how can i open a .CATPART as .CATPRODUCT?

how will i be able to save a part file as a product file so that i ca run further simulations and stickers on my part model?

Answer
 
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2 Answers

Practically Software wise not Possible,
But what i thinck your part file made some addional parts, so you want convert into Product file Right?

My Answer: Migration only Possible
First change to V4 and then again change to V5 using Migration Option with Result spec.

Brief Explain Here, just try
If this is result of migration from CV4 -> CV5, you have an option that allows to convert several Solids of one V4 model to a CV5 assembly with several parts. If you don't care about modelling history, you could try this:

- save your part as V4 model (save as - .model)
- Turn option ' CATPart by Solid' on in Compatibility-migration batch settings (tools-options)
- Use migration (Utility-MigrateV4toV5) batch to import V4 model to V5 assembly

=> job is done... I tested it and it works, but modelling history is more or less lost. You can use as SPEC or as RESULT options in impot.

Regards
Ezhumalai

 
Comments 0

You can use the below script to convert CATPart into CATProduct.

Language="VBSCRIPT"

Dim Component As Products
Dim BodyName
Dim OpenComponentName
Dim Pdoc1 As Document
Dim Body as Object
Dim SourceWindow As Window
Dim LastBody
Dim UserSel As Selection

Sub CATMAIN()
Dim ActiveDocument As Document

Dim Pstring As Long
PartName = CATIA.ActiveDocument.Name

Dim Docs As Documents
Set Docs = CATIA.Documents

Dim prods1 As Document
Set prods1 = Docs.Add("Product")

Dim ProductNew As Product
Set ProductNew = prods1.Product

Pstring = InStr(1, PartName, ".CATPart")
ProductNew.PartNumber = Mid (PartName,1,Pstring -1)

WindowsAlignment()
Set SourceWindow = CATIA.Windows.Item(1)
SourceWindow.Activate

Set ActiveDocument = CATIA.ActiveDocument
Set prods2 = ActiveDocument.Part.Bodies

Dim Bodycount
Bodycount = prods2.count

for i =1 to Bodycount

Set Body = prods2.Item(i)
BodyName = Body.Name

ActiveDocument.Selection.clear
ActiveDocument.Selection.Add Body
ActiveDocument.Selection.Copy
ActiveDocument.Selection.clear

Dim PartNew As Product
Set PartNew = ProductNew.Products.AddNewcomponent ("Part", BodyName)

ProductNew.Parent.Activate

PartSearch (ProductNew.Parent)

ProductNew.Parent.Selection.Clear
ProductNew.Parent.Selection.Add ProductNew.products.Item(PartNew).ReferenceProduct.Parent.Part
ProductNew.Parent.Selection.Paste
ProductNew.Parent.Selection.Clear

next
ProductNew.Update

End Sub

Sub PartSearch(Opar1)
Dim E As CATBSTR
Dim Was (0)
Was (0) = "Part"

Set UserSel = Opar1.Selection
UserSel.Clear

UserSel.Search("CATPrtSearch.PartFeature,all")

End Sub

Sub WindowsAlignment()

Dim Windows1 As Windows
Set Windows1 = CATIA.Windows

Windows1.Arrange catArrangeTiledVertical

End Sub

 
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