AddHorizontalAlign Method

Description

Adds a horizontal alignment relationship to a Relations2d collection.

Syntax

Visual Basic
Public Function AddHorizontalAlign( _ ByVal Object1 As Object, _ ByVal Index1 As Long, _ ByVal Object2 As Object, _ ByVal Index2 As Long, _ Optional ByVal guaranteed_ok As Variant _ ) As Relation2d

Visual Basic

Public Function AddHorizontalAlign( _
   ByVal Object1 As Object, _
   ByVal Index1 As Long, _
   ByVal Object2 As Object, _
   ByVal Index2 As Long, _
   Optional ByVal guaranteed_ok As Variant _
) As Relation2d

Parameters

Object1: Specifies the first object to which the constraint is to be applied.
Index1: Specifies the key point index of Object1.
Object2: Specifies the second object to which the constraint is to be applied.
Index2: Specifies the key point index of Object2.
guaranteed_ok: If set, checking is performed to ensure that the relationship does not contradict previously placed relationships.

Remarks

The method aligns the first specified key point to be horizontal to the second specified key point. 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 objCirc1 As SolidEdgeFrameworkSupport.Circle2d
    Dim objCirc2 As SolidEdgeFrameworkSupport.Circle2d
    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 Circle objects
    Set objCirc1 = objProfile.Circles2d.AddByCenterRadius(x:=0, y:=0, Radius:=0.05)
    Set objCirc2 = objProfile.Circles2d.AddByCenterRadius(x:=0.1, y:=0.1, Radius:=0.05)

    ' Create a HorizontalAlign Relation between the objects
    Set objRelns = objProfile.Relations2d
    Set objReln1 = objRelns.AddHorizontalAlign(Object1:=objCirc1, Index1:=0, _
                                               Object2:=objCirc2, Index2:=0)

    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objCirc1 = Nothing
    Set objCirc2 = Nothing
    Set objProfile = Nothing
    Set objRelns = Nothing
    Set objReln1 = Nothing
End Sub