Seven Tricks You Can Use Every Day in Pro/ENGINEER Wildfire 2.0

This tip outlines seven useful functions of Pro/ENGINEER Wildfire 2.0, and how these functions can be best utilized in your design.

Units for parameters

Units can be specified for user-defined parameters during creation and when using parameters in relations. Parameter units are recognized and supported by Pro/INTRALINK and Windchill PDMLink.

Benefits and description:

• You can specify parameters as unit-less or with units during their creation or when using them in relations. Parameters in relations are scaled correctly based on calculations.
  
  Example:
  TOTAL_LENGTH = 1 [in] + 5[mm] would evaluate
  TOTAL_LENGTH = 30.4[mm]
  
  
• Scaling increases flexibility and power when defining custom units. You can mix units when writing relations without having to convert the parameter values before using them. Scalar (unit-less) parameters are still supported and can be used with parameters with units in relations.
• Type must be set to Real Number

User interface location:

• Tools / Parameters (see Figure 1)

Groups

You can create multi-level groups, drag features in and out of groups, and perform operations on individual group members.

Benefits and description:

• You can organize features by creating groups of groups using shortcut menus and drag-and-drop operations. Ungrouping is not necessary when you perform feature operations on individual group members. You can also pattern groups of features or pattern a grouped feature pattern.

Full screen format

Pro/ENGINEER Wildfire 2.0 allows you to maximize your work area and take advantage of the entire screen.

Benefits and description:

• When opening additional windows they may not open full size. To have windows open full size by default, set the config.pro option "open_window_maximized" to "yes".

Composite curves

The ability to create a feature which crosses over multiple tangent boundaries or utilize multiple tangent datum curves as a single trajectory is often needed. In Pro/ENGINEER 2001, this was known as a composite curve.

Benefits and description:

• The workflow to create this feature has changed significantly with Pro/ENGINEER Wildfire 2.0 and is accessible by simply copy and pasting.
  • Click on the first curve once to select the curve feature, and a second time to select the underlying geometry (bold red)
  • Select Edit - Copy and Edit - Paste
  • A new dashboard will open
  • Select the first curve, hold down the Shift key and select any additional tangent curves
  • Select the check mark to finish the feature (Figure 2)

Pause show and erase

Anyone who has made a drawing in Pro/ENGINEER should be familiar with the Show and Erase dialog box. When showing objects in previous versions of Pro/ENGINEER you were required to close out the dialog box before working on the field of the drawing. With Pro/ENGINEER Wildfire 2.0, you have more flexibility with the option to Pause Show and Erase.

Benefits and description:

• You can move and/or cleanup dimensions and then resume adding additional dimensions without ever having to exit out of the Show and Erase dialog box.

User interface location:

• View - Show and Erase
• Select Dimension icon
• Select from options to place dimensions on drawing
• Hold down the right mouse button over the field of the drawing and select Pause Show and Erase
• Hold down right mouse button again and select Resume Show and Erase (Figure 3)

Editing drawing notes

When editing notes in Pro/ENGINEER Wildfire 2.0, you may have noticed that the spacing in the editor and what shows up on the field of the drawing is slightly different. If you are indenting lines you must space over the correct number of spaces (tab does not work). When you edit the editor the changes appear. No preview button exists.

Benefits and description:

• If you want to get a preview of your note changes without exiting the editor, simply click the left mouse button on the field of the drawing and the note will update with current changes. You do not need to exit out of the editor and then repeat the edit command several times to get what you want.

Fill pattern - use of multiple curves

When patterning a feature using the Fill option, you will be prompted to select a curve which defines the region the pattern is to occupy. You may want to select more than one curve or a pattern to fill the region between multiple curves.

Benefits and description:

• One of the options in the Pattern dashboard is to define an Internal Sketch. If you create sketches to define your region, you can then select Internal Sketch and Use Edge combined with the Loop option. In this way you can select multiple closed loops of curves for your pattern definition. The resulting pattern will fill the region between the curves.

User interface location

• Pattern Dashboard
• Set type to Fill
• Select References and under Sketch select Edit
• Sketch the closed boundaries to define areas to include or exclude pattern instances. Alternately you could create the sketches first and then use the Use Edge command to select the boundaries
• Complete the feature (Figures 4, 5 & 6)