View dependent partslist 2

[Ritchie]

Is there a way to make a partslist display only the parts that are shown in a drawing view? I have made an exploded view of some (not all) components of an assembly. However all the components show up in the partslist when I make one. I just want the partslist to display only the parts that are visible in the drawing view...

 

[JohnRBaker]

At the moment you'll have to 'edit-out' the ones that you don't want to include. Now if you're running NX 9.0, just go to the Assembly Navigator, which you should see ALL of your components, even the ones not currently seen in your Exploded View. Just select these 'missing' Components, either one at a time or all of them at once, press MB3 and select the 'Properties' option. When the dialog comes-up, select the 'Attributes' tab and in the 'Category' of Attributes titled 'DB Component Instance' you should find two Attributes, which currently has <No Value> assigned, named 'PLIST_IGNORE_MEMBER' and 'PLIST_IGNORE_SUBASSEMBLY'. If your 'missing' part is just a piece part select the first Attribute, 'PLIST_IGNORE_MEMBER', and change the value to 'Yes' and hit OK. If it's a subassembly and you wish to remove all included components in the sub-assembly, edit the value of the second Attribute, 'PLIST_IGNORE_SUBASSEMBLY', setting its value to 'yes' and hitting OK. This will remove those items from consideration when the Assembly parts List updates.

Now if you're running an older version of NX, this still works, just that you'll need to explicitly create whichever of these Attributes you need by going to the Assembly navigator in your Drawing file and adding it wherever you wish, just make sure that you give it a value of 'Yes' before hitting OK.

John R. Baker, P.E.
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Product Engineering Software
Siemens PLM Software Inc.
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[Ritchie]

Thanks for the elaborate answer, I managed to get the result that I wanted. What surprises me though is the amount of work that has to be done, it's al manual editing. After all the model view to generate the exploded view has already been defined. I can not help but feel it should only be right if the partslist can somehow be linked to this model view and inherit the hide/show status of the exploded view. To me this current solution seems a bit like a work around. Nevertheless it works and in the end that's what counts, so thanks again!

 

[JohnRBaker]

The Parts List is generated by the content of the Assembly that the Drawing is referencing, not by what you see in any one view on the Drawing, irrespective of where or how that view was created.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Ritchie]

OK John, that's clear to me now. Thanks!

 

[Ritchie]

Just one more thing. I suppose it's not done or maybe not even possible to have more partslists in one drawing? At least, not when these partlists have to display different components?

 

[JohnRBaker]

Yes, you can have multiple Parts Lists on the same drawing, however there is an environment variable in the 'ugii_env.dat' file that needs to be UNSET before that capability is enabled. As you can imagine, when in this mode you'll need to control the final contents of any additional Parts Lists manually and while it's possible to control which views are linked to which Parts List, this is only with respect to which set of call-out bubbles are seen in which Drawing view, NOT whether the visble Components in that view are actually controlling the content of the selected Parts List.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Ritchie]

OK thanks John, if I understand it correctly you would not recommend changing this setting? My local NX support have also informed me about this option, I would have to add: UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST=0 to the dat file you mentioned. I tried this, but without any result (yet). My local support is still looking into it.

But I guess the "best practice" is to have only one partslist per drawing?

 

[cowski]

As an alternative to editing attributes to remove components from the parts list, you can also use "edit levels". Right click your parts list and select "edit levels", choose the "select/deselect subassemblies" option and deselect any parts you don't want in the list.

www.nxjournaling.com

 

[Ritchie]

Thanks Cowski...this is exactly what I was looking for! Much easier than the attribute option and furthermore "view sensitive", meaning I can control the partlists per sheet/view. I now have 4 exploded views on 4 sheets in one drawing file (explaining the building order of the assembly), each with their own relative partslist. So it was possible after all!

 

[Ritchie]

I wanted to make some updates to this drawing and here is what happened. When I switch to modeling view (within the drawing file) I can access the exploded views that control the drawing views. I can make changes to them, but when I then switch back to the drawing the drawing views do not update to reflect these changes, not even when I choose the update command.

I have saved the file after making the hide/show changes to the exploded views, before switching back to the drawing. Have I forgotten something? Do I have to save the changes to the exploded views in a seperate way or is there some setting that overrules the hide/show status of the exploded views?

Thanks in advance...

 

[cowski]

What exactly do you mean by "hide/show changes to the exploded views"? Are you trying to hide a component in the exploded view by hiding it in the modeling view?

www.nxjournaling.com

 

[Ritchie]

Hi Cowski, yes that's exactly what I'm trying to do. Am I wrong?

 

[Ritchie]

I just remembered the way to control what is being displayed in the drafting view. Right click on the view, edit and a dialog box shows up where I can select the components I want to hide directly in the drawing view (under "hidden components").

This works, but nevertheless I'm a bit confused. What should be the correct workflow here? Apparently the hide/show status in the modelling view does not affect what is being displayed in the drafting view?

 

[JohnRBaker]

That is correct.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Ritchie]

OK, thank you for confirming that. I'm still a bit confused why things are the way they are, but sometimes it just is what it is .