Copying 2D from CATIA Version 4 to CATIA Version 5

The following task shows how drafting data is pasted As Result from an existing Version 4 model to a new Version 5 document.

Of course, you can also insert the V4 data into an existing Version 5 document alongside existing V5 drafting data by using the same procedure.

  The following data can be copied from CATIA Version 4 to CATIA Version 5:
V4 text thickness is migrated in V5 texts according to the following parameters:
  • if the thickness of V4 texts is superior to 0.2mm, V5 texts are displayed with a bold style,
  • if the thickness of V4 texts is inferior or equal to 0.2mm, V5 texts are displayed with a regular style.

Additionally, the following V3 data can now be migrated directly from CATIA Version 3 to CATIA Version 5:

  • V3 texts are migrated as V5 texts.
  • V3 dimensions are migrated as graphical elements.
    However, you can migrate V3 dimensions as V5 dimensions by using the following methodology: migrate V3 dimensions to V4 first using the V4 process, and then migrate these to V5.
  Refer to Managing standards for V4 to V5 migration of 2D Draw elements for more information on what data can be copied from V4 to V5 and on how to do this.
Open the DraftingInterop.model document and select the DRAFT tab.
  1. Open a CATDrawing document.

  2. In the specification tree or geometry area where the Version 4 drawing is displayed, select the view you wish to copy into CATIA Version 5. You can select several views if you prefer.

  3. Put the view(s) you have selected in the clipboard. To do this, either click the Copy icon , select the Edit->Copy command or select the Copy command in the contextual menu.

  4. In the specification tree of the CATIA Version 5 CATDrawing document, select the appropriate sheet.

  5. Now either click the Paste icon , select the Edit->Paste command or select the Paste command in the contextual menu. This operation recovers the view previously put in the clipboard.

  6. You may want to click the Fit All In icon to fit all data in the window.

Note that the toolbars change depending on whether a CATIA Version 4 model or a CATIA Version 5 document is selected.

The result should look something like this (using the Window -> Tile Horizontally command):


When copying V4 drawing data to V5, bear the following in mind:
  • Whatever the standard of the V4 view was prior to being copied into CATIA Version 5, once in V5 its standard is that selected when you open the CATDrawing document.
  • The smallest unit that you can copy is the view. All the elements that go to make up this view are included in the copy.
  • In the V5 Drafting mode Working Views (Edit -> Working Views), the copy described above creates a V5 view with the same name as in V4. In the V5 Drafting mode Background (Edit -> Background), the V4 elements are copied into the background view of the V4 view.
  • The migration of V4 drawing data to a V5 document generates a report (.rpt) file named after the model migrated:
    • on Windows: 
      in C:\Documents and Settings\username\Local Settings\Application Data\DassaultSystemes\CATReport
    • on UNIX: in /u/users/username/CATReport

    This reports contains different types of information regarding the migration results:

    • location and name of the input and output files, 
    • kind of migration performed (e.g. V4 to V5 CATDrawing), 
    • mode of migration performed (AS SPEC or AS RESULT)
    • status of migration for each V4 element: 
      - Correctly/OK: migration successful
      - KO: migration failed 
      - NOT: migration could not be performed for lack of a CATIA V5 equivalent
    • V4 attributes of V4 elements.
  • If, when importing 2D geometry, you want to create circle centers and curve end points, select Tools->Options,  select the Drafting category in the left-hand column and click the V4->V5 tab. In the Geometry Import section of the window that appears, check the Create centers and end points box.
  • If you want to define dimension conversion as a graphic, select the Tools->Options... command,  select the Drafting category in the left-hand column and click the V4->V5 tab. In the Dimension Conversion Mode section of the window that appears, check the Convert dimension as a graphic box.
  • The V4 structure of Detail/Ditto is migrated in a V5 structure of Detail (2D component reference) /Ditto (2D component instance).

    If you want to use the previous behavior (Explode Ditto) select Tools -> Options to specify the conversion mode of Dittos.

  • You can copy/paste as result V4 transparent views with NHR or HLR representation (the projection mode is retrieved from the browsing).