Hide Table of Contents

Create Detail Circle and Detail View Example (VB.NET)

This example shows how to create a detail circle and detail view.

' ---------------------------------------------------------------------------
' Preconditions:
' 1. Specified drawing document exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens specified drawing document.
' 2. Activates Drawing View4.
' 3. Creates detail circle and detail view using the visible
'    corner of Drawing View4.
' 4. Activates detail view.
' 5. Gets detail circle and some properties.
' 6. Examine the drawing document and Immediate window to verify.
'
' NOTE: Because this document is used elsewhere, do not save any changes.
' ----------------------------------------------------------------------------

Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
 
Partial Class SolidWorksMacro
 
    Public Sub Main()
 
        Dim swModel As ModelDoc2
        Dim swDrawing As DrawingDoc
        Dim swSketchManager As SketchManager
        Dim swSketchSegment As SketchSegment
        Dim swView As View
        Dim swDetailCircle As DetailCircle
        Dim swSelMgr As SelectionMgr
       
Dim swSelData As SelectData
        Dim fileName As String
        Dim status As Boolean
        Dim errors As Integer, warnings As Integer
 
        ' Open drawing
        fileName = "C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\samples\tutorial\api\replaceview.slddrw"
        swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocDRAWING, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
        swDrawing = swModel
        swSelMgr = swModel.SelectionManager
        swSelData = swSelMgr.CreateSelectData

        swApp.ActivateDoc3("replaceview - Sheet1"False, swRebuildOnActivation_e.swDontRebuildActiveDoc, errors)
 
        ' Activate Drawing View4 and create detail circle and detail view
        status = swDrawing.ActivateView("Drawing View4")
        swSketchManager = swModel.SketchManager
        swSketchSegment = swSketchManager.CreateCircle(0.007581, 0.053509, 0.0#, 0.013533, 0.016475, 0.0#)
        swView = swDrawing.CreateDetailViewAt3(0.22305342706156, 0.0762140266484527, 0, swDetViewStyle_e.swDetViewSTANDARD, 1, 1, "A", swDetCircleShowType_e.swDetCircleCIRCLE, False)
 
        swModel.ClearSelection2(True)
 
        ' Activate detail view
        status = swDrawing.ActivateView("Drawing View5")
 
        ' Get detail circle and some properties
        swDetailCircle = swView.GetDetail
        Debug.Print("Detail circle:")
        Debug.Print(
"  Selected: " & swDetailCircle.Select(True, Nothing))
        Debug.Print(
"  Label: " & swDetailCircle.GetLabel)
       
Dim xpos as Double
        Dim ypos as Double
   
    swDetailCircle.GetLabelPosition(xpos, ypos)
       
Debug.Print("  Label X position: " & xpos)
        Debug.Print("  Label Y position: " & ypos)
        Debug.Print("  Type of circle: " & swDetailCircle.GetDisplay)
        Debug.Print("  Name: " & swDetailCircle.GetName)
        Debug.Print("  Style: " & swDetailCircle.GetStyle)
        Debug.Print("  Default document text formatting? " & swDetailCircle.GetUseDocTextFormat)

    End Sub
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
 
End Class



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Create Detail Circle and Detail View Example (VB.NET)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2015 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.