Infrastructure

Getting Started with Automation

This article will show you how to use a scripting language to access CAA V5 automation objects to capture your own know-how and to increase your productivity. You can customize V5 applications to automate repetitive tasks, and to make it fit your own process.

The products that make up the CATIA and DELMIA applications share the same object model which can be accessed, as well as their own objects, by scripts written in Visual Basic with Windows, and scripts written in Basic Script for UNIX.

You can write your scripts from scratch, but you can also use the journalling facility from the Macros ...  command in the Tools menu that records end-user scenarios in scripts you can then use as is or modify. 

 Recording macros is not available in all workbenches.

We put here a simple script example, to show what is scripting, which are the different things to do to script, present briefly the scripting environment and dialog window, and what is journaling. This example is divided into the following parts:

You will then find information about the scripting languages and environments, and some keys for you if you are not familiar with writing macros in Invoking CATIA from a Scripting Language.

1-Recording the Scenario

This scenario creates a circle in a sketch, and uses this sketch to create a cylindric pad.

The recorded macro is stored in a file, and not in the document.

  1. Select the Tools->Macro->Start Recording ...  command to display the Record Macro dialog box:

A default macro library is provided. Macro libraries are places where a macro can be stored, they can be folders, VBA project or Documents.

Depending in the library, you can select different recording languages. Select CATScript to have a result similar to what you will find below.

 
 

  1. Click Start in the Record Macro dialog box to start recording the macro. The Stop Recording dialog box appears.

 
 
  1. In the File menu, click on New, or click on the
    2. icon, and double-click Part to create a new part. A new part is created and a window for this part is opened.
 
  1. Select the xy plane in the specification tree, and select the sketcher icon
    2. to create a sketch.
 
  1. In the sketcher toolbar, select the circle icon
    2. and click twice to successively  indicate the center of the circle and a current point on the circle.
 
  1. Click on the sketcher exit icon
 
  1. Select the pad icon to create a pad on the sketch.
 
  1. In the Pad Definition dialog box, choose a length of 20 mm and click OK. The pad is created.
 
  1. The pad creation is now complete.
 
  1. Click Stop Recording in the Stop Recording dialog box, or select the Tools->Macro->Stop Recording command. Your macro is now stored in the file you have selected.

 


2-Understanding the recorded macro

We detail below, line by line, what has been recorded, following the interactive steps. How to access the macro generated source is explained in the next step (Modifying the Generated Macro):

  1. Starting to record a macro creates the macro file and generates the first instruction stating the scripting language used and the macro entry point, the CATMain sub: 
Language="VBSCRIPT"

Sub CATMain()
  1. Click on the New item of the File menu, or click on the icon , and double-click Part to create a new part generates the following instructions: 
    Dim documents1 As Documents
Set documents1 = CATIA.Documents

Dim partDocument1 As Document
Set partDocument1 = documents1.Add("Part")

    A new document with the Part type is created. To do this, such a document is added to the Documents collection of the CATIA application. 

  2. Select the xy plane and click on the sketcher icon to create a sketch: 
    Dim part1 As Part
Set part1 = partDocument1.Part

Dim bodies1 As Bodies
Set bodies1 = part1.Bodies

Dim body1 As Body
Set body1 = bodies1.Item("PartBody")
    Dim sketches1 As Sketches
Set sketches1 = body1.Sketches

Dim originElements1 As OriginElements
Set originElements1 = part1.OriginElements

Dim reference1 As AnyObject
Set reference1 = originElements1.PlaneXY

Dim sketch1 As Sketch
Set sketch1 = sketches1.Add(reference1)

Dim arrayOfVariantOfDouble1(8)
arrayOfVariantOfDouble1(0) = 0.000000
arrayOfVariantOfDouble1(1) = 0.000000
arrayOfVariantOfDouble1(2) = 0.000000
arrayOfVariantOfDouble1(3) = 1.000000
arrayOfVariantOfDouble1(4) = 0.000000
arrayOfVariantOfDouble1(5) = 0.000000
arrayOfVariantOfDouble1(6) = 0.000000
arrayOfVariantOfDouble1(7) = 1.000000
arrayOfVariantOfDouble1(8) = 0.000000
sketch1.SetAbsoluteAxisData arrayOfVariantOfDouble1

Dim factory2D1 As Factory2D
Set factory2D1 = sketch1.OpenEdition()

    A Sketch object named Sketch1 is added to the Sketches collection using the reference1 Reference corresponding to the XY plane as a support. Using a reference allows to create a sketch either on an element, as here the XY plane, or on a solid planar face that is not directly accessible as a VB object. 

    The SetAbsoluteAxisData method is used to define the orientation of the sketch axis, that can be on either side and can rotate inside of the support plane. A Factory2D object is created by opening the sketch editor against the created sketch. This Factory2D object features methods to create 2D objects.

Dim geometricElements1 As GeometricElements
Set geometricElements1 = sketch1.GeometricElements

Dim axis2D1 As GeometricElement
Set axis2D1 = geometricElements1.Item("AbsoluteAxis")

Dim line2D1 As AnyObject
Set line2D1 = axis2D1.GetItem("HDirection")

line2D1.ReportName = 1

Dim line2D2 As AnyObject
Set line2D2 = axis2D1.GetItem("VDirection")

line2D2.ReportName = 2

When the sketch is created, an axis, that is the aggregation of a center point, and horizontal line and vertical line (directions), is created. 

The axis is retrieved in the GeometricElements collection of the Sketch object, the directions are retrieved as objects aggregated by the axis. The two lines are here assigned an identifier using their ReportName property that will be used by the 3D modeling services to retrieve those elements inside of the sketch. They have no end-user meaning.

  1. In the sketcher toolbar, select the circle icon and click twice to indicate successively the center of the circle and a current point on the circle 
Dim circle2D1 As Circle2D
Set circle2D1 = factory2D1.CreateClosedCircle(0.000000, 0.000000, 10.000000)
    
Dim point2D1 As AnyObject
Set point2D1 = axis2D1.GetItem("Origin")
    
circle2D1.CenterPoint = point2D1
    
circle2D1.ReportName = 3

The CreateCloseCircle method of the Factory2D object is used to create the circle. It is first created as centered at the point (0,0) with a radius of 10 mm. It is then constraint on the axis center point using the CenterPoint property. 

  1. Click on the sketcher exit icon 
        CATIASketch3.CloseEdition
    part1.Update

    The sketch editor is closed and the part udapted.

  2. Select the pad icon to create a pad, and in the Pad Definition dialog box, choose a length of 10 mm and click OK. The pad is created. 
        Dim shapeFactory1 As Factory
    Set shapeFactory1 = part1.ShapeFactory
    
    Dim pad1 As Pad
    Set pad1 = shapeFactory1.AddNewPad(sketch1, 20.000000)
    
    part1.Update

    The AddNewPad method of the ShapeFactory object is used to create the pad. It is created using the sketch and the length of 20mm. The part is updated.
     

  3. Click Stop Recording in the Stop Recording dialog box, or point to Stop Recording in the Macro item of the Tools menu.

This closes the macro recording sequence and saves the macro in the selected file.

This is all what you performed interactively in the previous chapter.

3-Modifying the Generated Macro

This task explains how to modify the generated macro to make it loop on the creation of five identical cylindric pads.
  1. Select the Tools->Macro->Macros... command to display the Macros dialog box.

 
 
  1. Select the name of the macro you have just created and click on Edit to display the Macro Editor window.

 
 
 

You can choose your own text editor to edit the macro by  setting the CATMacroEditor environment variable prior to launching CATIA with the name of the editor program:
    set CATMacroEditor=NOTEPAD

or using Control Panel/System/Environment on Windows, or:

   export CATMacroEditor=vi

On Unix. This editor must be accessible through the PATH environment variable. Consult your administrator for more information on how to proceed.

 

 
 
  1. The instructions written using the bold typeface are those you need to add or modify while the others already exist in the macro: 
    Language="VBSCRIPT"
'My macro creates five cylinders
    Sub CATMain()
...
Dim refer1 As AnyObject
Set refer1 = originElements1.PlaneXY

x = 0

Dim arrayOfVariantOfDouble1(8)
arrayOfVariantOfDouble1(0) = 0.000000
...
arrayOfVariantOfDouble1(8) = 0.000000

For I = 1 To 5

  Dim sketch1 As Sketch
  Set sketch1 = sketches1.Add(refer1)
  ...
  Dim circle2D1 As Circle2D
  Set circle2D1 =                   _
     factory2D1.CreateClosedCircle( _
                          x,        _
                          0.000000, _
                          10.000000)

  circle2D1.ReportName = 3
  ...
  part1.Update 

  x = x + 25
Next
End Sub

    You simply need to initialize a variable, here x, to allow for the sketch position in the plane to vary, and create a loop beginning with the For keyword and ending with the Next keyword. The For keyword specifies the counter variable I which will take all values between 1 and 5 inclusively. Move the array declaration and valuation outside of the loop:  those values do not change. Change the first parameter of the CreateCloseCircle method to x. Increment the value of the x variable to move the next center of 25mm from the previous one. 
 
  1. Save the macro using the File->Save command of the Macro Editor and exit the editor using the File->Exit command.
The source of the modified macro, CAAInfGettingStarted.CATScript, is available in the CAAScdInfUseCases module. Execute macro (windows only).

 

4-Running the Macro

This task explains how to run the modified macro.
After exiting the Macro Editor, you're back in the Macros window:

Your macro should be the current one. You just have to click Run to run this macro. Here is the result.

 

 

In Short

This use case has shown how to record a macro, modify it and then launch its execution.

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References

[1] Adding a Macro as a Command in a Toolbar

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