About Drafting Standards
When users modify the properties of an element in the Interactive Drafting workbench, the modifications are only applied to the selected element, in the current drawing. Standard files let administrators set the properties of an element so that they will be applied to all elements of the same type in a drawing, as well as in all drawings which use a given standard.
A standard file is an XML file which makes it possible to customize globally, for a CATDrawing, the appearance and behavior of drafting elements.
With standard files, administrators can:
- set standard styles that will be used as default
values when creating new elements, i.e.:
- define sheet styles
- define geometry styles
- define annotation styles
- define dimension styles
- define dress-up and dress-up symbols styles
- define callout styles
- set standard parameters, i.e.:
- control the user interface, with general parameters to restrict the values of some element properties
- customize dimensions
- customize annotations
- customize dress-up elements
- define new dimension tolerance formats
- define new dimension value formats
- control pre-defined formats for tolerance and dimension values
- control view generation parameters
- customize fixed-size frames
- customize line thickness
- customize patterns
Once defined, a format is applied to elements as a property.
Management of Drafting Standards
Standalone drawings
When users create a CATDrawing document (File > New), they specify the standard that will be associated with this document. The values of the parameters in the specified standard file are then copied into the CATDrawing document. Each drawing contains a copy of the standard and is therefore standalone. This makes it possible for users, projects, or companies to exchange CATDrawing documents without needing to send the standard file along.
Administrator-controlled access and modification
The administrator defines and controls the location of the standard files as well as the ability to define new standards, or to modify existing standards. For example, the administrator can define a single standard, and prevent users from modifying it.
Seven standard files available by default
By default, seven standard files are provided: four for each of the international standards available when creating a new CATDrawing file, and three for use with other workbenches. These files are located in install_root/resources/standard/drafting.
Some are specifically intended for Drafting:
ISO.xml
ANSI.xml
JIS.xml
ASME.xml
Some are specifically intended for the 2D Layout for 3D Design and Functional Tolerancing and Annotation workbenches. They are based on the Drafting standards and are suffixed with _3D. In these specific standards, the colors, for example, have been customized for optimized display.
ASME_3D.xml
ISO_3D.xml
JIS_3D.xml
Administrators can add as many standard files as needed. Refer to Administering Standards for more information.
Editing the standard file
The standard files can be edited using an interactive editor. This editor provides an easy-to-use graphic interface to let administrators customize the parameters included in the standard files. For information on how to customize these parameters, refer to Setting Standard Parameters.
The interactive editor is available in Tools > Standards. (It is the same editor with which you can customize generative view styles). For more information on how to use this editor, refer to the Customizing Standards chapter in the Infrastructure User's Guide.
Switching to another standard
When several standards are defined, users can switch a drawing to another standard. Refer to Switching to Another Standard.
Updating the standard of a drawing
When a standard file is modified, users need to explicitly update the drawings which use this standard. Note that only standard parameters are affected by this update, not styles. Refer to Updating the Standard of a Drawing.