Jump to content

Guitar Design

Recommended Posts

Hello. I have been working in Rhinoceros to design a guitar for personal use, to be cut from CNC, and was looking for critique along the lines of design flaws, potential problems, etc;

I wanted to design a hardtail 24-fret guitar, explorer style (but profiled to be lightweight, similar to an Ibanez S Series design), 2 humbuckers, 25.5 scale. So, some specs on the model as of right now:

Width of neck pocket: 2"

Width at nut: 1 11/16"

Length from nut to center of bridge mounting holes: 25 1/2"

Humbucker pocket specs from Hill Instruments website.

Neck Radius: 10" to 16"

The frets are on the model simply for display.

How CNC-able is this model? Any advice at all would be greatly appreciated.


Edited by Maiden69
Link to comment
Share on other sites

Do you have a CNC? The reason I ask is that I have a new CNC and also use Rhino. I'm just looking at the learning curve for building a guitar or two as a hobby for myself (I use the CNC for other purposes during the day). I've thought about cutting a body/neck or two just to get experience with bit selection. Let me know if you want me to play around with your file. I'm struggling to find spare time right now, but where there's a will...

You know, of course, the neck needs to be separated from the body before any toolpaths can be written. Otherwise, I think its looking pretty good. How do you plan to run the pickup wires to the other cavity? I'm also guessing the fretboard needs to be cut separately (or purchased).

Link to comment
Share on other sites

Do you have a CNC? The reason I ask is that I have a new CNC and also use Rhino. I'm just looking at the learning curve for building a guitar or two as a hobby for myself (I use the CNC for other purposes during the day). I've thought about cutting a body/neck or two just to get experience with bit selection. Let me know if you want me to play around with your file. I'm struggling to find spare time right now, but where there's a will...

You know, of course, the neck needs to be separated from the body before any toolpaths can be written. Otherwise, I think its looking pretty good. How do you plan to run the pickup wires to the other cavity? I'm also guessing the fretboard needs to be cut separately (or purchased).

I don't personally have a CNC, but a friend-of-a-friend does.

The file can be split up, any part isolated. I was planning on hand-drilling holes for the wiring.

If you'd like, I can send you the file, there are some parts that need re-done before I can (the neck pocket isn't completely squared away, I plan on lowering the "horn" on the right a tad to provide more access to upper registers, etc; etc; etc; nothing is ever really finished with me.)

Oh, I didn't mention this in the first post. The bridge is drilled for the Schaller 456 Stop/Tail w/ Fine Tuners. Haven't done the tuner holes yet.

Link to comment
Share on other sites

I'm game if you are. I have two CNCs, a 4'x8' bed (new) and a 19"x14" that I've had for about 8 years. Up to this point I've only cut 2D using Bobcad/cam. Rhino is new and I'm working through tutorials as time permits (vtc.com). The CNCs work for me during the day. I should have some time at night to start burning through the learning curve on making guitars that I enjoy playing. Free time is so valuable right now that working with someone on design might be the way to make it work.

Finish the drawing and let me know. We can exchange a PM to get email addresses. I have a webcam here in my workshop studio hooked up with MSN messenger. That might be a useful tool.

I'm just wondering... does anyone make a carved top version of an Explorer? I'm dying to try a carved top design. There's just something about the "plump-ness" of a carved top, and the CNC can do it so easily. This is just a thought. Maybe something to try in the future.

I just want to have some fun. I told my wife that this is the first thing I've done in many years which I'm doing just to have fun. Everything else seems to be to fulfill some responsibility, either to my business, wife, kids, house, family, etc., etc.

Link to comment
Share on other sites

wow awsome design...i have rhino too but im too dumb to work it so i just screw around and try to make weird shapes lol

There is no such thing as too dumb, it's just a matter of time.

Here's a quick little tutorial:

In the Top viewport, load a guitar design (Optional)

Type "InterpCrv"

Trace the guitar design, paying attention to corners and horns. You'll probably need more points in the corners to get it right. If you're freestyling (no design in the backround), you may want to allow yourself more points then necessary.

I can't think of the next command, but with your curve highlighted, turn control points on. (I think the command might be "ControlPointsOn". You'll get a display of all your point, and now you can tweak your curve to your specifications. This is why I said freestylers should leave more points in, so you have more to tweak. You can also delete points here that are causing problems.

When you are done, hit the escape key to turn off the control points.

With your curve selected again, type "ExtrudeCrv". Before you extrude it, check to see if in the command bar it says "Cap=Yes". If it says "Cap=No", type "C" and press enter to turn capping on.

This is a bit of an idiosyncratic step, but I think it works pretty well for guitar design. When it asks for extrusion length, type "1.75" (For a 1 3/4" thick body. If you're doing something thicker/thinner, your value will change.") Don't worry if your guitar appears chunky at this point, because it's actually at the proper height, and the length and width are wrong.

Select your body and type "Scale2D". This will uniformly scale your length and width without changing your height. You may want to use the Perspective viewport for reference so you can get a good idea of how the guitar looks when you scale.

Voila! A simple guitar body. To do any pocketing, you're going to use the command "BooleanDifference". If you want to round the edges, use "FilletEdge". Play around with it!

Link to comment
Share on other sites

"How CNC-able" is an unfortunately enormous question. If you have access to a 5+ axis machine with exceptionally accurate servo controllers and a good CAM program, almost anything is "CNC-able."

(Note to machinists, the following is simplified for the sake of some brevity and consumability, so be nice.)

Now, CNC, as in Computer Numeric Controlled, merely means you have a machine that is taking code from a computer and translating it into moves in 3D space primarily as moves in lines and circular-arcs between eithe relative or absolute coordinates. That is, in laymans terms, a CNC controlled machine will do things like move the cutter from one spot to another by 2 inches if you tell it to.

The most common CNC machines for guitar building, and probably the only ones you'll get access to, are 3-axis vertical milling centers. A 3-axis VMC has a spindle that spins various bits you chuck in there and moves them up and down in the Z-axis. Underneath is a table which moves sideways and front to back in teh X and Y axes respectively. Combining motion in the 3 axes allows the machine to make 3D cuts which, when combined over many passes, will result in sculpted surfaces.

For woodwork most non-hobby (i.e. you didn't make it yourself and it sits on the corner of your workbench) CNC machines are primarily limited by the axes it has as the accuracy it can achieve and the power it can drive tools with are far less relevant for wood than metal. With a 3-axis machine you can only make cuts that you can see from above, namely that the bit can reach from it's vertical position. You can't make undercuts or carve underneath edges. Iit may seem obvious to some, but you clearly can't cut the back of a guitar for a body cut when it's behind the rest of the guitar, the tool would be hacking out the desired body to reach the material behind it. The reason I mention this is this goes from small overhanging features too. On one part of your carved top, near the horns, it looks like the carve goes vertical and maybe past it. Have to be carefull there.

Now, once you have a 3D shape you can carve from above, it's pretty easy for most industrial CNC machines to cut them, but that's not the end of it. The CNC machine is driven by NC code, called G-code and composed of numbers and letters carefully constructed to tell the machine what to do and where to go. The creation of G-code is often the hard part of the machining operation. The CNC machine will dutifully do what it's told, but if you give it bad instructions to follow you will get back bad results.

You can write G-code by hand (hard and tedious and nearly impossible for anything but the simplest 2D shapes) or you can generate it by computer on a CAM program. Rhino is a CAD program, Computer Aided Design or Computer Aided Drafting, and is used to create the digital shape. A CAM program is Computer Aided Machining, and it takes your file from Rhino and, with a whole lot of your help, figures out how to machine it using your CNC machine. When you're done telling it how you want to be cut, it writes the code for your CNC machine.

This is where many people get stuck, CAM-work is an artform just like CAD-work. Machining is an artform just like hand-woodwork. (With CNC once you get it right, though, then it's button pushing and the art portion is finished.) It's not like a afile conversion, as easy as finishing the Rhino file and "saving as" a machinable file. You have to send it to a program like MasterCAM, choose and set-up your tools, set the speeds and feed, determine the cut type you want to use, the order of operations, debug the code for glitches, run tests on actual stock to make sure it works, and once it's ready for production work.

A good machinist, can do that in a day or so, but they've got real experience and skills that you don't.

Then, once your model is done and your CAM is done, only then can you hog out your nice piece of swamp-ash for your cool digitally created shape. Do not underestimate the challenges involved. Just because it is computer driven doe not mean is is mistake free or simple, just repeatable and with strong potential for accuracy.

ALL THAT SAID: CNC-mills are great tools, they do amazing work that would be almost impossible to replicate by hand. If you have the time and resources and don't want to do hand-work, then by all means use them.


Link to comment
Share on other sites

Wow, Dave, that was quite an articulate post. I don't think I've written that well since college, if at all. :D

My 3axis machine should have no problem with this design. Of course, you have to use a little enginuity to keep the machine's limitations from becoming an issue. For instance, I'd first create index holes in the outer margins of the wood blank. Then, I can rout the cavities on the backside before turning the blank over and doing the front. On this, I'd probably cut out the shape last. There are no undercuts in this body, and in fact, if the body took more than 20 min. to program, I'd be suprised.

The neck would be cut separately. The only issue I see is in drilling the holes for the tuning pegs and cutting the shape of the headstock. I'd probably rough out the head and then make a jig to hold the headstock for drilling the holes and doing any inlay work, as well as one finishing pass on the shape to clean it up. Nothing too tricky. Again, you'd need a system of indexiing to be able to do both front and backside, although I'd probably surface-plane the blank before machining and use that surface for attaching the fingerboard.

There are several different CAM programs, with varying complexity to their use. The speed at which this design can be programmed for onsie-twosie production should be fairly fast, depending on the skill of the programmer and the strategy the software uses to determine the toolpaths. Probably the most time consuming aspect would be thinking about what kind of jig to use on the headstock. That's one of those things you think about early in the morning before you get out of bed.

Link to comment
Share on other sites


Agreed for this shape all you'd prbably need to do is hog out the outline and then select the carve surface with a ball endmill and a ridge height of around 0.005" to easily sand out, or set it to 0 if you have all the machine time in the world. Not too many clicks in CAM once you know the ropes, but most packages have a steep learning curve.

Headstock fixturing... haven't thought about it since I don't have a VMC handy, but I think it depends on how you want to make the neck. If it's not angled but setback and remains parallel to the cutting plane like a Fender neck, no problem at all, just 2 operations. If you want to tilt that thing back 13 degrees or so it gets trickier for sure, especially for a one off. I imagine production houses, even small ones like Thorn, have production jigs to hold things tight and to the shapes and sizes they know they'll us in production.

I think for a one off, and pro builders with CNC capabilities can sound off here, I'd do something like this, keeping in mind this is only to do this once without spending too many bills on custom tooling and fixture nests, etc.:

1. Hand scarf joint and glue up the headstock angle between properly thicknessed blanks

2. Operation 1: Clamp the blanks in a soft-jawed vise with plenty of stock over the jaws. Face the neck for the fret board lamping surface (face mill or 3/4" end mill), slot the truss rod cavity (properly sized router bit). If working for a full blank and not a scarf jointed headstock you can hog out and surface the headstock face (3/4" ball end mill) from the billet and sand surfaced headstock paddle flat flat flat. Don't cut the headstock outline here. Also here blind drill 2 shallow holes (really one hole and one slot) for reference datums. Then separately make an aluminum plate with dowel pins for later alignment using this pin and slot.

3. Operation 2: Carefully align and double-stick tape neck blank to the aligning aluminum plate. You could also use a strap clamp to hold the flat heel of the bolt-on or set neck for security. Use a ball endmill to carve the neck to an acceptable ridge height, any volute, and the back of the headstock surface if carving out of billet. Cut the outline for the neck with a hard right angle leaving a paddle for the headstock. This face marks the start of the headstock and will be used later as a datum.

3. Here's where you could get really creative if you wanted to. I suppose the simplest thing would be to take that aluminum plate with the dowels for the truss channel or blind alignment holes and clamp it in a vise over an angle block to match the headstock angle. Tape the neck to the plate again and use an edge finder on the face meachined as a reference datum in the last operation and set that as your machine zero in that axis. Use the neck edge as the other axis zero or, better yet, use the plate edge and the datum pins to find your true centerline. Then push the button and cross your fingers. Cut the profile and drill the tuning machine holes.

I know to others out there in the machining or prototyping world that there are a whole lot of ways to skin a cat, but this method would probably work pretty well with some careful trammelling and only 1 semi-custom jig made of a plate with some alignment pins in a known location.


Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

  • Create New...