BITS U103 · First-time lesson · 2 of 4
Sketching and constraints
Why your lines are blue, what "fully defined" really means, and the twelve constraints — with a widget that walks a wobbly shape from eight degrees of freedom down to zero. Budget about 50 minutes. This is the most important page in the course.
Sketching is where beginners lose the most time, and almost none of it is lost to the drawing tools — lines and circles take ten minutes to learn. It's lost to constraints, which nobody explains properly, so people fight the software for weeks and conclude they're bad at CAD.
They aren't. They're missing one idea that takes about fifteen minutes to absorb. It's below. Learn it now and you skip the weeks.
1 · Blue means "not decided yet"
Draw a line in Fusion and it comes out blue. Add enough information and it turns black. That colour change is not decoration — it's Fusion telling you something precise:
Blue geometry can still move. Black geometry cannot.
A blue sketch is one where you haven't yet said enough to pin the shape down — so Fusion is guessing, and it's entitled to guess differently later. A fully black sketch is fully defined: exactly one shape satisfies what you've said, and nothing can shift it without your permission.
Try it yourself and the idea lands immediately: draw a rectangle, then click a corner and drag. If it's blue, the shape follows your mouse — the geometry is still negotiable. Do the same on a fully defined sketch and nothing budges.
Why care so much? Recall lesson 1: your model is a recipe, and later steps depend on earlier ones. An under-defined sketch is an instruction that says "a rectangle roughly here, roughly this big." Come back in a week, nudge something, and the roughness resolves differently — and every hole, fillet and shell built on it moves or breaks. Fully defined sketches are what make a model survive being edited.
2 · Degrees of freedom: counting what's still loose
The formal name for "how much can still move" is degrees of freedom, or DOF. The counting rule is simpler than it sounds.
A point on a flat sketch needs two numbers to locate it — an x and a y. So each point carries 2 degrees of freedom. A four-sided closed shape has four corner points, so it starts with 8 DOF: eight independent numbers still undecided.
Every constraint or dimension you add removes one or more of them. Get to zero, and the sketch turns black. That's all "fully defined" means — the number of things still undecided has reached zero.
Unpack: why lines don't get counted separately
A straight line is completely determined by its two endpoints — it has no freedom of its own beyond where those points sit. So counting the points counts everything. (Circles are the exception worth knowing: a circle is a centre point plus a radius, so 2 + 1 = 3 DOF.)
Below, a four-sided shape drawn carelessly — as you'd actually draw it, wobbly and unaligned. Press the button repeatedly and watch two things at once: the shape snapping into line, and the DOF counter falling.
Notice what the sequence shows. The first four constraints never mention a single number — they say only how the shape relates to itself: this edge is horizontal, that one vertical. That alone takes 8 DOF down to 2, turning a random quadrilateral into "some rectangle, sitting at the origin." Only then do two dimensions decide which rectangle.
That order is the professional habit, and it's worth adopting from the start: shape first, size last.
Check yourself: after all four "horizontal/vertical" constraints, exactly 2 DOF remain. What are they, in plain words?
The width and the height. The shape is locked as a rectangle anchored at the origin, but it can still be any rectangle — stretch it wide, stretch it tall. Two undecided numbers, so two dimensions finish the job. (Which is why a fully-defined rectangle needs exactly two dimensions, never four. Dimensioning all four sides means saying the same thing twice, and Fusion will object.)
3 · The twelve constraints
Fusion's sketch palette has twelve constraint types. You'll use the top three for perhaps 80% of everything, so don't try to memorise the table — read it once, then come back when a shape won't behave.
| Constraint | What it forces | Reach for it when… |
|---|---|---|
| Coincident | Two points sit on top of each other; or a point sits on a line or curve. | Closing a gap in a profile, or pinning a corner to the origin. The workhorse. |
| Horizontal / Vertical | A line (or the line through two points) lies along the horizontal or vertical axis — whichever it's already closer to. | Straightening anything that should be square to the world. One command handles both. |
| Equal | Two similar objects have identical size. | Four holes the same diameter, sides of a square. Saves repeat dimensions and keeps them in step. |
| Parallel | Two lines never meet. | Slots, angled features that must stay angled together. |
| Perpendicular | Two objects meet at 90°. | Corners that must stay square even when the whole shape is tilted. |
| Tangent | A curve touches another object at exactly one point without crossing. | Blending an arc smoothly into a straight edge — a slot's rounded end. |
| Midpoint | A point sits at the middle of a line or arc. | Centring something without arithmetic. Far better than dimensioning half the width. |
| Concentric | Arcs and circles share one centre. | A bolt hole inside a boss; any ring-inside-ring. |
| Collinear | Two objects lie on the same infinite line. | Separate edges that must stay in line across a gap. |
| Symmetry | Two objects mirror each other about a chosen axis. | Anything symmetrical. Halves your dimensions and keeps symmetry true under edits. |
| Fix / UnFix | Nails an object's size and position where it is. | Rarely. It's a blunt instrument — see the trap below. |
| Curvature | A spline flows into another curve with matching curvature (G2). | Styling smooth organic surfaces. Not first-course material. |
Using Fix to force a sketch black. It works, and it's a trap: Fix pins geometry in place without expressing why it belongs there, so the sketch stops responding to the parameters around it — precisely the flexibility you built a parametric model to get. A sketch made black with Fix is defined the way a jammed door is closed.
If you can't work out which real constraint is missing, leave it blue and ask. Blue is honest; Fix is a lie that looks like an answer.
4 · Constraints or dimensions? Prefer constraints
Both remove degrees of freedom, so both turn blue to black. They are not equally good.
A dimension (D) fixes a number: this edge is 60 mm. A constraint fixes a relationship: these two edges are equal, whatever they become.
Say you need a square. Two ways:
- Dimension the width 40 and the height 40. Black. But it's a square only by coincidence of two numbers — change one and you silently have a rectangle.
- Dimension the width 40, then add an Equal constraint between adjacent sides. Also black, same DOF count — but now it is a square by construction. Change 40 to 75 and it's still a square.
The second model knows something the first doesn't: it knows it's meant to be square. That knowledge is what people mean by design intent, and it's the difference between a model that survives its first revision and one that quietly goes wrong.
The working rule: express everything you can as a relationship; use numbers only for what genuinely is a number.
Check yourself: a plate has four identical holes, one near each corner, always 10 mm in from both edges. Which constraints do the work?
Equal between the four circles, so one diameter dimension sizes all four. Then either two dimensions (10 and 10) per hole from the nearby edges — or better, a Symmetry constraint about the plate's centre lines, so the pattern stays correct when the plate resizes. Total dimensions: one diameter and two offsets, instead of twelve numbers that all have to be kept in agreement by hand.
5 · Auto-constraints: the invisible thing that's been confusing you
Here's the piece that explains most early frustration. Fusion adds constraints on its own while you draw. Sketch a nearly-horizontal line and it silently applies a Horizontal constraint. Start a line near an existing endpoint and it applies Coincident. Watch closely and you'll see little constraint glyphs appearing next to your geometry as you work.
This is helpful roughly 90% of the time and maddening the rest, because it produces exactly the symptom beginners report most: "I can't move this line and I don't know why." An invisible constraint is holding it, one you never consciously added.
Three things to do about it:
- See them. The glyphs are small; zoom in. Clicking a piece of geometry highlights the constraints attached to it.
- Delete the wrong ones. Click the glyph, press Delete. The constraint goes, the DOF comes back, the line moves again.
- Suppress them when you need to. Hold Ctrl (Windows) or Cmd (macOS) while drawing and Fusion won't add automatic constraints for that stroke — useful when you deliberately want a line at 3° from horizontal and Fusion keeps insisting it's horizontal.
Over-constrained sketches. Add a constraint that contradicts one already present — dimension all four sides of a rectangle, say — and Fusion warns that the sketch is over-constrained. The reflex is to hunt for the constraint you just added. Usually the real culprit is an auto-constraint from ten minutes ago that already said what you're now trying to say.
Read the warning, look at the highlighted geometry, and delete the redundant constraint rather than abandoning the one you actually wanted.
6 · How to sketch, in practice
Put together, the professional sequence looks like this. Follow it literally for a couple of weeks and it becomes automatic.
| Step | Do | Don't |
|---|---|---|
| 1 · Anchor | Start the first shape at or near the origin, and constrain something to it. | Draw far off in empty space — the sketch then floats with nothing holding it. |
| 2 · Rough it in | Draw the shape quickly and approximately. Get the topology right — the right number of edges, all connected. | Try to draw at the correct size by hand. Pointless; the dimensions will fix it. |
| 3 · Shape | Add relationship constraints: horizontal, vertical, equal, symmetric, tangent. | Reach for dimensions yet. |
| 4 · Size | Now add dimensions (D) — the fewest that finish the job. | Dimension everything in sight. Redundant dimensions cause over-constraint warnings. |
| 5 · Verify | Confirm every line is black before leaving the sketch. | Extrude a blue sketch "just for now". There is no such thing as just for now. |
Fusion will also tell you outright: while a sketch is open, the status bar reports how many degrees of freedom remain, and it announces when the sketch becomes fully constrained. Get in the habit of glancing at it before you finish.
Check yourself: you finish a sketch and one short line is still blue, everything else black. What's the fastest diagnosis?
Click that line and drag it. Whichever way it moves tells you what's undecided: if it slides along its own direction, its endpoint isn't pinned (a Coincident is missing); if it tilts, its angle is free (Horizontal, Vertical, Parallel or Perpendicular is missing); if it stretches, its length is free (a dimension or an Equal is missing). Drag it and watch what it does — the movement names the missing constraint. Then undo the drag before adding it.
7 · What to do this week
- Do the drag test on any sketch you've already made. Feel the difference between blue and black. Five minutes.
- Rebuild one rectangle five times — origin-anchored, shape constraints, two dimensions, fully black, no Fix. Boring, and exactly how the habit forms.
- Then take on a shape with an arc in it — a slot, or a rounded bracket. Tangent is the one you'll need, and the first tangent constraint is a small revelation.
- Next lesson: features and design intent — turning these profiles into solids, and learning to see a part as a sequence of operations.
"In Autodesk Fusion, my sketch has 2 degrees of freedom left and I can't see what's loose. I have: a closed 6-sided profile, all lines horizontal or vertical, one corner coincident with the origin, and dimensions of 50 and 30 on two edges. List the most likely missing constraints, most likely first, and tell me the drag test to confirm each."
"Give me five small 2D profiles to sketch in Fusion, in words with dimensions, ordered easiest to hardest, each one needing a different constraint (equal, symmetry, tangent, midpoint, concentric). For each, tell me the DOF count I should end at."
Caution: an AI can't see your screen, so describe the sketch precisely — number of edges, what's already constrained, DOF remaining. Vague question, vague answer.