Fusion 360 Assembly Modeling Strategy

[billdresselhaus]

My students need to first model OTS components, then model subassemlies containing these components, then model a final master assembly of all subassemblies. QUESTION: What is the best Fusion 360 modeling strategy for this...model each OTS component and subassembly and master assembly in separate files and combine sequencially, or model everything in one file from the start??? In Inventor, the first way would be preferable, I think, but Fusion 360 does not have assembly mode, right???

Thanks,

Bill

[Phil.E]

No worries at all! I'm just glad to help.

Regards,

[Anonymous]

So what is the update on sub-assembly/separate x-file updating? Reading through this post it was to be implemented almost a year ago? 

I'm running into the same problem. I want to build sub-assemblies in separate files and have them all update in a master assembly as I make changes. It makes things way to complicated to try and build/assemble everything in one assembly file. Right now if I make a change I have to go back to the sub-assembly files I created and make changes--bit of a pia.

Thanks,

Brent

[TrippyLighting]

External components/assemblies has been implemented quite a while ago.

What makes it so difficult managing different assemblies and subassemblies in a single design/file ?

[Anonymous]

Hmmm, my sub-assembly files do not update when I make changes to them in a master assembly file--I can't use "get All Latest"? If I edit a part in a sub-assembly from the master assembly file, I still have to go back to the original sub-assembly file to update the changes, and then I have to return to the master assembly file and update that file. There is no automatic updating from the main assembly file throughout the chain. Am I doing something wrong here?

I'm dealing with small precision parts and assemblies.

Why "don't" I like having everything in one assembly file?

1) I have better organization of parts and complicated assemblies using separate sub-assembly files.

2) I can't create sub-assembly libraries in a single file.

2) I can't re-use sub-assemblies that are not saved into a separate files easily--unless there is something I am missing here?

3) It makes a complicated master assembly and design much easier when I have sub-assemblies.

5) etc............

[Anonymous]

Ok, after digging around I found this under the road map:

http://forums.autodesk.com/t5/fusion-360-product-roadmap/roadmap-check-in-may-2016/ba-p/6323238

"Deep update" they are calling it. This is what I need:) Looks like it has not been implemented yet. Unless there is something I'm missing......

"Deep Update

Previously if you inserted a design with referenced designs within referenced designs into a new design, then made changes in the deepest one, you had to go into each design and get all latest in each one with a referenced design. No, that’s not a riddle. Deep update allows you to get all latest for the entire stack at once. We’re estimating this to be available around June."

Big Thank you to the Fusion360 team.....I like the direction Fusion360 is going. Now the ability to work completely offline would be great:).....lol.......

[TrippyLighting]

Yes, deep update is certainly going to help you but one or two of your earlier statements has me wondering whether you are actually using the correct workflow with components.

If you are first creating sketches and then create 3d geometry (bodies)  and then create components from these bodies, that will certainly be very much limiting you in how to organize components into assemblies and subassemblies and how to make these re-usabe. It also makes the timeline a bear to work with.

 Many folks that come to this Forum also overuse linked components/assemblies. This applies to noobs as well as to seasoned CAD veterans often based on that being the only way you previously could work in other mainstream CAD packages.

[Anonymous]

Well, I'm learning Fusion360. I'm an engineer. My background is Pro/e, Solidworks, and Geomagic Design. I'm not a CAD professional.  In Fusion, I start with a sketch on paper and then design and import oem parts as needed and assemble as needed in a separate file. I use the assembly files to tweek the design and also to modify

geometry within the assembly. I like to have my files and assemblies kept separate for re-uses and organization. I'm sure I could work differently.

[TrippyLighting]

Fusion develops quickly, so in a way we're all learning Fusion 360 😉

A more optimal workflow, which you might well already be following, is to follow Fusion 360 R.U.L.E #1:

Before doing anything, create a component and make sure it's activated.

All objects created after activating the component such as sketches, bodies, construction geometry, joint origins, etc.  are created in that component.

This has several advantages:

1. On activation the timeline is filtered to show only those items in the timeline that pertain to that component. That will make the quickly growing timeline much easier to work with.
2. If a component is exported to the data panel with "save as" this will also export the complete parametric design history.
3. Drawings can only be created from components
4. The joints in the "Assemble menu only work with components.

When another component needs to be edited for example to add geometry, it should be activated before doing so.

[Noah_Katz]

@TrippyLighting,

> Yes, deep update is certainly going to help you

It still leaves an important unmet need, which is to be able to "check out" (I-DEAS terminology) a part so it can be modified within the context of the assembly w/o having to break the link.

More here https://forums.autodesk.com/t5/ideastation-request-a-feature-or/allow-editing-linked-components/idc-...

Is this on a roadmap?

Not to be snippy, but I find it a tad presumptuous to proclaim that F360 is a top-down design tool when quite often real life does not cooperate, i.e. when an OTS part is just a starting point and will be modified to suit.