Geometric Relations in Sketches

Relations preserve geometry when dimensions change

A geometric relation is a rule the sketch must continue to satisfy: two lines stay parallel, two circles keep one center, or an endpoint stays on a curve. Onshape generally calls these rules constraints; SOLIDWORKS calls them relations.

Choose the entities carefully. Selecting a circle's center is different from selecting its circumference. A relation can remove some motion while leaving other motion available. The diagrams show only the named rule, not a complete dimensioning scheme.

The before/after drawings are original geometry diagrams, not software icons. Their line colors do not indicate sketch status.

Coincident connects a point; midpoint puts it halfway along

Coincident

Two points share a location, or a point lies on a selected line or curve. Joining two endpoints closes their gap. A point on a line can still slide along it unless another rule locates it.

Before: separate line endpoints. After: one shared endpoint. — Coincident controls connection. It does not by itself set either line's length or angle.

Midpoint

A point stays halfway between a segment's endpoints. It is more specific than simply putting the point somewhere on the line. Onshape also supports midpoint on an arc.

Point selection and vendor names

See Onshape's Coincident and Midpoint. SOLIDWORKS also lists Merge Points for combining sketch points or endpoints in its relation reference.

Collinear shares a line; parallel shares only its direction

Collinear

Two straight segments lie on the same infinite line. They may have a gap between them; collinear does not join their endpoints.

Before: two differently directed segments. After: both lie on one dashed extended line, still separated. — Same underlying line does not mean same length or touching endpoints.

Parallel

Two lines keep the same direction. Their spacing, lengths, and positions along that direction still need other rules.

Before: two lines with different slopes. After: two separated lines with matching slopes. — Parallel lines can rotate together; neither must be horizontal.

Software vocabulary: SOLIDWORKS has a Collinear relation. Onshape's documented toolbar has no separate Collinear entry. For two nonzero straight segments, placing both endpoints of one coincident with the other's underlying line enforces the same geometric condition. This is a construction from point-on-line constraints, not an Onshape command name.

Horizontal and vertical use the axes; perpendicular uses another line

Horizontal

A line's endpoints have the same vertical coordinate. For two selected points, horizontal aligns their heights without joining them.

Before: a sloping line. After: a line parallel to the sketch x axis. — Length and position can still change.

Vertical

A line's endpoints have the same horizontal coordinate. Two selected points can likewise be aligned vertically.

Before: a sloping line. After: a line parallel to the sketch y axis. — Use the sketch axes, not the edges of the rotated screen view.

Perpendicular

Two line directions form a right angle. They may rotate together while preserving that angle. The relation does not require their finite segments to meet.

Before: oblique crossing lines. After: two lines whose directions are 90 degrees apart. — If a joint is required, also connect the intended endpoints.

Why horizontal plus vertical can already supply a right angle

A horizontal line and a vertical line already have perpendicular directions. Adding a 90-degree driving dimension can duplicate the existing control. Check the stored rules first. See Onshape: Working with Constraints.

Concentric shares a center; equal shares size; coradial shares both

Concentric

Circles or circular arcs share a center. They can have different radii. For arcs, their endpoints and sweep angles are not determined by this relation.

Before: two circles with different centers. After: nested circles with one center and different radii. — Concentric suits two circular boundaries around the same axis.

Equal

Selected line segments keep equal lengths; selected circles or circular arcs keep equal radii. Equal does not move their centers together. Equal arc radii do not imply equal arc lengths when the sweep angles differ.

Coradial

Two circular arcs share both center and radius: they belong to the same underlying circle. They need not touch or have equal sweep angles. SOLIDWORKS names this relation Coradial. In Onshape, concentric plus equal radius expresses this condition.

Before: arcs on different circles. After: separate arcs on the same dashed supporting circle. — Compare all three: same center, same size, or both.

Check the circular relation definitions

See Onshape's Concentric and Equal. The SOLIDWORKS 2025 relation table correctly places the coradial definition; the 2026 table misplaces its center-and-radius sentence under Perpendicular.

Tangent controls direction at contact; Fix holds a reference in place

Tangent

A line and a circle touch without crossing: the line is perpendicular to the radius at contact. Curves meeting tangentially have a common tangent direction. Tangency alone does not necessarily join the endpoints you intended; add endpoint coincidence when a continuous profile needs it.

Before: a line cuts through a circle. After: the line touches the circle at the end of a perpendicular radius. — A smooth-looking connection still needs the correct relations. Tangency does not require equal radii.

Fix

Fix grounds selected geometry at its current location. Fixing a point removes its freedom to move in the sketch plane. It is useful for a deliberate fixed reference, but does not explain why an arbitrary location or size is correct.

Before: a point can move relative to the origin. After: a lock marks the point held at its current position. — The example fixes a point. Do not generalize it to every entity's endpoints.

SOLIDWORKS qualification: its relation reference says endpoints of a fixed line can still move along the underlying infinite line, and arc endpoints can move along the supporting circle. Check the entity and its endpoints. Onshape describes Fix as grounding the selected entity on the sketch plane.

Vendor help for tangent and fixed geometry

Read Onshape: Tangent, Onshape: Fix, and the Fix row in SOLIDWORKS: Description of Sketch Relations.

Watch automatic relations, then check what was stored; Practice

Watch automatic relations, then check what was stored

Sketching tools can add relations while you draw. A visual alignment is useful feedback; inspect the resulting relation icons before assuming the intended rule is present.

SOLIDWORKS: with Automatic Relations enabled, its documented cursor cues include horizontal, vertical, coincident, midpoint, perpendicular, and tangent. Hold Ctrl while sketching to suppress automatic relations temporarily.
Onshape: Automatic Inferencing documents horizontal, vertical, midpoint, parallel, and coincident as common inferences. Hover near existing geometry to activate the relevant inference; Shift suppresses inferencing while dragging.

These are documented examples, not an exhaustive promise for every tool. For equal, concentric, coradial, collinear, or fix, deliberately apply or verify the required rule. Rectangle, slot, and other creation tools can supply their own relations.

If an unwanted rule was stored, remove that specific rule before adding a conflicting dimension. Continue with Fully Defined Sketches and Design Intent.

Automatic behavior depends on the tool and settings

Checked against SOLIDWORKS 2026: Using Automatic Relations and Onshape: Automatic Inferencing. The keys differ between programs.

Practice: distinguish circular relations