Ron Graham
With Brian Celeste, Dan Drury, Jason Hartman, and Wayne Poole

Introduction

Pro/Engineer is among the most powerful (and therefore among the most popular) computer-aided design (CAD) programs available today. Pro/E offers the user many functions and user-friendly operation, and is constantly being improved in both areas. It’s no surprise that Pro/E is now being used worldwide and is at the forefront of CAD software. More to the point, basic skills in Pro/E are highly sought on the job market, both in engineers and in designers.

The purpose of this micro-course is to give a new user of Pro/E familiarity with its most common functions, and to enable these users to continue to develop their skills on their own, without continuous training. We assume here that the new user is an engineer, or otherwise has some interest in mechanical design, but has no experience in any other CAD software.

The following are the basic skills with which we feel the user should become familiar:

• Datums and coordinate systems
• Extrusions via protrusion and revolution
• Alignment and dimensioning
• Repetition of common features
• Holes and slots
• Rounds and fillets
• Cuts
• Assembly

It’s impossible to gain exhaustive knowledge of these subjects in a single day, but it is possible in a single day to create an assembly (consisting of basic parts) using techniques in all these areas. That first assembly will give the new user enough confidence to continue forward.

Some Notes About Pro/E

Pro/E is a product of Parametric Technologies Corporation, whose Web site has this to say about their software:

Pro/ENGINEER is the de facto standard for mechanical design automation – based on a parametric, feature-based, fully associative architecture – that delivers a comprehensive suite of solutions for all areas of the development process, from a product’s conceptual design and simulation through manufacturing.

The new user should take a few moments to be clear on the terminology used here:

• Feature-based – you design a part using features (e.g., extrusions, holes, slots, rounds, etc.) instead of the part’s geometric characteristics (i.e., individual arcs and lines).
• Parametric – the shape of the created part is based on the dimensions of its features (or, parameters), and those dimensions can be related to (or, associated with) one another (e.g. edges can be parallel to or normal to one another; lengths or angles can be equal to one another).
• Fully associative -- if a given parameter is changed on a certain feature, any associated dimension(s) are automatically changed accordingly.

We make the following assumptions:

• Creation of a part, and of some simple features on that part, are the most fundamental actions not only within Pro/E, but in CAD in general.
• No actual instructions are included here – instructions can be found in other works – but readers are assumed to have basic ("point and click") computer competence. Actions that can be found on Pro/E menus are given in italics.

Creation of a Part

Of all Pro/E’s modes, part creation is the most fundamental. You can create a part by sketching an outline of the part’s cross-section on a datum plane, aligning the outline with respect to the coordinate system, and creating a solid protrusion from the outline. Protrusions are often created by extrusion, though it’s also convenient at times to create a solid of revolution (or, shaft) about a coordinate system axis. The steps involved are as follows:

1. Datum. A datum is a reference plane, used to define where in space the part is to be created. The space is completely defined by three orthogonal datums: users select two, and Pro/E generates the third. One datum is then selected as a sketch plane, on which the outline is drawn.
2. Coordinate system. The intersection of the three datums is the origin of the part’s coordinate system; coordinate axes are formed by the intersections of each datum pair. Users select axes convenient to the creation of their part for alignment of some of the part’s features. Your view is normal to the sketch plane (unless you want to sketch in 3-D – not recommended for the beginner). Protrusions are created normal to the sketch plane, toward you.
3. Sketch. Pro/E’s Sketcher feature allows you to be casual in defining the geometry of a part: it assumes anything "close" to horizontal actually is horizontal, and so on. On the other hand, the Sketcher won’t allow you to create a part from the sketch until it’s completed; and the sketch isn’t complete unless you provide exactly enough information to dimension the sketch.

The general steps in sketching are as follows:

• Mouse sketch (or, click and drag) for lines as needed, as with any graphics program.
• Add arcs and fillets as needed for rounded edges and corners.
• Align features of the sketch with features of the coordinate system (e.g. an edge with an axis, etc.) Again, the features need only be "close."
• Dimension the sketch by choosing a feature and a location on the sketch plane to locate the dimension. Pro/E assigns that dimension a name; you may replace the name with a number later.
• Regenerate the sketch. Pro/E "cleans up" the drawing (by completing alignment), and determines whether dimensioning is correct. If it isn’t, Pro/E indicates any undefined or improperly aligned features (allowing you to make appropriate changes), or any redundant dimensions (allowing you to delete them).
• Modify dimensions – assign a number for each name.
• Regenerate the sketch again. At this point the sketch is reproduced to scale. When you see the message "section regenerated successfully," you will be very, very happy. :-) Sketches will at times not regenerate successfully, for the following reasons:
  • A feature isn’t "close enough" to align properly.
  • Over- or under-dimensioning.
  • A segment is forced to a very small (or zero) length when you modify dimensions.
  • The sketch isn’t closed properly (disconnected or crossing lines).

The Pro/E Sketcher has the following internal rules for dealing with features that are "close":

• Equivalence of radius/diameter of similar circles
• Symmetry with respect to a centerline
• Horizontal and vertical lines
• Parallel and perpendicular lines
• Tangency with respect to curves
• Equivalence of length of similar segments
• Proximity of points to other features (the points actually lie ON the features)
• Equivalence of individual coordinates (e.g. two points with similar X-coordinates, etc.)

4. Protrusion. Select an extrusion depth (if extruding the protrusion) or an angle of rotation (if rotating a shaft) or a sweep characteristic (for a sweep or blend, in which the profile changes from beginning to end of protrusion). If the extrusion is successful, you’ll see the message "all elements have been defined.
5. Preview. Preview the resulting 3-D object. If it’s OK, accept it and save it. Otherwise modify dimensions and regenerate.

Addition of a Feature

Often, users want to add a feature to parts they’ve created. Typical features include holes, cuts, and slots. To add a hole:

• Select a surface on the part.
• Sketch a profile of the hole (it doesn’t have to be a round cross-section).
• Pro/E treats a typical hole (drilled into a part) exactly as an extrusion, except the hole is extruded into the part (into the screen) and away from you.
• Select a hole depth.
• Align the hole, either with an edge or its axis, to the part.
• Dimension the hole.
• Regenerate.

To add a cut or a slot:

• Select a surface on the part.
• Sketch a profile of the cut/slot cross-section. Unlike a hole, this cross-section doesn’t have to be a closed shape.
• As with holes, Pro/E treats cuts and slots as reverse extrusions.
• Select a depth.
• Align the cut/slot, by some convenient feature, to the part.
• Dimension the slot.
• Regenerate.

As with the original shape, anything that doesn’t regenerate properly can be modified. And once these features are completed, you may add fillets or chamfers to the resulting part in 3-D as you would fillet or radius an original 2-D sketch.

Patterned features: a single hole can be replicated in a pattern by defining the pattern characteristic (e.g. angular increment of radial placement).

Copied features: a protrusion (for instance) can be copied to another location on the part by defining the surface on which the copy is to be moved, and the distance (for translation) or angle (for rotation) of the move from the original. The copy may then have its dimensions changed if you desire.

Combining Parts into an Assembly

Assembly is another mode within Pro/E. Within Assembly, all constraints on individual parts are defined:

• Mate surfaces
• Align axes
• Insert solids into holes/cuts/slots
• Orient inserted solids to position individual features (e.g. a keyway on a shaft)

As in part creation, an assembly is ready for your review and acceptance when regeneration is completed successfully.

References

Toogood, R. Pro/E Tutorial Release 18/19. Edmonton, Alberta: ProCAD Engineering, Ltd. 1998.

Parametric Technologies Web site, http://www.ptc.com/products/proe/.