Insert Fill-surface Feature Example (VBA)

This example shows how to insert a fill-surface feature.

'--------------------------------------------------
' Preconditions: Ensure that the part template file named 
' part.prtdot exists in the specified path.
'
' Postconditions:
' 1. Sketches a circle on the Front Plane.
' 2. Offsets the Front Plane to create Plane1.
' 3. Sketches a circle on Plane1.
' 4. Creates a thin-feature loft using the circles
'    created in steps 1 and 3.
' 5. Selects one of the sketches to use for
'    the fill-surface feature.
' 6. Creates a fill-surface feature named Surface-Fill1.
' 7. To verify step 6, examine the FeatureManager
'    design tree.
'---------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSelMgr As SldWorks.SelectionMgr
Dim swSketchMgr As SldWorks.SketchManager
Dim swSketchSegment As SldWorks.SketchSegment
Dim swFeatMgr As SldWorks.FeatureManager
Dim swRefPlane As SldWorks.RefPlane
Dim swFeat As SldWorks.Feature
Dim selObj As Object
Dim status As Boolean

Sub main()

    Set swApp = Application.SldWorks    

    'Open a new model document
    Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2014\templates\part.prtdot", swDwgPaperAsize, 0, 0)    

    'Select the front plane and sketch a circle
    Set swModelDocExt = swModel.Extension
    status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)
    swModel.ClearSelection2 True
    Set swSketchMgr = swModel.SketchManager
    Set swSketchSegment = swSketchMgr.CreateCircle(0#, 0#, 0#, 0.018863, -0.048015, 0#)
    swModel.ClearSelection2 True
    swSketchMgr.InsertSketch True    

    'Offset the front plane to create Plane1
    status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
    Set swFeatMgr = swModel.FeatureManager
    Set swRefPlane = swFeatMgr.InsertRefPlane(8, 0.0762, 0, 0, 0, 0)
    status = swModelDocExt.SelectByID2("Plane1", "PLANE", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)
    Set swSketchSegment = swSketchMgr.CreateCircle(0#, 0#, 0#, 0.005144, -0.017148, 0#)
    swModel.ClearSelection2 True
    swSketchMgr.InsertSketch True    

    'Create a loft as a thin feature
    status = swModelDocExt.SelectByID2("Sketch2", "SKETCH", -1.20997659765269E-02, 1.31954647737917E-02, 0, False, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", -1.37458916138411E-02, 4.97220981864567E-02, 0, True, 1, Nothing, 0)
    swFeatMgr.InsertProtrusionBlend2 False, True, False, 1, 0, 0, 1, 1, True, True, True, 0.000254, 0.000254, 0, True, True, True, swGuideCurveInfluence_e.swGuideCurveInfluenceNextEdge    

    'Get the sketch for the fill-surface feature
    status = swModelDocExt.SelectByID2("Sketch2", "SKETCH", -3.09259362651374E-02, -1.50632202505945E-02, 2.65529245975468E-02, True, 257, Nothing, swSelectOptionDefault)
    Set swSelMgr = swModel.SelectionManager
    Set selObj = swSelMgr.GetSelectedObject6(1, 257)    

    'Insert the fill-surface feature
    Set swFeat = swFeatMgr.InsertFillSurface2(2, swOptimizeSurface, selObj, swContact, Nothing, Nothing)    

End Sub