Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Guitar Neck CAM - straight or round nose bit?

fritter63
Collaborator

Guitar Neck CAM - straight or round nose bit?

fritter63
Collaborator
Collaborator

Hi all, hoping for some advice on the best way to machine the back of this guitar neck, including the heel. See picture.

 

I've read that a round nose bit it best for finishing? Is that true? The problem is that if I use a round nose, I've got to cut deeper on the

sides where it meets the spoilboard to get a nice straight edge. However, I also still need to use a straight bit to clear the junction

where the heel meets the finger board cantilever. So why not just go ahead and do the whole thing with a straight bit? (I'm finding

it difficult to restrict the cam to just that area and still get it to cut into the angle). Can I get a nice finish doing that? Should it just be tiny stepovers? 

 

For that matter, would the stepovers be any different on round nose vs. straight?

 

Hoping that  can chime in here since he recently did the 3D guitar demo with CNCRouterParts.

 

Thanks.

 

RoundedHeel.jpg

0 Likes
Reply
1,658 Views
6 Replies
Replies (6)

daniel_lyall
Mentor
Mentor
it would be easier to do it in two ops if you get a tapper fluted ball nose, you don't have to over run with them, for the angled bit do a project on to it off the outline and leave the drawing turned on then you select the drawing as your cut profile and it will cut it to the angle, It's a not that known trick fusion can do or (drawn tool paths). if not sure post your model and I will show you. the step-over is a bit different depending on the size of the cutter and angle at flute tip


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes

RandyKopf
Collaborator
Collaborator

fritter63

I machine 3D shapes all the time for my main job. complex mold shapes etc. So I see some things that I'd like to point out. IF you want to end up with the actual shape you have modeled then the actual geometry dictates what tools you need to use. 

 

Just like Daniel Lyall was saying need at least 2 tools.

So I would break up the job based on key areas as follows:

 

1) The area I highlighted below in a green ellipse has a very small fillet and it would need a small ball mill to machine like maybe 1/4" diameter.

 

2) The other end where the neck meets the body shown with a blue line has a sharp corner, it would be best cut with a flat end mill maybe 3/4" diameter something with long flute length.  

 

3) The the area you are most concerned with is the main neck shape. What will be a challenge is the area I highlighted with Yellow arrows. The downward arrow would be best machined with waterline type of milling with a ball mill maybe 3/4 diameter. The yellow arrow that is more horizontal would be surfaces that would be best finish with a parallel cut.

 

4) Finally as for the red line I show at the bottom, you are concerned a ball mill would drop below... Mount the part onto a 2x4 and elevate it and don't worry about dropping lower.

 

Hope this helps...

 

:slightly_smiling_face:

Randy Kopf

http://desktopartisan.blogspot.com/

 

2016-04-11_21-22-00.jpg

Randy Kopf 

http://desktopartisan.blogspot.com/


If my post is helpful, press the LIKE Button If it resolves your issue, press Accept as Solution! Have a great day!
0 Likes

nathan.skalsky
Advocate
Advocate

Hi Fritter, 

 

You asked Jeff or I to chime in - however I think you already have good advise.  

 

If you watch our guitar video you might notice that we never used a ball endmill, it was pretty much a one-tool-wonder .25" Flat Endmill.    We got away with that because the surface of the guitar was purely convex so the edge of the cutting tool could be used (with a stepover of 0.05") to impart a smooth curve.  

 

Using a flat end mill - I've found you do indeed have to use finer stepovers - the exact value depends a bit on the material and geometry.

 

 

For the neck, I think you are best served (as previously metioned) by using both a flat and a rounded tool in two distinct sets of operations.  

 

You can probably see in our Ukulele neck below that we have the round nose tool extending well below the body to get the well-defined contour edge.  

 

Stepovers, you might use the simulation preview to get a sense for when things hit diminishing returns.  I used 0.0125" here - obviously its a balance between machining time and finshed part resolution (and sanding).  

Screen Shot 2016-04-11 at 10.21.32 PM.png

 

Good luck - let us know how you get on!

 

-Nathan

1 Like

daniel_lyall
Mentor
Mentor
if you use one off those tapper flute ball mills you can drive them very fast this one I use at 1250 mm/min at 21000 rpm 2mm depth of cut 25% stepover they last a long time and do a very good job http://www.toolstoday.com/p-6225-solid-carbide-spiral-cnc-2d3d-carving-tapered-and-straight-ball-nos...


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes

rumpelstielz
Collaborator
Collaborator

@fritter63 wrote:
The problem is that if I use a round nose, I've got to cut deeper on the

sides where it meets the spoilboard to get a nice straight edge. 

 

what i did was to cut the outline of the fingerboard from the topside first to a depth that overlaps height of the ball mill i'd use for the back of the neck. I used a 6mm ball mill for the back so i cut the outline with a flat mill from the topside to 3.5mm deep (3mm is the radius leftover the ball mill will leave on the other side). for me this worked because my fretboard is 5mm high and i'm keeping the edges of the fretboard straight and only start the slope of the back of the neck at the fretboard bottom. If your back neck radius is completely curve including the fretboard edges in the curve this will not work.

 

 

that way when i cut the back with the ball mill i don't have to go into the spoilboard. But you could also just mount the neck on a separate spoilboard, piece of MDF or scrap wood to gain a bit more height for the ball mill operation of the back.

 

in total i used 8 operations for this neck:

 

Topside:

- drill reference holes to align the fingerboard when gluing and reference holes for the tuners on the headstock part)

- contour the outline of the neck with a flat bit

- rough out the headstock with flat bit (adaptive clearing)

- parallel finish the headstock

- cut the truss rod channel with a flat bit (slot or pocket)

- cut a slot for the nut to align and fit

 

Backside

- rough out the neck (adaptive) .. make sure to leave a bit of extra stock to avoid cusps after finishing .. i typically use 0.25mm to 0.5mm (depending on the wood type, for highly figured wood that tends to tearouts i leave more stock, the ball mill minimises tearout on figured wood i've learned

- parallel finish the neck with a large ball mill and tiny stepover (6mm ball mill with 0,2mm stepover)

 

Little tip: while you're already milling the neck, make yourself some 'negative shapes' as neck rests/clamps .. they will come in handy for gluing, fretting and finishing:

 

==================================================
GENERAL DISCLAIMER: if there isn't a file attached to my posts then there is a reason for it. wherever i can i will attach a file for troubleshooting.If no file is attached i will always try to explain as clearly as possible with illustrative screenshots. when i have an issue that can only be helped by attaching a file which i cannot share publicly i won't ask about it here.
1 Like

Anonymous
Not applicable
You didn't really say if you are just making one of these or hoping to make 50 of them (or more). The best approach will always vary depending on factors like production numbers required, machine capabilities and tooling available.

That said, I would recommend having a look at the video at the link below. I used to work in the Gibson Montana factory and I've toured other factories as well (to get ideas of how others are doing things). In my opinion, the angled fixture that Gibson used to shape the back side of the necks is the best solution I've seen. It takes a machine with enough Z axis to make it happen, as well as the ability to put a pretty large lollipop bit in, but it's a sound approach to a difficult shape.

You are going to have to use more than one bit to do anything on a CNC router, so best thing is to just get used to changing bits when needed and learning to be efficient with the steps involved. Whether the machine changes the bits for you or you have to do so manually, a one bit fits all solution is not a great idea.

Good view of CNC fixture starts at about the 3 minute mark:

https://www.youtube.com/watch?v=bp_PM60SAFc

Also, the largest round end bit that can fit into any shape is always going to produce the best finish to a complex surface. The bigger the ball end, the closer to a tangent the cut surface becomes, so the step over is more similar to tangent/tangent rather than dish/dish, meaning that there will be a smoother finish resulting.
0 Likes