Hide Table of Contents

Insert Protrusion Blend Example (VBA)

This example shows how to create a loft using profiles, guide curves, and a centerline.

'---------------------------------------------------------------
' Preconditions: Verify that the specified part template exists.
'
' Postconditions:
' 1. Creates a new part.
' 2. Creates a profile sketch.
' 3. Creates a reference plane and another profile sketch on that
'    reference plane.
' 4. Creates five curves: four guide curves and one centerline.
' 5. Selects the profile sketches, four guide curves, and the 
'    centerline.
' 6. Creates a loft feature.
' 7. Examine the FeatureManager design tree and graphics area.
'---------------------------------------------------------------
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchSegment As SldWorks.SketchSegment
Dim swSketchManager As SldWorks.SketchManager
Dim swRefPlane As SldWorks.RefPlane
Dim swFeatureManager As SldWorks.FeatureManager
Dim status As Boolean

Sub main()
    Set swApp = Application.SldWorks    
    'Create new part
    Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2016\templates\Part.prtdot", 0, 0, 0)
    'Create profile sketch
    Set swModelDocExt = swModel.Extension
    status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    swModel.ClearSelection2 True
    Set swSketchManager = swModel.SketchManager
    Set swSketchSegment = swSketchManager.CreateEllipse(0, 0, 0, 7.06113079019074E-02, 0, 0, 0, 3.74944141689373E-02, 0)
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True    
    ' Create reference plane and another profile sketch
    ' on that reference plane
    status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
    Set swFeatureManager = swModel.FeatureManager
    Set swRefPlane = swFeatureManager.InsertRefPlane(8, 0.07, 0, 0, 0, 0)
    swModel.ClearSelection2 True
    status = swModelDocExt.SelectByID2("Plane1", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Set swSketchSegment = swSketchManager.CreateEllipse(0, 0, 0, 5.27205722070845E-02, 0, 0, 0, 1.54164850136235E-02, 0)
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True    
    ' Create guide curves
    status = swModelDocExt.SelectByID2("Point4@Sketch1", "EXTSKETCHPOINT", 0, 3.74944141689373E-02, 0, False, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Point4@Sketch2", "EXTSKETCHPOINT", 0, 1.54164850136235E-02, 0, True, 1, Nothing, 0)
    swModel.Insert3DSplineCurve False    
    status = swModelDocExt.SelectByID2("Point5@Sketch2", "EXTSKETCHPOINT", -5.27205722070845E-02, 0, 0, True, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Point5@Sketch1", "EXTSKETCHPOINT", -7.06113079019074E-02, 0, 0, True, 1, Nothing, 0)
    swModel.Insert3DSplineCurve False    
    status = swModelDocExt.SelectByID2("Point6@Sketch2", "EXTSKETCHPOINT", 0, -1.54164850136235E-02, 0, True, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Point6@Sketch1", "EXTSKETCHPOINT", 0, -3.74944141689373E-02, 0, True, 1, Nothing, 0)
    swModel.Insert3DSplineCurve False    
    status = swModelDocExt.SelectByID2("Point3@Sketch2", "EXTSKETCHPOINT", 5.27205722070845E-02, 0, 0, True, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Point3@Sketch1", "EXTSKETCHPOINT", 7.06113079019074E-02, 0, 0, True, 1, Nothing, 0)
    swModel.Insert3DSplineCurve False    
    ' Create centerline
    status = swModelDocExt.SelectByID2("Point2@Sketch2", "EXTSKETCHPOINT", 0, 0, 0, True, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Point2@Sketch1", "EXTSKETCHPOINT", 0, 0, 0, True, 1, Nothing, 0)
    swModel.Insert3DSplineCurve False    
    ' Create loft
    status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 7.06113079019074E-02, 0, 0, False, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 5.27205722070845E-02, 0, 0.07, True, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Curve1", "REFERENCECURVES", 9.99754519565386E-02, 4.47609702560072E-02, 0.128010464418594, True, 4098, Nothing, 0)
    status = swModelDocExt.SelectByID2("Curve2", "REFERENCECURVES", 0.037643674311596, 2.21603475855119E-02, 0.115437869126538, True, 8194, Nothing, 0)
    status = swModelDocExt.SelectByID2("Curve3", "REFERENCECURVES", 9.99909384372586E-02, -7.44308680111772E-04, 0.131301605626447, True, 12290, Nothing, 0)
    status = swModelDocExt.SelectByID2("Curve4", "REFERENCECURVES", 0.158600974878482, 2.18780932746938E-02, 0.129235804629445, True, 16386, Nothing, 0)
    status = swModelDocExt.SelectByID2("Curve5", "REFERENCECURVES", 9.98735089003162E-02, 0.022159545044488, 0.108064927518626, True, 4, Nothing, 0)
    swFeatureManager.InsertProtrusionBlend False, True, False, 1, 0, 0, 1, 1, True, True, False, 0, 0, 0, True, True, True
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:   Insert Protrusion Blend 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) 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.