Onshape keeps stalling and crashing

tony_459

I love Onshape but it keeps stalling and crashing. I spend far more time staring at a spinning circle telling me that things are still loading than I spend doing actual work. This happens at home, sure, where Comcast has thought it reasonable to allow download speeds to drop to under 10 mbps overnight despite my being on a 100 mbps plan... but it happens also in the office, where internet speeds are reliably in excess of 300 mbps.

Am I the only one struggling to be productive in creating models? I always wind up spending inordinate amounts of time just waiting for things to load. I can usually click a button to open a tool, change to a different tab to skim the news, and change back to Onshape only to wait still a little longer for the thing to fully load. Very difficult to finish a model like this. A full day of work today---I could have most definitely finished in an hour in a desktop CAD tool. It's very, very, very slow.

tony_459

How slow it gets: Even panning and rotating and zooming takes several seconds to register

NeilCooke

Well clearly that is not right. What browser and operating system are you using? Is everything (browser, OS, graphics driver) up to date? Is it a specific document or all documents? What does cad.onshape.com/check say? Thanks. 

tony_459

Windows and Mac; Firefox, Chrome, Opera, IE, and Safari---depending on the machine I'm on. I regularly update my browsers and have no issues using other 3D modeling software. Onshape checks look good, with only a suggestion to use a dedicated GPU for best performance. 

My home internet speed doesn't help, but I have the exact same performance issues on my work machine, which has very reliable and very fast download speeds. 

MBartlett21

Panning rotating and zooming are all done on the client side, meaning that it would probably be your gpu that is going slow (or the browser's renderer if you don't have a gpu or your settings are wrong)

Jake_Rosenfeld

@tony_soares459

Does your laptop have a dedicated GPU?  If so, your performance will improve greatly if you make sure it is being used.  Instructions for doing so are here:
https://cad.onshape.com/help/Content/webgl.htm

Sometimes Operating Systems or Browsers will try to use the integrated graphics (graphics on your CPU rather than graphics on your GPU) to save battery when using a browser, because they assume that no web site would be doing anything mission critical or graphically intensive in a browser.  Oh how wrong they are

tony_459

Thank you all for pitching in! It's always a relief to see folks who know the software in and out try to help us out  

I have yet to check my home laptop but on my work computer... I have a dedicated graphics card (NVIDIA Quadro a few years old, not top of the line, but still). I checked (with help from Tim, who must have the patience of a saint) that Firefox is using the GPU. We also turned on performance acceleration to the max setting. I do have a firewall on that computer though it's set so that all websites are allowed unless I specifically block them (which I have not done with Onshape ).

Sadly, performance is still a miss. Tonight, I found myself waiting upward of two minutes waiting for a simple change to a sketch to register (a coincident constraint, I think?) Things were excrutiatingly slow. At one point, the browser crashed and I had to start over.

I checked my internet speed and ping time was 2 ms (I should only be so lucky on my home network) and download speed was upward of 350 mbps. All I can say is that performance was very much on par with what I get at home (with internet speeds well under 10 mbps at times, I guess Comcast's interpretation of 100 mbps speed), so the issue must be somewhere else. 

The model has grown quite a bit and I remember running into speed issues while modeling another similar model a couple of years ago (of a tank truck which had many patterns in a single part studio). This model is of a roller coaster track, and it too has quite a few patterns and part copies (for things like columns and connection plates). No doubt this will impact performance, but would it fully account for the persistent sluggishness and occasional web browser crash?

I love Onshape and very much want to keep using it but I am always short on time and would love to find myself creating these models at a faster clip. I put so much time into them

owen_sparks

Is the model public?  A few of us could open it and compare notes?

O.S.

NeilCooke

@tony_soares459 how many features in each Part Studio? You should always try to keep them to a manageable size, say under 100 features in each, and use assemblies where there are a lot of copied parts and patterns. A good watch is @philip_thomas's webinar on fine-tuning performance: https://www.onshape.com/videos/tips-and-tricks-to-turbocharge-onshape-performance-and-speed-110618

john_rousseau

Hi @tony_soares459. I'm running some server-side performance traces on your document now.

Looking at your basic system metrics, I'm seeing the most common GPU your client is using is "Intel(R) HD Graphics Family". I'm only occasionally seeing your Quadro GPU. I'm also seeing low FPS and high, inconsistent latency which really makes me think you are using your integrated GPU.

I'll let you know what the server side traces show after a day or so of you using that document, but I think the GPU is the problem here.

tony_459

Hi all,

Thanks again for pitching in! @owen_sparks, you can find the model here:

https://cad.onshape.com/documents/7a718b6d8bf3b9c0547e6d8c/w/c80e2acd2d7ab0fa4ec09ecf/e/49d9646d7e3a9d6fa9128f53

@NeilCooke, I am sadly over 100 features. I need to keep the parts few in number for export at the end (keeping, for example, all the columns in one part, the whole of the track in one part, the tower and everything of its color in one part...). It would make sense to split at least these few parts into different tabs, though I have so little information about the exact part geometries and dimensions that I felt more comfortable modeling them together in one place—to make sure they all fit well and hopefully avoid unpleasant surprises at the end. I'll be rethinking this approach once I'm finished. Thanks for the link!

@john_rousseau, thanks for going the length of running actual tests on my document! I hope it wasn't too much of a hassle (I know you guys are busy and it wasn't my intent to tie up your resources). I'm working mostly on my personal laptop at home (which is itself a replacement for my macbook, which died a month ago). I'll have to double-check my graphics card there. In my work computer, the one I use only sporadically, I have the Quadro k620—an older graphics card, but hopefully still better than an integrated card. I just went through the steps that Tim sent me to ensure that my browser uses the Quadro (which I now see was not necessarily happening before today). I'll let you know how things change—although you might be able to see that in the performance data itself.

Thanks again, everybody. I can't remember getting help of this kind for any software (or for any other tool, now that I think of it)

tony_459

Sadly, the performance issues remain. I checked that my web browser (Firefox) is set to use my dedicated graphics card and configured settings to prioritize performance. I also configured the browser to allow hardware acceleration and set the acceleration to the maximum setting. The delay in Onshape persists and it is as severe as before. Minutes pass from the time I click to create a sketch to the time when the spinning circle disappears and the sketch tools are all responsive

lana

The curve pattern is a culprit in this part studio.

I'd second Neil's advice on rethinking the structure of this project. If you built layout curve structure in a separate part studio and derived it into other part studios you should be able to build all pieces in separate part studios.
If you are not ready to do the refactoring yet, suppress the pattern for while you are working with this part studio or, at least change it to "New" - merge probably takes significant time

john_rousseau

I'll second Lana's (and third Neil's?) advice. The performance traces confirm that you are seeing frequent, long regeneration times due to the structure of the project.

Cris_Bowers

My advice is to not treat the part studio as an assembly or weldment. It's easy to get trapped into that mindset because that's how Onshape was marketed to us. Just because you can, doesn't mean you should. I would break it down into lots of part studios and create an assembly to put it all together. You don't need to create identical components in the part studio, those can be placed and patterned in the assembly. Remember that you can use and mate to sketches in the assembly as well. I think that would help in this case.

Prachi

I have found a couple of things that will slow document down a lot.
1- I see a a lot of mate connectors in display above.
These tend to be extremely slow to display. Recommend hiding as much as possible.
2- Tim from support helped me find the next problem a couple days ago.
I had for expediency 'grouped parts in an asssy' while grouping its self is not a problem I had included a linear array which is redundant. This can cause something called recursive. Doesn't know when to stop calculating. Eliminating array from group solved the problem and document became very responsive again.

Just some things to think about when document gets slow.

billy2

I do most my instancing in an assembly to save speed. I'll have one part in the part studio then replicate in the assembly. I guess we need pattern by curve in the assembly next. You could pattern holes in the part studio and then use replicate in the assembly which works extremely well.

There is a Philipism: If a part isn't related to another part, put it in it's own partstudio. 

There are reasons why we have part studios & assemblies. I tend to use them both all the time even for the simplest of things. I'm double clicking parts in the assembly to ghost everything when working in a partstudio. Most of the time I refrain from incontext to preserve the double click ghosting pattern. Once an incontext is formed, updating the context has to happen which is slower and not as fluid when designing. 

I like designing in the assembly because I'm a "top down" type guy.