iLogic Rule - Convert part type from above assembly
If this is the entire rule, then I assume it is a local iLogic rule and that "SEAL_CUSTOM_EXTENTS" is the name of a local Parameter. If so, that Parameter would need to exist within the Assembly.
Or if that parameter only exists within the target part, you would have to access its similarly to this:
If Parameter.Value(oTargetDoc.DisplayName,"SEAL_CUSTOM_EXTENTS") = "REQUIRED" Thenfor it to work.
When using the iProperties.Value() route to access the iProperties, and you are not specifying a component name or a document name as the first input variable, you are accessing the iProperties of the document which contains this rule. To access the iProperties of the target part file, you would either need to specify that part documents name as the first input variable (similarly to how I am doing in the Parameter call above, or you will have to access its iProperties the long way and dig down through the part document object, PropertySets, PropertySet, Property, Value.
Here is an alternative rule that you might use if accessing the parts parameters and iProperties from the assembly:
(You will need to create a variable for the target part document, and set its value somehow, which is what this first line is attempting to do, first.)
Dim oTargetPart As PartDocument = ThisApplication.Documents.Open("C:\Temp\Part.ipt", False)
If Parameter.Value(oTargetPart.DisplayName,"SEAL_CUSTOM_EXTENTS") = "REQUIRED" Then
iProperties.Value(oTargetPart.DisplayName, "Project", "Part Number") = "N/A"
'or
'oTargetPart.PropertySets.Item("Design Tracking Properties").Item("Part Number").Value = "N/A"
iProperties.Value(oTargetPart.DisplayName, "Summary", "Keywords") = "RTSM"
'or
'oTargetPart.PropertySets.Item("Inventor Summary Information").Item("Keywords").Value = "RTSM"
Else
iProperties.Value(oTargetPart.DisplayName, "Summary", "Keywords") = "N/A"
'or
'oTargetPart.PropertySets.Item("Inventor Summary Information").Item("Keywords").Value = "N/A"
ThisApplication.ActiveDocument.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}"
End If
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Wesley Crihfield
(Not an Autodesk Employee)
if you run the rule from an assembly then "ThisApplication.ActiveDocument" will return the assembly document. You will need to get the part document object. From the code you gave i cant tell how you want to do that. But if you want to convert all part documents you could try the code below
Dim doc As AssemblyDocument = ThisApplication.ActiveDocument For Each refDoc As Document In doc.AllReferencedDocuments If refDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then ThisApplication.ActiveDocument.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" End If Next
Jelte de Jong
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Just an idea...but have you considered adding a custom iProperty, Attribute, or Parameter (or similar) within the parts in question, then changing its value according to your conditions. Then alter your other solution that exports all the sheet metal parts, so that it checks the value of this special iProperty, Attribute, or Parameter, before it exports them? And using this method instead of changing the part back and forth from being a regular part and being a Sheet Metal part?
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Wesley Crihfield
(Not an Autodesk Employee)
I see. Tough situation. Here is a more robust and complete version of my earlier code, with several checks in there to help eliminate some possible errors that may be preventing it from working.
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("An Assembly Document must be active for this rule (" & iLogicVb.RuleName & ") to work. Exiting.",vbOKOnly+vbCritical, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oADoc As AssemblyDocument = ThisAssembly.Document
For Each oRefDoc As Document In oADoc.AllReferencedDocuments
If oRefDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim oPDoc As PartDocument = ThisApplication.Documents.Open(oRefDoc.FullDocumentName, False)
For Each oUParam As UserParameter In oPDoc.ComponentDefinition.Parameters.UserParameters
Dim oExists As Boolean
If oUParam.Name = "SEAL_CUSTOM_EXTENTS" Then
oExists = True
If oUParam.Value = "REQUIRED" Then
oPDoc.PropertySets.Item("Design Tracking Properties").Item("Part Number").Value = "N/A"
oPDoc.PropertySets.Item("Inventor Summary Information").Item("Keywords").Value = "RTSM"
Try
'Check if it is a 'Regular Part', if not change it to one.
If oPDoc.SubType <> "{4D29B490-49B2-11D0-93C3-7E0706000000}" Then
oPDoc.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}"
End If
Catch
MsgBox("The attempt to change the SubType of " & oPDoc.FullFileName & vbCrLf & _
"to a 'Regular Part' failed.",,"")
End Try
Else 'if that parameter didn't have that value...
oPDoc.PropertySets.Item("Inventor Summary Information").Item("Keywords").Value = "N/A"
Try
'Check if it is a 'Sheet Metal Part', if not change it to one.
If oPDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
oPDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}"
End If
Catch
MsgBox("The attempt to change the SubType of " & oPDoc.FullFileName & vbCrLf & _
"to a 'Sheet Metal Part' failed.",,"")
End Try
End If
End If
If oExists = False Then
MsgBox("The User Parameter 'SEAL_CUSTOM_EXTENTS' was not found within" & vbCrLf & _
oPDoc.FullFileName & vbCrLf & _
"so this part was not processed.", , "Parameter Not Found")
End If
Next
oPDoc.Save
oPDoc.Close(True)
End If
NextAlso, just in case you weren't aware, there is another option for checking the document's SubType, that is actually readable/understandable. There are iProperties named "Document SubType" and "Document SubType Name" within the "Design Tracking Properties" set. I have found these to be very reliable, and found that they instantly update when changing a part back and forth between regular part and sheet metal part in my testing. In English, if a part is a regular part, the value of "Document SubType Name" is "Modeling", and if is a sheet metal part, the value is "Sheet Metal". Although, I am not sure if those values may change to different words for different language Inventor installations. I have also created an 'Idea' within the Inventor Idea Station to create a 'DocumentSubTypeEnum' to better handle these types of inquiries in a readable, stable way.
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Wesley Crihfield
(Not an Autodesk Employee)
OK. Some peoples installs don't seem to like that 'iLogicVb.RuleName' use, even though I've been using it for years without any problems. It is totally unnecessary though, and can simply be completely eliminated/deleted from that message, if it is causing issues. You can have that message say anything you want. It is just meant to inform you if the active document when the rule is started it the right type of document or not, and that if it is the wrong type, it is going to exit the rule without running.
If 'ThisAssembly.Document' is causing you problems, try replacing it with 'ThisApplication.ActiveDocument'.
Although I am curious why it is having a problem with it. Are you running this code as a local iLogic rule, an external iLogic rule, or from Visual Studio? If you are running it normally as an iLogic rule in Inventor, do you have the "Straight VB code" option turned on or are you using other settings within the header area of the rule? If so, you may need to turn that option off. And if necessary, put the whole code within a "Sub Main", then the code, then "End Sub", even though iLogic is supposedly implying those for you in the background.
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Wesley Crihfield
(Not an Autodesk Employee)
