Official Luthiers Forum!

What do you guys "typically" use for offsets in wood to wood inlays? I was playing around this afternoon and the male piece would not fit with a .000", or .005" offset. Next I tried .015" and it was sloppy then I tried .010" which was about right. I could have forced the .005" but I would never had been able to use wood glue in the joint.

I vaguely remember reading where you need about .012" clearance for wood glue joints but I could be mistaken?

_________________
tim...
http://www.mcknightguitars.com

On all inlays it's 0.001-0.0015" normally, 0.002-0.003" if it's not too intricate or the line won't show (dots on ebony, etc). I've done ones that were perfect fits, but I worry that the glue won't get completely under and around the inlay and it might pop out later. I use CA on all my inlays, though hide can get anywhere the CA can (you just need to move really fast) and I've done a few tests with it that worked fine.

0.003" is a pretty loose fit, the inlays just fall in.

That said, the problem isn't an offset problem; it's a cutting accuracy problem. It's either poor tool motion making off-shape parts, part warpage after cutting from sitting around too long, or cutter deflection making the parts oversized and the pockets undersized. I'd try the fix for cutter deflection first (run the finish pass twice on both parts) and see if that works as if it's a tool motion problem then that's a whole lot more annoyance!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I used a 1/8" bit, 16000 RPMs, at 1.7 IPS so I am unsure how much deflection I had though I suppose it is probable. I didn't consider running the cut twice though it makes sense. The pocket part was held by vacuum but the male piece was held with DS tape so I suppose it could have slid?

I don't want to use CA because this inlay is in a spruce top (rosette). Even though I have sealed end grain prior to using CA I have still had yellow halo issues so that is why I want to use wood glue. Perhaps I should consider using epoxy so that I won't have grain swelling issues?

When you cut the male piece is there a need to flip it over to fit the pocket or should it just drop straight down in? I tried both and it didn't really seem to matter.

On my first attempts the inlays were way off. I made the inlay file from a JPG and converted it to a vector file and found some array spacing errors. Then I went back to basics and mirror copied one half of one shape, joined the open vectors and then used the copy circular array function to make the spacings more consistent. That was a huge improvement to how the pieces fit.

_________________
tim...
http://www.mcknightguitars.com

I'd deal with the swelling from hide or with using medium CA before epoxy, but I probably have an unreasonably negative response to epoxy as an inlay filler since it seems to be the fill of choice on the real 'disaster' inlay fits

Pieces can move around on double stick tape, especially if it's not particularly tenacious stuff. I've got DST that barely holds stuff, and I've got DST I won't use on wood because it's so strong it'll rip grain out of anything! Stuff on a vacuum plate can move around, too, though I doubt your female piece was small enough for that to happen under vacuum (I still use pins on everything except acoustic tops and headplates to prevent lateral motion)

On wooden inlays, I sometimes like to cut the inlay as a mirrored positive on top of a 'block' and then mill away the excess after installation. That makes it a lot easier to keep everything lined up if there are multiple wooden pieces and I want them to stay in relative positions to continue grain, but also means you can't check anything about the fit or look until it's already glued in and you've milled off the 'backing'. Most wooden inlay I do is cut 'as it'll appear' and dropped in face up, though. The first method (leaving it attached to more material behind) also prevents it warping on you.

The perk of CNC is once we get this figured out you'll never have to mess with it again

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I setup my cuts for about .003" of clearance on a simple one piece inlay, but I do use more for multiple piece inlays (.005 or so). If you have a fancy machine like Bob's then you can go for a more accurate fit..

You should not be getting much tool deflection on a 1/8" tool running at 1.7 ipm. It sounds like you may have a positional or runout issue...(?)

_________________
http://www.PeakeGuitars.com

I dismissed runout since runout would make the cutter spin wide and actually make a larger cut (which would require a smaller or even negative offset).

The original post said IPS (which would be 1.7 IPS = 102 IPM). Just to be clear, which did you mean, Todd? As Parser said, 1.7 IPM won't give you deflection, but 102 IPM likely will.

I'd call my machine heavy or rigid, but not fancy...if I recall correctly,the chip in the controller is a 386!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Those Fadal's are great machines for this stuff....there's a reason PRS, Martin, Taylor, and many others use them.

I did assume he meant 1.7 ipm.....if it was IPS then I'd suggest slowing it down a bit to avoid deflection...probably to around 20 ipm or so. Might as well play it safe. At the higher speeds I think you start running into issues with how well the part is being held down....tape will "smush" around a bit...

_________________
http://www.PeakeGuitars.com

Yep, 1.7 IPS (second) not IPM. I have no clue about feed speeds yet so I an just getting my feet wet with this CNC stuff. I was told to make chips and not dust to reduce heat which is the enemy of carbide. Is there anywhere I can get some basic RPM/feed speed guidelines? I was also told to climb cut the majority of the time to produce cleaner cuts. Is this correct?

_________________
tim...
http://www.mcknightguitars.com

Hello Tim,

The speeds and feeds are usually provided by the manufacturers of the tools you are using, and they usually refer to something called "chip load." It also has to do with the chips like you said that the tool is cutting, and finding an optimum speed will allow you to cut faster, but will also allow the tool to remain cool under load (cooling is related to the number of chips the tool is expelling, and hence the correlation to chip-load).

A good site with cutter information and formulas is here:

https://www.onsrud.com/xdoc/ChipHardwood

Also, there are ways to do some experimentation with cutters you might have to find out the optimum speeds for your tools, and a good explanation for smaller cutters (like you use in inlays) is offered here:

http://precisebits.com/tutorials/calibr ... speeds.htm

Curious to see what CNC machine you went with? Did you build one from scratch?

peace...

_________________
-CyborgCNC
http://www.cncguitar.com
https://www.facebook.com/CncGuitar

Your feeds and speeds are dependent on everything from your machine (spindle power, machine stiffness, etc.) to the material you are cutting to the jig that is holding the part...and everything in between. You'll get a feel for it as you cut more and more..

_________________
http://www.PeakeGuitars.com

Hi guys,
Thanks for the sage advice and wisdom y'all shared. I will study the data sheets and try to make some more logical choices in my future cutting feeds and speeds.

Cyborg, I did a LOT of research (about 4 years worth) before taking the CNC plunge a little over a year ago. I would have loved to had the luxury of time on my side to build my own machine but unfortunately I didn't. My eyes were lusting after a Fadal or even a tricked out Bridgeport but my wallet told me otherwise. So based on my research, my needs, floor space, customer support and budget I purchased a ShopBot "Buddy" with a 24" x 32" x 5" cutting capacity. I am pleased with my purchase and looking back I would buy the same machine again if I had it to do over except with a spindle verses a router.

_________________
tim...
http://www.mcknightguitars.com

At 100 IPM I wonder if you're having issues with "Constant Velocity" rounding off corners too. I'm new to this as well and have been using 30 IPM for inlay. Seems to work well for bits down to 1/32" (I used 20 IPM for cutting fret slots). I learned about constant velocity while trying to cut pyramid bridges at ~200 IPM. The peaks ended up looking like blobs. After turning CV off I was able to get nice sharp peaks. Unfortunately I forgot to turn it back on and broke a 1/32 bit as soon as I tried running an inlay program. Too much jerking motion I guess. Lots of lessons to learn...


Bob

Hi Bob,

That is really something which I think you have hit the nail on the head on, the CV mode!
Might very well be the issue here.
I am not sure of the Shopbot controller software that Tim is using, but I know on mach3, there is a setting which will "automatically" set CV OFF, depending on angle!

So for example, you can have the machine switch to Exact Stop mode depending on an angle (like for example go to Exact stop if angle is smaller than say 90 degrees to get a sharp corner) and then back to CV for angles larger than 90, to get smoother motion.

Also, there is a function on mach3 for "look ahead" in the code....in that the software will look ahead say 200 lines of G-code, and allows it to better adapt to sudden changes...

Just a couple of more thoughts....

_________________
-CyborgCNC
http://www.cncguitar.com
https://www.facebook.com/CncGuitar

One difference that pops up between the Fadal class machines and the sub-$50k group of machines is in the loss of accuracy at higher speeds. The Fadal's maintain their precision throughout the range of speeds, whereas it is pretty common to see those other machines start to "take shortcuts" when rounding corners, etc. This is one reason why the big production shops use Fadal's and not the typical CNC router class of machine.

Unless you really need to cut that inlay in 2.5 minutes instead of 5...just slow it down a bit... (c:

Trev

_________________
http://www.PeakeGuitars.com

Climb cutting produces cleaner cuts, but also allows the cutter to deflect more as it's 'crawling over' the surface. A common strategy in metal is to do the same climb cut twice--once to rough the part, once as a finish--which relies on the cutter deflection! There are situations where both types of cut (climb and conventional) are more appropriate, but as a rule if you don't know where a conventional cut is more appropriate then you'll make the right choice 95% of the time by using a climb cut!

Don't worry about cooking your carbide in wood, you'll get a whole lot of smoke (and probably fire) long before you get near the temperatures that'll bother your cutter. The feed rate you use is the proper chip-load-derived feed rate for 16,000RPM but that's assuming a low-runout spindle on a rigid machine with perfect tool motion. I'd keep the 16,000RPM on wood but lower the feed rate to 60IPM for most cutting and down to 20-30IPM if you're trying to be really accurate. I'd say at this point we're pretty sure it's a tool motion issue so try a 20IPM two-pass, climb cut finish and see if the parts fit (then bump up the speed until they don't anymore )

The wood resin will cook onto the carbide sometimes, depending (or if you run hot enough for long enough). To clean it off, just drop the cutters in a bowl of drain cleaner or something else caustic enough to dissolve the gunk. It also works on aluminum, if you ever wad a cutter...


(Also, Trevor, 'smush' is the PERFECT word for what happens when a part moves around on DST!)

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Well I before I glued the (-.010") undersized inlay I could see a teeny gap around the male piece. I used LMI white and the gap was large enough that the glue squeezed out as I pressed it into the pocket. After the glue dried then running the top through the sander the wood swelled enough that there is NO visible line anywhere around the inlay even when viewed under 2X magnification. I am very pleased with the result.

When I chose -.010" offset does that mean there is a .010" gap all the way around or is that a total gap or .005" per side? When I viwed the dry fit it looked more like .005" gap.

_________________
tim...
http://www.mcknightguitars.com

it depends on the software you are using. What CAD/CAM package are you using?

_________________
http://www.PeakeGuitars.com

I use PartWorks v2 for 2-2.5 D design and PartWorks Cut 3D for 3D work. Both are CAD/CAM rolled into one. Its kind of like CAD/CAM for Dummies I also have Correl Draw, Rhino and access to AutoCAD but rarely use them. PartWorks is designed by Vectric Software and basically the same as their V-Carve Pro. I am able to import EPS, Bit Map, DWG and DXF files into either off the PartWorks programs.

_________________
tim...
http://www.mcknightguitars.com