ilogic rule that creating a cope of a drawing and changing its iPart instance.
Perhaps this iLogic rule code will work for you. I've included a lot of comment lines within it to help guide you through what's going on.
You WILL have to edit the middle portion of the code, where you need to define which other iPart you want to be represented within the drawing. I simply gave a generic manual name here. I assume this new iPart doesn't already have its own drawing file, or you wouldn't be creating one for it. I also didn't bother building a list of all the iParts that were already within the current assembly, because I literally have no idea if the new iPart is even in the assembly yet, or how you want to specify it.
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("This rule '" & iLogicVb.RuleName & "' only works for Assembly Documents.",vbOKOnly, "WRONG DOCUMENT TYPE")
Exit Sub 'or Return
End If
Dim oADoc As AssemblyDocument = ThisAssembly.Document
Dim oRefDoc As Document
'get an iPart within the assembly
For Each oRefDoc In oADoc.AllReferencedDocuments
If oRefDoc.DocumentType = DocumentTypeEnum.kDesignElementDocumentObject Then Exit For
Next
'get the path where this iPart's file is found.
Dim oPath As String = IO.Path.GetDirectoryName(oRefDoc.FullFileName) & "\"
'define which other iPart you want to be represented within the new drawing.
Dim oNewModelName As String = "NewModel"
Dim oNewPart As String = oPath & oNewModelName & ".ipt"
Dim oNewDrawing As String = oPath & oNewModelName & ".idw"
If IO.File.Exists(oRefDoc.FullFileName.Replace(".ipt", ".idw")) Then
'open the existing drawing for that iPart (assuming it has the same name and stored in the same directory)
Dim oDDoc As DrawingDocument = ThisApplication.Documents.Open(oRefDoc.FullFileName.Replace(".ipt", ".idw"), False)
'save a new copy of the file to disk, then close this old file
oDDoc.SaveAs(oNewDrawing, True) 'saves a new copy of it to disk, while leaving the old file open
oDDoc.Close(True) 'True = skip save (this is the old document, so we don't want to save it.
'now open the new copy of the drawing
Dim oNewDDoc As DrawingDocument = ThisApplication.Documents.Open(oNewDrawing, False)
'get the current file descriptor being referenced by this drawing
Dim oFD As FileDescriptor = oNewDDoc.ReferencedDocumentDescriptors.Item(1).ReferencedFileDescriptor
'replace it with the full file name of our new iPart's file.
oFD.ReplaceReference(oNewPart)
'update the drawing document
oNewDDoc.Update()
oNewDDoc.Save
oNewDDoc.Close(True)
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Wesley Crihfield
(Not an Autodesk Employee)
Sorry i am fairly new to iLogic and i didn't quite understand how to use it, is it correct how i filled it? (shown in the screenshot)
My idea was more of making a Ilogic/Macro/Script that makes a copy of oppend drawing, switch to the next iPart instance and saves it with the iPart instance name. thank you for your help and time.
Accepted solution
Sorry it took so long to get back to you, I've been really busy.
Within the image you posted:
- the iPart location you put in there should replace the "IO.Path.GetDirectoryName(oRefDoc.FullFileName)", instead of going behind it.
- your iPart name edit seems fine.
- Just checking though...that iPart does have a model file of its own saved out to disk right? (It's not just data on the iPart table, with no physical model that has been saved out to its own file right?) If that iPart is just data on a table, with no model file of its own saved out to disk, that's a different story, and this code may not work for that scenario.
Wesley Crihfield
(Not an Autodesk Employee)
Just to clarify the situation...
- You would be starting the iLogic rule from an 'iPart Factory' part document (the one with the complete table of variations defined within it), right?
- And you want this rule to create a new drawing that is to be used, not open an existing drawing, right?
- What path & file name do you want to save it as? This data will need to be specified in the rule.
- Will there just be one iPart variation shown per sheet, or multiple? If multiple, how many?
- How many views of the one iPart do you want the rule to create on each sheet?
- If more than one view per sheet, then please specify which types of views, what orientations, where they should be on the sheet, view settings such as shaded/hidden lines, representation settings, etc.
- Do actual separate model documents/files (iPart Members) exist in the file system for each variation within the iPart Factory?
- If so, we may need to specify the directory path in the rule somewhere, so we can specify full file name (FullPath\name.extension) of each file to replace the one being referenced in the copied drawing view.
Needless to say, this could likely be a large and complex task, depending on your needs/wants and how detailed/specific everything needs to be.
Wesley Crihfield
(Not an Autodesk Employee)
i have just created ipart with some different variants.
I create an idw file with a view number 1 that contains ipart variation number 1.
I want a macro that crate a new view (in the same idw file and sheet) with variation number 2.
But this new view has to be a copy of view number 1 with varition number 1 of ipart.
I can do manually but the variations are too much, about 100...
So can i do a macro to do this work automatica?
Hi @bseerapathy. Are all the iPart members the same exact geometry, but just different sizes, or do some members have 'features' that other members do not have (or Suppressed features)? If the geometry is the same for all members, but just different sizes, then that would make this process the simplest scenario. In that case, we could just 'copy' the existing drawing sheet, then paste it back into the same drawing document, as a new sheet, so that it already has the view and details in it. Then just switch the DrawingView_ActiveMemberName property value so that it is pointing to the 'next' iPart member. Some view scaling (DrawingView.Scale or DrawingView.ScaleString) may be required too, if there are large size differences among the other members, to keep the view fit within the sheet. Then repeat those steps until we have a Sheet for each iPart member. At least in theory. There is not a 'built-in' method for copying a sheet within a single drawing document though, just one for copying a Sheet from one drawing document to another drawing document (Sheet.CopyTo method). And the process of creating a 'New', temporary other drawing document, just for that copying process, then trying to do the sheet copying that way usually leads to multiple possible unexpected negative issues. The steps required are super simple manually...just select a sheet, press Ctrl+C on keyboard, then unselect that Sheet, and press Ctrl+V on keyboard. So, we would have to 'simulate' those manual actions by using code based object selections, and command executions, instead of true API methods.
Below is an example custom Function routine for copying a sheet within the same drawing document that I had likely posted elsewhere in this forum also. If any of the views on the sheet have 'parent' views on another sheet, this method will not work to copy it though. There are other, further developed versions of this code process, which check for things like that, and may even offer optionally assigning a name to the new sheet, or optionally create a specified number of copies of the specified sheet, but this example below is a simpler version, just to represent the main idea and process.
Sub Main
Dim oDDoc As DrawingDocument = TryCast(ThisApplication.ActiveDocument, Inventor.DrawingDocument)
If oDDoc Is Nothing Then Return
Dim oOrigSheet As Inventor.Sheet = oDDoc.ActiveSheet
Dim oNewSheet As Inventor.Sheet = CopySheet(oDDoc, oOrigSheet)
End Sub
Function CopySheet(oDDoc As DrawingDocument, oSheet As Inventor.Sheet) As Inventor.Sheet
Dim oSS As SelectSet = oDDoc.SelectSet
oSS.Clear()
Dim oCM As CommandManager = ThisApplication.CommandManager
Dim oCDs As ControlDefinitions = oCM.ControlDefinitions
Dim oCopy As ControlDefinition = oCDs.Item("AppCopyCmd")
Dim oPaste As ControlDefinition = oCDs.Item("AppPasteCmd")
oSS.Select(oSheet)
oCopy.Execute2(True)
oSS.Clear()
oPaste.Execute2(True)
Return oDDoc.Sheets.Item(oDDoc.Sheets.Count)
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Wesley Crihfield
(Not an Autodesk Employee)