Manufacturing DevBlog

Vault Performance tip – don’t access the server in a loop

By Wayne Brill

When using the Vault API to access the server you can improve performance by not having server calls inside a loop. Below is a code snippet that is using GetPropertyValue and GetFoldersByIds in a loop. (highlighted lines). In this example if there are 1,000 files in myResults, there will be 1,000 server calls. With network latency, there is just not a good way to make 1,000 server calls very quickly.

foreach (File myFile in myResults)
{
VDF.Vault.Currency.Entities.FileIteration fileIter = new VDF.Vault.Currency.Entities.FileIteration(base.VaultConnection, myFile);

EntityStatusImageInfo statusInfo = base.VaultConnection.PropertyManager.GetPropertyValue(fileIter, statusProp, null) as EntityStatusImageInfo;
MYVaultFileStatus myVltFileStatus = new MYVaultFileStatus(myFile.Name);

 

myVltFileStatus.VaultStatusText = statusInfo.Description;
myVltFileStatus.VaultStatusImage = statusInfo.GetImage();
long folderID = myFile.FolderId;

var folderFoundIn = base.VaultConnection.FolderManager.GetFoldersByIds(new long[] { folderID });

 

VDF.Vault.Currency.Entities.Folder folderOfFile;

folderFoundIn.TryGetValue(folderID, out folderOfFile);
myVltFileStatus.VaultPath = folderOfFile.FolderPath;
myVltFileStatus.VaultFileID = myFile.Id;
listDocumentStatus.Add(myVltFileStatus);
}

A better approach is to use web service calls that allow you to retrieve properties for a group or batch of files with a single call to the server. These methods typically accept an array of IDs or proxy objects so that you can retrieve a large collection of values with a single call.

The PropertyManager GetPropertyValues is nearly identical to  GetPropertyValue except that it takes an array of entities and property definitions and retrieves all the property values at once with a single server call. This is what “using batch API methods as a best practice” means.

Here is an update to the example code with just two calls to the server:

 
// batch up entities to retrieve properties for
List<VDF.Vault.Currency.Entities.FileIteration> fileIterations =
new List<VDF.Vault.Currency.Entities.FileIteration>(myResults.Select(result => new VDF.Vault.Currency.Entities.FileIteration(base.VaultConnection, result)));

// make a single call to get property values
VDF.Vault.Currency.Properties.PropertyValues propValues = base.VaultConnection.PropertyManager.GetPropertyValues(fileIterations, new VDF.Vault.Currency.Properties.PropertyDefinition[] { statusProp }, null);

// make a single call to get parent folders
IDictionary<long, VDF.Vault.Currency.Entities.Folder> folderIdsToFolderEntities = base.VaultConnection.FolderManager.GetFoldersByIds(fileIterations.Select(file => myFile.FolderId));

// individually process results returned from the server
foreach (VDF.Vault.Currency.Entities.IEntity fileIteration in fileIterations)
{
VDF.Vault.Currency.Properties.EntityStatusImageInfo statusInfo = propValues.GetValue(fileIteration, statusProp) as VDF.Vault.Currency.Properties.EntityStatusImageInfo;
MYVaultFileStatus myVltFileStatus = new MYVaultFileStatus(fileIteration.EntityName);

stVltFileStatus.VaultStatusText = statusInfo.Description;
stVltFileStatus.VaultStatusImage = statusInfo.GetImage();
VDF.Vault.Currency.Entities.Folder folderOfFile;

if (folderIdsToFolderEntities.TryGetValue(fileIteration.FolderId, out folderOfFile))
{
stVltFileStatus.VaultPath = folderOfFile.FolderPath;
}
stVltFileStatus.VaultFileID = fileIteration.EntityIterationId;
listDocumentStatus.Add(stVltFileStatus);
}

The key is that the calls to the server have been moved outside the loop.

Expand browser and select part by selecting edge in drawing view

By Wayne Brill

This VB.NET example is a Visual Studio 2012 project that connects to Inventor from out of process. It has one button on a form. When the button is clicked it prompts you to select a DrawingCurveSegment. When you select an edge in one of the views it finds the browser node for the part or assembly and expands it. The part or assembly is also selected.

This Post also selects a node: Get BrowserNode of an occurrence

Before running the code:

After the code was run. Notice the browser is expanded and the part is selected. 

To test have a drawing open that has views that reference an assembly or part. This example would need to be updated to handle every possible view that could exist.

Here is the pertinent code:

Public Sub browserSelect()

 

    Dim odoc As Inventor.Document

    odoc = m_InvApp.ActiveDocument

 

    Dim oSelectSet As Inventor.SelectSet

    oSelectSet = odoc.SelectSet

 

    ' Get the selected curve from the select set.

    Dim oDrawCurveSeg As DrawingCurveSegment

    oDrawCurveSeg = m_InvApp.CommandManager.Pick _

     (Inventor.SelectionFilterEnum.

      kDrawingCurveSegmentFilter,

      "Select a drawingCurve")

 

 

    ' Get the parent DrawingCurve

    Dim oDrawCurve As DrawingCurve

    oDrawCurve = oDrawCurveSeg.Parent

 

    ' Get the model geometry this curve represents.

    Dim oModelGeom As Object

    oModelGeom = oDrawCurve.ModelGeometry

 

    ' Check to see if the returned object supports

    ' the ContainingOccurrence property.

    Dim oOccurrence As ComponentOccurrence

    'oOccurrence = oModelGeom.ContainingOccurrence

 

 

    Dim oModelGeometry =

        oDrawCurveSeg.Parent.ModelGeometry

    Dim oCompDef As ComponentDefinition

 

    oCompDef =

        oModelGeometry.parent.componentdefinition

 

    partNameToTest = oCompDef.Document.DisplayName

 

 

    Dim intLength As Integer

    intLength = partNameToTest.Length()

    ' Going to use this to test to see if it is

    ' the right node Need to remove the extension

    ' and the dot

    partNameToTest = partNameToTest.Remove _

                                  (intLength - 4)

 

    Try

        oOccurrence = oModelGeom.ContainingOccurrence

 

        ' Get the drawing view

        Dim oDrwView As DrawingView

        oDrwView = oDrawCurve.Parent

 

        'Get the browser node definition of the

        ' drawing view

        Dim oNativeBrowserNodeDef As  _

                    NativeBrowserNodeDefinition

        oNativeBrowserNodeDef =

         odoc.BrowserPanes. _

             GetNativeBrowserNodeDefinition(oDrwView)

 

        ' Testing - Get an error eNotImplemented

        'Dim oNativeBrowserNodeDef2 As NativeBrowserNodeDefinition

        'oNativeBrowserNodeDef2 = _

        'odoc.BrowserPanes.GetNativeBrowserNodeDefinition(oOccurrence)

 

        'Get the top browser node

        Dim oTopBrowserNode As BrowserNode

        oTopBrowserNode =

         m_InvApp.ActiveDocument.BrowserPanes. _

                                      ActivePane.TopNode

 

        ' Get the browser node of the view using the

        ' browser node definition

        Dim oNode As BrowserNode

        oNode = oTopBrowserNode.AllReferencedNodes _

                      (oNativeBrowserNodeDef).Item(1)

 

        If oNode.BrowserNodes.Count > 0 Then

            Call recurseNodes(oNode)

            bNodeFound = False

        End If

        'END WB added

 

    Catch ex As Exception

       MsgBox("Problem getting part " & partNameToTest)

        Exit Sub

    End Try

 

End Sub

Sub recurseNodes(node As BrowserNode)

    Dim strNodeLabel As String

    strNodeLabel =

       node.BrowserNodeDefinition.Label

    'See if the node label contains

    ' the name of the part

    If InStr(strNodeLabel,

             partNameToTest) = 1 Then

        'Expand the node of the part

        node.Expanded = True

        'Select the node of the part

        node.DoSelect()

        ' make boolean flag true 

        'so Exit For will be called

        bNodeFound = True

    End If

 

    Dim bn As BrowserNode

    For Each bn In

                node.BrowserNodes

        If bNodeFound = False Then

            'The base view can have

            ' other views under it

            ' - skip them

            If Not TypeName(bn.NativeObject) _

                          = "DrawingView" Then

                Call recurseNodes(bn)

            Else

                'Skipping the DrawingViews

                ' under the Base View

                Continue For

            End If

        Else

            'Node has been found so

            'exit the loop

            Exit For

        End If

    Next

End Sub

Project file:  Download BrowserSelectTest

Inventor Virtual Component: Assign Base Quantity to the Parameter

by Vladimir Ananyev

Each new virtual component by default has Base Quantity settings as shown below.

How can I assign the base quantity to some parameter?  BOMQuantity.SetBaseQuantity method could do all this work for us.

Let’s say we have the virtual component “Paint:1” and the user parameter “Paint_Mass”:

The following code sample illustrates the workflow:

Sub SetQuantity()

    Dim oDoc As AssemblyDocument
    Set oDoc = ThisApplication.ActiveDocument

    Dim oDef As AssemblyComponentDefinition
    Set oDef = oDoc.ComponentDefinition

    'reference to the user parameter where mass value is stored

    Dim oPar As Inventor.UserParameter

    Set oPar = oDef.Parameters.UserParameters.Item("Paint_Mass")

    'get the reference to the virtual component by its name

    Dim oOcc As ComponentOccurrence

    Set oOcc = oDef.Occurrences.ItemByName("Paint:1")

    'virtual component definition

    Dim oVirtualDef As VirtualComponentDefinition

    Set oVirtualDef = oOcc.Definition

    'Assign the base quantity to the parameter oPar

    'Limitation: this works for length, volume, and mass units only.

    Dim oBOMQuantity As BOMQuantity

    Set oBOMQuantity = oVirtualDef.BOMQuantity

    Call oBOMQuantity.SetBaseQuantity( _ 
       BOMQuantityTypeEnum.kParameterBOMQuantity, oPar)

End Sub

If you check base quantity after this subroutine is completed you will see this:

Update TextBox in Sketch

By Adam Nagy

If you want to show the current volume of the model inside a sketch text box, then you either need to keep updating a TextBox with the latest information yourself or base the TextBox information on a User or Model Parameter that is updated from the actual Volume of the model.

In case of our simple model you could easily calculate the Volume yourself based on the 3 dimensions of this box model. However, in case of a complicated model you would need to rely on the calculated value provided by Inventor, e.g. iProperties.Volume. This however requires a model geometry recalculation to be correct. So if you use it right after a model parameter changed, but before the model geometry got recalculated, then it will be incorrect.  

If you subscribed the Rule to both Any Model Parameter Change and Part Geometry Change and your Rule relies on information that is calculated from geometry, like Volume, then Any Model Parameter Change event is too early and better to remove it from the list of events that trigger your rule:

If you did not do the above and your Rule is not forcing an update explicitly (e.g. using InventorVb.DocumentUpdate(False)) before reading the iProperties.Volume property then this would happen when changing parameters directly in the Parameters dialog:

So the above was enough to make sure that our own Volume User Parameter will always be up-to-date. Then to make the TextBox up-to-date as well, we can simply do this which will trigger an update after our Rule finished:

iLogicVb.UpdateWhenDone = True

We are also checking the Volume based on liters, so we use UnitsOfMeasure object to convert the Volume to liters. Here is the Rule code:

' This is in mm^3 because of the 
' Part Document's unit settings
' You have to set the rule
' so that it's only triggered for
' "Part Geometry Change" event, so 
' that the iProperties.Volume is correct
Volume = iProperties.Volume

' If we want it in liters
Dim uom As UnitsOfMeasure
uom = ThisApplication.ActiveDocument.UnitsOfMeasure
  
Dim lengthUnit As String
lengthUnit = uom.GetStringFromType(uom.LengthUnits)

' mm^3 to liters  
VV = uom.ConvertUnits(Volume, lengthUnit + "^3", "l")

' In liters
V_needed = 2500

' Need to use accuracy
acc = .0001

' The values are equal or VV is bigger
If VV > V_needed - acc Then
  iProperties.PartColor = "Green Pastel"
Else
  iProperties.PartColor = "Red"
End If

' This is enough to get the sketch text updated
' to the new Volume value
 
iLogicVb.UpdateWhenDone = True

Sample model:  Download Tank volume 2014

Set the offset of components to zero and ground them

By Adam Nagy

When you are inside an assembly then you can right-click on any of the components in the model tree and inside the iProperties dialog you can set their offset:

In the API you get/set that information through the Transformation matrix of the Occurrence. That has the component's position and alignment.

If you simply want to set all the offsets to zero and orient them the same way as the assembly then you just have to use an identity matrix (default of CreateMatrix()) as their Transformation. 

This is what the code could look like in iLogic:

Dim doc As AssemblyDocument
doc = ThisApplication.ActiveDocument

Dim tr As TransientGeometry
tr = ThisApplication.TransientGeometry

Dim occ As ComponentOccurrence
For Each occ In doc.ComponentDefinition.Occurrences
  ' If it's suppressed we cannot do
  ' anything with it
  If Not occ.Suppressed Then
    Call occ.SetTransformWithoutConstraints( _
      tr.CreateMatrix())
    occ.Grounded = True
  End If
Next

Use Inventor View without registering it

By Adam Nagy

As pointed out in this blog post, from Inventor 2012 onwards Inventor does not register the View component.

If you do not want to or cannot register the component using the regsvr32 utility, then you can embed a manifest in your application instead. In this case however, you'll need to make sure that InventorViewCtrl.ocx is in the same folder as your application: you can either distribute this file with your application or copy the one installed with Inventor or Inventor View.

You can use the mt.exe utility to get the manifest itself from VS Command Prompt run as Administrator:

Then through the Project Settings you can get it embedded in your project:

In case of Inventor 2015 you still need the workaround even when using Registration Free method:
http://adndevblog.typepad.com/manufacturing/2014/10/using-inventor-view-from-64-and-32-bit-process.html  

Here is the sample code: https://github.com/adamenagy/InventorView-FileDisplay-.NET-4.0-RegFree 

Vault GetFileAssociationLitesByIds() associationAlgorithm parameter

By Wayne Brill

GetFileAssociationLitesByIds is now the recommended API function for getting file relationships. This method is intended to replace all the other get-file-association methods in the document service. There is a plan to remove the older methods in a future release, leaving only GetFileAssociationLitesByIds (“lite” will probably be removed from the name).

The associationAlgorithm parameter essentially allows this one method to get the same relationships that could be obtained from any of the other methods. The API help topics describing the associationAlgorithm parameter will be improved too.

To better understand the concepts of the current release see the documentation for the older methods. (The documentation for GetFileAssociationLitesByIds will be improved so this extra lookup is unnecessary in a future release of the SDK).

Here is an guide for each FileAssocAlg enum. Only the first two are available in base Vault.

Actual - Gets the same relationships that GetFileAssociationsByIds would get.

LatestTip – Gets the same relationships that GetLatestFileAssociationsByMasterIds would get with releaseBiased=false. But file iteration IDs are passed – not file master IDs.

LatestConsumable - Gets the same relationships that GetLatestFileAssociationsByMasterIds would get with releaseBiased=true. But file iteration IDs are passed – not file master IDs.

RevisionConsumable - gets the same relationships that GetRevisionFileAssociationsByIds would get with releaseBiased=true.

RevisionTip - Gets the same relationships that GetRevisionFileAssociationsByIds would get with releaseBiased=false.

RevisionDate - Gets the same relationships that GetRevisionFileAssociationsByIds2 would get with dateBiased=true and releaseBiased=false. Essentially, the idea is to get the version of the revision that the end-user most likely had on disk when they checked-in the file. This is only used in rare cases in certain workflows. It should probably not be used for visualizations. Unlike the GetRevisionFileAssociationsByIds2 method, you can get parents when using this algorithm with the GetFileAssociationLitesByIds method.

Vault AcquireFiles and the PreFileAcquire event

By Wayne Brill

The Vault Development Framework (VDF) acquire files API will download a file to disk so long as the file to be downloaded is different than the one that is currently on disk. There are some restrictions that might be enforced that could prevent the download, but that is the general idea. However, you can extend the behavior of the acquire using the events on the AcquireFilesSettings object to avoid downloading files based on your own custom criteria.

On the AcquireFilesSettings.AcquireFileExtensibilityOptions class (which can be accessed using the AcquireFileSettings.OptionsExtensibility property for a specific instance of the download settings), there is a PreFileAcquire event.

You can register a handler to this event which will fire for each file that is to be downloaded. As part of the event arguments, the handler is provided info about the file that is on disk relative to the file to be downloaded. This info can be accessed via the PreFileAcquireEventAgrs.FileAcquisitionInfo property. The property contains an enum with flags that will specify if the file on disk is newer.

If you don’t want to download an older version of a file, have the custom handler check for that flag and set the SkipDownload flag on the PreFileAcquisitionResult property of the event args.

The VDF AcquireFiles API is written to avoid excess calls to the server whenever it can and so it will not download files if it determines that the file on disk matches the file that is attempting to be downloaded.

Using Inventor View from 64 and 32 bit processes

By Adam Nagy

As mentioned in this blog post you need to use some workaround to get the Inventor View 2015 component to show more than just a blank screen with a toolbar. 

You can set the PATH either system wide in System Properties >> Environment Variables, or just for your own application using System.Environment.SetEnvironmentVariable()

If you want to use Any CPU compilation for your application so that on a 32 bit OS it runs as a 32 bit process and on a 64 bit OS it runs as a 64 bit process, then you can just set the PATH variable to <Inventor install path>\Bin

However, if you want to compile your application with the x86 platform option so that it always runs as a 32 bit process no matter what OS it is on, then you could take advantage of the Environment.Is64BitOperatingSystem property introduced in .NET Framework 4.0, and could set the PATH variable based on the OS. To make the code work for all combinations of OS's and process bitnesses, you could use this in combination with Environment.Is64BitProcess:

public void AddInventorPath()
{
  // Note: System.Environment.Is64BitProcess and
  // System.Environment.Is64BitProcess were
  // introduced in .NET Framework 4.0
  string path =
    System.Environment.GetEnvironmentVariable("PATH");

  // In case process and OS bitness match it's
  // C:\Program Files\Autodesk\Inventor 2015\
  // otherwise it's
  // C:\Program Files\Autodesk\Inventor 2015\bin\
  string inventorPath = m_oserver.InstallPath;

  if (System.Environment.Is64BitOperatingSystem &&
      !System.Environment.Is64BitProcess)
  {
    // If you are running the app as a 32 bit process
    // on a 64 bit OS then you'll need this
    path += ";" + inventorPath + "Bin32";
  }
  else
  {
    // Otherwise you need this
    path += ";" + inventorPath + "Bin";
  }

  System.Environment.SetEnvironmentVariable("PATH", path);
}

public Form1()
{
  // Try to create an instance of apprentice server
  try
  {
    m_oserver = newApprenticeServerComponent();
    AddInventorPath();
  }
  catch (SystemException exception)
  {
    MessageBox.Show(this,
      "Failed to create an instance of Apprentice server.",
      "CSharpFileDisplaySample",
      MessageBoxButtons.OK, MessageBoxIcon.Warning);
    return;
  }

  m_odocument = null;
  m_oview = null;
  m_ocamera = null;
  m_bmouseDown = false;

  //
  // Required for Windows Form Designer support
  //
  InitializeComponent();
}

I started with the C:\Users\Public\Documents\Autodesk\Inventor 2015\SDK\DeveloperTools\Samples\VCSharp.NET\Standalone Applications\ApprenticeServer\FileDisplay sample as a test, but got this error when running the application if I changed the project's Target framework to .NET Framework 4:

System.IO.FileNotFoundException was unhandled
  HResult=-2147024894
  Message=Could not load file or assembly 'Interop.InventorApprentice, Version=1.0.0.0, Culture=neutral, PublicKeyToken=null' or one of its dependencies. The system cannot find the file specified.

I had the same issue even after changing the Interop.InventorViewControlLib assembly's Embed Interop Types to False. So I created new interop assemblies for the Inventor View component following this info: http://adndevblog.typepad.com/autocad/2012/07/use-64-bit-activex-component-from-a-net-assembly.html

Then I replaced the references in the project with the newly created ones, but still got the same error. However, once I changed the InventorViewControlLib assembly's Embed Interop Types to False the error went away.

See the sample in action:

Sample project: https://github.com/adamenagy/InventorView-FileDisplay-.NET-4.0 

Which DrawingView triggered OnViewUpdate

By Adam Nagy

Each drawing view has its own DrawingViewEvents object and the event you subscribe to through it is specific to that DrawingView. However, the event itself does not tell you which object triggered it.

If you want to listen to this event sent by only a couple of the drawing views then you can create a separate event handler function for each, and that way identify which DrawingView object sent it:

using System;
using System.Runtime.InteropServices;
using System.Collections.Generic;
using Inventor;
using MsgBox = System.Windows.Forms.MessageBox;

namespace InventorConsoleCs
{
  class Program
  {
    static DrawingView dw1, dw2;

    static void Main(string[] args)
    {
      Application app = (Application)
        Marshal.GetActiveObject("Inventor.Application");

      DrawingDocument doc =
        (DrawingDocument)app.ActiveDocument;

      dw1 = doc.ActiveSheet.DrawingViews[1];
      dw1.DrawingViewEvents.OnViewUpdate +=
        DrawingViewEvents_OnViewUpdate1;
      dw2 = doc.ActiveSheet.DrawingViews[2];
      dw2.DrawingViewEvents.OnViewUpdate +=
        DrawingViewEvents_OnViewUpdate2;

      System.Console.ReadKey();
    }

    static void DrawingViewEvents_OnViewUpdate1(
      EventTimingEnum BeforeOrAfter, NameValueMap Context,
      CommandTypesEnum ReasonsForChange,
      out HandlingCodeEnum HandlingCode)
    {
      HandlingCode = HandlingCodeEnum.kEventNotHandled;
      MsgBox.Show(dw1.Name);  
    }

    static void DrawingViewEvents_OnViewUpdate2(
      EventTimingEnum BeforeOrAfter, NameValueMap Context,
      CommandTypesEnum ReasonsForChange,
      out HandlingCodeEnum HandlingCode)
    {
      HandlingCode = HandlingCodeEnum.kEventNotHandled;
      MsgBox.Show(dw2.Name);  
    }
  }
}

However, if you want to do things dynamically so that you can listen to this event coming from any number of drawing views then the best thing might be to wrap the event handler inside a class. Each class instance will know which DrawingView's event it's listening to and so inside its event handler function we can tell who sent it:

using System;
using System.Runtime.InteropServices;
using System.Collections.Generic;
using Inventor;
using MsgBox = System.Windows.Forms.MessageBox;

namespace InventorConsoleCs
{
  class Program
  {
    class DrawingViewEventWatcher
    {
      public DrawingView drawingView;

      public DrawingViewEventWatcher(DrawingView v)
      {
        drawingView = v;
        v.DrawingViewEvents.OnViewUpdate +=
          DrawingViewEvents_OnViewUpdate;
      }

      void DrawingViewEvents_OnViewUpdate(
        EventTimingEnum BeforeOrAfter, NameValueMap Context,
        CommandTypesEnum ReasonsForChange,
        out HandlingCodeEnum HandlingCode)
      {
        HandlingCode = HandlingCodeEnum.kEventNotHandled;
        MsgBox.Show(drawingView.Name);  
      }
    }
  
    static List<DrawingViewEventWatcher> watchers =
      new List<DrawingViewEventWatcher>();

    static void Main(string[] args)
    {
      Application app = (Application)
        Marshal.GetActiveObject("Inventor.Application");

      DrawingDocument doc =
        (DrawingDocument)app.ActiveDocument;

      foreach (Sheet s in doc.Sheets)
        foreach(DrawingView v in s.DrawingViews)
        {
          watchers.Add(new DrawingViewEventWatcher(v));   
        }
     

      System.Console.ReadKey();    

    }
  }
}

When running the code on a drawing with the following content then this is what we get when we modify the assembly and switch back to the drawing: