CAD Software Designing Complex Fin Geometry in Fusion360 (and others)

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frogglicker

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For the past year, I have focused primarily on CAD using Fusion 360. Not to spark a holy war, it fits my kind of workflow and many other CAD options can do this. I get excited when I discover some design element that isn't straightforward and needs a bit of brain usage -- limited as it may be -- to solve. Please understand that I am self-taught, so there may be an easy button in Fusion to do many things that I demonstrate. Organic learning is my teacher, though it is, at times, a difficult schoolmaster.

Fin geometry has been my white whale, so I set out to overcome this. For example, the Nike Smoke has different variants, but most of us are familiar with the complex airfoil design (figure 1). It tapers from the center both horizontally and vertically, so a simple extrusion procedure will not work. After much trial and error (mostly error), I finalized a method for designing these complex fin geometries, which I will attempt to describe here. I will also follow with a video tutorial.

.1736956084482.png
Figure 1 - Nike Smoke Complex Airfoil

I recently started working on a 3-in Black Brant II upscale and while it isn't technically correct, I elected to use the BB-VC fin. The process works for most complex geometries and I will demonstrate using the BB-VC.

Design Process:

My first step is to find an engineering drawing of the fin. I found this image that was posted by @Bruiser (who is also my muse for this post). I also used the basic fin shape of the BB-II from an OpenRocket Sim design.

1736956330774.png
Figure 2 - BB-VC Engineering Rendering

I used this drawing for proportionate dimensions of the leading/trailing airfoil tapers going horizontally, and the center section with the tapers going vertically. Building a table in Excel to create proportions, I could then scale these segments to my fin (figure 3).

1736957386409.png
Figure 3 - Taper Scaling Calculations

Next, in Fusion, I sketched out the fin in two dimensions as I would with any other fin. It's not exact to scale, but it's approximate and reasonably resembles the fin shape. The 2D sketch acts as a centerline for the rest of the design. I switched the sketch to 3D and found my points at the leading and trailing edges and where the airfoil tapers begin both at the top and bottom of the fin and connected all the segments at the top and bottom. These values are split in half. In the end, I ended up with this sketch (figure 4).

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Figure 4 - 3D Sketch

Next, I selected the top and bottom of one section of the airfoil (figure 5). I used the loft process to create the complex taper from top to bottom, center to edge. I repeated this 3 more times, then did the same for the top and bottom center sections.
Screenshot 2025-01-15 163139.png
Figure 5 - Lofting Segments

In total, I have 6 separate lofts:
  • Bottom Forward airfoil
  • Top Forward airfoil
  • Bottom Aft airfoil
  • Top Aft airfoil
  • Bottom Center Section
  • Top Center Section

Screenshot 2025-01-15 163516.png

Figure 6 - Lofted FWD and AFT Airfoils


Screenshot 2025-01-15 163635.png
Figure 7 - Lofted Center Section


Finally, I extruded the fin tab. Since it's in the middle, I use the symmetric method with 3mm on either side. I also elected not to taper the tab with the fin. Fin tabs are for structure, not show and all of this will be covered by the fillet.
Screenshot 2025-01-15 163703.png
Figure 8 - Extruded Fin Tab


Once all these steps are complete, you are rewarded with a wicked-looking fin that will be the envy of all your friends.

Fin Slicer.png
Figure - Completed Fin as a Single Body

Conclusion:

I know that there are a lot of parts here that I glossed over, such as how I got the figures for my measurements. I will discuss these details in the video. If you're like me, a guide like this is helpful but a video is 10x the value. I hope this helps you on your journey in designing rocket parts.
 

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Very nice. I see the work that individuals like yourself and others are accomplishing using Fusion360 and the like, and it never fails to impress.

Will you now use this to generate a file/code to drive a CNC to have those fins machined?
 
A laser cutter will not be able to make that fin. A CNC router could do it, depending on the sophistication of the software running it, but you might not like the cost.
 
It would be easiest to get them 3D printed, if that would be strong enough for your build. At 3 inches, I'd seriously think about designing one half and hollowing it out with a frame structure inside, and gluing them together like an Estes 2-in. PSII E2X fin.

A CNC router would probably need to do one half at a time and then you'd glue them together, possibly on a thin plywood core. I think John Coker has a build where he did it that way.
 
It would be easiest to get them 3D printed, if that would be strong enough for your build. At 3 inches, I'd seriously think about designing one half and hollowing it out with a frame structure inside, and gluing them together like an Estes 2-in. PSII E2X fin.

A CNC router would probably need to do one half at a time and then you'd glue them together, possibly on a thin plywood core. I think John Coker has a build where he did it that way.
or you flip the stock over if you can deal with a few thou out of spec.
 
@NTP2 - It probably has something to do with the base plane in the middle of the sketch. I did try to do multiple planes at once and got very Van Gogh-like shapes. Its like Fusion wants to associate all the selected planes, even when there's a gap. I don't mind taking my time and trying to be precise.

I did try splitting these with the slicer into two parts, but it didn't really work very well. My build plate was basically a potato chip at the time, and the results reflected that but now I made it better. I might try that again.

ATM, I'm content with trad and 3D-print augmented design/build elements. I might expand into some other methods later. For now, I'm just trying not to blow up my L2 attempt.
 
That's a great approach. I didn't think of sandwiching G10 with the profile halves. That's really cool.
Thanks. We'll see how it works when I fly it. I printed each half with no base layers so the infill is exposed. The thinking is that this will promote better adhesion via the epoxy to the G10. I was originally going to just use 1/16th thick G10 but it was suggested that that might be too thin given the long semi-span of the fins and an especially energetic motor so increased it to 3/32". After assembling them, I'm leaning toward thinking that the 1/16th would have been more than sufficient. These fins are very rigid.
 
Thanks. We'll see how it works when I fly it. I printed each half with no base layers so the infill is exposed. The thinking is that this will promote better adhesion via the epoxy to the G10. I was originally going to just use 1/16th thick G10 but it was suggested that that might be too thin given the long semi-span of the fins and an especially energetic motor so increased it to 3/32". After assembling them, I'm leaning toward thinking that the 1/16th would have been more than sufficient. These fins are very rigid.
I look forward to that flight report!
 
Sorry for the video delay. My computer is in Potato mode and keeps freaking out when I'm doing screen recordings... I'm posting the Fusion360 file here. Sorry for those that cannot use it. I modified the thickness of the leading and trailing edges b/c they were a little thicker than I like but feel free to modify as it suits your needs.

I have posted this file with a .txt extension. Change the extension back to .f3d and it will load right up.
BB VC Fin Layout.png
 

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Another way to do that in Fusion is to use Surface modeling with profiles and rails and then Patch. You can model the whole shape in one go and then turn it into a solid. That is a complex shape and modeling the "outside" then filling it in is just a different method.
 
why 6 lofts? you should be able to do it in one or 3 max? at least in Inventor which I am trained (boy that feels nice to say), but 360 is close enough that it can't change that much.

I use Fusion 360 and SolidWorks, mostly, but also Inventor on occasion (I know, using Autodesk and Dassault is crossing streams, but I have used SW since almost the beginning, so Inventor was always the new kid on the block for me). You can't really compare Fusion to Inventor. There are SO many things Inventor does easily that are either a kludge in Fusion or pretty much impossible. However, Fusion is awesome when you need to get relatively simple things done quickly and it has just about the best CAM product around, so I find myself in Fusion almost daily and, recently, have spent less time in SW. However, even when I do design in SW, I still go back to Fusion for CNC because its CAM is just that much better.

Point, though, is that things you can do in Inventor don't usually translate 1:1 in Fusion. Then again, that is the main reason Fusion is a fraction of the cost of Inventor.

Second point, if you use Inventor or SW, I would still have Fusion on your desktop.

Third point, @frogglicker - great work here! Love the designs and files, thanks for sharing!
 
I use Fusion 360 and SolidWorks, mostly, but also Inventor on occasion (I know, using Autodesk and Dassault is crossing streams, but I have used SW since almost the beginning, so Inventor was always the new kid on the block for me). You can't really compare Fusion to Inventor. There are SO many things Inventor does easily that are either a kludge in Fusion or pretty much impossible. However, Fusion is awesome when you need to get relatively simple things done quickly and it has just about the best CAM product around, so I find myself in Fusion almost daily and, recently, have spent less time in SW. However, even when I do design in SW, I still go back to Fusion for CNC because its CAM is just that much better.

Point, though, is that things you can do in Inventor don't usually translate 1:1 in Fusion. Then again, that is the main reason Fusion is a fraction of the cost of Inventor.

Second point, if you use Inventor or SW, I would still have Fusion on your desktop.

Third point, @frogglicker - great work here! Love the designs and files, thanks for sharing!
Joseph Gordon Levitt Thank You GIF
 

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