Make a joint from a body

[paulMVAJU]

I have a body picture below. I have some construction points, but what I would like to do is make a joint. I tried to rough sketch a side view of what I am picturing below. The part with tang would need relief circles. And the part with the outside flanges would need to be circled so as to spin in the relief. I have tried different ways of splitting, but can't get it. Do I have to make two parts separately? Has anyone done a tutorial on this? With my vocabulary, the searches show two components being made into a joint. 

[davebYYPCU · Accepted solution]

Drill the hole first.

make a side view sketch for one piece - in position, 

Offset that chain of lines, the join them together for a sketch shaded profile of the gap.

Extrude > Cut > though All, 

make both parts to Component from bodies.

Use as built Joint to > Revolute

Set Joint Limits, 

Might help....

[paulMVAJU]

Yes, it helped. In fact other than the rounding which I should be able to do now it might work.

I may have more questions if I not I will post the final solution.

I did not know what an offset chain was until I searched. 

 

[davebYYPCU · Accepted solution]

Rounding - Select all the small vertical edges, and enter the radius (half width of bar) in the Modelling Fillet command, 

Might help....

[chrisplyler]

1. I used a single, common sketch to lay out BOTH components. As such, they were modeled in the right, relative place to each other. You don't HAVE to do this, but it kinda makes things easier.

2. Joints only work between components, so each body has to be its own component. Every part should always be a component.

3. Since I modeled both parts in position to begin with, I can use an 'As-built' joint. If you model them elsewhere, and need to move one of them into place relative to the other, use the regular Joint, not the As-built.

4. You'll see me go back and add a line to the original sketch, and edit the extrusions to correct my geometry stupidity.

5. You'll see me add Limit values to the joint, to prevent the bars intersecting each other.

https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/screencast/Main/Details/e00ca66...

[paulMVAJU]

Yes, that made life so much easier. Before the Fillet, I was using sketches and Extrude/Cut.  

I still have just a touch of interference. I will play, but I assume I need to move the hole.

A question, you 6 sides which leaves a straight edge. I Fillet the other but I can't tell if it helps any more.

Maybe back to moving the hole. I am learning now so I am going with the split, but in reality, I may switch to a half lap kind of joint, to make it easier to lock down after positioning. For now, this has been a good learning experience. 

Getting close.