at the ends). |
|
| Author: | Sprockett [ Mon Sep 03, 2007 3:08 am ] |
| Post subject: | |
Hmmmmm.... that's a good idea John, I use vaccum for everything but I should have enough air left over to rig up something like that using loc-lines. Thanks -Paul- |
|
| Author: | Bob Garrish [ Mon Sep 03, 2007 3:15 am ] |
| Post subject: | |
Hmm...I posted a reply last night right after Jim's above and it seems to have disappeared? Anyhow, the gist of it was that I take full-depth passes at 65000RPM using speeds based on pushing up the PreciseBits speeds until it sounds right to me. There was other stuff in there about small bits and things, responding to Jim's post, but I don't feel like remembering :) |
|
| Author: | Rick Turner [ Mon Sep 03, 2007 3:23 am ] |
| Post subject: | |
Jim, you may not know about these bits: http://www.precisebits.com/applications/luthiertools.htm These guys have developed bits specifically for our applications and the geometry is ideal for ebony and rosewood. I'm limited to a bit over 20,000 rpm on the Techno machine, though I suppose I could strap a high speed spindle to the router spindle. That might not be a bad way to go at some point. |
|
| Author: | Bob Garrish [ Mon Sep 03, 2007 8:24 am ] |
| Post subject: | |
Air Turbine Tools, Rick, everybody's doing it! http://www.airturbinetools.com/ |
|
| Author: | Rick Turner [ Mon Sep 03, 2007 9:20 am ] |
| Post subject: | |
Those are beautiful things, Bob. What HP for fret slotting and inlay? Didn't see the air inlet; it doesn't take air from the tool changer, does it? That would be entirely too slick... And I'm assuming these to be in the $1,200.00 range...is that about right? |
|
| Author: | John Watkins [ Mon Sep 03, 2007 10:56 am ] |
| Post subject: | |
Any HP will work. Mine is .2 They run from $300-$650 and require a lot lot lot of air. |
|
| Author: | Bob Garrish [ Mon Sep 03, 2007 2:10 pm ] |
| Post subject: | |
There are through-air versions, the one I use (same ones Kevin and Taylor use) has an air inlet on the side. Gotta be careful about how you run the air line if it's in an ATC. John's right on about the air, but I think it's very worth it. As for the HP requirements, it takes a pretty beefy cut to stall them. You can stall them cutting metal with a 1/16 or 1/8" mill, but I don't think you'll ever have the need to be using those in your line of work. |
|
| Author: | Rick Turner [ Mon Sep 03, 2007 2:12 pm ] |
| Post subject: | |
Thanks, John. I have a lot lot lot of air available. The price seems reasonable for what appears to be good precision and quality. I love the idea of it being compatible with my tool changer, and it looks like I have enough "Z" height to just pick it up in the router and just not turn the router on. I assume it needs some sort of anti turn and twist setup, right? |
|
| Author: | John Watkins [ Mon Sep 03, 2007 10:26 pm ] |
| Post subject: | |
If you get the kind with the shank on top and the inlet on the side, the resistance of the air hose will be enough to hold it still. These things were made originally for hand use, so they are extremely well balanced. They have bearings on par with your Colombo (I assume that's what you have on the Techno) whereby you can spin it with your thumb and it will turn 50 revolutions before it stops. |
|
| Author: | Rick Turner [ Tue Sep 04, 2007 1:16 am ] |
| Post subject: | |
I've got an HSK 5 hp spindle on my Techno. Sounds like the air spindle will work just fine. I have to say this spindle is amazingly quiet even cutting with a 3/4" roughing bit. A Dremel makes more noise than this thing. I got too used to my Ekstrom Carlson pin router! |
|
| Author: | Bob Garrish [ Tue Sep 04, 2007 2:33 am ] |
| Post subject: | |
The spindle on the Fadal doesn't even make a whole lot of noise, and it's a big sucker. I think most of the noise in a spindle would be vibratory in origin, though, so quiet is good. As for the air turbine, prepare for a bit more noise. Think 'dental drill' but way bigger. The air whistling through that turbine makes quite the squeal. |
|
| Author: | Sheldon Dingwal [ Wed Dec 19, 2007 11:37 am ] |
| Post subject: | |
I've cut slots manually and on the CNC. For production I've gone back to manual. Total time on the manual machine is about 1 minute. On the CNC 15 minutes or so. It sounds like my setup is similar in concept to Rick's Alembic machine. Although I bet Rick's was a lot more robust. Mine's made from a Hitachi sliding compound miter saw. The blade's a HSS hollow ground screw slotting blade. It's probably done 500 necks or so and still has lots of life. I machined a corian blade guard that doubles as a depth stop, tracking over the pre-radiused fingerboard. The sub table and neck fixtures are made from laser-cut 1/4" steel. On the sub table there are two indexing pins directly under and inline with the blade. The neck fixture has a hole and a slot for each fret slot that locate on the table pins. The neck fixture holds the neck during 3 processes, radiusing the fingerboard on an edge sander, cutting fret slots on this rig and routing the nut slot on a pin router. The cost of the last fixture was about $50.00 for the laser work plus a day's labor on the bits and pieces.  |
|
| Page 1 of 2 | All times are UTC - 5 hours |
| Powered by phpBB® Forum Software © phpBB Group http://www.phpbb.com/ |
|