Sloth-slow performance

don_williams909

I work for a Pro-Audio speaker manufacturer here in Massachusetts.  One of the things I use Onshape for is designing metal grilles for the front of speakers. 
These grills have lots and lots of perforations.  I am encountering enormous slow-downs when making these, and am wondering if there is any movement toward increasing the speed for regenerating all these features.
When using Creo, there was a way to make a grille and then create some sort of cloned version which didn't have all the operating math happening in the background.  It was a dummy part of sorts, but visually it was identical.  Any chance that Onshape can borrow that ability from PTC?

Thanks...

NeilCooke

Hi @don_williams909 I don't suppose you can share an example? If not publicly, please share with support (and mention me, if you like) so we can take a look. I don't recall any such thing in Creo, but at least I can now ask somebody who will know.

Jason_S

Hi @don_williams909 , 

How real do you need the speaker mesh and what is its CAD purpose? Is it only for drawings or rendering? I have an idea if you can create a ticket and send support an example.

john_mcclary

you can do that with configurations, add a config that suppresses the perforations and patterned features.

Colle

Hello, 

Jumping on this as well, I have be experiencing the same issue and am looking for a solution. Its not limited to grills, I experience very long redraws any time I apply one operation to many features of the same part or when one operation adds many features to that part, applying one Fillet to 100 edges for example.

You can easily demonstrate the issue; just extrude a rectangle 100x200mm 2mm thick, then sketch a couple smaller rectangles in one of the corners and extrude them to make two small holes, then using a Linear Feature Pattern first down then across to make a grill pattern and even at only an array 16x24 it will take seconds to redraw.. adding more complexity say Fillet to round the corner of each hole it will slow down even further and if you are adding the pattern to an already complex part.. well you get the idea. (see link, and yes i'm aware that there is a marginal gain to be had by adding the Fillet before the Feature is created)

https://cad.onshape.com/documents/5d05d2cd1a5a0f503f3d3854/w/d2cf7719560b3f7e709c4f90/e/dfb239eaf5a680eaad406a50

I've also experienced it on more complex Feature Studio's but this can usually be solved by splitting the needed parts over more Studio's but some times that's not an option, I have a single Feature Studio that only has a handful of parts but with over 20k faces and 1 Million Triangles. Making changes even towards the bottom of the Features list can have very slow redraws. I wonder if its a model cache issue as i notice the longer i spend in a drawing and the more edits i make the redraws seem to get longer, if i simply restart the browser it doesn't have any effect but if i leave it for a few hours and come back to it the redraw times will seemed to have dropped. is there a cleanup that runs server side, or is it the act of reloading the project on the server that could be having this effect.

I look forward to your thoughts.

tim_hess427

@don_williams909 @NeilCooke

Are you perhaps thinking about Simplified Representations in Creo? I remember using that when dealing with large assemblies. 

http://support.ptc.com/help/creo/creo_optm/usascii/index.html#page/optm%2Foptions_modeler%2Fasm_two_sub%2FAbout_Simplified_Representations.html%23

Maybe there's some workflow with derived parts/versions/in-context part studios that would produce a similar performance benefit when working with multiple parts? 

alnis

One thing to note is that face patterns regenerate much faster than feature patterns. For example, in @colle 's case, I was able to bring the regeneration time from ~40 seconds down to ~13 seconds by replacing the 3 linear feature patterns with a single face pattern. Here is my copy. I have had cases where a face pattern (instead of a feature pattern) reduces regeneration times to as little as 10%-20% of the previous time.

Cary_Bettenhausen

GREAT JOB ONSHAPE!

We are seeing significant performance improvements in heavily perforated sheet metal parts after this bugfix:

• Onshape SupportMonday at 11:20

  Hi Cary,

  Onshape has been updated to address your ticket:

  "Slow performance with Sheet metal cuts"

  This update (1.174.27783.ab3907bf6199) has been pushed to cad.onshape.com and is live for all users of Onshape. This version is displayed at the bottom of the Documents page or by clicking the ? menu and selecting About.

  NOTE:
  Some features will require redefinition or recreation to reflect the improvements made to Onshape. Please take the time to verify this update has resolved your reported issue. Please check https://forum.onshape.com for more details about this update.

  Thank you for making Onshape awesome!

• 
  jmoellersNovember 03, 2023 12:22

  Hi Cary,
   
  This is a bug in our current sheet metal functionality. I've added you to the bug ticket for this. 
   
  In the meantime, we recommend modeling the part in solid and then using sheet metal to convert the solid part to sheet metal. Alternatively, you could do something similar with surfaces and then thicken the surfaces to create the desired sheet metal model.
   
  Your support ticket:
   
  "Slow performance with Sheet metal cuts"
   
  has been identified as a bug and we are working on it. As soon as this gets addressed and is pushed to cad.onshape.com, we will update this ticket to so you can confirm the update.
  

  John Moellers
  PD | UX | Support | Community
  Onshape, Inc.

glen_dewsbury

Face pattern for the array will make a noticeable speed difference. Only one array needed. Third array is a duplicate in start version. Don't add fillets later(another performance hit).

https://cad.onshape.com/documents/68d7c96149a9cc517f300c53/w/3f4390015c843665d026d6fd/e/4554f737399013c26f66f1a0