Hi,
I have a part that was made from content center and modified further. I would like Inventor to no longer recognize this part as a content center part. It has been renamed and migrated to 2013 format, but still when inserting into an assembly the assembly recognizes it as a content center part in the browser.
Also, the browser title for the part will not update with the filename.
Solved! Go to Solution.
Solved by Curtis_Waguespack. Go to Solution.
Solved by Cadmanto. Go to Solution.
What is the part? Can you post the file? There are work features added to a part when it is published to the CC. It may be as simple as removing these work features. But what those are depnds on what the part is.
Chris Benner
Inventor Tube & Pipe, Vault Professional
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Open from content center --> save as.
Should be as simple as that. I've got a bunch of stuff that I've done that with, and it doesn't show as a CC part anymore.
Changing the browser name though, I think you have to do that manually once the file is open.
Rusty
See if this link helps you.
If this solved your issue please mark this posting "Accept as Solution".
Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!!
hi,
kindly read this blog, it will solve the issue.
I got thisbelow macro from the above site(bit modified for Autodesk Inventor 2011). I saved this as external macro and applied the macro to the part file which has been placed from content center as "Custom". The Macro solved the issue.....
Sub Main()
strip_CC()
End Sub
Sub strip_CC()
Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument
'Check to see if it is not a true content center part . otherwise bail out
If oDoc.ComponentDefinition.IsContentMember = False Then
' Enable all commands and set the subtype to a standard part.
oDoc.DisabledCommandTypes = 0
oDoc.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}"
' Optionally clean up other Content Center related properties.
On Error Resume Next
oDoc.PropertySets.Item("Content Library Component Properties").Delete
Dim DTPropSet As PropertySet
DTPropSet = oDoc.PropertySets.Item("Design Tracking Properties")
DTPropSet.Item("Catalog Web Link").Value = ""
oDoc.Save
End If
End Sub
Hi,
Kindly find the code for converting the selected "custom content center Part file" in an assembly to Normal File. Hope it will be useful for someone who search for the same.
Sub Main()
Dim oOcc As ComponentOccurrence
oOcc = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter, "Pick occurrence")
strip_CC(oOcc)
End Sub
Sub strip_CC(ByVal oOcc1 As ComponentOccurrence)
'Dim oDoc As PartDocument
'oDoc = ThisApplication.ActiveDocument
Dim oOccDef As PartComponentDefinition
oOccDef = oOcc1.Definition
' Just open it in the background
asm = ThisApplication.Documents.Open(oOccDef.Document.FullFileName, False)
'Check to see if it is not a true content center part . otherwise bail out
If oOccDef.Document.ComponentDefinition.IsContentMember = False Then
' Enable all commands and set the subtype to a standard part.
oOccDef.Document.DisabledCommandTypes = 0
oOccDef.Document.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}"
MsgBox(oOccDef.Document.FullFileName)
' Optionally clean up other Content Center related properties.
On Error Resume Next
oOccDef.Document.PropertySets.Item("Content Library Component Properties").Delete
Dim DTPropSet As PropertySet
DTPropSet = oOccDef.Document.PropertySets.Item("Design Tracking Properties")
DTPropSet.Item("Catalog Web Link").Value = ""
oOccDef.Document.Save
End If
End Sub
Hi
This rule Works great from an Assembly by picking the part I want to make normal.
But is it possible to rewrite the rule so it can be run directly on the ipt?
I would be very glad if you or someone else could help me out very soon
I figured it out
I used the code above and modified a little to my need.
Do you mind posting your updated code that worked for you so others can benefit from it?
Thanks
Hi mcgyvr,
I use a version of this with iLogic.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Run in the part file:
Try ThisApplication.ActiveDocument.PropertySets.Item("Content Library Component Properties").Delete MessageBox.Show("KA-POW!" & vbLf & "Content Center Properties smashed!", "iLogic") Catch MessageBox.Show("huh?" & vbLf & _ "Something didn't work..." &vbLf & _ "...file is read only maybe?" &vbLf & _ "...file has no Content Center Properties, maybe?" &vbLf & _ "...other?", "iLogic") End Try
@Curtis_Waguespack, Do you know if it is possible to restore the symbol to the default for an IPT file?
Hi lackas5C4Z4,
Give this a try. I didn't have time to test it much, post back if you run into problems.
Note you might to save or do a rebuild all on the assembly to see the icon for the component change, if the part was already placed in an assembly and that assembly is open.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
oError = 0 Try ThisApplication.ActiveDocument.PropertySets.Item("Content Library Component Properties").Delete oErrorMessage1 = "" Catch oError = oError + 1 oErrorMessage1 = "PropertySet not found: Content Library Component Properties" End Try Try ThisApplication.ActiveDocument.PropertySets.Item("ContentCenter").Delete oErrorMessage2 = "" Catch oError = oError + 1 oErrorMessage2 = "PropertySet not found: ContentCenter" End Try If oError = 2 Then MessageBox.Show("huh?" & vbLf & _ "Something didn't work..." &vbLf & _ "...file is read only maybe?" &vbLf & _ "...file has no Content Center Properties, maybe?" &vbLf & _ "...other?", "iLogic") ElseIf oError = 1 Then MessageBox.Show(oErrorMessage1 & vbLf & _ oErrorMessage2, "iLogic") Else MessageBox.Show("KA-POW!" & vbLf & "Content Center Properties smashed!", "iLogic") End If
This worked beautifully. Didn't even have to rebuild the assembly. Thank you very much!
Note: it did throw an error on the parts where I used the previous script but still got the job done.