Sketching¶

Sketches are constrained 2D profiles that you use to create 3D features. Start a sketch on an origin plane (XY, XZ or YZ) or on an existing face. When the model rebuilds, a face-based sketch resolves its plane again, so it continues to follow the geometry it was drawn on.

Each sketch sees the model as it existed at that point in the feature history. While you edit a sketch, N3XD rolls the part back to that point: it shows everything before the sketch and hides everything after it. The part rebuilds when you leave the sketch. This keeps early sketches usable in complex models, and it means a sketch cannot reference the result of a feature that uses it.

Drawing tools¶

The toolbar shows these tools when a sketch is open and nothing is selected. Select one or more elements to show the editing tools. Right-click or press Esc to cancel the active tool. Dragging with the right button pans the view and keeps the tool and the points you have placed.

• Line, rectangle, circle, arc (3-point or center-based), point and polygon. To draw a polygon, open the Circle dropdown, choose the number of sides and place it. A construction circle passes through its corners, and its radius sets the polygon's size. Its centre works like a circle's centre, so place it at the origin or dimension it later to locate the polygon. Only its rotation remains free.
• Spline (in the Line dropdown). Click a series of points to draw a curve that passes smoothly through them. Finish by double-clicking, clicking the last point again or closing the loop near the start. Right-click to cancel. Splines are fixed for now: you cannot drag their points after drawing them. They are real edges, so they can close profiles for extrude and revolve, and their endpoints snap to and join neighbouring geometry. Trim, offset, fillet and chamfer do not work on splines yet, although patterns do.
• Slot in one of five modes: center-to-center, overall, center-point, 3-point arc or center-point arc. N3XD stores slots as constrained lines and arcs, so you can use them in profiles and with 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 with a full set of constraints: matching corners, equal opposite sides, perpendicular adjacent sides, and horizontal and vertical locks. Slots use the same approach, with tangency at each line and arc junction. Sketch fillets and chamfers also constrain the corner they modify. As a result, dragging any of these shapes moves it without distorting it.

Projected geometry¶

Project works like a project or convert-entities tool in other CAD apps.

1. Open a sketch and select Project in the toolbar. This tool is available only while a sketch is active.
2. Keep the panel in Project mode, or switch it to Intersect.
3. Select body edges or faces in the viewport. Selecting a face adds its boundary edges. The panel shows the number of queued edges and previews their 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, so they follow changes to the source body whether or not the sketch feeds a downstream feature. N3XD skips and reports edges it cannot project onto the sketch plane, such as a circle viewed edge-on or a spline, rather than approximating them. You can also project from another part in the same assembly. N3XD transforms the source geometry into the active sketch's frame using the parts' relative placement, so the curves appear where the other part sits and follow it when it moves.

Within a part, the source body is the body as it existed at the sketch's place in the feature history. For example, a chamfer added later does not change geometry projected into an earlier sketch. You can select only geometry that exists at the sketch's point in the history.

When you project a face, N3XD links the curves to that face rather than to the edges it had when you selected it. For example, if you cut a hole through the face before the sketch, the circle appears in the projection; if you remove the hole, the circle disappears. Curves that remain keep their identity, so constraints that refer to them continue to work.

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 N3XD can no longer find a source edge, for example because a fillet removed it or the source changed drastically, the curve keeps its last shape and the feature using the sketch shows a warning. This makes a broken link visible. Select the geometry again or use Repair Projection Link.

Intersect mode adds the outline where the sketch plane cuts through the part. Unlike projected curves, intersected curves are static: they capture the current shape and do not follow later edits.

To detach a projected curve, select it and run Break Projection Link from the command palette. N3XD freezes the curve in place and draws it dashed. Use Repair Projection Link to re-attach it.

Typed dimensions¶

For dimensionable tools, enter values in the active label in the viewport:

• 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 rejected. A notification explains why.

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. Typing into a greyed-out readout that another dimension already determines moves the change onto that dimension, so the shape resizes the way you meant instead of reporting a conflict. A rectangle's top and left follow bottom and right, and a square's sides all follow one size, so a number or an expression typed on any of them resizes the shape. A polygon's side length follows its circumcircle, which takes a number typed on the side. When several dimensions determine a readout together, such as a rectangle's diagonal, the edit is refused and the notification names them. Dimensioning a line's length or a radius that already has a dimension edits that dimension, so a size never carries two. A new dimension placed on a size that another dimension determines works like the readouts above: it stays a greyed-out readout and moves the dimension that sets the size. Delete / Backspace also removes the selected dimension.

Constraints¶

The constraint group appears once the sketch contains geometry. The toolbar puts distance dimensions first; less common constraint types are in the adjacent dropdown. You can add distance, perpendicular, tangent, equal, midpoint, radius, diameter, angle, symmetric, coincident, concentric, collinear and point-on-curve constraints. Radius, diameter, equal and concentric take circles and arcs picked anywhere on the curve. Adding a diameter releases the circle's automatic radius constraint, so the two dimensions do not over-constrain it. For a symmetric constraint, choose the mirror axis after selecting the two points: the sketch's X axis, Y axis or Line. For Line, select any straight line in the sketch; a construction line works well.

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.

As you draw, N3XD previews inferred constraints such as parallel, collinear, perpendicular and tangent with temporary glyphs and snapping. It commits a constraint when the relationship is clear. Hold Alt to suppress inference for a segment and draw a line at a free angle; endpoint connections to the origin and existing points still apply. Automatically inferred constraints appear dimmer than constraints you add yourself. Use the Constraints toolbar toggle to show or hide all indicators.

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 reports the remaining degrees of freedom for your selection. For a sketch, it shows the sketch's remaining freedom (for example, "Sketch 3 DOF"). For a part, it adds the freedom across its sketches ("Sketches 12 DOF"). With nothing selected, it reports the whole project. For an assembly, it reports how freely the parts can move ("Assembly 6 DOF"), which is the freedom that mates remove. The status reads "Constrained" when nothing can move freely, or "Over-constrained" when any sketch in scope has conflicting constraints.

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. Release names the dimension whose release would actually let your change through, even when it is not one the solver reported as failing. 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¶

Drag a vertex (such as a line endpoint, circle or arc centre, arc endpoint, free point or spline endpoint) to move it. The solver updates connected, constrained geometry as you drag, so you can reshape an under-constrained sketch by hand. Arc endpoints slide along the arc at a fixed radius, so dragging one changes its angle. To resize a circle or arc, select it and drag the round radius handle on its edge. You can also drag an element's body to move the whole element. If the element is already selected, dragging it moves the whole selection; you do not need to select it first.

Fixed points and driving dimensions stay in place, so dragging moves only the unconstrained geometry. For example, dragging one corner of a partly constrained rectangle stretches its connected edges while the grounded corner stays put. Hold Ctrl (or Cmd) to box-select instead of moving geometry. As when drawing, the cursor snaps to nearby geometry. Releasing the mouse commits one undo step.

Editing tools¶

Select one or more sketch elements to use these tools. Offset, mirror, fillet, chamfer and pattern replace the drawing tools in the toolbar. Trim and Merge appear directly on the selected geometry.

• Trim: select one element that another one crosses and scissors appear on it at each cut. Click one to drop that piece.
• Offset creates associative offsets of closed loops and chains. The copies follow their sources, and a constraint or dimension on a copy acts on the sources too, so a frame welded onto an offset outline moves the outline it was offset from.
• 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. They take their size from the sources, so they show no dimension of their own and add no degrees of freedom. A length or radius you place on a copy is applied to its source. Any other constraint or dimension on a copy acts on its source too, so a width across the axis, a weld from other geometry to a copy or a dimension from a copy to the origin moves the source. Welding a source point to its own reflection keeps that point on the axis, where it can still slide.
• Pattern creates persistent linear or circular sketch patterns. The copies follow their sources like mirror copies do, so resizing a source resizes every copy, and a constraint on a copy acts on its source. Open the arrow beside the button to switch kinds. A negative spacing or angle reverses the direction. A dimension between a source and its copy, or between two copies, follows from the pattern, so change the spacing or angle to change it. Editing the count or spacing keeps the copies that remain, with whatever is built on them. Lowering the count removes the last copies, and a mirror or offset made from one of them becomes independent geometry.
• A copy can be mirrored, offset or patterned again, and the whole chain follows the original source.
• 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, N3XD keeps the downstream 3D model frozen. This keeps edits responsive even on large parts, where changing an early sketch would otherwise rebuild the entire feature chain after every adjustment. Your sketch edits are saved immediately, while the derived geometry waits. When you exit with Exit Sketch or Esc, N3XD rebuilds the part in the background.

Selecting regions¶

Region selection is additive, so you can select several closed profiles without holding a modifier key. N3XD uses the region outlines to resolve each click, so it can select small regions precisely and never toggles two at once. Click inside a region to toggle it. For extrude and rib, click the narrow band along its outline to select the region and any nested regions. This lets you fill a hole by selecting both the plate and the area inside it. The extrude and revolve panels also include Select all and Clear buttons.

Adding a loop to a sketch that an existing feature already uses does not change that feature's body. For example, a circle drawn inside an extruded rectangle becomes part of the solid; it does not cut a hole. To create a hole, edit the feature and deselect the circle in the region picker. This behavior lets you extend a sketch for a later operation without breaking downstream features.

See Modeling features for turning a profile into a solid.