When you create a part like a hollow cylinder, you often start by creating a sketch, then you create a pad by extruding the initial sketch, then you add other features to the created pad. The final document is made up of features which define the intrinsic properties of the document. Removing one of these features results in a modification of the document. These features are called parameters. Parameters play a prominent role in Knowledgeware applications. They are features that can be constrained by relations and that can also be used as the arguments of a relation.
In addition to these parameters, CATIA allows you to create user parameters. These user parameters are extra pieces of information added to a document.
User parameters are very handy in Knowledgeware applications:
A given relation may take as its arguments both types of parameters (intrinsic and user).
The user parameters are displayed in the specification tree provided you check the Parameters box in the Display tab in the Tools>Options>Infrastructure>Part Infrastructure dialog box. The user parameter list contains at least the Material parameter. The initial value of the Material parameter is set to None.
In addition, parameters can be displayed with their values provided you check the With Value box below the Parameter Tree View settings in the Tools>Options>General>Parameters and Measure dialog box
CATIA users working with non-Latin characters must check the Tools>Options>General>Parameters and Measure>Knowledge tab>Parameter Names>Surrounded by the symbol'. Otherwise, parameter names must be renamed in Latin characters when used in formulas.
You can access a parameter contextual menu by right-clicking this parameter in the specification tree.
|The Definition... command enables you to access the Edit Parameter window where you can edit the parameter value.|
|The Edit formula... command enables you to access the formula editor to add a formula to the parameter.|
|The Hide command enables you to hide the parameter. In this case, it will not display in the specification tree.|
|The Reorder... command enables you to reorder parameters.|
|The Lock... command enables you to lock the parameter.|
|When working with parameters of Length and Angle type, you can also use the Create Equivalent Dimensions command. For more information about this command, see Getting Familiar with the Equivalent Dimensions Interface or Using the Equivalent Dimensions Feature.|
You can hide a parameter by right-clicking this parameter in the specification tree and by selecting the Hide command.
External parameters are parameters that point parameters located in another document. There are 2 types of external parameters depending on their links:
Reference link type: Both parameters are located in 2 different documents.
Contextual link type: Both parameters are located in 2 different documents located in the same assembly.
You can access the external parameters contextual menu by right-clicking the external parameter in the specification tree. Note that these functionalities can also be accessed in the Edit links dialog box.
|Hide: Enables you to hide a parameter. In this case, it will not display in the specification tree|
|Reorder: Enables you to reorder parameters (if you have created more than 1 external parameter.)|
|Lock: Enables you to lock an external parameter.|
|Open the Pointed Document: Enables you to open the pointed parameter.|
|Isolate: Enables you to isolate the parameter.|
|Activate/Deactivate: Enables you to activate/deactivate the parameter. For more information, see Deactivating and Activating External Parameters.|