I have struggled with using the "SelectionManager" (not IModelDoc2::ISelectionManager from the API) feature of Solidworks through the API, and it's been hard to research considering SolidWorks named the feature the same as the interface. I have also struggled with the Sweep-Thin using a Circular Profile for the Sweep feature. both ideas are relatively new to SolidWorks, but are very powerful, especially in my profession of round tubular bending.
Here's a VBA macro that exposes both functions with some info on what's going on.
You can use the attached "Sweep-Thin.SLDPRT" to make your selections from different sketches.
' creates a basic Sweep-Thin feature using "Circular Profile"
' through selected path of sketch lines of uncommon sketches.
' Sequentially select a series of lines for sweep path.
' Change "ThinSweep" values as necessary.
' Sweep/Sweep-Thin Feature using "Open Group" and Circular Profile.
Dim swApp As SldWorks.SldWorks
Dim swModel As ModelDoc2
Dim swSelMgr As SelectionMgr
Dim vSkLines As Variant
Dim swSkSeg As SketchSegment
Dim j As Integer
Dim b As Boolean
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
If swModel Is Nothing Then End
If swModel.GetType <> swconst.swDocumentTypes_e.swDocPART Then
MsgBox "Run in part only."
Set swSelMgr = swModel.SelectionManager
j = swSelMgr.GetSelectedObjectCount2(-1)
If j = 0 Then
MsgBox "Please select a series of lines for sweep."
ReDim vSkLines(j - 1) As Variant
For i = 0 To j - 1
If swSelMgr.GetSelectedObjectType3((i + 1), -1) <> swSelEXTSKETCHSEGS Then
MsgBox "Non-SketchSegment selected." & vbCrLf & "Macro will End"
Set vSkLines(i) = swSelMgr.GetSelectedObject6((i + 1), -1)
For i = 0 To j - 1
swModel.Extension.SelectByID2 LineName(vSkLines(i)), "SKETCHSEGMENT", 0, 0, 0, True, 4, Nothing, 0
'Store selected entities as a selected Object Group for Path.
'Mark as "4" to identify as path for sweep
swModel.Extension.SelectByID2 "Unknown", "SELOBJGROUP", 0, 0, 0, False, 4, Nothing, 0
b = ThinSweep(0.006, 0.001, True)
If (b = False) Then MsgBox ("Feature not created")
Function LineName(ByVal line As SketchLine) As String
Set swSkSeg = line
Dim swSketch As Sketch
Set swSketch = swSkSeg.GetSketch
Dim swFeat As Feature
Set swFeat = swSketch
Dim strname As String
strname = (swSkSeg.GetName & "@" & swFeat.Name)
LineName = strname
Function ThinSweep(ByVal diameter As Double, ByVal thickness As Double, ByVal merge As Boolean) As Boolean
Dim swFeatMgr As FeatureManager
Set swFeatMgr = swModel.FeatureManager
Dim swFeatData As SweepFeatureData
Set swFeatData = swFeatMgr.CreateDefinition(swFeatureNameID_e.swFmSweep)
swFeatData.AdvancedSmoothing = False
swFeatData.AlignWithEndFaces = 0
swFeatData.AutoSelect = True
swFeatData.CircularProfile = True
swFeatData.CircularProfileDiameter = diameter
swFeatData.D1ReverseTwistDir = False
swFeatData.EndTangencyType = 0
swFeatData.FeatureScope = True
swFeatData.MaintainTangency = False
swFeatData.merge = merge
swFeatData.MergeSmoothFaces = True
swFeatData.PathAlignmentType = 10
swFeatData.StartTangencyType = 0
swFeatData.ThinWallType = 0
swFeatData.TwistControlType = 0
swFeatData.ThinFeature = False
If thickness > 0 Then
swFeatData.ThinFeature = True
swFeatData.SetWallThickness True, thickness
Set swFeat = swFeatMgr.CreateFeature(swFeatData)
If Not swFeat Is Nothing Then ThinSweep = True
If you have any suggestions for more reliable/simpler code, please feel free to contact me.