MACRO LIBRARY

Create points at a curve's intersections

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Create points at a curve intersections

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'Precondition: Two sketches are selected in the FM tree
'Result: A sketch pt is intersected with each combination of sketch segments from both _
    selected sketches
    
'Written by Keith Rice
'CADSharp LLC
'www.cadsharp.com
    
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swSelMgr As SldWorks.SelectionMgr
Dim swSketchFeat As SldWorks.Feature
Dim swSketch1 As SldWorks.Sketch
Dim swSketch2 As SldWorks.Sketch
Dim vSketch1Segs As Variant
Dim vSketch2Segs As Variant
Dim swSketchSeg As SldWorks.SketchSegment
Dim swSketchPt As SldWorks.SketchPoint
Dim i As Integer
Dim j As Integer
Dim strPlane As String
    
Sub main()
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    
    'Error handling
    If swModel Is Nothing Then
        Call ErrorHandler
    End If
    
    Set swSelMgr = swModel.SelectionManager
    If swSelMgr.GetSelectedObjectCount2(-1) <> 2 Then
        Call ErrorHandler
    End If
    For i = 1 To 2
        If swSelMgr.GetSelectedObjectType3(i, -1) <> swSelSKETCHES Then
            Call ErrorHandler
        End If
    Next i
    
    'Get sketch segments
    Set swSketchFeat = swSelMgr.GetSelectedObject6(1, -1)
    Set swSketch1 = swSketchFeat.GetSpecificFeature2
    Set swSketchFeat = swSelMgr.GetSelectedObject6(2, -1)
    Set swSketch2 = swSketchFeat.GetSpecificFeature2
    vSketch1Segs = swSketch1.GetSketchSegments
    vSketch2Segs = swSketch2.GetSketchSegments
    
    'Prompt user for plane on which sketches are located
    strPlane = InputBox _
        ("Enter the exact name of the reference plane on which the selected sketches reside.")
    
    'Create new "results" sketch
    Set swSketchFeat = swModel.FirstFeature
    i = 0
    Do While Not swSketchFeat Is Nothing
        If swSketchFeat.Name = strPlane Then Exit Do
        Set swSketchFeat = swSketchFeat.GetNextFeature
    Loop
    swSketchFeat.Select2 False, 0
    swModel.SketchManager.InsertSketch True
    
    'Prevent snapping
    swModel.SketchManager.AddToDB = False
    
    'Create a sketch pt for each sketch segment in first array
    For i = 0 To UBound(vSketch1Segs)
        For j = 0 To UBound(vSketch2Segs)
            'create sketch pt
            Set swSketchPt = swModel.SketchManager.CreatePoint(1, 1, 0)
            
            'select a seg from first sketch and sketch pt
            Set swSketchSeg = vSketch1Segs(i)
            swSketchSeg.Select4 False, Nothing
            swSketchPt.Select4 True, Nothing
        
            'select a seg from second sketch and sketch pt
            Set swSketchSeg = vSketch2Segs(j)
            swSketchSeg.Select4 True, Nothing
            swSketchPt.Select4 True, Nothing
            
            'add intersection constraint
            swApp.RunCommand swCommands_Add_Constraint_Atinter, Empty
        Next j
    Next i
    
    'exit sketch
    swModel.SketchManager.InsertSketch True
    
    'restore snapping
    swModel.SketchManager.AddToDB = True
End Sub
    
Sub ErrorHandler()
    MsgBox "Please open a part and select two sketches from the FeatureManager tree."
    End
End Sub