Fusion 360 unable to handle "large" assemblies

[Anonymous]

Dear Fusion 360 team,

From the beginning we have been big fans and great supporters of Fusion 360.

Me and 2 of my engineers have followed the Fusion training course locally and we enthousiastically (but step by step) migrated from Solidworks to Fusion.

In the beginning we took the lag and freezes while working on it for granted. It is/was still new, (almost) every update brougth some improvements. But still we do our production drawings on SW, because of speed and ease of use.

The main reason for sticking with Fusion was the easy way to collaborate and the fact that it runs on Mac as well.

In the meantime we have been able to design a complete new machine on Fusion. However the last part of the design process was hell. Which is quite an understatement. 

We now have stranded in a situation where it is merely impossible to work in a normal manner.

When designing a toaster, the program is probably great, but as soon as you create a 50+ parts assembly and/or put some 50+ parts assemblies together the fun starts....

We have had great help locally from Autodesk Germany. So let me start by first thanking Mike Grau for his help and support so far.

He checked hardware, internet connections, settings, etc. Great job.

I do however have a small problem with the final conclusion/answer.

- Fusion can not handle large assemblies. Probably in the future...

solution: 

Simplify as much components as possible by deleting bodies and faces
Re-model imported SolidWorks files where possible
Use Selection Sets to Hide not important components
Reduce the number of features by a scroll back in the timeline

If there were parts or faces in the assembly that we could miss, they wouldn't be there. Trust me.

We are far from building airplanes or any other complex assemblies and I do not consider our assemblies large. Even our old SW could handle our assemblies easily on our old workstation. 

I am sorry but I can not categorize this as a solution. 

So why market Fusion 360 as a SW alternative and why promote it with nice complex assemblies (for example the model of the sportscar) when in reality it can not handle a simple assembly of a machine?

Maybe you target a specific market of designers that make toasters, bicycles and other comparable products. If so, that is fine.

However reality is that I now ended up with disappointed engineers and a situation where we have lost confidence, hope and enthusiasm. One of us is already back on SW.

My believes in Fusion as the future platform for 3D cad, keeps me from accepting that this is the end of the line for us.

I am convinced that the majority of cad users have "larger" assemblies. Are they all encountering the same problems?

Could someone please give me some sensible advise what to do next? Go back in time with a traditional cad-program? Back to SW? Inventor? Try Onshape?

Thanks in advance.

Ivo Geukes 

[jeff_strater]

A 50 part assembly is not a large assembly (although if your 50 parts are each very complex, it could be).  If you are seeing bad performance on an assembly of that size, then there is a problem that needs to be addressed, certainly.  Is it possible to share one of your larger designs with us?

Just one question:  You are not, by chance, using Contact Sets for any of these designs, are you?

Thanks,

Jeff

[TrippyLighting]

@jeff_strater

http://www.gkspackaging.com/machines.html

Fusion 360 should be able to handle such machinery on a more up-to-date computer.

My current project has 400 comments and runs smoothly on a 6 year old i7 iMac.

[Beyondforce]

Hi @Anonymous,

I just want to add few things to @jeff_strater post:

1. If you have a complex sketch, which you are using to create some or all the bodies, that will effect the performance. Simplify the sketches and divide them to small sketches instead of one complex sketch.

2. You should avoid by any means Sketch Pattern! If you need to create a Pattern, then Pattern the features (Filets, Holes...) instead.

3. Make sure there are no Yellow or Red errors in the Timeline.

4. As @jeff_strater stated, don't use the Contact Set! It is a really cool feature, but it's downside is, it takes a lot from the performance.

Cheers / Ben
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[O.Tan]

Hi, I have similar issues as you where I work in large assemblies and Fusion just doesn't run well.

There's a few workarounds I can think of. 

1. I find that PC gives more FPS then the Mac version, so if you're dual booting. That could help

2. When working in a large assembly, to edit your parts, I would recommend using isolate as it'll turn off other components. So for example, if you're working in a sub-assembly, you just isolate the sub-assembly and work from there. Rather then using the unisolate command which will get all the components turn on again (and gives you performance issue), what you could do is to select other components/sub-assembly and click on isolate again.

3. You could try to turn off auto-aliasing (Display Settings > Effects > Auto-Aliasing)

4. Personally, this is my preference settings for graphics

Now I do wish Fusion would improve its large assembly performance, I already shared samples of non-NDA project that reflect Large Assemblies to the Fusion team previously and I hope some work is being done on it. And can anyone answer me, why does Fusion takes a long time to open large local-cached assemblies? When I use other softwares like Inventor or SolidEdge, the same assembly on the same hardware loads much faster wheres Fusion is embarrassing slow. 

[jeff_strater]

Another question:  When you say that the performance is bad, exactly what aspects of performance are you seeing that are bad?  Load time?  Viewing operations (rotate, pan, zoom), adding new features to the design?  Editing sketches or features?  Dragging components that are joined together?

Any additional info you can supply is appreciated.  It will help us improve Fusion, and we can possibly help you improve your experience as well.

Jeff

[Anonymous]

@jeff_strater Nope. No contact sets.

[Anonymous]

Tnx @Beyondforce for the tips. We already keep things as simple as possible without patterns etc..

[Anonymous]

@O.Tan Tnx for the tips. We will double check these settings again. @Anonymous

[Anonymous]

@jeff_strater

Hi Jeff, 

To be blunt....everything runs bad. Loading time, handling, moving, the whole works.... Both on pc and mac.

We already shared a complete machine design with @Mike.Grau.

You can open the case and contact him for more info.

Case no. 12354870

[Anonymous]

@TrippyLighting

My point exactly!

[Anonymous]

@Anonymous Can you share the same file with @jeff_strater as we have done with @Mike.Grau?

[O.Tan]

It's just a guess, but could it be that Fusion decision to have 1 single environment vs part and assembly causes poor performance when it comes to larger assemblies?

As unlike the traditional part and assembly, Fusion 1 single environment requires the software to make all surfaces editable all the time whereas in traditional part and assembly, these tools are somewhat reduced to managing part positions and relations to each other.

Adding to that, I do find turning off timeline somewhat improves performance in some areas as at the moment, Fusion really treats DirectModelling as a dumb modelling environment so the software doesn't have to constantly track changes for the whole assembly. Not sure how well is the programming done for the timeline but I'm not surprise if a very long timeline (even if the user follows Rule No.1) will eventually degrades performance.

Of course there's a pros and cons to both methods but I wont be getting into them at the moment as I'm just checking if this could be the reason of poor performance when the assembly file gets larger and that Fusion requires an even more powerful computer to handle these files in comparison to other traditional CAD softwares.

[Anonymous]

I run with history permanently disabled and have very poor performance on what I would call small assemblies, I do not think resources are the answer to this problem as when my performance starts to degrade I am only using just above 45% system memory.

I know when to shut Fusion 360 down just by how the program is responding and I know that system memory usage will be just above 45%, closing and restarting a program every 20 minutes or so can be a real pain.

[TrippyLighting]

Folks, before continuing the "me to" conversation, please provide some detail.

I'd be more than happy to help, but continuing to make assumption based on vague data is really unproductive. What is "large" to one user may not be large to another.

I've worked most of my career with custom automated machinery in two of the worlds largest automation machinery companies here and here.

In those environments a larger Assembly had easily a 1000+ components. I've never left the large assembly mode in Solid Works and parts and subassemblies were loaded lightweight.

As I mentioned above my current project has ~400 components and performs smoothly on a mid 2010 i7 iMac. I see no reason why an assembly with 1200 components would not perform smoothly on a more recent machine. In fact, in Kevin Schneider's class last week at Autodesk University (Assemblies - Master Class) last week one of the demo files, a  CNC machine with 1200 components, performed quite nicely. 

1. How many components/ assemblies/subassemblies are in your design?

You can get a relatively easy and quick shot at the situation by typing component.count into the text box command field 

2. Are any linked components/assemblies in the design ? Can you show the browser tree ?

3. What area of performance is bad ? Screen performance e.g rotating and panning geometry ? Or editing components/bodies ? Adding/Editing features or editing sketches ?

[Anonymous]

Tnx @TrippyLighting for your reply on my post.

I agree, a me too is not helping.

To already answer one of your questions regarding performance. I seriously do not know where to start by mentioning what is not working properly.

Looks like the whole system comes to a slowwwww-down.

I will be back at the office within the next hour and will do a part count as you suggested.

You are always weldome to take a look together with us using teamviewer. Then you can really experience what the problem is...

Is this maybe an option?

I will get back to your other questions.

cheers, Ivo 

[Anonymous]

@TrippyLighting

component count gives the following result:

Component.Counts

With Overrides: LeafOccurrences 1514: Bodies 1611: VisibleLeafOccurrences 1504: VisibleBodies 1599: LeafOccurrencesWithVisualMaterialOverrides 5: OccurrencesWithTransformOverides 209

I should mention that the problem starts as soon as we are building the complete machine assembly out of the modules (assemblies) from the ground up.

We start with the frame, then insert one assembly after the other.

After adding another assembly the performance collapses further and further...

See also a screenshot.

[PhilProcarioJr · Accepted solution]

@Anonymous @Anonymous

What I am about to say is in no way meant to derail your view on this problem, because it is a big problem.

In Solidworks I can build huge assemblies that have great performance. Huge in my opinion is larger then 5000 components.

Coming to Fusion I hit the performance issue very fast and had to develop a way around this, or at least make Fusion not run in turtle mode.

Right now I am working on an assembly that is 2700 bodies and growing and my performance is acceptable.

I can't say for sure if this will help in your case or not or if it is even a viable solution for you until they can work out large assembly performance but I will throw this out there just in case it helps at all.

What I had to do before creating any large assemblies was convert all models into dumb solids (while keeping the originals in case there was a need for editing later.)

Then I used only dumb solids in my assemblies with history turned off.

This worked great for me with the only inconvenience being you can't edit models in the assembly.

So if you have to make a change you edit the original, export to a dumb solid and replace the model in the assembly.

Do all joints last and make sure you have no linked components.

I realize this is a very inconvenient way to work and improvements need to be made to Fusion but this might allow you to continue on with your projects.

Currently Fusion just isn't setup to handle large assemblies properly and if work arounds like the one I posted are not a viable solution you may want to look to Inventor.

Getting large assemblies to have great performance is a very large coding challenge and given the cloud latency making things worse it will be a long time before you will have Solidworks like performance in Fusion with large assemblies.

I might also want to add that I am in no way trying to steer you towards Solidworks as there are a crapload of issues in their yard also...large assembly performance just isn't one of them.

[Anonymous]

How do you quickly convert your assemblies into solids (a single part)?

This could work for us for the time being.

[Anonymous]

How do you quickly convert your assemblies into solids (a single part)?

This could work for us for the time being.