AddSymmetric Method

Description

Adds a symmetric relationship to a Relations2d collection.

Syntax

Visual Basic
Public Function AddSymmetric( _ ByVal pLine As Object, _ ByVal Object2 As Object, _ ByVal Object3 As Object, _ Optional ByVal guaranteed_ok As Variant _ ) As Relation2d

Parameters

pLine: Specifies the Line2d object along which the symmetric relationship is to be applied.
Object2: Specifies the first object to which the symmetric relationship is to be applied. Object2 and Object3 must be of the same type.
Object3: Specifies the second object to which the symmetric relationship is to be applied. Object2 and Object3 must be of the same type.
guaranteed_ok: If set, checking is performed to ensure that the relationship does not contradict previously placed relationships.

Remarks

The method creates a Symmetric relationship between the second and third specified objects along the specified line. Relationship Add methods have checks to ensure that a new relationship does not contradict previously placed relationships. For example, AddHorizontal will return an error if the line already has a vertical relationship. This check can be turned off to enhance performance. The optional “guaranteed_ok” argument, if set to 1, bypasses relationship checking. However, this feature could leave the system in an unsolvable state, so use it with extreme caution. It is best to use this feature only on a new element with no other relationships.

Example

Example (Visual Basic)

Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objLine1 As SolidEdgeFrameworkSupport.Line2d
    Dim objArc2 As SolidEdgeFrameworkSupport.Arc2d
    Dim objArc1 As SolidEdgeFrameworkSupport.Arc2d
    Dim objRelns As SolidEdgeFrameworkSupport.Relations2d
    Dim objReln1 As SolidEdgeFrameworkSupport.Relation2d
    Dim objProfile As SolidEdgePart.Profile
    ' 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

    ' Create an empty Profile
    Set objProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:= _
                                                         objDoc.RefPlanes(1))
    ' Create 2 Arc objects
    Set objArc1 = objProfile.Arcs2d.AddByStartAlongEnd(xStart:=0.02, yStart:=0, _
                                                       xAlong:=0, yAlong:=0.05, xEnd:=-0.07, yEnd:=-0.04)
    Set objArc2 = objProfile.Arcs2d.AddByStartAlongEnd(xStart:=0.05, yStart:=0.01, _
                                                       xAlong:=0.07, yAlong:=0.05, xEnd:=0.1, yEnd:=-0.04)

    ' Create a Line object
    Set objLine1 = objProfile.Lines2d.AddBy2Points(x1:=0, y1:=0, x2:=0.1, y2:=0)
    ' Create a Symmetric Relation between the objects
    Set objRelns = objProfile.Relations2d
    Set objReln1 = objRelns.AddSymmetric(pLine:=objLine1, Object2:=objArc1, _
                                         Object3:=objArc2)

    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objLine1 = Nothing
    Set objArc2 = Nothing
    Set objArc1 = Nothing
    Set objProfile = Nothing
    Set objRelns = Nothing
    Set objReln1 = Nothing
End Sub