Edges Property

Description

Returns a collection of edges of a specified type that belong to a model, a feature, or a topology collection of faces.

Property type

Read-only property

Syntax

Visual Basic
Public Property Edges( _ ByVal EdgeType As FeatureTopologyQueryTypeConstants _ ) As Object

Parameters

EdgeType

Value	Description
igQueryAll	Feature Topology Query Type - All
igQueryCone	Feature Topology Query Type - Cone
igQueryCylinder	Feature Topology Query Type - Cylinder
igQueryEllipse	Feature Topology Query Type - Ellipse
igQueryPlane	Feature Topology Query Type - Plane
igQueryRoundable	Feature Topology Query Type - Roundable
igQuerySphere	Feature Topology Query Type - Sphere
igQuerySpline	Feature Topology Query Type - Spline
igQueryStraight	Feature Topology Query Type - Straight
igQueryTorus	Feature Topology Query Type - Torus

Remarks

The result of the Edges property is a topology collection. This topology collection is a temporary collection and is overwritten the next time the Edges, Faces, or FacesByRay property is used. By default, the Edges property returns all edges for the object. The topology collection can be restricted to a specified type of edge by supplying a value (from the FeatureTopologyQueryTypeConstants constant set) for the EdgeType argument for the feature objects only. For example, this property can be set to return all ellipse edges, straight edges, and so forth.

Example

Example (Visual Basic)

Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objProfile(1 To 2) As SolidEdgePart.Profile
    Dim objExtProt As SolidEdgePart.ExtrudedProtrusion
    Dim objModel As SolidEdgePart.Model
    Dim objLines As SolidEdgeFrameworkSupport.Lines2d
    Dim objRelns As SolidEdgeFrameworkSupport.Relations2d
    Dim objEdgs As Object
    Dim lngStatus As Long
    ' Report errors
    Const PI = 3.14159265358979
    ' Create/get the application with specific settings
    On Error Resume Next
    Set objApp = GetObject(, "SolidEdge.Application")
    If Err Then
        Err.Clear
        Set objApp = CreateObject("SolidEdge.Application")
        Set objDoc = objApp.Documents.Add("SolidEdge.PartDocument")
        objApp.Visible = True
    Else
        Set objDoc = objApp.ActiveDocument
    End If
    'Draw the Base Profile
    Set objProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(objDoc.RefPlanes(3))
    Set objLines = objProfile(1).Lines2d
    Call objLines.AddBy2Points(x1:=0, y1:=0, x2:=0.08, y2:=0)
    Call objLines.AddBy2Points(x1:=0.08, y1:=0, x2:=0.08, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.08, y1:=0.06, x2:=0.064, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.064, y1:=0.06, x2:=0.064, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.064, y1:=0.02, x2:=0.048, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.048, y1:=0.02, x2:=0.048, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.048, y1:=0.06, x2:=0.032, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.032, y1:=0.06, x2:=0.032, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.032, y1:=0.02, x2:=0.016, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.016, y1:=0.02, x2:=0.016, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.016, y1:=0.06, x2:=0, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0, y1:=0.06, x2:=0, y2:=0)
    ' Define Relations among the Line objects to make the Profile closed
    Set objRelns = objProfile(1).Relations2d
    Call objRelns.AddKeypoint(Object1:=objLines(1), Index1:=igLineEnd, Object2:=objLines(2), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(2), Index1:=igLineEnd, Object2:=objLines(3), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(3), Index1:=igLineEnd, Object2:=objLines(4), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(4), Index1:=igLineEnd, Object2:=objLines(5), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(5), Index1:=igLineEnd, Object2:=objLines(6), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(6), Index1:=igLineEnd, Object2:=objLines(7), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(7), Index1:=igLineEnd, Object2:=objLines(8), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(8), Index1:=igLineEnd, Object2:=objLines(9), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(9), Index1:=igLineEnd, Object2:=objLines(10), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(10), Index1:=igLineEnd, Object2:=objLines(11), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(11), Index1:=igLineEnd, Object2:=objLines(12), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(12), Index1:=igLineEnd, Object2:=objLines(1), Index2:=igLineStart)
    ' Check for the Profile Validity
    lngStatus = objProfile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Profile not closed")
    End If
    'Create the Base Extruded Protrusion Feature
    Set objModel = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, _
                                                             profileArray:=objProfile, profileplaneSide:=igRight, _
                                                             ExtrusionDistance:=0.05)
    objProfile(1).Visible = False
    ' Check the status of Base Feature
    If objModel.ExtrudedProtrusions(1).Status <> igFeatureOK Then
        MsgBox ("Error in the Creation of Base Protrusion Feature object")
    End If
    Set objExtProt = objModel.ExtrudedProtrusions(1)
    ' Get the Edges of the ProtrusionFeature object
    Set objEdgs = objExtProt.Edges(EdgeType:=igQueryAll)
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objProfile(1) = Nothing
    Set objProfile(2) = Nothing
    Set objExtProt = Nothing
    Set objLines = Nothing
    Set objModel = Nothing
    Set objRelns = Nothing
    Set objEdgs = Nothing
End Sub