Checking type of face/surface in SW

Hi,

I am a novice user of SolidWorks and frequently encounter situations
where i need to know the type a face / surface in the given model.
Is there a quick way / hack / trick to know whether the given face is
planar or spline.
Similarly, detecting spherical / toroidal / conical faces.
I am not much interested in knowing the surface defining properties
[like normal vector for a planar face, or center of spherical face],
but mainly in type of surface.

Thanks in advance for the reply.
-aditya

 

An easy way to see if it is planar or not is to select it and if the
sketch icon lights up, it's planar.

As for the other types, you can use either convert entities or
intersection curve, then put your mouse over the sketch and it might
show circle, spline, elipse, parabola, etc. Remember that 3D sketches
don't support all entity types, so use a 2D sketch.

 

In general SW does not classify faces in a way that can be easily
checked by a user. So for example if you have imported an IGES file
there is no easy way to determine what type of face is being selected.
However, if the face was created in the feature tree there are ways to
determine face type by implication. For example the analytical
faces/surfaces you mention would likely be made by revolving an arc,
circle or line about an axis. Therefore the feature would be a revolve
and the sketch would contain an arc, circle or line. This can also be
determined through the API. However, it is also possible to create
these features without a revolve. For example a sweep can also create
analytical faces.

See the API help for IsSphere, IsRevolved, IsParametric, IsPlane,
IsSwept, IsTorus, IsCone, IsCylinder etc. There is an example macro
called "Get Parameters of a Toroidal Surface Example (VB)" that you
could use to start with.

Option Explicit

'----------------------------------------------
' Taken from API help and modified to identify face type
'

' Precondition:

' 1) Part, assembly, or drawing document is open.

' 2) Face of toroidal surface is selected.

'

' Postcondition: None

'



Sub main()

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swSelMgr As SldWorks.SelectionMgr

Dim swFace As SldWorks.face2

Dim swSurf As SldWorks.surface

Dim vTorus As Variant

Dim i As Long

Dim bRet As Boolean

Dim lRet As Long

Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swSelMgr = swModel.SelectionManager

If (swSelMgr.GetSelectedObjectType(1) = swSelFACES) Or
(swSelMgr.GetSelectedObjectType(1) = swSelREFSURFACES) Then

Set swFace = swSelMgr.GetSelectedObject5(1)

Set swSurf = swFace.GetSurface

If swSurf.IsTorus Then
lRet = swApp.SendMsgToUser2("Torus", swMbInformation,
swMbOk)

ElseIf swSurf.IsCylinder Then
lRet = swApp.SendMsgToUser2("Cylinder", swMbInformation,
swMbOk)

ElseIf swSurf.IsCone Then
lRet = swApp.SendMsgToUser2("Cone", swMbInformation,
swMbOk)

ElseIf swSurf.IsPlane Then
lRet = swApp.SendMsgToUser2("Plane", swMbInformation,
swMbOk)

ElseIf swSurf.IsRevolved Then
lRet = swApp.SendMsgToUser2("Revolve", swMbInformation,
swMbOk)

ElseIf swSurf.IsParametric Then
lRet = swApp.SendMsgToUser2("Parametric", swMbInformation,
swMbOk)

ElseIf swSurf.IsSphere Then
lRet = swApp.SendMsgToUser2("Sphere", swMbInformation,
swMbOk)

Else
lRet = swApp.SendMsgToUser2("Unknown", swMbInformation,
swMbOk)

End If
Else

lRet = swApp.SendMsgToUser2("Select Face", swMbInformation, swMbOk)

End If

End Sub

 

Thanks for the replies. I will definitely try using your suggestions.
I understand going the API way is a sound method, but in case if
someone has some more tricks to determine the facetypes, please let me
know.

regards,
aditya

 

I added a check in case a face is not selected and a couple more
checks.

Option Explicit

'----------------------------------------------

'

' Precondition:

' 1) Part, assembly, or drawing document is open.

' 2) Face of toroidal surface is selected.

'

' Postcondition: None

'



Sub main()

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swSelMgr As SldWorks.SelectionMgr

Dim swFace As SldWorks.face2

Dim swSurf As SldWorks.surface

Dim vTorus As Variant

Dim i As Long

Dim bRet As Boolean

Dim lRet As Long

Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swSelMgr = swModel.SelectionManager

If (swSelMgr.GetSelectedObjectType(1) = swSelFACES) Or
(swSelMgr.GetSelectedObjectType(1) = swSelREFSURFACES) Then

Set swFace = swSelMgr.GetSelectedObject5(1)

Set swSurf = swFace.GetSurface

If swSurf.IsTorus Then
lRet = swApp.SendMsgToUser2("Torus", swMbInformation,
swMbOk)

ElseIf swSurf.IsCylinder Then
lRet = swApp.SendMsgToUser2("Cylinder", swMbInformation,
swMbOk)

ElseIf swSurf.IsCone Then
lRet = swApp.SendMsgToUser2("Cone", swMbInformation,
swMbOk)

ElseIf swSurf.IsPlane Then
lRet = swApp.SendMsgToUser2("Plane", swMbInformation,
swMbOk)

ElseIf swSurf.IsRevolved Then
lRet = swApp.SendMsgToUser2("Revolve", swMbInformation,
swMbOk)

ElseIf swSurf.IsParametric Then
lRet = swApp.SendMsgToUser2("Parametric", swMbInformation,
swMbOk)

ElseIf swSurf.IsSphere Then
lRet = swApp.SendMsgToUser2("Sphere", swMbInformation,
swMbOk)

ElseIf swSurf.IsSwept Then
lRet = swApp.SendMsgToUser2("Sweep", swMbInformation,
swMbOk)

ElseIf swSurf.IsBlending Then
lRet = swApp.SendMsgToUser2("Blending Face",
swMbInformation, swMbOk)

Else
lRet = swApp.SendMsgToUser2("Unknown", swMbInformation,
swMbOk)

End If
Else

lRet = swApp.SendMsgToUser2("Select Face", swMbInformation, swMbOk)

End If

End Sub

 

Just curious, but why do you need to know this?

I was playing with the macro a bit. One thing I noticed is that the
face type or should I say underlying surface type does not depend on
the feature type as much as what the surface really is. SW seems to try
to simplify down to analytical surfaces as much as possible. So if you
simply put a fillet on the edges of a cube you will get cylindrical and
spherical surfaces for the fillet. If draft is added prior to filleting
you still get cylindrical and spherical. If you put the fillets in the
sketch you get conical and toroidal and I haven't yet checked what
happens when the sketch is swept in a way to produce draft.

 

Did it another way that reveals another surface type. BSurf is added
and swept is not available.

Option Explicit

'----------------------------------------------
' SurfID
' Date By Comment
' 4/2/06 pbk Initial Coding
'
' Precondition:
' 1) Part, assembly, or drawing document is open.
' 2) Face is selected.
'
' Postcondition: None
'
Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2



Sub main()


Dim swSelMgr As SldWorks.SelectionMgr

Dim swFace As SldWorks.face2

Dim swSurf As SldWorks.surface

Dim vTorus As Variant

Dim i As Long

Dim bRet As Boolean

Dim lRet As Long

Dim nID As Long


Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swSelMgr = swModel.SelectionManager

If (swSelMgr.GetSelectedObjectType(1) = swSelFACES) Or
(swSelMgr.GetSelectedObjectType(1) = swSelREFSURFACES) Then

Set swFace = swSelMgr.GetSelectedObject5(1)

Set swSurf = swFace.GetSurface

nID = swSurf.Identity

Select Case nID

Case 4001
Announce ("Plane")

Case 4002
Announce ("Cylinder")

Case 4003
Announce ("Cone")

Case 4004
Announce ("Sphere")

Case 4005
Announce ("Torus")

Case 4006
Announce ("BSurf")

Case 4007
Announce ("Blend")

Case 4008
Announce ("Offset")

Case 4009
Announce ("Extrusion")

Case 40010
Announce ("SRev")

Case Else
Announce ("Unknown")

End Select


Else

Announce ("Select Face")

End If

End Sub


Sub Announce(Text As String)

Dim lRet As Long

lRet = swApp.SendMsgToUser2(Text, swMbInformation, swMbOk)
End Sub

 

THANX a bundle for the macro. I tried using the Macro [which was a new
thing for me] and things are looking perfect !
I'll try writing some macros myself for other things that I am looking
for.
thanks again,
aditya

 

Do we see a light bulb going on? *