Standard Planes on a Toolbar

Here's a modification... in the previous macro, changing that constant only changes which geometry gets selected first.  If reference geometry is already selected, it will still cycle through the features as before rather than going directly to the one specified by FIRSTREF.

Here's one that will only select the geometry specified.  It's one macro with four methods.  When you assign the macro to a button, you need to select the starting method (SelFront, SelTop, etc).  You can make four different buttons, each with a different method.  They'll all call the same selection code, they just pick different geometry.  You don't need to make four copies of the macro, just four buttons.  Or 3 if you just want the planes.  Or however many buttons you want.

'-------------------------------------------------
' Macro to select main reference geometry of an assembly component
' for easy mating.  Modified extensively from the
' "Select Origin of Assembly Component Example (VB)" in
' SolidWorks and Add-Ins API Help
' Preconditions:
'       (1) Assembly document is open.
' Postconditions: One of the reference planes or the
' origin of the last selected component is selected.
' Or, if nothing was selected, reference geometry of the
' top level assembly.
' Change the constant below to specify which piece of ref geometry to select
'--------------------------------------------------
  


'''''''''


Option Explicit
Sub SelFront()
    makeSel 1
End Sub
Sub SelTop()
    makeSel 2
End Sub
Sub SelRight()
    makeSel 3
End Sub
Sub SelOrigin()
    makeSel 4
End Sub


Sub makeSel(FirstRef As Long)
    Dim swApp                       As SldWorks.SldWorks
    Dim swModel                     As SldWorks.ModelDoc2
    Dim swSelMgr                    As SldWorks.SelectionMgr
    Dim swSelComp                   As SldWorks.Component2
    Dim swCompModel                 As SldWorks.ModelDoc2
    Dim swFeat                      As SldWorks.Feature
    Dim bRet                        As Boolean
    Dim GeneralSelObj               As Object
    Dim myFeatureCollection         As New Collection
    Dim i                           As Integer
    Dim CurSelCount                 As Long
    Dim MyTempPointObj              As Object
    Dim mySelStr                    As String
    Dim NewObjToSelect              As Object
    Dim Chunks                      As Variant
    Dim swVer                       As Variant
    Dim ResolveIt                   As Integer
    Dim DocTitle                    As String
  
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
      
    If swModel.GetType <> swDocASSEMBLY Then
        MsgBox "This macro works on assembly documents only."
        Exit Sub
    End If
    
    'This next block of code just gets the component for whatever was las selected (if one is selected)
    'and checks to see if it's suppressed, or if it's lightweight in SW<2006
    Set swSelMgr = swModel.SelectionManager
    CurSelCount = swSelMgr.GetSelectedObjectCount
    If CurSelCount <> 0 Then
        Set GeneralSelObj = swSelMgr.GetSelectedObject(CurSelCount)
        Set swSelComp = swSelMgr.GetSelectedObjectsComponent(CurSelCount)
        If Not swSelComp Is Nothing Then
            If swSelComp.GetSuppression = swComponentSuppressed Then
                MsgBox "Can't get to reference geometry of a suppressed component."
                Exit Sub
            End If
        End If
        swVer = Split(swApp.RevisionNumber, ".")
        If CInt(swVer(0)) < 14 Then
            If swSelComp.GetSuppression <> swComponentFullyResolved Then
                If swSelComp.GetSuppression <> swComponentResolved Then
                    ResolveIt = MsgBox("The component selected is not fully resolved." _
                       & vbCrLf & "This functionality is only available for lightweight" & vbCrLf & _
                       "components in SolidWorks 2006 or greater." & vbCrLf & vbCrLf & _
                       "Resolve this component now?", vbYesNo, "Upgrade Time!")
                    If vbYes = ResolveIt Then
                        swSelComp.SetSuppression2 swComponentFullyResolved
                    Else
                        Exit Sub
                    End If
                End If
            End If
        End If
        swSelMgr.DeSelect CurSelCount
    End If
    
    'If swSelComp is nothing, that means nothing was selected when the macro was run, therefore we
    'need to get the geometry of the top level assembly.  Then we get the first feature of
    'either top level or the selected component for iteration.
    If swSelComp Is Nothing Then
        Set swSelComp = swModel.ConfigurationManager.ActiveConfiguration.GetRootComponent3(False)
        Set swFeat = swModel.FirstFeature
    Else
        Set swFeat = swSelComp.FirstFeature
    End If
      
    'Now we iterate through the features of the component.  If the feature is a plane,
    'and it's not suppressed, we add it to a Collection.  Not selecting anything now,
    'just reading the feature tree.
    Do While Not swFeat Is Nothing
        If ("RefPlane" = swFeat.GetTypeName) And (False = swFeat.IsSuppressed) Then
             myFeatureCollection.Add swFeat
        End If
              
        'This sort of messy "If" block is what we have to do in order to select the origin in an
        'appropriate way for mating.  It's just added to the collection.
        If "OriginProfileFeature" = swFeat.GetTypeName Then
            Chunks = Split(swSelComp.Name2, "/")
            If StrComp(Right(swModel.GetTitle, 7), ".sldasm", vbTextCompare) <> 0 Then
                DocTitle = swModel.GetTitle
            Else
                DocTitle = Left(swModel.GetTitle, Len(swModel.GetTitle) - 7)
            End If
            mySelStr = "Point1@Origin@" & Chunks(0) & "@" & DocTitle
            For i = 0 To (UBound(Chunks) - 1)
                mySelStr = mySelStr & "/" & Chunks(i + 1) & "@" & Left(Chunks(i), (InStrRev(Chunks(i), "-") - 1))
            Next
            swModel.Extension.SelectByID2 mySelStr, "EXTSKETCHPOINT", _
                0, 0, 0, True, 0, Nothing, swSelectOptionDefault
            myFeatureCollection.Add swSelMgr.GetSelectedObject(swSelMgr.GetSelectedObjectCount)
            swModel.Extension.SelectByID2 mySelStr, "EXTSKETCHPOINT", _
                0, 0, 0, True, 0, Nothing, swSelectOptionDefault
            'This was the origin, which is assumed to always follow the 3 standard planes. Stop traversing the tree.
            Exit Do
        End If
        Set swFeat = swFeat.GetNextFeature
    Loop
  
    'At this point (assuming that STOPATORIGIN was left as "true"), we should have a
    'Collection containing 4 items: the three main planes and the origin.
    'Now we just CHOOSE the one that we PLAN to select.  Just to avoid weird errors in case the
    'collection didn't get loaded right,
    'we choose Item #1 to start, but then we go ahead and try to choose the one we wanted
    'per the constant up at the top of the code.  If that "choosing" fails, #1 remains "chosen"
    If NewObjToSelect Is Nothing Then
        Set NewObjToSelect = myFeatureCollection.Item(1)
        On Error Resume Next
        Set NewObjToSelect = myFeatureCollection.Item(FirstRef)
        On Error GoTo 0
    End If
    
    'This is the line that actually selects the item we chose from the collection.
    bRet = NewObjToSelect.Select(True): Debug.Assert bRet
  
End Sub
'-------------------------------------------------