Producing Drawings with Generative View Styles

This task deals with the following topics:
   
Generative view styles make it possible to customize the appearance of drawings via a set of parameters defined in an XML file, DefaultGenerativeStyle.xml. Some generative view style parameters are specifically available to produce customized drawings from parts designed in the Generative Sheetmetal Design workbench. It is the administrator's job to provide suitable styles.
   
For additional information on how to customize parameters, or more generally on generative view styles, see the Generative Drafting User's Guide. The Administration Tasks chapter deals with the administration of generative view styles. The Basic Tasks > Generative View Styles chapter explains how to use generative view styles. The SheetMetal Parameters task explains how to customize generative view styles for Generative SheetMetal Design.
   
Open the SheetMetalDrafting1.CATPart document.
Make sure you have an appropriate Generative Drafting license.

Specify your settings before you start: select Tools  -> Options  -> Mechanical Design -> Drafting -> Administration tab, and uncheck Prevent generative view style usage. This activates generative view style functionalities.
 

Producing a drawing with the default generative view styles file

  1. Select Start -> Mechanical Design -> Drafting.

    The New Drawing Creation dialog box appears. The empty sheet layout is pre-selected.
     

     

  2. Simply click OK. You switch to the Drafting workbench and an empty drafting sheet is created.

  3. For ease of use, tile the windows horizontally using the Window -> Tile Horizontally menu item.

  4. Click Unfolded View in the Projections toolbar from the Generative Drafting workbench. The Generative View Style toolbar is automatically displayed.
     

  5. Select one of the available styles from the list, DefaultGenerativeStyle in this case.

  6. Return to the 3D document and select a plane surface on the sheet metal part. The sheet metal reference wall plane is used automatically. 
     

    A preview of the view is displayed in the drawing.

  7. Click in the drawing to validate the view creation. The unfolded view is created, using the sheet metal-specific styles defined by the chosen generative view style. Here, the BTLs (Bend Tangent Lines) and the stamps are projected in the view, as specified in the DefaultGenerativeStyle.xml file.
     

    Note that the axis of upward and downward bends are represented in a different color, as well as upward and downward stamps.

    Annotations containing the bend's direction, radius and angle value, as well as the standard name of the stamp, if any, can also be displayed on the drawing, provided your administrator has activated the corresponding parameters contained in the DefaultGenerativeStyle.xml file.

    The bend axis and bend annotations are displayed according to the orientation of the part.
 

Producing a drawing with a customized generative view styles file
Save the DefaultGenerativeStyle_customized.xml file and place it in install_root/resources/standard/generativeparameters.

  1. Select Start -> Mechanical Design -> Drafting to open an empty drafting sheet.

  2. Click OK and tile the windows horizontally using the Window -> Tile Horizontally menu item.

  3. Click Unfolded View in the Projections toolbar from the Generative Drafting workbench.

  4. Select the DefaultGenerativeStyle_customized style in the Generative View Style toolbar that is automatically displayed .

  5. Return to the 3D document and select the surface on the sheet metal part.
     

  6. Click in the drawing to validate the view creation.
    The unfolded view is created with annotations specifying the parameters of bends and stamps. These parameters depend on the orientation of the part.

     


     

    Note that:
    • the hem is not represented in the drawing because non-canonical flanges are not represented since they do not generate planar and cylindrical faces only,
    • annotations are displayed only for surface stamps and not for the user stamp because the Standard name field available in the Surface stamp dialog box has been populated.
      Since this field is not available in the User Stamp dialog box, you should use the Formulas dialog box instead:
    1. Select the User Stamp.1 in the specification tree.
    2. Click Formula in the Knowledge toolbar.
    3. In the Formulas dialog box, select the Standard name parameter.
    4. Enter a value for the Standard name.
       
    5. Click OK to validate.
    6. Return to the drawing document and update Drawing1.
      The User stamp's annotation is displayed.

     
    Annotations can be freely positioned on the drawing. You can also modify them if needed. Yet, each time you update the drawing, they come back to their original place.

    For more information on annotations, refer to Creating a Text With a Leader in the Generative Drafting User's Guide.