CAD Forum

Our company upgraded from SW 2020 to 2021 SP5.1

For our large machInery assemblies I expected file size to increase to a certain extent due to detailIng mode.
What I am Investigating at the moment is some assembly drawing increasing at over 10 folds its size.

e.g.
one drawing went from 26MB to 200MB (down to 100MB after unchecking and checking again the tessallation data for the detailing mode)

another assembly drawing went from 7MB to 90+ MB taking a lot of tIme to save as well.

basically I found out what is written here:

https://www.cati.com/blog/2021/04/solid ... 2020-2021/

Our drawings are already unbearable, too slow and little support from our VAR or SW.

instead we got some new bugs, and this is another traIn wreck we are going to add to the collection.

After unchecking "Save model data" you will need to do a CTRL+Q rebuild of the drawing to get the file size back to closer to the original size. This should work on 2021 SP4.1 and later.

And another bug introduced to create a feature.

..or was it a feature created that introduced a bug? With so many, it's hard to keep track.

16MB to 200MB is kind of nuts....

Is the setting turn on by default from the installation?

Zhen-Wei Tee wrote: ↑Wed Mar 09, 2022 8:35 am 16MB to 200MB is kind of nuts....

Is the setting turn on by default from the installation?

I do believe this is enabled by default.

Not every file will have a drastic size increase. It will depend on how many and what kinds of views the drawing is using. The reason for the size increase is because all of the tessellated data has to be stored in the drawing for the various views of the model. You'll probably see the biggest size increases for drawings that use a lot of section views as it will have to create the tessellated data for each view instead of being able to share the same data as it would for normal views of the same model.

This seems to be "Detached Drawing" or "Rapiddraft" v2. We used to use those formats which was handled via "Save as" and changing the filetype. They store model data so the drawing can be opened and if the drawing had lots of "edges", it ballooned the file greatly. It's all about opening and doing some edits on large assembly drawings, tough problem to crack. Do you faster opening times and huge files which result in slower copying and checkout/check-ins? Or wait and go to the restroom, brew a pot of coffee, and make a sandwich while your assembly drawing opens?

Zhen-Wei Tee wrote: ↑Wed Mar 09, 2022 8:35 am 16MB to 200MB is kind of nuts....

Is the setting turn on by default from the installation?

I checked again and it was 26MB not 16, my bad, but the substance does not change so much unfortunatelly.

We had this setting turned ON since SW2020 and the file size was more or less affected but not at this level.
Obviously the more data are saved within the drawing the bigger it become.

Another issue I see is starting from SW2022 it is a document setting, while in SW2020/21 it is a general system option so we , as the CAD admin group, are going to lose control over what our engineers are doing out there. And the majority do not understand how to mess with SW settings and this is a point of concern.

It turns out to be

SPR 1208631

FIXED IN 2021 SP04

Customer impact Critical

Summary
Drawings - Detailing Mode Save, Close: Drawing files increase in size 10-15 times after they are saved in SOLIDWORKS 2021 due to the Detailing Mode Data

Technical Comments
Possible workaround is to deactivate "Include Detailing Mode Data when saving" option in Tools > Options > System Options > Drawings > Performance before saving legacy drawings in SOLIDWORKS 2021.

FIXED

@jcapriotti

Actually we have quite a mixed situation, like some unworkable 2D drawing. Most of the time the engineers just do no report the anomaly and they keep working with an unbearable slowness in Solidworks.

The idea behind detailing mode is not that bad, I have tryied it and I can actually work on some drawing that used to be very slow, but the moment you have to load it in fully resolved mode it turns in an unworkable state again, like 3-4 FPS for zooming and 3 seconds to select an single adge and other 3 seconds to get the dimension preview etc...

For some data could be worth, for some other you get very long save time with SW freezing for 5+ minutes.

I ran into this issue literally Thursday/Friday of last week. I was wondering initially if the issue had to do with in-context/circular references, as the assembly and drawing were saving into PDM but taking 10 minutes (consistently) to save. After some searching around, I came a similar article from Hawk Ridge and tried disabling that as well. File size of the drawing went from ~60 MB to ~12 MB.

Strangely enough, that drawing was last saved in Solidworks 2018 before I opened it in 2021, so I guess the size of the file ballooned on my first save? A curious issue that led me to work on other things that were getting pushed back continually due to design demands, so it was both a good-bad and a bad-bad thing to happen.

Detailing mode setting has been around since SW2020.
Updating from 2020 to 2021 takes even more space as the detailing data in the drawing file increased, but as usual some garbage from the older version is left in the fIle.

upgrading from 2018 is probably cleaner (at least until they start changing something in detailing mode again).

it is also geometry dependent. Assemblies of similar file size are going to take very different drawing space according to my tests.

We have some heavy assemblies that hang SW for minutes during save operation as you described.

I first noticed SW getting really slow in 2019. Others didn't see the slow down until later. I think this setting was a huge part of that, but I have no way to confirm that. I know I turned if off at some point in the last couple of years and it improved my speed quite a bit. (I'm still on 2020.)