Modeling features¶

Features are the operations that make up a part's history. This guide groups them by the input they need. The toolbar follows your selection, so selecting a body, face or edge shows the tools available for it. Each section below tells you what to select first. The F1 command palette contains every feature except Rib and Thread, regardless of your selection. Most features also show a live, semi-transparent preview before you apply them.

Sketch-based features¶

These features use one or more closed sketch profiles, and they appear when you select a body. Extrude requires at least one sketch in the part. Revolve and Helix require a sketch selected in the tree whose geometry closes a region. Loft and Sweep each require two sketches.

• Extrude a profile into a solid in one direction, symmetrically or in both directions. You can also choose a Boolean mode (add, cut or intersect). An extrude inside an existing body becomes a pocket automatically. For a cut, N3XD uses the entered distance as its depth and infers the inward direction. Select Through all to remove material through the whole body in the first direction; a second direction still stops at its own distance. Thin wall turns every loop of a closed profile, holes included, into a wall of the given thickness, grown into the profile (Inside), away from it (Outside, with rounded outer corners) or half each way (Both). A circle with a thin wall is a tube. For an open chain use Rib.
• Revolve a profile around an axis (origin axis, selected edge or datum axis), with an angle and boolean mode.
• Helix coils a profile around an axis, for springs, coils or custom threads (use Cut). Sketch the profile beside the axis on a plane that contains it, e.g. a circle on XZ next to the Z axis. Pick the axis as for Revolve, then set two of pitch, turns and height (the third follows from height = pitch × turns). You can also choose the hand, reverse the direction or add a taper angle for a conical spring. Closed ends adds one tightly wound turn at each end, and Ground ends trims both ends flat, like a compression spring. The pitch must exceed the profile's size along the axis, otherwise the coils overlap. Pitch, turns and height describe the active coils. With h = pitch × turns and d the profile's size along the axis (the wire diameter for a round wire), the overall length is h + d with plain ends, h + 3d with closed ends, h with ground ends and h + 2d with both. A ground spring starts flat level with the profile's centre and runs along the axis (against it with Reverse); without grinding, the wire reaches half the profile (d/2) past each end. So to fit a closed and ground spring between two seats a distance L apart, put the profile's centre level with the first seat and set the height to L − 2d. The closed turns sit 0.1 % looser than the wire so they never fuse, which adds 0.002 × d.
• Loft between multiple profiles. The panel shows each profile's regions so you pick one per profile.
• Sweep a profile along a path, both from sketches.
• Rib thickens a sketch profile into a thin support wall and joins it to the part. Draw an open chain to create a wall of the chosen thickness, or select a closed region. The wall grows along the sketch normal on one side, the other side or symmetrically. N3XD sizes and clips it so it does not extend through the far face. A rib needs an existing solid to support.

Primitives¶

Primitive builds a cylinder, tube, sphere or torus without a sketch. It appears when you select a body, and it does not need existing geometry. Place it by two points:

• Cylinder and Tube run from the start point to the end point. A tube has an outer radius and a wall thickness.
• Torus is centred on the start point, and its axis points towards the end point. Set the major and minor radius.
• Sphere is centred on the start point.

Each point is either a picked datum point or typed coordinates, and every coordinate and size accepts an expression. Put hard points such as pivots in parameter-driven datum points and run tubes between them: the tubes follow every parameter change. The Boolean mode works as for Extrude.

Face and edge modifications¶

These features modify existing solid geometry. They are topologically anchored, so N3XD can resolve their references again when the model rebuilds. Select a face for shell, draft, thread, hole, surface pattern or text emboss. Select an edge for fillet or chamfer.

When a tool needs a face (thread, hole, shell or draft), only faces are selectable. For example, click just inside a hole to select its wall or bottom face instead of the rim. Fillet and chamfer work the same way for edges, which makes them easier to select on dense parts: N3XD picks the edge under the cursor instead of the nearest edge in 3D.

• Fillet (edge): constant or variable radius, multi-edge.
• Chamfer (edge): distance, distance-and-angle or edge-length.
• Shell (face): hollow a solid to a wall thickness, optionally removing selected faces.
• Draft (face): a draft angle about a neutral plane.
• Thread (cylindrical faces): a real helical thread, internal or external, with ISO metric / UNC / UNF presets or a custom pitch. Select several faces to thread them all with the same pitch and handedness in one feature; a face already selected when you open the tool is carried in. Set a start and/or end depth to thread only part way down a hole, measured from a planar reference face you pick or from the open end. The smooth section above an internal thread's start is widened to the thread diameter so a bolt can pass through and reach it.
• Hole (planar face): click to place a simple, counterbore or countersink hole. Choose a blind or through-all depth and an ISO clearance or tap-drill size. When editing the hole, drag the on-face X/Y arrows or enter coordinates to reposition it. By default, the hole follows the face normal. Set Direction to use another direction, such as a planar face normal, datum axis, origin axis or edge. For example, you can place a hole on a wedge's slanted face and drill it perpendicular to the base. When you set a direction, N3XD extends the opening opposite the drill so uphill material does not cap it. Back clearance controls this extension: leave it blank for automatic sizing or set it to 0 to turn it off. The depth still controls how far the hole drills inward.
• Surface pattern (face): displace a face with a math function, smooth (fitted B-spline) or faceted.
• Text emboss (face): raise or engrave text with bundled fonts, alignment, rotation and a mirror toggle. Curved faces wrap conformally, with a toast warning that the preview may be slow.

Patterns and decomposition¶

All four are body-level tools, so select the body before choosing one. Linear and circular pattern share one toolbar button. Open the arrow beside it to switch kinds; the button then keeps the kind you picked last.

• Linear pattern: array along one or two directions with count and spacing. A negative spacing reverses that direction.
• Circular pattern: array around an axis with count and total angle. A negative angle turns the other way.
• Mirror: mirror the body about a plane. The operation picker decides what happens where the copy meets the original: a new body (default), add, cut or intersect.
• Split: divide a solid into separate bodies by a plane, choosing which pieces to keep.

Mirror, split and datum planes define their plane the same way and show it in the viewport while you set it up, with a drag handle for the offset.

Datums¶

Datum planes, axes and points are reference features for sketches, patterns, mirrors, splits and mates. Datum appears with the body and face tools, and its menu picks the kind. It does not require an existing solid: the origin-based, point-based and explicit modes also work on an empty part.

• Datum point: a hard point at X, Y, Z in the part frame. Each coordinate accepts a parameter expression, so pivots and pickup points can follow your parameters. Points show as small markers in the viewport.
• Datum plane: offset from a plane, midplane between two parallel planes, through 3 points, at an angle to a plane about an axis, perpendicular to an axis or edge, or origin and angles: the XY plane rotated about X, then Y, then Z, placed at a datum point or at typed coordinates. Flip reverses the normal, and every offset, angle and coordinate accepts expressions.
• Datum axis: two-point, from a cylindrical or conical face, plane intersection, or a reference line.

Wherever a plane or axis takes points, you can pick a datum point instead of typing coordinates, so a kingpin axis through two parametric hard points moves with them. A ball joint or distance mate can also use a datum point, which puts the pivot exactly on that point.

Repairing failed references¶

Face and edge features (fillet, chamfer, shell, draft, thread and surface pattern) store anchors: geometric signatures of the references they use. N3XD resolves these anchors again on every rebuild. If the upstream geometry has changed or been deleted, an edge may no longer exist or several candidates may look too similar. In that case, the feature enters an unresolved reference state and downstream features remain stale.

The feature's edit panel then shows a Repair button. Select it to see each unresolved anchor and its candidate references, ranked and highlighted in the viewport. N3XD preselects the best match and shows it most brightly. Choose the correct reference for each anchor and select Repair; N3XD applies them one at a time, rebuilding between each repair.

Select fix similar elsewhere first to repair the same broken reference in other features too. N3XD reports how many references it fixed when the repair is complete.

If another action rebuilds the model while the panel is open, N3XD refreshes the candidate list. This keeps you from repairing a reference against an outdated model.

Re-applying a warned feature¶

Extrude, revolve, helix, rib, sweep and loft remember which areas of a sketch they use. If you edit the sketch so much that N3XD cannot identify an area with confidence, it builds the feature using the closest match it can find and adds a warning.

Open the feature to see which sketch areas it currently uses. If they are correct, select the enabled Re-apply button, even if you have not changed anything in the panel. N3XD saves the selected areas as new anchors and clears the warning. If the areas are wrong, select the correct ones; the button then changes back to Apply.

N3XD offers Re-apply only when it can help. If a fillet failed, an imported body has open edges, or a sketch has dangling curves, Apply stays disabled because committing again would produce the same result. Fix the geometry, or use Repair or Use best guess when a reference is missing.

Simplified display pin¶

Threads, embossed text, surface patterns and small fillets or chamfers count as detail and are hidden when simplified display is on. Open one of those features to override that with Simplified display:

• Auto: follow the rule (the default).
• Hide: always drop this feature in simplified display, whatever its size.
• Keep: always draw it, for example a functional 1 mm fillet.

The pin only affects display. The feature stays in the model and in every export, measurement and simulation either way.

Deleting features and sketches¶

Deleting is best-effort. Removing a feature deletes only that feature. Removing a sketch also deletes the features built directly from it, because an extrude or revolve cannot exist without its profile. If a downstream feature can no longer compute, N3XD flags it in the tree instead of deleting it. You can then choose to repair or remove it. You can undo deletions.