Hide Table of Contents

Insert Surface-cut Feature Example (VBA)

This example shows how to insert a surface-cut feature.

' ******************************************************************************
' Preconditions: 
' 1. Specified file to open exists.
' 2. Open the Immediate window.
' Postconditions:
' 1. Opens part whose intersecting solid bodies to cut with a plane.
' 2. Creates a plane named Plane1.
' 3. Selects Plane1 to cut all intersecting solid bodies.
' 4. Inserts the surface-cut feature. All intersecting solid 
'    bodies were cut by the plane.
' 5. Examine the graphics area and Immediate window to verify.
' NOTE: Because this part document is used elsewhere, do not
' save any changes when closing it.
' ******************************************************************************
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swFeature As SldWorks.Feature
Dim swFeatureManager As SldWorks.FeatureManager
Dim swRefPlane As SldWorks.RefPlane
Dim swSurfaceCutFeature As SldWorks.SurfCutFeatureData
Dim fileName as String
Dim status As Boolean
Dim errors As Long, warnings As Long
Sub main()
    Set swApp = Application.SldWorks    
    ' Open part to cut with a plane
    fileName = "C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\samples\tutorial\multibody\multi_inter.sldprt"
    Set swModel = swApp.OpenDoc6(FileName, swDocPart, swOpenDocOptions_Silent, "", errors, warnings)
    Set swModelDocExt = swModel.Extension    
    ' Create and select the plane to cut
    ' all intersecting solid bodies in the part
    status = swModelDocExt.SelectByID2("Front", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
    Set swFeatureManager = swModel.FeatureManager
    Set swRefPlane = swFeatureManager.InsertRefPlane(swRefPlaneReferenceConstraint_Distance, 0.045, 0, 0, 0, 0)
    status = swModelDocExt.SelectByID2("Plane1", "PLANE", 0, 0, 0, True, 0, Nothing, 0)    
    ' Insert a surface-cut feature that cuts 
    ' all intersecting solid bodies
    Set swFeature = swFeatureManager.InsertCutSurface(False, 0, False, True, Nothing, errors)
    Debug.Print ("Were any errors generated by the surface cut (0 = no errors)? " & errors)
    Set swSurfaceCutFeature = swFeature.GetDefinition

    ' Get surface-cut feature and some properties
    Debug.Print ("Name of surface-cut feature: " & swFeature.Name)
    Debug.Print (" Is feature scope on? " & swSurfaceCutFeature.FeatureScope)
    Debug.Print (" Number of bodies cut by the plane: " & swSurfaceCutFeature.GetFeatureScopeBodiesCount)
    Debug.Print (" Is auto-select on? " & swSurfaceCutFeature.AutoSelect)   
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

Subject:   Feedback on Help Topics
Page:   Insert Surface-cut Feature Example (VBA)
*   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:


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

Web Help Content Version: API Help (English only) 2015 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.