V4 Integration Product

V5-V4 Interoperability White Paper
User White Paper
V1.1 (July 2001) CATIA V5R7 level

Introduction
CATIA V5 offers several functionalities to allow the reuse of V5 data in CATIA V4.

The general purpose is not to migrate V5 data into V4 data, but to provide the ability to exchange data between V4 and V5 while both versions coexist. This can happen between several customers, or for a single customer between two processes using different versions of CATIA. Typically, V5 to V4 Interoperability allows the integration of V5 designed parts in CATIA V4 downstream application.

Due to the considerable technological gap between V5 and V4, V5 to V4 Interoperability can not offer a completely seamless integration. This white paper explains some of the restrictions, and also brings some methodologies. However it will show you that CATIA V5 product, V4Integration, provides a unique and powerful interoperability mean between V5 and V4.

Application Levels Requirements
Sessions and models saved with CATIA V5 can be read with any version past CATIA V4.18. There is no exception to this rule.

V5-V4 Mapping

Saving a V5 CATProduct as a V4 session
Since V5R6 it is possible to save a V5 CATProduct as a V4 session. This functionality was only available on UNIX in CATIAV5R6 and is available on Windows NT platform since V5R7.

Generated Data:
The CATProduct is saved as a session document (mode "Save as reference only")

The V5 product has to be in design mode.

CATPart documents referenced by the V5 product are saved as models in the same directory as the session.

Model documents referenced by the V5 product are referenced by the session.

CATPart and .model instances are concerted into model instances (Modelos) in the session, with the same positioning as in the V5 CATProduct.

Nested products are taken into account. Consider the following structure:
product1.CATProduct has two components referencing product2.CATProduct,
product2.CATProduct has itself two components referencing respectively partV5.CATPart and modelV4.model

The resulting session will have four model instances:
2 modelos referencing modelV4.model
2 modelos referencing partV5.model, result of partV5.CAPart saved as a model)

The positioning of the modelos is computed according to the positioning of the instances in product1.CATProduct

Using DLNames
If the session is saved using a DLName, the pointed CATPart documents will be saved using this DLName, and the session will reference the resulting model using this DLName.

On the other hand, the session will reference the.model documents with the same type of links as the product.

Reading the native resulting session in V4 (No file transfer)
Without file transfer, this functionality only makes sense on UNIX platform, since CATIA V4 cannot be run on NT.

On UNIX, both file paths and DLNames used in V5 will have a sense in V4. Therefore the resulting .session document can be read in V4.

DLNames have to be declared in CATIA V4 in the following cases:
If some .model documents are linked using a DLName
If the CATProduct references at least one CATPart and is saved as a session using a DLName

Reading transferred sessions in V4
V4 sessions have not been designed to be used in data transfer. This requires some precautions.

V4 does not offer a Search Order functionality. The links stored in the V4 session have to be readable natively in V4. Therefore the resulting session should only contain DLNames:
All the .model documents should be referenced by the CATProduct using DLNames
If the CATProduct references CATPart documents, the Save As Session should be done using a DLName.

Identifying a V4 Model Coming From a CATPart
A V4 model coming from V5 can be identified in FILE/COMMENT: the CATIA version is V5. For an automatic batch process, a CATGEO routine is available to read this information: GIMVER.

Saving a V5 CATPart as a V4 Model

Generated Data
Any CATPart document can be saved as a model. Save As Model converts all the geometry in show mode.

The Part Body features are converted as volumes. The Save As Model automatically creates a SolidE entity (Extract Volume).

Open Body features and Sketches are converted as follow:
V5 surface features are converted as faces (*FAC). If the V5 feature consists in several faces, Save As Model automatically creates a federating skin (*SKI)
V5 sketches and wire frame features are converted as V4 curves (*CRV) and lines (*LN). If the V5 feature consists in several curves or lines, Save As Model automatically creates a federating composite curve (*CRV).
V5 planes are converted as V4 planes (*PLN)
V5 axis systems are converted as V4 local axis (*AXS)

Save As Model also takes into account some graphical properties:
V5 features layers are reported on the resulting V4 entities.
If the V5 feature is on layer none, the V4 entity is placed automatically on layer 0.
If the V5 layer is superior to 254, the V4 entity is placed on layer 254.
V5 features colors are reported automatically on the resulting V4 entities.
The color affected on the resulting is the nearest color found. V4 and V5 color tables may be quite different. However, if the color tables are similar (in fact if V4 table colors all belong to the V5 table) the resulting color will be identical.
V5 Part Bodies may have colors affected on their sub elements: this can be done in V5 by coloring specifically a feature in the Part Body tree, or even by coloring a face. Those colors will be lost during the Save As Model operation, and the volume will only have the color of the first feature.

Customizing V4 Standards
Save As Model is able to take into account V5 settings to put in place some standards, thus making the generated model compatible with your V4 environment. All those settings are located in Tools/Options/General/Compatibility/ V4-V5 Infrastructure preferences.

V4 code page can be specified through the "Writing Code Page" setting. V4 model dimension can be specified through the "Model Dimension" setting. Note that the tolerances values are computed accordingly to this model dimension value and V4 recommended ratios. V4 model unit can be specified through the "Model Unit" setting.

Other standard values such as thickness can not be parameterized. Save As Model automatically sets V4 default values.

N.B.: in a future release, it will be possible to replace those settings by a unique setting: a V4 Startup model. This will be a functionality equivalent to the "Init Model" declaration variable in CATIA V4.

Tolerances
CATIA V4 and CATIA V5 geometric modellers have two very different concepts for tolerances.

CATIA V4 tolerances are based mainly on two values:
Identical Curves Tolerance (default value: 0.1mm): maximum gap between two geometries to consider them as a single edge.
Intersection/Projection Tolerance (default value: 0.001mm): defines the minimal size of a geometric element.

In fact, CATIA V5 modeller has no tolerances. It does not mean it is not tolerant, but that there is no limit as to how big a gap between two identical points or edges can be.

On the other hand, V5 algorithms compute geometry with a high precision: geometry generated in V5 will have gaps lower than 10-3mm thus ensuring a good compatibility with less tolerant modellers.

In V5 the only remaining concept for tolerances is the resolution which defines the minimum length of a valid object. It is fixed to 10-3mm. The management of confusions ("Do two objects have the same geometry?") is a direct consequence of the resolution: if the distance between to geometric points is less than the resolution, the two points are considered to be geometrically at the same location.

Note: In V4, tolerances are driven by the Model dimension. The most appropriate value to fit V5 resolution is 10000mm. Note that this is also the V4 default value.

Consequences on V5 to V4 Geometry Conversion
Maximum Gap Size:
Theoretically, V5 infinite tolerances may be a problem when translating V5 geometry into V4 geometry. Practically, V5 generated geometry has been computed with a precision higher than V4 tolerances requirements: problems may occur only if V4 model dimension is very low (less than 0.1m)

The only remaining issues are the following:
When you convert into V4 geometries imported in V5 from other less precise modelers. In that case there is no guarantee that the V4 gap tolerance will be respected. Today, if such a problem is met, a solution is to use V5 GSD "Heal Surface" operator to close geometrical gaps. An automatic healing performed during the Save As Model operation is under study.
The V5 "Join" feature allows to assemble surfaces by specifying the maximum gap tolerance. If the specified tolerance is too high, the result of the Join feature may not be merged correctly during the Save As Model. If the Join has been used in a Part Body, the Part Body will not be converted into a volume and a warning will be displayed.

Minimum Element Size:
Translating V5 geometry into V4 can lead to degenerated elements only if V4 resolution is greater than V5 one. This may only happen if V4 model dimension is greater than 10m.

New V5R7:
To reduce the risk of inconsistency due to the difference between the geometric tolerances, a local healing has been introduced in the save as .model process. In R7, this capability is activated by a setting: set V5V4Heal=1. In future releases, this will be the default behavior.

Continuity Criteria
All V5 surfaces and curves are C2-continuous. This means their curvature is continuous.
In V4, surfaces and curves are G1-continuous: basically it means they are continuous at the tangency level.

Consequence on the V4 to V5 geometry conversion, and on a V4/V5 hybrid process:
When converting a non C2 V4 surface, CATIA V5 splits this surface into several C2 patches. The resulting patches can not be selected separately.

However, if you transfer this splitted geometry - or a descendant - back to V4 through a Save As Model, keeping several C2 patches instead of one unique G1 patch may be a problem in some V4 applications such as MFGPROG.

New V5R7
Save As Model automatically detects if several C2 patches have a same topological history and if they may be merged into a single G1 surface or curve. In R7, this capability is activated by a setting: set V5V4Simplif=1. In future releases, this will be the default behavior.