Lines, arcs, circles, and constraints — the flat shapes that become every 3D part you'll ever make.
Every 3D feature in parametric CAD starts as a 2D sketch. You draw geometry on a plane, then lock it with constraints and dimensions until it is fully constrained.
Robotics parts demand precision. A bearing pocket 0.1 mm too large allows play; a hole pattern that shifts on upstream edits causes assembly failures. Fully constrained sketches capture design intent mathematically, so changes propagate predictably.
Master these core 2D tools and you can create any profile, from a simple bracket to a complex cam.
Click two points for a straight segment. Chain clicks for connected polylines. Press Escape to finish.
Four-sided closed profile. Variants: center, 3-point, and corner rectangle. Great for plates, tabs, and slots.
Define by center + radius or three circumference points. Used for holes, shafts, and bearings.
Partial circle via center + endpoints, three points, or tangent continuation. Essential for manual fillets and rounded transitions.
Regular 3–64 sided polygon, inscribed or circumscribed. Useful for hex standoffs, knobs, and nut profiles.
Free-form curve through control points. Hard to constrain and manufacture — reserve for organic shapes and cam profiles.
Two semicircles connected by tangent lines. Common for adjustment slots in motor mounts and bearing blocks.
Reference-only geometry (dashed lines) for symmetry lines, layout guides, and constraint anchors.
X key. Construction geometry is invisible to Extrude but invaluable for organizing sketches.
Geometric constraints define relationships between entities without exact numbers. Two lines constrained as parallel stay parallel no matter how the sketch resizes.
| Constraint | Symbol | What It Does | When to Use |
|---|---|---|---|
| Coincident | Point-on-point | Forces two points (or a point and a line) to share the same location. | Connecting endpoints of separate lines; anchoring geometry to the origin. |
| Concentric | Two rings | Forces two arcs or circles to share the same center point. | Aligning a bolt hole with a counterbore; nesting bearing seats. |
| Parallel | ∥ | Forces two lines to remain parallel (same direction, any distance apart). | Opposite edges of a bracket; rail guides; slot walls. |
| Perpendicular | ⊥ | Forces two lines to meet at exactly 90°. | Corner joints; T-intersections; mounting flanges. |
| Tangent | Curve kiss | Forces a line and an arc (or two arcs) to meet smoothly with no kink. | Rounded transitions; cam profiles; fillet-like geometry. |
| Equal | = | Forces two entities to have the same size (length for lines, radius for arcs). | Symmetric bolt patterns; matched features; uniform spacing. |
| Horizontal | — | Forces a line (or two points) to be aligned with the sketch X-axis. | Top/bottom edges; flat surfaces; alignment references. |
| Vertical | | | Forces a line (or two points) to be aligned with the sketch Y-axis. | Side edges; uprights; vertical alignment of features. |
| Midpoint | Mid marker | Forces a point to lie exactly at the midpoint of a line or arc. | Centering geometry; placing holes at the middle of edges. |
| Symmetric | Mirror line | Forces two points or entities to be mirror images about a construction line. | Symmetric brackets; centered cutouts; balanced designs. |
Dimensional constraints define sizes and positions with explicit values. Combined with geometric constraints, they fully lock down a sketch.
Sets exact length of a line or distance between points/lines. The most common dimension type.
50 mm25 mm10 mmSets the angle between two lines or an arc's sweep, in degrees.
45°90°30°Sets the radius of a circle or arc. Preferred when center-to-edge distance matters (e.g., shaft clearance).
R3 mmR11 mmR2 mmSets full diameter. Preferred for holes and shafts since standard sizes use diameters (e.g., M5 = 5 mm).
∅5.5 mm∅8 mm∅22 mmCAD tools use color coding to show sketch constraint status at a glance. Learning these colors saves debugging time.
| Color | Status | What It Means | What to Do |
|---|---|---|---|
| Blue | Under-constrained | The geometry still has degrees of freedom — it can be dragged or resized. Some constraints or dimensions are missing. | Add more constraints and/or dimensions until the entity turns black. Try dragging the blue geometry to see which direction it moves freely. |
| Black | Fully constrained | The geometry is completely locked down. It cannot move in any direction. This is the ideal state for every sketch. | Nothing — this is your goal. The sketch is ready for feature operations like Extrude or Revolve. |
| Red | Over-constrained | Conflicting constraints or redundant dimensions have been applied. The solver cannot satisfy all rules simultaneously. | Delete the most recently added constraint or dimension. Check for redundant rules (e.g., a Horizontal constraint on a line that is already dimensioned at 0°). |
| Green / Dashed | Construction geometry | Reference-only lines, circles, or arcs that will not be used as profile edges by features. | Use construction geometry for symmetry lines, layout guides, and angular references. Toggle with the X key in most CAD tools. |
(0, 0) with a Coincident constraint to lock the sketch's position.Follow this process for every new feature to ensure consistent, predictable sketches.
Choose an origin plane (XY, XZ, YZ) or an existing flat face. This determines your sketch orientation.
Enter sketch mode. The view rotates to face the plane and the grid appears.
Draw the profile using Line, Rectangle, Circle, Arc, etc. Start from the origin; exact sizes come from dimensions later.
Apply constraints to define relationships. Verify auto-inferred constraints and add missing ones.
Set exact lengths, distances, angles, and radii. Dimension from the origin and watch the sketch turn from blue to black.
Verify all geometry is black (fully constrained) and forms a closed loop, then exit sketch mode.
Apply a 3D operation — Extrude, Revolve, Sweep, or Loft — to turn your constrained sketch into solid geometry.
Design a sketch for a motor mounting plate: a rectangle with 4 corner bolt holes and a center bore for the motor shaft.