Creating and Using Custom Drawing Templates in Pro/ENGINEER Wildfire 3.0

Drawing templates automatically create the views, set the desired view display, create snap lines, and show model dimensions. They contain three basic types of information for creating new drawings; basic information, instructions, and parametric notes.

Basic information is anything that makes up a drawing but is not dependent on the drawing model, such as notes, symbols, and so forth. This information is copied from the template into the new drawing.

Instructions are used to configure drawing views and the actions that are performed on that view. The instructions are used to build a new drawing with a new drawing object (model).

Parametric notes are notes that update to new drawing model parameters and dimension values. The notes are re-parsed or updated when the template is instantiated.

You can use drawing templates to:

• Define the layout of views
  
  
• Set view display
  
  
• Place notes
  
  
• Place symbols
  
  
• Define tables
  
  
• Create snap lines
  
  
• Show dimensions

You can also create customized drawing templates for the different types of drawings that you create. For example, you can create a template for a machined part versus a cast part or a sheet metal part. Creating a template allows you to create portions of drawings automatically, using the customizable template

Creating a Drawing Template

• Create a new drawing file from the File > New menu, and name the file
  
  
• Select Use default template and click OK
  
  
• Click Empty or Empty with format
  
  
• If you click Empty with format: Under Format, specify the format you want to use then click OK
  
  
• Pro/ENGINEER creates a new drawing with the specified format
  
  
• If you click Empty: Under Orientation, specify the template orientation by clicking Portrait, Landscape, or Variable. For Portrait or Landscape, choose a standard size under Size. For Variable, specify a size using the Width and Height boxes, and specify a unit by selecting Inches or Millimeters
  
  
• Click Applications > Template to enter drawing template mode
  
  
• Click Insert > Template View and type the view name or accept the default, and then specify the view orientation. Specify view options and view values in the View Options and View Values areas
  
  
• Click Place View and select the location of the General view (Figure 1)
  
  
• To place additional views, click New, type the new view name, and orient the new view. Specify the view options and view values of the new view. When you are done placing all of the desired views, click OK
  
  
• Save the template (Figure 2)

Create a Drawing Using a Drawing Template

• Create a new drawing (File > New. Click Drawing)
  
  
• Clear the Use default template checkbox, and then click OK
  
  
• In the New Drawing dialog select the model from which you want to create the drawing (Figure 3)
  
  
• Specify the template by clicking Use template
  
  
• Type the name of the template you want to use or select a template from the Template list. Click OK. The drawing is created

Note: The views with the correct attributes in both the template and the model are created. If attributes that are defined in the template do not exist in the model, errors occur when the drawing is being created. The Drawing Template Error Info dialog box opens and lists the errors. (Figure 4)

• To access the Drawing Template Error Info dialog box, click Info > Template Errors.

Now that you know how to use Drawing Templates you can incorporate them into your work, and create drawings quickly and easily knowing that all of your essential information will be included as soon as it’s created.