Official Luthiers Forum!

Hello, this is my first post on this forum although I've been on the MIMF for some time so maybe some of you have seen me before.

I'm looking at getting a CNC this fall to open up shop making a line of electric guitars (just me, stock and custom). Right now it's looking like a Techno-Isel 4x8 with a manual tool change (I'd really like an auto but it's going to be another 10K). The 4x8 because the price difference between that and a 4x4 is minimal.

What I'd like to do is talk to some of the guys in here about modeling parts for CNC and maybe get into methods a bit. I use Rhino and VisualMill.

Things I wonder about:
What sort of tools and feedrates should I use for the various woods? I'm going to go with a big core box bit but I have no idea how fast to feed it into a piece of rosewood as most information is published for metals.

How does one get a Les Paul type carved top to come out right in Rhino? I've had a pretty bad time with this one. Lots of posts on the Rhino user group and still can't get it quite right.

Do you guys have any good luthierly advice? Machines or tools you've liked/disliked or things you wish you'd known before you destroyed a nice piece of wood?

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Welcome to the OLF Bob!
I know nothing about CNC'ing but there are several very knowledgeable guy here that do, I suspect they'll chime in soon.

_________________
Support the OLF! Bookmark our STEWMAC link Today!
Lance@LuthiersForum.com

I'll be happy to share. You've touched a lot of ground in your post so I'll take a whack at some of that.

I've got a Techno, it's not 4x8 because I didn't have the room, otherwise definately a good idea because you can have multiple fixtures permanently mounted to the table and not have to spend time aligning them.

I use Rhino for a lot of my modeling along with Onecnc although I have a copy of VM. I can help with the carved top modeling; there are several methods however I've had the best results using a patch surface over a set of guide curves created by offsets from the body perimeter. Here's a sample singlecut top, the dish is only 1/32" the rendering makes it seem like more.

Speeds and feeds are something you are going to have to tweak for what you are doing. For finishing operations I'll go 100-150 ipm easily, for roughing I may be down at 75 ipm. The machine accelerates up to the speed you indicate so the smaller the area to be machined, the less real cut speed you can have. You could buy big $ servos to cut at 1000 inches per second but if you are cutting a 12" wide solidbody it cannot ever get to that speed over that distance. There's obviously a point where you overrun the power of the spindle/bit and rip the wood off the fixture or rip it apart so there is a balancing act. Techno can help size the machine right and you'll have to work out the rest.

Shoot away with more specific questions and I'll try to help.


Rand Kennedy38840.5486574074

What Techno model and spindle are you using? I guess the spindle and the drive type would be important with reference to feed speeds and whatnot.

The 4x8 is more so I can rent it out to cabinet shops than because I need the space. The cost difference is negligible. Is it a hassle to realign jigs and fixtures? I was hoping to use vacuum fixtures clamped to the T-slots (driven individually by an outside vacuum pump).

I've never tried using guide curves and patch surfaces. I've tried lofts, curve networks, rail sweeps, but each of them had their own particular problems. In the end the best solution I've found thus far is to do it in two parts but if I can just use straight curves that would be golden.

How is OneCNC for toolpathing? I think VisualMill is OK and quite adequate but it doesn't have the smoothness of most of my other apps in use.

I look foreward to hearing from others and maybe sharing some techniques, moreso once I've had time to experiment with my machine (which will be after I actually -have- a machine)

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I can't offer any techniques but I'm paying very close attention to what you guys are using and doing

I just procured a CNC machine, couldn't afford the Techno Isel so I wen't with the K2 machines, I'm also using Rhino and have Rhino Cam in the package I got. Since this is my first foray into CNC I had to keep costs down while I learned what I can and can't do...

Your both way above me in knowlege but I'll get there someday

Cheers

-Paul-

_________________
-Paul-

Patriot Guitars

I've got an 053 gantry machine with a 3HP HSD spindle. My woodshop is in the basement and I don't have 3-phase so I had to go with the smaller machine although I can't say I need more HP or cut speed. Aligning fixtures so the reference points are in exactly the same place does take some time & effort. 2 sided machining of interlocking parts can double or worse the error.

Here's a picture of that top with the contours. With a patch surface the geometry is there to help guide the surface so curve continuity isn't critical. The offsets are at different Z heights to create the proper dish and arch. There is more geometry for the bridge, pup and neck joint planes. Because it is stretching a surface over the guide curves it isn't going to follow them as exactly as it would a wireframe so some tweaking and trimming to the body perimeter may be needed.



Onecnc's CAM is excellent and very easy to use. Visual Mill is a good product but I prefer Onecnc hands down.

Sprockett - you know the old saying, it ain't the tool. I'm sure your K2/Rhinocam will do fine. There are so many ways to skin the cat with modeling and machining its the creativity of the designer/machinist and all that sanding that drives the end result.

If there's one thing I know now, it's how much I don't know....

Drawing 2D layouts in CAD is VASTLY less complicated than doing it in 3D and I haven't even started to play with Lofting or any other advanced topics.

I haven't even got to the CAM software yet, Rhino is so rich with features that I'm still figuring out what it can and can't do.

Do either of you know of any good books that breakdown 3D design in a logical common way?? The Rhino manual is actually pretty good and I bought some training manuals from one of their vendors but there is a great deal of terminology that they don't define very well. Like Elevator mode, it would be good to have a clear concise definition of some their terminology...

Thanks

-Paul-

_________________
-Paul-

Patriot Guitars

If it makes you feel better, I've been using 3D modelers for years and I don't know what Elevator Mode is. The best I can say to help you get started is to do some tutorials, learn the basic tools (curves, lofts, rail sweeps, extrusions), and ask questions on the Rhino newsgroup once you think you've really hit a wall.

Do you prefer OneCNC for toolpathing or for its modeling capabilities? I only need toolpathing software. Their website is not at all helpful at explaining why anyone who knows what they're doing should want their software instead of someone else's but that doesn't mean it isn't better just that they're not very good at explaining why.

What sort of tooling do you use for your roughing and finishing passes? Right now I'm looking at getting 1/2" chipbreaker bits for roughing and then a big (like 1.5") core box/ball end bit for finishing passes. How much scalloping do you find acceptable off the machine and how long does it take you to machine say a solidbody top?

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

There are lots of nuggets in the level 1 & 2 training materials on the Rhino CD but download updates for those first. ob.com has a bunch of tutorials and models for free as well as some more advanced training cd's.

I hybrid model doing most in Rhino and perhaps 25% in Onecnc's modeler which has much better precision but limited freeform curve & surfaces features. You have to call to get an online demo with Onecnc which is OK since it's better to see it run than read some marketing stuff. In my demo I discovered I could reduce cut time by 30%+ with smoother surfaces on a carved top I had worked with MEC to optimize the program for in VM5. If you already have VM, heck use that. They have version 6 coming out this summer which should be better.

I don't like the chipbreaker bits in mahogany or maple although they are nice for ripping up plywood/mdf. I use carbide spirals for most pocketing and generally a carbide tipped straight bit for profiling where I want a really clean edge. The 1" core box seems best for my carved tops and I think I step at around .075" for finish and scrape & sand the rest; scallops are only a few .001's. Stepping too fine compresses and hardens the maple making for more sanding time.