iLogic to Rename All Solid Bodies

Issue:
You've created a multi-body solid model with the intent to use the Make Components tool to write out each solid as a new part file. This works fine, but you find yourself wishing there was an easier way to tag each solid with a new name based on a prefix and a series number. For instance, you'd like to name each solid in a part file called 45-723 as such: 45-723_01, 45-723_02, 45-723_03, etc.

Issue:
You can use this iLogic rule to quickly rename the solid bodies for you. In this rule we first look for a custom iProperty named "Prefix" and create it if it is not present. Then we write the part number to the custom iProperty if it is found to be empty. Then the rule uses the value of the custom iProperty named "Prefix" in an input box to query the user for the prefix:

 

The user can change the prefix at this point or accept the existing one. When we press the OK button the rule renames each solid body using the prefix and an increment number, adding a leading zero for each number less than 10.

Thanks to Barbara Han for the original code I used for this rule.

'------- start of ilogic ------

'check for custom iProperty and add it if not found

Dim prefix As String = "Prefix"

customPropertySet = ThisDoc.Document.PropertySets.Item _

("Inventor User Defined Properties")

Try

         prop= customPropertySet.Item(prefix)

Catch

      ' Assume error means not found

            customPropertySet.Add("", prefix)

End Try

'write the part number to the Prefix iProperty if it is empty

if iProperties.Value("Custom", "Prefix") = "" Then

iProperties.Value("Custom", "Prefix") = iProperties.Value("Project", "Part Number") & "_"

else

end if

'check that this active document is a part file   

Dim partDoc As PartDocument

If ThisApplication.ActiveDocument.DocumentType <> kPartDocumentObject Then

MessageBox.Show ("Please open a part document", "iLogic")

End If

'define the active document

partDoc = ThisApplication.ActiveDocument

Dim solid As SurfaceBody

Dim i As Integer

'get input from user

prefix = InputBox("Enter a prefix for the solid body names", "iLogic", iProperties.Value("Custom", "Prefix"))

'write input back to custom iProperty

iProperties.Value("Custom", "Prefix") = prefix

i = 1

'rename all solid bodies incrementing suffix

For Each solid In partDoc.ComponentDefinition.SurfaceBodies

solid.Name = prefix + IIf(i < 10, "0" + CStr(i), CStr(i))

i = i + 1

Next

------- end of ilogic ------