Official Luthiers Forum!

I would like to get better results on endgrain. Here's a test piece of Khaya which machines nicer than the swamp ash and alder we will be mostly using.

The bottom piece is endgrain jointed with a spiral head jointer. The rim on the body above was machined with a 3/4" Onsrude downcut and the round overs were machined with an FS tool bit. I've played with the feeds and found that slower is better for tearout. I'm running the 3/4" bit at 4000 RPM with a .004" chipload. The roundover bit is doing 9000 RPM with a .006" chipload.

Is it possible to get a better finish on endgrain? If so, what direction to I need to head?

TIA

With wood it's all about getting a good shear in your cut, because the material doesn't really deform like metal during a cut and so if you don't get shear then it'll tear, break, or bend rather than deforming.

It's good to think of it like you're using a sword to cut it

1- Use the highest RPM you can, always, as the faster the edge is going the less chance the wood has to get out of the way
2- Higher diameters have higher edge speeds, which leads to the same effect. The finish you can get from a 4" cutter is freaking amazing!
3- Smaller chip loads and cutting orientation help prevent the chips from pulling along more wood when they go (which leaves tearout)
4- Sharp cutters, of course, are always important. Use carbide cutters specced specifically for aluminum or wood if in doubt.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Yep, what Bob said. Slower feedrates = less tear out. Also - African mahogany fuzzes more than genuine mahogany.

_________________
http://www.PeakeGuitars.com

Thanks guys. I'm trying to find a happy point between burning and tearing. I thought it would be as easy as adjusting the feed on the fly to zero in the sweet spot.

Bob, you mentioned a 4" cutter. Are you talking a shell mill? We've got a Spiramax head on our shaper and I love it. AFAIK they only make shaper heads.

I got a special shaper cutter made for the mill; the diameter at the cutting edges is either 3.5 or 4" (it's been awhile since I've done production using it). It leaves a finish so shiny that sanding ruins it.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

A shell mill would be ideal but I've found a four flute 3/4' - 1' endmill at 4000 rpm to be more than adequate.

If you have the means to check concentricity...that's a help too.

_________________
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

What did you use for inserts?

Solid carbide knives; they're EDM cut from ~1" x 3" x 0.125" carbide blanks. They're custom profile, so I order them from the company that made the head.

It's pretty much a big version of this : http://www.amanatool.com/cncroutingdetails/rc-2326.html

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

If you're not already doing it, try climb cutting as well. Your machine has to be stout enough to handle it though.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

The machine's a Fadal 4020. Fixturing is about as rigid as you can get.

I'll play with the chip loads some more. On our old router we used .001"-.002" CL (Onsrud 3/8" Downcut) for roughing and less than .0007" for finishing. I've been under the assumption that we could/should increase the chipload with the Fadal.

Anyone tried this style of insert endmill in wood?

http://www.glacern.com/em90_1

They look rigid as hell.

I use 0.012 IPT on a half inch end mill, 240 IPM at 10K RPM, for roughing. A quarter of that if I'm really worried about the finish.

I have one of the 1.5" EM90's (looks like they cut it down to just the smaller sizes now) and it's an awesome cutter. Sadly, I only have steel cutting inserts for it right now so I haven't run it in wood but the aluminum inserts they sell should work like a charm. I highly recommend having a big insert cutter. I've got a video of it cutting, but it's in tool steel . Check out the aluminum cutting video, too, if you want to see the machine really cooking with the new control.

Come to think of it, I won't be able to use that cutter in my new machine...I'm sure I won't have a CAT40 spindle. PM me if you want to buy it, it's a 3 flute version of the EM90 (same inserts) at either 1.375" or 1.5" cutting diameter. I'm going to miss using that thing. Heck, I'm going to miss my Fadal, too...got to sell it by the end of the month and the offers thus far aren't fantastic.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Yes - it is - cuts great with the aluminum inserts

_________________
www.morganguitarworks.com
www.morgancustomguitars.com

So I've reduced the chip load to .0005" for 1/8" and under, .001"-.002" for 1/4"-3/8" cutters and .003"-.004" for 3/4"-1" cutters. I'm getting much cleaner results but it's a lot slower than I'd hoped for. We'll still pickup time savings in sanding though. The first run saved a little over 30% in sanding.

Went for the 3/4" glacern indexable mill. LOVE it!

Anyone using the cnc cookbook for feed rates?

The software is called G-Wizard (the Cookbook is the blog) and I use it. It's great stuff, and has all kinds of useful functionality beyond feeds. On steel and stainless it's a lifesaver (and tool saver, too). As a baseline on wood I use 240 IPM at 10,000 RPM with a 1/2" cutter at 1/2" DOC and scale linearly for smaller cutters, so 1/4" at 10K and 120 IPM. Usually you can go faster but that's my baseline 'safe' ratio.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Wow, that's a .012' chipload. I run about .012" CL with the Glacern insert mill for roughing. That's the kind of cutting I was hoping to use even for finishing but anything above a couple of thou even on larger cutters tears the grain.

I drop it as low as 1/4 of that when I'm worried about tearing, but only on end grain parts. It's important to have razor sharp cutters - the ones from Ridiculous Carbide and USA Carbide made for aluminum are deadly sharp (I have a very deep scar to prove it).

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services