Macro to merge sketches using SOLIDWORKS API

This VBA macro merges the selected sketches (3D and 3D) into a single 3D sketch using SOLIDWORKS API. This macro is using convert entities API to copy the entities from the source sketches to a target sketch.

Options

Macro can be configured by changing the values of the constant at the beginning of the macro

DELETE_SOURCE_SKETCHES - True to delete original source sketches, False to not delete
NEW_SKETCH_NAME - Name for the newly generated merged sketch, Empty string to use default auto generated name

Const DELETE_SOURCE_SKETCHES As Boolean = True 'delete all source sketches
Const NEW_SKETCH_NAME As String = "MergedSketch" 'new merged sketch to be named 'MergedSketch'

Notes

Sketches in the assembly or drawings components are also supported
Relations and dimensions from the source sketch are not copied to a target sketch
Sketches are merged to an active 3D sketch, or new 3D sketch is created automatically

Use this macro in conjunction with Select Features By Type to select all sketches to be merged.

Const DELETE_SOURCE_SKETCHES As Boolean = False
Const NEW_SKETCH_NAME As String = ""

Dim swApp As SldWorks.SldWorks

Sub main()

    Set swApp = Application.SldWorks
    
    Dim swModel As SldWorks.ModelDoc2
    
try:
        
    On Error GoTo catch
        
    Set swModel = swApp.ActiveDoc
    
    If Not swModel Is Nothing Then
        MergeSelectedSketches swModel
    Else
        Err.Raise vbError, "", "Please open model"
    End If
    
    GoTo finally
    
catch:
    Debug.Print Err.Number
    swApp.SendMsgToUser2 Err.Description, swMessageBoxIcon_e.swMbStop, swMessageBoxBtn_e.swMbOk
finally:

End Sub

Sub MergeSelectedSketches(model As SldWorks.ModelDoc2)
    
    Dim swSketch As SldWorks.Sketch
        
    If Not model.SketchManager.ActiveSketch Is Nothing Then
        If False = model.SketchManager.ActiveSketch.Is3D() Then
            Err.Raise vbError, "", "Only 3D sketch is supported as a target sketch"
        End If
    End If
    
    Dim vSketchSegs As Variant
    Dim vSketches As Variant
    vSketchSegs = GetSelectedSketchSegments(model, vSketches)
    
    If model.SketchManager.ActiveSketch Is Nothing Then
        model.ClearSelection2 True
        model.SketchManager.Insert3DSketch True
    End If
    
    Dim swTargetSketch As SldWorks.Feature
    
    If model.Extension.MultiSelect2(vSketchSegs, False, Nothing) = UBound(vSketchSegs) + 1 Then
    
        model.SketchManager.SketchUseEdge3 False, False
        
        Set swTargetSketch = model.SketchManager.ActiveSketch
        
        model.SketchManager.ActiveSketch.RelationManager.DeleteAllRelations
                
        model.SketchManager.Insert3DSketch True
    Else
        Err.Raise vbError, "", "Failed to select sketches"
    End If
    
    If DELETE_SOURCE_SKETCHES Then
        If model.Extension.MultiSelect2(vSketches, False, Nothing) = UBound(vSketches) + 1 Then
            model.Extension.DeleteSelection2 swDeleteSelectionOptions_e.swDelete_Absorbed
        Else
            Err.Raise vbError, "", "Failed to selected sketches for deletion"
        End If
    End If
    
    If NEW_SKETCH_NAME <> "" Then
        swTargetSketch.Name = NEW_SKETCH_NAME
    End If
    
End Sub

Function GetSelectedSketchSegments(model As SldWorks.ModelDoc2, ByRef vSketches As Variant) As Variant
    
    Dim swSketches() As SldWorks.Feature
    Dim isSkArrInit As Boolean
    isSkArrInit = False
    
    Dim swSketchSegs() As SldWorks.SketchSegment
    Dim isInit As Boolean
    isInit = False
    
    Dim swSelMgr As SldWorks.SelectionMgr
    Set swSelMgr = model.SelectionManager
    
    Dim i As Integer
    
    For i = 1 To swSelMgr.GetSelectedObjectCount2(-1)
        
        If swSelMgr.GetSelectedObjectType3(i, -1) = swSelectType_e.swSelSKETCHES Then
            
            Dim swFeat As SldWorks.Feature
            Set swFeat = swSelMgr.GetSelectedObject6(i, -1)
            
            If Not isSkArrInit Then
                isSkArrInit = True
                ReDim swSketches(0)
            Else
                ReDim Preserve swSketches(UBound(swSketches) + 1)
            End If
            
            Set swSketches(UBound(swSketches)) = swFeat
            
            Dim swSketch As SldWorks.Sketch
            Set swSketch = swFeat.GetSpecificFeature2
            
            Dim vSegs As Variant
            vSegs = swSketch.GetSketchSegments
            
            Dim j As Integer
            
            If Not IsEmpty(vSegs) Then
                                
                For j = 0 To UBound(vSegs)
                                
                    If Not isInit Then
                        ReDim swSketchSegs(0)
                        isInit = True
                    Else
                        ReDim Preserve swSketchSegs(UBound(swSketchSegs) + 1)
                    End If
                    
                    Set swSketchSegs(UBound(swSketchSegs)) = vSegs(j)
                
                Next
                
            End If
            
        End If
    Next
    
    GetSelectedSketchSegments = swSketchSegs
    
    If isSkArrInit Then
        vSketches = swSketches
    End If
    
End Function