Manufacturing DevBlog

Print drawing with custom size

By Xiaodong Liang

PrintManager allows you customize the papaer size in the condition PrintManager.PaperSize is kPaperSizeCustom. The following code is copied from the VBA demo in API help reference. It demonstrates how to print a drawing with custom size, including setting specifics such as sheet range.

Public Sub PrintDrawing()

 

    _InvApplication = _

Runtime.InteropServices.Marshal. _

GetActiveObject("Inventor.Application")

 

    ' assumes you have had Inventor application

 

    ' Set a reference to the print manager

    ' object of the active document.

    ' This will fail if a drawing document is

    'not active.

    Dim oPrintMgr As DrawingPrintManager

    oPrintMgr = _InvApplication.ActiveDocument.PrintManager

 

    ' Get the name of the printer that will be used.

    If MsgBox("Using printer """ & oPrintMgr.Printer &

                """  Do you want to continue?",

                vbYesNo + vbQuestion) = vbNo Then

        ' Change to another printer.

        Dim sPrinterName As String

        sPrinterName = InputBox(

            "Enter name of new printer:", "New Printer")

        If sPrinterName = "" Then

            Exit Sub

        Else

            oPrintMgr.Printer = sPrinterName

        End If

    End If

 

    ' Set to print in color.

    oPrintMgr.ColorMode =

        PrintColorModeEnum.kPrintColorPalette

 

    ' Set to print two copies.

    oPrintMgr.NumberOfCopies = 2

 

    ' Set to print using portrait orientation.

    oPrintMgr.Orientation =

        PrintOrientationEnum.kPortraitOrientation

 

    ' Set the paper size.

    oPrintMgr.PaperSize =

        PaperSizeEnum.kPaperSize11x17

 

    ' Set to print all sheets.

    oPrintMgr.PrintRange =

        PrintRangeEnum.kPrintAllSheets

 

    ' Set to print full scale.

    oPrintMgr.ScaleMode =

        PrintScaleModeEnum.kPrintFullScale

 

    ' Submit the print.

    oPrintMgr.SubmitPrint()

 

    ' Change the number of copies to 1.

    oPrintMgr.NumberOfCopies = 1

 

    ' Change the paper size to a custom size.  The units are in centimeters.

    oPrintMgr.PaperSize =

        PaperSizeEnum.kPaperSizeCustom

    oPrintMgr.PaperHeight = 15

    oPrintMgr.PaperWidth = 10

 

    ' Get and set the current sheet range.

    Dim iFromSheet As Long

    Dim iToSheet As Long

    Call oPrintMgr.GetSheetRange(

        iFromSheet, iToSheet)

 

    MsgBox("Current sheet range is " & iFromSheet &

            " to " & iToSheet & Chr(13) & _

            "Setting to print sheets 1-2.")

 

    ' Change the print range to print sheets 1 through 2.

    oPrintMgr.PrintRange =

        PrintRangeEnum.kPrintSheetRange

    Call oPrintMgr.SetSheetRange(1, 2)

 

    ' Submit the print.

    oPrintMgr.SubmitPrint()

End Sub

 

AddRestriction() is not added correctly for several events in the Vault 2012 RestrictOperations SDK sample

By Wayne Brill

Applies to:
Autodesk® Vault Collaboration 2012
Autodesk® Vault Professional 2012
Autodesk® Vault Workgroup 2012

Issue

I am using the RestrictOperations SDK sample. AddRestriction() is not getting added for the UpdateFileLifeCycleState event even though it is checked in the Configurator. Is there a way to get this to work in the sample?

Solution

There is a typo in Configulator tool, and was fixed in the 2013 release.

This code snippet is from Form1.cs and is a list of strings that is used to determine which event will be restricted by a call to AddRestriction(). Notice that the "c" in "UpdateFileLifecycleState" is lower case.

public partial class Form1 : Form

{

  private List<string> m_commands =

                  new List<string>()

     {

        // File commands

            "AddFile",

            "CheckinFile",

            "CheckoutFile" ,

            "DeleteFile",

            "DownloadFile",

            "UpdateFileLifecycleState",

 

This code from EventHandlers.cs compares the event type name with the setting stored by Configulator tool to determine if AddRestriction() should be called. The Contains() function returns false because the commandName string is UpdateFileLifeCycleState which has an upper case "C", but the stored setting is “UpdateFileLifecycleState” which has a lower case. This causes the AddRestriction not to be called.

private void

  RestrictOperation

  (WebServiceCommandEventArgs eventArgs)

  {

   string commandName = eventArgs.GetType().Name;

   if (commandName.EndsWith("CommandEventArgs"))

          commandName = commandName.Remove

                 (commandName.Length -

                       "CommandEventArgs".Length);

 

   RestrictSettings settings =

                         RestrictSettings.Load();

   if (settings.RestrictedOperations.Contains

                                  (commandName))

       eventArgs.AddRestriction

                   (new ExtensionRestriction

                      ("", "Test restriction"));

   }

How to find a component occurrence from a balloon?

By Philippe Leefsma

Q:

Is there a way to get the component occurrence that a balloon is pointing to?

A:

The “LeaderNode.AttachedEntity” tells the geometry intent (attachment) for the node, from which we could know the model geometry. The code below supposes that the drawing view is created by an assembly and a balloon (one leader node) attached to one component of the assembly.

Another way is BalloonValueSet.ReferencedRow. A sample [GetComponentReferencedByBalloon] is available in the Inventor API help files.

    ' Assumess the drawing view is created from a assembly.

    ' Select a balloon manually before running this procedure

    Private Sub test(ByVal app As Inventor.Application)

 

        Dim doc As DrawingDocument = app.ActiveDocument

 

        Dim balloon As Balloon = doc.SelectSet(1)

 

        Dim leader As Leader = balloon.Leader

 

        'assuming the leader is a single line segment

        Dim leaderNode As LeaderNode = leader.AllNodes(2)

 

        Dim intent As GeometryIntent = leaderNode.AttachedEntity

 

        Dim curve As DrawingCurve = intent.Geometry

 

        Dim edgePx As EdgeProxy = curve.ModelGeometry

 

        Dim occurrence As ComponentOccurrence = edgePx.ContainingOccurrence

 

        Debug.Print(vbCrLf + "Occurrence Name: " + occurrence.Name)

 

    End Sub

 

Creating a drawing from scratch with the Inventor API

By Philippe Leefsma

Q:

Is it possible to create Drawing Dimensions and other annotation such as a text box with a leader using the Inventor API?

A:

The following VB.NET example show how to create a new drawing and add views. Dimensions in a view are created along with a text box and a leader.

The attached ipt file provided as link below has attribues attached to the edges that are used in the CreateDrawing function. Notice that the location of this file is hard coded to C:\Temp\Part1.ipt in the code. Change this to the location where you put the file.

ipt file

  

    ' Demonstrates the ability to automatically create a drawing. 

    ' It's hard coded to look for edges

    ' with specific attributes attached. The supplied Part1.ipt

    ' has the attributes attached to edges..

    Public Sub CreateDrawing(ByVal app As Inventor.Application)

 

        ' Create a new drawing document using the default template.

        Dim oDrawDoc As DrawingDocument

        oDrawDoc = m_inventorApp.Documents.Add(

            DocumentTypeEnum.kDrawingDocumentObject, _

            m_inventorApp.FileManager.GetTemplateFile(

                DocumentTypeEnum.kDrawingDocumentObject))

 

        Dim oSheet As Sheet

        oSheet = oDrawDoc.ActiveSheet

 

        ' Open the part to be inserted into the drawing.

        Dim oPartDoc As PartDocument

        oPartDoc = m_inventorApp.Documents.Open("c:\temp\Part1.ipt", False)

 

        Dim oTG As TransientGeometry

        oTG = m_inventorApp.TransientGeometry

 

        MsgBox("Create base and orthographic views.")

 

        ' Place the base front view.

        Dim oFrontView As DrawingView

        oFrontView = oSheet.DrawingViews.AddBaseView(

            oPartDoc,

            oTG.CreatePoint2d(15, 12),

            3,

            ViewOrientationTypeEnum.kFrontViewOrientation,

            DrawingViewStyleEnum.kHiddenLineDrawingViewStyle)

 

        ' Create the top, right and iso views.

        Dim oTopView As DrawingView

        oTopView = oSheet.DrawingViews.AddProjectedView(

            oFrontView,

            oTG.CreatePoint2d(15, 30),

            DrawingViewStyleEnum.kFromBaseDrawingViewStyle)

 

        Dim oIsoView As DrawingView

        oIsoView = oSheet.DrawingViews.AddProjectedView(

            oFrontView,

            oTG.CreatePoint2d(40, 30),

            DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle)

 

        MsgBox("Create section view.")

 

        ' Create a front section view by

        ' defining a section line in the front view.

        Dim oSectionSketch As DrawingSketch

        oSectionSketch = oFrontView.Sketches.Add

 

        oSectionSketch.Edit()

 

        ' Get the circular edge of the top of the part.

        Dim oObjs As ObjectCollection

        oObjs = oPartDoc.AttributeManager.FindObjects("Name", "Name", "Edge13")

        Dim oCircularEdge As Edge

        oCircularEdge = oObjs.Item(1)

 

        ' Get the associated drawingcurve.

        Dim oDrawViewCurves As DrawingCurvesEnumerator

        oDrawViewCurves = oFrontView.DrawingCurves(oCircularEdge)

        Dim oCircularCurve As DrawingCurve

        oCircularCurve = oDrawViewCurves.Item(1)

 

        Dim oCircularEntity As SketchEntity

        oCircularEntity = oSectionSketch.AddByProjectingEntity(oCircularCurve)

 

        ' Draw the section line.

        Dim oSectionLine As SketchLine

        oSectionLine = oSectionSketch.SketchLines.AddByTwoPoints(

            oTG.CreatePoint2d(0, 0.9),

            oTG.CreatePoint2d(0, -0.9))

 

        ' Create a constraint to the projected circle center point and the line.

        Call oSectionSketch.GeometricConstraints.AddCoincident(

            oSectionLine,

            oCircularEntity.CenterSketchPoint)

 

        oSectionSketch.ExitEdit()

 

        ' Create the section view.

        Dim oSectionView As SectionDrawingView

        oSectionView = oSheet.DrawingViews.AddSectionView(

            oFrontView,

            oSectionSketch,

            oTG.CreatePoint2d(34, 10),

            DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle,

            Nothing,

            False)

 

        MsgBox("Create detail view.")

 

        ' Create the detail view.

        Dim oDetailView As DetailDrawingView

        oDetailView = oSheet.DrawingViews.AddDetailView(

            oSectionView,

            oTG.CreatePoint2d(35, 15),

            DrawingViewStyleEnum.kFromBaseDrawingViewStyle,

            False,

            oTG.CreatePoint2d(21, 16),

            oTG.CreatePoint2d(24, 18), , 10, , "A")

 

        ' Get the various edges of the model.

        Dim aoEdges(0 To 13) As Edge

        Dim i As Integer

        For i = 1 To 13

            oObjs = oPartDoc.AttributeManager.FindObjects(

                "Name", "Name", "Edge" & i)

            aoEdges(i) = oObjs.Item(1)

        Next

 

        ' Get the equivalent drawing curves.

        Dim aoDrawCurves(0 To 13) As DrawingCurve

        For i = 1 To 13

            oDrawViewCurves = oFrontView.DrawingCurves(aoEdges(i))

            aoDrawCurves(i) = oDrawViewCurves.Item(1)

        Next

 

        MsgBox("Create dimensions to the curves in the view.")

 

        ' Create some dimensions

        Dim oGeneralDims As GeneralDimensions

        oGeneralDims = oSheet.DrawingDimensions.GeneralDimensions

 

        Dim oDim As GeneralDimension

 

        oDim = oGeneralDims.AddLinear(

            oTG.CreatePoint2d(15.5, 13),

            oSheet.CreateGeometryIntent(aoDrawCurves(1)),

            oSheet.CreateGeometryIntent(aoDrawCurves(3)),

            DimensionTypeEnum.kVerticalDimensionType)

 

        oDim = oGeneralDims.AddLinear(

            oTG.CreatePoint2d(16, 9),

            oSheet.CreateGeometryIntent(aoDrawCurves(2)),

            oSheet.CreateGeometryIntent(aoDrawCurves(4)),

            DimensionTypeEnum.kHorizontalDimensionType)

 

        oDim = oGeneralDims.AddRadius(

            oTG.CreatePoint2d(17, 19),

            oSheet.CreateGeometryIntent(aoDrawCurves(13)))

 

        oDim = oGeneralDims.AddDiameter(

            oTG.CreatePoint2d(8, 20),

            oSheet.CreateGeometryIntent(aoDrawCurves(13)),

            True, False)

 

        MsgBox("Create a text box with a leader.")

 

        ' Place a text box with a leader.

        Dim oObjColl As ObjectCollection

        oObjColl = m_inventorApp.TransientObjects.CreateObjectCollection

        Call oObjColl.Add(oTG.CreatePoint2d(17.5, 11))

        Dim oEval As Curve2dEvaluator

        oEval = aoDrawCurves(4).Evaluator2D

        Dim adParams(0) As Double

        adParams(0) = 0.6

        Dim adPoints(0 To 1) As Double

        Call oEval.GetPointAtParam(adParams, adPoints)

 

        Call oObjColl.Add(oTG.CreatePoint2d(adPoints(0), adPoints(1)))

        Dim oLeaderNote As LeaderNote

        oLeaderNote = oSheet.DrawingNotes.LeaderNotes.Add(

            oObjColl, "Text with a leader")

        oLeaderNote.DimensionStyle = oLeaderNote.DimensionStyle

 

    End Sub

   

 

What’s the GenericObject interface?

By Philippe Leefsma

Q:

I found a reference on a GenericObject interface in the Inventor documentation. What is it? and how to use it?

A:

GenericObject is an interface put in place to wrap an object that hasn't been designed or implemented yet, or that we haven't connected yet. All objects in the system will not support the GenericObject interface, and it's use will decrease over time, as the API coverage becomes more complete.

If you want a generic utility to query the object type, we added a utility (Rx::GetObjectType) for C++ programmers to do just this in DispatchUtils.h.

How to convert Icon/Bitmap to IPictureDisp without VisualBasic.Compatibility.VB6.Support.IconToIPicture?

By Philippe Leefsma

Q:

Is there another approach to convert an image to IPictureDisp than using the deprecated namespace method "Microsoft.VisualBasic.Compatibility.VB6.Support.IconToIPicture"?

A:

The following utility class lets you get rid of that namespace functionality

It’s pretty straightforward to use, juts call the static method “PictureDispConverter.ToIPictureDisp”, however even if the return type is the same, IPictureDisp, an image for a button needs to be created from an Icon resource and an image for a browser node, from a Bitmap resource.

Here is VB.Net code for that utility:

    Public NotInheritable Class PictureDispConverter

 

        <DllImport("OleAut32.dll",

            EntryPoint:="OleCreatePictureIndirect",

            ExactSpelling:=True, PreserveSig:=False)>

        Private Shared Function OleCreatePictureIndirect(

             ByVal picdesc As Object,

            ByRef iid As Guid,

             ByVal fOwn As Boolean) As stdole.IPictureDisp

        End Function

 

        Shared iPictureDispGuid As Guid = GetType(stdole.IPictureDisp).GUID

 

        Private NotInheritable Class PICTDESC

 

            Private Sub New()

            End Sub

 

            'Picture Types

            Public Const PICTYPE_UNINITIALIZED As Short = -1

            Public Const PICTYPE_NONE As Short = 0

            Public Const PICTYPE_BITMAP As Short = 1

            Public Const PICTYPE_METAFILE As Short = 2

            Public Const PICTYPE_ICON As Short = 3

            Public Const PICTYPE_ENHMETAFILE As Short = 4

 

           

            Public Class Icon

                Friend cbSizeOfStruct As Integer =

                    Marshal.SizeOf(GetType(PICTDESC.Icon))

                Friend picType As Integer = PICTDESC.PICTYPE_ICON

                Friend hicon As IntPtr = IntPtr.Zero

                Friend unused1 As Integer

                Friend unused2 As Integer

 

                Friend Sub New(ByVal icon As System.Drawing.Icon)

                    Me.hicon = icon.ToBitmap().GetHicon()

                End Sub

            End Class

 

            Public Class Bitmap

                Friend cbSizeOfStruct As Integer =

                    Marshal.SizeOf(GetType(PICTDESC.Bitmap))

                Friend picType As Integer = PICTDESC.PICTYPE_BITMAP

                Friend hbitmap As IntPtr = IntPtr.Zero

                Friend hpal As IntPtr = IntPtr.Zero

                Friend unused As Integer

 

                Friend Sub New(ByVal bitmap As System.Drawing.Bitmap)

                    Me.hbitmap = bitmap.GetHbitmap()

                End Sub

            End Class

        End Class

 

        Public Shared Function ToIPictureDisp(

            ByVal icon As System.Drawing.Icon) As stdole.IPictureDisp

            Dim pictIcon As New PICTDESC.Icon(icon)

            Return OleCreatePictureIndirect(pictIcon, iPictureDispGuid, True)

        End Function

 

        Public Shared Function ToIPictureDisp(

            ByVal bmp As System.Drawing.Bitmap) As stdole.IPictureDisp

            Dim pictBmp As New PICTDESC.Bitmap(bmp)

            Return OleCreatePictureIndirect(pictBmp, iPictureDispGuid, True)

        End Function

    End Class

 

You may also want to check this post from Mod The Machine blog, where my colleague Wayne took time to produce a full sample demonstrating how to use that in an Inventor add-in.

 

And here is the C# version:

    public sealed class PictureDispConverter

    {

        [DllImport("OleAut32.dll",

            EntryPoint = "OleCreatePictureIndirect",

            ExactSpelling = true,

            PreserveSig = false)]

        private static extern stdole.IPictureDisp

            OleCreatePictureIndirect(

                [MarshalAs(UnmanagedType.AsAny)] object picdesc,

                ref Guid iid,

                [MarshalAs(UnmanagedType.Bool)] bool fOwn);

 

        static Guid iPictureDispGuid = typeof(stdole.IPictureDisp).GUID;

 

        private static class PICTDESC

        {

            //Picture Types

            public const short PICTYPE_UNINITIALIZED = -1;

            public const short PICTYPE_NONE = 0;

            public const short PICTYPE_BITMAP = 1;

            public const short PICTYPE_METAFILE = 2;

            public const short PICTYPE_ICON = 3;

            public const short PICTYPE_ENHMETAFILE = 4;

 

            [StructLayout(LayoutKind.Sequential)]

            public class Icon

            {

                internal int cbSizeOfStruct =

                    Marshal.SizeOf(typeof(PICTDESC.Icon));

                internal int picType = PICTDESC.PICTYPE_ICON;

                internal IntPtr hicon = IntPtr.Zero;

                internal int unused1;

                internal int unused2;

 

                internal Icon(System.Drawing.Icon icon)

                {

                    this.hicon = icon.ToBitmap().GetHicon();

                }

            }

 

            [StructLayout(LayoutKind.Sequential)]

            public class Bitmap

            {

                internal int cbSizeOfStruct =

                    Marshal.SizeOf(typeof(PICTDESC.Bitmap));

                internal int picType = PICTDESC.PICTYPE_BITMAP;

                internal IntPtr hbitmap = IntPtr.Zero;

                internal IntPtr hpal = IntPtr.Zero;

                internal int unused;

 

                internal Bitmap(System.Drawing.Bitmap bitmap)

                {

                    this.hbitmap = bitmap.GetHbitmap();

                }

            }

        }

 

        public static stdole.IPictureDisp ToIPictureDisp(

            System.Drawing.Icon icon)

        {

            PICTDESC.Icon pictIcon = new PICTDESC.Icon(icon);

 

            return OleCreatePictureIndirect(

                pictIcon, ref iPictureDispGuid, true);

        }

 

        public static stdole.IPictureDisp ToIPictureDisp(

            System.Drawing.Bitmap bmp)

        {

            PICTDESC.Bitmap pictBmp = new PICTDESC.Bitmap(bmp);

 

            return OleCreatePictureIndirect(pictBmp, ref iPictureDispGuid, true);

        }

    }

Using Vault APIs to Check in/out Files from an Inventor Addin

By Barbara Han

Issue

From an Inventor Add-In how do I check out a file from the Vault and generate the corresponding DWF file for that file? Also how do I check the file and DWF file back into the Vault after making some changes?

Solution

Please find attached sample that demonstrates how to do what you are looking for. However, this sample can only be used with "leaf" file (e.g. part file). In case of assembly file, you may get into trouble if the assembly file is edited and references are modified. For example, some parts are added to the assembly, the new file dependencies would not show up if the sample code is used.

The attached C# Inventor Add-In sample application does the following:
- finds the part file in the Vault
- finds its DWF attachment
- checks-out the part file
- checks-out the DWF file
- change a user defined property in part file and save file
- checks-in DWF file
- updates the attachment info to be saved in Vault part file
- checks-in the part file

First of all, DocumentService.GetFileAssociationsByIds gets a list of associated attachments for a file (currently Attachment and Dependency are all supported). The GetFileAssociationsByIds() method can be used to find the information for constructing FileAssocParam that is to be used when checking in file later. GetFileAssociationsByIds() may return multiple attachments, so the results have to be scanned to see which file is DWF file. Because the DWF file's file name is the main file's file name appended with .dwf extension, so call GetLatestAssociatedFilePathsByMasterIds to get all file paths of attachments for a file, if file path matches with expected DWF file path, that file represents the DWF file.

When checking out file from the Vault Server, you can download the file to a local folder and open the local file in the Inventor.

After the file is checked out from the Vault server and is modified by the user in Inventor, you can use Inventor API SaveAs() method in the Document object to create a new DWF file for the document.

In the attached samples, the user name, Vault database and the file named are hard coded, please change them according to your environment settings.

Download Vault_checkout_in_2012

The below is the key code for Vault 2012 version. The code may change across different versions of Vault.

public class Vault

{

  /// <summary>

  /// Check out Inventor file from Vault to locak disk 

  /// open file from Inventor and then modify and save it,

  /// finally check Inventor file along with its DWF file in Vault

  /// </summary>

  ///

  public bool CheckOutInTest()

  {

    try

    {

      // Login Vault server

 

      VaultHelper helper = new VaultHelper("Administrator", "", "Vault");

 

      // Find part file and corresponding dwf file in Vault

 

      ArrayList fileAssocParamList = new ArrayList();

 

      String sPartinVault = "$/SampleProject/Part3.ipt";

      String sDWFinVault = "$/SampleProject/Part3.ipt.dwf";

 

      // Get our part file

 

      Autodesk.Connectivity.WebServices.File iFile =

        helper.GetFileAndAssociations(sPartinVault, ref fileAssocParamList);

 

 

 

      // Find DWF attachment

 

      FilePathArray[] filePaths =

        helper.DocumentService.GetLatestAssociatedFilePathsByMasterIds(

        new long[] { iFile.MasterId }, FileAssociationTypeEnum.None, false,

        FileAssociationTypeEnum.Attachment, true, true, true, false);

 

      Autodesk.Connectivity.WebServices.File dwfFile = null;

 

      Boolean bFound = false;

      foreach (FilePath filePath in filePaths[0].FilePaths)

      {

        if (filePath.Path == sDWFinVault)

        {

          dwfFile = filePath.File;

 

          bFound = true;

          break;

        }

        if (bFound == true) break;

      }

      // Check out two files 

 

      if (dwfFile != null) helper.Checkout(dwfFile);

      helper.Checkout(iFile);

 

      // Open part file in Inventor

 

      Inventor.Application iApp = AddInServer.Instance.Application;

      Document pMainDoc = iApp.Documents.Open(helper.checkOutPath + iFile.Name, true);

 

      // Do something here in Inventor environment...

      //...

 

      // Edit a custom property of the file, then Save

      // the file and its .dwf file to the disk

      PropertySet iPropSet = pMainDoc.PropertySets

        ["{D5CDD505-2E9C-101B-9397-08002B2CF9AE}"];

 

      try

      {

        Property iProp = iPropSet["mydata1"];

        iProp.Value = DateTime.Now.ToString();

      }

      catch

      {

        iPropSet.Add(DateTime.Now.ToString(), "mydata1", null);

      }

      iApp.SilentOperation = true;

      pMainDoc.Save();

 

      iApp.SilentOperation = false;

      string sDWFFullName = pMainDoc.FullFileName + ".dwf";

      pMainDoc.SaveAs(sDWFFullName, true);

 

 

      pMainDoc.Close(true);

 

      Autodesk.Connectivity.WebServices.File dwfFileNewVer = null;

 

      // Check-in dwf attachment first

 

      if (dwfFile != null)

      {

        dwfFileNewVer = helper.Checkin(dwfFile, dwfFile.FileClass, true);

      }

      else

      {

        // ToDo: Add dwf File to Vault

      }

 

      // Check-in part file

 

      helper.Checkin(iFile, iFile.FileClass, iFile.Hidden);

 

      MessageBox.Show("You update the part file and DWF file successfully.");

      return true;

    }

    catch (Exception ex)

    {

      MessageBox.Show(ex.ToString(), "Vault_checkout_in Application",

        MessageBoxButtons.OK, MessageBoxIcon.Information);

      return false;

    }

  }

}

 

/// <summary>

/// Helper class

/// </summary>

class VaultHelper

{

    private const int kBufferSize = 1024;

    private const string kCheckOutPath = "C:\\Users\\hanb\\Documents\\Vault\\";

 

    private SecurityService _secSvc;

    private DocumentService _docSvc;

    private ArrayList fileAssocParamList;

 

    public DocumentService DocumentService

    {

        get

        {

            return _docSvc;

        }

    }

    public string checkOutPath

    {

        get

        {

            return kCheckOutPath;

        }

    }

    public VaultHelper(string login, string password,

      string knowledgeVault)

    {

        // Security Service

        _secSvc = new SecurityService();

        _secSvc.Url = "http://localhost/AutodeskDM/Services/SecurityService.asmx";

        _secSvc.SecurityHeaderValue = new Autodesk.Connectivity.WebServices.

          SecuritySvc.SecurityHeader();

        _secSvc.SignIn(login, password, knowledgeVault);

 

        // Document Service

        _docSvc = new DocumentService();

        _docSvc.SecurityHeaderValue = new Autodesk.Connectivity.WebServices.

          DocumentSvc.SecurityHeader();

        _docSvc.SecurityHeaderValue.Ticket = _secSvc.SecurityHeaderValue.Ticket;

        _docSvc.SecurityHeaderValue.UserId = _secSvc.SecurityHeaderValue.UserId;

        _docSvc.Url = "http://localhost/AutodeskDM/Services/DocumentService.asmx";

        fileAssocParamList = new ArrayList();

    }

 

    // Check in the file

    public Autodesk.Connectivity.WebServices.File Checkin(Autodesk.Connectivity.

      WebServices.File file,

            FileClassification fileClassification, Boolean hidden)

    {

        Autodesk.Connectivity.WebServices.File retFile = null;

        string filePath = Path.Combine(kCheckOutPath, file.Name);

 

        using (FileStream stream = new FileStream(filePath, FileMode.Open,

          FileAccess.Read))

        {

            byte[] fileData = new byte[stream.Length];

            stream.Read(fileData, 0, fileData.Length);

 

            // Perform the upload

 

            if (fileClassification == FileClassification.DesignVisualization)

            {

                retFile = _docSvc.CheckinFile(file.MasterId, file.Comm,

                false, System.IO.File.GetLastWriteTime(filePath), null, null,false,

                file.Name, file.FileClass, hidden, fileData);

 

                for (int i = 0; i < fileAssocParamList.Count; i++)

                {

                    FileAssocParam param1 = (FileAssocParam)fileAssocParamList[i];

                    if (param1.CldFileId == file.Id)

                    {

                        param1.CldFileId = retFile.Id;

                    }

                }

                System.IO.FileAttributes attr = System.IO.File.GetAttributes(filePath);

                //the local file can't be read only.

                if ((attr & System.IO.FileAttributes.ReadOnly) == 0)

                {

                    System.IO.File.SetAttributes(filePath, FileAttributes.ReadOnly);

                }

            }

            else

            {

                // Get bom

                Autodesk.Connectivity.WebServices.BOM tbom =

                  _docSvc.GetBOMByFileId(file.Id);

 

                FileAssocParam[] paramArray = (FileAssocParam[])

                  fileAssocParamList.ToArray(typeof(FileAssocParam));

 

                retFile = _docSvc.CheckinFile(file.MasterId, file.Comm,

                    false, System.IO.File.GetLastWriteTime(filePath),

                    paramArray, tbom, true,

                    file.Name, file.FileClass, hidden, fileData);

                if (System.IO.File.Exists(filePath) == true)

                {

                    System.IO.FileAttributes attr =

                      System.IO.File.GetAttributes(filePath);

 

                    //the local file can't be read only.

                    if ((attr & System.IO.FileAttributes.ReadOnly) == 0)

                    {

                        System.IO.File.SetAttributes(filePath, FileAttributes.ReadOnly);

                    }

                }

            }

        }

 

        return retFile;

    }

 

    public Autodesk.Connectivity.WebServices.File Checkout(

      Autodesk.Connectivity.WebServices.File file)

    {

        Folder[] folders = _docSvc.GetFoldersByFileMasterId(file.MasterId);

        string filePath = Path.Combine(kCheckOutPath, file.Name);

 

        if (System.IO.File.Exists(filePath) == true)

        {

            System.IO.FileAttributes attr = System.IO.File.GetAttributes(filePath);

            // The local file can't be read only.

 

            if ((attr & System.IO.FileAttributes.ReadOnly) != 0)

            {

                System.IO.File.SetAttributes(filePath, FileAttributes.Normal);

            }

        }

 

        // Check out the file

 

        byte[] bytes;

        Autodesk.Connectivity.WebServices.File fileOut =

          _docSvc.CheckoutFile(folders[0].Id, file.Id,

          CheckoutFileOptions.Master, Environment.MachineName,

          kCheckOutPath,file.Comm, true, true, out bytes);

 

        // Get the latest data of the file from Vault                  

        System.IO.File.WriteAllBytes(filePath, bytes);

 

        return fileOut;

    }

 

    public Autodesk.Connectivity.WebServices.File

      GetFileAndAssociations(string path,ref ArrayList fileAssocParams)

    {

        string[] paths = new string[1];

 

        paths[0] = path;

        Autodesk.Connectivity.WebServices.File[] files =

          _docSvc.FindLatestFilesByPaths(paths);

 

        FileAssocArray[] assocArray = _docSvc.GetFileAssociationsByIds(

          new long[] { files[0].Id }, FileAssociationTypeEnum.None, false,

        FileAssociationTypeEnum.All,false, false, true);

 

        FileAssocArray assemblyAssoc = assocArray[0];

 

        if (assemblyAssoc != null)

        {

            foreach (FileAssoc assoc in assemblyAssoc.FileAssocs)

            {

 

                FileAssocParam param1 = new FileAssocParam();

                param1.CldFileId = assoc.CldFile.Id;

                param1.RefId = assoc.RefId;

                param1.Source = assoc.Source;

                param1.Typ = assoc.Typ;

                param1.ExpectedVaultPath = assoc.ExpectedVaultPath;

                fileAssocParams.Add(param1);

 

            }

        }

        return files[0];

    }

}

How to set the shortcut key to a customized command in Inventor?

Issue

"What is the best method to assign a shortcut key to a command in inventor programmatically via the api? I can see on the command definition there are default shortcut key and override shortcut key properties but which one should I set?"

Solution

The following VBA sample demonstrates how to assign a shortcut key to a customized button added to assembly Panel Bar.

Please note the following several points:

If the shortcut key has been consumed by another command, you can’t use it again for your own command, otherwise you will get a runtime error. For example Ctrl+A is used by the “Select All” command, so you can’t use “Ctrl+A” again. You can get a list of all commands and the shortcut keys consumed by Inventor through the “Copy to clipboard” command which is on the keyboard page of the Customize dialog (Tools>Customize¡­).

The DefaultShortcut property can be used to set the command alias, but can’t be used for setting the accelerator, you should use OverrideShortcut instead. The user interface won’t delete the controls you added, so you need to remove them manually from the user interface.

If the shortcut key is used by you, you can’t use it again even if you delete the corresponding control from UI, unless you reset all keys from the keyboard page on the customize dialog.

Shortcuts of kAcceleratorShortcut type are created by defining the OverrideShortcut to an allowed non-alphanumeric character, for example “Alt+U”, but those are defined as key combinations by Inventor, like “Ctrl+C” or “Alt+H”, you can’t use.

 

 

Private WithEvents oBtnDef As ButtonDefinition

Sub AddBtnDefWithShortcut()

Dim oControlDefs As ControlDefinitions

Set oControlDefs = ThisApplication.CommandManager.ControlDefinitions

'Create our own button command

Set oBtnDef = oControlDefs.AddButtonDefinition("MyControldefinition1", "Internal name for my controldef 1", kShapeEditCmdType)

'Assign shortcut key to the button command

oBtnDef.OverrideShortcut = "Alt+A"

' Find the main assembly command bar.

Dim oAsmCmdBar As CommandBar

Set oAsmCmdBar = ThisApplication.UserInterfaceManager.CommandBars.Item("AMxAssemblyPanelCmdBar")

' Add a control to the command bar.

Call oAsmCmdBar.Controls.AddButton(oBtnDef)

End Sub

 

You can delete the button command created by above code, like this:

 

Sub DeleteControlDef()

Dim oControlDefs As ControlDefinitions

Set oControlDefs = ThisApplication.CommandManager.ControlDefinitions

Dim oDef As ControlDefinition

Set oDef = oControlDefs.Item("Internal name for my controldef 1")

oDef.Delete

End Sub

API for representation view of assembly

By Xiaodong Liang

Issue

"Is there an API to control Design View Representations?  In the Model browser in assembly mode we see:

Representations
     -->View
        --> Private
        --> default
        --> view ...

Is there a way to get the current active view and other settings?

Solution

The Inventor API supports the manipulation to Design View Representations. Here is a code example:

 

VBA code

Public Sub test_VBA() 
 ' get the current assembly
 Dim doc As AssemblyDocument
 Set doc = _
    ThisApplication.ActiveDocument
 ' get AssemblyComponentDefinition
 Dim AssemblyDef As AssemblyComponentDefinition
 Set AssemblyDef = _
    doc.ComponentDefinition
 ' get Manager of Representations
 Dim dViewRepMgr As RepresentationsManager
 Set dViewRepMgr = _
    AssemblyDef.RepresentationsManager
 ' get active Representation view
 Dim dViewRep As DesignViewRepresentation
 Set dViewRep = _
    dViewRepMgr.ActiveDesignViewRepresentation
 Debug.Print dViewRep.Name
' get the first Representation view
 Set dViewRep = _
    dViewRepMgr.DesignViewRepresentations.Item(1)
 ' activate the first view
 dViewRep.Activate
  ' dump all Representations views
  Dim dViewReps As DesignViewRepresentations
  Set dViewReps = _
    dViewRepMgr.DesignViewRepresentations
  Debug.Print dViewReps.Count
  For Each dViewRep In dViewReps
       Debug.Print dViewRep.Name
  Next dViewRep
End Sub

VB.NET code

Public Sub test_VBNet()

 

    ' assume we have had Inventor application

    '  _InvApplication

 

    ' get the current assembly

    Dim doc As AssemblyDocument = 

        _InvApplication.ActiveDocument

 

    ' get AssemblyComponentDefinition

    Dim AssemblyDef As AssemblyComponentDefinition =

         doc.ComponentDefinition

 

    ' get Manager of Representations

    Dim dViewRepMgr As RepresentationsManager =

        AssemblyDef.RepresentationsManager

 

        ' get active Representation view

    Dim dViewRep As DesignViewRepresentation =

        dViewRepMgr.ActiveDesignViewRepresentation

 

    Debug.Print(dViewRep.Name)

 

    ' get the first Representation view

    dViewRep =

        dViewRepMgr.DesignViewRepresentations.Item(1)

 

    ' activate the first view

    dViewRep.Activate()

 

    Dim dViewReps As DesignViewRepresentations =

        dViewRepMgr.DesignViewRepresentations

 

    Debug.Print(dViewReps.Count)

 

     ' dump all Representations views

    For Each dViewRep In dViewReps

        Debug.Print(dViewRep.Name)

    Next dViewRep

 

End Sub

 

create dwf files using Inventor apprentice

By Xiaodong Liang

Using DataIO objects you can create DWF files from an Apprentice Server if the document is an .idw. (.ipt or .iam to DWF is not supported using Apprentice) A .dwf file can be created from an .ipt or .iam using the SaveAs method in the Inventor API. Here are VB.NET and VBA examples that open an .idw file and create a .dwf.

This VB.NET example is from a button on a form in a standalone exe.

Private Sub writeDWF()

 

    Try

        Dim oAApp As ApprenticeServerComponent = 

            New ApprenticeServerComponent()

 

        Dim oDoc As ApprenticeServerDrawingDocument =  

                oAApp.Open("C:\test.idw")

 

        Dim oSheet As Sheet = 

            oDoc.Sheets(1)

 

        Dim oDataIO As DataIO = oSheet.DataIO

 

        ' Create the DWF file.

        oDataIO.WriteDataToFile("DWF", "c:\temp\test.dwf")

 

    Catch ex As SystemException

        System.Windows.Forms.MessageBox.Show(ex.ToString())

    End Try

 

End Sub