Hide Table of Contents

Get Faces Associated with Feature Example (VBA)

This example shows how to get the faces associated with a feature.

 

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

'

' Problem:

'       In SolidWorks, a face is the result of evaluating

'       a feature. A face can be owned by several features.

'       IFeature::GetFaces returns all faces owned by this

'       feature. This is different from faces highlighted in

'       user-interface when feature is selected. The user-interface

'       filters out multiple feature faces. This filter is

'       for display purposes only.

'

'       An application must use IFace::GetFeature

'       to filter out multiple feature faces. This method

'       returns only the oldest feature from face; that is, the

'       first owning feature in the FeatureManager design tree.

'

'       This example shows how to eliminate multiple

'       feature faces.

'

' Preconditions:

'       (1) Part is open.

'       (2) Feature is selected in the FeatureManager design tree.

'

' Postconditions: Faces of the feature are colored blue.

'       The faces are the same faces as if the

'       feature was selected through the user-interface.

'

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

 

Option Explicit

 

Sub main()

    Dim swApp                   As SldWorks.SldWorks

    Dim swModel                 As SldWorks.ModelDoc2

    Dim swSelMgr                As SldWorks.SelectionMgr

    Dim swSelData               As SldWorks.SelectData

    Dim swFeat                  As SldWorks.feature

    Dim swFaceFeat              As SldWorks.feature

    Dim vFaceArr                As Variant

    Dim vFace                   As Variant

    Dim vFeatColor              As Variant

    Dim swFace                  As SldWorks.face2

    Dim swEnt                   As SldWorks.entity

    Dim i                       As Long

    Dim bRet                    As Boolean

    

    Set swApp = Application.SldWorks

    Set swModel = swApp.ActiveDoc

    Set swSelMgr = swModel.SelectionManager

    Set swFeat = swSelMgr.GetSelectedObject5(1)

    Set swSelData = swSelMgr.CreateSelectData

    

    Debug.Print "Feature = " + swFeat.Name + " [" + swFeat.GetTypeName + "]"

    Debug.Print "  Face count = " & swFeat.GetFaceCount

    

    swModel.ClearSelection2 True

    

    vFeatColor = swModel.MaterialPropertyValues

    vFeatColor(0) = 0  'R

    vFeatColor(1) = 0  'G

    vFeatColor(2) = 1  'B

    vFaceArr = swFeat.GetFaces: If IsEmpty(vFaceArr) Then Exit Sub

    For Each vFace In vFaceArr

        Set swFace = vFace

        Set swEnt = swFace

        Set swFaceFeat = swFace.GetFeature

        

        ' Check to see if face is owned by multiple features

        If swFaceFeat Is swFeat Then

            bRet = swEnt.Select4(True, swSelData): Debug.Assert bRet

            swFace.MaterialPropertyValues = vFeatColor

        Else

            Debug.Print "  Other feature = " & swFaceFeat.Name + " [" + swFaceFeat.GetTypeName + "]"

        End If

    Next

End Sub

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



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Get Faces Associated with Feature Example (VBA)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2012 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.