Hide Table of Contents

Create Layer for Selected View Example (VBA)

This example shows how to create a layer for the part in the selected drawing view.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Open a drawing of a part.
' 2. Select a drawing view in the FeatureManager design tree.
' 3. Open the Immediate window.
'
' Postconditions:
' 1. Creates a layer for the part in the selected drawing view.
' 2. Click the Layer Properties tool on the Line Format toolbar to verify
'    that the newly created layer is selected in the Layers dialog box.
' 3. Examine the Immediate window.
'----------------------------------------------------------------------------
Option Explicit

 
Private Sub ChangeComponentLayer _
( _
    swApp As SldWorks.SldWorks, _
    swDraw As SldWorks.DrawingDoc, _
    sLayerName As String _
)
    Dim bRet                    As Boolean

    ' Form a valid layer name
    sLayerName = Replace(sLayerName, "/", "_")
    sLayerName = Replace(sLayerName, "@", "_")

    bRet = swDraw.CreateLayer2( _
                sLayerName, _
                "Layer for part in " & sLayerName, _
                0, swLineCONTINUOUS, swLW_NORMAL, True, True)

    ' Change in all drawing views
    swDraw.ChangeComponentLayer sLayerName, True

End Sub

Sub main()

    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swDraw As SldWorks.DrawingDoc
    Dim swSelMgr As SldWorks.SelectionMgr
    Dim swView As SldWorks.View
    Dim swDrawModel As SldWorks.ModelDoc2
    Dim swDrawPart As SldWorks.PartDoc
    Dim vBody As Variant
    Dim swBody As SldWorks.Body2
    Dim swFace As SldWorks.Face2
    Dim swEnt As SldWorks.Entity
    Dim nErrors As Long
    Dim nWarnings As Long
    Dim bRet As Boolean
 

    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swDraw = swModel
    Set swSelMgr = swModel.SelectionManager
    Set swView = swSelMgr.GetSelectedObject6(1, -1)
    Set swDrawModel = swApp.OpenDoc6(swView.GetReferencedModelName, swDocPART, swOpenDocOptions_Silent, "", nErrors, nWarnings)
    Set swDrawPart = swDrawModel

    Debug.Print "File           = " & swModel.GetPathName
    Debug.Print "  View         = " & swView.Name
    Debug.Print "    View Model = " & swView.GetReferencedModelName
   

    vBody = swDrawPart.GetBodies2(swSolidBody, True)

    Set swBody = vBody(0)
    Set swFace = swBody.GetFirstFace
    Set swEnt = swFace

    bRet = swView.SelectEntity(swEnt, False)
   

    ChangeComponentLayer swApp, swDraw, swView.Name

End Sub



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 Layer for Selected View Example (VBA)
*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) 2018 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.