Fixing External Referanses (in context modeling) - Without PDM 2

[Helepolis]

Hi all,

I love(!) this software most of the time, but sometimes I F'ing hate the F'ing thing!!
(had to blow some steam off)

Now with that out of the way..

I'm working on an assembly in which some of the parts are virtual and had been created using in-context modeling method.
For the sake of the argument, I'm working on a version 2.0 of the assembly, while one of the virtual parts was made in the context of version 1.5 of the same assembly.
Now when I try to change a feature in the said virtual part, I get an error saying that the part has features defined in the context of another assembly (version 1.5), and that I can edit the part but can't create any new external references to the current assembly (version 2.0).

I scoured the internet for a possible solution, but everything I found had a PDM involved in it or it had nothing to do with in-context modeling (e.g. broken reference between a model and it's drawing which is easy to fix).

Is there a way to fix this F'ing issue, without having to rebuild the whole assembly again from version 1.5 to get to the feature needed to be changed?

Thanks!
SD

 

[Gupta65]

Tools > Options > External References and select "Allow multiple contexts for parts when editing in assembly"

Deepak Gupta
SOLIDWORKS Champion and Expert
SW 2022 SP0.0, 2021 SP5.1 and 2020 SP5.0
Boxer's SOLIDWORKS Blog

 

[Helepolis]

Thanks for the tip, but this didnt do a thing, still getting the the same error.

Checked the option you've suggested.

Tried to assigned a new reference.

Still getting the same error.

 

[Gupta65]

Try toggling the plane creation method and then change back to coincident. And then select the desired entity.

Deepak Gupta
SOLIDWORKS Champion and Expert
SW 2022 SP0.0, 2021 SP5.1 and 2020 SP5.0
Boxer's SOLIDWORKS Blog

 

[Helepolis]

Nope, didn't help either.

It turns out that I can't create any new feature (sketch, Plane etc.) using entities that were created at the 1.2d6 version of the assembly.
I'm getting an error

Is there a menu where I can pinpoint where/what is the conflict and is is fixable at all (without PDM)?

 

[Gupta65]

This looks strange. Will it be possible for your to share the complete assembly to check? OR you can send the issue to your reseller and let their team resolve it.

Deepak Gupta
SOLIDWORKS Champion and Expert
SW 2022 SP0.0, 2021 SP5.1 and 2020 SP5.0
Boxer's SOLIDWORKS Blog

 

[Helepolis]

Honestly, it might be an issue showing the feature tree (work related).
Best I can do. for now, is list the hierarchy of the top level assembly, it's sub-assemblies and where is the virtual part that is missing the context.

Are there any specifics that you are looking for, that might lead to figuring whats going on?

Regarding the reseller, it's a holiday right now so they're not working, and I really want to resolve this issue asap.

 

[Gupta65]

I understand the situation and issues for not able to share the files. But can you try to make a similar dummy assembly?

Deepak Gupta
SOLIDWORKS Champion and Expert
SW 2022 SP0.0, 2021 SP5.1 and 2020 SP5.0
Boxer's SOLIDWORKS Blog

 

[Helepolis]

Fortunately I think the issue has been solved, though It's a little bit convoluted without a PDM.

I used the Solidworks-File-Utilities (replacement for the Soldiworks-Explorer since 2020) to rename the sub-assembly (".._v1.4d_..") with the out-of-context virtual part, to the last file name where the assembly still had all the external references in place (the name that pops-up in the error; ".._v1.2d6_..").

I copy-pasted the problematic sub-assembly (so not to mess up the original v1.4d sub-assembly file) to another folder --> renamed the assembly from v1.4d to v1.2d6 --> opened the top assembly and using the "Replace Components" in Solidworks I've replaced the out-of-context assembly with the newly renamed one (which already fixed the out-of-context issue) --> closed everything in Solid and renamed the sub-assembly again (using the Solidworks-File-Utilities) back, from v1.2d6 to the proper version name --> Then I've cut-pasted the renamed sub-assembly back to the original folder --> opend soldiworks and loaded the top-tier assembly again to fix the missing file issue (due to moving the fixed sub-assembly file between folders).

Hope this will help someone in a similar situation.

Now everything checks out, no out-of-context issues.
But it still annoys me, even infuriates, as this whole BS could have been done by some simple interface that just "tells" solidworks that "this is the new file name for the same reference", which is basically exactly what I have done.
I guess this is another one of those F'ing greedy marketing strategies of Dassault for designers to buy the PDM (like placing one of the most rudimentary features, namely the "surface flatten" behind a pay-wall).

 

[jassco]

Hi, Helepolis:

How did you create version 2.0 of the assembly? This "issue" that you are complaining is not related to PDM system. Even if you don't use any PDM system, relationships between features are always. Your issue can be fixed easily if you know the relationships.

Best regards,

Alex

 

[Helepolis]

Hey, for some reason if I try to 'save as' the top assembly Solid either gives me an error that I can't save under the new name or on the occasion It does allows me to save I get a "christmas tree" of errors due to "out of context" external references (top down assembly).
So each time I need to make a new version I use the Solidworks File Utilities to rename a copied file of a relevant assembly.

Every search result I came across in relation to my issue was referencing PDM, and practically 99% of the "hits" gave a simple solution using the PDM to "reassign" the external references, basically the same thing I did but with not as convoluted.

Maybe I've missed something and made this whole thing way more complicated than it actually was, but again, I have exhausted every possible solution, to try and fix that issue that didn't involve the external referencing system of Solidworks.

 

[jassco]

Hi, Helepolis:

Your assembly is called a "Top down assembly". You have an in-context part which is controlled by the assembly. In another word, this in-context part is a "Custom" part.

If you need to make a version for your assembly, you will need to also create a new version for this in-context part simultaneously unless you want this in-context part to be controlled by the original assembly.

Each assembly model has a path feature that controls this behavior. If you want to have multiple assemblies that share a same part, you need to make it a stand-alone part (or a standard part).

Best regards,

Alex

 

[Helepolis]

Thanks for the clarification, but I'm a power-user so I'm familiar with all of what you have mentioned (probably should have used proper terms in my descriptions of the issue).
Although I'm working on a rather complex top-level-assembly (TLA) with all of it's in-context sub-assemblies and virtual-parts, I have to work and make due without a PDM, which basically manages the relations and versions of the in-context parts/assemblies automatically (on some level), without it I have to be diligent and manage those versions manually.

With that said, although I have multiple sub-assemblies and a few solid-parts (most of them are virtual) which are (*partially) controlled and driven by the TLA, I had no problem managing the file versions properly, with the exception of that one time I saved the "problematic" sub-assembly the wrong way (didn't notice it) and made is "out-of-context".
*The sub-assemblies began their life as a stand-alone file, which was later added to the TLA and new in-context features were added.