Motion Simulation in Solid Edge using sketches together with Microsoft Excel VBA Programming Part III

In a previous example, I showed how to control variables in a Solid Edge sketch using a direct link to an Excel spreadsheet. In this example, I am going to show how to use VBA (Visual Basic for Applications) in Excel to control the variables in a Solid Edge sketch directly.

1. Setup Excel VBA

Create a new file in Microsoft Excel.

Press Alt+F11 to enter the Microsoft Visual Basic window as shown below.

Right-click in the Project Explorer on the new file name (in this example, Book2) > Insert > Module.

2. Add References

To make Solid Edge type libraries available to the Visual Basic Object Browser, click References on the Tools menu (or Project menu depending on your version). On the References dialog box, select the Solid Edge libraries you want to access (specifically the Solid Edge Framework Type Library and Solid Edge Part Type Library).

All variable automation is accessed through the Variables collection and Variable objects. The Variables collection serves two purposes: it allows you to create and access variable objects, and it allows you to work with dimensions as variables.

Note: When debugging programs that interact with the Variable Table, it helps to have the Variable Table displayed while stepping through the program. The Variable Table shows the results as they are executed.

3. The VBA Code

Write the following code into the VBA code area as shown below:

You can copy & paste the following code to your Excel VBA module:

' =================================================================
' Example of using VBA code to control variables in Solid Edge document
' By AkeBlogger
' http://mechanical-design-handbook.blogspot.com/
' =================================================================

Sub Simulate()
On Error Resume Next

    'Declare the program variables.
    Dim iAngle As Single
    Dim objApp As Object
    Dim objVariables As Object
    Dim objVariable As Object
   
    '------------------------------------------------------------------
    ' Checking for the active document
    Set objApp = GetObject(, "SolidEdge.Application")
    If Err Then
        MsgBox "You must open Solid Edge before executing this module!!", vbOKOnly + vbExclamation, "Error"
        Exit Sub
    Else
        'Connect to a running instance of Solid Edge.
        Set objApp = GetObject(, "SolidEdge.Application")
        'Access the Variables collection.
        Set objVariables = objApp.ActiveDocument.Variables
    End If
       
    'SIMULATION STARTS!
    For iAngle = 0 To 360 Step 2
        ' Changing Cam_angle from 0, 2, 4, ..., 360 deg.
        Call objVariables.Edit("Cam_angle", iAngle)
       
    Next iAngle
   
End Sub

4. Prepare Solid Edge

Open the Solid Edge file from the previous example and delete the formula in the Variables Table as shown below. In this example, we will control the variable (dimension) using VBA code directly, so the link to the external spreadsheet must be removed.

5. Run Simulation

We are now ready for simulation. Resize the VBA Windows as shown below so you can see both applications, then click run to see the result.

Watch the following video for the actual result!