COE Administrator
    [Admin Group]
    Ive never touched V4 and I was wondering if I bring in a drawing from v4 to v5 with there be any kind of conflicts. Or is there a certian way to bring a file in to minimize any kind of data loss?
    COE Administrator
    [Admin Group]
    I don't think that you can do it without converting the v4 file into .dxf or any other appropriate extensions. You can copy and maste certain v4 3D models but not 2D.
    COE Administrator
    [Admin Group]

    Sure you can open V4 drawing (.model) to CV5, print, view etc. to it. Then you can copy any data from it (just selects from drawing tree + Copy) and create new CATDrawing (V5 drawing) and there Paste => drawing migrated to V5. Dataloss is quite minimal, performance can be bad, but mainly it actually works.

    For larger amounts of data, you can use Utility that doesbatch conversion of drawings.

    But if you want to save V5 drawing to V4... then you are in trouble.

    Keith Perkins
    [Lionheart Solutions Inc.]
    Do you wish to maintain associativity between the drawing and 3D part geometry used to create it or are you migrating just draw data? If you have 3D data and want to preserve those links then you must migrate your 3D data first (with the elements in the model creating either CATPart or CATProduct files) and then you copy + "paste special" then select AS SPEC when pasting. It will then give you an opportunity to select which 3D data file to associate with the view. You can select a file currently in the CATIA session or you can select a file on your hard drive from a list. It is best to do this separatly for each view because some may contain what V4 CATIA called "View filters" which is similar to overload properties in V5. Experiment with a couple files this way and youll see what I am talking about.

    If you do not wish to preserve links because the V4 to V5 data structure ends up being so dissimilar (in cases of model files with a large number of filtered solids) then you can copy + paste special AS RESULT and you will get V5 views with just normal, unassociated draw data.

    You will however occasionally see formatting changes in Text and some dimensions. Leaders may look different due to the different creation styles. Also, in V4 they used "symbol libraries" a lot which is similar to V5 catalogs to place 2D components. When migrated some of these may have their show/noshow status changed.

    To be absolutly sure you have no physical changes between the actual printed V4 drawing and a V5 drawing you would have to take an HPGL file (a printer language output file) and open it in some third party program, save it as a DXF file then open that in V5 CATIA.....the result will be a V5 drawing with no links but 100% accuratly reflects the contents of the V4 drawing thus eliminating any cleanup of translation errors which occur but also results in a file with little or no value other than archiving legacy data.

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