Drawing slow, lot faster with parasolid imported data

SOLIDWORKS 2D Drawings
1

I understand that there are a lot of parameters and metadata inside the native files, but view generation alone is taking too much time.

I am working on performance, to improve our workflows and to fix problematic data. Here is what I found. I made some tools with API to analyze drawings and apply settings in batches to all views, but there is something I do not understand yet.

An enclosure made with sheetmetals panels (not sheet metal features, only extrusions, cuts, holes, patterns, splits)

the first time I opened the mutibody model it rebuilt in 9 seconds. Now I make it rebuild in 3.5 seconds with the same amount of geometry and the same amount of features tweaking the way it was modeled.
(I am writing a separate post on the matter)

Nevertheless its 2d drawing is slow and SW hangs a lot.
E.g. If I try to hide some body (to clean up a view background) in the view property and I press apply it takes MINUTES to update with SW not responding.

There are a lot of holes, i tried to disable the annotation visuals and put the threads in draft quality.
no luck

I disabled di overlappIng edges high quality setting in the drawing document properties.
no luck

I exported the 3D data as parasolid, reimported in SW and I used the same 2D drawing relinked to the new 3D.
result: as expected the dimensions blown up, but the view generation and body hiding is an order of magnitude FASTER.

I suspected hole wizard as a culprit, and I am replacing the holes with cuts, but it does not seem to be the only cause.
my intuition is that SW is bringing a lot of overhead inside the drawing views, overhead not present with a dummy solid exported from the very same geometry that caused a slow drawing.

This overhead is apparently affecting view generation for whatever reason.
I want to understand that reason.
The amount of edges, view styles etc for native SW data based drawing and imported parasolid model are exactly the same.

Alin any idea you could share?

I cannot share data without an NDA.

2

Check the performance evaluation of the model and see which features are taking more time.

When you use imported body, all the history is gone and there are no features to rebuild. This makes the model/drawing faster.

3

I already did that and the slowest features take 0.15 seconds.
When I first opened it there where features in the order of 0.6 or even 2 seconds: i fixed them and the whole model rebuilds in 3.5 seconds down from 9seconds it was at the beginning
On average it is less than 0.015seconds per feature.
The rebuild is smooth and without aparent freezing.
I can try to improve further, but I need to remodel it with a different approach.
However I think it is impossible to get closer to the parasolid data as it rebuild in 0.03s

I have fixed a grill with hundreds of cuts in the same way and the drawing was noticeable faster, and the grill went from 13 to 2 seconds rebuild time. This model’s drawing slowness is not getting any better…

What is bugging me is what makes our drawings so heavy.
is it the feature reference database inside the model?
and if so why it is needed to generate a 2d drawing view?

4

Try freezing the features if that helps.

5

Did you un-select Detailing mode?
image.png

6

yes detailing mode is disabled.
it brought us more assle than good.
for 2022 is now in the templates as they moved it in document properties.

7

I could try, but we disabled the freeze bar years ago as I have been said it caused a lot of troubles in PDM. For my personal experience I had part corruption and instability with that bar enabled so I avoided it. but it was yars ago.

8

You can make a copy of the part and try with that.

Other thing to try is do a save as with a different name and then save as again with the original name. This might help. But make sure to keep a backup.

9

No luck with the freeze bar as well.

10

Do you have high quality or draft quality views in the original drawing?

11

Adding to what Alin said, do you have sections in your drawing? If so, do those section show surfacic bodies? Because for some reason, the setting in sections to show surfacic bodies slows everything down, even if you don’t have surfacic bodies.

Also, check to see if you have empty view shells laying around in your drawing
image.png
To view them, go to view>Hide/Show>Hidden views

12

Alin AlexLachance

I have written a macro to analyse all drawings view and output their properties in text format to check mainly:
・ the view quality (draft high quality)
・threads quality in the view (draft or high quality)
・surface show/hide status (for sections and detail views iirc)
・hatching status for faces in the view

with the same macro I can turn off or on them in batches. This drawing has all the views forced to High quality, the threads to draft (I even disable them from annotation view settings), and surface are hidden.

I re-installed a minimum SW from tje original files, instead of our admin image, left the settings to default and used the default templates and sheet format SW generates, and draw the same views: when I change the property of the front view to hide the background bodies 1 core of the cpu is maxed for 1-2 minutes, if view automati update this continue for 4-5 minutes.

4.5+ GHz xeon quad core, 32GB RAM, SSD, Quadro RTX A2000 12GB.
20 yrs ago I used to model die casted parts with unigraphics and a 32bit workstation with 2GB RAM. their drawings compared to this one were absolutely nuts. free form surfacing vs flat panels!

13

btw my VAR has still to come back to me after 3 days since I show them the comparative video of native vs parasolid, only to upload our files…
I made some complaint on the pLafOrM and it seems a dev from the drafting definition team could pick up the issue, but I need a SR number from my VAR…

My main question: why parasolid data is so light? same views same lines same section, the very same slddrw with swapped 3d data…

14

lol welcome to the circular reference world of troubleshooting with VAR’s and Dassault. Nobody seems to know their role.


parasolid data is featureless. It is information stocked within a feature from my understanding. In the case of parts or assemblies, we have multiple features and display states and sublevel of assemblies and whatnot so SolidWorks tends to get confused with everything after a while. I think the most noticeable example is display states, it’s not hard to get SolidWorks confused.

15

Everything.
Whatever you can’t see in the view is still there. Every update require recalculate what’s is visible and what’s not.

16

Frederick_Law the same 3D data exported in parasolid and relinked to the SAME drawing file is a order of magnitude faster and the same operation on the SAME VIEW with the SAME geometry takes seconds instead of minutes.
same edges same settings

17

I get that parasolid data is featureless, but the point of drawings is display edges and dimensions.
I can understand that calculatea section that does not exist in 3d needs to create a ad hoc configuration and the calculation takes time. what I struggle to understand is why a projection of edges and hiding edges that are already there is taking a whole cpu core for minutes. like SW is querying a huge database of features id, edges id or whatever else to do a useless job nobody asked for.

it would be nice to know from the technical point of view what is takIng so long to calculate. Reading the KB I understand that SW devs have a tool to open the drawings and see all the elements stored inside the files including garbage and other funny thIngs. it is a sort of viewer, I do not remember its name atm.

18

Btw I found the reference to the tool the technical support is supposed to use to open drawings..

Corrupted Drawing makes SOLIWORKS to crash
Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: Drawings
OS: Windows 11
Detected level(s): SOLIDWORKS 2023 SP4
DESCRIPTION
Corrupted Drawing makes SOLIWORKS to crash I tried to repair with
SldFileViewer > but no luck
CLOSURE INFORMATION
File is already repaired by R&D

Does someone know what SldFileViewer is?

19

I got back from my VAR.
They tested our file with SW2022 and it took them almost 5 minutes to generate a view and hide a body inside that.
They opened the same file with SW2023 and it took 1 minute including file opening and drawing editing. A few seconds to hide the bodies as expected.

So for this file problem was just solidworks 2022 SP5 to be BROKEN?

20

Impossible. SP5 is supposed to be the most stable.