Using the Interactive Checker

This first task shows you how to check CATIA Version 4 model data before copying it to CATIA V6.

Before checking either the geometry or specifications of Version 4 data, you should understand the distinction between the two:

• The geometry is just the three-dimensional representation of the elements contained in the data. An example would be the set of faces that make up a solid. It is roughly equivalent to the (BRep) used in CATIA Version 4.

• Geometry check is a check by transferring the solid's geometry only through copy - paste special - CATIA_RESULT.
• The specifications are made up of the entire history of the actions performed to obtain the data. They are shown in the form of a tree and are roughly equivalent to the used in CATIA Version 4.
• Specification check consists in transferring the solid with Geometry and the History tree: copy - paste special - CATIA_SPEC. Note that a specification check is only meaningful when applied to and .

1. Select one or more geometrical elements in the geometry area:

   
   
   

   This activates Geometry Check and Specification Check in the Version 4 model toolbar.

2. In the Version 4 model toolbar, click Check Specifications or Check Geometry . The Check Validity dialog box appears: In our example, the Check Validity box shows that: V4 Draft Reflect Line Keep Edges that have been copied / pasted CATIA_SPEC in CATIA V6, are migrated CATIA_RESULT, with their branches. No error is detected during the Check.

   Messages for the solid's transfer with history tree can be:
   

   • Geometry check OK: You can transfer the solid's geometry only through Copy - Paste Special - CATIA_RESULT. When you transfer the solid as geometry only, it is transferred as datum (BRep). You can only perform operations on the geometry.

   • 0 operations not implemented: All the operations (Fillet, Union, Intersection,...) of this solid's tree are implemented, which means that you can start the migration and the same operations will available in CATIA V6.

   • 1 primitive checked as geometry only: One primitive cannot be migrated as CATIA_SPECs, but only as CATIA_RESULT.

   Certain types of primitives will be converted as datum:

   
   
   • Pyramids
   • Sweep Spines, Sweep with non closed profiles, Until a Sweep
   • Projects
   • Import Solids (Link to a solid in another model)
   • If the solid contains one of the above primitives, unsupported solids are transferred as BRep only. The body is based on both specifications and datum features.
   • Draft Reflect Line Keep Edges. This feature is not a terminal leaf into the tree of feature. So all the branch standing before must be migrated CATIA_RESULT.

   In the Check Validity dialog box there are four columns:

   
   
   • the first column showing the overall result, color-coded as follows:
     
     • G (green): will be copied as is to CATIA V6. The check is OK.
     • R (red): will NOT be copied to CATIA V6 as is. This is a KO Check.
     • Y (yellow): will NOT be copied to CATIA V6 because of a link to a red-coded item. This is KO Check due to the element supporting by the solid.
   • the Version 4 identifier,
   • the format i.e. Specifications,
   • the Message column providing the number and type of problems.

3. To view the results of a specification check, double-click on the contents of any of the columns in the Check Validity dialog box. The tree structures of some models are very large. Use the scrollbars to locate any red elements. There are several in the model shown below. Here is just one example:

   
   
   

4. If one element is red, right-click it to find out exactly what the problem is: The $ symbol means that the Pipe item is an unresolved feature in V4 (same symbol in the V4 tree).

5. If you click the background and not an element, a menu containing two options is displayed:

   
   

   • Reframe graph, which centers the tree structure.
   • Print whole, which prints it (for details, see Printing Objects in the CATIA - Infrastructure User's Guide).

6. If you make an Interactive Checker and encounter a reading problem of V4 elements (not updated solid), the copy / paste operation is locked by the Check, the solid cannot be pasted. Then it is advisable to run the

   Using the CATIA V4 Cleaner utility on the model to be copied.

This task shows you how to convert a V4 model despite the invalid geometry of its Skin Offset.

1. Apply a Check validity operation on a V4 model, the model's Skin Offset cannot be converted into CATIA V6 because there is no image of a Skin Offset in CATIA V6.

   In CATIA V4, the Skin Offset is valid but this element cannot be migrated into CATIA V6 and it is systematically KO at the Check operation.

   You can however copy CATIA_RESULT and paste the V4 model into CATIA V6. But it will have the same defective quality in V6 as in V4. The Geometry Check operation allows to analyze the geometry quality of the V4 model's components.

2. You cannot copy / paste the V4 model into CATIA V6 otherwise a warning message is displayed :

   PartBody (*SOL1): The CATIA V4 skin has been partially pasted because of *SKI1 <The V4 element 
   could not be converted: Clean the model>

   It means that the V4 element could not be converted properly and you should "Clean the model". Indeed, you can resort to the Cleaner to repair some anomalies. The Cleaner will check the structural data of the model before migrating it in CATIA V6.

   The user has access to the V4 model geometry (except the Skin Offset) in V6:

   
   
   

   For more information about how to use the Cleaner, refer to Using the CATIA V4 Cleaner

This task explains how the V4 model can be migrated despite a KO Check result (on Surfaces).

The Geometry Check may be valid, but sometimes V4 Geometry cannot be supported in CATIA V6: design is tolerated in CATIA V4 but not in CATIA V6. Therefore, it is necessary to solve this incident during the migration.

1. Apply the Specifications Check on this model: select one or more geometrical elements in the geometry area and click Check Specifications. The Check Validity dialog box appears; the Geometry check is OK for the Faces:

   The Geometry of some Surfaces (*SUR1 > *SUR8; *SUR10, 11 and 13)is invalid but the Faces Check is OK. The Face geometry is valid whereas the Surface geometry is not, because the Face is an element that was created separately.

2. Copy / Paste the V4 model into a V6 representation.

3. Update the representation. You can visualize the model in CATIA V6 but there are anomalies in Surface 3 and Surface 4.

   
   
   

4. Before the Copy / Paste operation, the component does not always have the same shape as in V4. SUR 3 and SUR 4 (enclosed in red) do not have the same quality, both elements are twisted and have X shaped Faces.

5. You can send the invalid geometry in the Shape Design workbench. In the Freestyle workbench, you can display the control points in order to analyze the surfaces and modify them.