Help With Toolpath Creation For Inlays

[oldtbone55]

Hi All,

Been trying to create a toolpath for the recesses in a fretboard where inlays will be glued and I'll be darned if I can find a toolpath to do it. Since the recess is curved like the fretboard I thought a 3D pocket would do the trick but nothing doing. Seems like a straightforward toolpath to create but I've tried numerous other ones and nada. I've got all the other toolpaths worked out except for this one. Sure could use some help. I've attached my file.

Thanks.

[daniel_lyall]

So far redoing all the tool paths and setup is working, so for some reason, fusion does not like the setup and tool paths in your setup.

[oldtbone55]

Hello Daniel,

I'm not sure about what you're saying. How did re-doing the toolpaths work for you but the toolpaths I created not work in Fusion. I'm confused. Did you completely re-do the  toolpaths I had already done? 

Thanks.

[daniel_lyall · Accepted solution]

---

@oldtbone55 wrote:

Hello Daniel,

I'm not sure about what you're saying. How did re-doing the toolpaths work for you but the toolpaths I created not work in Fusion. I'm confused. Did you completely re-do the  toolpaths I had already done?

Just the one that failed and the setup I cheched with other toolpaths as well in the pockets you want cut, in your setup they where all failing in a new setup they where fine, this happens sometimes for no reasion. 

One of the things to do when a toolpath is failing is just do a new setup and do the toolpath again 99% of the time the new setup and toolpaths work.

Thanks.

---

[oldtbone55]

Thanks Daniel. I'll give that a try. This newer version of fusion seems to be a lot less stable than before. Maybe because I have a personal version?

[jda70az]

hello

I'm learning  guitar making and have a open builds CNC Lead 1010 and I looked at your file and I just wanted to say that

each inlay pocket is a unique shape. I know what it is, it's the Gibson inlay for a Les Paul .

I would just do each one on it's own.

What kind of bit do you intend to use to mill these out?

[oldtbone55]

I'm going to use 1/8" bit first to take out the majority of the material then an 0.023" bit to go around the perimeter to get the corners sharp. Each inlay doesn't have to be done separately even though they are all different. I know it's been done before.

I've looked at that 1010 and several others. I'm looking at building my own after seeing quite a few other builds. 

Thanks for your reply. 

[jda70az]

Hey I played around with that file  made a new fret board and new tool paths.

Hope you find this helpful in some way.

Feel free to ask any questions.

[oldtbone55]

Thanks for taking a look at the file and noodling with it. Spent some time going over what you did in order to understand it. Amazing the different ways you can approach this stuff. You obviously have a lot more experience at this than I do. I have some questions that I hope you won't mind answering. In my fretboard, the inlays/pockets follow the radius of the fretboard. Your inlays are flat at the bottom which means that at the ends they will stick out of the fretboard more than mine would. Does it really matter which pocket profile is used? Your method is simpler to do than mine. I was trying to make sure that the inlay thickness was uniform. If the pocket is flat then then the ends of inlays will be a lot thinner than the middle once you finish sanding them down level to the fretboard. Maybe I'm just being too picky? You've no doubt got a lot more experience with this. How did you choose the depth of the extrude for the inlays? Was it based on your experience? I'll be purchasing my inlays already made but maybe you make yours from scratch? I'm just a hobbyist but it sounds like you're a lot more serious about this stuff. You used a 2D pocket to machine the inlays which makes perfect sense. Shouldn't I be able to do the same thing using 3D pocket since my inlays have a curved bottom? The "Selected Contours" option doesn't come up in 3Dpocket. I don't know if this is because I have a personal use licence only. It's probably not the case but would be nice to have that option for 3D pocketing. Thanks again for your help. I hope we can continue to communicate about our projects. Cheers!

[oldtbone55]

Hey There,

Went back to my file and created a second setup. This time I used completed fretboard as my model rather than the plain one with no pockets or fret slots. The 3D pocket machining seemed to work this time if my eyes aren't deceiving me. Thought you'd like to see so I've attached the file. The initial machining of the surface does leave indentations where the pockets are but other than that I don't see any problem. The indentations were what I was trying to avoid by using the plain model. Let me know what you think.

Thanks.

[daniel_lyall]

Where are the indentations?

When you go to do the parallel toolpath use the unfinished body as the body in the toolpath it will not cut into the pocket this way.

Use the pocket toolpath to rough the pockets out then do a morph spiral or scallop toolpath to finish them off.

[oldtbone55]

Hi Daniel,

There are slight indentations created where the pockets are if using the finished fret body to do the clearing and parallel toolpaths. They are just slight indentations in the surface that don't really affect the finish. That's why I originally used the plain body in my first setup. 

I created Setup2  using the finished fretboard to see if maybe that would fix the problem with trying to do the pockets where the inlays go. That's when I got the pocket indentations.  I did Setup2 to also to see if the toolpath would work this time based on what you said. The pocket clearing did work this time. Seems crazy to me that Fusion would act up this way. It was making me think I lost my mind. 

So does it really matter which model of the fretboard I choose in the initial setup or is it best to choose the plain one first to do all of the material clearing and smoothing of the surface, then switch to the finished model when doing the operations for the inlays and fret slots? Are these the operations where you need to select Model in the geometry tab to override the initial setup model used? I'm trying to understand the meanings of a lot of these selections in the different tabs to understand how to go about machining the part or portion of the part. Your advice is greatly appreciated.

Cheers!

[jda70az]

What's up?

Usually what people do is buy those Gibson Inlay blocks pre cut to shape... and they are Flat on the bottom.

So the pocket needs to be flat. And yes after the board is radius the inlay are thinner on

the sides. Just like the fret board is thinner on the sides.

The sequence of operation would be something like...

Insert Stock fret board blank.

CNC Mill out Inlay pockets.

CNC Fret slots

Cut out Fret board

Remove and glue in Inlay material.

Either CNC the fret board radius or use a Radius block like sold at a Luthier store.

Cut off Tabs using a small saw.

You got to have Tabs so the board doesn't move while it's being milled.

And yes of course you can use 3D Pocket IF you want a curved Inlay pockets.

Same with the Fret slots. You can make them flat or following the Radius of the fret board.

I haven't done a curved Fret slot yet but I imagine it's not that hard as Fusion 360

have a lot of different tool paths.

😊

[oldtbone55]

Hey, glad to hear back from you.

I bought the inlays from Stewmac already cut and ready to go. I do have some real mother of pearl to cut my own inlays with if I decide to go that route. Your sequence of steps makes a lot of sense. Having the inlays follow the fretboard radius is pretty easy to do in Fusion but maybe that's really not necessary after all. Having the machining process finish off top of the fretboard and the inlays might be the way to go. Trying to get the CNC to do all or the majority of the work is the goal for me. 

I meant to reply to your earlier post and accidentally replied to myself (See my earlier post to myself). I attached my file where I did a new setup using the fretboard body with all of the features instead of the plain fretboard body. By doing this I wound up with little indentations where the inlays are when machining the radius. Then I did the 3D pocket toolpath for the inlays and it worked. I haven't figured out why it did here and not in my first setup. The only difference is the body that was used in the initial setup. Fusion just doesn't seem to like me referencing a different body geometry that didn't appear in the initial setup. I'm by no means an expert so whether or not this could be the case is for the experts to chime in on. 

Please have a look at my file if you have a moment to see my newer setup and how it worked. I'd love to hear about any projects you're working on. By any chance, have you done a CNC neck with an angled headstock like a Les Paul? I'm trying to figure out how to hold the headstock in place when machining around it. There's no option like in 2DContour to add tabs. Too bad there isn't a tab option in 3D contour. 

Thanks Again. 

Cheers!

[daniel_lyall]

I found what was making the indentations, it was the pocket being set to tool center on boundary and a little from the parallel toolpath as well, possibly a bug.

have a look at the attached example

[jda70az]

There are couple guys on You Tube I learned a lot from.

Highline Guitars

He has a bunch of videos and his videos on guitar making

with a CNC machine are really good.  You should check them out.

Audiohotshot

Uses Fusion 360 and has a couple CNC videos on Guitar making.

[oldtbone55]

Hey Daniel,

Thanks kindly for reviewing my file again. It really is odd the Fusion was doing that to me. I followed what you did and selected Model, then the model face in the Geometry tab for the parallel facing and finishing pass as well as the pocket path for the inlays and there were no indentations showing like there was the first time. I didn't have to change my model when I changed the operation either. Maybe it is a Fusion bug and I should report it. I thought I was losing my mind there. I also chose a different machining option than you did for cleaning up the corners of the inlay pockets. I used Trace instead of Scallop. Everything seems to look okay but I've attached my file for you to have one last look at before calling it completed. 

I'm not that well versed in the CAM side of Fusion so still trying to understand why and when certain toolpaths and selections work and others don't or which ones are the best to use. It's definitely an ongoing learning curve. 

Thanks again for the help and returning my sanity. 

Cheers!

[oldtbone55]

Hey There,

Yes, I've followed Highline Guitars and Audioshot on You Tube. There has definitely been a lot more interest in making guitars on a CNC now than there was a few years ago when I first started using Fusion. I got a lot of help from the folks on this forum. If it hadn't been for their help there's no way I could have built my guitars on the CNC. I've been away for quite a while and have been having to brush up on my Fusion skills. You sure do forget a lot when you're older real quick. The one thing I haven't seen anyone do on YouTube or here is make a Les Paul Style neck. The problem I'm having right now is how to hold the stock around the headstock when machining it. The angle its on presents some problems. 

I've attached my updated fretboard file. Was able to machine it in 4 steps the way I wanted to with the radiused inlays. Maybe it'll be some help to you.

Cheers!

[daniel_lyall]

The reason why I use scallop was the bits in the image get left behind by the Adaptive or Pocket toolpath as they use steep downs not the shape of the surfaces, I had to double-check that I was correct about how the Adaptive and pocket toolpath work.

  

With scallop 

[oldtbone55]

Hi Daniel, 

I honestly didnt notice that material was being left behind. The only material I could see that was getting machined was in the corners where the 1/8" bit can't reach. That's why I used the 0.023" end mill to get in the corners using trace. 

If you use 3D adaptive or 3D pocket to clear the inlays  I thought you could use them to also finish getting in the corners by selecting rest machining and using the 0.023" end mill but that didn't work. As I said, I don't quite understand how some of the selections really work and that leads to trial and error on my part. 

I'm definitely going to have a look at those toolpaths again after what you've shown me.

Thanks.