About Updating the Standard of a Drawing

This topic explains the concepts that you need to understand before you begin updating the standard of a drawing.

This page discusses:

See Also
Switching a Drawing to Another Standard
Setting Standard Parameters
Setting Styles
Updating the Standard of a Drawing

About the Update of a Standard File

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.

  • 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 most recent changes an administrator or you 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 change, that is styles modified in the updated standard file is not 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. For this, select the element whose style you want to update and select the updated style in the Object Properties panel, under Style.
  • When you update the standard of a drawing from previous release, the name of the views in the specification tree is changed. For example, Front view to FRONT.
    Note: The name in the View properties remains unchanged.

Annotations and Dimensions

During a standard switch or update, annotations and dimensions are automatically updated (to apply the new standard), but not the geometry. To avoid differences between updated annotations and not-updated geometry, it is recommended to update the drawing before any standard switch/update.

Note: The modification of a tolerance format is only applied to documents created after the tolerance format modification.

International Standards

When using international standards, the following dimension values are automatically updated with the new international standards:

  • Dimension's vertical position: When it follows the international standard, that is 0 for ANSI-ASME, 2 for ISO and 0.5 for JIS.
  • Dimension's orientation reference and orientation: When it follows its previous international standard, that is horizontal with screen reference for ANSI-ASME, parallel with dimension line reference for ISO and JIS.
  • Dimension symbols: When the chosen symbols are the international ones, that is Open Arrow for ISO and JIS, Filled Arrow for ANSI-ASME.

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

Styles Organization

Note that after updating the standards, when opening a drawing, the styles are not organized in the Style exactly as they are organized in the Standards editor. However, the order of the styles' types (Sheet, Construction point...) is kept. This minor modification improves the global performance.