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 

[Anonymous]

I will share link

File is too big for sending

 I will invite you

Can you give me your email address

regards.

Pieter

[Phil.E]

@Anonymous

I sent you a PM via the forum messaging system.

Thanks,

[Anonymous]

OK

I send link via PM

Hope it will work

regards,

Pieter

[Phil.E]

@Anonymous

Thanks for the model.

On my machine and on Jeff's machine, there is definitely some heavy load on performance, but nothing like what you are showing in the video.

This makes me think it's video related.

Couple things you could try to optimize video:

Use only one monitor (if you have more than one running on this video card)

Turn off all graphic effects (use the graphics diagnostic tool found under the ?Help menu)

If you have already tried that, try this:

Go to Display Settings and use only shaded view

Use component color cycling view to temporarily shut off the wood textures. (this is on the Inspect menu - main toolbar)

Does that improve anything? If so, it's graphics.

Other things you can try:

1. Update your graphics drivers if they are out of date. Go straight to the manufacturer, don't trust windows tools for this.

2. Make the parts you aren't working on invisible.

3. Restart your computer if you don't usually do this.

I've also attached a white paper from one of my AU classes on working with larger assemblies. There are some tactics you may find useful.

Please let us know how it goes.

Regards,

[JulianGroeli]

Hi All,

I was also running into performance bottlenecks importing large models.

This approach doesn't work for every case, but it has really helped me. Thanks @schneik-adsk for post this:

https://forums.autodesk.com/t5/fusion-360-design-validate/pcb-import-from-altium-designer-18-step-is...

[Anonymous]

I'm working on a fairly complex model on a laptop with a great CAD spec (i7 and Nvidea Geforce), and when I first opened it, fusion went into not responding mode. I'm not sure how many components I have, but I wouln't expect it to be above 1000. Are there any circumstances where fusion doesn't use the built in graphics card?

[Anonymous]

Turning of the design history in my small 150+ assembly solved the problem for me.

[O.Tan]

This is exactly why I felt Fusion attempt to make timeline to record parts and assembly in a single timeline as a flawed concept cause what's the point of being so diligent with managing timeline only having to scrap it cause of issues downstream? My opinion still stands that Fusion should just separate this whole universal component (both as a part and assembly file) concept and go back to a more traditional part-assembly file system as I felt it's hindering progress in areas like modeling, drawings, assembly, and performance-related stuff (traditional CAD tend to show a lower quality assembly model to make the CAD "faster" and only load the detailed information if the part is "activated/edited in place", but with the way Fusion does thing, this isn't really possible as it requires everything to be loaded) 

[TrippyLighting]

I work with another CAD system where I can also without a problem, work in large assemblies in a single file including drawings. Some of the concepts are in fact so similar to Fusion 360 that I find it very easy to transition between the two. 

The single-file approach is not necessarily the root cause for Fusion 360 performance limitations. The performance area simply needs some attention 😉

[ed.waugh]

Has anyone seen any updates from Autodesk on this?

I'm having the same performance problems described in the message from 2016. Moving a PCB assembly even after removing all the < 2 mm sized parts is taking 1 min+. Seems like there is something broken in the way this is handled.

Also some of the advice is not very clear to me, why are rigid groups and the unavoidable capture positions bad but joints are good?

Thanks
Ed

[Phil.E]

Fusion is constantly under development, and performance improvements are in every release. 

Depending on the size of the assembly you are moving, it might take 1 minute. Since you are able to remove components, I'm guessing it's a step import from another PCB modeling application. This exact case was the subject of major improvements some time ago.

Can you share the design so I can analyze it? If there is a performance issue with it, I'm happy to log a bug report using it as the case file.

[ed.waugh]

Hi Phil,

Thanks for such a positive response. You're right about the origin of the files. The first is a PCBA from here:

https://docs.toradex.com/107996-verdin_imx8m_mini_v1.0_step_model.zip

There is also a solidworks format file available if you think that would work better? I was having trouble moving it so I modified it by deleting pretty much all the small components. I had to do it manually as if I used select by size and pressed delete all the parts disappeared but they remained in the components list on the LHS. Maybe you will find the same?

The second imported model is attached. Just a connector. I insert one of them and then make a pattern to put four in a row. Then copy one to a new position and make a pattern to put four in a row there as well. Total 8 instances.

In my view, even without the delete these parts represent a pretty small model. Would be interesting to hear your views and any luck you have with them. Also advice on how to avoid having to 'capture position' while drafting designs would be great (assuming that is a performance problem).

Thanks

Ed

[TrippyLighting]

@Phil.E @ed.waugh I experimented with this and I believe there might be a bug here in how the "select by size" function works in conjunction with the selection filter.

I had set my selection filter to Through and Components.

Then I used select by size with a range between 0-2mm. It selected 2k+ "objects" and my expectation would be that it selects what I set in the selection filter, so I should be able to delete 2000+M components. But it still only selects the bodies and deletes those, which still leaves a large component structure now void of most of the geometry.

As can be seen in the component count taken once before the selection/deletion and once after, I still have all the components, but have deleted 2,438 bodies. 

However, if I use a rigid group joint at the top level to tie al the components together, that joint still includes over   2,438 components, and as every component has an origin when the assembly is moved, a component even if no geometry is present still has an origin which will have to be moved.

 

[ed.waugh]

Thanks for trying it out. I found the same and ended up going through the components list and deleting them in big groups based on their names.

[Phil.E]

There is no surprise here. These items are extremely detailed renditions of these designs. As such they carry vast amounts of data in the form of faces, edges, component structure and so forth.

I try to use very simple versions of reference components to give myself as much computing power as possible while I'm designing. If it doesn't need to be in a drawing, BOM, or rendering, and it doesn't impact my design tasks in any way, it doesn't belong.

Thanks @TrippyLighting for looking into it. I think this has been logged before, if so I'll update it, if not I'll log it. Good catch. The tool only selects bodies, and by the looks of it is designed to pick components if you change the filter while the Select by Size command is active. 

I tried this trick and managed to make an insertable copy of the pcb that would drag freely as I moved it.

• Set selection priority to body
• Copy the bodies to the root component
• Delete the components

This produces a design that drags freely when you insert it as linked, and then move it. However because the bodies are now all individual instances, the file is twice the size. How's that for irony. But it does show that @TrippyLighting  is spot on about computing all those component origins as you move them. It has now 219 bodies after deleting anything less than 1mm. This still has >2k edges, which is not that bad considering the amount of detail.

The connector part is a little different, I'll test it some more, but it has one basic flaw. It too is extremely detailed. It has one body with 2367 edges. If you are using this for renderings it's a fantastic model. If not, and you plan to use it as a standard component, consider simplifying it before copying/inserting it into designs.

This is not the first time it's come up. The high school robotics students are given step models of the kits they buy, and in the past those have been found to have excessive detail. All that does is make it harder for the computers they are using.

[ed.waugh]

Hi Phil,

Thanks for taking a look at it. I agree about the level of detail but I don't want to spend lots of time modifying supplier models, I want to just drop them in and keep working.

Are the parts available from mcmaster-carr and through the insert manufacturer part option already optimised for use in Fusion?

Can you recommend a fast way to reduce the complexity of the parts without losing important detail? 

We didn't take Inventor because the new licencing scheme is just too expensive for us. Do you think we would have better performance with that? 

Thanks

Ed

[Phil.E]

I guess it depends on where you want to spend time. The process to remove the smaller components takes about a minute if you convert it all to bodies. Weigh that against all the edits that will be longer, as you work with this design.

McMaster parts, other than screws, are usually really light weight and low on detail. Some popular screws have been converted to have cosmetic threads, but I'm not sure that works with sat/step insert into Fusion. Those might be the other cad format's cosmetic threads. 

Here are some tips and tricks to deal with screw threads and embossed logos.

Removing 3D screw threads and replacing with cosmetic threads

Removing 3D logos embossed onto imported parts

[Phil.E]

Opening and using the detailed step file in Inventor:

• 1 min. 30 sec. to open and convert to reference model
• 2 min. to save
• Free move does not function with this model
• Free rotate does
• Constraining it to the origin plane was instantaneous

I'd say Inventor is struggling a little with it, probably for the same reason, all those component origins. It showed when selecting the assembly. But, Inventor has had longer to get optimized for larger assemblies, hence the instantaneous constraint transform I just saw. The model moved/rotated during the operation.

[JulianGroeli]

Excessive detail will bring even the best CAD system to its knees, be it Inventor, SolidWorks, Creo, etc.

PCB model exports almost always have more detail that you need. In large assemblies with lots of hardware, simplified models of screws and nuts (that don’t interfere with each other and don’t have helical threads) can help a lot, and also make interference checks a lot faster later on.

Time spent optimizing model performance is almost always worth it, even though it doesn't feel like it while you're doing it. How much time it's worth spending on this depends on the overall complexity of the project and how long you're going to work with these models.

In Fusion 360 you can use the Component.Counts text command (as @TrippyLighting as shown) to get an idea of how heavy your model is.

As @Phil.E  mentioned, it’s best to copy and paste all of the bodies to the root of the document and then delete the components.

To do this, set your selection filter to "Select Through" and check only "Bodies," drag a rectangle around the entire model, and hit Ctrl-C, Ctrl-V. 

Far too many components

Depending on how big your file is, and if you know up front what size feature you want to delete, it's faster to delete small bodies before the copy/paste operation so that fewer bodies are duplicated during that step.

Now your model is easier for Fusion to deal with, and everything is fixed in place. No need to calculate a rigid group.

For really large boards, I’ll sometimes make multiple copies of the file at different levels of detail so that I can work fast with lighter weight files most of the time, and then load the full models just when I need them.

See attached .f3d model of the iMX8 pcb with bodies under 0.65mm removed. This removes all of the solder balls under the BGA’s and the solder points on the rest of the chips and resistors.

The model has 518 bodies and should be pretty easy to work with, while retaining most of the detail. You can further simplify it using “Select by size" and deleting more bodies. Inserting it into another file is reasonably fast and you can drag it around and assemble it pretty easily.

No components, only bodies

[dvd.mlm]

Cross-posting for more visibility - Show us your slow assemblies!

Link to our feedback hub thread.

Thank you!
David Milam