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Sketching · Lesson 10

Fully defined sketches in SOLIDWORKS

A sketch is fully defined when its dimensions and relations leave nothing free to move: every line has a size, a direction and a position. SOLIDWORKS shows it in black, writes Fully Defined in the status bar and drops the (-) from the sketch name in the tree. It is not required, but fully defined sketches change only the way you tell them to, which is why nearly every training course asks for them.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Same sketch shown under defined in blue and fully defined in black with the status bar text

Where to find it

Status bar (bottom right); Sketch tab → Display/Delete Relations flyout → Fully Define Sketch

Sketch states

State Colour Tree prefix What to do
Under defined Blue (-) Add dimensions or relations
Fully defined Black none Nothing — move on
Over defined Red (+) Remove or make driven a conflicting dimension or relation
Cannot be solved Red (?) Use SketchXpert (click the status bar message)

Fully Define Sketch options

Option Choices
Entities All entities in sketch, or selected entities
Relations Which relation types it may use (all on by default)
Dimension scheme Baseline, Chain or Ordinate — separately for horizontal and vertical
Datum Origin, a model edge or vertex, or a point or line in the sketch
Placement Above, below, left or right of the sketch

It works best on lines and points; add Equal relations to arcs yourself. A System Option, Use fully defined sketches, makes SOLIDWORKS insist on fully defined new sketches — useful for teams that want to enforce the habit. If the sketch turns red instead of black, see sketch errors.

Step by step

  1. 1

    Read the state

    Look at the status bar at the bottom right: Under Defined, Fully Defined or Over Defined. Blue entities can still move; black ones cannot.

  2. 2

    Drag to find what is free

    Drag a blue line or point. Whatever moves is missing a dimension or a relation — add exactly what describes your intent, nothing more.

    Three sketch states — under defined blue, fully defined black, over defined red — with tree prefixes
    Under defined, fully defined and over defined — the colours and tree prefixes.
  3. 3

    Tie the sketch to the origin

    A sketch can be fully sized and still float. A coincident relation or a dimension to the origin fixes its position.

  4. 4

    Or let SOLIDWORKS finish it

    While editing the sketch, open Display/Delete Relations → Fully Define Sketch. Choose All entities, which relation types it may add, a dimension scheme (Baseline, Chain or Ordinate) and a datum — usually the origin. Click Calculate, review the result, then the green tick.

  5. 5

    Find under defined sketches in the tree

    Under defined sketches show (-) before their name. Type (-) into the FeatureManager filter to list them all.

Common mistakes

  • Running Fully Define Sketch before adding your own key dimensions. It adds whatever fills the gaps, not necessarily your design intent. Add the important ones first.
  • Expecting Undo to be easy after Fully Define Sketch — once accepted, only Ctrl + Z reverses it.
  • Adding a dimension to a black sketch. It over defines it; make it driven instead.
  • Leaving one point blue on a line that looks black — drag the endpoints to check.

Lesson 10 of 17 in the sketching course.

Practice

Sketch a 60 × 40 rectangle with its bottom-left corner on the origin and a 20 × 20 notch cut out of the top-right corner (six lines). Fully define it with exactly four dimensions (60, 40, 20, 20) and relations — no Fix. Extrude 10 mm. Check: volume 20,000 mm³, and the sketch name in the tree has no (-).

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

What does fully defined mean in SOLIDWORKS?

+

All sizes, directions and positions in the sketch are set by dimensions and relations, so nothing can move. The geometry is black and the status bar says Fully Defined.

Do sketches have to be fully defined?

+

No, SOLIDWORKS lets you build features from under defined sketches. But they can change shape unexpectedly when you edit other features, so resellers and training courses recommend fully defining production parts.

What does (-) mean before a sketch name?

+

The sketch is under defined. (+) means over defined and (?) means the sketch cannot be solved.

Can SOLIDWORKS fully define a sketch automatically?

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Yes, with Fully Define Sketch in the Display/Delete Relations flyout. It adds dimensions and relations to everything still free. Add your design-intent dimensions first, then let it fill the rest.