Useful Tips

Useful tips and restrictions concerning parameters, formulas, and design tables are available in the CATIA Infrastructure User's Guide.

Relations

When using some objects, you need to indicate the destination of the formulas and the rules that valuate the parameters of these objects. If you valuate a time parameter in a kinematic simulation for example, the relation will not be located below the Relations set but in the mechanisms and commands tree of the simulation.

Hiding relations

You can hide a knowledge relation (formula, rule, check, ..) by right-clicking this relation in the specification tree and by selecting the Hide command.

A visual indicator located at the Relations set level indicates that the set contains hidden relations.
Note that this indicator is not recursive.
If you try to delete a relations set containing hidden relations, a message is displayed asking you if you want to delete the relations set that contains hidden relations.
Note that if you try to delete a relations set containing another relations set with hidden relations, the message will be displayed.

Relations Updates

The evaluation of relations containing measures can be integrated to the Part update only. In a .CATProduct or in a .CATProcess file, to create a parameter

which value is the result of a relation containing measures
updated when modifying the measure inputs:

Create the relation containing the measure at the Part level.
Integrate the relation evaluation to the Part update.
At the Product or the Process level, create a relation that valuates the parameter by using the result parameter of the relation created at the Part level. To get an example, see KwrUpdate.CATProduct.
Perform a local update at the Relations level.

Syntax errors in relations message

When loading a document, the message can appear asking you to load the necessary libraries. It means that during the load, some relations appeared as broken.

These relations use functions that are not recognized by the dictionary because the library containing the definition of the function is not still loaded. That's why you are asked if you want to load all the libraries containing functions definition. But loading all libraries may have an impact on performance. So, we recommend you to load only the libraries you are interested by. To do so, select the required libraries in the Knowledge Environment tab (Tools>Options>General>Knowledge>Knowledge Environment.)

More on Parameter Modification

A parameter is modified only when valuating it with a value that differs from the previous one.

For example, if we have the following language in a relation, each time the relation is evaluated, the parameter Real.1 is modified:

{ Real.1 = 0 Real.1 = 2 }

If a relation tries to valuate a parameter with the same value, then there is no impact at all.

For example, Real.1 = 0 is valuated only when Real.1 is not equal to Zero. When the value of Real.1 after evaluation of rule is same as it was before evaluation, then it does not impact the CATProduct or CATPart.

Rules

In a rule using features that need the geometry to return the type (such as extrudes), when the feature is deactivated, the type cannot be returned. To solve the problem, use the Set command to indicate the type in the rule. For more information, see KwrSetType.CATPart.
When working in Drafting workbenches, do not create rules applying to features to access the attributes of these features.

Rules and Update Cycle

This configuration is allowed because a modification of the parameter activity does not impact the formula update. But:

In such a case, it is highly recommended to use the reaction feature.
If you want to use a rule, do not deactivate and reactivate the activity parameter.
When working with a UDF feature, make sure that you have inserted the relation set when defining the UDF.

Loops

Generic Naming: Generic naming is a CATIA technique which creates a label whenever an element has been selected interactively. This label is a coded description of the selected element. When you specify a fillet to be applied to a face, you must select interactively the face definition but prior to doing this you must of course have generated the face to be filleted. This is why scripts requiring face, point or edge definitions cannot be generated in one shot. You don't have to mind about the generic naming itself as it is automatically captured from the geometry area. The thing you have to mind about is the order your instructions are to be written and executed in the script.

Message "property does not exist...": Check in the browser that the attribute name is correct. For attributes of list type (Fillets and Chamfers), check the indexes. The indexes specified must be consecutive from 1 to n without any gaps.

It is strongly recommended that you use Knowledge patterns instead of using Loops.

Specifying a File Path (2 methods)

Syntax

There are 2 ways to specify the file path:

import "File path"; : Indicate the path of the file to be imported:
import "E:\users\kwecx\Models\PartImport.CATPart" ;.Note that you must enclose the path within quotation marks and end the import statement with a semicolon (;).

import "File Name"; : Indicate only the name of the file to be imported if this file is located in the same directory as the document containing the loop: import "PartImport.CATPart";. Note that:

You must enclose the document name within quotation marks and end the import statement with a semicolon (;).

The file to be imported must be located in the same directory as the document containing the loop.

The document containing the loop must be saved.

To specify a file to be imported, you can use Insert File Path from the contextual menu. Selecting this command displays a file selection window. Quotation marks are automatically included but not the semicolon

Importing Sketches: Recommendation

When designing a document to be generated by a script, it is better to group all the required sketches in a single file. That way:

you minimize the overall size of your sketch-related data

no matter the method used to specify the input file, specify the path once

the design of the final document is made easier. You get a global view of the sketches on which the other features rely.

Specifying Strings: Recommendation: Double quotation marks as well as single quotation marks of apostrophe type (`) can be used to delimit strings. Single quotations marks (`) must be used to enclose character strings which contain other strings.

Reactions

There are 2 ways to react to parameter changes using the reaction feature:

Select the parameter and react to its Value Changed event

Select the feature (that owns the attribute corresponding to your parameter) and react to the Attribute Modification event. Note that this method does not work in all cases.

If you create a User Feature embedding a reaction that will be launched when the User Feature is instantiated, select Owner in the Reaction dialog box and make sure that the reaction is one of the internal components of the User Feature. If not, the reaction will not be launched when instantiating the User Feature.
When creating reactions that react to updates, do not delete or add features which impact the update therefore it may lead to an update error.

V6 to V5 Compatibility

The Knowledge features Viz. Parameters, Formulas, Equivalent dimensions, Laws, Rules, Checks, Set of equations, Reactions, Relation sets, Parameter sets, Actions, VB Actions, Optimizations, and rulesets embedded in the V6 representation can be fully retrieved in V5.

In case of Design Table, the source file is stored in the database and thus the file would lose the link after the import. To retain the data stored in the source file, you can select the option Duplicate data in CATIA model in Design Table properties dialog box. By using this option, the content of the source file of the Design Table is imported and is embedded in the CATIA Model.

You can modify the configuration on the imported data and apply the changes to your designs. You can also use the data in V6 if the data is re-imported to V6.