Insert Weldment End Cap Example (VB.NET)
This example shows how to create an end cap on the open face of a structural
member.
'----------------------------------------------------------------------------
' Preconditions:
' 1. Open public_documents\samples\tutorial\api\weldment_box3.sldprt.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Deletes End cap1.
' 2. Inserts End cap3 in the FeatureManager design tree.
' 3. Inspect the Immediate window.
'
' NOTE: Because the model is used elsewhere, do not save changes.
'
---------------------------------------------------------------------------
Imports
SolidWorks.Interop.sldworks
Imports
SolidWorks.Interop.swconst
Imports
System.Runtime.InteropServices
Imports
System
Imports
System.Diagnostics
Partial
Class
SolidWorksMacro
Dim
myFeature As
Feature
Dim
Part As
ModelDoc2
Dim
swEndCap As
EndCapFeatureData
Dim
boolstatus As
Boolean
Sub
main()
Part = swApp.ActiveDoc
boolstatus = Part.Extension.SelectByID2("End
cap1", "BODYFEATURE",
0, 0, 0, False,
0, Nothing,
0)
Part.EditDelete()
Part.ViewZoomTo2(0.632542197290199, 0.972121141705638,
0.0346184961022406, 1.1852319686392, 0.619681287512073, 0.0346184961022431)
boolstatus = Part.Extension.SelectByID2("",
"FACE",
0.58771345904097, 0.614999999999952, -1.01293869257864,
True, 0,
Nothing, 0)
boolstatus = Part.Extension.SelectByID2("",
"FACE",
-0.0124763445314215, 0.614999999999839, -1.0014248149476,
True, 0,
Nothing, 0)
myFeature = Part.FeatureManager.InsertEndCapFeature3(0.005,
False,
False,
0.003, 0.6, 0.003, True,
0.002, False,
2)
swEndCap = myFeature.GetDefinition
Debug.Print("File = "
& Part.GetPathName)
Debug.Print(" "
& myFeature.Name)
Debug.Print(" Chamfer distance
or fillet radius = " &
swEndCap.ChamferDistance * 1000.0# &
" mm")
Debug.Print(" Inset
distance = "
& swEndCap.DepthDistance * 1000.0# &
" mm")
Debug.Print(" Thickness
direction (0=outward, 1=inward, 2=inset) = "
& swEndCap.IsEndCapInward)
Debug.Print(" Offset
distance = "
& swEndCap.OffsetDistance * 1000.0# &
" mm")
Debug.Print(" Thickness of end
cap = " &
swEndCap.Thickness * 1000.0# & "
mm")
Debug.Print(" Thickness ratio
for offset = "
& swEndCap.ThicknessRatioForOffset)
Debug.Print(" Chamfer
corners = "
& swEndCap.UseChamferCorners)
Debug.Print(" Apply corner
treatment = "
& swEndCap.UseCornerTreatment)
Debug.Print(" Reverse
offset = "
& swEndCap.UseReverse)
Debug.Print(" Use thickness
ratio for offset = "
& swEndCap.UseThicknessRatioForOffset)
End
Sub
Public
swApp As
SldWorks
End
Class