Hide Table of Contents

Get Projected Curve Feature Data Example (VBA)

This example shows how to get data for a projected curve feature.

'--------------------------------------------------------------
' Preconditions:
' 1. Verify that the part document exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens the specified part document.
' 2. Selects a face and sketches a spline on that face.
' 3. Selects the sketch of the spline and a face.
' 4. Inserts a projected curve feature.
' 5. Gets some projected curve feature data and prints it
'    to the Immediate window.
' 6. Examine the Immediate window, FeatureManager design tree, and
'    the graphics area.
'
' NOTE: Because the part is used elsewhere, do not save changes.
'----------------------------------------------------------------
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchManager As SldWorks.SketchManager
Dim swSketchSegment As SldWorks.SketchSegment
Dim swFeature As SldWorks.Feature
Dim swSelectionManager As SldWorks.SelectionMgr
Dim swProjectionCurveFeatureData As SldWorks.ProjectionCurveFeatureData
Dim swSketch As SldWorks.Sketch
Dim pointArray As Variant
Dim points(10) As Double
Dim status As Boolean
Dim errors As Long
Dim warnings As Long
Dim fileName As String
Sub main()
    Set swApp = Application.SldWorks    
    'Open part document
    fileName = "C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\api\block20.sldprt"
    Set swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)    
    'Sketch a spline on the selected face
    Set swModelDocExt = swModel.Extension
    status = swModelDocExt.SelectByID2("", "FACE", -4.99223104334874E-02, 3.96239999998897E-02, 7.38137362270663E-03, False, 0, Nothing, 0)
    Set swSketchManager = swModel.SketchManager
    swSketchManager.InsertSketch True
    swModel.ClearSelection2 True
    points(0) = -6.24778997860176E-02
    points(1) = 7.29572078180673E-03
    points(2) = 0
    points(3) = -3.64588790258153E-02
    points(4) = 3.24586288177215E-02
    points(5) = 0
    points(6) = 1.04252377344665E-02
    points(7) = 1.40473535914225E-02
    points(8) = 0
    points(9) = 6.46002912861796E-02
    points(10) = 1.00590221094308E-02
    pointArray = points
    Set swSketchSegment = swSketchManager.CreateSpline2((pointArray), False)
    swSketchManager.InsertSketch True    
    swModel.ClearSelection2 True    
    'Insert projected curve
    status = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, True, 0, Nothing, 0)
    status = swModelDocExt.SelectByID2("", "FACE", -4.97146993259321E-02, 0, -2.56283866693252E-02, True, 0, Nothing, 0)
    Set swFeature = swModel.InsertProjectedSketch2(1)
    'Get projected curve data
    status = swModelDocExt.SelectByID2("Curve1", "REFCURVE", 0, 0, 0, False, 0, Nothing, 0)
    Set swSelectionManager = swModel.SelectionManager
    Set swFeature = swSelectionManager.GetSelectedObject6(1, -1)
    Set swProjectionCurveFeatureData = swFeature.GetDefinition
    swProjectionCurveFeatureData.AccessSelections swModel, Nothing
    Debug.Print "Is reversed = " & swProjectionCurveFeatureData.Reverse
    Debug.Print "Number of targeted faces = " & swProjectionCurveFeatureData.GetFaceArrayCount
    Set swFeature = swProjectionCurveFeatureData.Sketch
    Set swSketch = swFeature.GetSpecificFeature2
    Debug.Print "Name of sketch = " & swFeature.Name
    swProjectionCurveFeatureData.ReleaseSelectionAccess
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:   Get Projected Curve Feature Data 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) 2018 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.