Insert Reference Plane Example (VB.NET)
This example shows how to create a constraint-based, angle, reference
plane.
'
--------------------------------------------------------------------------
' Preconditions:
' 1.
Specified file exists on your system.
' 2.
Run the macro (press F5).
' 3.
Examine the Immediate window to find out the
type of
' reference plane created.
'
' Postconditions: Constraint-based reference plane is
created.
'
' NOTE: Because the specified SolidWorks document is
' used
in a SolidWorks online tutorial, do not
' save
any changes when closing the document,
'
--------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System
Imports System.Diagnostics
Partial Class SolidWorksMacro
Public
Sub main()
Dim
swModel As ModelDoc2
Dim
swModelDocExt As ModelDocExtension
Dim
swFeatureManager As FeatureManager
Dim
swFeature As Feature
Dim
swRefPlane As RefPlane
Dim
swSelMgr As SelectionMgr
Dim
swRefPlaneFeatureData As RefPlaneFeatureData
Dim
fileerror As Long
Dim
filewarning As Long
Dim
boolstatus As Boolean
Dim
planeType As Long
swApp.OpenDoc6("c:\Program Files\SolidWorks
Corp\SolidWorks\samples\tutorial\api\plate.sldprt", swDocumentTypes_e.swDocPART,
swOpenDocOptions_e.swOpenDocOptions_Silent, "", fileerror, filewarning)
swModel
= swApp.ActiveDoc
swModelDocExt
= swModel.Extension
swFeatureManager
= swModel.FeatureManager
swSelMgr
= swModel.SelectionManager
'
Create a constraint-based reference plane
boolstatus
= swModelDocExt.SelectByID2("",
"FACE", 0.028424218552, 0.07057725774359, 0, True, 0, Nothing,
0)
boolstatus
= swModelDocExt.SelectByID2("",
"EDGE", 0.05976462601598, 0.0718389621656, 0.0001242036435087,
True, 1, Nothing, 0)
swRefPlane
= swFeatureManager.InsertRefPlane(16,
0.7853981633975, 4, 0, 0, 0)
'
Get type of the just-created reference plane
boolstatus
= swModelDocExt.SelectByID2("Plane1",
"PLANE", 0, 0, 0, False, 0, Nothing, swSelectOption_e.swSelectOptionDefault)
swFeature
= swSelMgr.GetSelectedObject6(1,
-1)
swRefPlaneFeatureData
= swFeature.GetDefinition
planeType
= swRefPlaneFeatureData.Type2
Debug.Print("Type
of reference plane using IRefPlaneFeatureData::Type2: ")
Select
Case planeType
Case
0
Debug.Print("
Invalid")
Case
1
Debug.Print("
Undefined")
Case
2
Debug.Print("
Line Point")
Case
3
Debug.Print("
Three Points")
Case
4
Debug.Print("
Line Line")
Case
5
Debug.Print("
Distance")
Case
6
Debug.Print("
Parallel")
Case
7
Debug.Print("
Angle")
Case
8
Debug.Print("
Normal")
Case
9
Debug.Print("
On Surface")
Case
10
Debug.Print("
Standard")
Case
11
Debug.Print("
Constraint-based")
End
Select
Debug.Print("")
planeType
= swRefPlaneFeatureData.Type
Debug.Print("Type
of reference plane using IRefPlaneFeatureData::Type: ")
Select
Case planeType
Case
0
Debug.Print("
Invalid")
Case
1
Debug.Print("
Undefined")
Case
2
Debug.Print("
Line Point")
Case
3
Debug.Print("
Three Points")
Case
4
Debug.Print("
Line Line")
Case
5
Debug.Print("
Distance")
Case
6
Debug.Print("
Parallel")
Case
7
Debug.Print("
Angle")
Case
8
Debug.Print("
Normal")
Case
9
Debug.Print("
On Surface")
Case
10
Debug.Print("
Standard")
Case
11
Debug.Print("
Constraint-based")
End
Select
Debug.Print("")
swModel.ClearSelection2(True)
End
Sub
'''
<summary>
'''
The SldWorks swApp variable is pre-assigned for you.
'''
</summary>
Public
swApp As SldWorks
End Class