Overview#
Constraints are rules that tie sketch geometry together. Where a dimension says "this is 25 mm long", a constraint says "this is horizontal", "these two touch", or "these are the same size". The sketch solver combines every constraint and dimension to compute where each curve and point sits. A sketch with enough of them to leave nothing free to move is fully constrained, and that is the goal for any geometry that other features rely on.
Fusion's official Sketch help lists twelve constraint tools, all found in Sketch > Constraints. This page describes each, shows how to apply it, and explains inference, visibility, and conflicts.
Where to find it#
- Panel: Sketch tab > Constraints panel (a drop-down listing all constraint types).
- Automatic inference: As you move the cursor, object snap symbols appear when you snap to the grid or other geometry, and if you snap to a specific point the logical constraints are added automatically.
- Workflow: Constraint tools are available only in the Sketch contextual tab while a sketch is being edited. Start the tool first (the constraint icon appears next to the cursor), then click the geometry.
- Shortcut: No default shortcuts for individual constraints are documented. Press S to search the toolbox by name.
The constraints#
| Constraint | Definition (per Autodesk help) | Typical use |
|---|---|---|
| Horizontal/Vertical | Aligns a single line, or two points, to the horizontal or vertical axis, whichever is closer | Squaring up outlines; aligning center points |
| Coincident | Joins two points, or places a point on a line or curve | Closing profiles; attaching endpoints; locating a center on an edge |
| Tangent | Makes a curve and another object touch at one point without crossing | Smooth line-to-arc transitions; circles touching lines |
| Equal | Makes similar objects the same size so they update together | Equal-radius holes; equal-length sides |
| Parallel | Makes two lines extend in the same direction so they never intersect | Parallel edges, slots |
| Perpendicular | Sets two objects at a 90-degree angle | Right-angle corners |
| Fix/UnFix | Locks the size and location of a point or object | Anchoring the first piece of geometry |
| Midpoint | Places a point or object at the midpoint of another object | Centering features on an edge |
| Concentric | Gives two or more arcs, circles, or ellipses the same center point | Concentric holes, counterbores, rings |
| Collinear | Makes two or more objects share a common line | Aligning edges along one line |
| Symmetry | Makes objects mirror each other about a common axis | Symmetric designs |
| Curvature | Creates smooth G2-continuity curvature between a spline and another sketch curve | Fair blends between splines |
Horizontal/Vertical#
Start the tool and select a line: it snaps to the horizontal or vertical axis, whichever is closest to its original orientation. Select two points and they align horizontally or vertically. This is the most commonly inferred constraint. A single command handles both.
Coincident#
Select two points, or a point and a line or curve. Two points merge into one location; a point and a curve means the point is constrained along the curve. Coincident is the key to closed profiles. Unconstrained end points of lines and splines show as white dots (grey dots for internal spline fit points); point-to-point coincident constraints show no icon, while point-to-curve constraints show the coincident icon. Notice the difference between point on curve and point to point: the first leaves one degree of freedom (the point can slide along the curve).
Tangent#
Select a curve and another object. They touch at a single point and never cross. The geometry snaps to maintain a tangent connection.
Equal#
Select similar objects (lines for equal length, circles or arcs for equal radius). The geometry snaps to match the size of the first object you selected. Equal is powerful: dimension one hole and all equal holes follow.
Parallel and Perpendicular#
Select two lines. Parallel makes them point in the same direction; Perpendicular makes a 90-degree angle. Parallel is defined for two lines; Perpendicular for two objects. As general guidance (not from Autodesk's help), for long-term robustness, a Perpendicular constraint is often better than a 90-degree dimension because it cannot flip to 270 degrees.
Fix/UnFix#
Select a point or object to lock its size and location; it turns green. To unfix, select the Fix/UnFix tool again and click the geometry. Use Fix for the anchor of the sketch, typically a point at the origin, or sparingly on projected geometry. Overusing Fix is a common cause of sketches that cannot be edited: every dimension to a fixed item becomes a no-op, and changes to other items conflict.
Midpoint#
Select a point or object and the object whose midpoint it should sit on. Use it to center a hole on an edge, or to put a construction line's end at the middle of a side. Because the point can be any point (including a line's endpoint), midpoint can also attach one curve's endpoint to the center of another curve.
Concentric#
Select two or more arcs, circles or ellipses. They share the same center point.
Collinear#
Select two or more objects (for example a line and one edge of a rectangle). They share a common line. Segments do not need to touch. It keeps long edges aligned across gaps, for example two sides of a notched rectangle.
Symmetry#
Select the objects, then select the line of symmetry. They mirror across that line, which is typically a construction line or the sketch axis. Use symmetry to hold a profile centered about an axis with a minimum of dimensions: you can dimension half the overall width and have the other half follow.
Curvature#
Select a spline and the chained sketch curve. The result is smooth G2 continuity. It can be applied between a spline and another spline, or a spline and a regular sketch curve. See the splines page for the context.
Seeing and managing constraints#
- Show Constraints: Toggle in the Sketch Palette. When on, each constraint is shown as a small icon (badge) next to the affected geometry.
- Hover: Hovering a badge highlights the geometry it involves.
- Delete: Select the badge and press Delete (general practice). To remove a point-to-point coincident constraint, select the point, right-click and choose Delete Coincident. Deleting a constraint frees the geometry, and it turns blue (unconstrained).
- Hide: Use Show Constraints in the Sketch Palette to hide badges you do not need.
- Dimensions as constraints: Dimensions (see the dimensions page) are also constraints but they are called driving dimensions, and they have values.
Automatic constraints#
While you draw, Fusion infers constraints and shows a glyph near the cursor. If you click when a glyph shows, the constraint is added. Inference can add constraints you did not intend (a surprise Horizontal, an accidental Coincident with a distant projected edge), so keep an eye on the glyph before clicking.
Note: not confirmed in Autodesk's documentation: a "Constraint Settings" list in the Sketch Palette. The palette reference does not list it, so look for the inference options in your own build.
Order of application#
Apply constraints from the general to the specific: first Fix an anchor or constrain the geometry to the origin, then relationships such as Horizontal, Coincident, and Tangent, then Equal and Symmetry, and last dimensions. Doing so reduces the chance that a later constraint conflicts with an earlier one.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Constraint tool selection | Choose the constraint from Sketch > Constraints | Then click the objects; Equal matches the first selected |
| Show Constraints | Toggles badges | Sketch Palette |
| Delete constraint | Removes a relationship | Select the badge, press Delete |
| Fix/UnFix | Locks size and location (geometry turns green) | Select the tool again and click to unfix |
Tips and pitfalls#
Tip: The cheapest way to constrain a sketch is to draw carefully so Fusion infers the right constraints, then add the missing ones and dimensions by hand. Watch the glyphs.
Tip: Prefer Symmetry and Midpoint over a dimension pair for centered geometry. Fewer dimensions, and the design intent (centered) is recorded explicitly.
Tip: Use Equal early on. A set of ten equal-radius holes needs one diameter dimension.
Warning: Redundant or conflicting constraints are the primary cause of over-constrained sketches. If a new constraint produces a conflict warning, delete the last constraint rather than forcing it.
Warning: Fix everything and you will be unable to edit anything. Reserve Fix for one anchor, and prefer dimensions to the origin instead.
Warning: Tangent on a circle to a line has two solutions (either side of the line). If the circle jumps to the other side, drag it back and consider adding a dimension or a Coincident to lock the side.
Practice exercise#
- Draw four lines roughly forming a quadrilateral with a missing connection at one corner.
- Apply Coincident to close it. Apply Horizontal/Vertical to opposite sides, and Perpendicular to the adjacent ones. Confirm that the shape becomes a rectangle.
- Add a circle in the center. Use Midpoint on two construction diagonals (draw them first) and Coincident to locate the circle's center at their intersection.
- Add an Equal constraint between two opposite sides and see how many dimensions you still need.
- Toggle Show Constraints and count the badges.
Expected result: a rectangle with a centered circle that needs only a width, a height, and a diameter to be fully defined (plus an anchor).
Related#
- Dimensions (02-sketching/dimensions)
- Fully constrained sketches (02-sketching/fully-constrained-sketches)
- Sketch palette (02-sketching/sketch-palette)
- Troubleshooting sketches (02-sketching/troubleshooting)