I need to be generate a Lofted Flanges (AddLoftedFlange) in Solid Edge's Sheet Metal environment. The documentation simply does not give enough information as to what the parameters are.

I have been able to generate a Lofted Protrution (AddLoftedProtrution) in the Part environment. Most of the parameters are similar.

Can someone help me with a working example of the AddLoftedFlange method?

 

 

Here is the code the DOESN'T work...

____________
Imports SolidEdgeConstants
Imports System.Runtime.InteropServices

Module Module1
Sub Main()
Dim objApplication As SolidEdgeFramework.Application = Nothing
Dim objDocuments As SolidEdgeFramework.Documents = Nothing
Dim objSheetMetal As SolidEdgePart.SheetMetalDocument = Nothing
Dim objSketches As SolidEdgePart.Sketchs = Nothing
Dim objSketch As SolidEdgePart.Sketch = Nothing
Dim objProfiles As SolidEdgePart.Profiles = Nothing
Dim objProfile1 As SolidEdgePart.Profile = Nothing
Dim objProfile2 As SolidEdgePart.Profile = Nothing
Dim objRefplanes As SolidEdgePart.RefPlanes = Nothing
Dim objRefplane4 As SolidEdgePart.RefPlane = Nothing
Dim objRefplane5 As SolidEdgePart.RefPlane = Nothing
Dim objRelations2d As SolidEdgeFrameworkSupport.Relations2d = Nothing
Dim objRelation2d As SolidEdgeFrameworkSupport.Relation2d = Nothing
Dim objLines2d As SolidEdgeFrameworkSupport.Lines2d = Nothing
Dim objLine2d As SolidEdgeFrameworkSupport.Line2d = Nothing
Dim objModels As SolidEdgePart.Models = Nothing
Dim objModel As SolidEdgePart.Model = Nothing
Dim objCSArray(0 To 1) As SolidEdgePart.Profile
Dim lngCSTypeArray(0 To 1) As Long
Dim objOrigins(0 To 1) As Object
Dim dblOrigin(0 To 1) As Double

Dim X1 As Double = 0
Dim Y1 As Double = 0
Dim X2 As Double = 0.2
Dim Y2 As Double = 0.2

Try
' Connect to a running instance of Solid Edge
objApplication = Marshal.GetActiveObject("SolidEdge.Application")
' Get a reference to the documents collection
objDocuments = objApplication.Documents
' Create a new sheet metal document
objSheetMetal = objDocuments.Add("SolidEdge.SheetMetalDocument")
' Get a reference to the reference planes collection
objRefplanes = objSheetMetal.RefPlanes
' Add a reference plane
objRefplane4 = objRefplanes.AddParallelByDistance(objRefplanes(1), 0, SolidEdgePart.ReferenceElementConstants.igNormalSide, , , False)
' Get a reference to the sketches collection
objSketches = objSheetMetal.Sketches
' Add a new sketch
objSketch = objSketches.Add()
' Get a reference to the sketch's profiles collection
objProfiles = objSketch.Profiles
' Add a new profile
objProfile1 = objProfiles.Add(objRefplane4)
' Get a reference to the lines2d collection
objLines2d = objProfile1.Lines2d
' Draw a profile
objLine2d = objLines2d.AddBy2Points(X1, Y1, X2, Y2)
' Show the profile
objProfile1.Visible = True

' Add a reference plane
objRefplane5 = objRefplanes.AddParallelByDistance(objRefplanes(1), 0.2, SolidEdgePart.ReferenceElementConstants.igNormalSide, , , False)
' Add a new sketch
objSketch = objSketches.Add()
' Get a reference to the sketch's profiles collection
objProfiles = objSketch.Profiles
' Add a new profile
objProfile2 = objProfiles.Add(objRefplane5)
' Get a reference to the lines2d collection
objLines2d = objProfile2.Lines2d
' Draw the Base Profile
objLine2d = objLines2d.AddBy2Points(X1, Y1, X2, Y2)
' Show the profile
objProfile2.Visible = True

' Get a reference to the models collection
objModels = objSheetMetal.Models
' Create the lofted flange

dblOrigin(0) = X1
dblOrigin(1) = Y1
objOrigins(0) = dblOrigin

dblOrigin(0) = X1
dblOrigin(1) = Y1
objOrigins(1) = dblOrigin

objCSArray(0) = objProfile1
objCSArray(1) = objProfile2

lngCSTypeArray(0) = SolidEdgePart.FeaturePropertyConstants.igProfileBasedCrossSection
lngCSTypeArray(1) = SolidEdgePart.FeaturePropertyConstants.igProfileBasedCrossSection

objModel = objModels.AddLoftedFlange(NumSections:=2, _
                                                 CrossSections:=objCSArray, _
                                                 CrossSectionTypes:=lngCSTypeArray, _
                                                 Origins:=objOrigins, _
                                                 OriginRefs:=0, _
                                                 ThicknessSide:=SolidEdgePart.FeaturePropertyConstants.igLeft, _
                                                 varRadius:=0.01, _
                                                 varNeutralFactor:=0.5, _
                                                 varBnParamType:=SolidEdgePart.FeaturePropertyConstants.igNFType)


Catch ex As Exception
Console.WriteLine(ex.Message)
Finally
For x As Integer = 0 To 1
If Not (objCSArray(x) Is Nothing) Then
Marshal.ReleaseComObject(objCSArray(x))
objCSArray(x) = Nothing
End If
If Not (objOrigins(x) Is Nothing) Then
objOrigins(x) = Nothing
End If
Next

If Not (objModel Is Nothing) Then
Marshal.ReleaseComObject(objModel)
objModel = Nothing
End If
If Not (objModels Is Nothing) Then
Marshal.ReleaseComObject(objModels)
objModels = Nothing
End If
If Not (objRelations2d Is Nothing) Then
Marshal.ReleaseComObject(objRelations2d)
objRelations2d = Nothing
End If
If Not (objLine2d Is Nothing) Then
Marshal.ReleaseComObject(objLine2d)
objLine2d = Nothing
End If
If Not (objLines2d Is Nothing) Then
Marshal.ReleaseComObject(objLines2d)
objLines2d = Nothing
End If
If Not (objRelation2d Is Nothing) Then
Marshal.ReleaseComObject(objRelation2d)
objRelation2d = Nothing
End If
If Not (objRefplanes Is Nothing) Then
Marshal.ReleaseComObject(objRefplanes)
objRefplanes = Nothing
End If
If Not (objRefplane4 Is Nothing) Then
Marshal.ReleaseComObject(objRefplane4)
objProfile1 = Nothing
End If
If Not (objRefplane5 Is Nothing) Then
Marshal.ReleaseComObject(objRefplane5)
objProfile1 = Nothing
End If
If Not (objProfiles Is Nothing) Then
Marshal.ReleaseComObject(objProfiles)
objProfiles = Nothing
End If
If Not (objProfile1 Is Nothing) Then
Marshal.ReleaseComObject(objProfile1)
objProfile1 = Nothing
End If
If Not (objProfile2 Is Nothing) Then
Marshal.ReleaseComObject(objProfile2)
objProfile1 = Nothing
End If
If Not (objProfiles Is Nothing) Then
Marshal.ReleaseComObject(objProfiles)
objProfiles = Nothing
End If
If Not (objSketch Is Nothing) Then
Marshal.ReleaseComObject(objSketch)
objSketch = Nothing
End If
If Not (objSketches Is Nothing) Then
Marshal.ReleaseComObject(objSketches)
objSketches = Nothing
End If
If Not (objSheetMetal Is Nothing) Then
Marshal.ReleaseComObject(objSheetMetal)
objSheetMetal = Nothing
End If
If Not (objDocuments Is Nothing) Then
Marshal.ReleaseComObject(objDocuments)
objDocuments = Nothing
End If
If Not (objApplication Is Nothing) Then
Marshal.ReleaseComObject(objApplication)
objApplication = Nothing
End If
End Try
End Sub
End Module

____________
Here is the message:
The server threw an exception. (Exception from HRESULT: 0x80010105 (RPC_E_SERVER
FAULT))

Thanks,
Curt

Here is the code for AddLoftedProtution in Solid Edge Part. This DOES work. I am posting it because the parameters are very similar to the AddLoftedFlange in SheetMetal.

__________
Imports SolidEdgeConstants
Imports System.Runtime.InteropServices

Module Module1
Sub Main()
Dim objApplication As SolidEdgeFramework.Application = Nothing
Dim objDocuments As SolidEdgeFramework.Documents = Nothing
Dim objPart As SolidEdgePart.PartDocument = Nothing
Dim objSketches As SolidEdgePart.Sketchs = Nothing
Dim objSketch As SolidEdgePart.Sketch = Nothing
'Dim objProfileSets As SolidEdgePart.ProfileSets = Nothing
'Dim objProfileSet As SolidEdgePart.ProfileSet = Nothing
Dim objProfiles As SolidEdgePart.Profiles = Nothing
Dim objProfile1 As SolidEdgePart.Profile = Nothing
Dim objProfile2 As SolidEdgePart.Profile = Nothing
Dim objRefplanes As SolidEdgePart.RefPlanes = Nothing
Dim objRefplane4 As SolidEdgePart.RefPlane = Nothing
Dim objRefplane5 As SolidEdgePart.RefPlane = Nothing
Dim objRelations2d As SolidEdgeFrameworkSupport.Relations2d = Nothing
Dim objRelation2d As SolidEdgeFrameworkSupport.Relation2d = Nothing
Dim objLines2d As SolidEdgeFrameworkSupport.Lines2d = Nothing
Dim objLine2d As SolidEdgeFrameworkSupport.Line2d = Nothing
Dim objModels As SolidEdgePart.Models = Nothing
Dim objModel As SolidEdgePart.Model = Nothing
Dim objCSArray(0 To 1) As SolidEdgePart.Profile
Dim lngCSTypeArray(0 To 1) As Long
Dim objOrigins(0 To 1) As Object
Dim dblOrigin(0 To 1) As Double

Dim X1 As Double = 0.1
Dim Y1 As Double = 0.1
Dim X2 As Double = 0.4
Dim Y2 As Double = 0.2
Dim X3 As Double = 0.3
Dim Y3 As Double = 0.5
Dim X4 As Double = 0.0
Dim Y4 As Double = 0.6

Try
' Connect to a running instance of Solid Edge
objApplication = Marshal.GetActiveObject("SolidEdge.Application")
' Get a reference to the documents collection
objDocuments = objApplication.Documents
' Create a new part document
objPart = objDocuments.Add("SolidEdge.partDocument")
' Get a reference to the sketches collection
objSketches = objPart.Sketches
' Add a new sketch
objSketch = objSketches.Add()
' Get a reference to the profiles collection
objProfiles = objSketch.Profiles ' objProfileSet.Profiles
' Get a reference to the ref planes collection
objRefplanes = objPart.RefPlanes
' Add a new profile
objProfile1 = objProfiles.Add(objRefplanes.Item(3))
' Get a reference to the lines2d collection
objLines2d = objProfile1.Lines2d
' Draw the Base Profile
objLine2d = objLines2d.AddBy2Points(X1, Y1, X2, Y2)
objLine2d = objLines2d.AddBy2Points(X2, Y2, X3, Y3)
objLine2d = objLines2d.AddBy2Points(X3, Y3, X4, Y4)
objLine2d = objLines2d.AddBy2Points(X4, Y4, X1, Y1)
' Define Relations among the Line objects to make the Profile closed
objRelations2d = objProfile1.Relations2d
objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(1), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(2), _
KeypointIndexConstants.igLineStart)
objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(2), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(3), _
KeypointIndexConstants.igLineStart)
objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(3), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(4), _
KeypointIndexConstants.igLineStart)
objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(4), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(1), _
KeypointIndexConstants.igLineStart)
' Close the profile
objProfile1.End(SolidEdgePart.ProfileValidationType.igProfileClosed)
' Show the profile
objProfile1.Visible = True
'Add a new sketch
objSketch = objSketches.Add()
' Get a reference to the profiles collection
objProfiles = objSketch.Profiles ' objProfileSet.Profiles
' Add a new reference plane
objRefplane5 = objRefplanes.AddParallelByDistance(objRefplanes.Item(3), 0.25, SolidEdgePart.ReferenceElementConstants.igNormalSide, , , False)
' Add a new profile
objProfile2 = objProfiles.Add(objRefplane5)
' Get a reference to the lines2d collection
objLines2d = objProfile2.Lines2d
' Draw the Profile
objLine2d = objLines2d.AddBy2Points(X1, Y1, X2, Y2)
objLine2d = objLines2d.AddBy2Points(X2, Y2, X3, Y3)
objLine2d = objLines2d.AddBy2Points(X3, Y3, X4, Y4)
objLine2d = objLines2d.AddBy2Points(X4, Y4, X1, Y1)

' Define Relations among the Line objects to make the Profile closed
objRelations2d = objProfile2.Relations2d

objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(1), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(2), _
KeypointIndexConstants.igLineStart)

objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(2), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(3), _
KeypointIndexConstants.igLineStart)

objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(3), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(4), _
KeypointIndexConstants.igLineStart)

objRelation2d = objRelations2d.AddKeypoint( _
objLines2d.Item(4), _
KeypointIndexConstants.igLineEnd, _
objLines2d.Item(1), _
KeypointIndexConstants.igLineStart)

objProfile2.End( _
SolidEdgePart.ProfileValidationType.igProfileClosed)

' Show the profile
objProfile2.Visible = True

' Get a reference to the models collection
objModels = objPart.Models

' Create the lofted protrusion.

dblOrigin(0) = X1
dblOrigin(1) = Y1
objOrigins(0) = dblOrigin

dblOrigin(0) = X1
dblOrigin(1) = Y1
objOrigins(1) = dblOrigin

objCSArray(0) = objProfile1
objCSArray(1) = objProfile2

lngCSTypeArray(0) = SolidEdgePart.FeaturePropertyConstants.igProfileBasedCrossSection
lngCSTypeArray(1) = SolidEdgePart.FeaturePropertyConstants.igProfileBasedCrossSection

objModel = objModels.AddLoftedProtrusion(NumSections:=2, _
CrossSections:=objCSArray, _
CrossSectionTypes:=lngCSTypeArray, _
Origins:=objOrigins, _
SegmentMaps:=0, _
MaterialSide:=SolidEdgePart.FeaturePropertyConstants.igLeft, _
StartExtentType:=SolidEdgePart.FeaturePropertyConstants.igNone, _
StartExtentDistance:=0, _
StartSurfaceOrRefPlane:=Nothing, _
EndExtentType:=SolidEdgePart.FeaturePropertyConstants.igNone, _
EndExtentDistance:=0, _
EndSurfaceOrRefPlane:=Nothing, _
StartTangentType:=SolidEdgePart.FeaturePropertyConstants.igNone, _
StartTangentMagnitude:=0, _
EndTangentType:=SolidEdgePart.FeaturePropertyConstants.igNone, _
EndTangentMagnitude:=0)



Catch ex As Exception
Console.WriteLine(ex.Message)
Finally
For x As Integer = 0 To 1
If Not (objCSArray(x) Is Nothing) Then
Marshal.ReleaseComObject(objCSArray(x))
objCSArray(x) = Nothing
End If
If Not (objOrigins(x) Is Nothing) Then
objOrigins(x) = Nothing
End If
Next

If Not (objModel Is Nothing) Then
Marshal.ReleaseComObject(objModel)
objModel = Nothing
End If
If Not (objModels Is Nothing) Then
Marshal.ReleaseComObject(objModels)
objModels = Nothing
End If
If Not (objRelations2d Is Nothing) Then
Marshal.ReleaseComObject(objRelations2d)
objRelations2d = Nothing
End If
If Not (objLine2d Is Nothing) Then
Marshal.ReleaseComObject(objLine2d)
objLine2d = Nothing
End If
If Not (objLines2d Is Nothing) Then
Marshal.ReleaseComObject(objLines2d)
objLines2d = Nothing
End If
If Not (objRelation2d Is Nothing) Then
Marshal.ReleaseComObject(objRelation2d)
objRelation2d = Nothing
End If
If Not (objRefplanes Is Nothing) Then
Marshal.ReleaseComObject(objRefplanes)
objRefplanes = Nothing
End If
If Not (objRefplane4 Is Nothing) Then
Marshal.ReleaseComObject(objRefplane4)
objProfile1 = Nothing
End If
If Not (objRefplane5 Is Nothing) Then
Marshal.ReleaseComObject(objRefplane5)
objProfile1 = Nothing
End If
If Not (objProfiles Is Nothing) Then
Marshal.ReleaseComObject(objProfiles)
objProfiles = Nothing
End If
If Not (objProfile1 Is Nothing) Then
Marshal.ReleaseComObject(objProfile1)
objProfile1 = Nothing
End If
If Not (objProfile2 Is Nothing) Then
Marshal.ReleaseComObject(objProfile2)
objProfile1 = Nothing
End If
If Not (objProfiles Is Nothing) Then
Marshal.ReleaseComObject(objProfiles)
objProfiles = Nothing
End If

If Not (objSketch Is Nothing) Then
Marshal.ReleaseComObject(objSketch)
objSketch = Nothing
End If
If Not (objSketches Is Nothing) Then
Marshal.ReleaseComObject(objSketches)
objSketches = Nothing
End If
If Not (objPart Is Nothing) Then
Marshal.ReleaseComObject(objPart)
objPart = Nothing
End If
If Not (objDocuments Is Nothing) Then
Marshal.ReleaseComObject(objDocuments)
objDocuments = Nothing
End If
If Not (objApplication Is Nothing) Then
Marshal.ReleaseComObject(objApplication)
objApplication = Nothing
End If
End Try
End Sub
End Module

This code works!

___________
Option Explicit

Dim objApp As SolidEdgeFramework.Application
Dim objDoc As SolidEdgePart.SheetMetalDocument
Dim objCSections(1 To 2) As Object
Dim cSectionTypes(1 To 2) As Long
Dim sectionOrigins(1 To 2) As Object
Dim sectionOriginRefs(1 To 2) As Long
Dim varRad As Double
Dim varNF As Double
Dim varBPType As Long
Dim loftflange As Object

Private Sub Form_Load()

Set objApp = GetObject(, "SolidEdge.Application")
Set objDoc = objApp.ActiveDocument

'Assume that the file contains two cross section sketches

'Set profile array
Set objCSections(1) = objDoc.Sketches(1).Profiles(1)
Set objCSections(2) = objDoc.Sketches(2).Profiles(1)

cSectionTypes(1) = igProfileBasedCrossSection
cSectionTypes(2) = igProfileBasedCrossSection

'set start point array
Set sectionOrigins(1) = objDoc.Sketches(1).Profiles(1).Arcs2d(1)
Set sectionOrigins(2) = objDoc.Sketches(2).Profiles(1).Arcs2d(1)

sectionOriginRefs(1) = igStart
sectionOriginRefs(2) = igStart

varRad = 1
varNF = 0.5
varBPType = igNFType

' side can be igLeft or igRight
Set loftflange = objDoc.Models.AddLoftedFlange( _
2, _
objCSections, _
cSectionTypes, _
sectionOrigins, _
sectionOriginRefs, _
igLeft, _
varRad, _
varNF, _
varBPType)

Set loftflange = Nothing
Set sectionOrigins(1) = Nothing
Set sectionOrigins(2) = Nothing
Set objCSections(1) = Nothing
Set objCSections(2) = Nothing
Set objDoc = Nothing
Set objApp = Nothing

End Sub

Could somebody please provide me with a complete example of Curt's previous post. I'm hung up on his "'Assume that the file contains two cross section sketches" comment. I need this example but I also need it to create all of the necessary objects via code rather than assuming that a file is open.

Can anyone please help? I'm working on the SDK and need a good example. Please and thank you!