SAVE COPY AND REPLACE WITH I-LOGIC

[twinz3950]

I have searched the forums here but could not really find an answer.  I have an assembly that I am working on that will be used as a configurator, driven by I-logic. Everything is work fine but there is one part off the assembly that will be custom to each new assembly.  Is there a way to use I logic  to open the ipt file save it as copy with different name and replace the original in the assembly. I know this can be done manual through the productivity tab within the assembly environment, but I am trying to automate the process so the end user will just have to follow prompts that will be given by i-logic.

[twinz3950]

OK I have this code but I do not need it to go  through all the parts, is there any way to modify this so that it only looks for a part call "shell:1" with in the assembly?

Sub Main()

 Dim Path As String = ThisDoc.Path & "\"

 Dim FileChange As Boolean = False

 InvDoc = ThisDoc.Document

 Dim refDocs As DocumentsEnumerator = InvDoc.AllReferencedDocuments

 Dim refDoc As Document

 For Each refDoc in refDocs

 'MessageBox.show(refDoc.DisplayName)

 'input box to enter new file name

 NewFileName = InputBox("What is the new file name for " & refDoc.DisplayName & "?", "New File Name", refDoc.DisplayName)

 'NewFileName = InputBox("What is the new file name for " & refDoc.DisplayName & "?", "New File Name", iProperties.Value(refDoc.DisplayName, "Project", "Part Number"))

     'if the new file name is blank then use the same name

     If NewFileName = "" Then

         NewFileName = refDoc.DisplayName

     End If

     'if the user also types in the extesion then remove the extension.

     If NewFileName.EndsWith(".ipt") = True Then

         NewFileName = NewFileName.substring(0,NewFileName.length-4)

         'MessageBox.show(NewFileName)

     End If

     'if there is an change in the name then do the following.

     If refDoc.DisplayName <> NewFileName & ".ipt" Then

         'check to see the file already exist. if it does then replace.

         If System.IO.File.Exists(Path & NewFileName & ".ipt") Then

             Component.Replace(refDoc.DisplayName, Path & NewFileName & ".ipt", True)

         Else

             Dim oldName As String = refDoc.DisplayName

             'if it does not exist then recreate the file

             refDoc.saveas(Path & NewFileName & ".ipt",False)

             Call UpdateDrawing(Path, oldName, NewFileName)

         End If

         FileChange = True

     End If

 Next

 If FileChange = True Then

     NewAssemblyName = InputBox("What is the new file name for the assembly?", "New Assembly File Name", iProperties.Value("Project", "Part Number"))

     If NewAssemblyName <> "" Then

         Dim oldName As String = ThisDoc.FileName(True) 'include extension

         ThisDoc.Document.SaveAs(Path & NewAssemblyName & ".iam" , False)

         Call UpdateDrawing(Path, oldName, NewAssemblyName)

     End If

 End If

 iLogicVb.UpdateWhenDone = True

 End Sub

 Private Sub UpdateDrawing (ByVal Path As String, ByVal oldName As String, ByVal newName As String)

     Dim oDestinationDoc As DrawingDocument

     Dim strFileExtension As String = oldName.substring(oldName.Length-4,4)

     oldName = oldName.substring(0,oldName.Length-4)

     Dim sFileName As String = Path & oldName & ".idw"

     Try

         If System.IO.File.Exists(sFileName) Then

             oDestinationDoc = ThisApplication.Documents.Open(sFileName)

             oDestinationDoc.saveas(Path & newName & ".idw",False)

             Dim oDocDescriptor As DocumentDescriptor

             oDocDescriptor = oDestinationDoc.ReferencedDocumentDescriptors.Item(1)

             Dim oFileDescriptor As FileDescriptor

             oFileDescriptor = oDocDescriptor.ReferencedFileDescriptor

             oFileDescriptor.ReplaceReference(Path & newName & strFileExtension)

             oDestinationDoc.Update()

             oDestinationDoc.Close

         End If

     Catch

         oDestinationDoc.Close

         MessageBox.Show("error")

     End Try

 End Sub

[pcrawley · Accepted solution]

I'm not in front of Inventor right now, so I can't check any of this, but using my (badly) calibrated eyeball, try the following.  (I note that the code references "display name" rather than filename - so if you rename anything in your browser, this is likey to fail!)

InvDoc = ThisDoc.Document

 Dim refDocs As DocumentsEnumerator = InvDoc.AllReferencedDocuments

 Dim refDoc As Document

 For Each refDoc in refDocs

 'MessageBox.show(refDoc.DisplayName)

If refDoc.DisplayName = "shell:1" then

'This will find only "shell:1" and execute all the following code.  

'If the refDoc.DisplayName is not "Shell:1" it'll jump to the red "End If" and proceed to check the next component.

 'input box to enter new file name

 NewFileName = InputBox("What is the new file name for " & refDoc.DisplayName & "?", "New File Name", refDoc.DisplayName)

 'NewFileName = InputBox("What is the new file name for " & refDoc.DisplayName & "?", "New File Name", iProperties.Value(refDoc.DisplayName, "Project", "Part Number"))

     'if the new file name is blank then use the same name

     If NewFileName = "" Then

         NewFileName = refDoc.DisplayName

     End If

     'if the user also types in the extesion then remove the extension.

     If NewFileName.EndsWith(".ipt") = True Then

         NewFileName = NewFileName.substring(0,NewFileName.length-4)

         'MessageBox.show(NewFileName)

     End If

     'if there is a change in the name then do the following.

     If refDoc.DisplayName <> NewFileName & ".ipt" Then

         'check to see the file already exist. if it does then replace.

         If System.IO.File.Exists(Path & NewFileName & ".ipt") Then

             Component.Replace(refDoc.DisplayName, Path & NewFileName & ".ipt", True)

         Else

             Dim oldName As String = refDoc.DisplayName

             'if it does not exist then recreate the file

             refDoc.saveas(Path & NewFileName & ".ipt",False)

             Call UpdateDrawing(Path, oldName, NewFileName)

         End If

         FileChange = True

     End If

   End If

 Next

'Not sure if you need any of the following as it appears to be building new sub-assemblies - and you are only replacing a part.

'If you don't need it, comment it out using a  '  at the beginning of each line.

' If FileChange = True Then

'     NewAssemblyName = InputBox("What is the new file name for the assembly?", "New Assembly File Name",iProperties.Value("Project", "Part Number"))

'     If NewAssemblyName <> "" Then

'         Dim oldName As String = ThisDoc.FileName(True) 'include extension

'         ThisDoc.Document.SaveAs(Path & NewAssemblyName & ".iam" , False)

'         Call UpdateDrawing(Path, oldName, NewAssemblyName)

'     End If

' End If

 iLogicVb.UpdateWhenDone = True

 End Sub 'I'm not sure about this line.  

'It could exit the iLogic code at this point.  I've only ever used it to end a sub-routine, but none has been defined.  

'Someone who understands code better than me will tell you what it does!

'And this next part is to do with Drawings?  Again, you can probably ditch this too.

' Private Sub UpdateDrawing (ByVal Path As String, ByVal oldName As String, ByVal newName As String)

'     Dim oDestinationDoc As DrawingDocument

'     Dim strFileExtension As String = oldName.substring(oldName.Length-4,4)

'     oldName = oldName.substring(0,oldName.Length-4)

'     Dim sFileName As String = Path & oldName & ".idw"

'     Try

'         If System.IO.File.Exists(sFileName) Then

'             oDestinationDoc = ThisApplication.Documents.Open(sFileName)

'             oDestinationDoc.saveas(Path & newName & ".idw",False)

'             Dim oDocDescriptor As DocumentDescriptor

'             oDocDescriptor = oDestinationDoc.ReferencedDocumentDescriptors.Item(1)

'             Dim oFileDescriptor As FileDescriptor

'             oFileDescriptor = oDocDescriptor.ReferencedFileDescriptor

'             oFileDescriptor.ReplaceReference(Path & newName & strFileExtension)

'             oDestinationDoc.Update()

'             oDestinationDoc.Close

'         End If

'     Catch

'         oDestinationDoc.Close

'         MessageBox.Show("error")

'     End Try

' End Sub

[twinz3950]

thank you so much

[pcrawley]

Wow - you mean it worked?!!

Hope the rest of the project worked out too.

Glad I could help.

[Agenx]

Hi

I have the same desire like twinz390 to rename a particular ipt file (L-B.ipt) in the collection (Ban- master- template.iam) and rename the iam to a new name.
I have tried to copy the ilogic code that are writting, but I can not get the piece of program to virke.I AM NO wizard on the iLogic programming
Does anyone have a suggestion?

[MTheDesigner]

Here is a code I wrote to save and replace a part in an assembly. please note that it only works for parts not subassemblies as it is.

Dim oDoc As Document = ThisApplication.ActiveDocument

'Make sure we are in an assembly
If oDoc.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject
	MsgBox("This code only works on assemblies", "Error")
	Return
End If

'Pick the part and find the document path
Dim oPart As ComponentOccurrence = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter, "Pick Your Item")
Dim oPartDoc As Document = oPart.Definition.Document
Dim oPartPathAndName As String = oPartDoc.FullDocumentName
Dim oPartPath As String = System.IO.Path.GetDirectoryName(oPartPathAndName)
'pick a new name
Dim NewPartName As String = InputBox("Please enter a new file name", "Name Part",System.IO.Path.GetFileName(oPartPathAndName))
'open the document
If NewPartName = "" Then
	Return
End If
Try
	ThisApplication.Documents.Open(oPartPathAndName)
Catch 
	MsgBox("Part path could not be resolved")
	Return
End Try

'Save a new version of the document
Try
	oPartDoc.SaveAs(oPartPath & "\" & NewPartName & ".ipt", True)
	oPartDoc.Close()
Catch
	MsgBox("Could not save the part")
	Return
End Try
Try
	oPart.Replace(oPartPath & "\" & NewPartName & ".ipt",False)
Catch
	MsgBox("Couldn't replace the part")
End Try

 Edit: Fixed a bug and added handling for if the cancel button is pressed.

[MTheDesigner]

Well guys, turns out we all missed the easy way out. Inventor has a built in tool called save and replace, its under the productivity tab in the assembly ribbon, does exactly what we were all trying to do with code.

[pcrawley]

I might be missing something, but from the original post: "I know this can be done manual through the productivity tab within the assembly environment, but I am trying to automate the process so the end user will just have to follow prompts that will be given by i-logic."

[MTheDesigner]

Ah fair enough, you caught me sleeping. If they know the part though, my code will work as long as they just sight the known part in place of the pick command.