Another day of my life wasted on fusion, insert component garbage nonsense.

[Anonymous]

So I spent a day tweeking an assembly which had been imported into a larger project.

After updating the assembly in the larger project where it is used I noticed after doing quite a bit of work in the lager assembly that things were off with the imported assembly. Going back to the original component assembly it was fine. I tried redoing my changes with align and capture position. No dice it's still wrong in the imported assembly ?Even after update. I don't care what vodoo and happy dance you need to get fusion to work. If the original assembly is correct who thinks it is professional or even acceptable to have a part that is correct in it's original document to CHANGE when imported to another. How can Fusion ever be trusted with this behavior? Even an error warning that positions were altered from the original  would help. HERE IS THE KICKER. When I import the component assembly into a NEW design IT IS FINE!  How can send fusion files to be CNC'd  without triple checking every detail after I had already done that  in the original assembly.  I fixed it by breaking the Link removing the assembly and reinserting. So somehow the update function isn't right. I won't even get into the fact that I need to export DXF because DWG doesn't work even with Autocad's conversion tool.  Yes caps and yes bold, but no curse words considering I lost a day I can't bill for I'd say that is kind.

[seth.madore]

I'm not a "pro" modeling guy by any stretch, so take this with a grain of salt. I just wanted to acknowledge your post and provide my two cents.

Align and Capture positions are not the way establish relationships. As you can now see, they don't behave as expected in all scenarios and it's frustrating. What you should be using is Joints.

[Anonymous]

Seth thank you for your input. Before trying to fix this issue I did study videos on youtube posted by autocad. There is a full video "Fusion branded" video on building an assembly without using joints. As well I am designing as I work so I am making constant changes. I figured out what Fusion 360 is doing wrong in many ways. After placing the assembly in the larger assembly it was moved. When I updated the assembly in the original drawing I added screws and a new component. So when the 1st assembly was updated in the second assembly it didn't include the "move" in the second assembly. Yet the "move was in the second assembly's timeline. That is just wrong. So the screws were displaced. What is even worse I had included as sketch in the second assembly which had a hole to accommodate the 1st assembly. The modifications to the original part required. Even though I broke link and removed the 1st assembly, when I go back to edit that part I see the first part I no longer an using. That to some degree I understand as that was the state in the timeline when the sketch was  created. But inserting a part and moving it into position and not having that move factored in when a component is updated creates a dangerous situation for designers. The 1st assembly is fine when inserted into a new project, it's just that a project that was using it does not update properly. I would agree with you if I wasn't able to insert the assembly into a new project without problems. Thanks for your comments. ( not said with sarcasm)  Brad

[jeff_strater]

@Anonymous - this is a very important point to understand.  The behavior you described is fundamental to the way that Fusion works.  If you insert a design into a higher-level design that is NOT constrained using joints, then subsequently move components in that inserted design, you are only moving those components.  As you have seen, that move does not apply to newly added components in the inserted design.  This is intentional, as it captures the intent of that move.  This is, in fact, why the advice that @seth.madore offers is so important.  If you had constrained the referenced design with Joints, then you can fully constrain that design so that it all moves together.  Then, if you add components to that design later (provided they are also added with Joints) then any referencing design will be updated in the way that you expect.  Another way to achieve this, if you have a fully rigid sub-assembly, is to just create a rigid group of all components in that design (remembering that you need to update the group with new components when they are added).  Rigid group is really just a shortcut way to create rigid Joints between components.

You reference a video that advocates placing components without using Joints.  Can you point me to that video?  If it is, indeed, one produced by Autodesk, I'd like to know that, so we can take it down.  That method is NOT recommended, for exactly the reasons you describe here.

[Anonymous]

Jeff

Thank you for your response.

First here is the video. https://youtu.be/_W1S5EXHpvs

"Joing parts without Joints"

He does select the entire assembly and make it a rigid group. Yet to work out a design in the software with the design being fluid possibly Fusion isn't for me.

Now What I believe needs to be explained to me is why is the Fusion 360 method is an advantage not a fault?

If I design a carburetor in one assembly and an engine in another assembly. I insert the carburetor into the engine assembly and move it to align with the manifold. Later I add butterfly valve to the carburetor in the first assembly. Then "get Latest" the second engine assembly. Now in the engine assembly the the butterfly valve is not longer in the carburetor. What is the possible advantage of fusion not looking through the time line and making the proper adjustments of the whole assembly? This to me is even more baffling in that if I insert the carburetor to a new design it is correct. My design is fluid. A large box with many screws panels etc. The word back from the client is that the box is to heavy to meet the weight loads. I now need to push pull the sides and recenter the end panels. The panels have dozens of screws. Since screws were part of the problem here if every screw had a rigid joint to the panels. (The behavior of rigid joints is still not completely clear) but I expect it would be adding many steps. One other question I have is why when a component is moved is "capture position" not the default. It is not clear to me what "ok" means to me after a move, as opposed to capture position. Why would one want "OK" without the capture position selected?

Never the less I am still very curious as to how having a assembly inserted into another assembly, not updating the relative position of internal components is an advantage.  So if a user forgets to rigid joint a single component all bets are off as far as accuracy goes. WYSIWYG does not apply? Fusion can't even throw an error message by comparing positions of the referenced assembly ? seems a little dicey to me.

Another slight box i'm in with this issue. So lets say I updated the "carburetor" because it didn't update correctly I removed the carburetor and inserted a new one. Lets just say I needed to completely redesign the carburetor. So I break link and remove. I insert the new carburetor. I now want to modify the manifold. If I go into the sketch of the manifold I see the old carburetor.  I understand this is due to that is the state on the time line when the sketch was created, yet I feel I'm dealing with Q on Star Trek.

Brad

[jeff_strater]

The main reason for this behavior is so that each instance of a sub-assembly can be in a different position.  Imagine you have an assembly which is a door + a door frame.  You want to be able to insert two doors into your design and have one be in an "open" position, and the other "closed".  For this reason, positioning of child components of an inserted assembly is controlled, not by the inserted assembly, but by the top level assembly, in the form of position overrides.  When you insert a design with child components, the initial positions of those components are in the positions in the referenced design.  However, if you move them, those positions are now recorded by the top-level design.  If you go back and insert more components, the referencing design's move state does not know about those new children (or even know that it is the "right" thing to do to move them - remember the open/closed door scenario).

Now, it's a matter of opinion whether that is a good implementation or not, but if you are looking to understand how Fusion works, and therefore how to avoid frustration, this is important to understand.

The scenarios you describe would all work much better if the designs were all constrained with Joints.  The main difference between the Joint workflow, and the Align/Rigid Group workflow, is that Align is NOT associative to the selected geometry.  If you Align two faces of components, then go back and change an Extrude that moves one of those faces, Align will not update the relative positions of the components.  However, if they were positioned using Joints, they would be.