Copy, Paste, and Replace Instance

[jzecha]

Does anybody have a Macro that does anything close to the following:
1.Copy specific part.
2.Paste Special (Break Link).
3.Isolate Pasted Part.
4.Replace Initial Instance of Copied Part with Paste Special Isolated Part.
5.Delete Paste Special Part That is Not Being Used.

For context, I am using this on a customer designed tool I have to add Bolt/Dowel patterns too.
The customer used the same angle in 10+ different locations, I am unable to use the same Bolt/Dowel pattern in all those locations.
So I follow the steps above to create an identical part and change the pattern.

 

[HarunMusic]

Hi, i wrote little bit of code for ur problem but i stuck on operation how to isolate part, i cant find solution how to do it?
Is there anyone who knows how to isolate part? I tried with CATIA.command but nothing? Maybe if u have exact elements inside every part, i can isolate that, and it will be the same.

Language="VBSCRIPT"
Sub CATMain()

Dim productDocument1 As Document
Set productDocument1 = CATIA.ActiveDocument

Dim oSel
Set oSel = productDocument1.Selection
Dim strArray(0)
strArray(0) = "Product"
Dim sStatus As String
sStatus = oSel.SelectElement3(strArray, "Select main part", False, CATMultiSelectionMode.CATMultiSelTriggWhenUserValidatesSelection, False)

Dim CopyPart
Set CopyPart = oSel.item(1).value
Dim copyproduct
Set copyproduct = CopyPart.parent.parent

oSel.Add(CopyPart)
oSel.Copy()
oSel.Clear()
oSel.Add(copyproduct)
oSel.PasteSpecial("CATSpecBreakLink")

CATIA.StartCommand "Isolate"
End Sub

 

[ferdo]

Hi

Harun, is not working like this...

You need to create a new CATPart, copy all mechanical features from source CATPart and copy as result in the new CATPart.

Of course you need a loop for more CATParts...

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[HarunMusic]

jzecha can you send example of one part, i need to see what to copy in new part?

 

[ferdo]

If the bodies are published then it would be better to use copy/paste publications...

oActiveDocumentSelection.PasteSpecial "CATPrtResultWithOutLink"



Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[weagan22]

With error handling in VB.NET (not vba):

Sub CopyBreakLinkReplace()

If CATIA.GetWorkbenchId = "Drw" Or CATIA.GetWorkbenchId = "DrwBG" Then
MsgBox("Not for drawings. Try again on a model.", , "Error")
Exit Sub
ElseIf CATIA.GetWorkbenchId <> "Assembly" Then
CATIA.StartWorkbench("Assembly")
End If

Dim uSel As INFITF.Selection = CATIA.ActiveDocument.Selection

If uSel.Count = 0 Then
MsgBox("Please select a product to copy and re-run this macro.", , "Error")
Exit Sub
ElseIf uSel.Count > 1 Then
MsgBox("Please select only one product to copy then re-run this macro.", , "Error")
Exit Sub
End If

If TypeName(uSel.Item2(1).Value) <> "Product" Then
MsgBox("Please select a product to copy and re-run this macro.", , "Error")
Exit Sub
End If

uSel.Copy()
Dim selProd As ProductStructureTypeLib.Product = uSel.Item2(1).Value
Dim topProd As ProductStructureTypeLib.Product = selProd.Parent.Parent

uSel.Clear()
uSel.Add(topProd)

uSel.PasteSpecial("CATSpecBreakLink")

Dim newDoc As INFITF.Document = topProd.Products.Item(topProd.Products.Count).ReferenceProduct.Parent
Dim fileType As String = IO.Path.GetExtension(newDoc.FullName)
Dim newDocPath As String = CATIA.ActiveDocument.Path & "\" & newDoc.Product.PartNumber & fileType 'ActiveDocument must already be saved so that new component can be saved there as well.

CATIA.DisplayFileAlerts = False
newDoc.SaveAs(newDocPath)
CATIA.DisplayFileAlerts = True

Dim newProd As ProductStructureTypeLib.Product = topProd.Products.ReplaceComponent(selProd, newDocPath, False)

uSel.Delete()

CATIA.ActiveDocument.Product.Update
End Sub