School of Engineering · Playlist

Part Features

Planning a part as features: extrudes, revolves, sweeps, lofts, patterns, mirrors and applied features.

  1. Feature-based Modeling
  2. Extrude and Revolve
  3. Sweeps and Lofts
  4. Patterns, Mirror, and Applied Features
Engineering Graphics and CAD/CAD Modeling

Feature-based Modeling

Plan a solid part as a sequence of features, choose stable references, and test whether the model survives a change.

Build the main shape, then add and remove material

Build the main shape, then add and remove material

A parametric model stores instructions for building a shape. Dimensions and relationships are inputs; the solid is the result. Change an input and rebuild to see the result update.

The base feature creates the initial solid. Later features add material, remove material, or modify faces and edges. For a simple spacer, start with its main cross-section and extrude it. For a stepped round knob, a revolved section may describe the main shape more directly. There is often more than one valid feature sequence.

A body is a connected piece of solid geometry. A SOLIDWORKS part file can contain multiple bodies. An Onshape Part Studio can create multiple parts from a shared feature list. Neither arrangement, by itself, defines assembly motion or assembly relationships.

Start with sketch dimensions and relations in the Engineering Graphics collection. Then choose extrude or revolve for a straight or rotational shape, or sweep or loft for a path or a changing cross-section.

The feature tree records a build sequence and its dependencies

The feature tree records a build sequence and its dependencies

Read the tree from the base feature toward the end. A feature that supplies a sketch, face, edge, or other reference is a parent; a feature that uses that reference is a child. A child can depend on more than one parent. Being later in the list does not, by itself, make a feature a direct child of every earlier feature.

For example: a plate extrusion supplies a top face for a hole-position sketch. A hole feature uses that sketch. A pattern uses that hole as its seed. Delete the hole and the pattern loses its seed; delete the plate and the sketch loses its support as well. Inspect the deletion dialog before accepting dependent deletions.

Rename features for their purpose, such as Main plate, Locating hole, and Hole row. Renaming a feature in the tree is different from renaming a referenced part file. File references need their own reference-aware workflow.

Supporting detail: Addendum 1 — Why a small edit can break a later feature.

Rollback lets you inspect an earlier stage without deleting later work; Checklist

Rollback lets you inspect an earlier stage without deleting later work

Move the rollback bar above later features to inspect or edit an earlier stage. Return it to the end when checking the completed part. Rollback is a temporary stopping point in regeneration. Suppression instead leaves a selected feature in the tree but excludes it from the active model; dependent features may also be affected. Hiding changes visibility, not the solid's definition.

  • Find the earliest feature that fails or produces the wrong shape.
  • Roll back to inspect the geometry and references available at that point.
  • Edit the sketch for its dimensions or relations; edit the feature for its operation, depth, direction, or selected references.
  • Roll forward to the end, rebuild, and inspect the downstream results.

Supporting detail: Addendum 2 — Vendor help for history and rollback.

Choose references that express what must stay aligned

Choose references that express what must stay aligned

A reference plane locates a sketch or defines symmetry. A reference axis supplies a direction or center of rotation. Neither adds material. Use the origin and default planes when they express the design; add offset, angled, or mid-planes when needed. Reference geometry can also have parents.

Design intent is what should stay true when dimensions change. A centered plate should grow equally on both sides of its center plane. A hole required to pass through the plate should remain through when the plate gets thicker. A row of identical holes should share one seed definition and a spacing rule.

Put major shape and functional references early. Add small edge treatments later when they are finishing details. This is a useful starting order, not a rule that every fillet must be last: a large blend that defines the main shape may belong before shelling or other features.

Supporting detail: Addendum 3 — Fewest features is not always the best model.

Check units, bodies, material, and mass after a change; Checklist; Practice

Check units, bodies, material, and mass after a change

Assign the intended material or density before relying on mass. A surface color is not evidence that density is correct. For a uniform solid, mass = density × volume. Compare volume with a simple estimate, and inspect unexpected mass or center-of-mass changes.

A fresh example: a solid rectangular spacer measuring 30 × 20 × 8 mm has a volume of 4,800 mm³ = 4.8 cm³. With an assumed density of 2.50 g/cm³, its mass is 12.0 g. These are practice values, not a material specification. A hole should reduce that mass if the same body and density remain selected.

  • Confirm the document units and overall dimensions.
  • Confirm the expected body or part count and the scope of each add or cut.
  • Change one important dimension, rebuild, and check the intended relationships.
  • Check material assignment, selected bodies, and any mass overrides before trusting the result.

Practice a mass check Practice dependencies

Supporting detail: Addendum 4 — Mass properties are a check, not proof of a correct part.

Engineering Graphics and CAD/CAD Modeling

Extrude and Revolve

Turn a sketch into a straight or rotational solid, and choose an end condition that preserves the intended shape when dimensions change.

Extrude carries a cross-section in a straight direction

Extrude carries a cross-section in a straight direction

For a plain solid extrusion, select a closed sketch region and give it depth. A rectangular region makes a block; a circular region makes a cylinder. Without draft, the cross-section remains constant along the extrusion.

A boss/base extrusion creates or adds solid material. An extruded cut removes material where the extrusion intersects the target solid. Check the arrow, preview, and selected bodies. A cut pointing away from the part cannot remove material from it.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A closed rectangle is carried along a depth direction to create a rectangular solid.
Sketch → straight depth → solid. This schematic shows the geometry, not a software dialog.
Three-step sequence: steps 1 and 2 across the top, then step 3 below. In section, a rectangular sketch on a block is cut downward to leave a flat-bottomed pocket.
Section through a rectangular cut: the floor and surrounding body remain.

In Onshape, choose the result operation New, Add, or Remove. In SOLIDWORKS, check the boss/cut command and merge or feature scope settings. Adding touching material and creating a separate body are different intentions.

Supporting detail: Addendum 5 — Closed profiles, thin features, and surfaces.

Choose the end condition for what should happen after an edit; Interactive; Practice

Choose the end condition for what should happen after an edit

ConditionWhat controls the endUse when
BlindA specified distance in the selected direction.A pocket must keep a particular depth.
Through allAll target material along the selected direction.A cut must remain through as the part thickens. Check body scope and one- versus two-direction settings.
Up to nextThe next terminating surface that intercepts the entire profile.The next suitable boundary is the intended stop. It is not simply the first edge encountered.
Up to surface / faceA selected terminating surface or face.The feature must follow that particular boundary when it moves. The selection becomes a dependency.
Mid-planeA total depth split equally about the sketch plane.The part must stay centered. In SOLIDWORKS, a 14 mm Mid Plane depth extends 7 mm each way.

Worked thickness edit. One rectangular cut starts on the top face of one flat plate, travels downward normal to that face, and removes material from that selected body only. Compare a distance-controlled blind cut with a through-all cut before and after the plate becomes thicker.

All three sections use the same vertical scale: 8 drawing units per millimeter.

BLIND 12 · PLATE 10Open · floor 0 mm
The requested blind distance reaches beyond this plate; actual removal stops at the body boundary.
BLIND 12 · PLATE 16Closed · floor 4 mm
The blind distance stays 12 mm, so the later thickness edit leaves a floor.
THROUGH ALL · PLATE 16Open · floor 0 mm
Through all follows this selected plate in the stated direction.
Design goalChoice that survives the editWhy
Opening must stay throughThrough allThe termination follows the selected plate thickness.
Pocket must retain a floorBlind, with a depth smaller than the final thicknessThe fixed distance intentionally stops before the far face.

This teaching model does not cover up-to-face, up-to-next, multiple bodies, opposite directions or revolved cuts. Check the selected sketch region, direction and body scope in the CAD preview.

Do not substitute an oversized blind cut for a through-all requirement. It may work today and leave a thin floor after a later edit. Conversely, through all is wrong for a pocket that must retain its floor.

Onshape uses a Symmetric option for supported end types. Dialog names and available conditions depend on the selected operation; inspect the preview and measured result rather than transferring every setting by name.

Practice end conditions Practice symmetric depth

Supporting detail: Addendum 6 — Vendor help for extrusion boundaries.

Revolve rotates a section around an axis

Revolve rotates a section around an axis

Select a section, an axis of rotation, and an angle. A full turn is 360°; a smaller angle produces a partial rotational shape. A boss revolve adds material, and a revolved cut removes it. Start with a closed section on one side of the axis for a straightforward solid revolve.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A rectangular section offset from a vertical axis rotates through 360 degrees to make a hollow cylindrical sleeve.
The gap between the section and the axis becomes the bore. Rotating a section that reaches the axis can instead make a solid center.

A straight sketch line, centerline, or reference axis can define rotation when supported by the command. The axis must be deliberately located. A diameter describes the distance across a round shape; the distance from the axis to its outer wall is the radius.

A stepped sleeve can often be built with one revolved section including its bore. Repeated extrusions and cuts can also build it, but put the coaxial steps under separate controls. Choose the sequence that makes the important dimensions easiest to change.

Supporting detail: Addendum 7 — Check overlap and axis selection before adding complexity.

Pick the base feature from the shape's main organizing rule; Practice

Pick the base feature from the shape's main organizing rule

Use extrusion when a useful section stays the same along a straight direction. Use revolution when a useful section repeats around an axis. A cylinder can be made either way. A rotationally stepped part often makes the reason for choosing revolve clearer than a plain cylinder does.

Before accepting either feature, confirm the profile, direction or axis, end condition or angle, and result body. Then make one trial dimension change. Does the model still express the intent described in Feature-based Modeling?

Practice choosing a base Practice a scoped feature count

Engineering Graphics and CAD/CAD Modeling

Sweeps and Lofts

Use a sweep to carry a section along a path and a loft to transition through ordered sections, with references that control the result.

A sweep needs a profile and a path

A sweep needs a profile and a path

A profile describes the cross-section; a path describes where it travels. A circular profile swept around a smooth bend makes a bent solid rod. An annular profile can make a tube. For a basic sweep, keep the section size constant and choose how it stays oriented along the path.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A circular profile at the start of a curved path sweeps into a bent rod with a circular cross-section.
Profile + path → sweep → bent rod. The path is a reference curve, not another solid.

Place the profile on a plane normal (perpendicular) to the path at its start for an easy first construction. Constrain its position to the path. A shape that looks connected in one view can still be separated in three dimensions. Select the complete intended path, not a neighboring model edge.

A sweep can create material or remove it from an existing part. Advanced sweep options can control twist or scaling; a constant circular section is a simpler starting case. See Onshape: Sweep.

Sweep lab: how tight can a bend be before a thick profile folds?; Interactive

Sweep lab: how tight can a bend be before a thick profile folds?

Choose a profile and a path, then tighten the bend. Watch where the inside of the sweep turns red: there, the profile reaches the centre of the bend and the inner wall has to fold back through itself.

The rule this lab tests. Carry a profile along a path. At each point the path has a bend radius ρ: the radius of the circle that best fits the path there, measured to its centre of curvature. The profile also has a reach toward that centre: how far its edge extends from the path toward the inside of the bend. The inner wall folds through itself where

reach toward the centre of curvature ≥ local bend radius ρ

For a round rod centred on the path, the reach is its radius, so a rod of diameter D fails around a bend when D/2 ≥ ρ. Exactly equal is already a failure: the inner wall shrinks to an edge at the centre of curvature.

BUILDS · Ø16 rod, 12 mm bendØ16 circle · half-width across the bend 8 mm+ centre of curvature at the tightest bendbend radius 12 mm · reach 8 mmBuilds: no fold and no clash
Reach 8 mm is less than the 12 mm bend radius, so the inner edge stays a smaller arc with 4 mm to spare.
FAILS · Ø30 rod, 12 mm bendØ30 circle · half-width across the bend 15 mm+ centre of curvature at the tightest bendbend radius 12 mm · reach 15 mmFails · local fold
Reach 15 mm passes the 12 mm bend radius. The inner edge (red) passes the centre of curvature and runs backwards on the far side, folding the wall through itself.
Profile on a 12 mm arcReach toward centreResult
Ø16 mm rod8 mmBuilds (8 < 12)
Ø24 mm rod12 mmFails: inner wall collapses to an edge (12 = 12)
Ø30 mm rod15 mmFails: folds (15 > 12)
30 × 15 mm bar, 30 mm side across the bend15 mmFails: folds
Same bar turned, 15 mm side across the bend7.5 mmBuilds

Only the local bend matters for this test. On an S-curve the bend radius changes along the path, so the failure appears only near the tightest bends. Here a Ø20 mm rod (reach 10 mm) follows an S-curve whose tightest bend radius is 8 mm: 6% of the path fails.

S-CURVE · Ø20 rod, tightest bend 8 mmred: reach toward the centre ≥ local bend radius0481216path startend, 226 mm alongmmbend radiusreach toward centre
Where the reach line rises above the bend-radius line, that stretch of the sweep folds (red bands).

A passing local test is not a complete check. This lab calls a sweep “builds” only on the U-bend, where the geometry also rules out clashes; anywhere else a passing local test is reported as only that, with global clearance not established. A Ø20 mm wire wound with a 30 mm coil radius bends gently (bend radius 30.2 mm), but with a 16 mm pitch neighbouring turns are only 15.9 mm apart, so the wire hits the next coil. Coils collide: neighbouring turns are 15.94 mm apart along the chord between them, but the profile needs 20 mm. The local bend test cannot see this clash.

HELIX · no local fold, but the coils collideFails: neighbouring coils collide
The local test passes everywhere, yet the turns overlap. A real CAD check also looks for clashes between distant parts of the same feature.

Teaching model: the profile is centred on the path and carried without avoidable twist (a rotation-minimising frame). The red regions come from the local test only. It is not a complete validity check. The helix chord check can prove that neighbouring coils collide, never that they clear. A given CAD product may report failures differently or offer other orientation options. Sources: Patrikalakis, Maekawa and Cho, Local self-intersection of pipe surfaces and Global self-intersection of pipe surfaces; Onshape: Sweep.

A loft passes through profiles selected in order

A loft passes through profiles selected in order

A loft transitions between two or more sections. Put sketches on suitable planes, then select the sections in the order the shape should pass through them. A broad oval transitioning to a smaller oval is a simple example; the section size changes along the length.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. Three oval profiles on separated planes are selected from bottom to top and joined into a tapered transition. A guide touches the outside of every profile.
Ordered sections → transition → solid. A guide can control the side between the sections.

Use a guide curve when the profiles alone do not control the shape between them. For a straightforward boundary guide, constrain it to meet every profile at the intended boundary point. A Pierce relation can locate a sketch point where a curve crosses that sketch plane. Do not accept a connection solely because it looks right in an isometric view.

Match corresponding locations around successive profiles. If one section's corner connects to an unrelated corner on the next, the loft can twist. Inspect connection handles and a section view before adding more profiles.

Supporting detail: Addendum 8 — More profiles do not automatically make a better surface.

Loft lab: what moving a start point or reordering profiles does; Interactive

Loft lab: what moving a start point or reordering profiles does

Three profiles stay in place: a square, a circle and a slot. Change only which points the loft pairs and the order you select the profiles, then watch the connector lines twist, pinch or double back.

What decides a loft’s shape. Each profile is divided into the same number of points, counted from its start point (the connector) in the same direction. Point 1 of the first profile joins point 1 of the next, and so on; the loft passes through the profiles in the order selected. Three profiles sit on parallel planes: a 60 mm square at the bottom, a Ø44 mm circle 45 mm up, and a 56 × 24 mm slot at 90 mm.

MATCHED1 square2 circle3 slotMatched · sections checked
Matched start points: each connector runs straight from square to circle to slot.
CIRCLE START +90°1 square2 circle3 slotTwisted · sections checked
Circle start point moved 90°: the connectors spiral. No checked section crosses itself, but it is twisted.
CIRCLE START +180°1 square2 circle3 slotSections pinch or cross
Circle start point moved 180°: paired vertices sit on opposite sides, so sections pass through the middle and cross themselves (red).
ORDER: SQUARE, SLOT, CIRCLE1 square2 slot3 circleWrong order · doubles back
Selected square, slot, circle: the loft climbs to the slot, then comes back down to the circle through heights it already occupies (red).
ChangeResultFix
Start points do not correspondTwist; a large mismatch pinches or crosses itselfLine up the connectors or start points
Profiles selected out of their order along the partLoft doubles back across heights already occupiedSelect profiles in sequence
Whole selection reversedSame surface, built from the other endNothing to fix

Teaching model: every profile runs counter-clockwise, and corresponding points are joined by a smooth curve through all three profiles. A profile drawn in the opposite direction is a separate problem, not modelled here. Twist and crossing come from the actual sections. Source: Onshape: Loft (sequential profile order; connections control twist).

Use the controlling geometry to choose sweep or loft; Practice

Use the controlling geometry to choose sweep or loft

What you knowFirst feature to considerWhat to inspect
One section following a bent centerlineSweepPath continuity, section position, and orientation.
Different sections at several locationsLoftProfile order, connections, and shape between sections.
One section along a straight directionExtrudeDepth or end condition.
A section repeated around an axisRevolveAxis position and rotation angle.

These are starting choices, not exclusive capabilities. For example, a loft can follow a centerline, and a sweep can vary with advanced controls. Prefer the feature that states the intended change clearly.

Practice profile and path Practice changing sections

Challenge: choose the feature, then the one input that fixes it; Interactive

Challenge: choose the feature, then the one input that fixes it

Each target below comes with a failing attempt. Name the feature that states the shape, then pick the change that makes the attempt match the target.

Choose the feature, then the input to change. For each target, decide whether a sweep, loft or extrude states it, then which change fixes the failing attempt.

  1. U-shaped handrail. One Ø20 mm round section follows a U-shaped centreline with a 30 mm bend radius. Current attempt: fails: the inner wall folds through itself.

    Answer

    Sweep. Yes: one constant section follows a bent centreline, which is what a sweep states. Change: Open the bend radius to 30 mm.

  2. Square-to-round duct transition. A duct changes from a 60 mm square, through a Ø44 mm circle, to a 56 × 24 mm slot, with straight, untwisted sides. Current attempt: twisted: no crossing section found.

    Answer

    Loft. Yes: the section changes shape at known positions, which is what a loft states. Change: Move the circle’s start point back to 0° so it lines up with the square and slot.

  3. Three-section transition built out of order. The same square → circle → slot duct, built bottom to top. Current attempt: wrong shape: the loft doubles back.

    Answer

    Loft. Yes: three different sections at fixed heights. Change: Select square, circle, slot: the order the profiles sit along the part.

  4. Compression spring. Ø16 mm round wire wound with a 24 mm coil radius and a 28 mm pitch. Current attempt: fails: neighbouring coils collide.

    Answer

    Sweep. Yes: one wire section follows a helical path. Change: Increase the pitch to 28 mm.

Troubleshoot the inputs before changing every option; Checklist

Troubleshoot the inputs before changing every option

  • Check that the selected profile regions match the intended solid, surface, or thin result.
  • For a sweep, check path continuity and the profile's location and orientation.
  • For a loft, check profile order and each intended guide intersection.
  • Look for self-intersection: a thick swept section may overlap itself around a tight bend.
  • Inspect sections and confirm the expected part count; repair the first failed reference.

Shelling a complicated loft is a separate geometry problem: offset walls can collide where the shape becomes tight. Build and inspect the outer shape first, then check the wall thickness. See shell and other applied features.

Engineering Graphics and CAD/CAD Modeling

Patterns, Mirror, and Applied Features

Repeat geometry with a rule, model useful hole information, and finish a solid with edge treatments, shell, draft, and ribs.

Pattern a seed when the copies should change together; Practice

Pattern a seed when the copies should change together

A seed is the original feature being repeated. A feature pattern makes the repetition explicit: edit the seed's size once and rebuild the copies. Model independent features when their sizes or locations must change independently.

A linear pattern uses a direction, spacing, and count. For a single-direction row with N total instances including the seed, the distance from first center to last is (N − 1) × spacing. Some dialogs also offer a total-span mode; check which distance the field means.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. One hole is selected as the seed, a horizontal direction and spacing are set, and a row of four equally spaced holes results.
Seed → direction and spacing → repeated features.

A circular pattern repeats around an axis. N evenly spaced instances around a complete circle have an angular pitch of 360°/N. A partial arc with both endpoints occupied instead has N − 1 intervals across that arc. Inspect whether the dialog asks for total angle or angle between instances.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A hole offset from a center axis is repeated at four quarter-turn locations around the axis.
Seed + axis → full-circle spacing → four total holes.

Choose feature, face, or body/part pattern deliberately. A feature pattern repeats selected operations; a body/part pattern repeats a larger solid. Check target bodies, skipped instances, and whether every copy actually intersects the intended material.

Supporting detail: Addendum 9 — Copied geometry and recalculated end conditions can differ.

Practice linear spacing Practice angular spacing

Mirror across a plane when symmetry is the rule; Practice

Mirror across a plane when symmetry is the rule

A mirror reflects selected features or bodies across a plane. Corresponding points lie at equal distances on opposite sides. It is not a rotation: an asymmetric shape changes handedness.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. An L-shaped tab on the left of a center plane reflects to an oppositely handed tab at the same distance on the right.
Selected geometry + symmetry plane → reflected geometry.

A stable center plane is usually a better symmetry reference than a face likely to move independently. Check whether the mirror should join material into one body or create another. Assemblies use separate tools to position components; part-level mirror features do not define assembly motion.

See Onshape: Mirror for selection and result options.

Practice symmetry

Hole features store type and size as well as position

Hole features store type and size as well as position

Use a hole feature when the hole needs structured information such as a fastener size, fit, counterbore, countersink, or tapped-hole specification. A counterbore is a larger cylindrical recess; a countersink is a conical recess. A plain circular cut can make geometry, but does not automatically carry the same hole definition.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A center point locates a hole; the counterbore type specifies a wide cylindrical recess over a smaller bore; the sectioned result shows both diameters.
Position + hole definition → modeled hole. Section view shows the recess; no thread geometry is implied.

In SOLIDWORKS Hole Wizard, use Type for the hole parameters and Positions for its centers. Select the appropriate standard, type, size, fit where offered, and end condition. Locate the centers with dimensions and relations. Different hole types require separate Hole Wizard features.

For tapped holes, distinguish drill depth from thread depth. A cosmetic thread represents thread information without cutting a helical groove in the solid. Inspect the selected thread option before expecting detailed thread geometry in an export.

Read hole callouts and drawing symbols in the Engineering Graphics dimensioning topics. This page covers the model feature, not callout syntax.

Supporting detail: Addendum 10 — Hole options depend on type and software version.

Fillet rounds an edge; chamfer bevels it

Fillet rounds an edge; chamfer bevels it

A fillet creates a rounded transition. A chamfer creates a beveled transition. Select the intended edges, set the radius or chamfer dimensions, and inspect the preview all the way around the selection. A small radius can still fail where neighboring faces leave too little room.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A sharp outside corner is selected, a radius is applied, and a rounded corner replaces it in section.
Fillet: selected edge → radius → curved transition.
Three-step sequence: steps 1 and 2 across the top, then step 3 below. A sharp outside corner is selected, two equal setback distances are specified, and a straight bevel replaces it in section.
Chamfer: selected edge → setback dimensions → straight bevel in section.

Keep edge treatments separate when they have different functions or are likely to change independently. Cosmetic edge breaks often belong late; a large blend that controls the main shape may belong early. See planning feature order.

Shell hollows a solid and leaves a controlled wall; Practice

Shell hollows a solid and leaves a controlled wall

Select faces to remove and specify the remaining wall thickness. Removing the top face of a block makes an open container; keeping all faces can make an enclosed cavity. Check whether the thickness is offset inward or outward.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A solid block has its top face selected for removal; a wall thickness is set; the sectioned result is an open container with side walls and a floor.
Solid + opening face → wall thickness → hollow part, shown in section.

If shell fails, inspect small radii and narrow regions where offset faces collide. Try a simpler outer shape or revisit the intended thickness. Do not silently reduce a required wall just to make the command succeed. See Onshape: Shell.

Practice hollowing a part

Draft tapers faces; a rib adds a thin support; Practice

Draft tapers faces; a rib adds a thin support

Draft inclines faces relative to a pull direction, often to help a molded part release. In a neutral-plane construction, that reference keeps its size while selected side faces tilt. Check the direction and which end grows or shrinks. There is no universal draft angle for every material and process.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. Vertical sides of a block are selected with its bottom as the neutral plane; the sides tilt inward toward the top while the bottom width stays fixed.
Faces + neutral plane → angle → tapered sides, shown in section.

A rib adds a thin web between supporting regions. It usually starts from sketch curves plus a thickness and direction. Although grouped here with finishing features, a rib needs sketch geometry. Check that it meets the intended walls and merges with the intended part.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A diagonal sketch line bridges the corner of an L-shaped support; a rib thickness is specified; a triangular web joins the two legs.
Support + sketch → thickness → reinforcing web. Thickness runs across the sketch plane.

See Onshape: Draft, Rib, and the feature tool glossary. After any applied feature, rebuild, inspect the section, and make a trial change to its parent geometry.

Practice support features Practice draft

Supporting detail

Addendum

Additional evidence, standards context, and background referenced from the main text.

  1. Engineering Graphics and CAD/CAD Modeling/Feature-based Modeling

    Addendum 1. Why a small edit can break a later feature

    A face or edge can disappear when the shape changes. A sketch attached to that face, or a fillet attached to that edge, then has a missing reference. Repair the first failed feature before chasing errors farther down the tree. Reordering is constrained by dependencies: a feature cannot use geometry that has not yet been created.

    Back to reference 1

  3. Engineering Graphics and CAD/CAD Modeling/Feature-based Modeling

    Addendum 3. Fewest features is not always the best model

    A single complicated sketch can hide many unrelated decisions. Several named features may be easier to edit. Count features only after stating which operations are allowed and what the model must do when changed. A feature tree is also not a manufacturing operation sheet: a CAD cut does not specify tooling or setups.

    Back to reference 3

  5. Engineering Graphics and CAD/CAD Modeling/Extrude and Revolve

    Addendum 5. Closed profiles, thin features, and surfaces

    Closed regions are the simplest starting point for solids. Open sketches can be used with thin-feature or surface options, but those are different constructions: a surface has no solid volume, while a thin feature adds a wall thickness. Check the result type before accepting the preview. See Onshape: Extrude.

    Back to reference 5

  7. Engineering Graphics and CAD/CAD Modeling/Extrude and Revolve

    Addendum 7. Check overlap and axis selection before adding complexity

    A section that crosses the axis, overlaps itself during rotation, or creates zero-thickness contact can fail. Simplify the section, verify its closure and axis, and inspect a small-angle preview. For the command entry points see SOLIDWORKS: Sketching with Extruded or Revolved Bosses/Bases. A turned part may suggest a revolve, but CAD history does not specify a lathe process; see Lathe Operations.

    Back to reference 7

  8. Engineering Graphics and CAD/CAD Modeling/Sweeps and Lofts

    Addendum 8. More profiles do not automatically make a better surface

    Extra sections and guides can introduce unwanted waves or conflicting conditions. Start with the fewest that describe the intended shape, then add a control for a specific problem. Profile and guide rules vary with solid, surface, and thin options. See Onshape: Loft and SOLIDWORKS: Description of Sketch Relations.

    Back to reference 8

  9. Engineering Graphics and CAD/CAD Modeling/Patterns, Mirror, and Applied Features

    Addendum 9. Copied geometry and recalculated end conditions can differ

    Onshape feature patterns have a Reapply features option for regenerating the seed's dependencies and end conditions at each instance. A seed that ends at a sloping face may need different geometry at each copy. Do not assume every pattern automatically recalculates that boundary. See Linear Pattern and Circular Pattern.

    Back to reference 9