experiment on machining a guitar neck (tele)

Maching out a tele guitar neck.
An experiment as its much simpler to purchase the neck than making one.
But i had never machined out a 3D object so this would be a good start.
I used cut3D but it would not allow tabs 2 good heavy duty tabs at either end would have helped
as i selected .25 overcut so there would be no scrap wood left to hold the
neck in place.Secondly i should have allowed about 4 in at either end.
Then you need a fairly long end mill ,mine were 1/2 flat/round end 3 in long so about 2.25 is
ready for machining ,but i could have used about 2.75 as it was hitting the collet.
Not sure if you can get 3.5 in 3/8 or 1/2 end mills that long.
And its a very slow process,but did work and if i would have had better alignment when i flipped
the blank 180 degrees it would have machined more accurate.
Also the z=0 should be a standalone reference as when you do the first rough cut you loose your reference spot ,but it was the first and i will try it again with improvements

http://www.youtube.com/watch?v=M_sz0TTaLiw

Hi Stan,

It looks like you've got the whole thing up on its narrow side(s)? Life will be MUCH easier if you machine the neck face down/face up, and not standing up on the side like that. You can devise a strategy with tabs or without. Feel free to PM/email if I can help.

-Mike

because most necks have an angle on the end where the strings are fastened i think you have to machine it on the sides,or in the worst case all 4 sides.
I was all set to machine the face flip it machine the bottom but the tele has a slight angle some are 15 degrees

Every neck I've ever seen cut was cut fretboard down. I've never seen anyone do it on edge.

Quote:

---

Originally Posted by stan kern

because most necks have an angle on the end where the strings are fastened i think you have to machine it on the sides,or in the worst case all 4 sides.
I was all set to machine the face flip it machine the bottom but the tele has a slight angle some are 15 degrees

---

You're right, a lot of necks have an angled headstock. But the tele isn't one of them.

A traditional one-piece (50's style) neck is milled from ~1"-thick flat stock. The break angle of the strings down over the nut to the tuning pegs isn't from an angled headstock, but rather from the drop created when the headstock is thinned to a little over half the thickness of the rest of the neck.

Like I said, you can use tabs, or not. I prefer not when possible because I can use stock more efficiently that way.

The back of the headstock and the back of the heel end are coplanar faces and remain so even on the finished product. So that gives you a reference plane to work from throughout the machining process.

Ignoring the truss rod for the moment, for simplicity's sake, think about this sample schedule:

1. Workpiece fretboard side down on the table, machine the outer perimeter of the neck.
2. Machine the curve on the backside of the playing area/shaft of the neck.
3. Flip the piece fretboard side up, mill the headstock thickness dropoff.
4. Mill the fretboard radius, fret slots, dot marker holes, etc.

-Mike

you are right the tele is one without an angle ,ok will try it again.I only have 2 *.stl files for neck try outs the tele and one other with a 15 degree .
So what are you saying about holding it down because the cnc will cut it right out and chances are the neck will move into the cutter,also is a 1/2 bit to big,i used 1/2 because its the longest i have

Quote:

---

Originally Posted by stan kern

you are right the tele is one without an angle ,ok will try it again.I only have 2 *.stl files for neck try outs the tele and one other with a 15 degree .
So what are you saying about holding it down because the cnc will cut it right out and chances are the neck will move into the cutter,also is a 1/2 bit to big,i used 1/2 because its the longest i have

---

I'll see if I can attach some pictures here since I'm not great at explaining this stuff. The pics show the piece on the table with tabs and without.

Whether I use tabs or not, I put 1/8" diameter holes in the wood and in the table and use 1/2" long pins to keep things from shifting side to side. The holes and pins keep things aligned even when flipping the piece. Double-stick tape (no tabs) or screws (with tabs) provide the hold down. If I'm using tabs, the alignment holes and pins can be outside the perimeter of the neck. If I'm not using tabs then the holes and pins need to be on the neck itself. I deal with that by putting the holes in a spot that is either hidden (like on the heel) or in a spot where I will eventually need a hole anyway, like a tuning peg hole or a mounting screw hole.

1/2" diameter bit is not too big - I use a 1/4" or 1/2" flat mill for the 2d cuts and a 1/2" ballnose for the 3d cuts. Machining the neck flat, you only need 1" cutting length on the bit. I think mine are actually 1.25" cutting length but the material is only an inch thick...

tried a different method after some suggestions about doing top and bottom and it worked fine and because i used a board about 6 in wide
i was able to add tabs which turned out very good .But i used z=0 at the bottom left and when i flipped the board i was out by 1/8
so it looks like z=0 should be centre of the project and i also used 3/8 end mills probably a better finish.
Turn
http://www.youtube.com/watch?v=tx5b41uwTd8 guitar neck 2 2nd
http://www.youtube.com/watch?v=h6WNV9MXEIA cut3d videoed out ok

thanks for your help mike ,i am almost there .
Where did you get the *.stl file for the neck as they are not posted as often as bodies

Quote:

---

Originally Posted by stan kern

thanks for your help mike ,i am almost there .
Where did you get the *.stl file for the neck as they are not posted as often as bodies

---

Looking great now!

My pictures are of a neck of my own design, different overall length, heel design, headstock, etc. I don't have an STL of a tele neck handy. I'd be wary of most of them found online. It seems like anytime I download a CAD file anywhere, it's never quite right...

mike
are you using z=0 centre of the whole project ,then flip your blank using the pin to also check the alignment of the blank.
I'm still not 100% accurate when i flipped the blank .

Quote:

---

Originally Posted by stan kern

mike
are you using z=0 centre of the whole project ,then flip your blank using the pin to also check the alignment of the blank.
I'm still not 100% accurate when i flipped the blank .

---

I set Z=0 to the top of my material for everything I do. And XY zero is at the bottom left corner. That's just how I draw things up and it just seems easiest to me. I don't have a touchplate for zero'ing or anything yet - I do it all by eye, so setting Z=0 to the top of the material works best for me for now.

What I'll do usually first is cut the pinholes on one side of the workpiece (either with a template or with the CNC itself) then immediately mount the piece to the table with those pinholes and cut the pinholes on the other side as the very next operation. That way I know the alignment is good front to back and any alignment issues I run into are not a result of those pinholes being out of alignment. If the pinholes are good then any alignment issues would have to come from the machine being off zero, or problems with the toolpaths/files.

Are you using only Cut3d? Or do you also have Cut2d/Vcarve?

I am using cut3D and i also use the surface for z=0 but i think now the reference would be better at the centre and also having the pins after
say one side is machined and you punch 2 holes right through ,so when you line up the centre will be used but the final check would be the pins
My xeroing is the same as yours

*************************