|This task shows you how to generate resolved parts from parametric parts.|
|Each parametric part
that you use to generate resolved parts must refer to a design table. The
design table must have a column called "PartNumber", which should have a
value. This value is used to name the generated resolved part.
A project resource is used to control the naming convention for the generated part. For the resource PartiallyResolvedReferencePartNumberOptions, if the value of the Location field is 1, then the Part Number used in the design table is used for the name.
If the value is 2 then the object naming rules are used for naming.
You must be in design mode to generate parts. If you are in cache mode then you will not be able to generate CATShapes.
|1.||Create a directory and place in it the
parametric CATPart documents, associated design table documents and
CATShape documents, if any.
Create a second directory to hold the resolved parts when they are created.
|2.||Open a command prompt window and
change to the directory ...intel_a\code\command.
Type the following and press Enter: CATCloGenerateResolvedParts.bat -env
XXX YYY where EEE is the name of the CATIA environment
file. Ask your system administrator if you do not know its
name. XXX is the full path name of the directory
you created in Step 1 to hold parametric parts; and YYY is the
directory created to hold the resolved parts.
For UNIX enter CATCloGenerateResolvedParts.sh /XXX /YYY (replace XXX with the full path name of the directory you created in Step 1 to hold parametric parts; and YYY is the directory created to hold the resolved parts).
You can add certain options to the command line. These are:
-replace Existing parts in your YYY directory will be replaced
-strip The generated resolved parts will be stripped of sketch constraints. Do not use this option for Structure applications.
-direnv If the environment file is not in the default location, then use this option, followed by the full directory path of the environment file location. (The option -env EEE mentioned above is also required.)
For Structures Applications Only: If you are using this task
to resolve sections for structures applications like Structure Functional
Design, you must add the following at the end of the command lines listed
Structure parts must have a parameter called "ProfileType". New or existing parameters "PartNumber" and "SectionName" will be valuated with the part number from the design table. New parameters called "FamilyName" and "CatalogName" will be created unless they exist already (the name of the parametric part will be used to valuate these parameters if they do not exist, using the following naming convention: catalogname_familyname.CATPart). The "FamilyName" parameter is used by the automatic catalog creation function (Create/Modify Catalog) to place parts under different catalog families. See also Creating a Specifications Catalog.
|3.||After the program finishes executing, the parts are placed in YYY - the directory you created to hold the resolved parts. Each part has as its name the entry from the part number column of the design table. The design table association is removed from the generated resolved part.|
|4.||Add the parts to a catalog. To add the parts to an existing catalog see Modifying a Catalog. To create a new catalog see Creating a Catalog. See also Creating a Specifications Catalog.|
|If a part does not get added to the catalog it may not have a part type (component object type) defined. In that case you may need to add the part to a catalog individually.|