Using 3D notes in Pro/ENGINEER can be a powerful tool, especially when you’re dealing with large assemblies with moving parts. For instance, you can use them to control hinge angles, drawer slide travel, or any situation where you have to evaluate moving parts in different positions. Instead of picking through many datum planes to find and highlight the controlling dimensions, you can simply select and modify a 3D note that then updates the dimension via relations.

The following example presents a two-part assembly in which I will show how to set up and use two 3D notes—one controlling the angle, the other the slide length. The parts are assembled such that there is an Orient constraint with an angle to simulate a hinge. Part_2.prt has a dimension controlling the length of a secondary protrusion to simulate a drawer slide.

1. Create two parameters in the top-level assembly. Click Setup and then select Parameters. Choose Create and then Real Number. When prompted, enter a name and an initial value. In this example, hinge_angle and slide_len have initial values of 20 and 0.5, respectively.

2. Set the dimensions to be controlled equal to their respective parameters. Select Relations and select the dimensions to be controlled so that they appear in the main window. Make note of the dimension numbers (e.g., the angular dimension is d1:1). Click Edit Rel and type in the relation that will set the dimensions equal to their respective parameters. In this example, the relation is:

/* Controls angle between Part_1 and Part_2
D1:1 = hinge_angle

/* Controls length of slide
D22:0 = slide_len

where the comments are designated by the /*. When finished editing the relations, save the changes and exit the editor. Select Done from the Relations menu.

3. Create the 3D notes. In assembly mode, choose Setup, Notes, and New. Enter the text that ties the parameter to the note. In this example, the first note is for the hinge angle. Type “Controls the hinge angle” as a general description and hit enter, and then type [&parameter name] (in this case [&hinge_angle], as shown in Fig. 1). The ampersand (&) symbol tells Pro/ENGINEER that this value is a parameter.

Figure 1. Controls the hinge angle.

Click the Place button and place the note (with or without leaders) as you would in drawing mode. Here they are without leaders. Repeat the previous step for the slide_len parameter. After you’ve created both 3D notes, select Done/Return from the Notes menu and then select Done from the Assem Setup menu.

Figure 2. Initial state with 3D notes shown.

Figure 3. Controls the hinge angle.

4. Use the 3D notes. Click Modify from the top-level menu in assembly mode and choose the value on the note. (Make sure you select the number part of the note or it will not let you modify the value.-) You will be prompted to enter a new value for the note. If everything is set up correctly, the model should update according to the new values when you regenerate. These notes can also be toggled between Show and Erase when not in use.

Jason Taylor is a senior design engineer at NCR in Atlanta, Georgia, USA. He can be reached by email at Jason.Taylor@NCR.com.