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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



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