Double-Ended Ball Joint/Socket Issue
@StellarFusion wrote:Peter,
Thanks for the screencast. You approached the sketch design in a different way that I really didn't think of. I never really considered mirroring each quadrant. Curious though... you had pretty much sketched half of the component. Why didn't you just mirror the half component instead of mirroring it in quarters?
Thanks
That is indeed a very good question. I could have mirrored just a couple of lines in that sketch and then extruded half of the solid and then mirrored that. Sometimes in my own work I do it if I can reduce mirroring to one or two lines. But I have learned not even Avon that often and use more reliable methods.
The sketch mirror and sketch pattern commands in Fusion 360 I find incredibly lacking and they have caused many users a lot of grieve. As such I have learned to avoid them where I can.
In general keep in mind the purpose of a sketch. The purpose of a sketch is to create a solid foundation for base geometry. It is not for example to precisely resemble a finished piece of geometry. Fillets and chamfers in most cases do not belong into a sketch, they should be applied as solid features. If you can mirror solid geometry, then don't mirror sketch geometry. that same goes for patterns.
One more tip for the use of ball joints. Make sure to provide them with some reasonable joint limits. Otherwise they can go wonky. I'ts hard to describe what exactly that means, but once you experience it you'll know what I mean. 😉
@StellarFusion you voiced your frustration with the overwhelming amount of tutorials that are available on Youtube. You suggested that I take a break.
I used this break to go through some of the learning content that is created by Autodesk and is available directly through the learning resources button that is located right here in the top menu bar of of the browser.
No google or youtube search for sketch related content at all. Just official sources which would also include an official Fusion 360 youtube channel, that has a number of sketching quick tips.
I found 5 videos alone that explaining sketching:
https://help.autodesk.com/view/fusion360/ENU/
https://www.youtube.com/watch?v=PwVRaWxW7F0
https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-422FB3ED-0FD0-4E9E-97C6-A90E4E1C60F0
http://help.autodesk.com/view/fusion360/ENU/?caas=caas/video/youtube/watch-v-pqd-wlz9gpQ.html
So, based on these learning resources have you fixed the fully undefined sketches in your design ?
Without that you cannot hope to proceed in creating a functioning design.
@jasonhomrighaus wrote:
Triply,
Do you have any recommendations among those videos? Do any have a heavier focus on constrains? That’s the area where I could use some better understanding on myself.
Jason
No, I don't have a particular recommendation. I'd say the workflow Lars uses in his video is similar to my approach. I first make my sketch functional using constraints and then I dimension.
Sometimes when I develop a form I don't fully constrain my sketch, so I can easier adjust proportions "by feel".
However, before you want to go into manufacturing you should've all sketches fully defined.
Maybe not sketch related but there definitely is some problem that I did not come across in my design:
@TrippyLighting wrote:Maybe not sketch related but there definitely is some problem that I did not come across in my design:
The screencast you've included in your post shows a different design than what I'm working with. True, there are ball joints on each end, but the object they're attached to is more like a strut that has linear movement which is a lot more forgiving. Mine are rigid which I believe is causing the error I'm receiving due to there not being any type of constraint I can apply to the ball joint to make it fit.
What is odd is that I can create another socket that isn't associated to any component and attempt to create the joint and get the error. The fact that you don't get the error until you've already created numerous other joints makes me believe there's a limitation issue with the software as the product manage mentioned.
I have no problem creating an assembly with ball joints that resembles yours in function with the same stiff trusses.
And before you respond that the number of joints is the reason, there are 4*8=32 ball joints in the design below and not a single joint conflict. I can keep going for a long time 😉
The reason for this is that you need to consider the physical limits of your design.
The other design you found on this forum - you might have noticed that I helped that user as well - might well reach the limits of the joint solver, but your design does not. So where does your design differ from the design in my animation above or from the design in that other thread ?
Dude, I'm getting awfully tired of seeing you help people with examples that aren't rendered and self-illuminating. What gives? 
Thanks so much, @TrippyLighting for your time and effort on this thread. I apologize for my own lack of response - I was out of town last week, and have been trying to dig out of that hole this week...
It's nice to see that you can, indeed, create a design with that many ball joints, rigid or flexible. I also agree that the problems that @StellarFusion experienced are also real. What I've found is that the Fusion joint system can be fairly rigid (pun intended). That is, you have to have very precise geometry in situations like this, where you are combining components with more than one joint, especially in the case where the final result is meant to be rigid. It's easy for one component to be just slightly too large or too small, or the geometry is otherwise just a bit off, and that can cause the solve to lock up, or otherwise behave badly. This is often the case for the "joint conflict" errors that you see. So, when @TrippyLighting says that this could be a sketch problem, it is true that sketch problems can cause geometry errors to creep in that can ultimately affect the behavior of the joint system. I'm also not discounting the existence of bugs in the joint solver/data model. I have seen those as well. I've seen some pretty squirrelly behavior in some complex joint systems. I also know that the joint solver is happier when the initial conditions are somewhat close to the final result. If you place a component such that its orientation is very far away from where it ends up, then add a joint, the solve can get stuck. So, I tend to position my components somewhat close to where I expect them to end up.
Not sure I added anything of value to this particular discussion, but I wanted to acknowledge that this is an important topic to us on the Fusion team. If there is more that you need us to look at, let me know.
Jeff
Jeff Strater
Engineering Director
