Saving CATIA Version 5 CATPart Documents As CATIA Version 4 Models

This task shows you:

when a Progress Bar appears during the conversion of a CATPart into a model.
how to save CATIA Version 5 CATPart documents as CATIA Version 4 models, with particular cases.

This save procedure allows you to translate V5 data into native V4 Format. Sometimes, some entities are degenerated during the transfer. Therefore, when the transfer of some elements is incomplete, a report is available.

This page is divided in several steps:

Using a Progress Bar, Particular Cases of V5/V4 translation,: Saving a V5 CATPart As a V4 Model: Report of Identifiers,; Saving a V5 CATPart As a V4 Model: G1 Concatenation,; Saving a V5 CATPart as a V4 Model: Keep V5 Face Color,

Using a Progress Bar

When saving a CATPart as a .model, the user can see a Progress Bar during the process, giving the different steps of the migration.

Open a CATPart in CATIA V5.

Save this CATPart as a model. The Progress Bar appears, giving the different status of the V5 to V4 data translation:

First step: opening the model:

The Progress Bar corresponds to the creation and opening of the .model (empty). This step is generally very rapid.

Second step: converting the CATPart into V4 Data:

V5 data are converted into V4 data.

Third step (optional): checking V4 compliance rules:

Checking and possible modifications are made on the V4 data specifications that you have just created. This step is optional and it is launched only if repairs are necessary.

Fourth step: closing the model:

Particular Cases of V5/V4 translation

During the process of saving a V5 CATPart as a V4 Model, the colors of the Faces and the Identifiers of the Part Body and Open Body are automatically maintained in the model. During this V5/V4 translation, G1 concatenation takes place in order to get as few Surfaces as possible. You will find a demonstration in:

Saving a V5 CATPart as a V4 Model: Report of Identifiers
Saving a V5 CATPart as a V4 Model: G1 Concatenation
Saving a V5 CATPart as a V4 Model: Keep V5 Face Color

Once the Save As Model operation is completed, the resulting .Model file can be manipulated like any other existing. Model files.

Only the V5 elements in SHOW mode can be translated into V4 format: The V5 visualized geometry is transferred into V4 setting. You can work with V5 entities within the V4 environment.

The Save As Model Operation generates V5 geometry and topology into V4 and keeps canonical shapes :

V5 part bodies and volumes will be translated into V4 Solids without history.
a V5 Surface is translated into a Face or a Skin in V4.
V5 Wireframes are transformed into V4 Curves, Planes, Lines, ...
V5 Axis Systems are transferred into V4 Axis Systems.

Open the document MultiBodyAssembly.CATPart. It looks like this:

You will remember that in Version 4 the declaration parameter catsite. Writing_Code_Page declares the code page to be stored in the CATIA data to be written. Such information such as the writing code page was specified in V4 by means of the parameter settings in the declaration files. These declaration parameters are no longer supported in CATIA Version 5. Such information must therefore be provided by means of the dialog boxes described below, before attempting to save a V5 CATPart document as a V4 model.

If you want to use the writing code page ISO-8859-1 go straight to step 4. It is the default value so normally, unless another code page was already specified, you can go ahead with the save.

However, if you want to use a writing code page other than ISO-8859-1 start with step 1.

Select the Tools > Options... command. The Options dialog box appears with the General category selected in the left-hand column.
Click the Saving As V4 Data tab. For more information about these settings, please refer to Customizing.

Open the Writing_Code_Page list in the V4 Declarations part of the dialog box (indicated by the arrow above). Select the appropriate code page and click OK.
You can modify the V4 Model Dimension in order to be consistent with the V4 destination site value.
Select the File > Save As... command.
In the Save As dialog box, select the location of the .model document to be saved and rename it (or not) as required.
Click the Save as type: list and select model in the list displayed as shown below:
In the same box, click on Save. The MultiBodyAssembly.model just created can now be opened, in CATIA Version 4 and will look something like this:

Here is a summary of the translation of V5 Features into V4 Elements:

V5 Features (in the CATPart) =>	V4 Elements (in the model)
1 Surface	1 Face (*FAC)
1 Face	1 Face (*FAC)
Several Faces (contained in a Surface)	Skin (*SKI)
Sketches, Wireframe	Curves (CRV), Lines (LN)
Several Curves and Lines	Composite Curves (*CCV)
Part Body	Volumes (*VOL) (SolidE entity)
Open Body	Curves, Lines, Points, ...

If some elements cannot be correctly transferred, the migration of V5 data into native V4 format generates a report file (.rpt). Therefore, V5 CATPart documents are translated into V4 Models with an enhanced report of errors and problems. This report has the same name as the CATPart document and its location is:

on Windows: in C:Documents and Setting/Username/Local settings/Application Data/DassaultSystemes/CATReport

on UNIX: in /u/users/username/CATReport

By this way, the message lets the user know which element could not be translated in V4. Additional information about the error cause is provided as well. The supplied information (error cause) can be:

Detection of a gap greater than the maximum allowed value

Detection of an element with a dimension smaller than the minimum allowed value

Detection of a shell which cannot be closed into a volume or of faces which cannot be joined into a shell

A surface which is too small.

Here is the content of a report file:

`INFORMATIONS`
`Report File Name`	`C:/Documents and Setting/$Username/Local settings/Application Data/DassaultSystems/CATReport/MultiBodyAssemble.rpt`
`Originating Files Data`
`Input File`	`E:\V5ToV4PartMigr.tst\FunctionTests\NonManifoldAndOpenVolume.CATPart`
`Output File`	`E:\V5ToV4PartMigr.tst\FunctionTests\NonManifoldAndOpenVolume.model`
`Information for the` `Feature`
`Diagnosis`	`There is one or several non manifold edges`
`Information for the` `Feature`
`Diagnosis`	`The shell cannot be closed into a volume`
`Result of migration`	`0 of the 197 faces have not been migrated. The successful rate for the faces is 100`
`Result of migration`	`2 of the 2 volumes have not been migrated. The successful rate for the volumes is 0`

Saving a V5 CATPart As a V4 Model: Report of Identifiers

This task shows that you can save a CATIA Version 5 CATPart as CATIA Version 4 models with the reporting of V5 Identifiers (names) in the V4 Model.

The report of V5 Identifiers in the V4 Model can be applied on Part Bodies and Open Bodies.

Part Body features are converted as volumes. The Save As Model operation creates a SolideE entity (Exact Volume). During the Save As Model operation, the identifiers of the solid is no longer " *SOLn " and it automatically becomes the same identifier as the Part Body feature.

Open Body features and Sketches are converted as follows:

V5 surface features are converted as faces (*FAC). If the V5 feature consists in several faces, the Save As Model operation automatically creates a federating Skin (*SKI). V5 Identifiers are reported on the V4-generated Skin elements.
V5 Sketches and Wireframe features are converted as V4 curves (*CRV) and lines (*LN). If the V5 feature consists in several curves or lines, the Save As Model operation automatically creates a federating composite curve (*CCV).

V5 Identifiers of Open Body features are reported on V4 elements contained in the model.

For more information about the results of the V5 to V4 translation, please refer to the table above.

To illustrate this behavior, please look at the following image:

The identifier of the Part Body, Feat1, is kept and transferred into the .model.

The attributes of V5 Points (*PT) and Lines (*LN) are not taken into account during the Save as Model operation. You can compare this CATPart and the results of its conversion:

Points and Lines have lost their type attributes (thickness, dotting, star, cross, plus) during the V5 > V4 Migration.

Saving a V5 CATPart As a V4 Model: G1 Concatenation

In CATIA V4, surface of good quality are G1-continuous. In CATIA V5, the surfaces must be C2-continuous. It means that a surface already continuous in tangency must be continuous in curvature for the V5.

So copying a V4-surface and paste it into a CATPart often requires to split it in several surfaces. Thus, in order to reduce the topology and geometry complexity when going back to the V4 by saving a part as a model, surfaces are concatenated when the G1-continuity can be kept during their transfer. The number of faces lying on these surfaces are concatenated when possible. The result is : simplification of the geometry and topology by reducing the number of elements. It is also a means to retrieve a V4 topology similar to the one that would be used to generate a V5 Part.

Open the SIMPLIF-EXAMPLE-1.model document.

Copy/Paste the .model document into a V5 CATPart in order to be able to add geometric elements in the CATPart in CATIA V5 (in the FreeStyle workbench).

During the transfer into CATIA V5, the initial V4 Surfaces, copied As Result, are splitted into several Surfaces in order to keep a C² continuity. They are still NUBS Surfaces.

When going back into CATIA V4, you must be able to find the same original Surfaces, when they have not been modified in CATIA V5. This is why there is a reconcatenation if a G¹ continuity with V4 tolerances is detected between Surfaces originating from the same V4 initial Surfaces.

The faces lying on the concatenated Surfaces are simplified with an elimination of the shared Edge chains.

Save this CATPart As a V4 model to go back into CATIA V4 and be able to use a V4 application.

Note that the number of Surfaces have been reduced. During the V5 to V4 translation, Surfaces are concatenated when the G1-continuity can be kept during their transfer. It allows a de-synchronization of the migration of the Geometric Modeler's applications, in CATIA V5.

In CATIA V4, to be able to retrieve the concatenation of the whole initial V4 Surface, you must have migrated either all this Surface into CATIA V5 or a topology containing all the G¹ cuttings.

Saving a V5 CATPart as a V4 Model: Keep V5 Face Color

During the process of saving a V5 CATPart as a V4 Model, the colors of the Solids, Faces and Skins are automatically maintained in the model:

Save as model with face color kept

Previously, only one color -the color of the PartBody- was reported onto the .model. Now, it is possible to transfer the colors of different Faces belonging to the same Surface.

As there are more colors in V5 than in V4, V4 color is the "nearest" color defined in the V4 color table.
Moreover, the Transparency attribute cannot be migrated into the model because this attribute does not exist in CATIA V4.

During the V5 > V4 translation, this is the color of the V5 document that is associated to the model not the color eventually associated to a Layer in Standard/Color/Layer in CATIA V4.

During the migration, the following window may appear:

This window means that memory usage has reached its limit. The process has not enough memory to migrate volume into solid. You can try the same operation in associative mode or in not associative mode with "No solid creation" option (refer to Tools Options > Compatibility > Saving as V4 Data). If it still does not work, you should try to reduce the size of the CATPart.