Official Luthiers Forum!

I've been messing around with my existing bits and find that clearance between the tool holder and stock material are a fair issue.

I'm wondering what bits people are successfully using to cut their acoustic heels all the way down to the profile.

I've got something in mind but before spending the cash I thought I'd see what others are doing

As you can see, my current longest bit is about 30mm too short of getting to the bottom of the profile

Hey allan, I use long shank end mills with replaceable carbide bits, gives the full length needed,

Steve

Do you have a link to purchase? What make?

I've used special extra long 0.5in. diameter end mills with a 3in. flute length and they work well but I'd much rather have what Steve is describing with the replaceable carbide inserts.

+1 for any further info from you Steve.

Leo

Allan, you can buy these in Australia if your limited to Z height, I have purchased these and they are okay.

http://www.ebay.com.au/itm/271925818042 ... EBIDX%3AIT

This is the one I use

http://www.ebay.com.au/itm/C20-21-200L- ... 5b146e92d2

As its an end mill, the finished job needs sanding, I have contemplated machining up a ball nose for myself, but the amount of clean up work is quite trivial IMO

(AKA Simso ANZLF)

Steve

Thanks. Not quite what I was imagining, also, I knew who you were, not many Mirwa's in Australia that I've heard of!

For now I think I'll keep looking for a extended shaft ball nose, I can imagine one day forgetting to check that those removable blades are tightened up and then having one spin off at 18000 RPM. Pretty sure it'd lodge it's way somewhere in the middle of my head!

Thanks for the info Steve.

I'll check Canadian eBay for the same thing.

Cheers.

I use a long shaft 1/2 inch copy mill (the largest my spindle will carry). I used to use a long shaft regular round nosed mill, but I think I get a better surface with the indexable cutter--definitely easier to keep a good sharp cutting edge. Found mine on EBay.

Dave

If you can, get the shortest flute possible on extended length mills. Long flutes make cutters really floppy.

The cutter Dave's using is a great way to go, and I also like 'reduced neck' end mills which have short flutes and a long reduced neck. I used to just cut necks on their sides for the heel...

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Would you flip them over for a left side/right side milling? If so, how would you support the now carved side when you flipped it over on your table?

Actually, from nuts to soup can you share how you did this? I am slowly remembering that I spent a few frustrating weeks trying to this. Guess I was blocking out the memory!

I could not see how to hold the neck securely on the side, how to index it, how to accommodate headstock wings, how to hold it once half was carved. I would love to see how someone solved those issues. I can cut with a 6"x1/2" bull nosed bit, but I get flex and often blowout at the edges of the heel. It feels like a left/right side carve would be the right move if the fixturing could be figured out.


Sent from my iPad using Tapatalk

Hold it by the fretboard face, and index with pins. You can rotate it any way by building your fixture at that angle.

The sort of basic vacuum fixtures used by Taylor/PRS and visible in all their videos are pretty much the standard, and mine aren't much different.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I'll look at some videos from both sources, but are you saying that the neck blank is held on its side by vacuum alone? It doesn't slip or pop off with the force of carving?
I know you are supper busy with your new medical devices business, but could I persuade you to post a picture or two? It'll save a thousand words or so...


Sent from my iPhone using Tapatalk

I use these here, just cut down on length a little bit but I'd love to have something like what Dave's using. I searched and searched for 1/2" shank copy mills and have never found anything.

http://dapra.com/cutting/ballnose/index.html

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

What inserts do you use Andy, and how's the surface finish?

It's always difficult to pick the right ones when they are all intended for something other than timber.

_________________
Allen R. McFarlen
Barron River Guitars & Ukuleles
Facebook
Cairns, Australia

I use the non-coated inserts for aluminum. The cheapest ones they have. I spoke with the rep and he said they'll give the best finish and I can attest that it is fantastic.

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

It's been a couple years since I've used those fixtures, and have no pics, so can't really help there. If you're careful with your toolpaths, though, it's totally feasible to do it all with vacuum hold-down. The pins are important for indexing AND taking up shear forces. Longer pins make more stable fixturing.

So far as tooling goes, anything marketed as being specialized for aluminum works well on wood. Wood and aluminum both prefer sharp uncoated tools with a positive rake.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Thanks. I had assumed as much, but it's always great to get the opinion of someone using them.

_________________
Allen R. McFarlen
Barron River Guitars & Ukuleles
Facebook
Cairns, Australia

Bob, I looked at both PRS and Taylor CNC neck carves and both seem to be carving the neck with the blank fretboard down on the CNC table, not with the fingerboard on the Z-X plane. Did I misunderstand you?

Regardless, it was interesting to see. Obviously PRS is not dealing with a two inch tall heel. However, I notice they both carve the heel by carving DOWN the face of the heel rather than in a water line X-Y plane stepped carve.

I'm not sure how to generate those tool paths, but that's for a different forum. I am curious if that is what people are doing here? Is a 1/2" bit rigid/strong enough for that? Those seem to be beefy bits, maybe 1"?


Sent from my iPhone using Tapatalk

There's no need for more than two setups to do the front and back of the necks + a third for the tenon/dovetail. I currently do the tenon/dovetail without the use of CNC but will probably build a separate machine for that down the road.

I use a 1/2" bit and have been able to do heels up to about 3.8" tall with that. The problem isn't so much the tool flexing but the vacuum holding the pice down if you're aggressively cutting the end of the heel. Lots of torque on the part at that time. As you get closer to the fixture surface, that's no longer an issue.

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

Andy, so you cut down the face of the heel like Taylor, not in terraced steps? That sure would cut down on carving time and help avoid blowout at the unsupported top of the heel!
This forum is awesome!


Sent from my iPhone using Tapatalk

I do a roughing step which has the terraced step sort of thing going on to remove the majority of the material. I think I leave behind about .040-ish or so. I then just do parallel finishing at a feed rate as fast as my machine can handle, about 375ipm right now. I'm planning on upgrading to servos which I'm hoping should let me do finishing passes at about 450 to 500ipm.

The parallel finishing is along the length of the neck. Blowout can happen during the roughing passes but if you have it set correctly to climb cut, it minimizes that issue. leaving behind only about .040" there's very little to no blow out on the finishing passes.

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

This bit works fairly well and last reasonable length of time......... there are better and worse.

http://grizzly21-px.rtrk.ca/products/1- ... Mill/H7650

Attaching some photo's that may help as you decide what you want to do.......
YouTube......
This shows a uke neck being cut (posted this quickly and this was a test run..... so there is some movement on the part....... held down with double sided tape)........ but same principle was used as on a guitar neck.
https://www.youtube.com/watch?v=7zkj8vekG4o

Blessings

Kevin

Thanks for the replies guys, don't think that my lack of comments means I'm not still following, I am.

I'll need to measure up the depth of my acoustic heel and see if that last 6" Grisly ball end will be long enough and still allow for a decent mounting depth in the tool holder. That one could be a winner.

In response to the tear out when roughing, I've only cut one heel so far on the CNC (I do electric ones all the time but only one acoustic so far) and just like someone else mentioned, when the cutter came up it blew a large piece of mahogany off the side, I quickly stopped the machine and altered the CAM (using Camworks in Solidworks) to change the paths so it did not zigzag and so there was less crossover and entry from the top of the heel not the bottom, after this I was able to run again and I didn't experience any blow out.