Patterns, Mirror, and Applied Features

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.

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.

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

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.

Hole options depend on type and software version

Use the preview and parameter descriptions instead of assuming every hole has the same options. See SOLIDWORKS: Hole Wizard Type PropertyManager and Hole Wizard Overview. Standard names in a menu do not replace checking the specified hole requirements.

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