Official Luthiers Forum!

Hey, I just thought I would throw up a couple of pictures of my latest CNC neck



http://i202.photobucket.com/albums/aa201/jer7440/P1010241.jpg

http://i202.photobucket.com/albums/aa201/jer7440/P1010239.jpg

I cut this neck on the Haas VF-3 at my work. I've done 3 of them complete now and it takes me about 1.5 hrs to machine one. I do end up doing a little manual blending with some sanding but I can have this done in about 10-15 min.

_________________
________________
Jeremy Vonk

Looks like you're getting a good finish. How much stepover do you run on the finish pass?

And cutter size, of course. Without the cutter size, the stepover doesn't tell much.

That's a nice looking neck, though the cycle time can definitely be shortened a lot unless the machine has a 5K spindle.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Nice looking neck! I am interested in your spindle speed and cutter type and size as well.

_________________
Reguards,

Ken H

Hey guys...I'm running a .5", carbide ball endmill. .025 stepover. I am running at 5K spindle speed and about 40"/min. I am using this cutter setup for no other reason than it's what I have on hand.

Here is a picture of the guitar body that this neck is going into....carved with the same setup

_________________
________________
Jeremy Vonk

Nicely done!

Thank you

_________________
________________
Jeremy Vonk

GREAT JOB!!!

I have to say, those look really good.

What software are you using for Design and Machining?

Keep up the good work!

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

Thanks for the compliments. I am using mastercam for my design and tool paths. I have been wondering if Rhino wouldn't do a better job on the design side though. I just don't know if I can get my brain to switch...

_________________
________________
Jeremy Vonk

Rhino will do a better job in design, it has a lot of surfacing tools that MasterCAM doesn't.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I'm curious if you used the CNC to route the channels for the wiring and POTS also? If so, was this done prior to the glue up of the top? I have been looking at something similar, but find that it would most likely be necessary to do it in a 2 step process because of the wiring channels. Just wanted to get your input on this? How did you handle it?

_________________
Reguards,

Ken H

Hey Ken,

When I made this Les Paul, I did the mahogany body and the maple top separately.



http://i202.photobucket.com/albums/aa201/jer7440/P1010100.jpg



I cut the mahogany body first, and I put in the control cavity and the wire chase at this time...I also drilled in 3, 1/8" dowel holes that I used to align the maple cap. When I cut the maple cap, I started with the maple "upside down". I cut the outside perimeter and drilled the corresponding blind dowel holes. Then when I was ready to carve the maple top, I again used the 3 dowel holes only this time I drilled them into a piece of MDF, then I lined up the maple cap and stuck it to the mdf with double sided tape. After carving the top I used the dowels to line it up the the mahogany base and I glued the whole thing together.

The biggest problem I ran into working with the body parts individually was the expansion and contraction of the different woods. I had to cut my maple cap quite some time after the mahogany body (it was almost a year later because I destroyed my first maple cap) and even though I used the exact same cad data the two pieces didn't line up very well because the mahogany had changed from when I cut it. I ended up setting the whole thing up and creating a binding channel to fix the problem.

With the PRS style guitar I am working on now, I started with the alder body and the maple cap already glued together. I started with the alder side up and I cut the outside contour of the body and the control cavity and the ledge for the cavity cover. Then I cut a 1/8" deep pocket in a piece of MDF that would hold the guitar in position after I flipped it over. I use double stick tape to hold the guitar in the pocket. Then I route the pickup cavities and the neck pocket and then carve the top. I plan to use a long drill to put in the wire chase (hand drill).

Both methods have their positives and negatives. If you do cut the body and the cap separately, just make sure you machine them close together time wise. I by no means have this process perfected, but these are the ways I have tried.

_________________
________________
Jeremy Vonk

Sorry to bring up old posts but I have a few questions. I've been making guitars over the last 15 years and now I'm doing it with CNC. I pretty proficient in CAD and certain CAM packages but still am falling short in a few areas. I'm using Rhino and had tried RhioCAM and it didn't seem to work very well. Then I got a trial, full working, of MADCAM from a friend who is a reseller of it. He's helping me out but my neck carving simulations come out pretty rough. When I model something in Artcam, even importing the CAD I drew in Rhino, the simuations come out smooth. But you really can't use artcam effectively with imported 3d stuff, plus I want to be able to do it in Rhino. So I guess my question is since a lot of people out there are using Rhino what are you using as a CAM?

I use RhinoCAM basic...it's adequate but certainly not fancy.

_________________
http://www.PeakeGuitars.com

I know this might not be good from a cost $$$ perspective, but Mastercam X2 is basically one of the best if not "the" best CAM software package. Gibson, as well as Taylor are using it every day to cut their guitars and fixtures.

I said cost, since it is not cheap at all, but earlier versions (like 9) had substantial student/small shop discounts. You might be able to find a reseller that will be willing to get you some deep discounts (it is worth a try). Head over to their site, and hit some local resellers.

As far as simulation, all CAM packages will have some sort of an integrated simulator, but this DOES NOT in most cases test the G-code! What I mean by that, is that you can get a good simulation, and you might have a line of g-code that will gouge your part that the simulator did not pick up. I have found the simulation of Mastercam to be great, but again, no g-code testing.

So, this is where third party simulators come in. Vericut is one of the best

http://www.cgtech.com/usa/index.php

These will actually simulate from the IMPORTED and POSTED G-code generated, so they are testing the "actual" cutting instructions that a machine will see. As such, it is a lot more accurate, and they can spot mistakes before happening.

Some others are made by:

http://www.cimco-software.com/
http://www.brt-solutions.com/ncsimul.htm
http://www.predator-software.com/

(Predator is popular as well, but not as popular as Vericut).

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

There are a lot of reasons that a simulation might not be an accurate view of what is actually going to come out the other end. The way the simulation is rendered has a lot to do with how the simulated model is going to look and, past the most basic 'huge vs small scallops' view, you can't tell a whole lot about the part finish unless you're using high-end verification software (like MetaCut or similar). Even the MasterCAM verification should be taken with a grain of salt. It'll tell you if you're going to crash into the part, and if you're missing some areas, but I wouldn't trust it entirely on part finish. So, the answer is that you either need to understand what your toolpath is doing, buy high-end verification software, or go cut a part to be sure about surface finish.

MADCAM all of a sudden got really expensive (when I bought it it was like $500 for a seat!), but it's a very capable piece of software. RhinoCAM will do the trick, as well. If you can machine along curves in your CAM software, then Rhino has all the power you need to generate nearly all the toolpaths in any but the highest-end CAM software if you understand what you're doing and how they work.

In my view, Visual Mill puts out a better value per dollar than all of MasterCAM's offerings except level 3 (ie: if you don't want to spend more than 10K, then MasterCAM is out of the competition).

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

yep, mc is def'ly overpriced. Not to mention their proprietary file formats and the "almost" windows interface (reminds me of AutoCAD pre release 12...)

_________________
http://www.PeakeGuitars.com

I'm getting into this thread late, but I use BobCAD/CAM for all of my CAM work. So far it has done everything I have wanted it to do.

One of the "tricks" to getting the machine to give you a finished look is to tell it to overlap the cuts. In other words, if you are using a 1/8" round nosed bit, tell the CAM software to overlap it by 40 to 60%. This will usually end up with almost sanded finishes.

You can rough cut most of your work using standard toolage, then do a final cleanup using the overlap method and taking off very little.

_________________
Reguards,

Ken H

That's the standard practice with milling, Ken. When using a half-inch ball, to get a good finish on a flat, you'd be looking at 0.015-0.025" or so of stepover (ie: only moving it 3-5% over each time). Even in roughing the passes shouldn't be full-width of the cutter unless you're leaving a lot of material for the finish pass.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Yep, on this neck my cutter was a .5" ball nose and I used a .025" stepover. Very little sanding was required after machining.

_________________
________________
Jeremy Vonk

Bob good info in your post. I agree on the simulation problem and would like to comment on the increase in price of Madcam. I am the US reseller of Madcam and have some insight on what has happened in the past as well as what is planned for the future. When the decision was made to make Madcam4 with 4 and 5 axis capability, it was then decided (before my time) that the price needed to increase to reflect the added features, and my understanding, to keep it in price line with the other software similar.

I can tell you that a new 3 axis version is about to be released that will not have the 4/5 axis, and is going to be very affordable. Upgrades will be affordable as well and we are attempting to develop a competitive upgrade but there have been no real decisions made on that.

Madcam was developed as a [color=#0000FF]M[color=#000000]old [color=#0000FF]a/color]nd [color=#0000FF]D/color]ie cam system based upon Rhino and the surfaces it can work with. Only after I came on board as a user did Joakim get real serious about wood working due to my constant

If I can be of service to anyone who wants to try Madcam, ask questions etc, please feel free to contact me.

Mike

Mike, are you following me around the web...LOL. Did you know it was me, Carter?

Hey Carter,
I knew it was you, because like me, you use the same user name several places! It is amazing to see it really is such a small world!

Mike

Hey guys, I thought I would throw up a couple of pictures of the fretboard I made up for this neck.

Here i s the whole board.



Here is a close up of the inlay at the 12th fret.

I did everything but the fret slots on my cnc.

_________________
________________
Jeremy Vonk

Those aren't Dr.Sholl's Corn Pads are they? The finger board looks great. Nice work.

_________________
Waddy

Photobucket Build Album Library

Sound Clips of most of my guitars