Get Projected Curve Example (VBA)

This example shows how to create and get a projected curve feature on one or more faces.

'--------------------------------------------------------------
' 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. Creates a projected curve feature.
' 5. Gets the projected curve feature.
' 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
Dim faceArr As Variant
Dim eachFace As Variant
Dim swFace As SldWorks.Face2
Dim swEnt As SldWorks.Entity

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
    faceArr = swProjectionCurveFeatureData.FaceArray
    For Each eachFace In faceArr
        Set swFace = eachFace
        Set swEnt = swFace
        status = swEnt.Select4(True, Nothing)
        Debug.Print "Type of entity (2 = face): " & swEnt.GetType
    Next eachFace
    swProjectionCurveFeatureData.ReleaseSelectionAccess

End Sub