Wow, thanks for figuring that out and writing it up. There’s certainly some cool projection of curves onto curved services math going on that I can’t quite visualize, but it makes sense.
I found creating separate assemblies the way to go. It is annoying to set up, but very robust. I create what I call “phantom stays” which are linked copies of the CS and SS sub-assemblies, laid out on the top plane:
When I create the 2D drawings of the CSs, I just hide all other components.
…and BOOM!, there’s the solution to my (currently) last problem with my CAD project.
Many, many thanks, Daniel. 
All the best,
I really need to take the time to learn Fusion. Everytime I jump in and try to use it I’m stuck in my years of AutoCAD/microstation thinking. Some things are similar and others aspects make no sense. 
Microstation! That’s a blast from the past haha. I’m stuck in Rhino over here. Although do wonder if NURBS modelling is the way to get smoother lofts/surfaces and better shells for 3D printed elements.
I still have a copy of Microstation at home. I use it when AutoCAD struggles with fillets and blending etc. I use AutoCAD so much at work that MS now feels a bit odd but even this older version I have is still better than ACAD in a lot of ways.
Hey all, I’m still pretty new to Fusion360 and I’m in the process of designing a frame after following Daniel’s tutorial and I’m wondering what’s the best way to integrate Paragon dropouts to the frame. For reference, I’m using their hooded track dropout (https://paragonmachineworks.com/files/public-docs/DR0012.PDF).
In Daniel’s tutorial there was a reference point on the dropout that would snap easily on the axle line, but either I can’t see it or there doesn’t seem to be one with the Paragon’s. So what I tried doing is using the “Joint” tool and find the middle of the dropout:
And snap it along the axle line, but it seems to leave a gap from the chainstay, and doesn’t fully touches the seatstay:
To miter the stays I made a round profile of 33.3mm and used extrude:
I’m sure there’s a small detail I’m missing or had wrong along the process but I can’t seem to figure it out. Either I misread Paragon’s drawing, either my point of reference on the dropout is wrong, or I’m not using the joint tool properly?
I figured I could have integrated the dropouts first and then use that body to miter the stays, but I’m not sure I’m integrating them properly.
Thanks!
Dang, I wrote up a whole tutorial using the move tool and stuff and then realized that wasn’t what your question was about.
The little thing you’re missing is that the rear of the axle slot and the dropout shell are not concentric.
Use the outside of the bottom bracket as your reference and you should be good!
Thank you @jellywerker, I didn’t even have to fire up F360
@ViSav great job with the CAD! It looks very sharp.
As Jelly suggested, you need move your dropout sketch backward by 1.43mm
I use reference sketch(es) that model all the important data points for where the ‘hard’ contact points are going to be. So I position the BB, the headtube and the bottom bracket based on these dimensions and then place the tubes afterwards using these same reference points as the ‘end’ points for the tubes. I then use the BB, HT or dropouts as the cutting tool to ‘mitre’ the tubes to fit these parts. I like doing it this way rather than modelling the tube as it means if I want to lengthen the front-centre for example, the tubes will just move and extend with the model, I don’t need to redraw the tube. Sometimes it can get a bit funky if your tubes are offset from the centre of the BB or the centre of the axle in the case of stays but creating offset planes to hold these sketches isn’t too much of an issue. Doing it this way also allows you to create your model using parameters so changing your driving dimensions is really easy.
I’m not sure I’m following, wouldn’t that make the dropout sit even more behind if I use the same reference point on the dropout?
Thanks to @jellywerker I did manage to figure out a way. I realized that by selecting the whole dropout body with the joint tool it would actually show me all the various reference points and I could select the concentric one you showed:
I’m pretty sure I was using the point slightly to the left before. Then I again used the axle line as reference and now it looks like the dropout is mating perfectly
My next question is, how do you usually go about modeling a fork with a specific cast fork crown? Is it worth reproducing the whole crown, or just a crude model? I would like to use this Allotec fork crown:
That’s the only drawing I could find, and it doesn’t specify the “stack”, or the distance from the bottom of the shoulders to the crown race. I’m lucky that I can actually have it physically without buying it and measure it, but what do you do when you can’t? I’d like to make sure I’ll have fork legs long enough, since the fork is a little longer than usual for that type of bike. I could model it as a segmented fork but I would like the model to be as close as possible to what I want it to be in the real world.
let me try to explain better…
Orignially, your assumption was that the axle center was the center of your dropout.
Now, They way you joined the dropout to your sketch, the axle center is actually further back than your base sketch. That means your chainstay length is longer than you intended.
In this case, there is only a minor difference, but it’s technically incorrect. With most other dropouts, the axle center and the dropout center are not close at all, so I think its important to know how to visualize it.
(re-edited a third time because I keep realizing things as I reread your posts)
Okay so if I understand correctly, when I drew the base sketch with 400mm chainstay, that’s where I would technically want my axle center to be and not the dropout center, which would explain why you drew an offset from my axle line 1.43mm further back. Do I get this right?
And just to make sure, was I right to assume that this point in Paragon’s drawing is the dropout center and not the axle center? And if I want to figure chainstay length without a 3D program, I would just have to measure the axle radius to find the axle center?
Sorry for making this hard, I really appreciate your help. I’ve been racking my brain with this all afternoon. Like you said I know it’s a very minor difference, especially with horizontal dropouts, but I want to make sure I understand it so that it doesn’t causes issues in other, less forgiving, scenarios
It’s a bit tricky/harder to visualize with this specific dropout, since they are very close to concentric, but aren’t.
The centerline mark you circled is the axle center, and not the dropout/center of circle marked with the 33.3mm dimension.
A simpler way to do this, as noted above, would be to reference the dropout to your sketch using the axle center, and then use it to create the necessary cuts in your tubes.
Regarding the fork crown: I do a lot of reverse engineering. If you can dig up the original specification drawing, you may be able to model it without the physical part, but typically you need the physical part so you can measure it. Even if you scale and reference that catalog drawing, which appears to be taken from their cad, because of the model variations, you can’t guarantee it’s the version you’re looking to create. Also, the line width of small drawings like that adds a lot of uncertainty when trying to reference them.
So, in short, if you can’t borrow it somehow, then you buy it. In some cases you may be able to convince the company to send you a model, but usually they don’t share that kind of data.
correct!
Awesome thank you so much for your help @Daniel_Y and @jellywerker !
Hello all,
I am trying to convert my miter/copes to sheet metal flat patterns, keeping them in a drawing with the ability to still change bike geometry from the model and have it update the miter templates in the drawing. Currently I’ve used the split command to break the tubes into pieces that can be unfolded when converted to sheet metal (this seems to be where things are falling apart). I then have the miter templates in a 2d drawing that will update based on the geo changes and tubing diameter changes made in the model. Problem is that when I update the model I find some functions appear with errors such as the “convert to sheet metal” function “missing source face” but the model itself is still functioning. Or similarly the split function is “missing target bodies” and then whole components disappear or move. Perhaps I have missed something as well that is not allowing the model to be parametric. I’ve attached my fusion file here for the model, I am new to fusion360 so I am quite sure I could have missed some things in my model.
Are others still using fusion for their miter templates? Do you have a parametric workflow or do you add this as a final step after your model is complete?
Any tips or perspective would be great!
Miter Template Model v1.f3z (1.7 MB)
Looks like this might be your problem - the cut isn’t going all the way through, so the bodies your commands are expecting to find don’t exist.
You need to modify how this works to make sure that the cut length is always long enough to completely split the tube.
Good luck!
Edit: I’d suggest creating the cut length with a parameter that’s a function of the top tube length parameter. There seems to be some overlap in how you’re creating the top tube (both an extrusion and a sweep, and the cut is only longer than the extrusion).
Thanks jellywerker! I should have noticed that, I though I looked everywhere. Now I’m realizing how much I hadn’t defined parametrically. Lots to clean up too.
Thanks for looking through my messy file!
