SOLIDWORKS 2023 confirmed bugs

[mp3-250]

I am testing sw 2023 sp5 before installing it in our company.

I felt it was a release with a fewer bugs, but reading here and there about some annoyances I felt i need a place to list all the bugs I need to test against our workflows.
I am going to post 1 reply for every bug i encountered and the KB references I am aware of.
every other contribution is welcome!

LIST for future update here.

[mp3-250]

SPR1218372: Add an option to hide configuration table under System Options/ FeatureManager/ Tables.

regression from 2022. it was possible to avoid the configuration table automatic creation when a configuration was added to the model.

[AlexLachance]

SolidWorks 2023 SP5
Regression from SolidWorks 2023 SP4

Items with different file names that callout same item number combine and merge themselves into one item in the BOM, in SP5 they combine themselves but one of the item is not balloonable.

When the items are named differently and the configuration calls out the item number, the BOM comes up correctly but we are unable to balloon the culprit items. The balloons come out with an * rather then the item number they should call-out.

The work-around is to revert back to SP4.

It is still being analyzed. Will update when assigned an SPR.

[mp3-250]

***FIXED IN SW2024 SP2***


BR10000370892

Abstract : "Refresh cache during log in" fails to trigger on initial vault view login (after reboot) when login prompt is suppressed via "DisableAutoLoginPrompt" registry option

login from explorer with RMB does not trigger the local cache refresh.
login from pdm client icon (edmserver.exe) does trigger the refresh cache as expected.

[mp3-250]

happened in 2022 and still present in 2023

BR10000369019 - 'Add-in loading performance….' warning message cannot stay hidden if turn off 'Remind me when a document has not been saved for' option in System Options.

I had users that disabled the pdm add-in by mistake due to the popup (which is completely unwanted and pops up in a absolutely negligible scenario)

[doobes]

One that I've run into a couple of times is doing an sketch extrude mid-plane, or extrude all both sides, only does one side as shown in the preview, and if you accept the solution the extrude is only one side.

If you change to a one directional extrude and then go back to the double ended extrude, it functions properly.

Kinda hinky.

SP3 definitely didn't do this.

[mp3-250]

***WORKED AROUND FORCING THE LAST LOADED PATH FOR EACH TABLE IN THE REGISTRY***

BR Default template (BOM, Cut List, Revision table) is not being recalled

Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: Structure Systems-Weldments
OS: Windows 10 64 bits
Detected level(s): SOLIDWORKS 2023 SP1

DESCRIPTION
Create a folder name "Cutlist Templates" under c:\temp
Tools->Options->File Locations->Weldment Cut List Templates and point the folder directory created in step 1. Ok
Open a drawing
Insert, Table, Cut List. Notice the default cut list template is not pointing to the assigned folder

CLOSURE INFORMATION
This issue is reported to Dassault Systèmes development team.

It seem present in SP5 as well

[mp3-250]

I thought it was supposed to be a new enhancement available from 2023...but the what is new mentions tranparent "bodies" not "components"

Assembly components are not displayed as transparent with See through transparent components in HLR/HLV enabled in HLR drawing view
Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: Drawings
OS: Windows 10 64 bits
Detected level(s): SOLIDWORKS 2023 SP3
Description

Assembly components are not displayed as transparent with See through
transparent components in HLR/HLV enabled in HLR drawing view

Closure Information

This issue is reported to Dassault Systèmes development team.

https://help.solidworks.com/2023/englis ... 98396a#Pg0

[mp3-250]

Another drawing related issue introduced with the new transparency option for views

BR Article: BR10000354471
Status: Opening transparency related problem (again: this was supposed to be a new enhancement in 2023!)

BR Drawing Template saved with option 'See through transparent components in HLR/HLV' disabled , doesnt remember the settings when used.
Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: Systems
OS: Windows 10 64 bits
Detected level(s): SOLIDWORKS 2023 SP2
Description

Steps to reproduce this issue : 1. Open a new drawing document in SW 2023.
2. Click Tools > Options > Document Properties > Detailing a. Disable ' See
through transparent components in HLR/HLV '> Ok 3. Save this file as a new
drawing template. 4. Create a new drawing using the template saved in 'step
3' 5. Observed that the option ' See through transparent components in
HLR/HLV ' is enabled again.

Closure Information

This issue is reported to Dassault Systèmes development team.

Drawing templates do not save the new transparency setting or the new settings is not recognized by SW in document properties and new views are created with the transparent flag on and shown transparent in their 2D views.

[mp3-250]

STILL OPEN FROM SW2022SP5 REPRODUCED ON 2023SP5 AS WELL

workaround unbreak, remake balloons break again, but if you move the balloons they show an asterisk again.

BR Auto Balloon Balloons on a detail view disappear after the creation of a Broken Out Section View
Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: Drawings
OS: Windows 10 64 bits
Detected level(s): SOLIDWORKS 2022 SP5
DESCRIPTION
Within a SOLIDWORKS drawing the balloons on a detail view may disappear
when you create a Broken Out Section view to one of the parent views.
CLOSURE INFORMATION
This issue is reported to Dassault Systèmes development team.

Also balloon and detail view related

Balloons on the Detail view made from Section view disappear or become dangling if there is a Broken-out Section (BOS) on that Section view
Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: Drawings
OS: Windows 10 64 bits
Detected level(s): SOLIDWORKS 2023 SP0
Description

1. Open attached drawing 2. Annotations > Balloon 3. Attempt to place
Balloon on Detail View J on any edge 4. Notice Balloon disappears Problem
not reproducible if Broken Out Section view is deleted Same as SPR 1150111

Closure Information

This issue is reported to Dassault Systèmes development team.

[AlexLachance]

STILL OPEN FROM SW2022SP5 REPRODUCED ON 2023SP5 AS WELL

you can "unbreak" the view and see if the balloons are hidden within it and if so move them out of the break. Doubt that's the case but figured I'd point it out in case.

[mp3-250]

SW CRASH ON EDITING EXCEL DESIGN TABLES *HOTFIX AVAILABLE*
REPRODUCED ON EMPTY PART AND ASSY FILES WITH 2023 SP5

Design Table - Editing Design Table may cause SOLIDWORKS crash.
Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: Assemblies
OS: Windows 10 64 bits
Detected level(s): SOLIDWORKS 2023 SP4
Description

• Environment:
Tested and reproduced: SW2023SP3, SW2023SP4
Not reproducible: SW2022SP5, SW2023SP2.1

• Scenario1: (from scratch)
1. Create a new part.
2. Create a sketch and insert some sketch entities and smart dimensions.
3. RMB on Annotations > Show Feature Dimensions.
4. Insert > Tables > Excel Design Table
5. Double click on the dimensions to add them into Design Table.

• Scenario2: (existing files)
1. Open an existing file with a design table.
2. Edit the design table.

• Actual Result:
SOLIDWORKS crashes.

• Expected Result:
SOLIDWORKS should not crash during editing Design Table.

• Workarounds:
Not found.

Closure Information

This issue is non-reproducible in SOLIDWORKS Desktop 2024 SP0.1.
A HotFix for SOLIDWORKS Desktop 2023 SP5 are implemented.
Please refer to QA00000307226 for further instructions and how to get the HotFix.

[RonE]

Another drawing related issue introduced with the new transparency option for views

BR Article: BR10000354471
Status: Opening transparency related problem (again: this was supposed to be a new enhancement in 2023!)




Drawing templates do not save the new transparency setting or the new settings is not recognized by SW in document properties and new views are created with the transparent flag on and shown transparent in their 2D views.

There is a hotfix available for 2023 SP5 since a few days: BR10000354471 -> HF-1114811

[mp3-250]

There is a hotfix available for 2023 SP5 since a few days: BR10000354471 -> HF-1114811

I was sent it from mt VAR few days ago and testing it right now. once completed I will update the post.
thank you for the remainder!

[SolidKeke]

We just updated from sw22sp5 to sw23sp5 and faced first annoying issue:

If drawing view has tangent edges hidden, it's impossible to dimension structural members. When you switch to tangent edges with font, you can dimension. Anyone else has this same behaviour?

EDIT:
Found fix SPR1254289
"workaround: In SW2022, it works if Options > Selection > Selection of hidden edges > ‘Allow selection in HLR and shaded mode’ option is selected"

[Hansjoerg]

BR10000367139: Insert > Part > Break link to original part - the Part Material of the child part replaces the that stored in the parent
The 2023 SP5 hotfix to address this issue is available in the attachment HotFix_HF-1210441_2023sp05.exe

[Hansjoerg]

And the next one.

If you place the "View from behind" command on the mouse gestures and select this command, the current view is adopted as the default view rather than being rotated to the view from behind.
The behavior is reproducible in 2024.

I am trying to reprogram the command with a small macro and then place this macro on the mouse gesture. I'll report back if it works.

Solution:
The problem only occurs if you insert the command again from the command selection on a mouse gesture.
If, for example, you take the existing command from the 8-fold mouse gesture and move it to a position on the 4-fold mouse gesture, the command works as expected.

[mp3-250]

We just updated from sw22sp5 to sw23sp5 and faced first annoying issue:

If drawing view has tangent edges hidden, it's impossible to dimension structural members. When you switch to tangent edges with font, you can dimension. Anyone else has this same behaviour?

image.png


EDIT:
Found fix SPR1254289
"workaround: In SW2022, it works if Options > Selection > Selection of hidden edges > ‘Allow selection in HLR and shaded mode’ option is selected"

I saw this bug too, but limited to some model based on a verycold template. edges were not selectable, but switching from no tangent edges to tangent edges visualized solved the poblem. you can switch the viee back once dimensioned.

[martin]

Exported STEP files may be invalid due to Windows region settings

Steps to reproduce:

1. Open Windows region settings
2. Set Format to English (United States)
3. Open Additional settings...
4. Under the Number tab set a new value for the Decimal symbol, like comma "," or some other character (Windows allows up to three, but only the first one will be used) and click apply
5. Open a model in SOLIDWORKS and save as STEP (AP203 or AP214)
6. Inspect the STEP file with a text editor

Incorrectly formatted STEP file (decimal symbol set to comma):

Code: Select all

#1 = DIRECTION ( 'NONE',  ( 0,000000000000000000, 0,000000000000000000, 1,000000000000000000 ) ) ;

Correctly formatted STEP file:

Code: Select all

#1 = DIRECTION ( 'NONE',  ( 0.000000000000000000, 0.000000000000000000, 1.000000000000000000 ) ) ;

Successfully reproduced using SOLIDWORKS 2023 SP5 on Windows 10 and 11.

If any other format is used, such as English (United Kingdom), it seems like the decimal symbol setting is ignored and the dot "." will be used. So this is most likely to occur for those who prefer English (United States) as the OS language, but have customized it to follow local number formats.

BR10000347928 mentions this issue, but doesn't include much details.

[mattpeneguy]

Need to make sure the STEP file is also in the proper NTSC format instead of PAL...

[IndianaDave]

Love that we can open a drawing from the BOM on the sheet now...
Unfortunately, I can't right click and open the drawing of a part in the drawing view. It seems to be broken.

[AlexLachance]

Love that we can open a drawing from the BOM on the sheet now...
Unfortunately, I can't right click and open the drawing of a part in the drawing view. It seems to be broken.

Odd, it seems to work for me...?

[IndianaDave]

Odd, it seems to work for me...?

image.png

Unfortunately, when I click on the "open drawing" nothing happens.
Have tried on multiple files.

[AlexLachance]

Unfortunately, when I click on the "open drawing" nothing happens.
Have tried on multiple files.
image.png

I recall this happening in the first SP of 2023 or 2022, what SP are you running...?

[SPerman]

It doesn't work for me either. My 2 thoughts:

PDM is causing the problem. (I'm pretty sure Alex isn't on PDM, and we are.)

All parts / assemblies / drawings have to live in the same folder. (We do not follow this convention. Parts and assemblies are in different folders.)

[AlexLachance]

It doesn't work for me either. My 2 thoughts:

PDM is causing the problem. (I'm pretty sure Alex isn't on PDM, and we are.)

All parts / assemblies / drawings have to live in the same folder. (We do not follow this convention. Parts and assemblies are in different folders.)

That could be the cause, the issue I refered to related to documents not being in the same folder if I recall correctly.

I don't use PDM and our drawings are in the same folders as their parts/assemblies.

[mp3-250]

That could be the cause, the issue I refered to related to documents not being in the same folder if I recall correctly.

I don't use PDM and our drawings are in the same folders as their parts/assemblies.

There is user a setting that allow PDM to search the whole vault for a drawing.
The only problem we had with opening drawings was the "bug" that shown more than one drawing file, from a old version.
When the file was derived from another 3D+DRW couple with a "save as" and later renamed, so you have a old version of the drawing that termporary referenced the wrong 3D or someting like that.
This is why I recomend to use tree copy even for a single file instead of copy-paste or save as.

[IndianaDave]

I recall this happening in the first SP of 2023 or 2022, what SP are you running...?

SW23 SP5.0

[IndianaDave]

There is user a setting that allow PDM to search the whole vault for a drawing.
The only problem we had with opening drawings was the "bug" that shown more than one drawing file, from a old version.
When the file was derived from another 3D+DRW couple with a "save as" and later renamed, so you have a old version of the drawing that termporary referenced the wrong 3D or someting like that.
This is why I recomend to use tree copy even for a single file instead of copy-paste or save as.

I can not find that setting...
Unfortunately, these drawings are in the same folders as their respective parts.

[bnemec]

Probably a dumb question, but can you confirm that the part.slddrw that you are trying to open from an assembly.slddrw is in local cache?

In several ways, we've had issue like this where SW (completely unaware of PDM managing the local cache) cannot access a file because it's not in local cache. I would expect it to show the "file does not exist" error, but maybe the SW people didn't bother checking for that and just swallow the exception as they assumed the user always has access to the entire dataset. I'm guessing the SW people don't give a comprehensive list of changes to the PDM people so the PDM add-in can be updated by adding event handlers to these user inputs so PDM has a chance to cache the needed file before SW tries to load it. It's probably much more complicated than that, but it makes sense in my laymind.

[mp3-250]

Probably a dumb question, but can you confirm that the part.slddrw that you are trying to open from an assembly.slddrw is in local cache?

In several ways, we've had issue like this where SW (completely unaware of PDM managing the local cache) cannot access a file because it's not in local cache. I would expect it to show the "file does not exist" error, but maybe the SW people didn't bother checking for that and just swallow the exception as they assumed the user always has access to the entire dataset. I'm guessing the SW people don't give a comprehensive list of changes to the PDM people so the PDM add-in can be updated by adding event handlers to these user inputs so PDM has a chance to cache the needed file before SW tries to load it. It's probably much more complicated than that, but it makes sense in my laymind.

Are you on 2023?
I kind of saw this situation a couple of times, but I was not able to reproduce it.
I remember I was opening the file from the most recent used list, but I think it was after cleaning up a vault view on that workstation.

[mp3-250]

I can not find that setting...
Unfortunately, these drawings are in the same folders as their respective parts.

Right-click a user or group and select Settings.

Look for drawings in the entire vault (instead of only the same folder).

https://help.solidworks.com/2021/Englis ... ECK_IN.htm

[bnemec]

Are you on 2023?
I kind of saw this situation a couple of times, but I was not able to reproduce it.
I remember I was opening the file from the most recent used list, but I think it was after cleaning up a vault view on that workstation.

Still on 2019, in process of updating to 2023.

Only way I know to confirm is from Search tool or Vault view and check the version column, that tells me the cached version. I'm trying to reproduce it myself right now, but I cannot get PDM to clear the local cache of a file I pick in the recent file list. Even with SW and other vault views closed. I think the preview tab in vault view will cache files, maybe the recent list does to, sometimes.

[SPerman]

I first discovered/reported this in 2022, but it remains unfixed in 2023.

SPR 524858

I am a GIF, Click me.

[AlexLachance]

I first discovered/reported this in 2022, but it remains unfixed in 2023.

SPR 524858

image.png



I am a GIF, Click me.

ordinate.gif

Do you have a direct link for me to vote on..?

[SPerman]

I'm not sure about voting. I am not swamp literate. (I avoid that place like the plague.)

I tried to paste a direct link to the SPR, but it only provides a link to the knowledge base.

[AlexLachance]

I'm not sure about voting. I am not swamp literate. (I avoid that place like the plague.)

I tried to paste a direct link to the SPR, but it only provides a link to the knowledge base.

Understandable, I'm fighting a losing battle trying to get their attention as it happened when "One and Two" occured but besides that, I try to stay as far away as possible from it. Just to give a glance of how much I do not enjoy the platform, I come on here every now and then from home or from my phone but have never went on the Platform from home or my phone.

[SPerman]

Am I correct in remembering that everything in the old knowledge base was abandoned and needed to be resubmitted on the platform?

[AlexLachance]

Am I correct in remembering that everything in the old knowledge base was abandoned and needed to be resubmitted on the platform?

Something along that line but a lot more complex with a lot less intuity and no actual "transition". So all these things submitted on the platform aren't attached to your account unless you took the effort to attach it yourself.

[SPerman]

Do you have a direct link for me to vote on..?

I reached out to my VAR, and they sent me this link.

https://support.3ds.com/knowledge-base/ ... 0000369143

I tried clicking "Subscirbe"

image.png (3.91 KiB) Viewed 8610 times

I tried submitting a rating/comment

It is hard to believe this is a multi-billion dollar company.

[AlexLachance]

I reached out to my VAR, and they sent me this link.

https://support.3ds.com/knowledge-base/ ... 0000369143

I tried clicking "Subscirbe"

image.png

I tried submitting a rating/comment

image.png

It is hard to believe this is a multi-billion dollar company.

Odd, it worked for me. Perhaps you're not on the account that is linked to your dashboard..?

Do you have your name at the top right...?

[DanPihlaja]

Unfortunately, when I click on the "open drawing" nothing happens.
Have tried on multiple files.
image.png

It ONLY works if the filename of the part and the filename of the drawing are exactly the same AND they reside in the same folder. The only thing that command does is search the current folder that the part is in for a drawing with the same filename as the part and opens it.

[ryan-feeley]

I tried to paste a direct link to the SPR, but it only provides a link to the knowledge base.

~If you click the "send by email" icon near the bottom, you'll get a draft email that includes a direct link to the article. It is a pretty simple format. Something like~ [Update: while the bottom right of a knowledge base page has only two icons (share by email and print) the top right has three icons, including "copy link"! This is the easiest way to get a direct link]

Code: Select all

https://support.3ds.com/knowledge-base/?q=docid:QA000000###### 

[SPerman]

I'm not sure if this is a bug, or intended behavior.

I needed to duplicate a sketch on multiple planes. I created the sketch, and tied the dimensions to equations. I then copied the sketch onto the different planes. When I open the copied sketch, the dimensions only show the value, and are no longer tied to the equations.

Similarly, in an assembly if you copy a bunch of parts whose relations are described by equations, the copied mates will only show the value, and not the equation.

Hopefully this GIF will help with my explanation.

[SPerman]

I have been having issues with the command manager. (These predate 2023, but are still around.)

First, the command manager will randomly go blank, as if a tab with no features were selected. All I did in this GIF was to click in a couple of random places and move my mouse to the command manager. Where I click does not seem to be related to the problem.

The other problem I have is SW will randomly add tabs to the command manager that I have hidden.

[Glenn Schroeder]

I have been having issues with the command manager. (These predate 2023, but are still around.)

First, the command manager will randomly go blank, as if a tab with no features were selected. All I did in this GIF was to click in a couple of random places and move my mouse to the command manager. Where I click does not seem to be related to the problem.

cm1.gif

The other problem I have is SW will randomly add tabs to the command manager that I have hidden.

I don't remember ever seeing that before. I wonder if having it docked on the side of your monitor instead of at the top has something to do with it?

[SPerman]

I don't remember ever seeing that before. I wonder if having it docked on the side of your monitor instead of at the top has something to do with it?

I definitely have a non-standard layout. I remember one time my VAR remoted in, and you would think I had asked them to do Cad in Word Perfect. They were absolutely lost because the buttons aren't where they expected them.

[AlexLachance]

I have been having issues with the command manager. (These predate 2023, but are still around.)

First, the command manager will randomly go blank, as if a tab with no features were selected. All I did in this GIF was to click in a couple of random places and move my mouse to the command manager. Where I click does not seem to be related to the problem.

cm1.gif

The other problem I have is SW will randomly add tabs to the command manager that I have hidden.

That's odd, perhaps related to the bar being on the side? I haven't seen many people work with it on the side.

For the copy-paste, I don't think I've ever seen a use-case where we copy a sketch with an equation on another plane so I can't say if it's normal behavior or not.


Edit: lol me and Glenn think alike

[mp3-250]

This one is quite annoying as I wanted to make some self explaining datacard using tooltips, but two close textboxes end up stealing the focus from each other making the input quite frustrating. (and losing a lot of time in the process)

BR10000369318

workaround: do not use tooltips or move them on labels or in places where the user is unlikely to put the mouse pointer during data input... =)

When two adjacent datacard controls both use a Tooltip the focus is lost when editing one of the controls if the Tooltip of the other control is displayed by moving the cursor
Portfolio / Domain: SOLIDWORKS Desktop / E-Apps
Product: SOLIDWORKS PDM
OS: Windows 10 64 bits
Detected level(s): SOLIDWORKS 2023 SP5
Platform: n/a
Description

In a default vault create tool tips in the SW part datacard for the 'Number' and 'Description' variable controls
In the explorer select a part and click the 'Data Card' tab
Make an edit in the 'Number' field
Move the cursor so that it engages the tool tip in the 'Description' field
Notice the focus in the 'Number' control has been lost so it is not possible to carry on typing
You have to click in the 'Number' control again to continue editing it

[AlexLachance]

lol, I've had that in 2019, the tooltip would span across the entire screen. What a P.I.T.A. that was.