Hide Table of Contents

Rotate and Copy 3D Sketch About Coordinates Example (VB.NET)

This example shows how to rotate and copy 3D sketches.

'--------------------------------------

' Preconditions: Part document with two 3D sketches,

'                named 3DSketch1 and 3DSketch2,

'                is open.

'

' Postconditions:

' 1. 3DSketch2 is copied and rotated around

'    the center point of the 3DSketch1

'    sketch's arc.

' 2. The 3DSketch1 sketch is rotated around the

'    center point of its arc.

'-------------------------------------

Imports SolidWorks.Interop.sldworks

Imports SolidWorks.Interop.swconst

Imports System

Imports System.Diagnostics

 

Partial Class SolidWorksMacro

 

    Public Sub main()

 

        Dim swModel As ModelDoc2

        Dim swSelMgr As SelectionMgr

        Dim swModelDocExt As ModelDocExtension

        Dim swSelData As SelectData

        Dim swSketchMgr As SketchManager

        Dim swSketch As Sketch

        Dim boolStatus As Boolean

        Dim varSketchSegments As Object

        Dim i As Integer

 

        ' If SolidWorks isn't running,

        ' then exit

        If swApp Is Nothing Then Exit Sub

 

        ' Document with two 3D sketches, named 3DSketch2 and

        ' 3DSketch1, is open and active

        swModel = swApp.ActiveDoc

        If swModel Is Nothing Then

            MsgBox("Failed to open document.")

            Exit Sub

        End If

 

        swModelDocExt = swModel.Extension

        swSelMgr = swModel.SelectionManager

        swSelData = swSelMgr.CreateSelectData

        swSketchMgr = swModel.SketchManager

 

        ' Select 3DSketch2 sketch

        boolStatus = swModelDocExt.SelectByID2("3DSketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)

        If boolStatus = False Then

            MsgBox("Failed to select sketch 3DSketch2.")

            Exit Sub

        End If

 

        ' Open 3DSketch2 sketch in edit mode

        swModel.EditSketch()

        swSketch = swSketchMgr.ActiveSketch

        If swSketch Is Nothing Then

            MsgBox("Failed to get pointer to 3DSketch2 sketch.")

            Exit Sub

        End If

 

        ' Select all sketch segments in 3DSketch2 sketch

        varSketchSegments = swSketch.GetSketchSegments()

        For i = 0 To UBound(varSketchSegments)

            boolStatus = varSketchSegments(i).select4(True, swSelData)

            If boolStatus = False Then MsgBox("Failed to select sketch segment instance." & i & ".")

        Next i

 

        ' Copy and rotate 3DSketch2 sketch about center

        ' point of 3DSketch1 sketch's arc

        Debug.Print("Rotating and copying 3DSketch2 sketch about the center point of 3DSketch1's arc? " & swSketchMgr.RotateOrCopy3DAboutXYZ(True, 1, True, -0.09925811702374, 0.004131001848179, 0, 1.5707963267949, 0, 0))

        swModel.ClearSelection2(True)

 

        ' Exit 3DSketch2 sketch

        swSketchMgr.InsertSketch(True)

 

        ' Select 3DSketch1 sketch

        boolStatus = swModelDocExt.SelectByID2("3DSketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)

        If boolStatus = False Then

            MsgBox("Failed to select sketch 3DSketch1.")

            Exit Sub

        End If

 

        ' Edit 3DSketch1 sketch

        swModel.EditSketch()

        swSketch = swModel.GetActiveSketch2

        If swSketch Is Nothing Then

            MsgBox("Failed to get pointer to sketch 3DSketch1.")

            Exit Sub

        End If

 

        ' Select all sketch segments in 3DSketch1 sketch

        varSketchSegments = swSketch.GetSketchSegments()

        For i = 0 To UBound(varSketchSegments)

            boolStatus = varSketchSegments(i).select4(True, swSelData)

            If boolStatus = False Then

                MsgBox("Failed to select sketch segment instance." & i & ".")

                Exit Sub

            End If

        Next i

 

        ' Rotate 3DSketch1 sketch about the

        ' center point of its arc

        Debug.Print("Rotating 3DSketch1 sketch about the center point of its arc? " & swSketchMgr.RotateOrCopy3DAboutXYZ(False, 1, True, -0.09925811702374, 0.004131001848179, 0, 1.5707963267949, 0, 0))

        swModel.ClearSelection2(True)

        ' Exit 3DSketch1 sketch

        swSketchMgr.InsertSketch(True)

 

    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:   Rotate and Copy 3D Sketch About Coordinates 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) 2012 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.