TUTORIAL: Dimension Pattern in Pro/ENGINEER Wildfire (Angular Dimension)

Version: Pro/E Wildfire, Wildfire 2.0, Wildfire 3.0, Wildfire 4.0

This tutorial shows you the steps how to create a circular pattern using the dimension type pattern (angular) in Pro/ENGINEER Wildfire. Download the ProE part file used in the following dimension pattern tutorial here (ProE file: dimension pattern angular start.prt ).

1. Open the downloaded tutorial start file (dimension_pattern_angular_start.prt ). The ProE model should look like below.

2. Select the hole feature which to be patterned. After that, press and hold RMB to access the context sensitive menu. Choose the Pattern command from the list.

3. Pattern dashboard will appear to you at the message area. Dimension type pattern is the default for pattern dashboard.

The dimensions of the hole feature will be displayed for you to select it as the 1st direction.

4. Select the angle dimension as shown in the image below (red) for the 1st direction. Input 45 degree and ENTER for the increment value for the 1st direction in the pattern. After that, Change the quantity to 8 instances.

The pattern instances will be represented as black dots for the preview purposes.

5. Next, we need to activate the 2nd direction definition for Pro/E Wildfire pattern feature. Click the cell in the pattern dashboard as show in the image below.

6. Repeat step 4 to define the 2nd direction for the pattern feature. (see image below)

This time, we are controlling the PCD of the holes. Input 60 as the increment value and 4 in quantity. The Pro/E model should look like below at the end of step 6.

7. We are done with the tutorial, click the check mark   button on the pattern dashboard to confirm the dimension pattern feature. A regeneration bar (WF2 and above) will appear to indicate the progress of the calculation.

The image below shows you the final model for the dimension pattern (linear) in Pro/E Wildfire.