Selecting a CATPart or Sub-product to work in that document

[l3ob]

I have a VBscript that works well in a catpart but it fails in a catproduct. I want to be able to select the catpart or a sub-product within the top-product to make it active and/or set the partdocument from the list of documents within the product. In the code below, assuming I don't know the name of document "PartName.CATPart", I need to have code to select the tree item and Set partDoc1 from that selection.

Sub CATMain()

Set doc1 = CATIA.Documents

'--------------
Set partDoc1 = doc1.Item("PartName.CATPart")
>>> name not known, so I need to replace this line
>>> with selection process below
'--------------

InputObjectType(0)= "AnyObject"

Set oSelA = doc1.Selection

oSelA.clear

Result = oSelA.SelectElement(InputObjectType, "Select Tree Item", False)

If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If

Set partDoc1 = oSelA.Item(1)
>>>> this is where I'm stuck. I can't get the document
>>>> out of the selection to set partDoc1

Set part1 = partDoc1.Part

Set hybridShapeFactory1 = part1.HybridShapeFactory

 

[AHay]

Hi, You need to use the .Value property of the selected object, e.g. Set partDoc1 = oSelA.item(1).Value.

You should also use .SelectElement2 rather than SelectElement if you want the code to run in R11 onwards.

 

[l3ob]

Tried that. The '.Value' gives a reference not a part document. The next line fails. I need to extract the part document from the selected tree item ( part or sub product )
to make active in whick to work. The 'Set partDoc1 = oSelA.item(1).Value.name' shows the name of the instance....'part1.1', its document would be 'part1.CATPart'.

 

[AHay]

See if this can give you what you are after...

Set doc1 = CATIA.ActiveDocument
InputObjectType = Array("Part", "Product")
Set osela = doc1.Selection
osela.Clear
Result = osela.SelectElement2(InputObjectType, "Select Part", False)
If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If
If osela.Item(1).Type = "Product" Then
' do some sub product code
Debug.Print "Selected Product"
ElseIf osela.Item(1).Type = "Part" Then
' do some part code
Debug.Print "Selected Part"
End If


If it is a product you need to use the PartNumber not the Name and you should be able to construct the appropriate document name from that, e.g.

set oDoc = CATIA.Documents.Item(selecteditem.PartNumber & ".CATProduct")

or something like that. However, you need to ensure that people don't select the 'Product node' for a part in the assembly tree (the node above the part in the tree). If they select the wrong node then the code assumes it is a product and not a part and you would get an error. You just need to put in some simple error trapping or limit them to just parts if this is possible.

 

[l3ob]

From your suggestion, I ended up with the following code example that lets me select the Part in the tree and aquires the .CATPart document.

Within a CATProduct, it works well up until the 'COPY' line. It errors with : Selected element not allowed for this operation!

It works all the way through within just a CATPart.

Sorry to pick your brain, but, got any ideas?

Code:
Language="VBSCRIPT"

Sub CATMain()

Dim InputObjectType(0)
Dim InputDocType(0)
InputDocType(0) = "Part"

Set ActiveDoc = CATIA.ActiveDocument

' Prompt to select destination part document if a Product is active

Set oActDocSel = ActiveDoc.Selection
InputDocType(0) = "Part"
Result = oActDocSel.SelectElement2(InputDocType, "Select CATPart", False)
msgbox result

If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If

Set DestinationDoc = CATIA.Documents.Item(oActDocSel.Item(1).value.name & ".CATPart")

oActDocSel.Clear

Set oSelB = DestinationDoc.Selection

InputObjectType(0)= "Face"
Result = oSelB.SelectElement2(InputObjectType, "Select a face", False)

If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If

oSelB.copy <---- Error:Selected element not allowed for this operation!

msgbox "copied"

End Sub

 

[AHay]

Hi,

Try changing your script to:


Dim InputObjectType(0)
Dim InputDocType(0)
InputDocType(0) = "Part"

Set ActiveDoc = CATIA.ActiveDocument

' Prompt to select destination part document if a Product is active

Set oActDocSel = ActiveDoc.Selection
InputDocType(0) = "Part"
Result = oActDocSel.SelectElement2(InputDocType, "Select CATPart", False)
MsgBox Result

If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If

Set DestinationDoc = CATIA.Documents.Item(oActDocSel.Item(1).Value.Name & ".CATPart")

oActDocSel.Clear

InputObjectType(0) = "Face"
Result = oActDocSel.SelectElement2(InputObjectType, "Select a face", True)

If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If

oActDocSel.Copy '<---- Error:Selected element not allowed for this operation!

MsgBox "copied"


You should perform the copying using the top level document selection object (in this case the active document).

 

[l3ob]

Thanks 'AHay'. This put me in the right direction. The program works in a catproduct and a catpart now.

I had to select the face first from a foreign CATPart within the Product, copy to clipboard , aquire the destination CATPart by selection, and Paste the Externally Linked Surface in the destination.

The only problem I have now is I want the program to check the selected Face properties to see if it is already in the selected destination CATPart and not foreign before I choose to copy/paste. In the full (larger) program, the face is used as a reference for creating normal lines through points.

Resulting Sample code that works:

Language="VBSCRIPT"
Sub CATMain()

Dim InputObjectType(0)
Dim InputDocType(0)

InputDocType(0) = "Part"
Set ActiveDoc = CATIA.ActiveDocument
Set ActDocSel = ActiveDoc.Selection

InputObjectType(0)= "Face"
Result = ActDocSel.SelectElement2(InputObjectType, "Select a Face ", False)

If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If

ActDocSel.copy
ActDocSel.Clear

'Select Destination CATPart

InputDocType(0) = "Part"
Result = ActDocSel.SelectElement2(InputDocType, "Select CATPart", False)

If Result = "Cancel" Then
MsgBox ("Command Canceled")
Exit Sub
End If

Set WorkDoc = CATIA.Documents.Item(ActDocSel.Item(1).value.name & ".CATPart")

WorkDoc.part.InWorkObject = WorkDoc.part
ActDocSel.PasteSpecial "CATPrtResult"
WorkDoc.part.update

Set Ref1 = ActDocSel.item(1).value

End Sub