Determine if selected face is hole or boss using SOLIDWORKS API

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Holes and bosses in the body
Holes and bosses in the body

This example demonstrates how to identify if the selected cylindrical face is internal (i.e. hole) or external (i.e. boss) using SOLIDWORKS API.

Select cylindrical face and run the macro. Message box is displayed with the type of the selected face. Macro will work with any face (it is not required for faces to have planar adjacent faces).


This macro identifies if the face is hole or boss based on the direction of the normal of the face. The normals for the holes are always directed towards the cylinder axis, while the normals for the bosses always directed outwards of the cylinder axis.

Macro finds random point on the face (in this example this is a middle between U and V parameters of the face) and normal at this point. After, the vector between this point and the cylinder origin is calculated. If the angle between this vector and normal is less than 90 degrees (PI / 2) than the normal is directed towards the cylinder axis which means that the face is a hole, otherwise (if angle is greater than 90 degrees (PI / 2)) the face is external (boss).

Please see image below:

Normals for the hole and boss
Normals for the hole and boss

Const PI As Double = 3.14159265359

Dim swApp As SldWorks.SldWorks
Dim swMathUtils As SldWorks.MathUtility

Sub main()

    Set swApp = Application.SldWorks
    Set swMathUtils = swApp.GetMathUtility
    Dim swModel As SldWorks.ModelDoc2
    Set swModel = swApp.ActiveDoc
    If Not swModel Is Nothing Then
        Dim swSelMgr As SldWorks.SelectionMgr
        Set swSelMgr = swModel.SelectionManager
        Set swSelMgr = swModel.SelectionManager

        Dim swFace As SldWorks.Face2
        Set swFace = swSelMgr.GetSelectedObject6(1, -1)
        If Not swFace Is Nothing Then
            If IsHole(swFace) Then
                MsgBox "Selected face is hole"
                MsgBox "Selected face is boss"
            End If
            MsgBox "Please select face"
        End If
        MsgBox "Please open the model"
    End If
End Sub

Function IsHole(face As SldWorks.Face2) As Boolean
    Dim swSurf As SldWorks.Surface
    Set swSurf = face.GetSurface
    If swSurf.IsCylinder() Then
        Dim uvBounds As Variant
        uvBounds = face.GetUVBounds
        Dim vEvalData As Variant
        vEvalData = swSurf.Evaluate((uvBounds(1) - uvBounds(0)) / 2, (uvBounds(3) - uvBounds(2)) / 2, 1, 1)
        Dim dPt(2) As Double
        dPt(0) = vEvalData(0): dPt(1) = vEvalData(1): dPt(2) = vEvalData(2)
        Dim sense As Integer
        If False = face.FaceInSurfaceSense() Then
            sense = -1
            sense = 1
        End If
        Dim dNormVec(2) As Double
        dNormVec(0) = vEvalData(UBound(vEvalData) - 2) * sense: dNormVec(1) = vEvalData(UBound(vEvalData) - 1) * sense: dNormVec(2) = vEvalData(UBound(vEvalData)) * sense
        Dim vCylParams As Variant
        vCylParams = swSurf.CylinderParams
        Dim dOrig(2) As Double
        dOrig(0) = vCylParams(0): dOrig(1) = vCylParams(1): dOrig(2) = vCylParams(2)
        Dim dDirVec(2) As Double
        dDirVec(0) = dPt(0) - dOrig(0): dDirVec(1) = dPt(1) - dOrig(1): dDirVec(2) = dPt(2) - dOrig(2)
        Dim swDirVec As MathVector
        Set swDirVec = swMathUtils.CreateVector(dDirVec)
        Dim swNormVec As SldWorks.MathVector
        Set swNormVec = swMathUtils.CreateVector(dNormVec)
        IsHole = GetAngle(swDirVec, swNormVec) < PI / 2
        Err.Raise vbError, , "Selected face is not cylindrical"
    End If
End Function

Function GetAngle(vec1 As MathVector, vec2 As MathVector) As Double
    'cos a= a*b/(|a|*|b|)
    GetAngle = ACos(vec1.Dot(vec2) / (vec1.GetLength() * vec2.GetLength()))
End Function

Function ACos(val As Double) As Double
    If val = 1 Then
        ACos = 0
    ElseIf val = -1 Then
        ACos = 4 * Atn(1)
        ACos = Atn(-val / Sqr(-val * val + 1)) + 2 * Atn(1)
    End If
End Function


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