[Tutorial] Drawing a mountain bike in Fusion360 (WIP)

WORK IN PROGERSS. Need to transfer all photos

Why Learn Fusion360?

  • Solve problems from the comfort of your armchair
  • Prototype complex 3D designs: dropped chainstays, tire clearances, etc…
  • Complete design freedom:
    • full suspensions, unicycles, cargo bikes, triathlon bikes
  • Parameterized designs:
    • update base sketch, or parameter table, and the entire model updates automatically
    • 2D drawings can automatically update as well (sort of)
  • Knowing 3D CAD opens up a lot of doors:
    • Design fixtures and tooling
    • 3D printed parts
    • CNC workflows
  • It’s free (sort of)

Step 0: Get your ducks in a row

It’s hard to design something if can’t visualize it, especially if you are learning the tools at the same time.

I do a lot of hand sketches, bikeCAD, holding parts in my hand, etc… to help visualize how things come together before I open up CAD. The brainstorming phase takes most of my time.

  • Gather your 3D parts:
    • Dropouts
    • Headtube
    • Yoke
  • Understand the standards and dimensions of your design:
  • Have a general idea of how the tubes are going to connect
    • what radius are your bends?
    • what chainstays and seat stays are you using?
    • Will the seat tube or downtube need a bend?

Final Comments Before Beginning:

  • This tutorial is going to require some basic understanding of Fusion360
    • See resources… (TODO: add links to resources)
  • Resist the urge to click buttons until you have read the entire step of the tutorial
  • While creativity is always encouraged, I suggest completing this tutorial verbatim first, then designing the 61deg HTA frame of your dreams
  • CAD Download Link: (TODO: link model)
  • Companion video, coming soon, maybe.

Step 1: Base Geometry Sketch

Start with the seat tube:

Then fill in the rest:

This is the sketch that everything else will be linked to. Do not draw your tube centerlines in this sketch. That will be step 2. Name this sketch “ Base Sketch”


  • Please don’t deviate from this example yet, it might lead to complications later
  • if you did everything correctly, your entire sketch should be black, meaning that it is fully constrained

Step 2: Draw the Centerline Sketch

  1. Create a new sketch, named “ centerlines
  2. Use Project geometry from the base sketch to obtain the following features:
  3. head tube centerline
  4. seat tube centerline
  5. rear dropout point
  6. draw the centerlines of your front and rear triangles
  7. Dimension the “offsets” as shown

Don’t forget the seat stay offset!


  • If you did this sketch correctly, all the lines should be black or purple
  • Make sure you offset the seat stay as shown above. this prevents the SS from colliding with the CS.

Step 3: Chainstay Centerline

  1. Create a reference plane: Construct > Plane at Angle > Click the CS centerline from your centerline sketch

  2. Create a new sketch on the CS plane as shown:


  • The “Yoke dimensions” come from your yoke’s design. If you are not using a yoke, you will need to draw the CS bends to clear the tire and the chainring
  • You will need to toggle the visibility of your base sketches to grab the correct geometries to project
  • Don’t forget the two small lines at the axles. Those are used to join the dropouts!

Step 4: Seatstay Centerline

  1. Create a reference plane: Construct > Plane at Angle > Click the SS centerline from your centerline sketch
  2. On that SS plane, sketch:
    a. sketch the SS centerline
    b. make sure you include the offset at the dropout and the seat tube


  • if you are drawing the seat stays for reals, you need to make sure they will clear the tires!

Step 5: Join the parts

(todo: add CAD model of joined parts, and a video?)
This is probably the hardest step. Fusion360 uses “Joints” which is different from how other CAD packages do it.

  • Join the dropouts, yoke, and headtube to the base sketch
  • In the example provided, I drew the headtube from scratch, that way it changes length with the base sketch


  • Don’t be afraid to delete your part and start over
  • Uses the reference sketches to help position your parts
  • there are many ways to join the dropouts, this is the best way I have found
  • (todo) I provided an example with all the parts and joints

Step 6: Draw the BB and ST assembly

From here, it is all downhill. You are past the hardest part. I like to add new tubes into the assembly as “components”

  1. Assemble > New Component > name it “BB ST” > create new sketch

  2. Draw the BB shell, and Project the seat tube centerline from your “base sketch”
    a. BB is 1.5in diameter, 3mm thick, 73mm wide

  3. Draw the ST cross-section profile
    a. Create the sketch plane: Construct > Plane Along Path
    b. Draw the ST cross-section: New Sketch > draw two concentric circles

  4. Extrude the bottom bracket shell: Create > Extrude > Click the BB

  5. Sweep the seat tube: Create > Sweep > click the ST cross section > click the ST path > choose “New Body”

  6. Trim the ST with the BB: Modify > Combine > Target Body: ST > Tool Bodies: BB > Cut > check Keep Tools

  7. Remove the extra cutoffs: Design tree> right click the cutoff bodies > remove

Step 7: Draw the rest of the tubes

The remaining tubes: TT, DT, SS, CS follow the same workflow

  1. Create a sketch plane using “Plane Along Path”
  2. Sketch the tube’s cross-section
  3. Sweep the cross-section along the path
  4. make sure you create “New Body”
  5. Trim the miters using “Combine”
  6. make sure you “keep tools”
  7. Remove cutoff bodies with “Remove”

Step 8: Cleaning Up

  • Add a Brake tab
  • Add brake brace (SS to CS)
  • Add SS bridge

The rest is up to you! The next big tutorial will be how to translate your 3D drawing into 2D construction plans for your bike! (todo: make this tutorial)


Extremely helpful, thank you. Cannot wait for the 2d translation steps.

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This is really great stuff. I’m curious if there’s ways of getting your tube miter templates from fusion or if its just easier going to a traditional template software with your specs?

When I work with tapered head tubes I use Fusion to make miter templates.

This video helped me out: Fusion 360 - Unfolding Sheet Metal Tubing Update - YouTube


WHAAAAT!?!?! I didn’t even think this would be possible, thanks for sharing! This will make my life so much easier.


I forgot to mention that if you select a Paragon head tube in BikeCAD, including the few tapered models, it’ll produce accurate miter templates.

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This is so awesome. I am banging me head against the desk trying to learn F360.
Thank you so much for the time and effort in doing this.

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I need to design my own yoke. This should help

@Daniel_Y - why do you sweep the tubes instead of using create->pipe?


I try to avoid the “special” features in fusion360. I can’t speak to the pipe feature, but in my experience, the special features are not as robust (can break the model). I prefer to have more control over the model, even if it takes a bit more time.

Also, the sweep workflow allows for oval and weird shaped tubes:

That being said, if the pipe feature is robust then it could save a chunk of time!


+1 to that! I had been sweeping/lofting tubes, but experimented with revolving them on my most recent design. Revolving makes it a lot easier to line up butt profiles parametrically if that’s something of interest to you. Otherwise it ends up being a bunch of offset planes :face_with_spiral_eyes:

Not sure if this helps, but I’ll often model the parts that I’ve purchased (chainstays, seatstays, dropouts) and use them in an assembly with the front triangle. That way I can save save a copy of the mitered stays, modified brake tabs, etc. It saves me from having to create another to model of a stay the next frames that use the same stay. I also use tube profiles so that I don’t have to model a profile for each tube. There could be challenges with doing it this way for a spreadsheet driven design, but it may depends on the way the models are setup. It may not be the best way to do it, but it works okay for me.


I’ll have to play around with this. I assumed there was a way to get a miter template in fusion, jut hadnt dug into it too much yet. Thanks for the link!

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I did that with a recent design, modeling the oval/round tapered CS and roudn tapered SS, then using assembly joints to place. I consistently use the Pipe tool, as I first saw in Cobras video on using 360, and have yet to run into a problem with it using parametrics.


Thank you very much for this tutorial @Daniel_Y! I hacked my way through my last model, which was a mess. Following this really cleaned-up my recent model, and makes it much more editable.

Are people modeling components like shown in the render from @DHJustin? Or is there an open source market somewhere out there?


There are plenty parts on GrabCad that I’ve used to put into my model for visuals. I have not verified any of them for dimensional accuracy.

I created a newer/better tutorial and video on this thread:

I will keep this thread visible but closed. let’s move all the new discussions to the new tutorial. Thanks for the encouragement and feedback everyone!