CATIA V5 – Creating a Catalog of Standard Parts

It is possible to create a Catalog of Standard Parts in two different ways: 

  • Creating a single part as a basis and with the use of the Design Table function, creating a family of similar parts
  • Inserting mutually different parts in the Catalog


The next example shows how to create a standard part, insert parameters and with the help of those parameters creating a family of similar parts. After that the parts are entered in the Catalog.

We need to create a screw with standard parameters according to the picture below.

Kreiranje vijka sa standardnim parametrima

The screw can be modelled without parameters and inserted afterwards. 

Modeliranje vijka bez parametara

After the screw model is finished click on Ikona za dodavanje parametara u CATIAi and add the parameters. For the first parameter select type String and under Part Number assign a value (P1). For parameters d, k, s, a, l the parameter type Length needs to be selected and the values for the first position entered (e.g. M6x12). For the last parameter, Navoj (Thread), select type String as well and enter the value M6. 

Dodavanje parametara u CATIAi


After all of the parameters have been defined, all of the dimensions (within sketch or feature) which are conditioned by the parameters need to be linked together. By double clicking on a dimension in the window Constraint Definition, right click on Value and select Edit formula.

Povezivanje dimenzija s parametrima u CATIAi


In Formula Editor select the parameter from the tree structure, then select OK. The inserted parameter is now visible in the tree structure (if not select Tools/Options/Infrastructure/Part Infrastructure/Display and check the options to show parameters and relations, so they can be visible in the tree structure). 

Dodavanje parametara i relacija u CATIA stablo


In the same way the other dimensions must be linked with the corresponding parameters. On the picture below the screw head height is connected with the parameter k. 

Povezivanje visine glave vijka s parametrom


For the thread add formula under Thread Description and link it with the parameter Navoj (Thread). The length of the thread needs to be defined by formula as well (l – a). 

Dodavanje formule u Thread Description


After the dimensions have been linked with the parameters, a Design Table needs to be created, with which a family of similar parts can be generated. Clicking the icon Design Table  CATIA Design Table, opens a window in which the option Create a design table with current parameter values is selected.

Kreiranje Design table u CATIAi

Clicking on OK creates a Design Table which can be edited and new values for the entire family of parts can be added.

Design Table u excelu

After the Excel table is filled in and saved, a message appears Design Table is synchronized with Excel Table. Now all 10 positions are visible in the Design Table

Design Table s unešenim parametrima

In the tree structure under Design Table the current configuration is shown and can be changed by double clicking on it and then selecting the icon Design Table.

Trenutna konfiguracija u CATIAi

When a different configuration is selected and confirmed with OK the model will be updated according to the parameters for the selected configuration.

Ažuiranje modela prema parametrima

After a family of parts is created we can start making a Catalog. Open a new CATIA file of the type  CatalogDocument (File → New → CatalogDocument). A new folder with the title Chapter.1 appears which can be renamed by right clicking on it, then selecting Chapter.1 object and selecting Definition. On the right hand side of the screen a toolbar for organizing the Catalog is visible. Using the icon Add chapter Add chapter ikona u CATIAi it is possible to add new folders and in this way structuring the Catalog.

CATIA Catalog Document

After adding a new folder, the structure of the Catalog is visible.

Struktura kataloga u CATIAi

Select the folder Vijci (Screws) and click on the icon Add Part Family  Add Part Family ikona u CATIAi. A new window opens in which we need to select a document (part) from which a family of parts will be created. After selecting the document it appears within File name. The title of the family of parts can be changed as well (in this case Hexagonal Head Screws).

Kreiranje familije partova u CATIAi

By clicking  OK the family of parts is generated. If we select the family we can see all of the parts (as a list or graphically, by clicking on tab Preview).

Pregled partova u CATIAi

Inside one folder more families of parts can be created. Select the folder (double click) then click the icon Add Family Add family ikona u CATIAi . A new window opens where the name of the new family is entered. In this case a family of parts named Hexagonal Socket Head Screws is entered and becomes immediately visible in the tree structure.

Dodavanje imena familije partova u CATIAi

In the created family it is possible to individually add parts by clicking the icon Add Component Add Component ikona u CATIAi. A window appears in which we select the part we want in the family. The procedure needs to be repeated for each part.

Dodavanje parta u familiju u CATIAi

After the new parts are added, they become visible within the family.

Pregled partova unutar familije u CATIAi

The Catalog is saved the same way as part with the difference that the extension catalog is assigned automatically.