Hide Table of Contents

Modify Derived Part Example (VB.NET)

This example shows how to insert and modify a derived part.

' Preconditions:
' 1. Verify that the part documents to open and insert exist.
' 2. Open the Immediate window.
' Postconditions:
' 1. Opens the specified part document.
' 2. Inserts a derived part in the part document
'    opened in step 1.
' 3. Changes some parameters of the derived part feature.
' 4. Examine the Immediate window.
' NOTE: Because both part documents are used elsewhere,
' do not save any changes.
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
Partial Class SolidWorksMacro
    Public Sub main()
        Dim swModel As ModelDoc2
        Dim swPart As PartDoc
        Dim swModelDocExt As ModelDocExtension
        Dim swComp As Component2
        Dim swSelMgr As SelectionMgr
        Dim swDerivedFeat As Feature
        Dim swFeat As Feature
        Dim swDerivedData As DerivedPartFeatureData
        Dim bRet As Boolean
        Dim fileName As String
        Dim derivedFileName As String
        Dim errors As Integer
        Dim warnings As Integer
        'Open part, insert another part, and select the derived part feature
        fileName = "C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2017\tutorial\api\holecube.sldprt"
        swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
        derivedFileName = "C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2017\tutorial\api\box.sldprt"
        swPart = swModel
        swFeat = swPart.InsertPart2(derivedFileName, swInsertPartOptions_e.swInsertPartImportSolids)
        swModelDocExt = swModel.Extension
        bRet = swModelDocExt.SelectByID2("box""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        'Get the selected derived part feature
        swSelMgr = swModel.SelectionManager
        swDerivedFeat = swSelMgr.GetSelectedObject6(1, -1)
        swComp = swSelMgr.GetSelectedObjectsComponent3(1, -1)
        Debug.Print("Name of derived part feature = " & swDerivedFeat.Name)
        'Get and modify import planes with derived part
        bRet = TestImportPlane(swDerivedFeat, swModel, swComp)
        'Get and modify import absorbed sketches with derived part
        bRet = TestImportAbsorbedSketches(swDerivedFeat, swModel, swComp)
        'Get and modify import unabsorbed sketches with derived part
        bRet = TestImportUnAbsorbedSketches(swDerivedFeat, swModel, swComp)
        swDerivedData = swDerivedFeat.GetDefinition
        Debug.Print("Derived file's path and name = " & swDerivedData.PathName)
    End Sub
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
    Function TestImportPlane(ByVal feat As Feature, ByVal doc As ModelDoc2, ByVal comp As Component2) As Boolean
        Dim featData As DerivedPartFeatureData
        Dim startVal As Boolean
        Dim boolstatus As Boolean

        featData = feat.GetDefinition
        startVal = featData.ImportPlane
        Debug.Print("Import planes with derived part? " & startVal)
        featData.ImportPlane = True
        Debug.Print("Modified import planes with derived part? " & featData.ImportPlane)
        boolstatus = feat.ModifyDefinition(featData, doc, comp)
        featData = Nothing
    End Function
    Function TestImportAbsorbedSketches(ByVal feat As Feature, ByVal doc As ModelDoc2, ByVal comp As Component2) As Boolean
        Dim featData As DerivedPartFeatureData
        Dim startVal As Boolean
        Dim boolstatus As Boolean

        featData = feat.GetDefinition
        startVal = featData.ImportAbsorbedSketches
        Debug.Print("Import absorbed sketches with derived part? " & startVal)
        featData.ImportAbsorbedSketches = True
        Debug.Print("Modified import absorbed sketches with derived part? " & featData.ImportAbsorbedSketches)
        boolstatus = feat.ModifyDefinition(featData, doc, comp)
        featData = Nothing
    End Function
    Function TestImportUnAbsorbedSketches(ByVal feat As Feature, ByVal doc As ModelDoc2, ByVal comp As Component2) As Boolean
        Dim featData As DerivedPartFeatureData
        Dim startVal As Boolean
        Dim boolstatus As Boolean
        featData = feat.GetDefinition
        startVal = featData.ImportUnAbsorbedSketches
        Debug.Print("Import unabsorbed sketches with derived part? " & startVal)
        featData.ImportUnAbsorbedSketches = True
        Debug.Print("Modified import unabsorbed sketches with derived part? " & featData.ImportUnAbsorbedSketches)
        boolstatus = feat.ModifyDefinition(featData, doc, comp)
        featData = Nothing
    End Function
End Class

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:   Modify Derived Part Example (VB.NET)
*   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) 2017 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.