Determine if Sketch Suitable for Feature Example (VBA)
This example shows how to determine if a sketch is suitable for use
in a feature.
'------------------------------------------------
'
' Problem:
' Sketch
geometry can be used in a variety of ways in SOLIDWORKS.
' However,
not every sketch is suitable for every purpose.
' For
example, (non-thin) extrusions require a closed profile.
'
' This
code shows how to check a sketch to determine
' if
it can be used in various features.
'
' Preconditions:
' 1)
Part or assembly is open
' 2)
Sketch is selected
'
' Postconditions: None
'
'--------------------------------------------------
Option Explicit
' List of feature types to be used with the Sketch::CheckFeatureUse
Public Enum swSketchCheckFeatureProfileUsage_e
swSketchCheckFeature_UNSET
= 0
swSketchCheckFeature_BASEEXTRUDE
= 1
swSketchCheckFeature_BASEEXTRUDETHIN
= 2
swSketchCheckFeature_BOSSEXTRUDE
= 3
swSketchCheckFeature_BOSSEXTRUDETHIN
= 4
swSketchCheckFeature_SURFACEEXTRUDE
= 5
swSketchCheckFeature_BASEREVOLVE
= 6
swSketchCheckFeature_BASEREVOLVETHIN
= 7
swSketchCheckFeature_BOSSREVOLVE
= 8
swSketchCheckFeature_BOSSREVOLVETHIN
= 9
swSketchCheckFeature_SURFACEREVOLVE
= 10
swSketchCheckFeature_CUTEXTRUDE
= 11
swSketchCheckFeature_CUTEXTRUDETHIN
= 12
swSketchCheckFeature_CUTREVOLVE
= 13
swSketchCheckFeature_CUTREVOLVETHIN
= 14
swSketchCheckFeature_SWEEPSECTION
= 15
swSketchCheckFeature_SURFACESWEEPSECTION
= 16
swSketchCheckFeature_SWEEPPATHORGUIDE
= 17
swSketchCheckFeature_LOFTSECTION
= 18
swSketchCheckFeature_SURFACELOFTSECTION
= 19
swSketchCheckFeature_LOFTGUIDE
= 20
swSketchCheckFeature_RIBSECTION
= 21
swSketchCheckFeature_SHEETMETAL_BASEFLANGE
= 22
End Enum
' A list of return status values for the Sketch::CheckFeatureUse
API
Public Enum swSketchCheckFeatureStatus_e
swSketchCheckFeatureStatus_UnknownError
= -1
swSketchCheckFeatureStatus_OK
= 0
swSketchCheckFeatureStatus_EntXEnt
= 1
swSketchCheckFeatureStatus_EntXSelf
= 2
swSketchCheckFeatureStatus_EntUnspecBad
= 3
swSketchCheckFeatureStatus_ThreeEnts
= 4
swSketchCheckFeatureStatus_EmptySketch
= 5
swSketchCheckFeatureStatus_WrongOpen
= 6
swSketchCheckFeatureStatus_WrongManyContours
= 7
swSketchCheckFeatureStatus_ZeroLengthEnt
= 8
swSketchCheckFeatureStatus_ManyOpen
= 9
swSketchCheckFeatureStatus_NoOpen
= 10
swSketchCheckFeatureStatus_MixedContours
= 11
swSketchCheckFeatureStatus_CturXCtur
= 12
swSketchCheckFeatureStatus_DisjCturs
= 13
swSketchCheckFeatureStatus_OpenWantClosed
= 14
swSketchCheckFeatureStatus_ClosedWantOpen
= 15
swSketchCheckFeatureStatus_DoubleContainment
= 16
swSketchCheckFeatureStatus_MoreThanOneContour
= 17
swSketchCheckFeatureStatus_OneOpenContourExpected
= 18
swSketchCheckFeatureStatus_OneClosedContourExpected
= 19
swSketchCheckFeatureStatus_WantSingleOpenOrMultiClosedDisjoint
= 20
swSketchCheckFeatureStatus_NeedsAxis
= 21
swSketchCheckFeatureStatus_OpenOrUnclear
= 22
swSketchCheckFeatureStatus_ContourIntersectsCenterLine
= 23
End Enum
Sub main()
Dim
swApp As
SldWorks.SldWorks
Dim
swModel As
SldWorks.ModelDoc
Dim
swSelMgr As
SldWorks.SelectionMgr
Dim
swFeat As
SldWorks.Feature
Dim
swSketch As
SldWorks.sketch
Dim
nRetVal As
Long
Dim
nOpenCount As
Long
Dim
nClosedCount As
Long
Dim
i As
Long
Set
swApp = CreateObject("SldWorks.Application")
Set
swModel = swApp.ActiveDoc
Set
swSelMgr = swModel.SelectionManager
Set
swFeat = swSelMgr.GetSelectedObject5(1)
Set
swSketch = swFeat.GetSpecificFeature2
Debug.Print
"Feature = " & swFeat.Name
For
i = 0 To 22
nRetVal
= swSketch.CheckFeatureUse(i,
_
nOpenCount,
nClosedCount)
Debug.Print
" FeatCheckType
= "
& i
Debug.Print
" RetVal
=
" & nRetVal
Debug.Print
" OpenCount
=
" & nOpenCount
Debug.Print
" ClosedCount
= "
& nClosedCount
Debug.Print
""
Next
i
Debug.Print
"---------------------------------------"
End Sub
'------------------------------------------------