Reorder Method

Description

Inserts the referenced object in front of or behind another feature.

Syntax

Visual Basic
Public Sub Reorder( _ ByVal TargetFeature As Object, _ ByVal InsertBefore As Boolean _ )

Parameters

TargetFeature: Specifies the feature object for which the referenced feature object is to be inserted in front of or behind.
InsertBefore: Specifies if the active feature object is to be placed before or after the target object. If this argument is True, the active feature object is inserted before the target object. If this argument is False, the feature object is placed after the target object.

Example

Example (Visual Basic)

Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objModel As SolidEdgePart.Model
    Dim objProfile As SolidEdgePart.Profile
    Dim objExtCutout As SolidEdgePart.ExtrudedCutout
    Dim objEdges As Object
    Dim objEdgeArray(1 To 1) As SolidEdgeGeometry.Edge
    Dim objRounds As SolidEdgePart.Rounds
    Dim objRound As SolidEdgePart.Round
    Dim dblRadiusArray(1 To 1) As Double
    Dim lngStatus As Long
    Const TESTFILE = "T:\vbtests\testcases\cube.par"
    ' 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
    Call objDoc.Close
    ' opening the test case file
    Set objDoc = objApp.Documents.Open(TESTFILE)
    Set objModel = objDoc.Models(1)
    ' *** Create a simple cutout
    ' Create a profile for the extruded cutout feature and validate it
    Set objProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(1))
    Call objProfile.Circles2d.AddByCenterRadius(x:=0.015, y:=0.015, Radius:=0.005)
    lngStatus = objProfile.End(ValidationCriteria:=igClosed)
    If lngStatus <> 0 Then
        MsgBox "Profile for the Extruded Cutout feature is not closed"
    End If
    ' Create the Extruded Cutout feature and validate it
    Set objExtCutout = objModel.ExtrudedCutouts.AddFinite(Profile:=objProfile, _
                                                          ProfileSide:=igLeft, ProfilePlaneSide:=igRight, Depth:=0.05)
    objProfile.Visible = False
    If objExtCutout.Status <> igFeatureOK Then
        MsgBox "AddFinite method of ExtrudedCutouts object failed"
    End If
    ' *** creating a simple round on a single edge
    ' defining the radius for rounding an edge
    Set objRounds = objModel.Rounds
    Set objEdges = objModel.ExtrudedProtrusions(1).Edges(edgetype:=igQueryAll)
    Set objEdgeArray(1) = objEdges(1)
    dblRadiusArray(1) = 0.005
    ' Create the round feature and validate it
    Set objRound = objRounds.Add(NumberOfEdgeSets:=1, EdgeSetArray:=objEdgeArray, _
                                 RadiusArray:=dblRadiusArray)
    If objRound.Status <> igFeatureOK Then
        MsgBox "Round feature failed"
    End If
    'Reorder the round feature ahead of cutout feature
    Call objRound.Reorder(TargetFeature:=objModel.Features(1), InsertBefore:=False)
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objModel = Nothing
    Set objEdges = Nothing
    Set objEdgeArray(1) = Nothing
    Set objRounds = Nothing
    Set objRound = Nothing
End Sub