Joints stop functioning when inserting into a new design

[Anonymous]

Hi there!

  I've been getting back into Fusion 360 recently and built a small prototype yesterday in it, which contains a few joints. The design seems functional (I can grab parts of the model, and movement is constrained appropriately). However, when I insert this into a new design (I need to arrage 7 of this specific part around a larger part), the joints no longer function. I can drive them manually by clicking each one, but none of the joints constrain properly when I grab the model. Screenshots are below.

Arm design by itself, being moved around fine:

Arm inserted into another design, being dragged in the same manner as before:

As you can see, the component at the back preserves it's grounding (I turned this off and on a few times, as you can see in the Timeline, to see if that would help), but none of the other pieces move correctly. I'm sure it's something I'm doing wrong, but I can't find any additional options when it comes to joint manipulation inside the viewport.

Unrelated: I know there was supposed to be an update soon to allow joint manipulation inside Animation view, but I still don't see the option (I took a month or two off from Fusion 360 to let some of the features cook). Would there be any word on when that will be implemented?

Thanks!

~Lexikitty

[Phil.E]

I'm testing this scenario and cannot reproduce the bad effect.

Would it be possible to add me to the project so I can look at your data first hand?

phil dot eichmiller at autodesk dot com

Thanks!

[Anonymous]

I believe I've invited you correctly. Let me know if you don't see it. 

The original part is "Arm Bracket (v17)", which is being inserted inside "Gauntlet with Arm Bracket (v7)". 

Thanks!

[Phil.E]

Thanks for the invite. I'll check this out today and respond soon.

[Phil.E]

Couple of things:

Thanks for posting this. I've turned it over for investigation by development. I can't find the reason the joints would fail.

Good news is there is a workaround. Try this:

1. When you insert the jointed assembly, the base is grounded. This ground must be removed in order to apply joints to this model.

2. Assuming the base is where it joins the main assembly component, use a joint to assemble the base of your insert to the main component.

3. The assembly comes apart. (this is the thing that should be investigated, this is not expected behavior).

4. Next just apply another joint to re-attach the swing arm portion to the base. The joints seem to work well now.

Please let me know if this helps and when I get a better answer I'll follow up here.

Thanks,

[Anonymous]

Thanks for your quick reply, and for looking into this! 

Unfortunately, following your steps, there doesn't seem to be any change in the results. To check to see if there was something perhaps odd with the sculpted section, I created a new design containing only one component - a box serving as the "main assembly base", and the inserted swing-arm assembly. I un-grounded the swing-arm base, attached the swing arm base to the main assembly base with a Rigid joint, and then attached the swimg-arm bracket with a Revolute, as below. 

Again, animating/driving the joint works fine. But as soon as I click and drag the swing-arm, it ignores the revolute and wanders off into space:

I zoomed fairly far out and tried to see if the swing-arm was following any other sort of constrait (perhaps a ball-joint or cylindrical joint around a different axis/component) but there doesn't seem to be any limitation to it. The test/basic design is called "Gauntlet with Arm Bracket 2" inside the Testing Desk project, if you need to look at it/send it along. 

Thanks again for your help, and sorry to be a pain. I just need to start protyping something for a project beginning June 1, and I'm trying to use this as my migration point to Fusion 360 from Blender/Sketchup. 

Cheers, 

~LK

[Anonymous]

A bit more data. I also tried adding a rigid joint from the corner of the inserted base to the main assembly base, then re-creating the revolute, in case Fusion was unhappy about me putting two joints along one hole. Unfortunately, still no dice. 

Cheers, 

~LK

[Phil.E]

Thanks for the additional info.

I made a video showing the workaround. In my case it works, perhaps this will help. See below.

As soon as we know what's going on we'll let you know! Sorry for the trouble.

Thanks,

Phil

https://screencast.autodesk.com/main/details/3f9862e0-0674-4849-bfcb-ccebb9902215

[Anonymous]

Perfect! Thanks for that - it's working now. I believe I may have found the source of the problem, (and it's probably my fault, but I'm surprised Fusion 360 allowed it/didn't yell at me for doing it). 

When selecting the bracket>inserted base joint, you selected the rim of the hole in the bracket, whereas I selected the middle of the hole. This selected a visible Sketch17, which was what I used to cut the hole in the bottom of the bracket. So instead of joining the bracket and it's friends, Sketch17 was being moved over and joined. However, that doesn't explain why driving and animating the joints still worked, but it does perhaps give some insight to the dev team on where Fusion got confused. Perhaps in later versions of Fusion, joint selection can be restricted to components only, and not sketches. *shrug* Thanks for your help, and sorry that it ended up being my fault!

Cheers, 

~LK

[Phil.E]

I'm glad it's working and thanks for the additional info. Sometimes it's the little things and this should be shown to the UX team, so thanks again.

For the sake of any other users that may encounter this, toggling sketch visibility (off) or using a Selection filter would help to prevent this.

[Phil.E · Accepted solution]

Here is a more detailed explanation from the developer:

"...the sketch was in the root of component A. Hence it was automatically grounded (root can’t move). This made it work properly in A because the component that was supposed to be joined was grounded (my guess). Note: if the component that was supposed to be joined was not grounded in A, the user would have noticed the mis-selected component earlier.

When A is inserted into B, A:1 becomes ungrounded. This is proper and would cause headaches if we grounded A:1. Once the sketch is free to move, the joint no longer functions as expected.

So there are two issues:

1. It is easy to accidently attach a joint to sketch geometry instead of body geometry. This is a selection priority issue, not a joint command issue I think. Normally, this would be noticed sooner, perhaps during joint animation. In this case, due to grounding, it was not noticed.
2. The root of an inserted component is ungrounded in the parent. This is proper, but can cause confusion if joints are created with assumption that it will stay grounded.

[Anonymous]

Wow, thanks for the detailed explination. I really appreciate the level of detail in your answer. I only have one question - what defines/identifies a sketch as being the "root" of a component? The sketch in question was applied halfway through the design of that component, and is in the middle of the list, so I just wondered if there is an easy way to identify (and manage) sketches considered as "root" by F360. 

Other than that, I'm totally up and running, and I will pay closer attention to accidentally interacting with sketch geometry!

Cheers,  

~LK

[Phil.E]

Great question.

For designs with one component, the root is the entire component: sketches, bodies, analysis, construction, etc. with necessarily no joints or subcomponents.

Since Fusion allows each file to be either a single component (minimally perhaps just one sketch, one body, no child components), or an assembly (multiple components), or BOTH (!), there are some rules that allow this flexibility, but require a little diligence. Yours was a "BOTH" case and  the Arm Bracket is a good example of top-down design.

In Top Down designs, it's possible that all sketches and bodies start at the root and later get pushed into Components. This is totally fine for a single design that will not be inserted into other designs. And actually, most of the time there is no problem at all with re-use/insertion. In your case, we found a UI problem, but the program was functioning as designed. The next update has improvements to this area.

Generally, the best practice for top-down designs that are going to be assemblies:

1. Use New Component (RMB top root node)

2. Activate the new sub-component.

3. All sketches and bodies will go into the sub-component that is active.

4. Activate the root to add things to the root - like inserting more parts.

Here are some pictures.

Use the radio button to activate components.

Another benefit of this style:

[Anonymous]

Jibbers Crabst, y'all are a helpful lot. Thanks very much for that additional information - it lends a lot of clarity to the situation (and how to cleanly edit assemblies). Good to know for this and future F360 designs!

Cheers, and thanks a ton, 

~LK