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Get DimXpert Extrude Feature Example (VB.NET)

This example shows how to build a part and get attributes for the following DimXpert feature:


    *  Extrude


' Preconditions:

' 1. Open:

' <SolidWorks_install_dir>\samples\tutorial\api\plate_ads_plusminus.sldprt

' 2. Open the DimXpert toolbar from View > Toolbars

'    (select the first instance of Toolbars on the View menu).

' 3. Create the Extrude Feature:

'    a. Click the Auto Dimension Scheme icon on the DimXpert toolbar.

'    b. Ensure the Scope is set to All Features.

'    c. Click the green check mark to accept the settings.

' 4. Observe the following DimXpert features on the DimXpertManager tab:  

'    Hole Pattern1, Pocket1.

' 5. Open an Immediate window in the IDE.

' 6. Ensure that the SolidWorks.Interop.swdimxpert.dll interop assembly

'    is loaded (right-click on project in Project Explorer,

'    click Add Reference, click the .NET tab).

' 7. Run this macro (F5).


' Postconditions: Compare the output in the Immediate Window

' with the features displayed on the DimXpertManager tab of the Management Panel.

' NOTE: Because this part is used in a SolidWorks online tutorial,

' do not save any changes when you close it.


Imports SolidWorks.Interop.sldworks

Imports SolidWorks.Interop.swdimxpert

Imports SolidWorks.Interop.swconst

Imports System

Imports System.Diagnostics

Partial Class SolidWorksMacro


    Dim swModel As IModelDoc2

    Dim swModelDocExt As IModelDocExtension

    Dim swSelMgr As ISelectionMgr

    Dim swConfig As IConfiguration

    Dim swFeature As IFeature

    Dim swAnn As IFeature

    Dim swSchema As IDimXpertManager

    Dim swDXPart As IDimXpertPart

    Dim featureType As swDimXpertFeatureType_e

    Dim features As Object

    Dim appliedFeatures As Object

    Dim appliedAnnotations As Object

    Dim appliedAnnotation As IDimXpertAnnotation

    Dim feature As IDimXpertFeature

    Dim appliedFeature As IDimXpertFeature

    Dim msgStr As String

    Dim msgStr2 As String

    Dim msgStr3 As String

    Dim msgStr4 As String

    Dim n As Long

    Dim o As Long

    Dim p As Long

    Dim boolstatus As Boolean

    Sub main()

        swModel = swApp.ActiveDoc

        swModelDocExt = swModel.Extension

        swSelMgr = swModel.SelectionManager

        ' Get the default DimXpert schema using IModelDocExtension.DimXpertManager()

        swSchema = swModelDocExt.DimXpertManager("Default", True)

        ' Get IDimXpertPart from the IDimXpertManager

        swDXPart = swSchema.DimXpertPart

        Dim featCount As Long

        featCount = swDXPart.GetFeatureCount

        msgStr = "Total of "

        msgStr2 = featCount

        msgStr = msgStr + msgStr2 + " DimXpert features in " + (swSchema.SchemaName)



        ' Get IDimXpert features through IDimXpertPart

        features = swDXPart.GetFeatures

        msgStr = (swSchema.SchemaName) + " has the following features: "



        For n = 0 To UBound(features)

            feature = features(n)

            Debug.Print("  " + "Feature name: " + (feature.Name))

            featureType = feature.Type

            Call GetPatternType(featureType, msgStr2)

            msgStr = "     Feature type "

            msgStr3 = " is suppressed on the DimXpertManager tab? "

            msgStr4 = feature.IsSuppressed()

            Debug.Print(msgStr + msgStr2 + msgStr3 + msgStr4)

            msgStr = "     " + "Model feature: "

            swFeature = feature.GetModelFeature()

            If Not (swFeature Is Nothing) Then

                msgStr2 = swFeature.GetTypeName2()

                Debug.Print(msgStr + msgStr2)

            End If

            msgStr = "     " + "Number of SolidWorks face entities in this feature: "

            msgStr2 = feature.GetFaceCount

            Debug.Print(msgStr + msgStr2)

            msgStr = "     " + "Number of applied features: "

            msgStr2 = feature.GetAppliedFeatureCount()

            Debug.Print(msgStr + msgStr2)

            appliedFeatures = feature.GetAppliedFeatures()

            If Not (IsNothing(appliedFeatures)) Then

                For o = 0 To UBound(appliedFeatures)

                    appliedFeature = appliedFeatures(o)

                    Debug.Print("        " + "Applied feature name: " + (appliedFeature.Name))


            End If

            msgStr = "     " + "Number of applied annotations: "

            msgStr2 = feature.GetAppliedAnnotationCount()

            Debug.Print(msgStr + msgStr2)

            appliedAnnotations = feature.GetAppliedAnnotations()

            If Not (IsNothing(appliedAnnotations)) Then

                For p = 0 To UBound(appliedAnnotations)

                    appliedAnnotation = appliedAnnotations(p)

                    Debug.Print("        " + "Applied annotation name: " + (appliedAnnotation.Name))


            End If

            Debug.Print("     ")


        ' If you know the name of a DimXpert feature, you can get it directly using IDimXpertPart.GetFeature("name"),

        ' which can return a general IDimXpertFeature or a more specific interface on the feature

        ' Get IDimXpertExtrudeFeature for the Pocket1 feature

        Dim extrudeFeature As IDimXpertExtrudeFeature

        extrudeFeature = swDXPart.GetFeature("Pocket1")

        msgStr = extrudeFeature.Name + " is a DimXpert extrude feature"




        ' Get the bottom blends

        feature = extrudeFeature.GetBottomBlends

        If Not feature Is Nothing Then

            msgStr = "The bottom blends for the extrude is "

            msgStr2 = feature.Name

            Debug.Print(msgStr + msgStr2)

        Else : Debug.Print("There are no bottom blends for this extrude.")

        End If

        ' Get the bottom feature

        feature = extrudeFeature.GetBottomFeature

        If Not feature Is Nothing Then

            msgStr = "The bottom feature for the extrude is "

            msgStr2 = feature.Name

            Debug.Print(msgStr + msgStr2)

        End If

        ' Get the reference feature

        feature = extrudeFeature.GetReferenceFeature

        If Not feature Is Nothing Then

            msgStr = "The reference feature for the extrude is "

            msgStr2 = feature.Name

            Debug.Print(msgStr + msgStr2)

        End If

        ' Get the sub-features

        Dim featureCount As Integer

        featureCount = extrudeFeature.GetSubFeatureCount

        msgStr = "The number of sub-features of the extrude is "

        msgStr2 = featureCount

        Debug.Print(msgStr + msgStr2)

        features = extrudeFeature.GetSubFeatures

        For n = 0 To UBound(features)

            feature = features(n)

            Debug.Print("  " + "Feature name: " + (feature.Name))

            featureType = feature.Type

            Call GetPatternType(featureType, msgStr2)

            msgStr = "     Feature type is "

            Debug.Print(msgStr + msgStr2)


        ' Get whether the extrude is blind

        boolstatus = extrudeFeature.Blind

        msgStr = "The extrude is blind: "

        msgStr2 = boolstatus

        Debug.Print(msgStr + msgStr2)

    End Sub

    Public Sub GetPatternType(ByRef featureType As swDimXpertFeatureType_e, ByRef msgStr2 As String)

        If (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Plane) Then

            msgStr2 = "Plane"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Cylinder) Then

            msgStr2 = "Cylinder"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Cone) Then

            msgStr2 = "Cone"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Extrude) Then

            msgStr2 = "Extrude"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Fillet) Then

            msgStr2 = "Fillet"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Chamfer) Then

            msgStr2 = "Chamfer"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_CompoundHole) Then

            msgStr2 = "CompoundHole"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_CompoundWidth) Then

            msgStr2 = "CompoundWidth"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_CompoundNotch) Then

            msgStr2 = "CompoundNotch"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_CompoundClosedSlot3D) Then

            msgStr2 = "CompoundClosedSlot3D"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_IntersectPoint) Then

            msgStr2 = "IntersectPoint"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_IntersectLine) Then

            msgStr2 = "IntersectLine"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_IntersectCircle) Then

            msgStr2 = "IntersectCircle"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_IntersectPlane) Then

            msgStr2 = "IntersectPlane"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Pattern) Then

            msgStr2 = "Pattern"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Sphere) Then

            msgStr2 = "Sphere"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_BestfitPlane) Then

            msgStr2 = "Bestfit Plane"

        ElseIf (featureType = swDimXpertFeatureType_e.swDimXpertFeature_Surface) Then

            msgStr2 = "Surface"

        End If

    End Sub


    Public swApp As SldWorks

End Class

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