Moving a component breaks its internal joints

[lure23]

I spend more time in the forum than with the Fusion 360 tool, unfortunately.

Why did the wheel come loose?

What I tried to model here:

- The wheel and its support as a single component ("Wheelset"); wheel rotates around the support in that component (rev4).

However:

- When I try to move the component to a new location, Fusion 360 doesn't allow me to select the "Wheelset" component from browser. It allows to select the support from the picture, so I did that.

- Problem: only the support is moved. The joint keeping the wheel in place is ignored.

Why is this?   Is Fusion 360 doing it right?

I tried multiple variations, but it's getting kind of tedious that I simply cannot throw my design intent to the tool but need to "fight" (understand?) the tool, all the time. Lots of friction, in this one...!

[lure23]

Tried with regular joints and -boom- immediate gratification.

Is there any reason I should (ever) use as-built joints?

[whittakerdw · Accepted solution]

Use as built joints when you already have the model set up the way you want it and all it needs is joints. You use regular joints when you have all the components laid out but not in the correct position.

[chrisplyler]

Click-on (highlight) the Wheelset component in the Brower, then press your 'M' key to initiate the Move command.

PS - Also, the wheel support should be a sub-component nested within the Wheelset, just as the Wheel is.

[therealsamchaney]

I'm having the same issue. According to the description of the As-built Joint tool, it should constrain the two components' positions relative to each-other, but when I then go to align or move one of them, the other one stays put as if I never made the As-built Joint.

What's the point of the As-built Joint tool if the relationship breaks any time you move one of the components? It's not really joined then is it?

It seems there is no way to achieve what I would like, which is to simply lock two components together (but with space in-between them) the way they would be in the final assembly, but still be able to move them around as one.

The Rigid Group tool seems like it would be perfect for this, but alas, if I apply a rigid group between the two components then move one, the other one does not move with it, even though in the description of the tool it says "The components are treated as a single object when moved...". So I guess I have to move both of them? Doesn't that completely defeat the idea of them being rigidly grouped? I could just move both of them anyway, I don't need a Rigid Group tool to be able to do that.

I can't use a normal joint because I need to maintain the specific gap between them and regular joints require that the two points mate to each-other.

Just another thing that would be easy, intuitive and reliable in Solidworks and is nigh impossible in Fusion.

[jeff_strater]

@therealsamchaney - you CAN do exactly what you want in Fusion Joints.  You need a regular joint to do it, and you introduce the specific gap in the Joint command.   Not really sure how to make it any simpler than that.  I will address as-built in a separate post.

[jeff_strater]

As-built joint works as well.  In the screencast below, I model the two components with one sketch, with a "specific gap" added in the sketch itself.  But, there are other ways to add this gap.  Basically, as-built joints take the relationship of the components at the time the joint is created, and maintain that during any component move.  However, if you move a body, then that moves the body within the component, and yes, the gap will be violated, because that move occurs in the timeline after the joint.

[jeff_strater]

@therealsamchaney - did this help, or not?

[therealsamchaney]

No @jeff_strater that's not the issue. I'm sorry if I'm frustrated but Fusion can be a very frustrating application. It crashed on me 10 times in one day this week.

This time, however it was a rare case of user error. I had the Move tool set to Bodies when I thought it was set to Components. the Move tool and align tool actually work as expected after applying a Rigid Group when you have them set to Component. Please delete my initial comment or get some other admin who can. Again, I think it's ridiculous that we have to ask to have our own comments and posts edited or deleted. I have heard all the arguments for this and for me they don't hold water. If this policy made sense, it would be used on many other forums across the internet but it's not used on any.

Anyway thanks for your help.

[Phil.E]

@therealsamchaney Thanks for letting us know you crashed. I found 5 crashes from you recently, and they are all related to sketch constraints.

Any time you can repeatedly crash, it's good to send in every report (thank you) but also if you can share a design that crashes when you take specific steps, let us know in the forum here and it can greatly help efforts to fix such crashes. Repeatable crashes are easy to debug. This one you refer to appears to be data related, and thus your help is critical.

I did notice that the crashes are from the previous build. I'm assuming you have updated to 2.0.10560 by now, and I don't see any recent crashes from you, using this build. Did the sketch problem go away with the latest update?

[therealsamchaney]

@Phil.E I have updated to the most current build since but that's not what resolved that crashing issue.

To bring that design back to stability I had to do some fancy footwork with the timeline. The design had a parameter that controlled the height and shape of a body (basically it allowed me to have one design that could switch between different versions of a part) and when I changed the parameter, it crashed for some reason, even though I had used that design for a long time and never experienced that behavior (and this was a parameter that I changed frequently). It took me a few tries of changing the parameter around and rewinding the timeline before I isolated the sketch that was causing the crash. In the end I had to just clear out the sketch and re-draw it from scratch which fixed the issue. The strange thing is I re-drew it exactly as it was before so I still don't know what was causing the instability.

Fusion does some very strange things with sketch constraints I've found. It will pretty regularly just remove or delete dimensions or constraints without telling me. For example, I use extruded text a lot, and I usually dimension the vertical of the textbox so I can use a parameter to control the text height. About 8 times out of 10 changing the text height parameter works fine, but the other 2 times, it will just delete the dimension, as if I had never put it there at all. Other times, I have noticed my designs acting weird and found that one of the sketches earlier in the timeline was now  showing as unconstrained whereas it was previously fully constrained because Fusion had deleted a mirror constraint or something like that. I'm guessing this is some unhandled corner case where Fusion can't compute but it isn't caught by the exception handler.

Another example is that sometimes I will change a parameter and I will get a "compute failed" error in a sketch even though the value I changed it to shouldn't cause any problems. I will go into the sketch, delete the red dimension, and recreate the exact same dimension with the same parameter and it will work fine. 

I have started to export designs to my computer when I encounter these issues and post them on the forums but a lot of the time, I will make a detailed bug report post with attached screencast and/or design, and not get any responses at all which is pretty discouraging. 

I really wish Autodesk would create a dedicated bug reporting pipeline here.

Thanks!

-Sam