PDM and/or linking problem

[rudragoo]

Hi

We are having problems with our PDM vault and can't get any real answers from our VAR.

We are creating a manual of the top assembly - breaking each sub-assy and BOM into seperate pages- top assy, top assy bom, first sub-assy, first sub-assy bom, etc. Many of these subs are on several top assemblies.

The top assembly model has been attached to each sub-assy. When I open a valve assembly (sub-assembly) the manual and assembly model of every assembly that uses that sub is attached to the sub-assembly model and drawing and is opened at the same time so instead of six components I get eighty downloading from the vault.

I now have sub-assys with three huge manuals/models attached that load whenever I load a sub-assy.

My VAR says "too bad live with it" but is there any way to have the subs attached to the top assy models rather than the top assembly models attached to the subs? I thought that was how SW was supposed to be designed.

Thanks

 

[Standing]

rudragoo,
Your issue sounds like when I put a SolidWorks "Model / Drawing" into an AutoCAD drawing. Yes, I had to live with it or manually drawing the picture into the AutoCAD drawing. We do not insert SolidWorks Models into AutoCAD drawings anymore.


Standing
SolidWorks Pro 2009 x64, SP3.0, PDMWorks Workgroup, SolidWorks BOM,
HP xw8600, 64-bit Windows Vista Business, Service Pack 1
Intel Xeon CPU, 3.00 GHz, 16 GB RAM, Virtual memory 166682 MB, nVidia Quadro FX 4600

 

[CorBlimeyLimey]

rudragoo,

I have never used PDM so am having difficulty understanding the problem.

How can the TL model be 'attached' to it's sub-assys? Were they created in-context?

Are you trying to create an electronic or printed manual?

What program are you using to create the manual? (Word, Adobe, ???)

Are you placing the manuals in the Design Binder sections?

 

[rudragoo]

We found this problem when we were creating a manual as a SW multi-page drawing. The top assy model had several sub-assys as children. The way it is supposed to work is the sub-assys are referenced as children to the top model. When opening the top model the vault would search for the subs and load them too. The drawing/manual is a drawing file of the top assembly model.

Now, however, when I look at the sub-assy models in the PDM vault I see that the top assy model drawing is referenced as a child to the sub-assy.

When we check out the sub-assy from the PDM vault, since the top assy drawing is referenced as a child, everything in the top assy loads too. And since the subs are used in several top assys- all those top assys are children and load as well.

Basically I need help in keeping the top assy models/drawings from being a child of the sub-assy. My VAR says that is just the way it is and we should live with it. However SW training says the sub is the child of the top assy.

Any suggestions?

Thank you

 

[CorBlimeyLimey]

Drawings are created from the models. The drawings contain the references, not the models.

Upper level model assys are created from lower level sub-assys and parts. The upper level assys contain the references, not the subs or parts.

The only way I could see the TL assy being referenced at the sub-assy level drawing, is if the TL assy is called into a sub-assy drawing and then all components are hidden except for the sub being detailed. Or if the TL assy is being used outside the sheet border for sections or item number synchronising. Are you doing anything like that?

 

[rudragoo]

Hi

This is the answer I got for this problem. Thought I would share.

The issue here is not related to the parent/child relation of the files (part/assembly/drawing) but to the reference of the part and assembly files to the drawing file. For example if you have a drawing with just one assembly being displayed in it, the drawing will only display a reference to the assembly in the vault. But when you decide to add another view of one of the parts from the assembly into the same drawing (so now the drawing is displaying the assembly and one component), the drawing will now be display under the assembly as well as the component in the vault since they are both being referenced by the drawing. As you continue to add more components and sub assemblies into the drawing, these files will also display the same drawing in the vault since they too are being referenced by the drawing. So if you have 10 different files in the same drawing, each file in the vault that is being referenced by the drawing, will display the drawing underneath them. This is not creating multiple files of the same drawing within the vault, it is only creating and displaying a reference tag to the original drawing and it references. This is an intended functionality of PDMWorks which allows the user to quickly see what files are currently being referenced by other files.

As far as trying to check out just one file and having all of the associated files come with it, there is a workaround for this. If you go to your SolidWorks Workgroup PDM options, click on the "commands defaults" tab and make sure "select all references, include drawings and include attachments" are unchecked then this will check out only the file you want checked out and not any of its referenced files.

Regardless of how many sheets you use with your drawing, the reference is still looking at the drawing file as a whole and not the individual sheets. So for example, you could have 10 different components on one sheet or 10 sheets with one component on each sheet and as long as the components are all in the same drawing file (regardless of the number of sheets), They (the components) will all have a reference to the same drawing within the vault.

 

[rgrayclamps]

Hi, rudragoo:

It does not seem you got answers for your problem. I am trying to help you, but it seems from your posts, you do not completely understand relationship between part models, assembly models, and drawing documents (parts or assemblies). For example, what do you mean you say "The top assembly model has been attached to each sub-assy."? (A dog trails its own tail.) Relationship between drawings and models is one-way. CorBlimeyLimey made very accurate statements about this relationship. You should reread his comments. When you change documents, you have to pinpoint to make sure what documents you really want to change. When you do that, your problem will not exist.

Good Luck!