Engineering CAD

Engineering CAD is a two-person modeling event. Your team gets paper drawings and a starter Onshape file that already holds some of the parts you need. You model the named parts from the drawings, combine them with the supplied components into an assembly, and get scored on how close each named part's volume, and your assembly's center of mass, come to the correct values for the drawings. The event tests three things at once: reading a drawing correctly, building geometry that stays editable, and working fast enough that modeling time decides ties. Strong teams spend more of their early minutes reading drawings than clicking, and they check volumes, materials and units before they submit rather than after.

Engineering CAD is a Division C event only. Everything below follows the 2027 rules manual, where the whole event fits on one page (printed page C32).

Event format

Because no personal notes are allowed, everything you need during the event has to live in your head or on the drawings. That changes how you prepare: you memorize the handful of formulas and unit conversions that matter, and you practice reading a drawing until its conventions feel automatic.

What the rules cover

The 2027 manual has four numbered sections on a single page. Section 1 is the overview: the team reads a set of drawings, builds the parts together in Onshape, and joins those parts with supplied components into an assembly. Section 2 sets the parameters: the software, the hardware, the ban on outside resources, the starting document, and a new step in which the team hands over two Onshape account emails before the event. Section 3 describes the competition, including how many parts a team models at each level. Section 4 defines the two scores and the tiebreaker. Division C is the only division that runs this event, and there are no rotating topics or themes: the skill tested is the same every season.

Three changes from last season matter for preparation. First, the part score now compares each part's volume with the correct value, where it used to compare mass. Volume depends only on geometry and units, so the part score no longer rewards or punishes a material choice. Materials still matter, because the assembly score uses the center of mass, and the center of mass depends on how mass is shared among the parts. Second, the part counts went up at both levels. Third, the team must send the supervisor two Onshape account emails before the event, and the test materials arrive through those accounts.

The drawings are the only reference for the numbers you enter. The rules say the drawings specify the geometry, the materials and the units for each part, so a material or a dimension should always come from the packet, never from memory.

Reading engineering drawings

A drawing is a set of two-dimensional views that together describe one three-dimensional object. Each view shows some edges and hides others. A front view shows the outline of the object as seen from the front; a top view shows the same object from above. Neither view alone is enough. You build the 3D shape in your head by reading the views together, then you check your picture against the dimensions.

Three conventions do most of the work:

• Solid lines show visible edges. Dashed lines show hidden edges behind a surface. A through-hole appears as a circle in the view looking along its axis, and as a pair of parallel dashed lines (with a center line) in the adjacent views. If the dashed lines run the full thickness, the hole goes through; if they stop short, it is a blind hole, so read its depth.
• Center lines show axes of symmetry and the centers of holes and arcs. A hole is located by the intersection of two center lines, and a revolved part is described by a single center line about which its profile turns.
• Section views cut through the object and show the inside. A cut face is shaded with hatch lines. A section is the fastest way to find a bore, a pocket or a wall thickness that the outside views cannot show.

Read the title block before you read the views. It gives the units, the material, the scale and the drawing's name. Units are the single most common source of lost points in this kind of event, so write the unit system on your scratch paper at the start. If the title block says one unit and a dimension has a different unit or no unit at all, treat that as a question for the Event Supervisor before you model the part, not as a detail to guess at.

Then work through the drawing in a fixed order: list the named parts you must model, sketch a rough plan for each one (the base feature, the cuts, the holes and the finishing features), and list the dimensions that define each feature. Circle any dimension that controls a part's volume or where a part sits in the assembly, since those are the values that score. A drawing often gives a dimension once and expects you to infer the rest, such as a symmetric part whose dimension is given on one side only. Look for symmetry before you start dimensioning anything.

Sketching and constraints in Onshape

Most of your modeling starts with a sketch: a two-dimensional profile drawn on a plane, which a feature such as an extrude or a revolve then turns into a solid. A sketch is well behaved when it is fully constrained, meaning every point in it has a position fixed by dimensions or geometric relations. The number that matters is the degree of freedom count. A free point in a plane has two degrees of freedom, one for each coordinate. A line segment with free endpoints has four, because it has two endpoints. Each dimension or relation removes one degree of freedom, and a coincident relation between two points removes two at once.

The mechanism matters because of what happens when you change a number later. If every point is locked, changing one dimension moves exactly the geometry it controls. If a point is free, the solver chooses where it goes, and a later edit can move it somewhere you did not intend. The result is a model that looks right until a second dimension changes and a hole wanders off center.

Onshape shows the constraint state of a sketch with color: geometry that is still free to move is drawn in blue, and geometry that is fully defined turns black. Glance at the color before you leave a sketch, and add dimensions or relations to anything still blue. (Interface details change between releases, so confirm the colors on your own account.)

Choose dimensions the way the drawing does. If the drawing locates a hole from a center line, place the sketch dimension from that same center line. Dimensions that chain from one feature to the next accumulate small errors and make edits fragile, while dimensions referenced to a shared datum stay put. The printed drawing is your guide to the reference, so copy its logic instead of inventing your own.

Building parts from features

A feature is a sketch turned into geometry. The features you will use most are the extrude (a profile pushed along a direction to make a prism), the revolve (a profile turned about an axis, for turned parts), the cut (a profile or hole removed from the solid), the fillet and chamfer (rounded or beveled edges), and the pattern and mirror (copies of a feature placed by a rule). Sweeps and lofts exist for transitions, but they take longer to set up, so spend most of your practice time on the first five.

The order matters. Build the base feature first, because every later feature references it. Put cuts and holes next, and add fillets and chamfers late, because a fillet changes the edges that other features reference. A fillet placed early can break a later feature when a reference edge no longer exists, and the rebuild fails with an error that is hard to trace quickly under time pressure.

Patterns and mirrors encode repetition. A circular pattern of eight holes spaced evenly around a circle has an angle of 360 ÷ 8 = 45° between neighboring holes. Patterns should reference a real axis or a datum, not a face that may move. If you pattern a hole about a face and that face later moves, the whole pattern shifts with it. A mirror across a plane of symmetry is only correct if the part really is symmetric about that plane. Check the drawing before you mirror, because an asymmetric detail such as a keyway or an offset boss will be copied to the wrong side.

Revolves suit turned parts such as shafts, bushings and bosses with stepped diameters. Sketch half the profile on one side of the center line, with the center line as the axis, and revolve it through 360°. The result is a body of revolution with one sketch instead of several cylinders stacked by hand. A revolved part is easy to dimension incorrectly if you place a diameter where the drawing gives a radius, so check that the value on the sketch is the one the drawing lists.

Two worked micro-examples show the reasoning. A plate with eight equally spaced holes on a bolt circle is built by sketching one hole located from the plate's center, cutting it, and then circularly patterning it about the plate's center axis by eight instances. A stepped shaft is built by sketching its half-profile with each step's radius and length, then revolving it. In both cases the features reference the drawing's own reference geometry, so changing the overall size later moves everything consistently.

Sketch relations and extrude options worth knowing

Besides dimensions, a sketch is fixed by relations. The ones you will use constantly are coincident (a point on a point, line or origin), horizontal and vertical, parallel and perpendicular, equal (two lengths or radii forced to match), concentric (shared circle centers), tangent, midpoint, and symmetric (two points mirrored about a line). Using one equal or symmetric relation instead of two dimensions is faster and keeps the part consistent when a size changes.

When you extrude, the choices that matter are the end condition and the operation. A blind extrude runs a set distance; a symmetric extrude runs half that distance each way from the sketch plane (handy for a plate centered on the origin); "up to face" and "through all" tie the depth to existing geometry. The operation is New (a separate part), Add (merge into an existing part), Remove (cut), or Intersect. Choosing New by accident is a classic way to end up with two bodies where the drawing has one, which splits the volume across two parts and leaves the named part too small.

Working in Onshape

An Onshape document holds tabs. A Part Studio is where you sketch and build parts; one studio can hold several parts. An Assembly tab is where part instances are placed and mated. The starter document already contains an assembly with the supplied components, so your parts must end up as instances in that assembly, not as loose parts in a studio.

Four habits protect your score. First, set the document units to match the drawing's title block before you sketch, because the part score is a volume and a unit slip multiplies volume by the cube of the conversion factor. Second, name each part exactly as the drawing names it, since the scores are tied to named parts and a supervisor checking an unnamed "Part 3" may not find it. Third, assign each part the material the drawing names. Volume does not depend on material, but mass does, and the assembly's center of mass is a mass-weighted average, so a wrong material on one part pulls the assembly's center toward or away from that part. Fourth, use the Mass properties tool (in the Part Studio and in the Assembly) to read volume, mass and center of mass, and compare each readout with a quick hand estimate. A feature that is defined with a variable or a named dimension (for example a shared hole diameter) lets you correct one number and have every dependent feature follow.

Assemblies and mates

An assembly places part instances in relation to each other. The usual first step is to fix a base component so it cannot move, then bring the other components in and locate each with a mate. A mate relates two parts through their faces, edges or axes. A mate attaches a connector (a coordinate frame placed on a face, edge or hole) on one part to a connector on another, so the connector you pick decides where the part lands. In Onshape the common mate types are Fastened (no motion, the default choice for a rigid joint), Revolute (rotation about one axis), Slider (translation along one axis), Cylindrical (rotation and sliding along one axis), Planar, Parallel, Pin slot and Ball. The scoring only cares where components end up, so a Fastened mate is usually the right choice unless the drawing shows a different relationship.

Use the fewest mates that fix each component. A part with unconstrained freedom can drift when you move another component, and a part that is mated redundantly can conflict with its neighbors, which makes the assembly solve badly. Keep the mate list short, and check that each mate matches what the drawing shows. For a mate that matches a feature on a drawing, use the same face or axis the drawing uses.

Assembly positioning has a direct effect on the score. The center of mass of an assembly depends on where each component sits, so a correctly modeled part placed a few millimeters away from its drawn location shifts the assembly's center of mass and costs points on the affected axis. Do not treat the assembly step as a formality. After you mate the components, check the assembly against the drawing's locations, and compare the reported center of mass with a rough hand estimate before you submit.

Volume, mass and center of mass

The two numbers that score in this event come from mass properties: the volume of each named part, and the center of mass of the assembly. Onshape computes both for you, but you need to estimate them by hand to catch a modeling error before you submit.

Volume: what the part score measures

Volume is the space a solid occupies. It depends only on the geometry and the length unit, so two parts with identical shape have identical volume whether one is aluminum and the other is ABS plastic. That is why the 2027 part score is a pure geometry check: if every feature is the right size and in the right place, the volume is right.

Most parts in this event are built from simple solids added together and cut away from each other, so the volume of a part is the sum of the volumes of the material you added minus the volumes you removed. The shapes you need are few:

The extrusion rule is the one you use most: any shape extruded straight has a volume equal to its sketch area times its depth, however complex the outline. A plate with a rounded slot is the plate's area minus the slot's area, times the thickness.

Units are the place where volume goes wrong most dramatically. Because volume is a length cubed, a length conversion factor gets cubed too: 1 in = 25.4 mm, so 1 in³ = 25.4³ = 16,387.064 mm³, and 1 cm³ = 1,000 mm³. A part drawn in inches but modeled in millimeters is not 25 times too small; it is about 16,000 times too small, and the part score drops to zero.

Mass

Mass is the amount of matter in an object. It does not score directly in 2027, but it decides where the assembly's center of mass falls. For a solid of uniform material, mass is density times volume:

The center of mass (CoM) of a set of bodies is the mass-weighted average of their positions. Every body pulls the combined center toward itself in proportion to its mass, so a heavy body near the origin drags the center toward the origin even when a lighter body sits far away. The CoM is a point, and it has an X, a Y and a Z coordinate, one for each axis of the coordinate system the drawing or starting document defines.

A feature that removes material reduces the mass, and it moves the CoM toward the material that remains. Work through a hole the same way: subtract the hole volume from the block volume and recompute the mass.

Now the center of mass. Suppose a second, smaller body of 12.0 g sits with its own CoM at x = 40 mm, and the 27.0 g block has its CoM at x = 0. Using the formula along the X axis:

Units are the place where this calculation most often fails. The formula works in any consistent length unit, but a mixture of millimeters and centimeters, or a mass in pounds with a density in grams, yields a number that looks plausible and is wrong. One pound is exactly 453.59237 g, and one inch is exactly 25.4 mm, so a conversion error of either kind is easy to make and hard to notice. Decide the unit system from the title block and convert once, at the start, rather than mid-calculation.

How the score works

The 2027 rules define the event score as the sum of the Individual Part Scores (IPS) and the Individual Assembly Score (IAS). High score wins. Both scores measure relative error against the correct value, so what matters is how far off you are as a fraction of the target, not in millimeters.

Part score: volume

Each named part is scored on its volume. The relative error is your volume minus the correct volume, divided by the correct volume, and the part earns 100 points minus 100 times the size of that error. A perfect volume earns 100, and the score cannot drop below 0.

The falloff is linear: every 1% of volume error costs 1 point, whether you are too big or too small. Because each part is scored on its own, a team modeling six parts at Regionals can earn up to 600 part points, and a team modeling eight at State can earn up to 800. Those part points outweigh the single assembly score, so a clean, correct set of parts is the foundation of a good result.

The lesson is that small detail errors cost a few points each, while unit errors and doubled or halved sizes wipe out a part. Check units and diameters first.

Assembly score: center of mass

The assembly is scored on the X, Y and Z components of its center of mass. For each axis, the relative error is the difference between your component and the correct component, divided by the correct component. Each axis's relative error is divided by 3 before it is subtracted, so a 3% error on one axis costs 1 point, and a 100% error on one axis costs a third of the 100 points.

That last point is the key property of a relative-error score. A component whose correct value is small is very sensitive: if the correct Z were 0.5 mm and your assembly gave 1.5 mm, Δz would be 2.0 and that axis alone would cost 66.7 points. A sign flip (−10 mm instead of +10 mm) gives a relative error of 2.0 for the same reason. This is why mating components to the drawn references and keeping the provided origin untouched matter so much.

Material choice feeds into the assembly score even though it does not affect the part score. Suppose two parts of 10.0 cm³ each sit with their own centers at x = 0 and x = 40 mm. If both are the same material, the assembly's center is at x = 20.0 mm whatever that material is, because the density cancels. If the drawing makes the first part aluminum (2.70 g/cm³) and the second steel (about 7.85 g/cm³), the masses are 27.0 g and 78.5 g and the center moves to 78.5 × 40 ÷ 105.5 = 29.8 mm. A team that leaves both parts as aluminum reports 20.0 mm, a relative error of 0.33 on X, and loses about 11 points on that axis alone.

Tiebreaker and submission

If two teams tie on the event score, the team with the lower modeling time wins. The clock runs from the moment the team presses "Start assignment" to the moment it presses "Submit." Work done after the last submission is not graded, so the model as it stands at your final submission is the one that counts.

Units, signs and conventions

Pick one length unit before you model anything, and write it down. Drawings in this event give lengths in millimeters or inches, and different parts in one packet may use different units, so read the units on every sheet. The conversions you need are 1 inch = 25.4 mm (exact), 1 in³ = 16,387.064 mm³ (exact, since it is 25.4 cubed), 1 cm³ = 1,000 mm³ (exact), and, for hand checks of mass, 1 lb = 453.59237 g (exact by definition). Convert a dimension once, check the result against the drawing's overall size, and then never mix units inside a single formula.

Signs matter for the center of mass. A coordinate on the negative side of an axis is negative, so a body placed on the negative X side pulls the X component of the combined CoM toward negative values. The origin of the coordinate system is set by the starting document or the drawing. If you compute a CoM relative to a different origin than the one the assembly uses, every component is offset and the score falls even if each body is correct. Confirm where the origin is before you compute.

Keep significant figures reasonable and consistent with the drawing's precision. Carrying five digits in an intermediate step and rounding at the end is safe. Rounding each intermediate value to two digits can shift a final answer by enough to matter when the score depends on closeness.

Common pitfalls

Strategy

Split the work by independence. Two students and two computers make parallel modeling possible, but only if the parts do not depend on each other. Decide the split in the first minute. A common pattern is one partner models the parts that have no dependencies while the other reads the next drawing and prepares the dimensions for the parts that come next. Assign each part a single owner, so two students never model the same feature in two places. Competing copies of one part produce a model that is hard to trust and slow to fix.

Plan before you click. Spend the first few minutes reading the title block, the drawings and the named-part list, and sketch a short plan for each part: base feature, cuts, holes, finishing features. Circle the dimensions that control volume and placement. A plan takes two minutes and saves many minutes of rebuilding.

Check volume as you go. After each part, compare Onshape's volume with a rough hand estimate (the bounding box minus the big cuts is usually enough to catch a factor-of-two error). A mismatch found after the assembly is built is far more expensive than one found on the part. If a volume is off, look first at units, then at a diameter-radius mix-up, then at a missing feature, since those are the most common causes.

Plan for up to eight parts. At State and Nationals you may model as many as eight parts in about 50 minutes, which is roughly five minutes per part once planning and assembly are counted. Split the parts by owner at the start, put the parts the assembly depends on (the ones other parts mate to) first, and leave decorative fillets and chamfers for last, but do not skip them, since each one changes the volume a little.

Keep the order of features clean. Build the base, then cuts and holes, then fillets and chamfers. Put the fillets last so that no later feature loses a reference.

Manage the clock. Modeling time is the tiebreaker, so do not hold back a submission waiting for perfection. Submit at a checkpoint when the parts are in, then correct errors and resubmit. Since work after the last submission does not count, submitting regularly also protects your final state.

Prepare without notes. Since no resource material is allowed, practice the things you will need from memory: the volume, mass and CoM formulas, both scoring formulas, the conversions in the units section, and the habit of checking units first. Keep the physics practice short and focused on these formulas, since a formula you have to look up costs time you do not have.

Practice with your own drawings. Draw a simple part with dimensions, model it in Onshape, and compare the software's volume and center-of-mass readout with your hand calculation. Repeat with a hole, a pattern and a two-part assembly. Time yourself to about 50 minutes to match the event's time limit.

How tournaments test this

The event is a modeling assignment, so the scored result is the Onshape model rather than a written answer. Supervisors build a packet of drawings, a starting document with some components already in an assembly, and a key with the correct volume of each named part and the correct center of mass of the assembly. At Regionals expect 3 to 6 parts; at State and Nationals expect 4 to 8.

The question archive holds 12 Engineering CAD items, all from two 2026 Division C Northview listings (six each), all with numeric answers. They come from last season, when the part score used mass rather than volume. The most frequent terms are:

Read these numbers as a direction, not a profile. Twelve items is a small sample, and they ask for masses because last season scored mass. Under the 2027 rules, the per-part answer is a volume, so treat the mass items as practice for the assembly's center of mass rather than for the part score. Half of the items use pounds, so be ready for imperial units as well as metric ones.

None of the 12 has a verified answer key, so the self-test below is written for this guide rather than linked to archived tests. The best practice is still a full mock: a printed drawing packet, a starting document, a 50-minute timer, and a key you compute yourself.

Test yourself

The questions below are original practice written for this guide. Each one is solved in the answer key, and each uses only the formulas and conversions taught above. Work them without notes, then check your answers.

1. A rectangular block measures 50 mm × 20 mm × 10 mm and has a density of 2.70 g/cm³. What is its mass?
2. The same block has a 6 mm through-hole drilled along the 10 mm direction. What is its mass?
3. Body A has a mass of 27.0 g with its CoM at x = 0 mm. Body B has a mass of 12.0 g with its CoM at x = 40 mm. What is the X coordinate of the combined CoM?
4. Three bodies have masses and CoM positions in millimeters: 10 g at (0, 0, 0), 20 g at (30, 0, 0), and 30 g at (0, 40, 10). What is the combined CoM?
5. Convert a mass of 27.0 g to pounds, using 1 lb = 453.59237 g.
6. Eight holes are spaced evenly around a circle. What is the angle between two neighboring holes?
7. A 2D line segment has two free endpoints. How many degrees of freedom does it have before any constraints are applied, and how many constraints fully fix it?
8. Team A has part scores totaling 280 and an IAS of 85. Team B has part scores totaling 270 and an IAS of 95. Which team has the higher event score, and what happens next if the scores are equal?
9. In one sentence, explain why a ruler measurement from a printed drawing is a poor substitute for the drawing's dimension values.
10. A part's correct volume is 12,500 mm³ and your model's volume is 12,200 mm³. What is its IPS?
11. A part is drawn in inches, but you modeled every dimension as millimeters. By what factor is your volume off, and what is the IPS?
12. The correct center of mass is (50.0, 20.0, −8.0) mm and yours is (49.0, 20.0, −10.0) mm. What is the IAS?
13. Two parts with the same volume share one material. Does changing that material change the assembly's center of mass? Explain.

References and further reading

• Current rules: the Division C Engineering CAD manual on the Science Olympiad event pages at soinc.org. Use the 2027 manual; the part counts and the part-score quantity (volume) changed from 2026.
• Recommended resources: the Science Olympiad store at store.soinc.org sells general Science Olympiad resources; the 2027 event rules list no recommended resources.
• Software: Onshape, with the education access page at onshape.com/edu. Use Onshape's built-in help to look up sketch constraint colors and the mass properties tool in your version.
• Center of mass and mass properties: the center-of-mass chapter of OpenStax University Physics Volume 1, free at openstax.org.
• Density and unit definitions: the CRC Handbook of Chemistry and Physics for material densities, and the NIST Guide for the Use of the International System of Units for exact unit conversions.
• Drawing conventions: ISO 128 (general principles of technical drawing presentation) and ASME Y14.5 (dimensioning and tolerancing). Your teacher or a library copy is the easiest way to read the full standards.
• Event overview on the SciOly Wiki: Engineering CAD on the SciOly Wiki. Use it as a link for background, not as a source of scope.

There are no subtopic guides for this event yet. The related guides in this library are Boomilever and Electric Vehicle, which share the design, measurement and careful-building habits this event rewards.