Setup Catia in Admin Mode to Edit Drafting Standards

Setup Catia in Admin Mode to Edit Drafting Standards

Modifying CATIA Drafting Standards

March 25, 2011

CATIA Drafting Standards 2

Modifying CATIA V5 Drafting Standards

The default units, precision, and various other default drawing properties are controlled by the Drafting Standards XML files that are located, by default in the CATIA V5 installation directory (<INSTALL>\resources\standard\drafting). To modify, or create new drafting standards, CATIA must be launched in Admin mode. From there, changes to the drafting standards can be done through the Tools > Standards… dialog.

Starting CATIA in Admin Mode

Modify the CAT Environment File

A CATIA Environment (CATEnv) is a set of runtime environment variables in a text file that contain a value or a path searched by the software when starting a session. There can be several separate environments for an install of CATIA. By default, the CATEnv text files are located in the following location: Windows XP: C:\Documents and Settings\All Users\Application Data\DassaultSystemes\CATEnv
Windows 7: C:\ProgramData\DassaultSystemes\CATEnv

To start CATIA in Admin mode, the CATReferenceSettingPath and CATCollectionStandard paths need to be modified from their default blank values.

       CATReferenceSettingPath: points to the directory where administrator settings are stored
       CATCollectionStandard: points to the directory containing the standards customized by the administrator. This is where the custom drafting standards will be saved.

Create Custom Directories

1. Create a directory on a local or server share for the administrator settings (CATReferenceSettingPath)
2. Create a directory on a local or server share for the custom drafting standards (CATCollectionStandard) Create a subdirectory in this location named “drafting”.
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Set the CATEnv Variables

1. Open the CATEnv text file to be edited (CATIA.V5R10.B19.txt) for example, and modify the CATReferenceSettingPath and CATCollectionStandard to point to the newly created directories.
2. Save the CATEnv text file.

Create Admin CATIA Shortcut

The Target field of a CATIA shortcut specifies the environment directory where the CATEnv text files are located, as well as the name of the CATEnv file to load on startup.

1. Copy and paste the existing CATIA shortcut to the desktop.
2. Rename the new CATIA shortcut to “CATIA V5R19 Admin” or similar.
3. View the original shortcut’s target, Right-Click on the shortcut on the desktop and select Properties.

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4. Copy and paste the Target into notepad. Here is an example of what the target will look like once pasted into Notepad:

"C:\Program Files\Dassault Systemes\B19\win_b64\code\bin\CATSTART.exe" -run "CNEXT.exe" -env CATIA_P3.V5R19.B19 –direnv "C:\ProgramData\DassaultSystemes\CATEnv" –nowindow

-env specifies the CATEnv file to load (excluding the .txt extension)
-direnv specifies the directory where the CATEnv files are located. This can be a shared directory.

5. Modify the target to include “-admin” after “CNEXT.exe”:

"C:\Program Files\Dassault Systemes\B19\win_b64\code\bin\CATSTART.exe" -run "CNEXT.exe -admin" -env CATIA_P3.V5R19.B19 -direnv "C:\ProgramData\DassaultSystemes\CATEnv" –nowindow

6. Paste the modified target into the Target textbox in the properties of the new CATIA Admin shortcut. Once CATIA loads, a message box will notify you that you are in running in Administration mode.

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Modifying the Drafting Standards

Creating a New Standard

Once CATIA is running in Administration mode, you can edit the drafting standards through Tools > Standards…

1. Select “Drafting” in the drop down box labeled Category.
2. Select the standard you would like to begin to modify in the second drop down box labeled File.
3. Select the Save As New button and save the new XML file into the created CATIAStandards\drafting directory.
4. Changes to the drafting standards will now be saved to the new XML file which can be used when creating a new drawing.

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Changing the Default Units and Precision

Modify the default unit type for dimensions in:
       Standard\<Standard Name>\Styles\Length/Distance Dimension\Default\Value Display Format\Main Value\Name
       Standard\<Standard Name>\Styles\Radius Dimension\Default\Value Display Format\Main Value\Name
       Standard\<Standard Name>\Styles\Diameter Dimension\Default\Value Display Format\Main Value\Name

Modify the default dimension precision in:
       Standard\<Standard Name>\Styles\Length/Distance Dimension\Default\Value Display Format\Main Value\ Precision
       Standard\<Standard Name>\Styles\Radius Dimension\Default\Value Display Format\Main Value\ Precision
       Standard\<Standard Name>\Styles\Diameter Dimension\Default\Value Display Format\Main Value\Precision

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Creating a new Drawing

When creating a new drawing, the user will be prompted to select the drawing’s Standard. From the drop down selection box, select the newly created drafting standard. This new drawing will assume the settings defined in the previous section.

Administration Notes

       To edit CATIA’s drafting standards in Tools > Standards… the user must have read/write privileges to the directory specified in CATCollectionStandard. This is typically done by the CATIA administrator.

       End user CATIA shortcuts will typically point to an environment directory and CATEnv text document on a shared drive. The CATReferenceSettingPath and CATCollectionStandard variables in the CATEnv document also point to shared network locations (with write protection) so that all CATIA users have access to the same standards.
       Reference the CATIA Help Documentation for detailed descriptions of the modifiable values in Tools > Standards…

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