Hide Table of Contents

Create Loft Body Example (VB.NET)

This example shows how to create a loft body using IModeler::CreateLoftBody2.

' ******************************************************************************

' Preconditions:

'       (1) Part document is open.

'       (2) Two closed sketches representing the profiles for the loft body exist.

'       (3) One curve representing a guide curve for the loft body exists.


' Postconditions: Loft body is created and displayed.

' ******************************************************************************

Imports SolidWorks.Interop.sldworks

Imports SolidWorks.Interop.swconst

Imports System

Imports System.Diagnostics


Partial Class SolidWorksMacro


    Public Sub main()


        Dim swModel As ModelDoc2

        Dim swModelDocExt As ModelDocExtension

        Dim swFeatMgr As FeatureManager

        Dim count As Integer

        Dim featArr As Object

        Dim feat1 As Feature

        Dim feat2 As Feature

        Dim feat3 As Feature

        Dim swSelMgr As SelectionMgr

        Dim swModeler As Modeler

        Dim boolstatus As Boolean

        Dim profileIn As Object

        Dim guideCurve As Object

        Dim pProfile(1) As Feature

        Dim pGuide(0) As Feature

        Dim bValue As Boolean

        Dim swBody As Body2

        Dim bIsTempBody As Boolean


        swModeler = swApp.GetModeler

        swModel = swApp.ActiveDoc

        swModelDocExt = swModel.Extension


        ' Select the sketches for the profiles

        ' for the loft body and make them

        ' elements of an array to use to

        ' create the loft body

        swFeatMgr = swModel.FeatureManager

        count = swFeatMgr.GetFeatureCount(False)

        featArr = swFeatMgr.GetFeatures(False)

        swSelMgr = swModel.SelectionManager

        boolstatus = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 0.01432052560262, 0.03232526173853, 0, False, 0, Nothing, 0)

        feat1 = swSelMgr.GetSelectedObject6(1, -1)

        Debug.Print("First profile's feature name:       " & feat1.Name)

        pProfile(0) = feat1

        boolstatus = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)

        feat2 = swSelMgr.GetSelectedObject6(1, -1)

        Debug.Print("Second profile's feature name:      " & feat2.Name)

        pProfile(1) = feat2

        profileIn = pProfile


        ' Select a guide curve for the loft body

        ' and make it an element of an array

        ' to use to create the loft body

        boolstatus = swModelDocExt.SelectByID2("Curve1", "REFERENCECURVES", 0.1353192072154, 0.1043159291966, 0.09477145953832, False, 0, Nothing, 0)

        feat3 = swSelMgr.GetSelectedObject6(1, -1)

        Debug.Print("Guide curve's feature name:         " & feat3.Name)

        pGuide(0) = feat3

        guideCurve = feat3


        ' Create the loft body

        swBody = swModeler.CreateLoftBody2(swModel, profileIn, guideCurve, Nothing, False, 0, 0, 0, True, False, True, False, True, 1, 1, 1, True, True, 1, 1, True)


        ' Test whether the loft body is a temporary body

        bIsTempBody = swBody.IsTemporaryBody

        Debug.Print("Is the loft body a temporary body?  " & bIsTempBody)


        ' Display the loft body

        bValue = swBody.Display3(swModel, 256, swTempBodySelectOptions_e.swTempBodySelectOptionNone)


    End Sub


    ''' <summary>

    ''' The SldWorks swApp variable is pre-assigned for you.

    ''' </summary>

    Public swApp As SldWorks


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:   Create Loft Body 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) 2013 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.