Fully Constrained Sketches

Overview#

A sketch is fully constrained (also called fully defined) when constraints and dimensions leave no geometry free to move. In Fusion, fully defined geometry turns black; unconstrained geometry is blue (and unconstrained centerlines are orange). In the Browser, a red lock appears on the sketch's icon when it is fully constrained. Autodesk's Sketch help treats this as its own topic: "fully defining sketches" and "finding underconstrained geometry" are separate documentation pages.

Why does it matter? Because a parametric model changes only in the ways you specify. Under-defined geometry changes in ways nobody chose: it drifts when you drag it, it may flip to a different solution when a dimension changes, and downstream features that reference it may fail. A fully constrained sketch is predictable, editable, and robust.

This page gives you a systematic, repeatable method for reaching a fully constrained sketch quickly.

Where to find it#

There is no single command. You work with:

• Sketch > Create > Sketch Dimension (D)
• Sketch > Constraints panel (including AutoConstrain)
• Sketch Palette: the sketch Status line (Under-Constrained or Constrained), Find Under-Constrained and Compute Sketch, plus Show Constraints and Show Dimensions
• Color feedback in the canvas (blue versus black)

Degrees of freedom#

Think of each piece of geometry as having a number of freedoms:

Each independent constraint or dimension removes freedoms. Horizontal/Vertical removes 1 from a line (its angle). Coincident of two points removes 2. A length dimension removes 1. Tangent removes 1 (between a line and an arc at a shared endpoint, it also helps determine the arc). The sketch is fully defined when the total is zero. This counting is a general modeling idea (not from Autodesk's help); Fusion shows the sketch Status in the Sketch Palette and the blue-to-black color change rather than a freedom count, so you rely on those and on testing.

A worked example: a rectangle#

A free rectangle drawn with the 2-Point tool has four lines (16 freedoms) before constraints. Assuming the tool adds four Coincident corners (removing 8) and two Horizontal and two Vertical constraints (removing 4; Autodesk's help does not state exactly which constraints each rectangle tool creates) That leaves 4 freedoms: position X, position Y, width, and height. You remove them by pinning one corner to the origin (2 freedoms, via Coincident) and dimensioning width and height (2). Now the rectangle is fully defined and turns black. Four is also the number of things a person would intuitively say they need to specify to describe a rectangle, which is a useful sanity check.

Step by step: the systematic method#

1. Anchor the sketch. Make one significant point coincident to the origin, or constrain symmetric geometry about the origin axes. This removes the free translation of the whole sketch.
2. Draw with intent. As you draw, accept the inferred horizontal, vertical, coincident, tangent, and perpendicular constraints that match your design. Reject the ones that don't.
3. Close the loops. Make sure every endpoint that should meet another is Coincident. Closed loops are the basis for profiles and for solving.
4. Add geometric relationships. Apply Equal, Parallel, Symmetry, Midpoint, Concentric, and Collinear where they express intent. These are cheaper than dimensions and carry design meaning.
5. Add dimensions last. Dimension sizes first (lengths, diameters, radii), then positions (distances from the origin or a reference). Aim for dimensions that mirror how the part will be made or checked.
6. Check the status. Anything blue still has freedom. Read the Status line at the top of the Sketch Palette, click Find Under-Constrained to list the under-constrained entities (selecting one highlights it and zooms to it; the list updates as you add constraints and dimensions), or use Show Constraints and look for what is missing. If the status looks out of date after edits, click Compute Sketch to re-analyze the whole sketch.
7. Test by dragging. Grab a blue point or curve and drag it. How it moves shows which freedom is open: sliding along an edge, rotating about a point, or scaling.
8. Finish when everything is black. Do not chase tiny leftover details in non-critical geometry, such as a decorative construction line; focus on geometry used by features.

Strategies that save effort#

Use symmetry and mirror#

For a symmetric part, draw one half, dimension it, and Mirror. Or draw a Center Rectangle, dimension overall width and height (each only one dimension, since the center is on the origin and the shape is symmetric), then place features with symmetric constraints. You specify half as many numbers.

Let AutoConstrain suggest constraints#

On the Constraints panel, AutoConstrain generates result tiles with suggested constraints and dimensions shown in purple on the canvas. Each tile reports the number of constraints and dimensions and a status (Fully Constrained or Partially Constrained). Use the slider (Reduce Constraints / Add Constraints) to change how many are added, tick Modify Geometry to allow geometry changes within a tolerance, click Generate more for more options, and click OK to apply. You can set a datum (the point that dimensions align to) from a result tile with More > Set datum. Autodesk suggests adding some initial constraints and dimensions first. Finish with AutoConstrain in the Finish Sketch menu applies it as you finish. AutoConstrain is not available in Fusion for personal use.

Use construction geometry as a skeleton#

Draw construction lines and circles that carry the key positions: a centerline, a bolt circle, a reference rectangle. Dimension the skeleton, then constrain normal geometry to it. Edits happen in one place.

Prefer constraints that express intent#

If two holes are the same size, use Equal rather than two identical diameter dimensions. If a hole is in the middle of a plate, use Midpoint or Symmetry rather than half-width dimensions. Each captures intent in a way that survives edits.

Reduce the number of dimension chains#

A dimension chain accumulates changes: change the first and the rest shift. Dimension from a common datum to each feature instead (the origin, or one edge), so edits are independent.

Reference the origin in the right place#

The sketch should be located relative to something stable. You can constrain curves to the origin or dimension them to the origin, and Autodesk lists these along with the Fix constraint as ways to fix the position of curves.

How to find what is still free#

When some geometry is blue and you can't tell why:

• Show Constraints and inspect each badge; look for missing Coincident dots at corners, absent Horizontal/Vertical on lines, or no radius on an arc.
• Drag the blue geometry. If it moves, that is a missing freedom.
• Isolate. Temporarily hide Dimensions and look at geometry relationships, or the reverse.
• Arcs and fillets often hide freedoms: an arc has 5 and is commonly left with an undimensioned radius.
• Splines hold many freedoms; fix them by dimensioning or constraining each fit point, or by acknowledging that they are intentionally free.
• Projected geometry is locked by default and follows its source; your own geometry attached to it still needs constraints.

When not fully constrained is acceptable#

Fully constraining everything is a goal, not an absolute. It is reasonable to leave geometry under-defined when:

• You are sketching a quick concept and will refine it.
• A shape's exact size is irrelevant (a decorative spline outline).
• Fully constraining would require inventing dimensions that have no design meaning.
• The sketch is a one-off cut that will never change.

But: any geometry that other features reference, or that must remain stable when the model is edited, should be fully defined. Under-defined sketches are the number one source of "it changed by itself" surprises.

Options reference#

Tips and pitfalls#

Tip: Constrain as you draw rather than afterward. Locking each part as you go keeps the sketch stable while you add more.

Tip: If dragging a blue point does nothing visible, it may be constrained in one direction. Try dragging along both axes.

Tip: Save a version before the final dimensions so you can return to a good state (general guidance).

Warning: Adding a dimension to something already fully defined over-constrains it. Make it a driven dimension (right-click > Toggle Driven) or delete the existing one first.

Warning: Do not use Fix to turn things black. A sketch that is black because everything is Fixed is rigid, not parametric, and editing it is a nightmare.

Warning: Beware of the "looks right, but is blue" condition. Geometry that appears correct may be one click away from moving.

Practice exercise#

Fully constrain this part profile: a 100 x 60 mm center rectangle with a centered slot 40 mm center-to-center and 10 mm wide, and two 8 mm holes 15 mm from the short edges on the horizontal centerline.

1. Draw the center rectangle on the origin. Dimension 100 x 60.
2. Draw the slot (Center To Center Slot). Make its midpoint coincident with the origin (for example with a Midpoint constraint on a horizontal construction line), and make the slot's axis Horizontal. Dimension its center-to-center distance (40) and width (10).
3. Draw one circle; dimension its diameter 8 and its distance from the right edge as 15 (so its center is 15 mm from the short edge). Constrain its center to the horizontal construction line.
4. Mirror the circle across the vertical axis, or draw a second circle and use Equal plus a Symmetry constraint.
5. Confirm that all geometry is black. Drag any element to verify it does not move.

Expected result: a fully defined profile driven by six dimensions (100, 60, 40, 10, 8 and the 15 mm offset).

Related#

• Constraints (02-sketching/constraints)
• Dimensions (02-sketching/dimensions)
• Sketch best practices (02-sketching/sketch-best-practices)
• Troubleshooting sketches (02-sketching/troubleshooting)