Updating the Standard of a Drawing

When a standard file is modified, there is no automatic update of the drawings which use this standard. Each drawing contains a copy of the standard it uses, and retains this version until you explicitly update this copy or switch the drawing to another standard. 
In this task, you will learn how to update the standard used by a drawing.
Open any existing CATDrawing file.

  1. Select File > Page Setup from the menu bar. The Page Setup dialog box opens, displaying the standard currently used by the drawing.

  2. Click the Update button to update the current standard. 
     

  3. Click OK to close the dialog box.
 

About the Update of a Standard File
 
  • The most recent version of the updated standard is copied into the drawing and the previous standard parameter values are replaced by the latest ones, reflecting the latest changes an administrator or user may have performed in the standard file. This may have an immediate impact on the appearance of the elements inside the drawing.  
  • Styles are not affected by this update, i.e. styles modified in the updated standard file will not be re-applied to existing elements. Indeed, styles are applied when creating elements (as they define the default values to be used for creation). If needed, new style parameters can be re-applied to an element using the Style toolbar: simply select the element whose style you want to update and select the updated style in the Style toolbar.
 
Since there is no automatic update of drawings when a standard file is modified, you need to update the standard of drawings created before V5 R9 if you want them to benefit from the new parameters.
   
 

International standards
 
When they follow international standards, some dimension values are automatically updated with the new international standards:
  • Dimension's vertical position:
    When it follows the international standard, i.e. 0 for ANSI, 0.5 for ISO and 2 for JIS.  
  • Dimension's orientation reference and orientation:
    When it follows its previous international standard, i.e. horizontal with screen reference for ANSI and ASME, parallel with dimension line reference for ISO and JIS.  
  • Dimension symbols:
    When the chosen symbols are the international ones, i.e. Open Arrow for ISO and JIS, Filled Arrow for ANSI and ASME.

Furthermore, if the target international standard is ANSI or ASME, radius type dimension has its dimension line representation set to 2 parts.