Official Luthiers Forum!

So here's my latest. I have cut a pocket out of a scrap piece of Padauk, and the inlay piece I cut previously fits snugly in it. Here it is glued in -- the picture is just a bit fuzzy, but it looks like a very clean fit to me.



I think the fit may be too snug. I had to press the inlay a bit to get it in, and it broke in a couple places (although I just kept pushing it in, and you can't tell that it ever broke). The inlay is very fine -- .017" wide lines -- so I'm not surprised that a little pressure caused breakage, but I'm assuming it's better to make it just a little looser so it doesn't require pressure to fit it in.

Realizing that I've given only a vague description of the fit, any guestimates as to how much more clearance (if any) you would normally want in this type of situation? An extra .001" all around? I can keep experimenting, but I confess I don't know how tight of a fit you want at the end of the day.

I'd say the answer is- as tight as you can make it without breaking the shell. I have been setting my offset at .0001" with good results.

Best, M

I like to leave a little bit more of a gap. After it's done, the wood still moves but the shell, not so much. I've had inlays crack years after they were done because of fitting them a bit too tight when I did them (and this was fit by hand, not to CNC tolerance). I typically leave .001 to .0015 all the way around, but will somwtimes vary this one way or the other based on the size, shape and material. I set my inlays with epoxy and want room for just a little bit of squeezeout.

Dave

Looks good but tight. I have different fit tolerances for different inlays and what wood its going into. Lighter the wood the tighter, ie maple, any spec of glue shows. It's hard to seal up a really tight fit with glue and then come finish time the lacquer finds the hole and it's drop fills aplenty. For a rosewood headplate or fretboard, a small consistent glue line is nearly invisible and solves other issues. I'd think the trial and error process would be much nicer if your control supported diameter adjustment (wear) so you didn't have to tweak the program and repost for everything you try (mine does not).

It's arbitrary to specify any particular amount of fit allowance if you can't guarantee your tooling is accurately spec'd or whether it's concentrically mounted. This is why I advocate getting into the practice of "sneaking up" to a fit. Once a fit is achieved you can run multiples (for that session only) without worrying but I would never commit to using a standard fit allowance without expecting it to bite me in the butt at some point.

The inlay material should slide freely into the recess without being loose.

Glue needs to escape. On large areas it may be prudent to mill a few very small recesses, or drill a few small holes, to allow glue a place gather. Sometimes I'll drill a hole all the way through the recess to allow glue out the back...if the application permits.

If your cam package allows a "draft" option to be applied...you can actually create slightly angled edges on both your inlay and your recess...which, when clamped, will provide a net fit every time. That's a lot of work for a dubious gain, however. A nice "slip" fit will not be perceived by the naked eye.

Your inlay picture looks very nice and will never be questioned by any customer.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Good advice from Stuart.

One frustrated day I decided to make some thick veneer to cut practice pockets and inlays from. Basic shapes like ellipse, square, circle etc. so I could figure out my allowance for fit and glue etc. From there it was pickguard scraps for inlay into wood scraps then finally shell scraps into wood with more complex shapes. Learned a lot from that.

Thanks, everyone!

I totally understand Stuart's advice on "sneaking up," and that's precisely what I've tried to do. Here's how I've approached it:

I'm using a bit that is reportedly .0157" thick from Precise Bits to cut the pocket. I have no way of knowing how accurate that number is. When I generated the code to cut the pocket, I initially told the software that the bit is .0145", such that using a .0157" bit would result in an oversized pocket by .0012". The resulting pocket was too tight. So I tried again, this time telling the software that the bit is .0135". This resulted in a pocket that allow me to insert the inlay, but I had to press it in, and it broke in a couple places. It looked great once it was in, but I think it's still too tight. Next time, I'll tell the software that the bit is .0125" and see where that takes me. The obstacle now is that there is no way to get the broken pieces out of the slot I made last time (so I glued it in and sanded it down to see how it would look). So, to do another test, I'll have to cut another piece of inlay as well. That's fine. My gut tells me that another .001" will be pretty good. The final version is going in ebony, so even a small gap won't be visible, but hopefully I won't be dealing with a gap at all.

The software I use has a parameter called "Leave For Finish". Generally that's used so that you can do a rough pass leaving some material that then another final finishing pass will remove. It basically offsets the toolpath by the desired amount and generally can accept both positive and negative values. I use the real tool size and only monkey with LFF. I think visual mill had something like that. Bit deflection is pretty unavoidable with these tiny bits, ebony is hard, not as hard as shell. If you are not careful, the shell will get cut too large and the wood will get under-cut due to deflection. Doing a final finishing pass taking the last bit of material off helps because the amount of material to cause the deflection is small. Look to see what your software supports. Also check your controller and see if it supports tool compensation, I thought the B&R did. I suspect Stuart is using that in his Haas control.

Thanks! My software does have a roughing pass and finishing pass options, so that may be the right way to go.

Madcam has stock to leave. And i can put in a negative number. Look for something like that.


Sent from my iPhone using Tapatalk
Ken

_________________
Ken

Not sure how your software does it, but you might want to check to make sure it does what you want, and how it works.

The software that I use has an automatic finishing option which for example adds a profiling pass after pocketing or profiling. So for profiling the inlay, I might choose a leave amount of .002 and it will oversize the inlay by that amount and then it will make a second pass to part size. Choosing a negative value for leave for finish for an inlay pocket will make it do the pocket to the size of the geometry and then do a second profile operation to make it larger. I often turn off the automatic finishing for inlay work and use the leave for finish to control the size offset and do a second operation for final size.

Tools are usually within .002 undersize and .000 oversize.
I generally use .004 as a gap as a starting point and may increase or decrease from there if needed.
Tool paths aren't always a perfect match when cutting a contour vs a pocket. (Can be for a number of reasons, the software generating the code, machine' ability to accelerate/decelerate, machine's repeatabiltiy/tolerance...etc.)
Always use a finishing pass as it is more accurately calculated. As Ken says, using a negative stock to leave on walls is a good way to go.

Your machine's parameters are more likely to cause errors than cutter diameters in the tiny sizes, so it's down to each individual machine. Backlash will add to the required offset. On my old Fadal (machining center) I used 1.5 thou all around. Inlays dropped in but you couldn't see the glue line without a loupe. Now, whether that was actually one thou or even less because of backlash or something else, who knows...

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services