Cnc for lutherie work: AR 4 v ar6

[brad]

Can anyone advise whether the ar 4 basic is big enough for lutherie work--I make ukes and acoustic guitars and before I make the plunge for my first cnc I want to make sure the 4 is large enough--the 4 seems big enough for accustic guitar necks but would like input of those who are currently using the ar machines for lutherie.  Thanks!

[germanguitars]

I purchased an AR6 last month instead of the AR4 since I make both flattops and archtops, and my archtop necks include the fingerboard extension as a single piece, exceeding 24 inches. My previous machine was 48" x 48", and that was much larger than I ever needed.
I'm planning to cut out a flattop neck for the first time with this machine later today.

[brad]

Thanks, that makes sense. I don't make arch tops currently. So for a standard acoustic/steel string neck that joins at the body without an extension, do you think the AR4 would be large enough?

[brad]

Have you been happy with the machine?

[germanguitars]

It should be large enough, depending on how you make necks. The one I just cut is a two piece that is nested like this and its blank is exactly 24" long: 


Yes - I've been very happy so far.
-gg

[brad]

Super thanks! I'm am ordering the AR4 basic.  So you have the two necks from 2 separate blocks, and carved them on the sides rather than the top and backs?

[brad]

What software do you prefer for the 3D modeling? I've used sketchup so far. Thanks

[germanguitars]

Dec 30, 2016 18:16:51 GMT -5 brad said:

Super thanks! I'm am ordering the AR4 basic.  So you have the two necks from 2 separate blocks, and carved them on the sides rather than the top and backs?

No - I prefer two-piece necks cut from flatsawn slabs so that the business end is quartered towards the fretboard.  

I've used many different modeling programs, but now I prefer Rhino.

[brad]

Can you give guidance on the feeds and speeds you're using for the guitar necks (and what bits)? I've designed a uke neck but it's showing many hours to carve it in Vcarve and I'd like to reality check my parameters. 
Thanks,
brad

[germanguitars]

Takes about half an hour -
90 IPM with a 1/4" end mill [up-spiral, 1.75" LOC in this case].
The photo in the post above was cut with a 1/4" ball-end in two passes with a little more time (previous machine).

I start with a relief cut on each side of the curved surfaces:

Then I shape the whole thing in one pass leaving 0.015" to sand/scrape off. The step-over is variable but 0.040" at most, so the curved surface has a pretty high resolution despite the square-end bit. Ball-end gets you closer to a 'final' looking surface finish, but you still end up sanding the same amount of time to remove tool marks and do the final shaping as with this rougher look.

[brad]

Thank you--just so I'm clear what is the plunge rate and pass depth? And do you raster cut along the length of the neck (I think so) as opposed to z level carving?

[germanguitars]

Plunge rate is also 90 IPM.
0.125" depth per pass on the relief cuts and cutout, 0.25" depth of cut when hogging off material at the tenon.
Raster cut is not a term I am familiar with, but I think I know what you  mean.
The cuts along the neck/heel surface are arranged thus:
-RhinoCAM has a machine toolpath labeled 'between two curves' [https://www.youtube.com/watch?v=qxL6SQ3UTkU]
-the first curve traces the neck along the fingerboard edge and curves downward to the tip of the heel near the body joint.
-the second curve is nearest the cutout line from the volute to the tip of the heel furthest the body joint.
-the operation interpolates between the two, creating 'water line' offset cuts

[brad]

OK thanks. I think where I'm stuck is the wood I'm planning on using is 2 inches thick--so will I need a bit with an LOC of at least that much, or can I use a bit with a shorter LOC as long as the stick out is say 2.2 inches?

[germanguitars]

To stay within the bounds of the LOC yet quickly machine the surface, you may need to do some strategic relief cuts. I have broken a few 1/4" bits milling necks. One strategy would be to mill a pocket above the deepest cuts before you begin to even out the depth of cut.

[germanguitars]

Just did a maple archtop neck from a blank that was 1.8" thick. Used an up-spiral with a 1.75" LOC. I did a relief cut from the top surface down to 1/8" off the table all the way around both sides first. I carve the curved surfaces starting at the fingerboard edges and working down the slope towards the back of the neck. At the point where I am using almost all of the LOC the remaining 'wall of wood' is getting pretty thin so it vibrates rather than pull the bit. I monitor it and break it with a chisel to save the machine some work if it sounds like it struggles. The end of that cut isn't necessarily precise since it will be a 1/8" x 1/4" tab for glue-up:

 
You can see the tear-out areas at the treble ear - always leave extra wood there in your model.