Solid Edge ST7 SDK
Working with DrawingViews
Programmer's Guide > Solid Edge > Environments > Draft > Working with DrawingViews

A DrawingView object is a 2-D representation of a 3-D part or assembly model. A drawing view is used to display design space geometry in document space. A view of design space is enclosed by the drawing view border (a handle that allows manipulation of the drawing view). Only one part or assembly document can be used as the basis for drawing views in a draft document.

See Handling 'Application is Busy' and 'Call was Rejected By Callee' errors for information regarding the use of OleMessageFilter.
DrawingViews in Visual Basic .NET
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Imports SolidEdgeFramework
Imports System.Runtime.InteropServices

Module Program
    <STAThread()> _
    Sub Main()
        Dim objApplication As SolidEdgeFramework.Application = Nothing
        Dim objDocuments As SolidEdgeFramework.Documents = Nothing
        Dim objDraft As SolidEdgeDraft.DraftDocument = Nothing
        Dim objSheet As SolidEdgeDraft.Sheet = Nothing
        Dim objModelLinks As SolidEdgeDraft.ModelLinks = Nothing
        Dim objModelLink As SolidEdgeDraft.ModelLink = Nothing
        Dim objDrawingViews As SolidEdgeDraft.DrawingViews = Nothing
        Dim objDrawingView As SolidEdgeDraft.DrawingView = Nothing

        Try
            OleMessageFilter.Register()

            ' Connect to a running instance of Solid Edge
            objApplication = Marshal.GetActiveObject("SolidEdge.Application")

            ' Get a reference to the documents collection
            objDocuments = objApplication.Documents

            ' Add a Draft document      
            objDraft = objDocuments.Add("SolidEdge.DraftDocument")

            ' Get a reference to the active sheet
            objSheet = objDraft.ActiveSheet

            ' Get a reference to the model links collection
            objModelLinks = objDraft.ModelLinks

            ' Add a new model link
            objModelLink = objModelLinks.Add("C:\Part1.par")

            ' Get a reference to the drawing views collection
            objDrawingViews = objSheet.DrawingViews

            ' Add a new drawing view
            objDrawingView = objDrawingViews.AddPartView( _
              objModelLink, _
              SolidEdgeDraft.ViewOrientationConstants.igFrontView, _
              1, _
              0.1, _
              0.1, _
              SolidEdgeDraft.PartDrawingViewTypeConstants.sePartDesignedView)

            ' Assign a caption
            objDrawingView.Caption = "My New Drawing View"

            ' Ensure caption is displayed
            objDrawingView.DisplayCaption = True

        Catch ex As Exception
            Console.WriteLine(ex.Message)
        Finally
            OleMessageFilter.Revoke()
        End Try
    End Sub
End Module
DrawingViews in C#
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using SolidEdgeFramework;
using System;
using System.Reflection;
using System.Runtime.InteropServices;

namespace SolidEdge.SDK
{
    class Program
    {
        [STAThread]
        static void Main(string[] args)
        {
            SolidEdgeFramework.Application application = null;
            SolidEdgeFramework.Documents documents = null;
            SolidEdgeDraft.DraftDocument draft = null;
            SolidEdgeDraft.Sheet sheet = null;
            SolidEdgeDraft.ModelLinks modelLinks = null;
            SolidEdgeDraft.ModelLink modelLink = null;
            SolidEdgeDraft.DrawingViews drawingViews = null;
            SolidEdgeDraft.DrawingView drawingView = null;

            try
            {
                OleMessageFilter.Register();

                // Connect to a running instance of Solid Edge
                application = (SolidEdgeFramework.Application)
                    Marshal.GetActiveObject("SolidEdge.Application");

                // Get a reference to the documents collection
                documents = application.Documents;

                // Add a Draft document
                draft = (SolidEdgeDraft.DraftDocument)
                    documents.Add("SolidEdge.DraftDocument", Missing.Value);

                // Get a reference to the active sheet
                sheet = draft.ActiveSheet;

                // Get a reference to the model links collection
                modelLinks = draft.ModelLinks;

                // Add a new model link
                modelLink = modelLinks.Add(@"C:\Part1.par");

                // Get a reference to the drawing views collection
                drawingViews = sheet.DrawingViews;

                // Add a new drawing view
                drawingView = drawingViews.AddPartView(
                    modelLink,
                    SolidEdgeDraft.ViewOrientationConstants.igFrontView,
                    1,
                    0.1,
                    0.1,
                    SolidEdgeDraft.PartDrawingViewTypeConstants.sePartDesignedView);

                // Assign a caption
                drawingView.Caption = "My New Drawing View";

                // Ensure caption is displayed
                drawingView.DisplayCaption = true;

            }
            catch (System.Exception ex)
            {
                Console.WriteLine(ex.Message);
            }
            finally
            {
                OleMessageFilter.Revoke();
            }
        }
    }
}