It ain't pretty but gets the job done

' SOLIDWORKS 2016
' This macro will remove sketch entities smaller than a specified length (mm)
' Run the macro whilst editing a sketch OR
' You can select multiple sketches and it will ask for a dimension for each one
' By the way if you remove all the sketch entities SW will delete the sketch
' Warning - I'm a joiner not a programmer, so use at your own risk!
' https://forum.solidworks.com/people/1-2SZI4TC
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swSelMgr As SldWorks.SelectionMgr
Dim swFeature As SldWorks.Feature
Dim bs As Boolean
Sub main()
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    If Not swModel Is Nothing Then
        If Not swModel.SketchManager.ActiveSketch Is Nothing Then
            Call ProcessActiveSketch
        Else 'check selections
             Set swSelMgr = swModel.SelectionManager
            With swSelMgr
                Dim sketchFeatureCollection As New Collection
                Dim i As Integer
                For i = 1 To .GetSelectedObjectCount2(Mark:=-1)
                    If .GetSelectedObjectType3(index:=i, Mark:=-1) = swSelectType_e.swSelSKETCHES Then
                        Set swFeature = .GetSelectedObject6(index:=i, Mark:=-1)
                        Call sketchFeatureCollection.Add(Item:=swFeature)
                    End If
                Next
                Select Case True
                       Case sketchFeatureCollection Is Nothing, sketchFeatureCollection.Count = 0
                                Call swApp.SendMsgToUser2("No Active Sketch or Sketches Selected", swMbStop, swMbOk)
                                Exit Sub
                End Select
            End With 'swSelMgr
            For i = 1 To sketchFeatureCollection.Count
                Set swFeature = sketchFeatureCollection(i)
                bs = swFeature.Select2(Append:=False, Mark:=-1)
                swModel.EditSketch
                Call ProcessActiveSketch
            Next i
        End If
    End If
End Sub
Private Sub ProcessActiveSketch()
    Dim swSketchSegment As SldWorks.SketchSegment
    Dim smallSegmentCount As Integer
    Dim vSegments As Variant
    Dim minLength As Double
    Dim exitLoop As Boolean
    exitLoop = False
    Do Until exitLoop
        With swModel.SketchManager.ActiveSketch
            vSegments = .GetSketchSegments
            swModel.ClearSelection2 True
            Dim userInput As Variant
            userInput = InputBox("Minimum Length(mm)", .Name)
            If userInput = "" Then
                exitLoop = True
            Else
                minLength = CDbl(userInput) / 1000
                smallSegmentCount = 0
                Dim j As Integer
                For j = LBound(vSegments) To UBound(vSegments)
                    Set swSketchSegment = vSegments(j)
                    If swSketchSegment.GetLength < minLength Then
                        smallSegmentCount = smallSegmentCount + 1
                        bs = swSketchSegment.Select4(True, Nothing)
                    End If
                Next j
                Select Case swApp.SendMsgToUser2(smallSegmentCount & " entit" & _
                                                IIf(smallSegmentCount = 1, "y", "ies") & " less than " & minLength * 1000 & "mm selected in " & .Name & vbCr _
                                                & "Delete? - Yes" & vbCr & "Change threshold - No" _
                                                , swMbQuestion, swMbYesNoCancel)
                       Case swMbHitYes: swModel.EditDelete: exitLoop = True
                       Case swMbHitCancel: exitLoop = True
                      'Case swMbHitNo: exitLoop = False
                End Select
            End If
        End With 'ActiveSketch
    Loop
    swModel.SketchManager.InsertSketch True
End Sub