CNC Router Fin Beveling

[BryRocket]

I recently purchased a CNC router table for making odds and ends. For rocketry, I like the ability to make my own centering rings, fins, stepped AV lids and whatever else I needed. I ultimately decided on the Shapeoko 3. It is a fun process trying to get your machine set up correctly and learning how to cut things with dimensional accuracy. I can't tell you how many pocketed squares I made...

Getting the 2D/2.5D cutting down is relatively straight forward and not too difficult when you're designing with Carbide Create or similar programs. I am quite familiar with Fusion 360 though as I use it for all 3D designing and even 2D sketching for fins and other 2D .dxf files.

This is a short thread about how I beveled in 3D with a CNC mill. I know lots of people here that can make beautiful bevels with a router table (@rfjustin for example) but I wasn't getting it down. I tried a few different methods and then just punted on it and started working on this method. When researching CNC options, @KC3KNM offered up some good advice and then threw me off into the rabbit hole of trying to mill the bevels and I figured it would be a fun learning opportunity.

I started by designing my fins in Fusion 360. I then exported the fin sketch as a .dxf. That file can then be imported into Carbide Create if you'd like. I'm going to kind of skip over how to use the CNC to cut the 2D fin file but I ultimately used a beautiful piece of 3/16" carbon plate from McMaster and cut out 4 fins (although I only need 3).



Next on to beveling.

I circled back to F360 and created a 12" x 12" x 0.5" guide plate that I made two pockets in for 2 fins. Each pocket was a depth of 1/2 the fin thickness. I made it 12" x 12" because that is the dimensions of the MDF I had ready to go. I then just modeled the fins with the exact thickness of the actual fins and created the bevels I wanted with a chamfer that was 15mm x 1.75mm per edge.



From there I switched from DESIGN to MANUFACTURE mode in F360 so I could create setups and toolpaths for the CNC. I started by creating a setup for the pocketing of the fin spots using a 2D pocket using an 1/8in flat endmill. For the first run I used the Leave Stock option and set to 0.5mm radially but left axial at 0.0. The first pocket was definitely too tight so I tried again with the radial setting at 0.0. Again too small but setting the axial to leave at -0.5mm made a nice, very snug fit.


From there I then created another setup for each fin. I don't think this is necessary and you can likely just use one setup for all 4 edges and is probably the better way to go. I ultimately created 4 different toolpaths, one for each bevel. I figured this would be more time consuming but allow me to watch it closer and I could then tape off the other bevels for work holding. I used the 3D Contour toolpath for the bevels. I used a 1/8" round nose end mill for this. It took me a lot of modeling and simulating to get the toolpath the way I wanted it so I'll just post screenshots of all the settings in the next post.


That was pretty much it for the modeling/setup part. Now it was time to actually see if it would work.

 

[BryRocket]

Knowing I wanted this piece of MDF to stay attached to the base good, I used Carbide Create again to knock some holes in it for securing the center and then I'd use other clamps for the sides. CC always gets me with its calling for RADIUS and not DIAMETER so you'll notice 3 holes that were twice the size needed. Once completed the MDF piece was not going anywhere.

Time to pocket the guide. For this, I set the XYZ zero at the bottom left corner as I did in F360. The setup/toolpath was organized this way. I then ran the file and as mentioned had to use the Leave Stock Axial set to -0.5mm.

Now it was time to change bits from the 1/8" flat end mill to the round 1/8". I then placed a fin into the left pocket. IMPORTANT** You NEVER want to rezero XY again. This has been established in the machine and won't change going forward during this process. Once the fin was snapped in place, I used some tape to make sure it didn't move any. Probably not needed since the fin was so snug but why not. I then moved the endmill to the center of the long edge of the bevel to be cut and did a touch-off zeroing of Z. Once that was done I hit start and crossed my fingers. (14mins each bevel)


What was left was, to my excitement, a very nice and extremely smooth bevel.

I then left all settings the same and switched to a new fin and repeated the procedure for all 4. Every one came out the same. Then we went back to the first fin and taped it off different to expose the rear bevel to be done. At this time, I did rezero Z like I did the other, right in the center of where the bevel was going to be. Hit start, cross fingers.

Nice. Do the other 3 fins the same way by just switching them out, taping and hitting start. (4mins each)

On to the other side and I used the exact same procedure of zeroing Z and workholding.


After it was all said and done I had 4 exact fins with very nice bevels and I didn't lose my finger to the router table.

 

[rfjustin]

 

[BryRocket]

Here are the settings I used for the contour. Probably too conservative but it worked albeit a little slow. For the pocketing toolpaths, I set the zero to the MDF stock top. For the Contour toolpath I set Z zero to the top of the fins.

For those familiar with F360 and it's toolpaths I'm sure my process isn't optimal. This has been a learning process for me. For those of you not familar with them, F360 is amazing but holy cow are there a lot of settings. Simulate, simulate and simulate again. I had always planned on using my CNC for more 2D/2.5D stuff and hadn't really considered this possibility. I'm now realizing you can do so much. In fact, there are likely much more efficient bevel modeling that could be done with rounded edges, etc that could be accomplished with this.

If you have any more specific questions if you give this a try let me know and I'll do my best to help. There are others here much more proficient with this stuff though.

 

[Jowayen]

What I did on my CNC router was used a sine plate so I could machine the bevel flat with a machined surface on the fin. No sanding of ball mill grooves required.

 

[BryRocket]

Very cool! Lots of possibilities with the CNC. I had not thought of doing it that way. FWIW, there are no grooves at all from the ball mill. Not that you could ever feel anyway. It's smooth as smooth can be. Like super slick smooth and may need to be roughed up a bit before the tip to tip carbon. I used 0.05mm stepdowns which I think helped with that but it made each bevel take about 15 minutes.

 

[BDB]

This is awesome!!!