Logging in to CATIA as an Admin to Revise CATIA Standards

The CATIA V5 Standards define default values for the element properties within the program, such as the default drafting standards and user standards. Default values for annotations and dimension units can be customized by changing the CATIA V5 standards. But first, there is preparation that must be done before making these changes. 

Contents

Define the Environment Variables Needed to Edit the Standards

The Standard Definitions must be accessed in CATIA V5 Admin Mode

Opening CATIA via Administration Mode

There are two types of Standards available with CATIA V5. Both are located in an application outside of the CATIA The first type is Default Standards, which are provided by Dassault Systèmes. These files are stored in the location defined by the environment variable CATDefaultCollectionStandard. The default location of the default Standards is set by Dassault Systèmes to be:

C:\Program Files\Dassault Systemes\BXX\win_b64\resources\standard

Figure 1: An example of the default Windows folder for a Windows 64-bit installation on Environment Editor

The second type of Standards available is User Standards, which are also known as the Customized Standards. These Standards are created and managed by the CATIA V5 Administrator. They are stored in the locations defined by the environment variables CATReferenceSettingPath and CATCollectionStandard. By default, values for these environment variables are not defined, as shown in Figure 1.

Your paths will look similar to these, and you will be adding them to enable customization:

C:\Program Files\Dassault Systemes\BXX
C:\Program Files\Dassault Systemes\BXX\win_b64\resources\standard

To modify the CATIA V5 Standards, we will reproduce the steps taken throughout the following sections.

Define the Environment Variables Needed to Edit the Standards

1. Open the Windows Start Menu > All Programs > Navigate to your CATIA Folder
2. Expand the folder and right-click on Environment Editor > Select More > Run as Administrator
   
   Figure 2: Opening the Environment Editor application as Administrator
   
   The Environment Editor from Figure 1 will open. The CATReferenceSettingPath variable defines the directory that stores the Administrator's CATSettings files that are created when modifying CATIA settings in admin mode. This is also the location for the storage of the locked CATSettings.
3. Navigate to the following locations within your (C:) drive, and copy the paths in Figures 3 and 4. NOTE: The example in this process uses the install folder "B29." Your install folder may be formatted differently.
   Figure 3: Location for CATCollectionStandard
   
   Figure 4: Location for CATReferenceSettingPath
   
4. You will then right-click on the two different locations in the environment, select Edit Variable, and paste the 2 addresses in their respective locations. See Figure 5 below. Right-click near the location noted in the bottom right, and select Save:Figure 5: Shows where to place the file paths and Save afterwards
5. Select Yes when this message pops up:
   
   Figure 6: Environment Editor modify confirmation message

The Standard Definitions must be accessed in CATIA V5 Admin Mode

Open CATIA and access the Standard Definitions using Tools > Standards. Because you did not open CATIA in Admin Mode, you will only be able to view the Standards. The Standard values are not editable (greyed out), and the Save as New icon is not selectable. This is shown in Figure 7.

Figure 7: Standard Definition Window - View Mode

For example, when you open a new drawing in CATIA and attempt to make a drawing of a part, even if it is a metric part, the Standard Dimensioning will be in Feet-Inches. You would have to revise each dimension to Metric as you created them, as shown in Figure 8. Here’s how to revise that standard setting so your drawings will now create Metric dimensions.

 
Figure 8: Numerical Display showing FEET-INC as the default

Opening CATIA via Administration Mode

1. Close any CATIA sessions.
2. Then open a Command Prompt window as shown in Figure 8, select Run as administrator
   Figure 9: Start Menu, opening the Command Prompt as Administrator
3. Change the directory by typing in cd C:\Program Files\Dassault Systemes\B29\win_b64\code\bin
4. Type in cnext -admin at the end of the next line in Figure 9
   Figure 10: "cnext -admin" typed into the Command Prompt
5. A new CATIA session will open in Administration Mode. Select OK
   Figure 11: Administration Mode
6. Select Tools > Standards
   
   Figure 12:  CATIA Tools Menu showing the Standards option
7. Navigate to Styles > Length/Distance Dimension > Default > Value Display Format
8. Within Main Value and Dual Value, you can choose to set the
    -Name
    -Displayed Factor Number
    -Precision Mode
    -Precision
   It's best to select Save As New at the bottom of the window to save out a separate Standard if you do not wish to alter the original. 
   
   Figure 13: Demonstrates the Standards Menu and tree to navigate to the Value Display Format
9. Click OK to save your changes.
10. Close the CATIA Administration session. Close then restart CATIA, and your Standards are now set to your preferences, as shownFigure 14: The changed Numerical Display Description

NOTE: In Drafting, you may need to go to File > Page Setup to set the standard.
 
Figure 15: Page Setup Window showing the Standard Dropdown

Figure 16: Standard Change or Update confirmation window.

Select OK to accept the changes.

For further technical support, please contact Hawk Ridge Systems at 877.266.4469 for the U.S. or 866.587.6803 for Canada and support@hawkridgesys.com.