iLogic - Create new sheet in existing drawing

[Anonymous]

Hi everyone,

I'm trying to build a new template for our laser parts. I create a seperate sheet in my .idw for every laser part we need to buy. I do this because it's easier for us to sort the parts when they arrive. We don't have fancy machines because we're a fairly small business. I already found a iLogic code where you can create a new drawing from my template and place the part automatically. 

But what I want to do is:

For example, I have the file "Laser Parts 1.idw"

Set "Laser Parts 1.idw" as the location where I need the next sheet

Press "Create Laser Part" in my .ipt 

Then it creates a new sheet in "Laser Parts 1.idw" and places my part

Hope this is understandable and possible 😃

Greetz

Daniel

[Ralf_Krieg]

Hello

You can do this with this external rule. Your part file and the drawing file must be open. The part file must be the active document.

Private Sub main
	'assume your laser part document is open and active
	Dim oPartDoc As PartDocument = ThisApplication.ActiveDocument
	Dim oDrawDoc As DrawingDocument
	Dim oDoc As Document
	
	For Each oDoc In ThisApplication.Documents
		If oDoc.DocumentType = DocumentTypeEnum.kDrawingDocumentObject Then
			If System.IO.Path.GetFileNameWithoutExtension(oDoc.FullFileName) = "Laser Parts 1" Then
				oDrawDoc = oDoc
				Exit For
			End If
		End If
	Next
	
	If oDrawDoc Is Nothing Then
		MsgBox("Drawing file " & Chr(34) & "Laser Parts 1" & Chr(34) & " not open.", "iLogic")
		Exit Sub
	End If

	Dim oActiveSheet As Sheet = oDrawDoc.ActiveSheet
	Dim oSheetSize As DrawingSheetSizeEnum = oActiveSheet.Size
	Dim oOrientation As PageOrientationTypeEnum = oActiveSheet.Orientation
	Dim sSheetName As String= System.IO.Path.GetFileNameWithoutExtension(oPartDoc.FullFileName)
	Dim oWidth As Object = oActiveSheet.Width
	Dim oHeight As Object=oActiveSheet.Height
	
	Dim oSheet As Sheet = oDrawDoc.Sheets.Add(oSheetSize, oOrientation, sSheetName, oWidth, oHeight)
	oSheet.AddTitleBlock(oActiveSheet.TitleBlock.Definition)
	oSheet.AddDefaultBorder()
	
	oSheet.Activate
	Dim oPoint As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oSheet.Width/2, oSheet.Height/2)
	
	oSheet.DrawingViews.AddBaseView(oPartDoc,oPoint,1,ViewOrientationTypeEnum.kFrontViewOrientation,DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle )

MsgBox("Done")	
End Sub

[Anonymous]

Hey!

Thanks, it works 🙂 

Is it possible to get a pop-up that wants you to pick a location of the idw? 

Thanks

Daniel

[bradeneuropeArthur]

Try this:

Dim oFileDlg As Inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.InitialDirectory = oOrigRefName
oFileDlg.CancelError = True
On Error Resume Next
oFileDlg.FileName = ThisDoc.FileName
oFileDlg.ShowSave()

[Ralf_Krieg]

Hello

What do want to pick?

The drawing template to create a new LaserPart1.idw if not already open?

The drawing LaserPart1.idw if it's not already open?

The location for the drawing LaserPart1 to be saved to with/without new name?

[Anonymous]

I edited the code so that I can put the Name of my .idw file. In my case I saved the file as "200389-390 Brennteile.idw". Inventor now finds the opened idw and places my part on a new sheet. I'd like to have like a "Open" button and then pick my .idw through the windows explorer instead of writing down the name in a text field. I think it would look more professional, even if it's the same result. 

BTW: I put quantities into my .ipt parts. I always have to adjust them to our order. For example we need 4 pieces for one assembly, but we have to build the same thing two times - so we need 8 pieces in total. Is it possible to write down 4 parts and then chose the amount of assemblies in the idw so it multiplies 2*4=8? (Independent from the .ipt, there should always be 4)

[Ralf_Krieg]

Hello

With this code snippet you can gat the full document name including path of the selected drawing document. This can be used to check if this document is already open or open it.

Dim oFileDlg As Inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.Filter="Autodesk Inventor-Drawing (*.idw)|*.idw|All Files (*.*)|*.*"
oFileDlg.FilterIndex = 1
oFileDlg.DialogTitle = "Open Laser Part Drawing"
oFileDlg.CancelError = True
On Error Resume Next
Err.Clear 
	oFileDlg.ShowOpen()
If Not Err.Number = 0 Then
	Exit Sub
Else
	MsgBox(oFileDlg.FileName,,"GetDrawDocName")
End If

Why do you manipulate quantitys by hand? It's the worst case to write quantitys in part files. A part is a part and has no quantity. Even if sub-contractor says it's necessary to write down amounts on a part drawing. Amounts can be taken out of the BOM. Don't make this manual.

Take an assembly and insert the required amount of parts for 1 tank. Then create a second assembly for the whole order and place the required amount of tanks in that assembly. In the parts only view of BOM you'll find all infos you need to order your parts. Export this BOM view to Excel and sort/filter the rows needed for order.

[Anonymous]

Hi,

thanks for the code! Sadly it's not opening my drawing 😞 It only shows the message box with the path

I will put all my laserparts in an assembly from now on and extract qty from there

[Ralf_Krieg · Accepted solution]

Hello

Ok, here's the complete one. Link this rule to your "Auf .idw platzieren" button. Your text field to enter the drawing name is obsolete now and can be removed.

Private Sub Main()
	'assume your laser part document is open and active
	
	If ThisApplication.Documents.Count=0 OrElse Not ThisApplication.ActiveDocumentType = DocumentTypeEnum.kPartDocumentObject Then
		MsgBox("This rule can only start with an part document active.", , "iLogic")
		Exit Sub
	End If
		
	Dim oPartDoc As PartDocument = ThisApplication.ActiveDocument

	Dim oDrawdoc As DrawingDocument = GetDrawing	
	
	If oDrawdoc Is Nothing Then
		MsgBox("Somethign went wrong getting selected drawing.", , "iLogic")
		Exit Sub
	End If
	
	'Call the rule with the drawing view creation
	Call CreateDrawingView(oDrawdoc, oPartDoc)
	
	MsgBox("Done",,"iLogic")
End Sub

Private Function GetDrawing() As DrawingDocument

Dim oFileDlg As Inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.Filter="Autodesk Inventor-Drawing (*.idw)|*.idw|All Files (*.*)|*.*"
oFileDlg.FilterIndex = 1
oFileDlg.DialogTitle = "Open Laser Part Drawing"
oFileDlg.CancelError = True
On Error Resume Next
Err.Clear 
	oFileDlg.ShowOpen()
If Not Err.Number = 0 Then
	Return Nothing
End If

Dim oDoc As Document
For Each oDoc In ThisApplication.Documents
	If oDoc.FullFileName = oFileDlg.FileName Then
		GetDrawing =oDoc
		Return GetDrawing
	End If
Next

GetDrawing=ThisApplication.Documents.Open(oFileDlg.FileName)

End Function


Private Sub CreateDrawingView(ByVal oDrawDoc As DrawingDocument, ByVal oPartDoc As PartDocument)
	
	Dim oActiveSheet As Sheet = oDrawDoc.ActiveSheet
	Dim oSheetSize As DrawingSheetSizeEnum = oActiveSheet.Size
	Dim oOrientation As PageOrientationTypeEnum = oActiveSheet.Orientation
	Dim sSheetName As String= System.IO.Path.GetFileNameWithoutExtension(oPartDoc.FullFileName)
	Dim oWidth As Object = oActiveSheet.Width
	Dim oHeight As Object=oActiveSheet.Height
	
	Dim oSheet As Sheet = oDrawDoc.Sheets.Add(oSheetSize, oOrientation, sSheetName, oWidth, oHeight)
	oSheet.AddTitleBlock(oActiveSheet.TitleBlock.Definition)
	oSheet.AddDefaultBorder()
	
	oSheet.Activate
	Dim oPoint As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oSheet.Width/2, oSheet.Height/2)
	
	oSheet.DrawingViews.AddBaseView(oPartDoc,oPoint,1,ViewOrientationTypeEnum.kFrontViewOrientation,DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle )

End Sub

[Anonymous]

Thank you!!