content center part properties after save as

[b.ziegler]

I am having a problem with content center parts after a "Save As" is performed and the file is saved elsewhere.  In this case a bearing that was dimensionally the same as a CC part was saved with a new part number in the project folder (old part number: ES21-0-2953, new part number: 10377-C-1027).

After the save as and replacement, the assembly display name still shows the display name of the CC part (which is a formula of the filename and the description)

Under properties, on the general tab, the filename is displayed as correct (10377-C-1027)

On the project tab: the part number, which should display the file name (10377-C-1027), displays the old filename of the CC part (ES21-0-2953).

The top of the properties box and at the top of the inventor screen, the CC part display name is shown, see highlighted fields below.

My questions:

how can I set up inventor so that the proper information is displayed for the part?

how do I prevent this from happening in the future.

Please note: this did not use the "save as custom" from the insert from content center dialog, this was a part in the assembly that was opened and "Save As" was performed.  Im not sure if that makes a difference.

Thank you in advance.

[jan_priban]

Hello,

this is standard behavior - Part placed from Content Center As Standard is displayed in assembly browser in the format "Family Name - Size Designation", while part placed from Content Center As Custom behaves as part placed manually by user by the "Place component" command = is displayed in assembly browser as File Name.

Both As Standard and As Custom have same PartNumber - defined by family Content Center table (column PartNumber)

Reading your post I think you want all part being displayed as File Name in assembly browser. For such need there is the Rename Browser Nodes utility - see please the RenameBrowserNodes1.jpg picture.

Regards

Jan Priban

[b.ziegler]

Good morning,

Thank you for this reply.  This helps a little bit but does not address 75% of my issues/concerns.

Renaming browser nodes changes the browser display of both the renamed and all of the content center parts, which is better than nothing.  But when I open the part it still has all of the old CC information.

how can I have Inventor display the proper information here:

[jan_priban · Accepted solution]

Hello,

I think I see what you want. Brief description:

Basically IPT/part file has displayName same as FileName by default. But user can override displayName.

Assembly browser shows/honors displayName of component/IPT placed in assembly, as said line above, it could be by default IPT's fileName or overridden name/string.

Content Center for components placed As Standard overrides display name. For components placed As Custom does not overrides displayName.

In your workflow, you placed Content Center part As Standard into assembly, then you open it and Save As to another location (outside CC library folder to make it writable/modifiable)  with different file name, like MySaveAsCCpart.ipt - I suppose

Than you placed MySaveAsCCpart.ipt into assembly.

Explanation what happens: The MySaveAsCCpart.ipt has displayName overriden by Content Center, so even it was Save As new IPT, it still has overridden displayName which Inventor honors/follows. By Save As displayName doesn't "reset" to fileName, but remains. When you place MySaveAsCCpart.ipt into an assembly, assembly browser shows it by its overridden displayName. Since overridden value/string has higher priority/value than default displayName = fileName, Save As file is still displayed in assembly browser as Content Center part (format Standard & Designation).

Basically: MySaveAsCCpart.ipt still has overridden displayName defined by Content Center, because Save As does not influence displayName

So what you need: you need to delete overridden IPT's displayName in MySaveAsCCpart.ipt and let Inventor show default fileName.

1. Open your IPT Save As file

2. Delete its displayName = let Inventor use default fileName

See please the video 2020-01-17_9-03-24.mp4 

You can leverage for such process API or iLogic and let Inventor do that automatically for all Save As IPTs

Here is iLogic code that does it

' Get the active assembly.
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisApplication.ActiveDocument

' Iterate through all referenced documents.
Dim oDoc As Document
For Each oDOc In oAsmDoc.AllReferencedDocuments
If oDoc.DocumentType = kPartDocumentObject Then
If oDoc.IsModifiable Then
'MsgBox(oDoc.DisplayName, , "Name")
oDoc.DisplayName = ""
End If
End If
Next

My suggestion: If you want to have modifiable CC part with displayName = fileName, create them from Content Center As Custom - 2020-01-17_9-01-25.mp4 

Regards

Jan Priban

[b.ziegler]

That fixes the problem, thank you.