Adds a hole callout at the specified position to the hole whose edge is selected.
.NET Syntax
| Visual Basic (Declaration) | |
|---|
Function AddHoleCallout2( _
ByVal X As System.Double, _
ByVal Y As System.Double, _
ByVal Z As System.Double _
) As System.Object |
| Visual Basic (Usage) | |
|---|
Dim instance As IDrawingDoc
Dim X As System.Double
Dim Y As System.Double
Dim Z As System.Double
Dim value As System.Object
value = instance.AddHoleCallout2(X, Y, Z) |
| C# | |
|---|
System.object AddHoleCallout2(
System.double X,
System.double Y,
System.double Z
) |
| C++/CLI | |
|---|
System.Object^ AddHoleCallout2(
& System.double X,
& System.double Y,
& System.double Z
) |
Parameters
- X
- X position of hole callout in meters
- Y
- Y position of hole callout in meters
- Z
- Z position of hole callout in meters
Return Value
Display dimension representing the hole callout
Example
'VBA
'---------------------------------------------------------
' This example shows how to add a hole callout to
' a hole in a drawing.
'
' Preconditions:
' 1. Open the drawing of a part that contains a hole.
' 2. Select the edge of the hole where to add the callout in the graphics area.
' 3. Open the Immediate window.
'
' Postconditions:
' 1. A hole callout is added to the hole in the drawing.
' 2. Examine the drawing and Immediate window to verify.
' 3. Close the drawing without saving any changes.
'
' Tested using SolidWorks 2011 SP1.
'-----------------------------------------------------------
Option Explicit
Const Xpos As Double = 0.165
Const Ypos As Double = 0.435
Const Zpos As Double = 0#
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swDraw As SldWorks.DrawingDoc
Dim swDispDim As SldWorks.DisplayDimension
Dim swAnn As SldWorks.Annotation
Dim status As Boolean
Dim annType As Long
Set swApp = CreateObject("SldWorks.Application")
Set swModel = swApp.ActiveDoc
Set swModelDocExt = swModel.Extension
Set swDraw = swModel
status = swDraw.ActivateView("Drawing View1")
' Select the edge of the hole where to add the callout
' status = swModelDocExt.SelectByID2("", "EDGE", 0.6280838894175, 0.4565734807731, -499.9234340021, False, 0, Nothing, 0)
Set swDispDim = swDraw.AddHoleCallout2(Xpos, Ypos, Zpos)
Debug.Print "All = " + swDispDim.GetText(swDimensionTextAll)
Debug.Print "Prefix = " + swDispDim.GetText(swDimensionTextPrefix)
Debug.Print "Suffix = " + swDispDim.GetText(swDimensionTextSuffix)
Debug.Print "CalloutAbove = " + swDispDim.GetText(swDimensionTextCalloutAbove)
Debug.Print "CalloutBelow = " + swDispDim.GetText(swDimensionTextCalloutBelow)
Set swAnn = swDispDim.GetAnnotation
annType = swAnn.GetType
Debug.Print "Annotation Type = " + Str(annType)
End Sub
Remarks
See Also
Availability
SOLIDWORKS 2001Plus FCS, Revision Number 10.0