From 3D planes and sketches to associative solids

01 · MODEL ORIGIN

Three permanent reference planes

Every project owns stable Top (XY), Front (XZ), and Right (YZ) planes. They meet at the model origin and cannot be deleted. Select a plane in the viewport or in 3D Objects, then use the eye control to keep the scene as quiet as needed.

The coloured X, Y, and Z triad shows the world axes. Millimetres remain the exact model unit.

02 · CONSTRUCTION

Choose a construction plane type

Choose Plane in the dedicated 3D tool rail. Cadivari reveals existing reference planes and highlights supported planar solid faces, including base-extrusion faces, terminal Join caps, Cut floors and ceilings, straight planar modifier walls, stored Loft Start/End caps, and genuinely flat side panels of polygonal Lofts. Adjacent coplanar Loft mesh strips are merged into one semantic face, so selection follows the modeled panel rather than an individual renderer triangle. The compact task card beneath the camera controls offers four exact workflows while the object tree and ordinary Properties panel remain visible. A fixed key beside the tool rail identifies the red X, green Y, and blue Z origin lines without placing camera-facing labels over the model.

Offset uses one plane or planar face plus an exact positive or negative millimetre distance. A face-based plane begins directly on the chosen face at 0 mm; enter an exact offset afterward or click the gold normal arrow or anywhere on the draft plane to grab it, move along the normal, then click again to place the rough offset. Movement snaps to 1 mm; hold Shift for 0.1 mm increments. Crossing the reference reverses the signed offset and arrow. The Offset label provides the same adjustment directly in the task card: drag left or right for 1 mm changes and hold Shift for 0.1 mm changes. Exact typed entry remains available, and Escape during label scrubbing restores the starting value. Create plane is still the final model commit.

Midplane uses two parallel planes or planar faces and stays halfway between them as either reference changes. Angled rotates one plane or planar face by an exact degree value about its local U or V axis. Angled and Edge plane Angle labels can also be scrubbed in 1 degree increments, or 0.1 degree while holding Shift. Edge highlights stable straight extrusion edges; selecting one uses that exact start-cap, end-cap, or rail edge as the hinge for an editable rotation angle. Every type supports a reversible normal and remains editable after creation.

Planes made from supported extrusion, modifier, Loft faces, and straight extrusion edges retain semantic feature-and-face or feature-and-edge references. Changing the source sketch, feature dimensions, Loft section plane, feature direction, or another upstream plane therefore rebuilds the construction plane from current geometry. Chained plane relationships remain associative through save and open.

03 · PLANE-LOCAL DRAWING

Sketch and 3D are two views of one model

Choose Sketch, then click either a visible reference plane or a highlighted planar face on a solid. Supported faces include base-extrusion caps and sides, uniquely identifiable planar faces after direct Push/Pull and sketch Join/Cut, remaining planar faces after compatible finishing, Loft caps, and genuinely flat polygonal Loft side panels. Cadivari respects the global Planes control and every plane's individual eye state during this step. A hidden plane remains available from the Reference planes list without being made visible in the viewport. Cadivari reuses an existing linked sketch when possible, aligns the camera, centres the plane-local origin in the drawing viewport, and opens the exact drawing tools. Rectangle, Line, Circle, Arc, Spline, Mirror, Measure, Text, Move, Offset, and Combine continue to work in millimetres; their coordinates are local to the active plane or face. Choosing a drawing tool while in 3D also starts the same plane-or-face selection step.

A sketch created directly on a face receives dashed teal projected edges automatically. These edges remain associated with the selected solid face and rebuild when its source sketch, plane, extrusion, modifier, or Loft section changes. They provide visible snap points but remain reference-only: they are excluded from editable Objects, closed-profile detection, drawing export, and CAM until the user draws ordinary sketch geometry from them.

When a sketch is attached to an edited solid, its face reference records the history stage at which it was picked. Earlier changes move the attachment and its projected edges. Later operations made from that sketch do not move its own support or create a circular dependency. Cadivari reports a missing or ambiguous reference if the intended face can no longer be identified.

The compact References control also exposes drawing context from other sketch planes. Parallel sketches appear as subdued projected outlines, while a visible non-parallel closed profile appears as its true dashed teal intersection with the active plane, including snap points at both boundary crossings. This makes a perpendicular Loft rail sketch show exactly where each section starts and ends. Previous shows all intersections plus the nearest earlier parallel sketch, All adds every earlier parallel sketch, and Off hides all of these references. They rebuild live but remain non-editable and do not enter profile recognition, exports, solids, or CAM.

Choose 3D to leave the aligned editor and inspect the sketch. Double-click a plane to reopen its latest sketch, or use the Sketches group to choose a specific saved sketch. Non-parallel geometry is represented only by its exact plane intersection, preventing misleading flattened shapes or cross-plane path joins.

04 · FEATURE INPUT

Closed faces are recognized automatically

Sketch mode stays focused on drawing and editing geometry. When you return to 3D and activate Push/Pull, hovering identifies the smallest closed face under the pointer. A directly contained boundary becomes a hole, so a rectangle with an inner circle resolves as one extrudable face with one hole; the inner disk remains a separately selectable face.

05 · ASSOCIATIVE SOLID

Sketch extrusions and repeated face edits

Return to 3D and choose Push/Pull. Choose New body, Join or Cut in its task card before grabbing a closed sketch face. Click to grab, move to inspect the preview, then click to place it. Alternatively, type a signed millimetre distance and press Enter. Escape cancels the preview.

New body creates a separate solid. Join adds connected material to a selected target; Cut removes it. New sketch Join/Cut operations use 3D solid Booleans, so the sketch can face the top, side or another orientation instead of having to be parallel to the base extrusion. Sketches attached to a body face suggest that body as the target, with an outward Join or inward Cut direction. For independent construction-plane sketches, choose the target explicitly. Detached Joins, operations that make no change and invalid solids are rejected.

After grabbing a sketch face, Extent offers Distance, Through all for Cut, or Up to face. Through all recalculates the cut length from the target body. Up to face stops at the supporting plane of a selected parallel planar face; it does not trim the profile to the face's outline. Select a stored extrusion to change its extent in the inspector. Adaptive extents follow upstream geometry instead of keeping a fixed typed length.

To edit a solid directly, hide any covering source sketch and select a supported planar solid face with Push/Pull. Pull outward to add material or push inward to remove it. Repeat on the same face or another supported face; each placement stores another Face Push/Pull feature. Sketches remain editable and can be created on the resulting planar faces. A covered visible sketch profile takes selection priority over the underlying solid.

06 · ASSOCIATIVE LOFT

Shape a capped body through an ordered section stack

Choose Loft in the 3D tool rail, then click from two to twelve visible closed sketch faces in the order the surface should follow. The first face is Start, the last is End, and every face between them is an intermediate section. The viewport keeps persistent numbered highlights and displays one translucent capped surface. Use the row arrows for local reordering, click a selected numbered face or its remove control to take it out, or reverse the complete order without moving geometry.

Automatic seams are the correct default for ordinary aligned sections. If a mixed or rotated stack visibly twists, adjust only the affected section's Seam slider. Its normalized boundary offset updates the surface, marker, seam, correspondence lines, and diagnostics live. Reset restores that section to Auto.

Endpoint tangency independently controls how the Loft leaves Start and enters End. None preserves the established linear span. Normal follows that endpoint sketch plane's normal with an adjustable 10–100% Influence, which is useful when the surface should begin or finish perpendicular to a section rather than immediately aim at the next profile. Reverse order swaps both endpoint definitions with the section stack. These controls do not alter the source sketches.

Guide rails use ordinary sketch geometry. First draw an open Line, Arc, Spline, or connected mixed chain in a normal perpendicular or side sketch. Return to 3D, prepare the Loft sections, turn Use guide rails On, and choose Select guide rails. Click an existing chain to add it; the whole connected component highlights in teal and receives a numbered marker. Click it again to remove it, press Enter or Escape to finish selection, or turn the control Off to compare the unguided surface without discarding the selected paths. Guided surfaces add longitudinal stations adaptively around tight rail curvature, smoothing close-radius bends without unnecessarily densifying straight spans.

Each enabled rail must cross and touch every ordered section boundary exactly once. Valid rails disable the manual seam controls and deform intermediate surface sections along their sampled curvature. Up to eight rails can be selected to control different areas around the profile. When endpoint tangency is also active, each exact guide intersection remains authoritative at the boundary. A missing or repeated crossing, branching or self-crossing path, or boundary miss blocks creation with a direct diagnostic.

Sections must progress consistently through space from Start to End. An order such as middle → bottom → top would make one span retrace another, so Cadivari blocks it instead of displaying a misleading overlapping solid. Bottom → middle → top and its complete reverse are both valid.

Matching low-complexity polygons align actual corners. Polygons with different corner counts map their real corners onto a shared anchor topology; a square-to-triangle Loft collapses one square edge into the unmatched triangle corner. Mixed and curved profiles use a common radial-seam convention and even arc-length resampling without changing editable source geometry. The compact card summarizes section count, spacing, plane angle, winding, correspondence mode, surface rule, sample count, and side-face count. A safe green result enables Create Loft body.

The committed Loft v5 stores ordered profile references, seam offsets, Start/End tangency modes and influences, and enabled guide-path references rather than renderer triangles. Editing a source curve, guide path, or reference plane rebuilds the body. Select a stored Loft in 3D Objects to inspect its definition or reopen every linked section and guide sketch. Older Loft v1/v2/v3/v4 project data remains readable.

Choose Sketch or Plane and click either terminal Loft cap or a genuinely flat polygonal side panel. A selected face creates an associative 0 mm face plane and can receive an exact offset afterward. Flat side panels remain linked as the Loft sections change; curved side surfaces remain intentionally unavailable.

LOFT DISPLAY

Selection without hiding the surface

A committed Loft keeps its muted green material while idle. Hovering adds a restrained warm cue, and selecting the body applies a subtle olive-amber surface wash with stronger gold terminal-profile edges. Hovering an active Loft raises that cue slightly. Click empty viewport space with Select active to clear the selection and return the body to its idle material. This follows Cadivari's active-object language without replacing the smooth shading that communicates the Loft's form.

07 · ASSOCIATIVE REVOLVE

Turn one profile around a straight sketch axis

Draw one closed outer profile, any contained closed profiles that should become holes, and one straight Line in the same sketch. Return to 3D, choose Revolve, click the material face, then click the Line. Cadivari treats the complete line as an infinite axis and automatically carries nested boundaries through the revolution. Enter an exact sweep angle from greater than 0 to 360 degrees, set the Start angle, then choose Positive or Negative direction. Symmetric direction relabels this orientation as Centre angle. The viewport shows a subtle 0-degree reference, the active radial direction, and an angle arc. Full rotations close around the axis; partial rotations receive planar start and end caps around every hole. The profile may end on the axis, as a bowl or spindle section often does, but it cannot cross through it.

Choose New body to create a separate solid, or choose Join and explicitly select an eligible prismatic Extrude body. Join highlights the target, requires the Revolve to contact it and extend beyond its existing volume, and appends the Revolve to that body's ordered associative history. Detached profiles and revolutions contained entirely inside the target remain blocked. The stored definition retains the linked face boundaries, exact line axis, sweep angle, start angle, direction, operation, and target relationship rather than renderer triangles. Select the committed feature to restore its orientation guides, inspect its definition, reopen the linked sketch, or delete only the joined feature. Changing any linked outer or inner boundary rebuilds the result. The verified workflow covers full and partial sweeps, symmetric orientation, nested holes, linked edits, multiple candidate targets, ordered prismatic modifiers, and save/open.

08 · ASSOCIATIVE CHAMFER

Bevel an edge on the current solid

On an Extrude-based body with face edits or additional features, choose Chamfer, click one continuous straight convex edge between planar faces, enter an equal Distance and choose Apply Chamfer. Select the saved feature to edit its distance. It can follow compatible sketch extrusions, face edits and finishing features, and can be followed by further modelling operations.

A clean Extrude retains the existing multi-edge, loop and circular-rim controls, including Equal distance, supported Distance + angle, and Miter or Blend where applicable. These broader selection controls are specific to the clean prismatic workflow. The current-solid workflow selects one straight convex edge per feature.

Collapsed faces, ambiguous references and bevels that break into unrelated walls are rejected. See 3D Chamfer for both workflows and their exact limits.

09 · ASSOCIATIVE 3D FILLET

Round an edge with an editable radius

On a supported edited Extrude-based body, choose Fillet, select one continuous straight convex edge between planar faces, enter Radius and choose Apply Fillet. The saved radius and face references rebuild in history; later sketches and face edits remain possible on supported flat faces.

A clean Extrude retains its existing Edge, Tangent, Loop and All scopes, partial multi-edge selection and bounded radius slider. General curved or concave edge Fillets are not enabled. A radius that consumes a face or breaks into an unrelated pocket or Shell wall is blocked. Create Shell before Fillet when the Shell would otherwise need to offset rounded surfaces.

See 3D Fillet for selection, editing and collision feedback.

10 · ASSOCIATIVE SHELL

Open a face and form inward walls

On an edited Extrude-based body, Shell accepts one connected convex solid made entirely of identifiable planar faces. Choose Shell, click the face to remove, enter Thickness and choose Apply Shell. The opening can be a supported top, bottom or side face. Other face planes offset inward to form one cavity.

This works after direct resizing or a compatible Chamfer while the solid remains convex and planar. Apply it before pockets, holes or Fillets; these can follow Shell as later features. A subsequent direct wall edit changes that wall independently of the stored Shell thickness.

Clean Extrudes retain their original terminal-cap Shell workflow, including supported source-profile holes. The guarded full-360-degree Revolve workflow also remains available for a flat axial terminal cap and suitable source walls. General concave or curved Shells, multiple removed faces, partial-Revolve Shells and Loft Shells remain unsupported.

Select a current-solid Shell to edit its Thickness; clean Extrude and Revolve Shells retain Edit opening and thickness. See Shell for examples, history behaviour and body requirements.

11 · VIEWPORT APPEARANCE

Read solid form without entering a render mode

Open Display beside the camera controls. Shaded shows clean studio-lit surfaces, while Shaded with edges adds smooth 1.5 px near-black CAD feature boundaries without adding silhouette geometry or changing the lighting pipeline. Matte, Plastic, and satin Metal change roughness, clear coat, and reflection response. Visual style and surface finish remain independent.

The studio environment is generated locally and remains available offline. Neutral tone mapping, normal-buffer screen-space ambient occlusion, 4× multisampling, Ultra SMAA, and a restrained key/fill setup help Chamfers, Fillets, Revolves, Lofts, Shell interiors, touching surfaces, and curved outlines read clearly. Reference planes use neutral low-opacity surfaces and subdued orientation grids so they remain legible without overwhelming sketches or solids. Revolves also use denser display tessellation with crease-aware normals. Selection gold, live previews, face and edge picking, and invalid-geometry colors continue to override the decorative finish.

12 · CAMERA

Inspect the model from predictable views

Use the Planes control to hide or reveal all reference planes without changing their individual visibility settings. Sketch and Plane selection both preserve that global choice and each plane's individual eye state; hidden planes can still be selected from the right panel. Planar solid faces remain available directly in the viewport. Use Top, Front, Right, or ISO in the viewport toolbar; each preset also reframes the model. Drag with the middle mouse button to orbit. Hold Shift while middle-dragging, or right-drag, to pan. Use the wheel to zoom. These camera gestures also work during sketch and solid-face Push/Pull previews: sizing pauses during navigation, then resumes from the current distance in the new view.

CURRENT ITERATION

Supported modelling workflows

Extrude-based modelling now combines repeated planar Push/Pull, face-attached sketches and projections, sketch Join/Cut in arbitrary orientations, Distance/Through all/Up to face extents, and compatible Chamfer, Fillet and Shell features. Up to face currently requires a parallel planar target. Direct face editing requires a uniquely identifiable connected planar face; it does not turn individual triangles on a curved surface into editable flat faces. Finishing on edited bodies supports straight convex edges between flat faces, and Shell requires a convex planar body at the moment it is applied. Existing specialized clean Extrude finishing and guarded full-Revolve Shell workflows remain available.

Loft supports two to twelve ordered profiles, stored seams, endpoint plane-normal tangency and up to eight associative guide rails. Revolve supports full and capped partial rotations with nested holes and a same-sketch straight axis; guarded Revolve Join targets eligible prismatic bodies. Those workflows retain their separate validation and references.

General curved-face offsets, curved-edge finishing, ambiguous or disconnected face references, direct editing of Loft/Revolve/Split Body results, Loft holes or Join/Cut, Revolve Cut, general concave or curved Shells, and multi-face Shell openings remain outside this update. Each operation validates its result and reports unsupported or missing references. Reference planes, projections and solid display meshes do not enter ordinary SVG/PDF drawing output or create CAM operations automatically.