Lesson 1 -- I-beam

Pro/ENGINEER Functions 

Part            Sketch          View            Dbms            Exit
Protrusion      Dimension       Shade           Extrude

Design Objective

In this lesson you will learn how to extrude a 3D part by using a 2D cross section.

Modeling Strategy

I. Use the PART menu to create the I-shaped solid object.

II. View the part.

III. Save the part.

Detailed Construction

I. Use the PART menu to create the I-shaped solid object shown in Figure II.1-1.

  1. Begin a new part:
    1. Choose Mode from MAIN.
    2. Choose Part from MODE.
    3. Choose Create from ENTERPART.
      Since you currently have no parts saved, you cannot list or retrieve anything. Therefore, the List and Retrieve options are unavailable.
    4. Enter part name [ I-beam ] in the message window and enter.
  2. Create Datum Planes
    1. Choose Feature from PART.
    2. Choose Create from FEAT.
    3. Choose Datum from FEAT CLASS
    4. Choose Plane from DATUM
    5. Choose Default from MENUDTM OPT
  3. Set up the base feature:
    1. Choose Feature from PART.
    2. Choose Create from FEAT.
    3. Choose Solid from FEAT CLASS
    4. Choose Protrusion from SOLID.
      Note that the other features are unavailable. All new parts must begin with a protrusion feature.
    5. Choose Extrude and Solid from SOLID OPTS. (These are already the highlighted defaults)
    6. Choose Done from SOLID OPTS.
    7. Choose Both Sides and Done from Attributes

    You will next choose how the feature you are building will be oriented with respect to any datums present.

    1. Left Mouse Click on the label named DTM2 to pick that plane for sketching (default menu picks for Setup New and Plane and Pick allow you to choose the plane that the crossesection will be sketched in).
    2. Choose Okay from DIRECTION
    3. Choose Bottom from SKET VIEW
    4. Choose Plane from SETUP PLANE
    5. Left Mouse Click on the label for DTM3 to pick that plane for sketching


    The grid and SKETCHER menu are displayed.

  4. Sketch the outline:
    1. Create the I-shaped cross section shown in Figure II.1-2.by clicking with the left mouse button at the start and end of each line segment. Clicking with the center button terminates the line.
      If you make a mistake as you're sketching, choose Delete from the SKETCHER menu and then select the entity you want to erase. The selected entity will disappear; you can now choose the Sketch menu option and resume sketching.
  5. Dimension the section:
    1. Choose Dimension from SKETCHER.
      Use the procedures given below to dimension the section as shown in Figure II.1-2
      To dimension a single entity (such as the length of a line):
      Select the entity with the left mouse button and place its dimension somewhere on the sketch plane with the middle mouse button.
      To dimension between two entities (such as the distance from one line to the Datum Plane you wish it to be parallel to):
      Use the left mouse button to select the first and second entities, and place their dimensions with the middle mouse button. (There is no need to specify dimensions for the right angles. If you drew them to look like right angles, then Pro/ENGINEER assumes that they are right angles. If your sketching was not very exact, Pro/E will not be able to assume right angles, and you should delete those line segments and redraw them)
  6. Regenerate the section:
    1. Choose Regenerate from SKETCHER.
      If you have dimensioned the sketch properly, default numerical values will appear for the dimensions that you specified. Note that the Modify option is already highlighted in the SKETCHER menu. You are expected to change the dimensions.
  7. Modify the section:
    Modify the dimension values to equal those shown in Figure II.1-2. by Selecting a dimension value with the left mouse button, then key in its new value, followed by a RETURN. Repeat this procedure until you have made all of the necessary changes.
  8. Regenerate the final design:
    1. Choose Regenerate from SKETCHER.
      This updates your section based on the the new dimension values.
    2. Choose Done from SKETCHER.
    3. Choose Blind from SPEC FROM
    4. Enter extrusion depth [ 200 ] in the message window.
    5. Choose OK from PROTRUSION: Extrude

II. View the part:

  1. To display a shaded image of the I-shape:
    1. Choose View from MAIN.
      The View option controls all aspects of how objects are displayed.
    2. Choose Cosmetic from MAIN VIEW.
    3. Choose Shade from COSMETIC.
    4. Choose Display from SHADE.
      The shaded image will be displayed in a moment.
  2. To erase the shaded image and bring back the default "wireframe" view:
    1. Choose Repaint from MAIN VIEW.
  3. On your own, change the color of the part

III. Store the part as I-beam:

  1. Choose Dbms from MAIN.
  2. Choose Save from DBMS.
  3. I-beam should be the default, so you can press RETURN. After a moment, a messge stating "I-BEAM has been stored" should appear in the message window at the bottom of the screen.

Lesson 1 is complete.

NOTE: Before you continue on to Lesson 2, select the Quit Window menu option from the MAIN menu, located at the top of the main Pro/ENGINEER working window . Doing this will clear your current working window, save working memory, and will re-open the Mode menu. You can now start creating a new part, such as the Clip Flange discussed in Lesson 2.