Number of bends of sheet metal part and direction
You can try this:
Dim doc As DrawingDocument = ThisDoc.Document
Dim sheet As Sheet = doc.ActiveSheet
Dim refDoc As PartDocument = sheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
Dim refDef As SheetMetalComponentDefinition = refDoc.ComponentDefinition
Dim flatPattern = refDef.FlatPattern
Dim ups = 0
Dim downs = 0
For Each result As FlatBendResult In flatPattern.FlatBendResults
If (result.IsOnBottomFace) Then Continue For
If (result.IsDirectionUp) Then
ups += 1
Else
downs += 1
End If
Next
Dim insertPoint = ThisApplication.TransientGeometry.CreatePoint2d(10, 10)
Dim headers = New String() {"Direction", "number"}
Dim table = sheet.CustomTables.Add("Bends", insertPoint, 2, 2, headers)
table.Rows.Item(1).Item(1).Value = "Up"
table.Rows.Item(1).Item(2).Value = ups
table.Rows.Item(2).Item(1).Value = "Down"
table.Rows.Item(2).Item(2).Value = downsJelte de Jong
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You also might want to have a look at my blog post: Automatically generate bend dimensions
Jelte de Jong
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try this:
Public Class ThisRule
Sub Main()
Dim doc As DrawingDocument = ThisDoc.Document
Dim sheet As Sheet = doc.ActiveSheet
Dim refDoc As Document = sheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
Dim infos As New List(Of DocumentInfo)
If (refDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject) Then
If (refDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then
infos.Add(New DocumentInfo(refDoc))
End If
Else
For Each assDoc As Document In refDoc.AllReferencedDocuments
If (assDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject) Then
If (assDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then
infos.Add(New DocumentInfo(assDoc))
End If
End If
Next
End If
If (infos.Count = 0) Then
MsgBox("No sheetmetal found.")
Return
End If
Dim insertPoint = ThisApplication.TransientGeometry.CreatePoint2d(10, 10)
Dim headers = New String() {"Part", "Size", "Up", "Down"}
Dim table = sheet.CustomTables.Add("Bends", insertPoint, headers.Length, infos.Count, headers)
For i = 1 To infos.Count
Dim row = table.Rows.Item(i)
Dim info = infos.Item(i - 1)
row.Item(1).Value = info.DisplayName
row.Item(2).Value = info.Size
row.Item(3).Value = info.Ups
row.Item(4).Value = info.Downs
Next
End Sub
End Class
Public Class DocumentInfo
Public Sub New(doc As PartDocument)
Dim uom = doc.UnitsOfMeasure
Dim def As SheetMetalComponentDefinition = doc.ComponentDefinition
Dim flatPattern = def.FlatPattern
For Each result As FlatBendResult In flatPattern.FlatBendResults
If (result.IsOnBottomFace) Then Continue For
If (result.IsDirectionUp) Then
Ups += 1
Else
Downs += 1
End If
Next
Dim width = uom.ConvertUnits(flatPattern.Width, UnitsTypeEnum.kDatabaseAngleUnits, UnitsTypeEnum.kDefaultDisplayAngleUnits)
Dim length = uom.ConvertUnits(flatPattern.Length, UnitsTypeEnum.kDatabaseAngleUnits, UnitsTypeEnum.kDefaultDisplayAngleUnits)
Size = String.Format("{0}x{1}", Math.Round(width, 5), Math.Round(length, 5))
DisplayName = doc.DisplayName
End Sub
Public Property Ups As Integer = 0
Public Property Downs As Integer = 0
Public Property Size As String
Public Property DisplayName As String
End ClassJelte de Jong
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Thanks A lot , it's working great , sorry for bothering you can the outputs be as custom property so I can added to existing table , below is snap for the table , thanks in advance.
This will fill the properties "ups" and "downs".
Public Sub main()
Dim doc As DrawingDocument = ThisDoc.Document
For Each refDoc As Document In doc.AllReferencedDocuments
If (refDoc.DocumentType <> DocumentTypeEnum.kPartDocumentObject) Then Continue For
If (refDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then Continue For
Dim def As SheetMetalComponentDefinition = refDoc.ComponentDefinition
If (Not def.HasFlatPattern) Then
def.Unfold()
End If
Dim flatPattern = def.FlatPattern
Dim ups = 0
Dim downs = 0
For Each result As FlatBendResult In flatPattern.FlatBendResults
If (result.IsOnBottomFace) Then Continue For
If (result.IsDirectionUp) Then
ups += 1
Else
downs += 1
End If
Next
SetCustomProperty(refDoc, "Ups", ups)
SetCustomProperty(refDoc, "Downs", downs)
Next
End Sub
Public Sub SetCustomProperty(doc As Document, name As String, value As String)
Dim propSet = doc.PropertySets.Item("Inventor User Defined Properties")
Try
propSet.Item(name).Value = value
Catch ex As Exception
propSet.Add(value, name)
End Try
End Sub
Jelte de Jong
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Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Blog: hjalte.nl - github.com
Hi @JelteDeJong thanks for your quick response , sorry for the confusion , is it possible to get how many sides has bend for example the below part has 4 edges so all edges will have 4 bends .
