Assembly of Components (Joints not working)

[Zero__]

Hi guys,

I am making a big assembly using a lot of joints. I've been linking individual bodies together using joints and everything has been fine. However, for the first time I made a separate "sub-assembly" and brought that into my Assembly. When I try to position this sub-assembly using joints, the joints do not seem to work. For instance, I made a Planar joint between one plane of this subassembly and a plane of another part in my assembly. Though my subassembly went to the right place, I can just grab it and pull it away. It isn't locked to the plane I just jointed to, and I have no idea why. A line shows up showing how offset it is but when I right click on the joint and Edit it, it ishows there being no Offset. Confused why I just made a mechanism using joints but now they seem to not be holding. Advice would be great!

[jeff_strater]

If you are willing to post the design, it would help us debug the problem more quickly.  However, just from your description, my guess is that the way that Fusion treats sub-assemblies may be getting in the way.  In Fusion, all sub-assemblies are "flexible".  That is, constraining to the sub-assembly itself does not constrain any of the child components.  So, if you are constraining to a plane that is owned by the subassembly itself (as opposed to the component inside of the sub-assembly), it will appear as if the sub-assembly is not constrained at all.  You need to either:

1. if you want your sub-assembly to act as a rigid body, then create a "rigid group" for all of the components inside that sub-assembly.
2. If you want the sub-assembly to be flexible, make sure that all components inside the sub-assembly have joints that completely describe their behavior, and create joints not to the sub-assembly itself, but to the child components.

I can try later (tomorrow - headed out to a wedding just now) to make a screencast to illustrate.  In the meantime, if you can post your design, I'd be happy to take a look at it.

Thanks for posting!

Jeff Strater (Fusion development)

[Zero__]

Hi Jeff,

Thank you for the info. The first thing I did after I added the subassembly to my higher assembly was right click on it in the part tree and select "Rigid Group". Yet, still, when I tried to make a Planar Joint between a face on the subassembly and a face on the assembly, it wouldn't hold. Also, the subassembly's movement is completely defined with its own internal joints, so no components get left behind when I drag it around my higher assembly, whether I've selected Rigid Group or not.  I'll happily post my design, but I'm not sure how. Here is the public link, if that's what you meant! http://a360.co/1GbLw8N

The subassembly in question is "motor assy". When I try to make a Planar Joint constraining it to either the Slant Support or Untitled, it doesn't seem to hold.

Enjoy the wedding!

[jeff_strater]

Thanks for the design link.  That definitely helps.

A couple of observations I noticed from looking at the design:

1. there is one rigid group that is not happy:  RigidGroup36:
   
   
   if I edit that group, I get a warning that there is also a joint among some of those components:
   
   
   so, I deleted that rigid group.  I'm not sure what that was trying to do, but in its current state, it can only hurt.
   
   
2. There is already a planar joint between "Untitled" and "Motor Platform" inside of "Motor Assembly".  You can see this if you try to create a new joint between these two:
   
   
   
   This is Planar45, so I deleted this joint
   
   

After that, things seemed to behave how I expected.  I could create a planar joint that behaves as I expect it to.  Here is a screencast:

Hopefully that helps you move forward on your design

Jeff

[Zero__]

Jeff! Thank you! That seemed to do it. Do you think it was the Rigid Group or that lingering Planar Joint that was the problem. I'll have to be more careful in the future. One difficulty I have with Fusion360 is that after you make a lot of Joints, it's hard to figure out which is which. I really wish it said when I edited a Joint which two parts it was constraining, or at the least, the two faces/points/edges that were constrained together highlighted. Either of these would help a lot.

I've got another question for you. I'm assuming that to measure the angle between two planes - in order to make sure they are parallel - you select Measure and select the two planes. If the angle is 0.000, they are parallel, yes?

I have two Slant Support parts in my model. The outer face of one Slant Support is not parallel to the outer face of the other Slant Support. When I Inspect>Measure the two outer faces, the Angle is 0.1. I assumed one of my hole patterns was off or I'd made a small modeling mistake. But I've checked a lot. I checked the Slant Support part, thinking the hole pattern was misaligned. Everything was square. I checked the Untitled part they both align to, and sure enough, the hole pattern on both sides was square.

Then - as shown in the picture below - I checked the Angle between the outer face of one of the slant supports and the outer face of one side of Untitled. Sure enough, the Angle read 0.00. Then I selected the same face on Untitled, and the outer face of the other Slant Support. And sure enough, the angle read 0.00! Now, if Plane A is parallel to Plane B, and Plane A is parallel to Plane C, then Plane B must be parallel to Plane C, correct?

For the life of me, I can't figure out why the outer faces of each slant support are not parallel to one another. The only thing I can think is that the Measure tool is not giving me the angle between the planes in the way I'm thinking it does?

[Zero__]

I managed to find the problem. Thanks though and thanks again for your help with the assembly joint!

[jeff_strater]

Glad you were able to fix the problem!  Good luck going forward on your design.

Jeff

[Zero__]

Hi Jeff,

Got another question for you. The model's come along quite a way and all has been great. I've changed hole patterns, added slots for brackets, and updated the main assembly hundreds of times over the past week. Everything holds together just fine. Last night, I added in a quick hole pattern for a mcmaster braket and updated the main assembly. It exploded. Every joint broke and the parts were all over the screen. I was dumbstruck. I assumed it had to be some sort of weird glitch. I ctrl+z's the Get All Latest command (the model reverted back into it's state), and tried to update the component (Untitled). Sure enough, my entire assembly exploded again. I'm pretty confused. What could have happened to break my model? As it is I can't update my main assembly without it imploding, but having to rebuild the entire thing would be quite a pain - there are about a hundred joints involved. Do you have any idea what might be happening?

Link: http://a360.co/1GbLw8N

[O.Tan]

I have the exact problem with Fusion when there's just too many joints, I ended up grouping related things under rigid group and joints for the actual connecting/motion related parts but the negative of that move is, editing components becomes real hassle as I'll have to remove the affected components from the rigid group first before making my modifications (depends on how severe the part change is). I wish Fusion has a proper workflow or alternative for this

[jeff_strater]

Hi @Zero__,

It looks like the link you sent me does not have "allow download" enabled on it:

But, that may not be enough, since your problem is with the update.  The downloaded file will just contain the current versions of referenced designs.  What I really need is to have you invite me to your project.  I can get what I need from there, without modifying your design at all.  If that's OK, then invite jeff.strater@autodesk.com to your project.

thanks,

Jeff

[Zero__]

A-ok @jeff_strater. I just invited you to the project.

[jeff_strater]

Got it.  Thanks.  We're taking a look at the design.  Sure seems like a Fusion bug at this point, but we'll let you know what we find

Jeff

[Zero__]

Thanks @jeff_straterJeff. Any updates or workarounds? Making it a little hard for me to move forward with my design.

@O.Tan, thanks for the suggestion. I'll try making the non-moving frame a rigid group and seeing if that helps hold it all together.

Edit: It's no good. It just broke my rigid group. This is rapidly becoming a big problem so I really hope some progress is made soon.

[jeff_strater]

unfortunately, your design continues to have us scratching our heads.  There is clearly something wrong here in Fusion, but we have not yet figured it out.  Something in (we think) the "wing" component went haywire, but we are still looking at it to see if a) we can prevent it, or b) we can fix your model.

Sorry it is taking so long, but it's not for lack of effort.

Jeff

[Zero__]

No worries @jeff_strater, really appreciate your guys' support!

[anuhya.das]

I had a quick question about joints as well! In a sub-assembly, I have a slider joint which works perfectly, but in a larger assembly, the component jointed moves around freely. However, all the other joints work perfectly fine, including a different, identical slider joint. Do you have any idea on how to fix this joint so it works in the larger assembly?

[jhackney1972]

Your really need to start a new thread.  When you do, please attach your model and indicate the problem area.  To attach your model, open it in Fusion 360, select the File menu, then Export and save to your hard drive.  Attach it using the Attachment section of your post.