Hide Table of Contents

Insert Model Annotations Example (VBA)

This example shows how to automatically insert a model's dimensions marked for drawings into a drawing.

'---------------------------------------------------------------------------
' Preconditions:
' 1. Assembly document to open exists.
' 2. Run the macro.
'
' Postconditions:
' 1. A new drawing document is opened.
' 2. A drawing view of the assembly document is created.
' 3. The dimensions in the assembly document that are marked for drawings,
'    including any duplicate dimensions, appear in the drawing view.
' 4. The dimensions in the drawing, which are annotations,
'    are selected and marked.
'---------------------------------------------------------------------------
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swDrawing As SldWorks.DrawingDoc
Dim swSelmgr As SldWorks.SelectionMgr
Dim swView As SldWorks.View
Dim annotations As Variant
Dim annot As Variant
Dim swAnnotation As SldWorks.Annotation
Dim swSelData As SldWorks.SelectData
Dim mark As Long
Dim retval As String
Dim status As Boolean
Sub main()
    Set swApp = Application.SldWorks
    retval = swApp.GetUserPreferenceStringValue(swDefaultTemplateDrawing)
    Set swModel = swApp.NewDocument(retval, 0, 0, 0)
    Set swDrawing = swModel
    Set swModelDocExt = swModel.Extension
    Set swSelmgr = swModel.SelectionManager
    ' Create drawing from assembly
    Set swView = swDrawing.CreateDrawViewFromModelView3("C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\api\wrench.sldasm", "*Front", 0.1314541543147, 0.1407887187817, 0)    
    ' Select and activate the view
    status = swModelDocExt.SelectByID2("Drawing View1", "DRAWINGVIEW", 0, 0, 0, False, 0, Nothing, 0)
    status = swDrawing.ActivateView("Drawing View1")    
    swModel.ClearSelection2 True    
    ' Insert the annotations marked for the drawing
    annotations = swDrawing.InsertModelAnnotations3(0, swInsertDimensionsMarkedForDrawing, True, False, False, False)    
    ' Select and mark each annotation
    Set swSelData = swSelmgr.CreateSelectData
    mark = 0    
    For Each annot In annotations
        Set swAnnotation = annot
        status = swAnnotation.Select3(True, swSelData)
        swSelData.mark = mark
        mark = mark + 1
    Next
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:   Insert Model Annotations 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) 2013 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.