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Get DimXpert Extrude Feature Example (VBA)

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 that all feature filters are selected.

'    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 latest SolidWorks DimXpert type library is loaded

'    in Tools > References.

' 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.

'---------------------------------------------------------------------------

Option Explicit

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swModelDocExt As SldWorks.ModelDocExtension

Dim swSelMgr As SldWorks.SelectionMgr

Dim swConfig As SldWorks.ConfigurationManager

Dim swFeature As SldWorks.feature

Dim swAnn As SldWorks.feature

Dim swSchema As SldWorks.DimXpertManager

Dim swDXPart As DimXpertPart

Dim featureType As swDimXpertFeatureType_e

Dim features As Variant

Dim appliedFeatures As Variant

Dim appliedAnnotations As Variant

Dim appliedAnnotation As DimXpertAnnotation

Dim feature As DimXpertFeature

Dim appliedFeature As DimXpertFeature

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()

    Set swApp = Application.SldWorks

    Set swModel = swApp.ActiveDoc

    

    Set swModelDocExt = swModel.Extension

    Set swSelMgr = swModel.SelectionManager

    

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

    

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

    

    ' Get IDimXpertPart from the IDimXpertManager

    Set swDXPart = swSchema.DimXpertPart

    

    Dim featCount As Long

    featCount = swDXPart.GetFeatureCount

    msgStr = "Total of "

    msgStr2 = featCount

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

    Debug.Print ""

    Debug.Print msgStr

    

    ' Get IDimXpert features through IDimXpertPart

    

    features = swDXPart.GetFeatures

    

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

    Debug.Print ""

    Debug.Print msgStr

    For n = 0 To UBound(features)

        Set 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: "

        Set 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 (IsEmpty(appliedFeatures)) Then

            For o = 0 To UBound(appliedFeatures)

                Set appliedFeature = appliedFeatures(o)

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

            Next

        End If

        

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

        msgStr2 = feature.GetAppliedAnnotationCount()

        Debug.Print msgStr + msgStr2

        

        appliedAnnotations = feature.GetAppliedAnnotations()

        If Not (IsEmpty(appliedAnnotations)) Then

            For p = 0 To UBound(appliedAnnotations)

                Set appliedAnnotation = appliedAnnotations(p)

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

            Next

        End If

        

        Debug.Print "     "

    Next

    

    ' 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

    Set extrudeFeature = swDXPart.GetFeature("Pocket1")

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

    Debug.Print ""

    Debug.Print msgStr

    Debug.Print ""

        

    ' Get the bottom blends

    Set 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

    Set 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

    Set 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)

        Set feature = features(n)

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

        

        featureType = feature.Type

        Call GetPatternType(featureType, msgStr2)

        

        msgStr = "     Feature type is "

        

        Debug.Print msgStr + msgStr2

    Next

    

    ' 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, ByRef msgStr2)

    If (featureType = swDimXpertFeature_Plane) Then

            msgStr2 = "Plane"

    ElseIf (featureType = swDimXpertFeature_Cylinder) Then

            msgStr2 = "Cylinder"

    ElseIf (featureType = swDimXpertFeature_Cone) Then

            msgStr2 = "Cone"

    ElseIf (featureType = swDimXpertFeature_Extrude) Then

            msgStr2 = "Extrude"

    ElseIf (featureType = swDimXpertFeature_Fillet) Then

            msgStr2 = "Fillet"

    ElseIf (featureType = swDimXpertFeature_Chamfer) Then

            msgStr2 = "Chamfer"

    ElseIf (featureType = swDimXpertFeature_CompoundHole) Then

            msgStr2 = "CompoundHole"

    ElseIf (featureType = swDimXpertFeature_CompoundWidth) Then

            msgStr2 = "CompoundWidth"

    ElseIf (featureType = swDimXpertFeature_CompoundNotch) Then

            msgStr2 = "CompoundNotch"

    ElseIf (featureType = swDimXpertFeature_CompoundClosedSlot3D) Then

            msgStr2 = "CompoundClosedSlot3D"

    ElseIf (featureType = swDimXpertFeature_IntersectPoint) Then

            msgStr2 = "IntersectPoint"

    ElseIf (featureType = swDimXpertFeature_IntersectLine) Then

            msgStr2 = "IntersectLine"

    ElseIf (featureType = swDimXpertFeature_IntersectCircle) Then

            msgStr2 = "IntersectCircle"

    ElseIf (featureType = swDimXpertFeature_IntersectPlane) Then

            msgStr2 = "IntersectPlane"

    ElseIf (featureType = swDimXpertFeature_Pattern) Then

            msgStr2 = "Pattern"

    ElseIf (featureType = swDimXpertFeature_Sphere) Then

            msgStr2 = "Sphere"

    ElseIf (featureType = swDimXpertFeature_BestfitPlane) Then

            msgStr2 = "Bestfit Plane"

    ElseIf (featureType = swDimXpertFeature_Surface) Then

            msgStr2 = "Surface"

    End If

    

End Sub



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