CATIA macro selection is a very important topic and concept to learn when automating CATIA processes. The following example will show you several useful CATIA programming basics, including:

1. Prompt the user to select multiple parts
2. Search selected parts for a specific element
3. Copy and paste the element into a new part

As usual, I have inserted my comments in the code to help you follow along.

‘Every CATScript begins with this statement

Sub CATMain()

‘start by declaring the selection

Dim oSel As Selection
Set oSel = CATIA.ActiveDocument.Selection

‘Create an array for CATParts

ReDim strArray(0)

‘Display a messagebox prompting the user to select CATIA parts

Dim sStatus As String
Msgbox “Please select parts to join.”

‘SelectElement3 is used to allow user to select multiple parts from the spec tree or the Interactive area

sStatus = oSel.SelectElement3(strArray, “Select parts”, False, CATMultiSelTriggWhenUserValidatesSelection, false)

‘CATMultiSelTriggWhenUserValidatesSelection option displays the following handy little toolbar:

catia vba select

‘Count the number of selected parts
iCount = oSel.Count
‘Create a For…Next loop to cycle through all selected parts
‘Isn’t vb scripting fun?
For i= 1 to iCount
Dim myObject2
Set myObject2 = oSel.Item(i).value

‘Search only the selected objects for the object named “PartBody”
oSel.Search “Name=PartBody,sel”
‘now we take all the PartBody objects found and copy them
ReDim copies(iCount)

For k=1 to iCount
Set copies(k)=oSel.Item(k).Value
oSel.Add copies(k)

‘close the loops
Next ‘k
Next ‘i
‘Now use CATIA scripting basics to create a new part
Dim part2
Set part2 = CATIA.Documents.Add(“CATPart”)

Dim partDocument2 As PartDocument

‘rename the new part
part2.Product.PartNumber = “My New Part”

‘optional step: create a new geometrical set and rename it
Dim GSet1 As HybridBody
Set GSet1 = part2.Part.HybridBodies.Item(1)
GSet1.Name = “My Geometry”

‘set the newly create part to the active document
Set partDocument2= CATIA.ActiveDocument
Dim ActSel As Selection
Set ActSel=partDocument2.Selection
ActSel.Add GSet1

‘paste special the PartBody objects from the orginial file and paste ‘as result without link
ActSel.PasteSpecial(“CATPrtResultWithOutLink” )

‘clear the selection
End Sub
Concluding Thoughts
In this CATScript tutorial you learned several CATIA V5 scripting basics including: how to select multiple objects, how to create a new CATPart, how to create a new geometrical set, how to rename a part, how to rename a geometrical set, how to copy and paste, how to paste special result without link. Please use the contact form if you have any questions.