Derive in iProperties of a part.

[Anonymous]

Hello,

I am trying to write a code that will, with a part open (lets call it part A), will open a template part (part B), and then in part B, derive in specific user parameters of part A, and set them as parameters in part B. Then save part B as part A-1 or something.

I have a general idea of how it would work, however am unable to figure out which commands would allow me to derive one part from another part document, and then how to specify to only bring in certain parameters but not work geometry.

Can anyone give me an idea of where to look? Once I have that I'm sure I'll have other problems but I need somewhere to start.

Thanks.

[Anonymous · Accepted solution]

Hi,

try creating a rule in part A, and paste the following code.

Dim NewFileNameAddition As String = "-1"
Dim TemplateFileName As String = "D:\Template.ipt"

Dim CurrentDocFileName As String = ThisDoc.Document.fullfilename
Dim NewDocFileName As String = strings.left(CurrentDocFileName,strings.instrrev(CurrentDocFileName,".") - 1) & NewFileNameAddition & ".ipt"

Dim oNewDoc As Inventor.PartDocument = ThisApplication.Documents.Add(Inventor.DocumentTypeEnum.kPartDocumentObject, TemplateFileName, True)
oNewDoc.SaveAs(NewDocFileName, False)

Dim oNewDocDef As Inventor.PartComponentDefinition = oNewDoc.ComponentDefinition
Dim oDerivedPartDefinition As Inventor.DerivedPartDefinition = oNewDocDef.ReferenceComponents.DerivedPartComponents.CreateDefinition(CurrentDocFileName)
' oDerivedPartDefinition.IncludeAllParameters = True
oDerivedPartDefinition.ExcludeAll()
oDerivedPartDefinition.Parameters.Item("YourParameterName1").IncludeEntity = True
oDerivedPartDefinition.Parameters.Item("YourParameterName2").IncludeEntity = True
oDerivedPartDefinition.Parameters.Item("YourParameterName3").IncludeEntity = True

Dim oNewDerivedPartComponent As Inventor.DerivedPartComponent = oNewDocDef.ReferenceComponents.DerivedPartComponents.Add(oDerivedPartDefinition)

oNewDoc.Save()

MsgBox("Done", MsgBoxStyle.Information, "Done")

Edit the first 2 lines of code to determine which template to use, and how your new filename will look like.

Also don't forget to replace "YourParameterName1"with the parameters of your choice.

Good luck.

[Anonymous]

Thanks a ton! I got what I needed for my code and its working great!

[bradeneuropeArthur]

Hi,

Maybe this idea should be voted!

forums.autodesk.com/t5/inventor-ideas/derived-part-and-assembly-copy-i-properties/idi-p/634

Regards,