iLogic to Retrieve Path And File of a Model on a Drawing

[felix.cortes5K3Y2]

Hi Forum,

Does anyone know how I get the path and file of a model inside an idw?

Best regards,

Felix Cortes

[Sergio.D.Suárez]

Hi, look at the following code maybe I can help you. With it you can access the model document from the drawing view.
I used a view selection method. You can select the view through the item or otherwise if you need it.
I hope this helps. regards

Dim oView As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Seleccione Vista")
If oView Is Nothing Then Exit Sub
	
Dim oModelDoc As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument

Dim oViewModelName As String = oModelDoc.DisplayName
Dim oFullFilePath As String = oModelDoc.FullFileName

Dim oFolderPath As String = Left(oFullFilePath, (InStrRev(oFullFilePath, "\", - 1, vbTextCompare) - 1))

MessageBox.Show("DisplayName: " & oViewModelName)
MessageBox.Show("FullFilename: " & oFullFilePath)
MessageBox.Show("FolderPath: " & oFolderPath )

[Anonymous]

Felix,

You can use the ModelDocument code snippet from Advanced Drawing API. This will retrieve the model associated to the drawing. If there's more than one model, it will pick the first one. If there is more than one model, you can use the ModelDocument(View) snippet and this will let you define the view name and it will retrieve the model associated to the view. Once the model is retrieved, which is a document object, you can get different properties such as Displayname, FillFileName, etc.

So the code will look something like this. Hope that helps.

DanV

doc = ThisDrawing.ModelDocument 'from the Model Document snippet
MessageBox.Show(doc.FullDocumentName) 'use FullDocumentName to get path & file name
MessageBox.Show(doc.DisplayName) 'use to get the file name only

[tjvz85]

Hi DanV,

I would like to add a sheet, based on an existing sheet format, for the part/assembly in my drawing.

The snippet you suggest fetches the file path, but how would I insert it into the code below, to fulfill the function I require? Any guidance would be appreciated.

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

'Set a reference to the sheet format named "C size, 4 view"
Dim oFormat As SheetFormat
Try
oFormat = oDrawDoc.SheetFormats.Item("C size, 4 view")
Catch
MessageBox.Show("Error: C size, 4 view might not exist.", "iLogic")
Return
End Try

'Open the model document invisible
Dim oModel As Document
oModel = ThisApplication.Documents.Open("C:\TEMP\block.ipt", False)

'Create a new sheet based on the sheet format using the specified model
Dim oSheet As Sheet
oSheet = oDrawDoc.Sheets.AddUsingSheetFormat(oFormat, oModel)

[Anonymous]

Hello tjvz85,

I'm not sure if I understand your request. Can you give me more detail as to what you are looking to do?

The code that you have there will create a new sheet using the "C Size, 4 View" sheet format. It will use the block.ipt as the model for the sheet format. So when it first starts, there is no model yet. It's a blank sheet therefore this is no model path to retrieve.  Then it will look for the block.ipt in C:\temp and use that as the model for the sheet format. The block.ipt is hard coded into the rule. Are you asking if you can be prompted for the model? If so, you can do something like this. Hopefully that's what you are looking for. If not, repost and let's try again.

Dan

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

'Set a reference to the sheet format named "C size, 4 view"
Dim oFormat As SheetFormat
Try
	oFormat = oDrawDoc.SheetFormats.Item("C size, 4 view")
Catch
	MessageBox.Show("Error: C size, 4 view might not exist.", "iLogic")
	Return
End Try

Dim openfiledia As New OpenFileDialog()
Dim strModelFile As String

With openfiledia
	.Filter = "Autodesk Inventor Part|*.ipt|Autodesk Inventor Assembly|*.iam"
	.Multiselect = False
	'if user cancelled, exit this subroutine
	If .ShowDialog() = DialogResult.Cancel Then
		Exit Sub
	End If
	
	strModelFile = .FileName
End With

'Open the model document invisible
Dim oModel As Document
oModel = ThisApplication.Documents.Open(strModelFile, False)

'Create a new sheet based on the sheet format using the specified model
Dim oSheet As Sheet
oSheet = oDrawDoc.Sheets.AddUsingSheetFormat(oFormat, oModel)

[tjvz85]

Hi DanV,

Thanks for your response.

My goal is this:

We create new drawings for every part or assembly and we use the same template.

For parts, there will only be one sheet per drawing, but for assemblies, we add a sheet for a production specific partslist.

I would like to add the sheet for the assembly file that is on the first sheet.

I have code (written by Curtis Waguespack) to check the Views on the sheet to see whether a part or assembly has been placed and then call a specific function. But I wanted to see if I can rather just check the file placed in the drawing, determine whether it is a part or assembly, and then place the second sheet if it is an assembly.

The code below checks the views, if they are of an assembly, it checks if the model file has a Design view named colour and the writes the colour to a custom iproperty that I use in the title block. If we can't just verify whether the referenced file is an assembly, I would like to run through the views and place the sheet, based on existing Sheet Format.

Thank you in advance for your further assistance.

Sub Main 
	' Get the active drawing document. 
	Dim oDoc As DrawingDocument 
	oDoc = ThisApplication.ActiveDocument 
	
	Dim oSheet As Sheet
	oSheet = oDoc.ActiveSheet	
	
	Dim oViews As DrawingViews
	Dim oView As DrawingView
	

	'get the collection of view on the sheet
	oViews = oSheet.DrawingViews		
	
	' Iterate through the views on the sheet
	For Each oView In oViews	
		
		Dim docDesc As DocumentDescriptor 
		docDesc = oView.ReferencedDocumentDescriptor  
		
		' Verify that the drawing view is of an assembly. 
		If docDesc.ReferencedDocumentType <> kAssemblyDocumentObject Then 
			Continue For
		End If  
		
		' Get the component definition for the assembly. 
		Dim asmDef As AssemblyComponentDefinition 
		asmDef = docDesc.ReferencedDocument.ComponentDefinition 
		
		'define view rep collection
		Dim oViewReps As DesignViewRepresentations
		oViewReps = asmDef.RepresentationsManager.DesignViewRepresentations
		
		oColourViewRepFound = False
		For Each oViewRep In oViewReps
			If oViewRep.Name = "Colour" Then
				oColourViewRepFound = True 
			End If
		Next
		
		If oColourViewRepFound = True Then
			Call ProcessAssemblyColor(oView, asmDef.Occurrences) 
		End If
	Next

End Sub 



Private Sub ProcessAssemblyColor(drawView As DrawingView, _ 
                                 Occurrences As ComponentOccurrences) 
   ' Iterate through the current collection of occurrences. 
   Dim occ As ComponentOccurrence 
   For Each occ In Occurrences 
      ' Check to see if this occurrence is a part or assembly. 
      If occ.DefinitionDocumentType = kPartDocumentObject Then 

         ' Get the render style of the occurrence. 
         Dim color As RenderStyle 
         Dim sourceType As StyleSourceTypeEnum 
         color = occ.GetRenderStyle(sourceType)  
		If color.name IsNot Nothing Then
		 iProperties.Value("Custom", "Lackierung") = color.name
		 Exit For
	 	End If
			

      End If 
   Next 
End Sub