[Video Tutorial] Drawing a real mountain bike in fusion360

[Daniel_Y]

Here is a new and improved Fusion360 video + tutorial. This took me quite a long time and heartache (I killed my microphone for half the video, so I had to dub over). If you want to show thanks, do the tutorial and post up your results!

Video: make sure you select 1080p resolution!

Fusion 360 Tutorial: How to design a mountain bike frame

Forward:

Unlike other “how to draw a frame in F360” CAD tutorials, this one parallels real-world fabrication workflows. This is what @Neuhaus_Metalworks and I used to make over 100 mountain bike frames. Completing this tutorial is the first step toward creating 2D construction drawings. Once you have mastered both, you will have a fully digital design workflow!

Although the video is less than 40min, I expect it to take a beginner much longer (3-4hrs). I split the tutorial and forum thread into manageable chunks. You may find it useful to replay each step and flip back and forth between the video and this guide.

There are many ways to CAD a frame. This tutorial is a simplified version of my workflow, where I purposefully omit more complex geometries and features. I encourage you to follow the tutorial verbatim, then go back to applying custom geometry or fancier workflows!
Good luck, have fun!

Step 0: Get your ducks in a row (do this before the video!)

Download Parts:

Fusion360 drawing method (preferred!):

1. click Fusion360 Link: parts
2. download > fusion360 Archive > enter in email
3. downloading the drawing archive will download all the parts with it!

Forum Files:
Dropout+1p5+NDS.f3d (171.2 KB)
Dropout+1p5+DS.f3d (152.2 KB)
Yoke+DUMMY.f3d (300.3 KB)

Download finished model:
Fusion 360 link: Finished Model
This is a completed model and drawing. If you get stuck, you can reverse engineer this model to un-stuck yourself.

Step 1 - Base sketch 01:07

Tools used:

• basic sketching
• sketch constraints

Comments:
The base sketch contains the fundamental 2D geometry of our bike. We will base the entire CAD off this sketch. If you build your model correctly, when you edit the base sketch, your entire 3D CAD will update as well as your 2D construction drawings (tutorial coming soon).

Step 2 - Centerline sketch 04:32

Tools used:

• Projecting geometry
• sketch constraints

Comments:
The rear triangle centerline sketch is a bit more complicated due to the non-conccentric paragon 1.5in round dropouts. Concentric dropouts would simplify the drawing quite a bit, however if you follow this tutorial exactly, you will be able to figure it out!

Dropout details:

Step 3 - Draw headtube 08:33

Tools used:

• creating a new component
• toggling sketch visibility
• sketch constraints

Comments:
Don’t forget to create a new component! Don’t forget to go back to your main assembly after you are done modeling your headtube!

Step 4 - BB ST 12:19

Tools used:

• symmetric extrude
• extrude to object

Step 5 - Front triangle 14:47

Tools used:

• construction plane along path
• sweeps
• using combine tool to cut bodies

Comments:
In the video, I tried hiding the extra cutoffs to save time. This ended up biting me in the butt when I created the 2D drawings (it automatically displays all hidden bodies). The correct workflow is to right click the body > then remove

Step 6 - CS centerlines 18:49

Tools used:

• construction plane at an angle
• “look at” feature to view normal plane

Comments:
If you are using complex tapered, ovalized, and dimpled chainstays, it may not make sense to time draw “real” chainstays in CAD. Unless you had high confidence in your measurements, it will be more accurate to figure out the chainstay miters in real life.

Step 7 - Tire clearance body 22:14

Tools used:

• revolve tool

Comments:
I normally use a more complex tire body with side knobs and 6-8mm of clearance:

Step 8 - SS centerlines 23:45

Tools used:

• construction plane at an angle
• project > interset geometry

Step 9 - CS body 27:46

Tools used:

• construction plane along path
• sweeps
• cut extrude

Step 10 - SS body 29:36

Tools used:

• construction plane along path
• sweeps
• cut extrude
• using combine tool to cut bodies

Step 11 - Joining the dropouts and yoke 31:20

Tools used:

• adding existing components to an assembly
• joints
• joints to a reference sketch

Comments:
There is no easy way around it, joints in fusion360 are very difficult to understand! If you get stuck, download the finished model from above and try to reverse-engineer the joitns. There are some great videos on youtube to help you learn more about joints: Joints in Fusion 360: A Comprehensive Tutorial! FF117 - YouTube

Step 12 - Conclusions 34:59

I hope you found this tutorial useful. Feel free to ask questions or leave comments below!

Teaser: 2D drawing tutorial coming soon!

[sikocycles]

Wow. What a great forum this has become

[Meriwether]

Amazing… thanks so much for this! No excuse now not to try this. Just need to make the time.

[Neuhaus_Metalworks]

Thanks @Daniel_Y, this is incredibly valuable information!

[Neuhaus_Metalworks]

Still missing a few pieces.

[earle.b]

Thanks for the video. Some stuff in there i wasn’t doing. The projecting the line into another sketch.

I found that using the parameters list and naming the dimensions on the base sketch has been helpful. You can edit the paramter list at any point and not need to go back to the base sketch or any particular sketch. Possibly for the next advanced tutorial.

My next model I want to use the parameter list for the suspension location points. Would be nice if Linkage would export a table of location points to speed the process of updating a model.

[liberationfab]

I think you could do a pretty hacky workflow of linkage > csv > Excel/google sheet > Fusion but by the time you got data through that pipeline it would’ve been easier to type it manually.

[Neuhaus_Metalworks]

Now were getting somewhere.

[Daniel_Y]

Nice! S bend stays and horizontal dropouts. Someone wasn’t following directions. but I’m glad it worked out!

[Neuhaus_Metalworks]

I’ve always been a bit of a rebel.

[Neuhaus_Metalworks]

The cs yoke needs a little love but all of the clearances are right.

[anon68659156]

I have a headache from concentrating. I’ve learned more about fusion in a day than I did in a year. Thank you!

I got sloppy at the end and I have a lot more work to do to get the model right, but I think I can actually do it now.

[Daniel_Y]

Very nice! Different dropouts, S bend stays, yokes chainstays, and HT rings. You get all the extra credit additions!

One tip: not sure if it was intentional, but it’s easy to miss: You don’t seem to have any SS offsets. Drawing the SS’s is one of the benefits 3D CAD. You can really zoom in and fine-tune the millimeters. In the real world, you are stuck bending a tube and trying to make it work!

The SS-dropout offset can be found in the side centerline sketch:

The SS-ST offset can be found in the SS centerline sketch:

[Neuhaus_Metalworks]

Done.

[jeremy]

This is a great resource Daniel, thank you so much for putting it together! I do the same thing for my drawings, and although it’s a little bit more work up front to set everything up with parameters it ends up saving so much time down the line.

I have started putting in a couple little additions to my frame layout sketch for positioning the down tube in relation to the head tube so that I can control the distance between the lower end of the HT and the bottom of the DT miter.

I have a parameter for the diameters of the DT and the HT (or just the bottom end of the HT), and I sketch out a couple lines to outline that intersection. The centerline of the DT is only constrained to be coincident to the centerline of the HT, and the vertical position is driven by a parallel line representing the edge of the tube. I’m probably explaining it badly - hopefully the picture helps.

The thing I like so much about this is that the room I’m leaving for a weld remains constant as I vary angles or tube diameters down the line, without the need to go back and fudge anything. Hopefully this is helpful to someone!

[Daniel_Y]

Everyone is way ahead of me haha. I have been slowly revealing my CAD secrets to feed the forum.

This is how I constrain the tube locations:

A few tips:

• I don’t use the offset tool to create the tube diameters. The offset tool breaks the CAD too much
• I use a circle to make the tangent tube. I found the circle to be more robust than a perpendicular line
• the top tube is driven by a constant 6-8mm offset
• Fork crown clearances can be found on fox’s 2022-2023 fork drawings:
  • I use the Grip 1 51mm offset crown spec because it is the most constraining
  • Fox 34 clears the MRP ribbon SL
  • Fox 36 clears pretty much anything that you would want to stick on a hardtail

Source: All Specification Sheets | Bike Help Center | FOX

[jeremy]

@Daniel_Y

I found the circle to be more robust than a perpendicular line

Oh, that’s very good. Filing that one away for later!

[CharlieSBI]

Holy cow Daniel thank you so much. I’ve tried some fusion tutorials but this series is amazing. You made it so easy to understand the workflow, this is the most progress I’ve ever made doing this kind of thing. Still have some work to do on the tutorial but I’m so stoked about this!

[Daniel_Y]

Thanks for all the support everyone! Make sure you check out the how to create 2D drawings tutorial. That is where the true magic happens!

[Video Tutorial] Creating useful 2D frame construction drawings Fusion360

When it rains video tutorials, it pours. But really though, its been raining on and off the past month, and I am getting stir-crazy. [image] Forward: In this tutorial, I show how to create useful 2D drawings that can be used to construct a bike in real life. If you take the time to understand this tutorial, you will have a very powerful tool in your toolbox. Fusion360 2D drawings are more accurate, customizable, and automatically generated. It has taken me over 500hrs in CAD to develop this …

Feel free to chat about general fusion360 and framebuilding topics on this thread.

Also, let me know if there are any designs you would like me to cover in the next video. Once you have the fundamentals, it’s really easy to build off of. Some random ideas:

• drawing tapered headtubes
• using sliding dropouts
• gravel bikes
• using pre-made chainstays (don’t ask me to do this please haha)
• designing a flatmount adapter

[Daniel_Y]

Thanks for all the support everyone! Make sure you check out the how to create 2D drawings tutorial. That is where the true magic happens!

[Video Tutorial] Creating useful 2D frame construction drawings Fusion360

When it rains video tutorials, it pours. But really though, its been raining on and off the past month, and I am getting stir-crazy. [image] Forward: In this tutorial, I show how to create useful 2D drawings that can be used to construct a bike in real life. If you take the time to understand this tutorial, you will have a very powerful tool in your toolbox. Fusion360 2D drawings are more accurate, customizable, and automatically generated. It has taken me over 500hrs in CAD to develop this …

Let me know if there are any designs or concepts you would like me to cover in the next video. Once you have the fundamentals, it’s really easy to build off of. Some random ideas:

• gravel bike
• drawing tapered headtubes
• drawing a parameterized IS brake tab
• using sliding dropouts
• gravel bikes
• using pre-made chainstays (don’t ask me to do this please haha)
• designing a flat mount nub
• Other: recommend below!