relationship joints

[zenkustumz]

trying to figure out what I am doing wrong on the joints i have created..

its a pivot or cantilever set up.. most of the limits are set up but wont more correctly. can anyone assist?

http://a360.co/2cC68Ji

Thank for the help in advance

Let me know what i'm doing incorrectly please

[xander.luciano]

Hey!

First off, great model! This was one of the cooler projects I've helped someone with on the forums haha.

Anyways though, you were actually really close to having it perfect man! The only issue was the space you used had a fixed joint on it when you needed to use a cylindrical joint. I went ahead and made that edit for you and you can download and view the file here: http://a360.co/2cCS72H

Hope that helps man! Looks like a sweet project!

Keep up the good work!

Edit: In case I delete that file later on, I'm also attaching it here.
Edit 2: File removed - see below for updated file

[TrippyLighting]

three things:

1. You probably should not work with linked components this early in your design process as it makes the design workflow unnecessarily complicated. It has the advantage of creating the correct component / assembly structure in your design file, provide that correct structure is maintained in the assemblies you insert. You can perfect fine create a complete assembly in a single Fusion 360 file as Fusion 360 does not use separate file types for assemblies and components.

You may want to review Fusion 360's R.U.L.E #1

2. The reason out joints did not work is because the structure in your "shifter Lever" assembly was incorrect. The main body was still a body, not a component. There should not be any bodies in the top level of an assembly, just components.

It should not look like this:

—+— Assembly
    |—+—Component
         |— Sketch
         |— Body
    |—+—Component
         |— Sketch
         |— Body
    |—+—Component
         |— Sketch
         |— Body

or like this

—+— Assembly
    |—+—sub-assembly
       |—+—Component
          |— Sketch
          |— Body
       |—+—Component
          |— Sketch
          |— Body
    |—+—sub-assembly
       |—+—Component
          |— Sketch
          |— Body
       |—+—Component
          |— Sketch
          |— Body

3. When the assembly structure is fixed, one of the joints will create a failure. that is because for a revolute joint to work, the two implicit joint origins you pick then creating the joint have to be in the same plane. That can indicate a design problem, or if it does not then the over constrained condition can be removed by turing that revolute joint into a cylindrical joint.

[zenkustumz]

thank you.. I was kinda lost with Trippy's explenation. i dont know technical terms and stuff very well.. kinda self taught.. no professional training here..

[zenkustumz]

i tried to open and says cant open?

[xander.luciano]

I'll try to explain trippy's in a second. To be quick, he's technically right about that, but I'm guessing you might have some solidworks background maybe? Either way, I do things similarly to how you did it so don't stress it too much. I just prefer having separate files because that's what I was used to with solidworks.

As far as not being able to open the file, that's my bad! I accidently did that in the dev build of fusion! Sorry about that! I'll have that fixed and attached in just a moment.

Best,

[TrippyLighting]

If you don't understand how to apply my advice you'll likely run into problems again, so lets work on that step by step.

BTW the only professional training I had on any CAD system in my career was one week off CATIA 2D training 20 some years ago. The rest is entirely self taught.

[xander.luciano]

Sorry about that file issue! Here's the update link: http://a360.co/2cCS72H

And I also attached the updated file. Let me know if this works for you!

[zenkustumz]

i meant it in no way as offensive.. ive only been using fusion and dabble a very little in solid works.. mostly self taught.. you tube.. the forum.. always looking to better myself..

I just dont understand terminology that was being used. 

If items were broke down and explained 1 at a time then it might make sense.. I dont expect people to bottle feed me.. i just need more time to learn the proper way of doing things..

I am always willing to learn..

Thank for your input also sir..

John

[TrippyLighting]

I was not offended 😉

Let me know if a screencast would help. 

[TrippyLighting]

---

@xander.luciano wrote:
 I just prefer having separate files because that's what I was used to with solidworks.

---

You should try to break that habit as you are missing out on a lot of the power that Fusion 360 has for top down design.

[zenkustumz]

I'm so sorry to be a pain.. can you tell me the process of down loading this?

I clicked on the link.. when window opened and saw model, i clicked on down load and put in my email. says cantilever but can import into 360 and when i tried to open with i get an error..

Give me steps please to do this correctly.. again sorry

John

[TrippyLighting]

If it is a .f3d file you can open it directly with "new design from file" rom your download flower.

If it is a f3z as your original file you need to use the upload functionality in the data panel.

[xander.luciano]

Alright, gunna try and break this down to be as simple as possible.

Fusion works great with single files. There is really no need to have more than 1 file. The top level file (1) is what we would call the assembly. It has all components, joints, bodies, sketches, etc of everything.

Under it, we would have Components and/or "sub-assemblies"
Number (2) is an example of a sub-assembly. This Sub assembly in turn has components (like Brake Lever and Foot Shift peg). Looking at Foot shift peg(3) is iscomposed of bodies(4) and sketches(5).

In this manner, we keep everything related together in one single file. Everything is separated still, but it all exists together. If you look at Shifter Lever (2), you will see the icon just to the right of the light bulb looks like a stack of boxes, this indicates it's a subassembly, and has components within it. Skipping down to the Brake Cable Bracket, we can see it's icon is just a box, indicating it is a single component or part, with no components within.

Keeping designs in a single file is nice in that it allows you to reference geometry from other parts in all your sketches, as well as keeping your file structure free of clutter.

Hopefully that helps explain it a bit, but if you would like a screencast, I would be happy to make one as well for you 🙂

@TrippyLighting Haha I hear that, and I do to a certain degree. The only thing I hold onto it with as of now is for all my CAM operations. I have one single "master file" that has my vice and machine setup on it, and I just put referenced components into that file. It's also useful to have separate part files when I'm working with someone so they don't have to deal with my machine setup in the structure tree and if my project has lots of parts, I'd prefer to take each part out and create a separate "tool path" file for each. That way I can  focus more on the individual part instead of having to navigate an entire tree structure to find that one sketch. What can I say, old habits can be hard to break 

[zenkustumz]

ok i know i'm not stupid but its not a f3d file , its says autodesk.com and looks like a hard drive picture.. its not called cantilever cable brake anymore. the precioius file acted correctly and was a f3d file but could not open.

[xander.luciano · Accepted solution]

Try downloading the file I attached to Post #8, that is just a normal .f3d file and should work as you would expect.

[zenkustumz]

Got it now.. thanks again.

Your explanation was very good also. i forget sometimes to make bodies into components.. I have version that seem to also hold into previous versions that  i cant delete from my library..

Very aggravating..

Is there a way to clean this? or undo a relationship to another file?

Again thank you..

John

[xander.luciano]

No problem! Glad I could help!

If you wanna break a link to a referenced file, you can right click it and choose "Break Link"



Is that what you are looking for?

Happy modeling - and if you feel any of the posts answer your question(s), mark them as a solution so others see this post was solved if they are google around and have a similar issue 🙂

- Xander Luciano

[xander.luciano]

Hey @zenkustumz

Hope you don't mind, but I really liked your model so I rendered an animation of it inside Fusion 360!

Here's a link to the gif: http://gfycat.com/ImperfectFlashyAntelopegroundsquirrel

Best,

[zenkustumz]

Thats sooo nice.. i dont know how to do any of that stuff..