Revolute joint with limits gets stuck on one side during rotation (Mac OS 10.14)
I would suggest you go through the introductory tutorials in the Support & Learning sections.
Your small model already contains several incorrect techniques that will make things more difficult as you proceed in th design.
As as it pertains to assembly, one of the components needs to be grounded.
It's not a bad idea to familiarize yourself with Fusion 360 R.U.L.E #1
The answer is in my post. Please ground one part. Then the joint limits will be properly observed.
You are correct, that is unexpected behavior and looks like bug to me as well. Thanks for posting this!
I still would recommend for you to go through the tutorials, because if you did you would not have modeled this the way you did.
I saw the behavior in the file you shared, but I was able to get it to work by re-building the joints and setting the limits. I'm not denying that this is an error but at this point I'm looking for what is causing it. It could have something to do with your hardware which is why I was asking you to try it for me. If you remove the mirror, create a new component and rebuild the joints from scratch does it give you the same behavior?
Thanks for your help 
Ok, that's good info. Thank you for your help and attention!
I've logged this with the team as FUS-47386 so they can start working on it.
Let me first say that I don't always do this for quick tests either, but in general it is a good practice fo fully constrain and dimension sketches. In Fusiosn 360 you can drag sketch elements in the viewport, even when you are not actively editing a sketch. While that can be very useful, it can also accidentally destroy your design.
In order to fully constrain and dimension a sketch some sketch element needs to reference the sketch origin, circled in red below. That can be with a constraint or dimension or both.
It can also be fully defined by referencing projected sketch geometry.
Once a sketch if fully dimensioned and constrained it all sketch elements will turn black (in the Infinity Pool environment). The sketch icon in the browser will get a pin aded to its icon.
However, the first thing to consider when starting a design if this is only for a single object or if this design is going to be made from several discrete objects. In that case you should not start with a sketch, but probably with making an empty component and activating it. I'l refer to Fusion 360's R.U.L.E #1 so I can save myself some typing here.
Then you use a cylinder primitive to create. whole. Noting "wrong" with that. But danger is lurking here. ON creation the primitives snap to geometry, but that snapping is not parametric, meaning that when you change the length of one of the arms the hole will not update accordingly and remain in the old position.
The next thing you'll notice is that all of your sketches are somewhat disassociated from the geometry that they were created with. Working with Fusion 360 R.U.L.E #1 will prevent thins IF you don't use the move body feature, which are the tow cross hair arrow icons in the timeline. This is a modeling tool and should not be used to move objects into location for assembly.
We squashed this bug with our recent September update. Please feel free to report back if you can still reproduce this issue.
Thanks!
Rishabh Bisht
Product Owner
