Relations

A relation ties two sketch pieces (or points on them) together so they stay that way as the sketch changes.

Step by Step: Adding a Relation

Open a sketch and draw the pieces (see Lines, Circles and Rectangles).
Click Select on the Sketch tab (or press S).
Click the first piece. It lights up. Click the second piece: each click adds one, and a click on a chosen piece drops it. To pick points instead of whole pieces, click the small point marks that show as the pointer passes over a piece.
Rest the mouse for about half a second. A compact bar of icons appears beside the pointer, offering only the relations that fit that selection. Hover an icon to see its name.
Click the relation. The pieces move to meet it, and a small green square marks it on the sketch.
Esc, a click elsewhere, or picking a new selection closes the bar without adding anything. You can also right-click the selection while the Select tool is active: the top of the menu, under Make them, lists the same relations. The menu opens only when at least one whole piece is selected. With only points picked, use the bar, or Add a relation in the Properties panel.

To see or delete a relation later, click Edit on the Sketch tab: every relation and dimension in the sketch is listed under Constraints, the ones added for you while you draw included, each with an x (see Edit Menu). Clicking a row selects the pieces it ties. To remove one from the sketch itself, click its green square, then click it again (or press Delete); Ctrl+Z puts it back. An AI assistant on the connector lists, adds (Merge and Pierce included, on a point) and removes constraints the same way. Select a piece and Properties lists the relations on it too. The bar and the menus leave out Coradial, Merge and Pierce to keep them short: tick Offer Pierce, Merge and Coradial when making relations under Constraints to get them back. Relations already in a sketch stay and are listed either way.

With the Node tool you can pick two points (hold Shift for the second), or a point and a line, and get the point relations (see Node).

Every Relation

Listed alphabetically:

Coincident: two points (or a point and a line, or a point and a round) sit on top of each other
Collinear: two or more lines lie on the same infinite line
Concentric: two or more circles or arcs share a center
Coradial: two or more circles or arcs share a center and a radius, so they lie on one circle (see Coradial Relation)
Equal: lines match length, or circles/arcs match radius
Fix / Unfix: pins a piece in place (or releases it); a Fixed piece behaves like an anchor (see below)
Horizontal / Vertical: a line runs level or upright in the sketch plane
Intersection: a point sits where two lines, circles or arcs cross (see Intersection Relation)
Merge: two points become one point and move together (see Merge Relation)
Midpoint: a point sits at the midpoint of a line
Parallel: two or more lines run the same direction
Perpendicular: two lines meet at a right angle
Pierce: a point sits where an edge of the part or a reference axis passes through the sketch plane (see Pierce Relation)
Symmetric: two pieces of the same kind sit as mirror images about a construction line; or a line is held midway between two parallel lines; or two points sit as mirror images about a line. Mirror Entities adds this relation to its copies (see Mirror Entities)
Tangent: a line meets a circle or arc smoothly, with no kink; or two circles or arcs, in any mix, touch at one point, side by side or one inside the other (see below)

Relations on Points

Pick points rather than whole pieces and the choices change:

Two or more points: Coincident, Horizontal (level with the first point) or Vertical (straight above or below it). Each point after the first is tied to the first.
Exactly two points: Merge as well, which makes them one point.
A point and two lines, circles or arcs: Intersection, the point goes where they cross.
A point and a line: Coincident (the point goes onto the line) or Midpoint (to its middle). The line stays and the point moves.
A point and a circle or arc: Coincident (on the round) or Concentric (at its center).
Two points and a line: Symmetric about the line.
One point: Fix pins the point where it is, Unfix lets it go. The rest of its piece can still move. When an edge of the part or a reference axis passes through the sketch plane, Pierce is offered too.

Tangent Between Circles and Arcs

Pick two circles, two arcs, or a circle and an arc, then Tangent. The second piece moves along the line between the two centers until it just touches the first, and keeps its size. Whether it ends up outside (side by side, the centers a radius plus a radius apart) or inside (one within the other, the centers a difference of the radii apart) is decided by which the pieces are already nearer to when you add it. For example, a 2 inch circle sitting near the edge of a 6 inch one is made tangent on the inside; one clear of it is made tangent on the outside. Drag either piece afterward and the other follows, still touching. A Tangent that cannot hold with the relations already there, such as circles whose centers are tied together, is refused and nothing changes. Two circles of the same size that overlap are made tangent on the outside. A size typed for either piece later is taken, and they stay touching.

Automatic Relations

While drawing, Add relations while drawing (under Edit on the Sketch tab, in the Constraints part; it is on by default) ties things for you: snapping a line's end to another end, a midpoint, or the origin ties it there automatically, and a line drawn level or upright stays so, all without opening the relation bar yourself. Turn this off if you would rather add every relation by hand.

The Trim and Extend tools tie the new ends they make to the piece that cut them, so a trimmed corner stays closed. See Power Trim, Trim to Closest and Extend.

Dimensions in the List

Each dimension you place is listed with the relations under Edit on the Sketch tab, with its name (such as D1@Sketch1) and, when a formula drives it, the formula. The × deletes it, unless an equation reads it; then a message names the equations. See Equations.

Fully Defined and the Colors

Sketch geometry is drawn in color to show how constrained it is:

Blue: under defined, the piece can still move
Black: fully defined, every relation and dimension on it is satisfied and it cannot move further
Red: over defined, a relation or a typed size on it cannot hold together with the others
Orange, dashed: construction geometry
Grey: a reference to a part edge, which follows the part and never moves in the sketch

A small green square beside a piece marks a relation on it (untick Show relation markers on the sketch under Edit on the Sketch tab if they clutter a busy sketch); Properties, with a piece selected, lists every relation on it and lets you delete any one.

When you drag a point with the Node tool and the relations cannot follow, the piece simply stays at the last place they could hold it; a drag never turns a piece red.

Tips and Common Problems

The relation you want is not in the bar: the bar only shows relations that fit what is selected. Two lines offer Parallel, Perpendicular, Equal and Collinear; a line and a circle offer Tangent; one line offers Horizontal and Vertical. Check that you picked what you meant to (a point or a piece).
A message says the relation was refused and nothing changed: it would fight a relation or dimension already there. Delete the one in the way from the list under Edit, then try again.
A combined outline cannot hold a relation: right-click it and choose Break apart, add the relation to the pieces, then combine again if you like (see Select).
Pieces turned red: they are over defined. Delete the newest relation or dimension from the list under Edit; Undo also works.
Turn on Add relations while drawing under Edit on the Sketch tab, in the Constraints part, so common ties are added for you as you draw.

The Anchor Rule

When a relation involves one piece that is anchored (a part edge, the origin, a Fixed piece, or a piece the solver already has fully pinned down through other relations) and one that is not, the anchored one never moves and the other one moves to meet it. Only when neither piece is anchored does the one you picked first stay put and the other one move. This is what decides which side "gives" when you add, say, a Coincident relation between a free line and a part edge.

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