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Relations

Relations hold sketch geometry in place relative to other geometry: level, parallel, tangent, on a point and so on. Together with dimensions they define the sketch.

Sketch tab > Add Relations. The sketch page also offers the relations for the selection, as does the right-click menu in the graphics area.

The Add Relations page with a line and an arc in the Entities box, Tangent offered under Add Relations, and the arc's existing relations listed.

Adding a Relation

  1. In a sketch, click Add Relations.
  2. Select the points and entities to relate. Plain clicks add them; Ctrl is not needed.
  3. Under Add Relations, click the relation.
  4. Click OK or press Enter.

In the sketch, holding Ctrl to select a second item that can take a relation opens this page with the selection in Entities. With geometry selected otherwise (a box selection), click a relation under Add Relations on the sketch page, or right-click and choose it.

Only the relations that fit the selection are offered. Once a relation is added, the selection is cleared, ready for the next. A relation that would over-define the sketch is not added; the page says so under the buttons, and the selection is kept.

Selected Entities

Entities
The points, lines, arcs and circles to relate. What was selected when the page opened is already in it. Select an item again, or press Del in the box, to remove it.

Add Relations

A button for each relation that applies to the items in Entities. Each relation added is a step of its own for Ctrl+Z. Relations added stay when the page closes. Entities is emptied after each relation added.

Existing Relations

The relations of the items in Entities, each with a delete button.

Relation Types

Relation Mark Select Result
Horizontal — One or more lines, or two points The lines are horizontal; the points level
Vertical | One or more lines, or two points The lines are vertical; the points plumb
Collinear ⁄ Two or more lines The lines lie on one line
Parallel ∥ Two or more lines The lines are parallel
Perpendicular ⊥ Two lines The lines are perpendicular
Equal = Two or more lines, or two or more arcs or circles Equal lengths, or equal radii
Coincident • Two points, or a point and a line, arc or circle The points meet, or the point lies on the entity
Midpoint M A point and a line The point is at the middle of the line
Tangent T A line and an arc or circle, or two arcs or circles The entities are tangent
Concentric ◎ Two arcs or circles The centers meet
Symmetric ⇹ Two points and a line; or two lines, arcs or circles and a line (the centerline among them, else the last picked) The points are symmetric about the line; the entities are mirror images (circles of equal radius). Two lines each crossing the line are each centered on it

Coincident on two sketch points merges them into one point, so no relation remains to delete. With the origin, or a fixed point such as a model vertex, it adds a Coincident relation instead, which can be deleted to free the point.

A point entity counts as a point. With Horizontal, Vertical, Parallel, Collinear and Equal, each line after the first is related to the first.

Splines

A spline takes only these relations, at an end where it meets the other entity:

Relation Mark Select Result
Tangent T A spline and the line or arc at its end, or two splines meeting end to end Tangent there
Curvature κ The same Tangent and equally curved there (G2)

With two splines, the second one selected follows the first. A new Tangent or Curvature at a spline end replaces the one it had there.

Fixed and On Edge

These show with the relations but are set in other ways:

Fixed (⚓)
A point held in place. Select points or entities and click Fix in the Options section of the sketch page; Float releases them. Its delete button under Existing Relations on the sketch page unfixes the point.
On Edge (⛓)
Geometry made by Convert Entities, held on its model edge and following it. Deleting it under Existing Relations on the sketch page leaves the geometry in place, no longer following the model. When the model edge no longer exists, the mark shows brown and the relation reads dangling.

Relations Added While Drawing

Drawing tools add Coincident, Midpoint, Horizontal and Vertical relations, and relations to model edges, where the pointer snaps. A label beside the pointer names the relation before you click. See Automatic Relations While Drawing.

Relating to the Model and to a Line's Midpoint

In a sketch, clicking a model vertex adds a reference point at it, which can be related like a sketch point and follows the model. A point, line or circle of another sketch shown can be selected the same way.

Right-click a line > Select Midpoint to select a point at its middle in place of the line. Make it Coincident with another point to put that point at the midpoint, or dimension to it.

Showing and Deleting Relations

Each relation shows as its mark in a small green box beside the geometry. Hover over a mark for the relation's name. View > Sketch Relations shows or hides the marks.

A sketched slot-shaped profile showing Horizontal, Tangent, Coincident and Equal marks beside its lines and arcs.

On small or crowded geometry some marks are left out, and the status bar says so. Zoom in, or select the geometry, to see its marks; the marks of selected geometry are shown first.

To delete a relation:

  • Click its mark to select it (Ctrl + click for more), then press Del.
  • Or select the geometry and click the delete button beside the relation under Existing Relations, on the sketch page or the Add Relations page.

See Also