Assembly: Relationships don't update?

[Anonymous]

Hi there,

I made a joint... a butt joint between two plates to form an L.

I adjusted the length of one of the plates and now the joint forms a ⊥ and it's fixed.

My time spent in CAD has taught me these things update automatically. Are Fusion's joints based fixed to component origin and not geometry?

[Mike.Zhang]

I guess you just selected the center of one plate as Joint Origin, so when you edit one plate, the assembly shape changed.

Could you attach the model you're working on？ It'll be more better if you can show me the before and after screenshots.

[Anonymous]

Hi Mike, sorry I don't have any. I've had the habit of spending so much
time on these forums trying to solve problems instead of just getting my
hands dirty so I neglected to get photo or video of this one.

Take two "boards" with the same length.

Use joints assembly with the edge of one to the edge of the other at the
center of each edge

This produces a 90* butt joint

Then make one part WIDER so it makes a T joint instead of a 90* butt

It should make a 90* butt if it works like all the CAD programs I am aware
of (ie assembly relationships based on features not points calculated from
features)

[Mike.Zhang]

Seems I can't reproduce it. Below is my video to show it.

https://screencast.autodesk.com/main/details/ed6c77c5-cd3e-4a30-a460-49013a0c2ba7

Could you also record the a video to show it on your way？

You can use the free screen recorder of Autodesk to do it.

http://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/ENU/123112/files/download-autod...

And here is a video showed how to use it in Fusion 360.

http://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/video/youtube/watch-v-9ySynnfdlB...

[Anonymous]

Hi Mike, here's a video for you.

https://screencast.autodesk.com/Main/Details/18387e92-1bb6-46ac-8a71-72778268b12d

[Anonymous]

Also, if I mirror a component and then move it, the other one stays stationary. I wonder if this is related?

[TrippyLighting]

There are a few things visible in your screencast. I see a sketches folder in top level, so I am assuming when you sarted that design

1. you started sketching the base extrusions for your components
2. then extruded them to get your bodies
3. created component from your bodies

If that's true, then you eed to change your workflow to eleiminate problems later:

1. Create new component #1
2. Activate component #1 (this is crucial!!!)
3. Sketch your base extrusion
4. Extrude to det a body.
5. Activate top level
6. Create new component #2
7. Activate component #2
8. Sketch your base extrusion
9. Extrude to det a body.

That way your components will have their sketches, bodies, jont origins saved within the component and if you ever want to export a component it'll take all those elements with it including it's timeline and will remain fully editable.

I'll create a screencast to show how you can create your desired assembly function.

[Anonymous]

Hi Luke,

Thank you for the post, I can reproduce your problem now, and I think you found a problem with our software;

Like what Mike shown you, if you just create one body, leave it in Root component, and create another one in a new component, after putting Join with those components, no matter which type(Rigid/Slider/...) you selected, the Assembly relationship would remain there;

BUT, by looking into your video(appreciate for the efforts!), noticed you have two bodies assigned into two new components, and seem hence Assembly been ruined and not automaticlly update anymore... I have reported this problem as a defect in our system and will keep you updated.

Merry Xmas and happy new year:)

- Adele

[adelemm]

Hmm, change to my another account. Please take a look at this video;

https://screencast.autodesk.com/Main/Details/b6e8279c-f59b-4481-ae5e-f094fce02c03

The first part is the problem you hit, and in the second part of this video you can see how it works as desired:) bug has been logged and we will take priorities to look at it!

Thank you for reporting this issue!

-Adele

[TrippyLighting]

Here are two screencasts showing two methods of how to achieve what you are looking for:

This first method does not even require you to joint the components 😉 

https://screencast.autodesk.com/Main/Details/c1a716a4-ed63-4392-bf02-4ef296599285

https://screencast.autodesk.com/main/details/4209db35-ec5e-4980-b3e9-1919dbee9279

[adelemm]

Mark: FUS-15852

[Anonymous]

Adele, I do not understand what was done differently in your second example. First one functionality is broken IMO and second one it isn't. Is there something I'm missing?

[TrippyLighting]

I don't see that there is anything broken. You just have to adapt to slightly different workflow. You'll see that if you watch the two screencasts that I've posted.
I would not be too surprised if there is yet another way to skin that cat.

[Anonymous]

OK but I literally have no idea what was different between Adele's two examples. That is why I say the first looks broken.

I also have no idea why my Fusion won't maintain assembly relationships before but it seems to now.

I have two components with their own body. I made a joint. The joint breaks and doesn't work at all like any of the videos you guys have posted. But now it works. I dont know why.

I'm frustrated because I have no idea what different workflow is necessary or what I'm doing differently.

Is there geometry relationships created/refuted by Fusion in the background that you can't actually see?

[TrippyLighting]

I have to say that I don't understand what is differnt in Adeles first example as well. It looks,like she has two components that are being joined and it does not work. Oddly enough I show in my screencast that it does work.
Unless, of course the difference is how the bodies in these components are generated. I prefer to use the parametric approach, meaning I create a sketch to extrude a body from,.
Adele seems to prefer the direct approach that does not require a sketch, but will not allow you to parametrize. I will need to test that later.

Adeles second example is differnt in that one of the parts is actually just a body that is not converts into a component and the other part is a component (with a body inside).
Try and see if you can make it work following my second video step by step exactly.

Also, i am not sure this makes a difference, but I am not using the F360 version from the App Store, but the one that downloads from the Autodesk website.

[adelemm]

The first example indicates a problem of Fusion that I had reported to our bug system, in some situations Assembly relationship broken, for example Assign two bodies into two separate components. This is what you have seen in your video.
The second example is show how it should work. There is a very tiny difference that one body is been assign to root component, the other one been assigned to a new component.
This problem seems not reproduce every time, but I hope we can fix it so it won't bring confusion to user:)

[adelemm]

Yes, the difference is how the bodies in these components are generated, but in either workflow Assembly relationship should keep:) both my workflows are been finished in Parametric environment.
I'm able to reproduce Luke's problem in his video, will follow up with developer team see how we can address this.

[TrippyLighting · Accepted solution]

I now also have been able to recreate the problem.

If you first create bodies and then turn these into components with "Ctreate components from bodies" this creates a problem. I agree that this is buggy and should not happen.

It would also make a LOT more sense if the default would be "create component" insted of "create body" in direct modeling mode. I bet this problem would not even have appeared if that would be the case!

However, if one adheres to the practice to always first creating a component - this is possible in direct editing and in parametric design - then this eliminates the problem.

Here's a screencast showing both behaviours:

https://screencast.autodesk.com/main/details/f8001510-3c8f-4ffc-aab4-7579a5f6369e

[Anonymous]

Thanks for clearing that up TrippyLighting! I usually draw my part and then turn it into a component. From here on out I will start with a component.