Sketching¶

Sketches are constrained 2D profiles that drive 3D features. Start one on an origin plane (XY, XZ, YZ) or on an existing face; a sketch placed on a face re-resolves its plane on rebuild, so it follows the geometry it was drawn on.

A sketch sees the model as it stood where the sketch sits in the history. Opening one rolls the part back to that point for as long as you edit: everything before it is shown, everything after is hidden, and the part rebuilds when you leave. That keeps an early sketch workable in a deep model, and it is why a sketch can never reference the result of a feature it drives.

Drawing tools¶

• Line, rectangle, circle, arc (3-point and center-based), point and polygon (in the Circle dropdown: pick an edge count, place a circumscribed regular polygon). A polygon comes with a construction circle through its corners; its centre behaves like any circle centre, so start the polygon on the origin — or dimension that centre later — to locate it. What is left free is then just the rotation.
• Spline (in the Line dropdown). Click a series of points and the curve passes smoothly through each; finish with a double-click, by clicking the last point again, or by closing the loop near the start. Right-click cancels. Splines are fixed curves for now: the points are set when you draw them and cannot be dragged afterwards. They are real edges, so they close profiles for extrude and revolve and their endpoints snap to and weld with neighbours, but trim, offset, fillet and chamfer do not work on them yet. Patterns do.
• Slot in the standard modes: center-to-center, overall, center-point, 3-point arc and center-point arc. Slots are stored as constrained line and arc geometry, so they work with profiles, trim, offset and patterns.
• Project turns solid edges and faces into associative sketch geometry, and Intersect sections the part with the sketch plane. See below.

Rectangles enter the solver as a full constraint bundle (corner coincidences, opposite-side equality, adjacent perpendicularity, horizontal/vertical locks) rather than four loose lines. Slots get the same, with tangency at every line/arc junction, and sketch fillets and chamfers constrain the corner they cut. Dragging any of them moves the shape instead of distorting it.

Projected geometry¶

Project is the equivalent of a project / convert-entities tool.

1. Open a sketch, then click Project in the toolbar (enabled only while a sketch is active).
2. Leave the panel in Project mode, or switch to Intersect.
3. Click body edges and faces in the viewport to queue them; picking a face queues its boundary edges. The panel counts what is queued and previews the curves on the sketch plane.
4. Tick Construction geometry to add them as construction, excluded from profiles.
5. Project creates the curves, Cancel discards the queue.

Projected curves are associative and follow the source body as it changes, whether or not the sketch feeds a downstream feature. Edges that cannot be projected onto the sketch plane (a circle seen edge-on, a spline) are skipped and reported rather than approximated. You can also project from another part in the same assembly: the source geometry is brought into the active sketch's frame through the two parts' relative placement, so the curves land where the neighbour sits and follow it if it moves.

Within one part, "the source body" means the body as it stood where the sketch sits in the history. A chamfer added at the end of the tree never moves geometry projected into an earlier sketch, and only geometry that exists at that point can be picked at all.

Projecting a face ties the curves to that face rather than to the edges it had at the time. Cut a hole through the face, before the sketch, and its circle appears; remove the hole and the circle goes. Curves that survive keep their identity, so constraints drawn against them keep working.

Because a projected curve is driven by its source, its dimensions are reference dimensions: they read the current size and cannot be made driving. Dimension the source geometry instead and the projection follows.

If a source edge can no longer be found (it was filleted away, or you resized the source drastically in one step), the curve keeps its last shape and the feature using the sketch reports a warning, so a projection never stops following its source quietly. Re-pick the geometry or use Repair Projection Link.

Intersect mode adds the cross-section outline where the sketch plane cuts the part. Unlike Project these curves are static: a one-time snapshot that does not follow later edits.

To detach a projected curve, select it and run Break Projection Link from the command palette; it freezes where it is and is drawn dashed. Repair Projection Link re-attaches it.

Typed dimensions¶

Dimensionable tools accept typed values on the active in-viewport label:

• Type a number or an expression after placing the first anchor point.
• Tab advances through multi-field tools such as rectangles, slots and arcs.
• Enter commits.
• Zero, a negative value or an expression that does not resolve is refused with a short notification saying why, rather than silently doing nothing.

Every dimensionable element gets a sketch-local alias (d1, d2, ...). While a dimension value is being entered, click another label to insert its alias into the equation, so dimensions can reference each other. Double-click a label to edit its value, which promotes a reference dimension to a driving one. Single-click selects it and floats a small toolbar to toggle between an enforcing dimension and a greyed-out reference readout that tracks the solved geometry, and to delete a driving dimension. Delete / Backspace also removes the selected dimension.

Constraints¶

Authoring is dimension-first: the primary toolbar action starts a distance dimension and the less common types live in the dropdown beside it. Available are distance, perpendicular, tangent, equal, midpoint, radius, diameter, angle, symmetric, coincident, concentric, collinear and point-on-curve. Adding a diameter releases the circle's auto radius so the two do not over-constrain each other. Symmetric asks for its mirror axis after the two points: the sketch's X axis or Y axis, or Line and any straight line in the sketch (a construction line makes a good axis).

Selecting one or two elements floats the applicable one-click constraints next to them: two lines offer parallel, perpendicular, equal and collinear, a line and a curve offer tangent, two curves offer concentric, equal and tangent, a single line offers horizontal and vertical. Each button reflects the current state, so a filled one removes the constraint and an outlined one adds it.

While you draw, N3XD infers and previews constraints (parallel, colinear, perpendicular, tangent) with transient glyphs and snapping, committing them when the relationship is well defined. Hold Alt to suppress that for a segment and place a line at a free angle; endpoint welds to the origin and to existing points still apply. Auto-inferred constraints render dimmer than the ones you add by hand, and the Constraints toolbar toggle shows or hides the indicators globally.

Every line carries its own length dimension, which would leave a closed shape describing the same size twice: a rectangle's opposite sides are equal, so four lengths say what two do. The surplus ones quietly become reference dimensions, keeping their name and their live readout but no longer driving the geometry. A rectangle drawn with snapping ends up fully constrained with nothing to fix.

The geometry signals its state per element: an edge still free to move keeps the accent colour, a fully constrained one turns to the dark ink tone, so you can see which elements still need work. A fully constrained sketch is all ink; an over-constrained one turns red, with the conflicting or redundant constraints highlighted on their indicators.

The sidebar's Status section counts the same thing over whatever you have selected: a sketch's own remaining degrees of freedom ("Sketch 3 DOF"), a part's accumulated total ("Sketches 12 DOF"), or the whole project with nothing selected. An assembly switches to a different quantity, how freely its parts can still move ("Assembly 6 DOF"), which is what mates take away. It reads "Constrained" once nothing is free to move, "Over-constrained" if any sketch in scope conflicts.

If a dimension edit or a new constraint would conflict, a message names the constraint it clashes with, highlights it, and offers to Release that dimension (make it a reference) or Delete it and then apply your change. The dimension tool stays available while the sketch is over-constrained. A dimension the sketch already defines is not a conflict: it is stored as a reference dimension so you still get the number. Remaining redundancy is listed once per constraint that has to give, not once per constraint involved, and a dimension row there offers Make reference beside delete.

When picking constraint targets, a vertex, endpoint or centre always wins over an edge or axis passing nearby, so points stay reachable. The sketch origin is a small marker at (0, 0): make a corner coincident with it to ground the sketch, so editing a dimension or fillet moves only the geometry that should change instead of translating the whole profile.

Dragging geometry¶

Grab a vertex (a line endpoint, a circle or arc centre, an arc endpoint, a free point, a spline endpoint) and drag: the point follows the cursor while the solver pulls the constrained geometry along live, so you can reshape an under-constrained sketch by hand. Arc endpoints slide along the arc at fixed radius, so dragging one sets its angle. To resize a circle or arc, select it and drag the round radius handle on its edge. Dragging an element's body moves the whole element, or the whole selection if you grabbed a selected one, with no need to select first.

Fixed points and driving dimensions hold, so a drag moves only what is free: dragging one corner of a partly constrained rectangle stretches the connected edges while the grounded corner stays put. Hold Ctrl (or Cmd) to box-select instead of moving. Dragging snaps to nearby geometry just like drawing, and releasing commits one undo step.

Editing tools¶

• Trim splits at detected intersections.
• Offset creates associative offsets of closed loops and chains.
• Fillet and chamfer round or bevel sketch corners.
• Mirror reflects selected elements across an axis line, typically construction geometry. The copies are associative: editing a source or moving the axis re-reflects them.
• Pattern creates persistent sketch patterns with constraint remap.
• Selecting two or more colinear lines surfaces a Merge action.

Construction geometry gets the same dimension labels as regular geometry but is excluded from 3D features and profile generation.

Recompute¶

While you edit a sketch the downstream 3D model is held frozen, so each edit stays instant even on large parts; a change to an early sketch would otherwise rebuild the whole feature chain on every tweak. Your edits are saved immediately, only the derived geometry waits. Exiting the sketch (Exit Sketch or Esc) rebuilds the part in the background.

Selecting regions¶

Region clicks are additive, so you can pick several closed profiles without a modifier. Which area a click hits is resolved from the region outlines themselves, so even a very small area is picked exactly and two are never toggled at once. Clicking inside a region toggles that area; clicking within a narrow band along its outline grabs the region plus any areas nested inside it (extrude and rib only, which is how you fill a hole by selecting the plate and the area inside it together). The extrude and revolve panels also have Select all and Clear.

Adding a new loop to a sketch a feature already uses does not change that feature's body: a circle drawn inside an already-extruded rectangle is absorbed into the solid, not punched as a hole. To make it a hole, edit the feature and deselect it in the region picker. This keeps downstream features from breaking when you extend a sketch for a later operation.

See Modeling features for turning a profile into a solid.