Faces Property

Description

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

Property type

Read-only property

Syntax

Visual Basic
Public Property Faces( _ ByVal FaceType As FeatureTopologyQueryTypeConstants _ ) As Object

Parameters

FaceType

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 Faces 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 Faces property returns all faces for the object. The topology collection can be restricted to a specified type of face by supplying a value (from the FeatureTopologyQueryTypeConstants constant set) for the FaceType argument for the feature objects only. For example, this property can be set to return all faces that are spheres.

Example

Example (Visual Basic)

Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objBaseProfile(1 To 2) As SolidEdgePart.Profile
    Dim objLine1 As SolidEdgeFrameworkSupport.Line2d
    Dim objLine2 As SolidEdgeFrameworkSupport.Line2d
    Dim objArc1 As SolidEdgeFrameworkSupport.Arc2d
    Dim objArc2 As SolidEdgeFrameworkSupport.Arc2d
    Dim objModel As SolidEdgePart.Model
    Dim objExtProtrusion As SolidEdgePart.ExtrudedProtrusion
    Dim objRelations As SolidEdgeFrameworkSupport.Relations2d
    Dim objTraceRefPlane As SolidEdgePart.RefPlane
    Dim objTraceprofile(1 To 2) As SolidEdgePart.Profile
    Dim objCSRefPlane As SolidEdgePart.RefPlane
    Dim objCSProfile(1 To 2) As SolidEdgePart.Profile
    Dim vOriginArray(2) As Variant
    Dim objSweptCutout As SolidEdgePart.SweptCutout
    Dim objFaces As Object
    Dim lngStatus As Long
    Dim lngTraceCurveTypes(1 To 2) As Long
    Dim lngCrossSectionTypes(1 To 2) 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
    On Error GoTo 0
    'Create an Extruded Protrusion as Base feature
    'Draw the base Profile
    Set objBaseProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(1))
    Set objLine1 = objBaseProfile(1).Lines2d.AddBy2Points(x1:=0.05, y1:=0, x2:=0.05, y2:=0.15)
    Set objArc1 = objBaseProfile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0.15, _
                                                               xStart:=0.05, yStart:=0.15, xEnd:=0, yEnd:=0.15)
    Set objLine2 = objBaseProfile(1).Lines2d.AddBy2Points(x1:=0, y1:=0.15, x2:=0, y2:=0)
    Set objArc2 = objBaseProfile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0, _
                                                               xStart:=0, yStart:=0, xEnd:=0.05, yEnd:=0)
    ' Define Relations among the Line and Arc objects to make the Profile closed
    Set objRelations = objBaseProfile(1).Relations2d
    Call objRelations.AddKeypoint(Object1:=objLine1, Index1:=igLineEnd, _
                                  Object2:=objArc1, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc1, Index1:=igArcEnd, _
                                  Object2:=objLine2, Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine2, Index1:=igLineEnd, _
                                  Object2:=objArc2, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc2, Index1:=igArcEnd, _
                                  Object2:=objLine1, Index2:=igLineStart)
    ' Check for the Profile Validity
    lngStatus = objBaseProfile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Base feature profile is not closed")
    End If
    'Create the Base Extruded Protrusion Feature
    Set objModel = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, ProfileArray:=objBaseProfile, _
                                                             ProfilePlaneSide:=igRight, ExtrusionDistance:=0.05)
    objBaseProfile(1).Visible = False
    Set objExtProtrusion = objModel.ExtrudedProtrusions(1)
    ' Check the status of Base Feature
    If objExtProtrusion.Status <> igFeatureOK Then
        MsgBox "Base Feature is not created properly"
    End If
    'Create SweptCutout with Add method
    'Draw the Trace profile
    Set objTraceRefPlane = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(1), _
                                                                  Distance:=0.05, NormalSide:=igRight, Local:=True)
    Set objTraceprofile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objTraceRefPlane)
    Set objLine1 = objTraceprofile(1).Lines2d.AddBy2Points(x1:=0.05, y1:=0, x2:=0.05, y2:=0.15)
    Set objArc1 = objTraceprofile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0.15, _
                                                                xStart:=0.05, yStart:=0.15, xEnd:=0, yEnd:=0.15)
    Set objLine2 = objTraceprofile(1).Lines2d.AddBy2Points(x1:=0, y1:=0.15, x2:=0, y2:=0)
    Set objArc2 = objTraceprofile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0, _
                                                                xStart:=0, yStart:=0, xEnd:=0.05, yEnd:=0)
    ' Define Relations among the Line and Arc objects to make the Trace Profile closed
    Set objRelations = objTraceprofile(1).Relations2d
    Call objRelations.AddKeypoint(Object1:=objLine1, Index1:=igLineEnd, _
                                  Object2:=objArc1, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc1, Index1:=igArcEnd, _
                                  Object2:=objLine2, Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine2, Index1:=igLineEnd, _
                                  Object2:=objArc2, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc2, Index1:=igArcEnd, _
                                  Object2:=objLine1, Index2:=igLineStart)
    ' Check for the Trace Profile Validity
    lngStatus = objTraceprofile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Trace profile is not closed")
    End If
    ' Create a reference plane for Cross section profile
    Set objCSRefPlane = objDoc.RefPlanes.AddNormalToCurve( _
                        Curve:=objLine1, _
                        PlanePoint:=igCurveStart, _
                        OrientationPlaneOrPivot:=objDoc.RefPlanes(1), _
                        PivotOrigin:=igPivotEnd, _
                        Local:=True, _
                        ParentCurve:=objTraceprofile(1))
    ' Draw the Cross Section profile
    Set objCSProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objCSRefPlane)
    Call objCSProfile(1).Circles2d.AddByCenterRadius(x:=0, y:=0, Radius:=0.01)
    ' Check for the Cross section Profile Validity
    lngStatus = objCSProfile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Cross-section profile is not closed")
    End If
    'Create SweptCutout Feature
    lngTraceCurveTypes(1) = igProfileBasedCrossSection
    lngCrossSectionTypes(1) = igProfileBasedCrossSection
    vOriginArray(1) = 0
    Set objSweptCutout = objModel.SweptCutouts.Add(NumCurves:=1, _
                                                   TraceCurves:=objTraceprofile, TraceCurveTypes:=lngTraceCurveTypes, NumSections:=1, _
                                                   CrossSections:=objCSProfile, CrossSectionTypes:=lngCrossSectionTypes, _
                                                   Origins:=vOriginArray, SegmentMaps:=0, MaterialSide:=igLeft, StartExtentType:=igNone, _
                                                   StartExtentDistance:=0, StartSurfaceOrRefPlane:=Nothing, EndExtentType:=igNone, _
                                                   EndExtentDistance:=0, EndSurfaceOrRefPlane:=Nothing)
    objTraceprofile(1).Visible = False
    objCSProfile(1).Visible = False
    ' Check the status of SweptCutout Feature
    If objSweptCutout.Status <> igFeatureOK Then
        MsgBox "Add method of the SweptCutouts object Failed"
    End If
    'Get the Faces of the SweptCutout Created using Faces property
    Set objFaces = objSweptCutout.Faces(FaceType:=igQueryAll)

    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objBaseProfile(1) = Nothing
    Set objBaseProfile(2) = Nothing
    Set objLine1 = Nothing
    Set objLine2 = Nothing
    Set objArc1 = Nothing
    Set objArc2 = Nothing
    Set objModel = Nothing
    Set objExtProtrusion = Nothing
    Set objRelations = Nothing
    Set objTraceRefPlane = Nothing
    Set objTraceprofile(1) = Nothing
    Set objTraceprofile(2) = Nothing
    Set objCSRefPlane = Nothing
    Set objCSProfile(1) = Nothing
    Set objCSProfile(2) = Nothing
    Set vOriginArray(1) = Nothing
    Set vOriginArray(2) = Nothing
    Set objSweptCutout = Nothing
    Set objFaces = Nothing
End Sub