Hello all,
I found a code to Save all sheetmetal parts from assembly to DXF. I make some changes to apear below the drawing parts, Material and thickness. But I whant to put the QTY also? Can I help me to make the necessary changes in the code?
Thanks in advance
Code:
Sub Main
'iLogic Code by Jhoel Forshav - originally posted at https://clintbrown.co.uk/ilogic-export-all-flat-patterns-to-one-dxf
'Check that the active document is an assembly file
If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then
MessageBox.Show("This rule can only run from an Assembly file", "DXF-creator", MessageBoxButtons.OK, MessageBoxIcon.Error)
Exit Sub
End If
'Dim the active document as AssemblyDocument
Dim oDoc As AssemblyDocument = ThisApplication.ActiveDocument
'Make sure the assembly is saved
If oDoc.FullFileName = ""
MessageBox.Show("Please save the Assembly before running this rule.", "DXF-creator", MessageBoxButtons.OK, MessageBoxIcon.Information)
Exit Sub
End If
'Get the assembly filename without extension
Dim oAsmName As String = System.IO.Path.GetFileNameWithoutExtension(oDoc.FullFileName)
'Get the assembly filepath
Dim oPath As String = System.IO.Path.GetDirectoryName(oDoc.FullFileName)
'Get the parts only BOM.
Dim oBOM As BOM = oDoc.ComponentDefinition.BOM
'Make sure Parts Only is activated
oBOM.PartsOnlyViewEnabled = True
'Parts only will be last BomView (difficult to get by name since it's different depending on your language)
Dim oBOMview As BOMView = oBOM.BOMViews.Item(oBOM.BOMViews.Count)
'Set a reference to the TransientGeometry object
Dim oTG As TransientGeometry = ThisApplication.TransientGeometry
'oX and oY will be used to create points for view placement
Dim oX As Double = 0
Dim oY As Double = 0
'Create the Baseview options to place flatpattern-views
Dim oBaseViewOptions As NameValueMap
oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap
oBaseViewOptions.Add("SheetMetalFoldedModel", False)
'Set a variable for the drawing document
Dim oDrawing As DrawingDocument
'Create a String to return a message if any SM-parts are not saved
Dim unsavedSmParts As String = ""
Dim i As Integer = 1
Dim oInfo As String = ""
'Traverse Parts Only BOM
For Each oRow As BOMRow In oBOMview.BOMRows
Try
'Get the component definition for the part
Dim oDef As ComponentDefinition = oRow.ComponentDefinitions(1)
'Check if the part is SheetMetal
If TypeOf (oDef) Is SheetMetalComponentDefinition
'Set a reference to the partdocument
Dim smPartDoc As PartDocument = oDef.Document
'Check if the part is saved
If smPartDoc.FullFileName = "" Then
If unsavedSmParts = "" Then unsavedSmParts = "The fallowing SM-documents were not saved and therefore " & _
"no drawingviews were created:" & vbCrLf
unsavedSmParts = unsavedSmParts & vbCrLf & oDef.Document.DisplayName
Continue For
End If
'Create flatpattern if it doesn't already exist
If Not oDef.HasFlatPattern
oDef.Unfold()
oDef.FlatPattern.ExitEdit()
End If
'Create the drawing if it doesn't already exist
If oDrawing Is Nothing
oDrawing = ThisApplication.Documents.Add(DocumentTypeEnum.kDrawingDocumentObject, _
, False)
'Set the drawings length units to the same as the assemblys length units
oDrawing.UnitsOfMeasure.LengthUnits = oDoc.UnitsOfMeasure.LengthUnits
End If
'Set a reference to the drawing sheet
Dim oSheet As Sheet = oDrawing.ActiveSheet
'Create the flatpattern view
Dim oView As DrawingView = oSheet.DrawingViews.AddBaseView(smPartDoc, oTG.CreatePoint2d(oX, oY), 1 _
, ViewOrientationTypeEnum.kDefaultViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle, _
"FlatPattern", , oBaseViewOptions)
oView.Name = smPartDoc.DisplayName & vbNewLine & "Espessura: " & smPartDoc.ComponentDefinition.Thickness.Expression _
& vbNewLine & "Material: " & smPartDoc.PropertySets("Design Tracking Properties")("Material").Value
oView.ShowLabel = True
'Set the position with our oX and oY
oView.Position = oTG.CreatePoint2d(oView.Position.X + oView.Width / 2, oView.Position.Y)
'Move oX to place the next view to the right of this one
oX = oView.Left + oView.Width + 1
'Remove the bend lines of the view
RemoveBendLines(oView, oDef.FlatPattern)'You could comment out this line to keep bend lines
oInfo = oInfo & "Here" & If (i = 1, "", vbCrLf) & i & ". " & smPartDoc.PropertySets.Item("Design Tracking Properties"). _
Item("Part Number").Value
i += 1
'Close the part
smPartDoc.Close(True)
End If
Catch Ex As Exception
MsgBox(Ex.Message)
End Try
Next
If oDrawing IsNot Nothing
'Create the save location string for the DXF
Dim oDXFName As String = oPath & "\" & oAsmName & "_FlatPatterns.dxf"
'Save the DXF
oINI = "C:\Users\LF\Desktop\Configuracoes Inventor LF\config Inventor\exportdxf.ini" 'Specify your INI file location here (eg C:\TEMP\DXF Export.ini)
If oINI = "" Then
MessageBox.Show("You need to specify an INI file location in the code - Look for oINI and set the path", "Error", MessageBoxButtons.OK, MessageBoxIcon.Error)
End If
SaveDXF(oDrawing, oDXFName, oINI)
'Create the save location string for the information txt
Dim oInfoName As String = oPath & "\" & oAsmName & "_FlatPatterns.txt"
'Create the txt
CreateTXT(oInfo, oInfoName)
End If
'Close the drawing
oDrawing.Close
'return information about any unsaved parts
If unsavedSmParts <> "" Then _
MessageBox.Show(unsavedSmParts, "Some parts were not saved", _
MessageBoxButtons.OK, MessageBoxIcon.Information)
'Update the assembly (could be dirty if any flatpatterns were created)
oDoc.Update
End Sub
Sub SaveDXF(oDrawing As DrawingDocument, oFileName As String, oIniFile As String)
'Set a reference to the DFX translator
Dim DXFAddIn As TranslatorAddIn
DXFAddIn = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}")
'Create translation context
Dim oContext As TranslationContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
'Create options for the translation
Dim oOptions As NameValueMap = ThisApplication.TransientObjects.CreateNameValueMap
'Create a DataMedium object
Dim oDataMedium As DataMedium = ThisApplication.TransientObjects.CreateDataMedium
'Set the options (which .ini-file to use)
If DXFAddIn.HasSaveCopyAsOptions(oDrawing, oContext, oOptions) Then
oOptions.Value("Export_Acad_IniFile") = oIniFile
End If
'Set the filename property of the DataMedium object
oDataMedium.FileName = oFileName
Try
'Try to save the DXF
DXFAddIn.SaveCopyAs(oDrawing, oContext, oOptions, oDataMedium)
MessageBox.Show("Dxf saved to: " & oFileName, "DXF SAVED", MessageBoxButtons.OK, MessageBoxIcon.Information)
Catch
MessageBox.Show("Couldn't save dxf!", "Error", MessageBoxButtons.OK, MessageBoxIcon.Error)
End Try
End Sub
Sub RemoveBendLines(oView As DrawingView, oFlattPattern As FlatPattern)
'Get all the bend edges from the FlatPattern
Dim oBendEdgesUp As Edges = oFlattPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendUpFlatPatternEdge)
Dim oBendEdgesDown As Edges = oFlattPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendDownFlatPatternEdge)
For Each oEdge As Edge In oBendEdgesUp
'Get the curves representing these edges in the drawing view
For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge)
For Each oSegment As DrawingCurveSegment In oCurve.Segments
'Set visibility to false
oSegment.Visible = False
Next
Next
Next
For Each oEdge As Edge In oBendEdgesDown
For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge)
For Each oSegment As DrawingCurveSegment In oCurve.Segments
oSegment.Visible = False
Next
Next
Next
End Sub
Sub CreateTXT(oText As String, oFileName As String)
Dim oTxtWriter As System.IO.StreamWriter = System.IO.File.CreateText(oFileName)
oTxtWriter.WriteLine(oText)
oTxtWriter.Close()
End Sub
Solved! Go to Solution.
Solved by JhoelForshav. Go to Solution.
Solved by JhoelForshav. Go to Solution.
Hi @Anonymous
I'm glad you found my code 😄
Try this to get the Qty as well.
Sub Main 'iLogic Code by Jhoel Forshav - originally posted at https://clintbrown.co.uk/ilogic-export-all-flat-patterns-to-one-dxf 'Check that the active document is an assembly file If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then MessageBox.Show("This rule can only run from an Assembly file", "DXF-creator", MessageBoxButtons.OK, MessageBoxIcon.Error) Exit Sub End If 'Dim the active document as AssemblyDocument Dim oDoc As AssemblyDocument = ThisApplication.ActiveDocument 'Make sure the assembly is saved If oDoc.FullFileName = "" MessageBox.Show("Please save the Assembly before running this rule.", "DXF-creator", MessageBoxButtons.OK, MessageBoxIcon.Information) Exit Sub End If 'Get the assembly filename without extension Dim oAsmName As String = System.IO.Path.GetFileNameWithoutExtension(oDoc.FullFileName) 'Get the assembly filepath Dim oPath As String = System.IO.Path.GetDirectoryName(oDoc.FullFileName) 'Get the parts only BOM. Dim oBOM As BOM = oDoc.ComponentDefinition.BOM 'Make sure Parts Only is activated oBOM.PartsOnlyViewEnabled = True 'Parts only will be last BomView (difficult to get by name since it's different depending on your language) Dim oBOMview As BOMView = oBOM.BOMViews.Item(oBOM.BOMViews.Count) 'Set a reference to the TransientGeometry object Dim oTG As TransientGeometry = ThisApplication.TransientGeometry 'oX and oY will be used to create points for view placement Dim oX As Double = 0 Dim oY As Double = 0 'Create the Baseview options to place flatpattern-views Dim oBaseViewOptions As NameValueMap oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap oBaseViewOptions.Add("SheetMetalFoldedModel", False) 'Set a variable for the drawing document Dim oDrawing As DrawingDocument 'Create a String to return a message if any SM-parts are not saved Dim unsavedSmParts As String = "" Dim i As Integer = 1 Dim oInfo As String = "" 'Traverse Parts Only BOM For Each oRow As BOMRow In oBOMview.BOMRows Try 'Get the component definition for the part Dim oDef As ComponentDefinition = oRow.ComponentDefinitions(1) 'Check if the part is SheetMetal If TypeOf (oDef) Is SheetMetalComponentDefinition 'Set a reference to the partdocument Dim smPartDoc As PartDocument = oDef.Document 'Check if the part is saved If smPartDoc.FullFileName = "" Then If unsavedSmParts = "" Then unsavedSmParts = "The fallowing SM-documents were not saved and therefore " & _ "no drawingviews were created:" & vbCrLf unsavedSmParts = unsavedSmParts & vbCrLf & oDef.Document.DisplayName Continue For End If 'Create flatpattern if it doesn't already exist If Not oDef.HasFlatPattern oDef.Unfold() oDef.FlatPattern.ExitEdit() End If 'Create the drawing if it doesn't already exist If oDrawing Is Nothing oDrawing = ThisApplication.Documents.Add(DocumentTypeEnum.kDrawingDocumentObject, _ , False) 'Set the drawings length units to the same as the assemblys length units oDrawing.UnitsOfMeasure.LengthUnits = oDoc.UnitsOfMeasure.LengthUnits End If 'Set a reference to the drawing sheet Dim oSheet As Sheet = oDrawing.ActiveSheet 'Create the flatpattern view Dim oView As DrawingView = oSheet.DrawingViews.AddBaseView(smPartDoc, oTG.CreatePoint2d(oX, oY), 1 _ , ViewOrientationTypeEnum.kDefaultViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle, _ "FlatPattern", , oBaseViewOptions) oView.Name = smPartDoc.DisplayName & vbNewLine & "Espessura: " & smPartDoc.ComponentDefinition.Thickness.Expression _ & vbNewLine & "Material: " & smPartDoc.PropertySets("Design Tracking Properties")("Material").Value & _ vbCrLf & "Quantity: " & oDoc.ComponentDefinition.Occurrences.AllReferencedOccurrences(smPartDoc).Count oView.ShowLabel = True 'Set the position with our oX and oY oView.Position = oTG.CreatePoint2d(oView.Position.X + oView.Width / 2, oView.Position.Y) 'Move oX to place the next view to the right of this one oX = oView.Left + oView.Width + 1 'Remove the bend lines of the view RemoveBendLines(oView, oDef.FlatPattern)'You could comment out this line to keep bend lines oInfo = oInfo & "Here" & If (i = 1, "", vbCrLf) & i & ". " & smPartDoc.PropertySets.Item("Design Tracking Properties"). _ Item("Part Number").Value i += 1 'Close the part smPartDoc.Close(True) End If Catch Ex As Exception MsgBox(Ex.Message) End Try Next If oDrawing IsNot Nothing 'Create the save location string for the DXF Dim oDXFName As String = oPath & "\" & oAsmName & "_FlatPatterns.dxf" 'Save the DXF oINI = "C:\Users\LF\Desktop\Configuracoes Inventor LF\config Inventor\exportdxf.ini" 'Specify your INI file location here (eg C:\TEMP\DXF Export.ini) If oINI = "" Then MessageBox.Show("You need to specify an INI file location in the code - Look for oINI and set the path", "Error", MessageBoxButtons.OK, MessageBoxIcon.Error) End If SaveDXF(oDrawing, oDXFName, oINI) 'Create the save location string for the information txt Dim oInfoName As String = oPath & "\" & oAsmName & "_FlatPatterns.txt" 'Create the txt CreateTXT(oInfo, oInfoName) End If 'Close the drawing oDrawing.Close 'return information about any unsaved parts If unsavedSmParts <> "" Then _ MessageBox.Show(unsavedSmParts, "Some parts were not saved", _ MessageBoxButtons.OK, MessageBoxIcon.Information) 'Update the assembly (could be dirty if any flatpatterns were created) oDoc.Update End Sub Sub SaveDXF(oDrawing As DrawingDocument, oFileName As String, oIniFile As String) 'Set a reference to the DFX translator Dim DXFAddIn As TranslatorAddIn DXFAddIn = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}") 'Create translation context Dim oContext As TranslationContext = ThisApplication.TransientObjects.CreateTranslationContext oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism 'Create options for the translation Dim oOptions As NameValueMap = ThisApplication.TransientObjects.CreateNameValueMap 'Create a DataMedium object Dim oDataMedium As DataMedium = ThisApplication.TransientObjects.CreateDataMedium 'Set the options (which .ini-file to use) If DXFAddIn.HasSaveCopyAsOptions(oDrawing, oContext, oOptions) Then oOptions.Value("Export_Acad_IniFile") = oIniFile End If 'Set the filename property of the DataMedium object oDataMedium.FileName = oFileName Try 'Try to save the DXF DXFAddIn.SaveCopyAs(oDrawing, oContext, oOptions, oDataMedium) MessageBox.Show("Dxf saved to: " & oFileName, "DXF SAVED", MessageBoxButtons.OK, MessageBoxIcon.Information) Catch MessageBox.Show("Couldn't save dxf!", "Error", MessageBoxButtons.OK, MessageBoxIcon.Error) End Try End Sub Sub RemoveBendLines(oView As DrawingView, oFlattPattern As FlatPattern) 'Get all the bend edges from the FlatPattern Dim oBendEdgesUp As Edges = oFlattPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendUpFlatPatternEdge) Dim oBendEdgesDown As Edges = oFlattPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendDownFlatPatternEdge) For Each oEdge As Edge In oBendEdgesUp 'Get the curves representing these edges in the drawing view For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge) For Each oSegment As DrawingCurveSegment In oCurve.Segments 'Set visibility to false oSegment.Visible = False Next Next Next For Each oEdge As Edge In oBendEdgesDown For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge) For Each oSegment As DrawingCurveSegment In oCurve.Segments oSegment.Visible = False Next Next Next End Sub Sub CreateTXT(oText As String, oFileName As String) Dim oTxtWriter As System.IO.StreamWriter = System.IO.File.CreateText(oFileName) oTxtWriter.WriteLine(oText) oTxtWriter.Close() End Sub
Jhoel Forshav
Download my free Inventor Addin - Hole Projector
LinkedIn | Ideas | Contributions | Blog posts | Website
First of all, thanks for your contribution and your site, help me a lot.
The code works perfectly.
Thanks, one more time.
Thanks @JhoelForshav can the rule write that quantity material and thickness in the txt file
Sure, @Anonymous
This should do it 🙂
Sub Main 'iLogic Code by Jhoel Forshav - originally posted at https://clintbrown.co.uk/ilogic-export-all-flat-patterns-to-one-dxf 'Check that the active document is an assembly file If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then MessageBox.Show("This rule can only run from an Assembly file", "DXF-creator", MessageBoxButtons.OK, MessageBoxIcon.Error) Exit Sub End If 'Dim the active document as AssemblyDocument Dim oDoc As AssemblyDocument = ThisApplication.ActiveDocument 'Make sure the assembly is saved If oDoc.FullFileName = "" MessageBox.Show("Please save the Assembly before running this rule.", "DXF-creator", MessageBoxButtons.OK, MessageBoxIcon.Information) Exit Sub End If 'Get the assembly filename without extension Dim oAsmName As String = System.IO.Path.GetFileNameWithoutExtension(oDoc.FullFileName) 'Get the assembly filepath Dim oPath As String = System.IO.Path.GetDirectoryName(oDoc.FullFileName) 'Get the parts only BOM. Dim oBOM As BOM = oDoc.ComponentDefinition.BOM 'Make sure Parts Only is activated oBOM.PartsOnlyViewEnabled = True 'Parts only will be last BomView (difficult to get by name since it's different depending on your language) Dim oBOMview As BOMView = oBOM.BOMViews.Item(oBOM.BOMViews.Count) 'Set a reference to the TransientGeometry object Dim oTG As TransientGeometry = ThisApplication.TransientGeometry 'oX and oY will be used to create points for view placement Dim oX As Double = 0 Dim oY As Double = 0 'Create the Baseview options to place flatpattern-views Dim oBaseViewOptions As NameValueMap oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap oBaseViewOptions.Add("SheetMetalFoldedModel", False) 'Set a variable for the drawing document Dim oDrawing As DrawingDocument 'Create a String to return a message if any SM-parts are not saved Dim unsavedSmParts As String = "" Dim i As Integer = 1 Dim oInfo As String = "" 'Traverse Parts Only BOM For Each oRow As BOMRow In oBOMview.BOMRows Try 'Get the component definition for the part Dim oDef As ComponentDefinition = oRow.ComponentDefinitions(1) 'Check if the part is SheetMetal If TypeOf (oDef) Is SheetMetalComponentDefinition 'Set a reference to the partdocument Dim smPartDoc As PartDocument = oDef.Document 'Check if the part is saved If smPartDoc.FullFileName = "" Then If unsavedSmParts = "" Then unsavedSmParts = "The fallowing SM-documents were not saved and therefore " & _ "no drawingviews were created:" & vbCrLf unsavedSmParts = unsavedSmParts & vbCrLf & oDef.Document.DisplayName Continue For End If 'Create flatpattern if it doesn't already exist If Not oDef.HasFlatPattern oDef.Unfold() oDef.FlatPattern.ExitEdit() End If 'Create the drawing if it doesn't already exist If oDrawing Is Nothing oDrawing = ThisApplication.Documents.Add(DocumentTypeEnum.kDrawingDocumentObject, _ , False) 'Set the drawings length units to the same as the assemblys length units oDrawing.UnitsOfMeasure.LengthUnits = oDoc.UnitsOfMeasure.LengthUnits End If 'Set a reference to the drawing sheet Dim oSheet As Sheet = oDrawing.ActiveSheet 'Create the flatpattern view Dim oView As DrawingView = oSheet.DrawingViews.AddBaseView(smPartDoc, oTG.CreatePoint2d(oX, oY), 1 _ , ViewOrientationTypeEnum.kDefaultViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle, _ "FlatPattern", , oBaseViewOptions) oView.Name = smPartDoc.DisplayName & vbNewLine & "Thickness: " & smPartDoc.ComponentDefinition.Thickness.Expression _ & vbNewLine & "Material: " & smPartDoc.PropertySets("Design Tracking Properties")("Material").Value & _ vbCrLf & "Quantity: " & oDoc.ComponentDefinition.Occurrences.AllReferencedOccurrences(smPartDoc).Count oView.ShowLabel = True 'Set the position with our oX and oY oView.Position = oTG.CreatePoint2d(oView.Position.X + oView.Width / 2, oView.Position.Y) 'Move oX to place the next view to the right of this one oX = oView.Left + oView.Width + 1 'Remove the bend lines of the view RemoveBendLines(oView, oDef.FlatPattern)'You could comment out this line to keep bend lines oInfo = oInfo & If (i = 1, "", vbCrLf) & i & ". " & smPartDoc.PropertySets.Item("Design Tracking Properties"). _ Item("Part Number").Value & " - Thickness: " & oDef.Thickness.Expression & " - Material: " _ & smPartDoc.PropertySets("Design Tracking Properties")("Material").Value & " - Quantity: " & _ oDoc.ComponentDefinition.Occurrences.AllReferencedOccurrences(smPartDoc).Count i += 1 'Close the part smPartDoc.Close(True) End If Catch Ex As Exception MsgBox(Ex.Message) End Try Next If oDrawing IsNot Nothing 'Create the save location string for the DXF Dim oDXFName As String = oPath & "\" & oAsmName & "_FlatPatterns.dxf" 'Save the DXF oINI = "C:\TEMP\INI.ini" 'Specify your INI file location here (eg C:\TEMP\DXF Export.ini) If oINI = "" Then MessageBox.Show("You need to specify an INI file location in the code - Look for oINI and set the path", "Error", MessageBoxButtons.OK, MessageBoxIcon.Error) End If SaveDXF(oDrawing, oDXFName, oINI) 'Create the save location string for the information txt Dim oInfoName As String = oPath & "\" & oAsmName & "_FlatPatterns.txt" 'Create the txt CreateTXT(oInfo, oInfoName) End If 'Close the drawing oDrawing.Close 'return information about any unsaved parts If unsavedSmParts <> "" Then _ MessageBox.Show(unsavedSmParts, "Some parts were not saved", _ MessageBoxButtons.OK, MessageBoxIcon.Information) 'Update the assembly (could be dirty if any flatpatterns were created) oDoc.Update End Sub Sub SaveDXF(oDrawing As DrawingDocument, oFileName As String, oIniFile As String) 'Set a reference to the DFX translator Dim DXFAddIn As TranslatorAddIn DXFAddIn = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}") 'Create translation context Dim oContext As TranslationContext = ThisApplication.TransientObjects.CreateTranslationContext oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism 'Create options for the translation Dim oOptions As NameValueMap = ThisApplication.TransientObjects.CreateNameValueMap 'Create a DataMedium object Dim oDataMedium As DataMedium = ThisApplication.TransientObjects.CreateDataMedium 'Set the options (which .ini-file to use) If DXFAddIn.HasSaveCopyAsOptions(oDrawing, oContext, oOptions) Then oOptions.Value("Export_Acad_IniFile") = oIniFile End If 'Set the filename property of the DataMedium object oDataMedium.FileName = oFileName Try 'Try to save the DXF DXFAddIn.SaveCopyAs(oDrawing, oContext, oOptions, oDataMedium) MessageBox.Show("Dxf saved to: " & oFileName, "DXF SAVED", MessageBoxButtons.OK, MessageBoxIcon.Information) Catch MessageBox.Show("Couldn't save dxf!", "Error", MessageBoxButtons.OK, MessageBoxIcon.Error) End Try End Sub Sub RemoveBendLines(oView As DrawingView, oFlattPattern As FlatPattern) 'Get all the bend edges from the FlatPattern Dim oBendEdgesUp As Edges = oFlattPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendUpFlatPatternEdge) Dim oBendEdgesDown As Edges = oFlattPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendDownFlatPatternEdge) For Each oEdge As Edge In oBendEdgesUp 'Get the curves representing these edges in the drawing view For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge) For Each oSegment As DrawingCurveSegment In oCurve.Segments 'Set visibility to false oSegment.Visible = False Next Next Next For Each oEdge As Edge In oBendEdgesDown For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge) For Each oSegment As DrawingCurveSegment In oCurve.Segments oSegment.Visible = False Next Next Next End Sub Sub CreateTXT(oText As String, oFileName As String) Dim oTxtWriter As System.IO.StreamWriter = System.IO.File.CreateText(oFileName) oTxtWriter.WriteLine(oText) oTxtWriter.Close() End Sub
Jhoel Forshav
Download my free Inventor Addin - Hole Projector
LinkedIn | Ideas | Contributions | Blog posts | Website
Was trying to use your code, (wonderful concept by the way) and I'm running into the Couldn't save dxf! error. Any ideas on how I fix this? I'm currently just testing it on a small assembly with 4 sheet metal parts (no formed parts yet). I'm running Inventor 2020. I tried diagnosing it myself, but I am severely lacking in ilogic knowledge. Any advice is greatly appreciated.
Hello,
You need to specify an INI file location in the code first!
If you have not "extracted" the .INI file jet, follow the instructions in the link below.
iLogic: Export All Flat Patterns To One DXF – Clint Brown
Hey guys, I've stumbled across this thread while trying to figure out how to remove/turn off the bend lines on views in an IDW. Bend lines currently come through in profile drawings and we usually have a separate drawing for the folding of any profiled parts; the goal is to only have the information for cutting on the profile drawing.
This is what I've managed to get so far from reusing parts of Jhoel's code above, but it seems to struggle accessing the flat pattern. Looks like lines 6 and 15/16 are causing issues. Any ideas on where I've gone wrong?
Thanks in advance!
Dim oDrawDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Sheet
Dim oView As DrawingView
Dim oViews As DrawingViews
Dim oDef As ComponentDefinition
Dim oFlatPattern As FlatPattern
oSheet = oDrawDoc.ActiveSheet
oViews = oSheet.DrawingViews
For Each oView In oViews
''Remove the bend lines of the view
'RemoveBendLines(oView, oDef.FlatPattern)'You could comment out this line to keep bend lines
'Get all the bend edges from the FlatPattern
Dim oBendEdgesUp As Edges = oFlatPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendUpFlatPatternEdge)
Dim oBendEdgesDown As Edges = oFlatPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendDownFlatPatternEdge)
For Each oEdge As Edge In oBendEdgesUp
'Get the curves representing these edges in the drawing view
For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge)
For Each oSegment As DrawingCurveSegment In oCurve.Segments
'Set visibility to false
oSegment.Visible = False
Next
Next
Next
For Each oEdge As Edge In oBendEdgesDown
For Each oCurve As DrawingCurve In oView.DrawingCurves(oEdge)
For Each oSegment As DrawingCurveSegment In oCurve.Segments
oSegment.Visible = False
Next
Next
Next
Next
@StuartRoodt You may want to start a new post and reference this one. I don't think you'll get much help on a solved forum.
Olá @JhoelForshav :).
I have a question.
Do You have maybe a solution how to change the code so that all components could be separately saved as DXF?
Thanks in advance 😊.
I asked for a solution and got one if you are stil interested.
Solved: Re: ilogic batch create flat pattern to individual dxf - Autodesk Community - Inventor
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