Copying CATIA Version 4 Model Data to CATIA Version 5

• surfaces (both polynomial and BSpline),
• faces,
• volumes,
• skins and exact solids,
• mockup solids (see remarks regarding copy/pasting mockup solids below),
• polyhedral surfaces and solids,
• circles,
• ellipses,
• points,
• lines,
• planes,

• clouds of points,
• edges,
• parabolas,
• hyperbolas,
• curves (both polynomial and BSpline),
• CCVs,
• NURBs (curves and surfaces),
• PIP elements (Tubing),
• GPR elements (AEC Primitives),
• STR elements (planar structures, linear structures).

You should have already completed the task Checking CATIA Version 4 Model Data Before Copying It to CATIA Version 5.

You may want to customize certain settings before proceeding with this task. For more information, see Customizing Compatibility Settings.

1. Open a new CATIA Version 5 CATPart document. To do this, refer if necessary to "Creating New Documents" in the CATIA - Infrastructure User's Guide.

2. In the specification tree or geometry area where the Version 4 model is displayed, select the geometrical element or elements you wish to convert.

3. If you intend to copy the geometry you can either:

• drag and drop the elements onto the appropriate location in the CATIA Version 5 document. The cursor changes slightly i.e. the symbol appears indicating where a drop is allowed. If the cursor changes to the symbol , the drop is not allowed in that location.
• or:

a. Put the element you have selected in the clipboard by clicking Copy , select the Edit > Copy command or select the Copy command in the contextual menu.

b. In the specification tree of the CATIA Version 5 document, select the appropriate item (for example, PartBody or Body.1, Body.2, etc. in the PartDesign workbench).

c. Click Paste or select the Edit > Paste command or select the Paste command in the contextual menu.

This operation recovers the specifications previously put in the clipboard.

4. If you intend to copy the specifications:

a. Put the element(s) you have selected in the clipboard by clicking the Copy , selecting the Edit > Copy command or selecting the Copy command in the contextual menu.

b. In the specification tree of the CATIA Version 5 document, select the appropriate item (for example, PartBody or Body.1, Body.2, etc. in the PartDesign workbench).

c. Select the Edit > Paste Special... command or select the Paste Special... command in the contextual menu.

The dialog box below appears:

d. Select CATIA_SPEC and click OK. This operation recovers the specifications previously put in the clipboard.

5. Click the Update icon to view the copied data or use Edit > Update.

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

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

If you copied the geometry the result should look something like this (using the Window > Tile Horizontally command):

If you copied the specifications the result should look something like this (using the Window > Tile Horizontally command):

• The migration of V4 model data to a V5 document generates a report (.rpt) file named after the model migrated:
• on Windows: in C:\Documents and Settings\user\Local Settings\Application Data\DassaultSystemes\CATReport

• on UNIX: in /u/users/username/CATReport , but this depends on the path setting in env file.

When copy/pasting sets of surfaces : If you want to get a unique surface in V5, it is more efficient to perform the join in V4 before the migration than in V5 on the resulting surfaces.