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Introduction

The goal of this tutorial is to use the Alibre Design API to connect to a running instance of Alibre Design and create a new part file containing a shiney, blue, one-inch cube cenetered about the origin. This is targeted to a beginner audience and will touch on the following topics:

• Internal units
• Connecting to Alibre Design
  • AutomationHook
  • IADRoot
• Creating a New Part
  • IADPartSession
  • BGR Colors
• Creating a Sketch
  • IADDesignSession
  • IADDesignPlane
  • IADSketch
  • [Begin/End]Change()
• Creating a Feature
  • IADSession
  • IADExtrusionFeature
  • [Open/Close]ParameterTransaction()
• Saving and Closing
• Cleaning Up

The line numbers are for reference only -- you should not type them into the program.

To follow along with this tutorial you will need to have Alibre Design (or Alibre Design Xpress) installed and running on your machine. You will also need to have a Microsoft Visual Studio product such as Visual Basic Express, which is available from Microsoft free of charge, at least for a limited time.

This tutorial will also give you an idea of how similar VB.Net and C#.Net are. Using Alibre Design does not require VB specifically. Any programming language that can integrate COM objects will do the trick.

Internal Units

Alibre Design works in centimeters internally, so we much convert our cube dimension accordingly. It doesn't matter what units the user prefers because Alibre Design will convert to those units from centimeters automatically. We just need to get the measurements into Alibre Design in centimeters. We'll also set up some other data here.

' Internal Units & other variables
Dim dimension As Double = 2.54D  ' 2.54 cm = 1 in. 
Dim filePath As String = "c:/"
Dim partName As String = "MyCube"

// Internal Units & other variables
double dimension = 2.54D;  // 2.54 cm = 1 in. 
string filePath = "c:/";
string partName = "MyCube";

Connecting To Alibre Design

A hook essentially enables communication between different applications. Alibre Design provides this by way of the AlibreX.AutomationHook COM object, which is installed and registered on your system when you install Alibre Design. We want to connect to a running instance of Alibre Deisgn, so we'll access the Running Objects Table (ROT) via the GetActiveObject() method, and cast the result to the Alibre AutomationHook. (You can also start up Alibre Design if it's not already running, but that's out of scope for this example.) Then we'll grab a reference to the hook's IADRoot, which is basically like the "Home" window of Alibre Design, enabling us to create parts, assemblies, etc.

' Connect to Alibre Design
Dim hook As AutomationHook _
    = Marshal.GetActiveObject("AlibreX.AutomationHook")
Dim root As IADRoot = hook.Root

// Connect to Alibre Design
AutomationHook hook = (AutomationHook)Marshal
    .GetActiveObject("AlibreX.AutomationHook");
IADRoot root = (IADRoot)hook.Root;

Creating a New Part

Now we'll create the part and assign a couple of its properties. Note that we're converting from an RGB value of (255,0,0) to a BGR value as an integer. We do this because Alibre Design likes to think of colors in terms of blue-green-red sets of values, and the normal order you see working in Windows is red-green-blue.

' Create a New Part
Dim part As IADPartSession _
    = root.CreateEmptyPart(partName, False)
part.Color = Color.FromArgb(255, 0, 0).ToArgb()
part.Reflectivity = 50

// Create a New Part
IADPartSession part 
    = root.CreateEmptyPart(partName, false);
part.Color = Color.FromArgb(255, 0, 0).ToArgb();
part.Reflectivity = 50;

Creating A Sketch

First let's get a design plane to work with. Because we're making a cube that's centered on the origin, we can just use the first plane (probabaly XY-Plane). There are tips for tracking down the localized names of planes in the API documentation, but for now we'll just stick with this. We'll start by getting IADDesignSession interface from the part.

' Get the first design plane
Dim design As IADDesignSession = part
Dim plane As IADDesignPlane =
    = design.DesignPlanes.Item(0) ' first plane

// Get the first design plane
IADDesignSession design = (IADDesignSession)part;
IADDesignPlane plane = design.DesignPlanes.Item(0); // first plane

Now we'll add a sketch based on the plane, give it an appropriate name.

' Add a sketch
Dim sketch As IADSketch _
    = part.Sketches.AddSketch(Nothing, plane, "Square")

// Add a sketch
IADSketch sketch 
    = part.Sketches.AddSketch(null, plane, "Square");

Now draw the square. Note that we must call BeginChange() and EndChange(). These methods in effect "activate" the sketch for 2D drawing. You can ALT-TAB over to the Alibre Design part during all of this and actually see it working on these commands.

' Draw the square
' allow us to center about the origin
Dim offset As Double = dimension / 2D  
Call sketch.BeginChange()
sketch.Figures.AddRectangle(-offset, _
    -offset, offset, offset)
Call sketch.EndChange()

// Draw the square
  // allow us to center about the origin
double offset = dimension / 2D;
sketch.BeginChange();
sketch.Figures.AddRectangle(-offset, 
    -offset, offset, offset);
sketch.EndChange();

Creating an Extrusion Feature

Now we'll create a simple extrusion feature and add a comment to its parameter while we're at it. Note that parameters must only be changed from between OpenParameterTransaction() and CloseParameterTransaction() calls, which are part of the Parameters collection of the part's IADSession interface.

' Create an Extrusion Feature
Dim session As IADSession = part
Dim extrusion As IADExtrusionFeature _
    = part.Features.AddExtrudedBoss( sketch, dimension, _
    ADPartFeatureEndCondition.AD_MID_PLANE, _
    Nothing, Nothing, 0D, ADDirectionType.AD_ALONG_NORMAL, _
    Nothing, Nothing, False, 0, False, "MyCube", _
    "The Depth Parameter", Nothing)
Call session.Parameters.OpenParameterTransaction()
extrusion.DepthParameter.comment _
    = "This is an important feature."
Call session.Parameters.CloseParameterTransaction()

// Create an Extrusion Feature
IADSession session = (IADSession)part;
IADExtrusionFeature extrusion 
    = part.Features.AddExtrudedBoss( sketch, dimension, 
    ADPartFeatureEndCondition.AD_MID_PLANE,
    null, null, 0.0D, ADDirectionType.AD_ALONG_NORMAL,
    null, null, false, 0, false, "MyCube", 
    "The Depth Parameter", null);
session.Parameters.OpenParameterTransaction();
extrusion.DepthParameter.comment 
    = "This is an important feature.";
session.Parameters.CloseParameterTransaction();

Saving and Closing the Part

We also use the session interface to save and close the part. Note the explicit "boxing" of the string into an object to ensure compatability with the SaveAs() method.

' Save and Close the Part
Dim temp As Object = filePath
Call session.SaveAs(temp, partName)
Call session.Close(False)

// Save and Close the Part
object temp = (object)filePath;
session.SaveAs(ref temp, partName);
session.Close(false);

Cleaning Up

We late-bound a COM object, so we really should clean up a bit when we're finished with it. The call to GC will allow the garbage collector to do a little housekeeping.

' Clean Up
Call Marshal.ReleaseComObject(hook)
Call GC.GetTotalMemory(True)
 

// Clean Up
Marshal.ReleaseComObject(hook);
GC.GetTotalMemory(true);