Fusion Reference — parametric CAD for scale models that print in colour

What Fusion is

and what it is not

Fusion is a tool that models parts as solids — closed volumes with exact faces — from constrained 2D sketches, records every operation in a timeline, and replays that history whenever an earlier step changes. It also carries a surface modeller, a T-spline sculptor (Form), a mesh editor, assemblies with joints, rendering, drawings, CAM and a Python API, all in one document type saved to Autodesk's cloud.

It is not a mesh sculptor (Blender), a code-CAD kernel (OpenSCAD, CadQuery) or a slicer. STL and 3MF are what it exports; it can import them as mesh bodies and, on Personal, convert them faceted only. Think of it as the place where dimensions live; the slicer is where colours and layers live.

Five ideas that carry the rest of the sheet

Sketch → feature → body. A closed sketch loop is a profile; a feature turns profiles into bodies; the body is what you print.
The timeline is the model. Geometry is the result of the features in order. Edit the feature, not the geometry.
Bodies live in components. A component is a container with its own origin, and the unit of assembly. One printed part = one body; one kit = one component per part.
Parameters drive dimensions. Any number in a dialog can be an expression of named parameters; a scale factor is one parameter.
Colour is a body boundary. For a toolchanger the slicer assigns a tool per body, so the CAD job is a clean partition of the part into touching, non-overlapping bodies.

The hierarchy of a design

project › design › component › body — read down, built inside-out

Project	A folder in the Data Panel, inside your hub. One project per subject — a layout, a ship, a group of buildings — never one per part.
Design `.f3d`	One document is one kit, not one part. Personal allows ten editable designs, so a thirty-piece kit is one design holding thirty components.
Root component	The top line of the Browser. It takes the document's name and is the assembly. Keep it clear of geometry — child components, joints and canvases only.
Sub-assembly	A component that holds other components: bogie, chassis, deckhouse. Nest as deep as the real object does and no deeper.
Component	The part. Its own origin, sketches, bodies, joints and appearance, and its own Save As Mesh. One component = one thing you can pick up.
Body	Geometry, living inside a component. One per part — or one per colour (§10). A body has no position of its own and cannot be jointed.
Feature	A timeline step — Extrude, Revolve, Hole, Fillet — that creates or modifies bodies. The feature is the model; the body is only its output.
Sketch	Constrained 2D on a plane, owned by the component that consumes it. A closed loop is a profile.

The order a professional actually works

name the designSave it under the real name before drawing anything the root component inherits that name component firstASSEMBLE › New Component — empty, named on the spot, then activated (the radio button in the Browser) this is the step beginners skip, and the one that costs a rebuild sketch inside iton that component's origin planes, not the root's the part then carries its own datum and travels with it feature → bodyExtrude the profile; one body per part, or one body per colour next partback to the root, New Component again never grow two parts in one component meaning to sort it out later groupdrag components onto a parent component in the Browser to form a sub-assembly visibility, patterns and mirrors then work per assembly assembleactivate the root, Ground the base part, Joint J the rest to it joints connect components, not bodies — another reason the wrapper matters

Promoting what you already drew

sketch → bodyFinish Sketch, then Extrude E (or Revolve, Sweep, Loft) on the profile — and set Operation: New Body it defaults to Join the moment the new shape touches an existing one body → componentselect the body in the Browser or canvas › right-click › Create Components from Bodies. Each body becomes its own component, named after the body, and a step appears in the timeline or ASSEMBLE › New Component with From Bodies ticked, which lets you set the name and the parent in the dialog …and its sketchthe sketch does not follow. Drag it in the Browser out of the root's Sketches folder and onto the component's own Sketches folder do it now, while you still know which sketch made which part the catcha component wrapped round an existing body is placed on the root origin, so its origin planes are not on the part enough for a rigid kit; it bites the first time you mirror or pattern about the part's own centre. Cure: a construction plane inside the component, or redraw the sketch in a fresh one components → sub-assemblyASSEMBLE › New Component, leave it empty, name it (Bogie, Chassis), then drag the child components onto it in the Browser — positions are kept Rigid Group is not this: it locks parts together for motion, it adds no level to the tree sub-assembly → rootyou never create the root — it exists from the first save and carries the document's name, so renaming the design in the Data Panel renames it its job is components, joints and canvases, nothing else close the assemblyactivate the root, Ground the base component, then Joint J each remaining part to what it touches

The check that tells you it worked: the root component should have no Bodies folder and no Sketches folder left in the Browser — every one of each should sit inside the part it belongs to. Anything still at the root is loose geometry that will not export, pattern or joint as a part. Components, joints and the timeline in full at §05.

Name it as you make it. Component1:1, Sketch7 and Body3 are unreadable a week later, and they follow you into the timeline, the Browser and every exported file. Use the part's own name — Boiler, Cab-Side-L, Chassis — renaming with a slow double-click on the Browser entry.

The window

top to bottom

Application bar	Data Panel toggle (grid icon) · File menu (New, Open, Recover, Upload, Save, Save As, Export, Share, 3D Print, Capture Image) · Save · Undo/Redo · job status · notifications · Help · account · Autodesk Assistant button.
Document tabs	A Home tab (recent designs, projects, tutorials) followed by one tab per open design. The 10-document Personal cap counts editable designs in your hub, not open tabs.
Toolbar	Workspace switcher (DESIGN · GENERATIVE DESIGN · RENDER · ANIMATION · SIMULATION · MANUFACTURE · DRAWING) then the Design tabs SOLID · SURFACE · MESH · SHEET METAL · PLASTIC · UTILITIES; contextual SKETCH and FORM tabs appear while editing. Each tab is panels: CREATE · MODIFY · ASSEMBLE · CONSTRUCT · INSPECT · INSERT · SELECT.
Browser (left)	The tree: root component › Document Settings (units) · Named Views · Origin (XY, XZ, YZ planes; X, Y, Z axes) · Analysis · Joints · Sketches · Construction · Bodies · Canvases · child components. Radio button = activate; eye = visibility; chain link = external reference.
Canvas	ViewCube top-right; navigation bar bottom-centre (Orbit, Look At, Pan, Zoom, Fit, Display Settings, Grid & Snaps, Viewports); the Sketch Palette floats right while sketching.
Timeline (bottom)	Every feature in order. Drag the marker to roll back; double-click to edit; right-click for Edit Feature, Edit Sketch, Suppress, Rename, Create Group, Delete. Yellow = warning, red = error.
Data Panel (slide-out)	Hubs › Projects › folders › designs with versions; Editable / Read-only toggle per design; Upload; Export (.f3d).

Workspaces

what each one is for

Design	Everything on this sheet: sketch, solid, surface, form, mesh, sheet metal, plastic, assemble.
Render	Appearances, scene settings, in-canvas render and a local ray-traced render. Cloud rendering is a paid feature.
Animation	Explode views and storyboards, exported as video.
Drawing	2D sheets with views, dimensions and a title block; PDF out. Useful for a kit's assembly diagram.
Manufacture	CAM. Includes an Additive tab (FFF setups, machine library with Prusa printers, print settings, supports, G-code post). PrusaSlicer does the same job better for a Prusa; the useful part here is Utilities › Make › 3D Print.
Simulation · Generative	Present in the menu, paid.

Cycle with ⌘] / ⌘[. Fusion remembers the tab and workspace per document.

Personal plan — what you have

non-commercial, renewed yearly

Documents	10 editable designs at a time; unlimited read-only (Data Panel › design › Editable / Read-only). Read-only designs open, view and export. Keep one design per kit with many components rather than one per part.
Design tools	Sketch, Solid, Surface, Form, Mesh, Sheet Metal and the Plastic tab are all present. Not on Personal: Configurations (the Configure panel is greyed), the Product Design Extension tools (Volumetric Lattice, Organic mesh conversion, Prismatic mesh conversion), Simulation, Generative Design, cloud render, multi-user collaboration.
Export	F3D/F3Z, STEP, STL, OBJ, 3MF (Save As Mesh), SKP, SMT, FBX, USDz, IPT/IAM, sketch DXF. Not: IGES, SAT, DWG. Everything a printer needs is in the first line.
Import	STEP, F3D, STL/OBJ/3MF (as mesh), SVG, DXF, SKP, IPT. The Rhino/SolidWorks/CATIA family of importers is paid.
CAM	2- and 2½-axis milling, turning and FFF additive included, with rapids linked and one tool per post output.
Drawings	Sheets and PDF export; DWG out is restricted.
Support	Forums only. The title bar reads Personal – Not for Commercial Use.

Preferences worth setting once

Fusion menu › Preferences

Default Units › Design	mm. Per-document override lives in the browser under Document Settings › Units.
General › Default modeling orientation	Y up is Fusion's default and matches the ViewCube labels; Z up matches the slicer. Either works — export handles the swap — but pick one and never mix, or every Insert Mesh lands on its side.
General › Pan, Zoom, Orbit shortcuts	Fusion / Alias / SolidWorks / Tinkercad / PowerMill mouse schemes; Reverse zoom direction; Default orbit type Constrained vs Free.
General › Design	Capture Design History on for new designs (keep it); Auto project edges on reference (off — projected edges appear silently); Auto look at sketch; Allow 3D sketching of lines and splines.
General › Material	Default physical material and appearance for new bodies — set a plain PLA-coloured plastic so body colours are yours to change.
Preview	Feature flags for pre-release tools; leave alone unless a tutorial demands one.
Data Panel › Editable	Not a preference, but the switch you flip when the 10-document warning appears.

History vs direct

Capture Design History

New designs are parametric: the timeline records every feature and edits replay. Right-click the root component › Do not capture Design History turns the design into direct modelling — no timeline, Press Pull and Move edit faces in place, nothing rebuilds. Switching back keeps the current geometry as a single base feature.

The in-between is Create › Create Base Feature: a direct-modelling island inside a parametric timeline. Use it for imported meshes and STEP parts you only need to trim, and for one-off fixes where a fully parametric rebuild would cost more than it gives.

Rule for scale models: stay parametric. The whole point is changing the scale, the wall thickness or a window pitch in one place and letting the timeline redo the rest.

The three keys that matter

S · right-click · Esc

the shortcut box — type any command name, ↑↓ pick, ↩ runShover the box entry's ↑ arrow to pin it as a favourite; drag a toolbar command into the box to give it a hotkey the marking menu — commands radiate around the cursorright-clickright-click and flick toward a command without waiting for the menu: the gesture alone runs it repeat the last commandright-click → Northtop slot of every marking menu; there is no separate key cancel a command · clear the selectionEscconfirm is ↩ — the dialog's OK undo / redo⌘Z · ⇧⌘Zalso West / East of the marking menu

The Solid marking menu (nothing selected): N Repeat · NE Press Pull · E Redo · SE Hole · S Sketch submenu (N Finish Sketch, NE 2-Point Rectangle, E Fit Point Spline, SE Project, S Line, SW Offset, W Dimension, NW Center Diameter Circle) · SW Move · W Undo · NW Delete.

Mouse and trackpad

Preferences › General › Pan, Zoom, Orbit

action	3-button mouse	MacBook trackpad
Orbit	⇧ + middle-drag	⇧ + two-finger drag
Pan	middle-drag	two-finger drag
Zoom	scroll wheel	pinch, or ⌘ + two-finger drag
Zoom to a point	scroll over it	pinch over it
Fit everything	double-click middle button · `F6` · navigation bar ⤢ (Fit)
Look at a face	select the face → navigation bar ▣ Look At; sketches auto-look-at on creation
Orbit centre	right-click → Set Orbit Center puts the pivot where you click; Reset returns it

The navigation bar under the canvas holds Orbit (free / constrained), Look At, Pan, Zoom, Fit, plus the display-mode, grid and viewport menus. Constrained orbit keeps the Z axis vertical, which is what you want for buildings and rolling stock; free orbit is for hull work.

If your muscle memory comes from another package, Preferences › General › Pan, Zoom, Orbit shortcuts offers Alias, Inventor, SolidWorks, Tinkercad and PowerMill mouse schemes; Reverse zoom direction is in the same panel.

ViewCube

top-right of the canvas

Click a face for an orthographic view, an edge or corner for an isometric, the arrows to rotate 90°, the house for Home. Drag the cube to orbit. Right-click it for Set current view as Home, Set current view as Front (re-labels the whole cube — do this once when a model's front is not the sketch's front), Orthographic / Perspective / Perspective with Ortho Faces, and Reset Front.

Model buildings and vehicles with the Y axis up (Preferences › General › Default modeling orientation) so the ViewCube's Top really is the roof; Prusa's slicer treats Z as up, and 3MF/STL export handles the swap for you.

Design hotkeys

as defined in this build

key	command	key	command
`E`	Extrude	`Q`	Press Pull
`H`	Hole	`F`	Fillet
`M`	Move / Copy	`A`	Appearance
`J`	Joint	`⇧J`	As-Built Joint
`I`	Measure	`⌘B`	Compute All
`⌫`	Delete	`⇧S`	Scripts and Add-Ins
`V`	Show / hide the selection	`S`	Shortcuts box
`⇧N`	Display Component Colors	`⇧F`	Display Face Groups (mesh)
`1` `2` `3`	Window · Freeform · Paint select	`⇧H`	Autodesk Assistant chat

Sketch

`L`	Line	`R`	2-Point Rectangle
`C`	Center Diameter Circle	`D`	Sketch Dimension
`T`	Trim	`O`	Offset
`P`	Project	`X`	Normal ↔ Construction line

Inside a sketch Tab moves between the value fields of the tool you are drawing with; typing a number while dragging fills the highlighted one. Esc ends the line chain; a right-click marking menu offers OK/Cancel.

Application & window

Neutron shell hotkeys

`⌘S`	Save (version + comment)	`⇧⌘S`	Save As
`⌘O`	Open	`⌘W`	Close document
`⌘X` `⌘C` `⌘V`	Cut · Copy · Paste (bodies/components/sketch curves)	`⌘0`	Fusion Home
`⌘]` · `⌘[`	Next / previous workspace	`⌘F`	Filter the Data panel
`⌥⌘B`	Browser show/hide	`⌥⌘N`	Navigation bar show/hide
`⌥⌘V`	ViewCube show/hide	`⌥⌘C`	Text commands palette
`⌥⌘A`	Activity feed / comments	`⌥⌘R`	Reset to default layout
`⌥⌘I`	Insert dialog	`⌥⌘P`	Dashboard mode
`⌥⌘O`	Performance overlay	`⌘M`	Minimise

Plain clicks accumulate a selection until the command finishes; ⌘-click removes one item; ⇧-click in the browser or timeline selects a range.

Selection

the Select panel, every tab

1 Window (left-to-right drag selects what is fully inside, right-to-left anything crossed), 2 Freeform lasso, 3 Paint. Selection Filters (the funnel) limit picks to faces, edges, bodies, sketch curves, components…; the priority buttons put Bodies, Faces, Edges or Components first when several overlap. Select Through (shown as the filter's last option) picks hidden geometry.

Hover-scroll pick. Hover, hold the left button, and a stack of everything under the cursor appears — pick the hidden one.
Double-click an edge selects the chain of tangent edges — the fast way to fillet a whole rim.
Select by Name / Size / Boundary and Invert live under Selection Tools; Seed & Boundary Faces grabs everything between two rings of faces.
The Component Drag toggle stops accidental dragging of assembled parts.

Sketch workflow

Create Sketch → draw → constrain → dimension → Finish

startCreate Sketch (first icon on every tab, or right-click a plane/face) → pick an origin plane, construction plane or flat face the view turns to look at it draw roughlyL lines · R rectangle · C circle · arcs, polygons, slots, splines shape first, size later — never chase exact positions with the mouse constraincoincident · horizontal/vertical · tangent · equal · symmetry · concentric… most are inferred while drawing (the glyph by the cursor); hold ⌘ to suppress inference dimensionD then pick one or two entities, type a value, an expression or a parameter name right-click a diameter dimension to switch to radius checkevery line black = fully constrained; blue = free to move; the sketch gets a lock badge in the browser drag a blue point and watch what moves finishFinish Sketch (tick, top right) → Extrude the profile re-enter with a double-click on the sketch in the timeline

Draw one feature per sketch. A sketch with forty lines rebuilds slowly, fails opaquely and cannot be reused; a sketch with six lines does the opposite. Reference earlier geometry with Project (P) instead of redrawing it.

The Sketch Palette

floats at the right

Linetype	Construction (`X` toggles a selected line) — dashed, guides only, makes no profile. Centerline — a construction line that dimensions as a diameter when you dimension across it: draw the revolve axis as a centerline.
Look At	Turn the view square to the sketch plane again.
Sketch Grid · Snap	Grid display and snapping. Turn Snap off when tracing a canvas; leave it on for boxy parts.
Slice	Temporarily cuts the model at the sketch plane so you can see inside a shell while sketching.
Show Profile	Shades closed regions blue — the profiles Extrude will offer. A region that will not shade has a gap somewhere.
Show Points / Dimensions / Constraints / Projected / Construction	Display toggles. Show Constraints puts the glyphs on screen; click a glyph and press ⌫ to remove a constraint.
3D Sketch	Lets lines and splines leave the plane — for sweep paths and loft rails. Off by default.

Constraints

the twelve, and when

constraint	fixes	typical use
Coincident	point on point or point on curve	closing loops; a corner on the origin
Collinear	two lines on one line	window sills in a row
Concentric	same centre	bosses and their holes, wheels and axles
Midpoint	point at a curve's middle	centring a door in a wall
Fix / UnFix	locks position (green)	tracing a canvas; avoid otherwise — a fixed sketch ignores parameters
Parallel · Perpendicular	line direction	roof pitches, angled walls
Horizontal / Vertical	a line, or two points, aligned to the sketch axes	almost every rectangle edge
Tangent	curve meets curve smoothly	fillet arcs, hull sections
Curvature (G2)	matching curvature across a join	splines that must not show a crease
Equal	equal lengths or radii	one dimension driving a row of identical windows
Symmetry	two entities mirrored about a line	anything with a centreline — half the dimensions

AutoConstrain (the AI button in the Constraints panel) proposes a full constraint-and-dimension scheme; accept it on simple sketches, check it on anything with intent.

Dimensions

D · driving vs driven

A driving dimension sets a size; a driven one (shown in parentheses) just reports it. Fusion makes a dimension driven automatically when it would over-constrain; right-click to toggle. Every driving dimension becomes a model parameter d1, d2, … that any later dialog can reference.

type any of these in the dimension box 24in the sketch's units 3 inunit suffixes convert wall * 2 + 0.4 mmexpression of user parameters d12 / 2another dimension storey = 2.7 m * screates the user parameter storey on the spot and uses it

Dimension order matters less than constraint order. Constrain shape first, then add the few dimensions that express intent (overall width, a pitch, a diameter), and let symmetry and equal constraints carry the rest. Dimension to the origin or to projected model edges, not to other free sketch points.

Project, Intersect, Include

reusing what is already modelled

Project `P`	Copies body edges, silhouettes, sketch curves or construction geometry onto the sketch plane as purple curves. Projection Link on keeps them associative (they move when the source moves); off makes a plain copy. Selection filter Bodies projects a whole body's outline in one click.
Intersect	Only the geometry that actually crosses the sketch plane — the section outline of a hull at that station, or the door opening at floor level.
Include 3D Geometry	Brings model edges into a 3D sketch without flattening — rails for lofts and sweeps.
Project to Surface	Pushes sketch curves onto a curved face (along a vector or closest point) — lettering on a boiler, panel lines on a fuselage.
Intersection Curve	The 3D curve where two sketches or surfaces meet.
Spun Profile	Revolves geometry about an axis and projects its outline — the envelope of a rotating part.

Projected curves are the safe way to line a new feature up with an old one. Dimensioning to a purple curve keeps the alignment through every later edit.

Sketch tools that earn their keep on models

beyond line and circle

Text — a box or a path; font, height, bold, alignment; Fit on Path curves a name around a boiler band. Right-click › Explode Text turns letters into editable curves. Extrude it 0.4–0.6 mm proud, or cut it 2 layers deep for an inlay.
Rectangular / Circular Pattern — window grids, rivet rings, portholes; drive Quantity and Spacing with parameters; suppress individual instances with the checkboxes.
Mirror — draw half a façade about a centreline construction line; adds symmetry constraints.
Offset O — wall thickness, window frames, a moulding profile's inner line. Chain selection follows the loop.
Slot — louvres, grab-rail slots, coupler pockets; five ways to define one.
Conic Curve — ship stems and aircraft noses; the rho value shifts it from ellipse (<0.5) through parabola (0.5) to hyperbola.
Fit Point Spline passes through points (tracing); Control Point Spline is shaped by a cage (fairing a hull). Fewer points, smoother curve.
Break · Trim · Extend — clean up a traced outline before extruding; a profile will not shade until every loop closes.
Insert SVG / DXF (Insert panel) — logos, plan drawings, laser-cut kits; SVG must be paths, not strokes, and long imports extrude slowly.
Canvas + right-click › Calibrate — drop a photo or drawing on the sketch plane, click two points of known distance, and trace over it.

Operation: the option in every Create dialog

Join · Cut · Intersect · New Body · New Component

operation	result	use for
Join	merges into the body it touches	adding a chimney to a roof
Cut	subtracts from the bodies it crosses; Objects to Cut picks which	windows, doors, pockets
Intersect	keeps only the overlap	trimming a hull to a waterline block
New Body	a separate body in the same component	a second colour; a part to be cut with later
New Component	a new component containing the body	a separately printed part of a kit

Fusion guesses Cut when the profile lies inside a body and Join when it touches one. Check the drop-down every time — a Join that should have been a New Body is the commonest way to lose a colour boundary.

Extrude

Type	Extrude a closed profile or face; Thin Extrude an open or closed curve into a wall (Wall Location side 1 / side 2 / centre, Wall Thickness) — a building wall from a single line.
Profiles	Click regions, or faces; Chain picks adjacent regions.
Start	Profile Plane · Offset (start above the plane — a raised platform without a second sketch) · Object (start from a face).
Direction	One Side · Two Sides (independent distances) · Symmetric (half or whole length).
Extent	Distance · To Object (a face, plane or body; Extend to adjacent faces) · All (through everything that way).
Taper Angle	Draft per side; negative narrows. A 1–2° taper makes a chimney or funnel look cast rather than cut.
Operation	See above. Objects to Cut lists the bodies a Cut may touch — untick the colour bodies you want left alone.

A negative distance reverses direction. Type an expression (-wall, storeys * storey) rather than a number.

Revolve · Sweep · Loft

the other three profile features

Revolve	Profile + Axis (sketch line, centerline, construction axis or model edge). Type Full · Angle · To; one/two sides/symmetric. Wheels, domes, boilers, funnels, tanks — anything a lathe would make.
Sweep	Profile along a Path; types Single Path, Path + Guide Rail (rail controls scale/twist), Path + Guide Surface. Distance 0–1 each way, Taper, Twist, Orientation Perpendicular (profile follows the path) or Parallel (stays as drawn). Gutters, mouldings, handrails, pipe runs, rail with its profile.
Loft	Two or more Profiles (sections, faces or a point) in order; end conditions Connected / Direction / Tangent / Smooth; optional Rails (curves touching every section) or a Centerline; Closed loops back to the first section. Hulls from station sections, car bodies, tapered towers, a nose cone to a point.
Rib · Web	An open sketch curve extruded to the nearest faces as a thin wall — Rib parallel to the sketch plane, Web perpendicular. Bracing inside a hollow model; a gusset under an awning.
Emboss	Sketch profile raised or recessed on a flat or curved face by a depth; Wrap around cylinders. Lettering on a tank, rivets on a boiler, panel lines.

Loft profiles want the same number of segments and matching start points; a twisted loft means one section's vertices are numbered from a different corner — add a rail or split a segment.

Hole · Thread · primitives

Create panel

Hole `H`	Placement single / multiple on sketch points / at point; type Simple · Counterbore · Countersink · Counterdrill; tap type Simple · Clearance · Tapped · Taper tapped; extent Distance · To · All; drill point flat or 118°. Add ~0.2 mm to a printed horizontal hole's diameter.
Thread	On a cylindrical face; ISO Metric, ANSI Unified, ACME, pipe; tick Modeled for real geometry a printer can make (cosmetic threads are texture only). Printed M6 and up work with 0.15–0.25 mm radial clearance.
Box · Cylinder · Sphere · Torus · Coil · Pipe	Primitive solids without a sketch; Coil has revolutions/height/pitch and a circular, square or triangular section (springs, ropes at 1:16); Pipe follows a path or edges, hollow with a wall thickness (handrails, plumbing).
Stock Model	A solid envelope around a selection — a quick box to cut a mould or a display base.
Boundary Fill	Pick tool bodies/surfaces/planes, tick the enclosed cells to keep — extracts a cavity as a body (the inside of a shelled building, to see how much filament it is).
Thicken	Gives a surface body a wall thickness → solid. The last step of every surface-modelled hull.

Patterns and mirror

Create › Pattern

Rectangular Pattern	Type Faces / Bodies / Features / Components; one or two directions; Quantity; Distance as Spacing or Extent; Symmetric; suppress instances by unticking. Compute Type: Optimized (fast), Identical, Adjust (each instance recomputed against the model — required when a cut pattern runs across changing geometry).
Circular Pattern	Axis; Full, Angle or Symmetric; Quantity. Wheel spokes, portholes, bolt circles, gear teeth.
Pattern on Path	Distance along a path, Quantity, orientation Identical or Path Direction. Sleepers along curved track, stanchions along a deck edge, rivets along a seam.
Geometric Pattern	Size and spacing gradients across a face — texture, not modelling.
Mirror	Faces, bodies, features or components across a plane; Join or New Body. Model half a symmetric hull, mirror, Combine.

Pattern features (the window cut) rather than bodies when the pattern must follow later edits; pattern bodies when the instances will be separate colours or separate prints.

Modify — shape

Press Pull · Fillet · Chamfer · Shell · Draft · Scale

Press Pull `Q`	One tool, three behaviours: a face → Offset Face; a sketch profile → Extrude; an edge → Fillet. Drag the arrow or type. In a parametric design it edits the existing feature when it can.
Fillet `F`	Edges/faces/features; Constant, Chord Length or Variable radius (add points along the edge); Tangent Chain; Rolling Ball vs Setback corners; G2 Curvature option. Rule Fillet fillets by rule (all edges of a body, between faces). Double-click an edge to grab the tangent chain.
Chamfer	Equal Distance · Two Distances · Distance and Angle. A 45° chamfer under an overhang prints unsupported where a fillet would sag.
Shell	Pick the faces to open (none = a closed hollow), thickness inside / outside / both. Wall ≥ two perimeters (0.45 mm on the 0.2 mm nozzle, 0.9 on a 0.4); a shelled building with an open bottom prints upright with no infill.
Draft	Fixed plane, parting line or fixed edges; angle. Cast-looking funnels and cabs; a degree or two also helps parts release from a printed mould.
Scale	Bodies, components or sketches about a point; Uniform or per-axis; the factor takes an expression (`1/87`). Scales everything, including walls and fillets — see §08 for when to use it and when not.

Modify — bodies and faces

Combine · Split · Offset · Move

Combine	Target + Tools; Join · Cut · Intersect; Keep Tools keeps the tool bodies afterwards; New Component. Cut + Keep Tools is the inlay recipe: the tool becomes the second colour and the target has an exact pocket for it.
Split Body	Body + splitting tool (plane, sketch, face or surface; Extend splitting tool stretches a surface through). Both halves stay, touching on a shared face. The colour-boundary tool.
Split Face	Divides faces without splitting the body — for a different appearance, a decal area or a Press Pull region.
Silhouette Split	Splits along the outline seen from a direction — mould halves, or a hull into above- and below-waterline prints.
Offset Face	Moves faces in or out; negative insets. The direct way to thicken one wall.
Replace Face	Swaps faces for a surface — a flat roof becomes a curved one.
Move / Copy `M`	Components, bodies, faces or sketch objects; Free Move triad, Translate, Rotate, Point to Point, Point to Position; Create Copy; Set Pivot. Moving faces in a history design records a Move feature.
Align	Moves a body/component so picked geometry lands on target geometry — mating a roof body to its walls.
Delete vs Remove	Delete erases a feature and everything downstream that needed it; Remove adds a timeline feature that hides a body from here on (the history survives).
Physical Material · Appearance `A`	Material drives mass in Properties; Appearance is colour only. Give each colour body its filament colour so the canvas previews the print; PrusaSlicer will not read it, but you will.

Construct and Inspect

planes, axes, points · measure and analyse

Construction planes: Offset (the workhorse — one per storey, per deck, per colour band), Plane at Angle (roof pitch), Tangent Plane (lettering on a cylinder), Midplane (mirror plane between two walls), Perpendicular plane, Through Two Edges, Through Three Points, Along Path (sections along a hull). Axes through a cylinder, an edge, two points, two planes, or perpendicular at a point. Points at a vertex, two edges, three planes, a circle centre, an edge and plane, along a path. All parametric.

Inspect: Measure I (distance, angle, area, volume; two selections give the gap and the Δx/Δy/Δz), Interference between bodies (turn it on before exporting a kit), Section Analysis (a live cut plane — the only way to see a shell wall thickness), Center of Mass, Curvature comb / Zebra / Curvature map (hull fairing), Draft analysis, Minimum radius, and the ⇧N component-colour toggle.

Bodies vs components

Rule #1

A body is geometry. A component is a container with its own origin, its own sketches and bodies, a position in the assembly and joints to other components. The community's Rule #1: create a component before the first sketch, name it, and keep the root for assembly only. Sketches and bodies then belong to the part they describe, patterns and mirrors of components work, joints work, and Save As Mesh on the component exports exactly that part.

one printed part	one component; inside it one body per colour (§10)
a kit	root › one component per part, joined together so you can see the fit; export each component separately
a repeated part	copy the component (⌘C ⌘V or Pattern › Components) — instances share geometry; Paste New makes an independent copy
a part from another design	Insert › Insert into Current Design (linked, chain-link icon; Get Latest updates, Break Link localises) or Insert Derive for selected bodies, sketches and parameters

The radio button in the browser activates a component: new features go into it and everything else dims. Forgetting to activate is why bodies land in the root.

Joints

J · Shift+J

Joint J picks a snap point on the moving component then one on the fixed component and moves the first to meet the second; As-Built Joint ⇧J leaves both where they are and just defines the motion. Snap points are face centres, edge midpoints, vertices, or Between Two Faces; a placed Joint Origin is a reusable snap point.

type	freedom	model use
Rigid	none	roof on walls, deckhouse on deck — the default for kits
Revolute	1 rotation	wheels, doors, turntable, crane jib
Slider	1 translation	drawers, sliding doors, coupler travel
Cylindrical	rotate + slide, one axis	a shaft in a bearing
Pin-Slot	rotate + slide, different axes	a pin riding in a slot
Planar	2 translations + 1 rotation	a part loose on a table
Ball	3 rotations	a ball-and-socket mast foot

Ground (right-click › Ground) pins the base component. Rigid Group locks several components as one. Drive Joints sets a joint value; Motion Link ties two joints (a ratio); Enable Contact Sets makes dragged parts collide; Motion Study keyframes joints. Joint limits (min/max/rest) are on the joint's right-click menu.

The timeline

rolling, editing, grouping

edit a featuredouble-click it, or right-click › Edit Feature · Edit Sketch · Edit Profile insert a feature earlierdrag the marker back to the spot, model, drag it forward again later features replay on top turn a feature offright-click › Suppress Features the printed base version vs the detailed version tidyselect a run › right-click › Create Group; Rename features (F2 does not work here — right-click) warningsyellow = a reference was lost but Fusion coped; red = a feature failed hover for the reason; usually a deleted edge that a fillet or a sketch projection pointed at force a rebuild⌘B Compute All

Order that rebuilds cleanly: big shapes → shells → holes and cuts → patterns → fillets and chamfers → colour splits → text. Fillets last, because every earlier edge edit invalidates the fillet that referenced it. Colour splits after the shape is final, because Split Body references faces too.

Kits that fit

clearances and registration

fit	per-side clearance	notes
press fit	0.10–0.15 mm	peg into socket, glued or not
sliding	0.20–0.30 mm	lids, drawers, sliding roofs
free-moving	≥ 0.40 mm	wheels on axles, hinges
horizontal hole	+0.2 mm diameter	holes print undersize; vertical holes less so
print-in-place	0.3–0.4 mm	and a chamfer where the gap meets the bed

Keep clr = 0.25 mm as a user parameter and write every socket as peg + 2*clr. Register parts with a peg and a socket rather than a butt joint; make the peg on the part that prints it pointing up, so it needs no support. Check with Interference before exporting.

Change Parameters

Modify › Change Parameters · no default key — give it one

User Parameters	Your names: + → Name, Unit (mm · cm · m · in · ft · deg · rad · No Units · mass, area, etc.), Expression, Comment. Star the ones you touch often (Favorites filter).
Model Parameters	Everything Fusion created, grouped per component › sketch or feature: sketch dimensions `d1…`, extrude distances, hole sizes, pattern counts. Rename them to use them by name.
Names	Letters, digits, underscore; not starting with a digit; case-sensitive; not a function name.
Operators	`+ - * / % ^`, brackets, comparisons `> < >= <= == <>`, `and or not`, `if(test; a; b)`.
Functions	`sin cos tan asin acos atan sinh cosh tanh` (degrees unless you write `rad`), `sqrt abs sign exp ln log pow floor ceil round max min random`; arguments separated by `;` (a comma also works in the English locale).
Constants	`PI` · `E` · `Gravity` · `SpeedOfLight`.
Units	Every expression must resolve to the parameter's unit. `10 mm`, `2 in`, `1.5 m`, `45 deg` convert; bare numbers take the parameter's unit; length × length is an area and will not fit a length parameter. No Units is for pure factors.

Sort in timeline order, or search. A parameter can only be deleted when nothing references it. Values are stored internally in cm — you will notice in the API, never in the dialog.

A parameter set for a scale model

copy this first

the scale, as a unitless factor s = 1/87No Units · HO. Change to 1/160 and the model re-sizes itself prototype dimensions in real units, scaled at the point of use storey = 3.2 m * s36.8 mm at 1:87 wall_real = 300 mm * s3.4 mm — but see the next two lines print-driven minimums that do NOT scale wall = max(300 mm * s; 0.5 mm)never thinner than two perimeters of a 0.2 mm nozzle (0.45 mm) detail = max(50 mm * s; 0.25 mm)window mullions, trim, rivets clr = 0.25 mmsliding-fit clearance, per side layer = 0.1 mmso colour bands and steps are whole layers: 3 * layer counts and pitches bays = 6No Units — drives a pattern's Quantity bay_pitch = 4.5 m * sdrives its Spacing

Dimension the sketch as storey, bay_pitch * bays, wall; extrude by storey * floors; pattern by bays. Now one edit to s re-scales every prototype dimension while the walls, mullions and clearances hold at what the nozzle can print. That is the whole reason to model parametrically at all.

Model at 1:1 or at scale?

two honest answers

At scale, with `s`	Every dimension is real value × s and every print-limited feature is a floor via `max()`. Best for buildings, rolling stock, anything with walls: you see the print as it will be, and Save As Mesh exports at 1:1 with no surprises. Recommended.
At 1:1, scale on export	Model in metres with prototype dimensions, then Modify › Scale a copy by `1/87` (or scale in PrusaSlicer). Simplest for tracing plans and for organic shapes with no walls to protect. Cost: walls, fillets, text and clearances all shrink with it, so you check minimum feature sizes afterwards, by hand, every time.
Hybrid	Trace the plan at 1:1 in a reference sketch, project it into scaled sketches with `Sketch Scale`, or Insert Derive the 1:1 design into a new one and Scale once. Useful when the same prototype will be printed at two scales.

Fusion's Scale command takes an expression, so 1/87, s or 25.4 mm / 87 all work. Scale bodies inside a component; scaling the component moves its origin too.

Design intent habits

what keeps a model editable

Sketch on origin planes and offset planes, not on faces that a later cut may remove. If you must sketch on a face, project the edges you need with P and dimension to those.
Dimension to the origin. A sketch anchored at the origin survives everything; one anchored to another sketch's free point moves with it.
Name things — bodies, components, sketches, parameters, timeline groups. Body12 is where models go to die; roof-red tells the slicer step what tool it gets.
One feature per intent. A window is a sketch and a cut; a row of windows is that cut patterned by bays. Do not draw twelve windows.
Suppress, do not delete when trying an alternative. Suppress the fine detail features to print a fast test at 0.3 mm layers.
Save with a comment (⌘S asks for one). Versions are free and the Data Panel can promote any of them.
Configurations are paid; on Personal the substitute is user parameters plus suppressed features, or Save As copies.

Surface

SURFACE tab

A surface body has faces but no volume. Build the skin with Extrude, Revolve, Sweep, Loft, Patch (fill a closed loop of edges with position, tangent or curvature continuity), Ruled (a surface from an edge at a distance and angle) and Offset; cut it with Trim and restore with Untrim; Extend edges; Stitch the pieces — when a stitched quilt closes, Fusion turns it into a solid. Thicken gives an open surface a wall. Reverse Normal decides which side Thicken and Offset grow from; surface backs shade a different colour so you can tell.

A hull in five features

1sketch station sections on offset planes along the length (Construct › Offset Plane × n, or Plane Along Path) — half-sections only, one side of the centreline 2a sheer line and a keel line in a 3D sketch or on the profile plane as rails 3Surface › Loft the sections with both rails; check with Zebra / Curvature Comb 4Mirror across the centre plane, Stitch, Patch the transom and deck → a solid 5Shell or Thicken to the print wall; Split Body at the waterline for the two-colour hull

Form (T-splines)

Create › Create Form · FORM tab · Finish Form

A push-pull sculpting environment for smooth organic bodies: locomotive noses, car bodies, figures, sacks and tarpaulins. Start from a primitive (Box, Plane, Cylinder, Sphere, Torus, Quadball, Pipe) or Extrude / Revolve / Loft a sketch into a form, then Edit Form — select vertices, edges or faces and drag the triad (⌥-drag a face extrudes it). Double-click an edge for the loop.

add control	Insert Edge · Subdivide · Insert Point — put density only where the shape changes
join and fill	Bridge · Merge Edge · Fill Hole · Weld Vertices · Erase and Fill
sharpen	Crease / UnCrease · Bevel Edge (a smooth-but-tight corner)
fair	Smooth · Flatten · Straighten · Cylindrify · Pull (to a target) · Match (to a curve) · Interpolate
symmetry	Mirror-Internal (edit one side, both move) · Circular-Internal · the Duplicate variants create linked copies · Clear · Isolate
display	Box (the cage) ↔ Smooth; Repair Body and Make Uniform when Finish Form refuses

Finish Form converts to a B-rep solid (closed) or surface (open) and becomes one Form feature in the timeline; double-click it to sculpt again. Keep the cage coarse — a form with thousands of faces converts into a body that fillets and slices slowly.

Mesh

MESH tab

Insert Mesh (STL, OBJ, 3MF; unit type; flip up direction; centre or ground) brings a downloaded model in as a mesh body. Mesh bodies cannot be extruded from or cut by solid tools until converted, but they can be measured, sectioned, and edited with the mesh tools.

Prepare	Repair (close holes · stitch and remove · rebuild · wrap) · Generate Face Groups (colour patches by normal angle, `⇧F` shows them) · Combine / Create face groups
Modify	Reduce (fewer triangles — do it before converting) · Remesh (uniform or adaptive) · Plane Cut (trim or split — a hull at the waterline) · Shell · Combine (join/cut/intersect meshes) · Separate (loose shells into bodies) · Smooth · Reverse Normal · Erase and Fill · Bridge · Mesh Align · Attract to Reference · Texture Extrude (image → relief) · Scale Mesh · Direct Edit
Create Mesh Section Sketch	Slices the mesh with a plane and traces the outline as sketch curves; Fit Curves to Mesh Section turns the polyline into lines, arcs and splines. The route from an STL to a clean parametric rebuild.
Tessellate	Solid → mesh body inside Fusion (same refinement settings as export).
Convert Mesh	Mesh → solid or surface. Faceted (one face per triangle) is the only method on Personal; Prismatic (clean planar/cylindrical faces from face groups) and Organic are paid. Parametric operation keeps it in the timeline.

Rule of thumb: Reduce to under ~50 k triangles before a faceted convert, and only convert if you must Boolean it. To add your own parts to a downloaded model it is usually faster to leave the mesh as a reference, section-sketch the outline, and model the new parts as solids around it.

Sheet Metal and Plastic tabs

there, rarely needed here

Sheet Metal — Flange, Bend, Fold, Unfold/Refold, Flat Pattern, rules for thickness and K-factor — exists for folded-metal parts; the flat-pattern DXF is the useful output if you ever laser-cut a scale roof. Plastic — Boss, Snap Fit, Lip/Groove, Rest, Plastic Rules for wall and draft — targets injection moulding; Snap Fit and Boss are handy for kit joints, the rest of the tab (and Volumetric Lattice on Solid › Modify) needs the paid extension.

Scales, gauges and factors

mm per real foot = 304.8 / N · mm per real metre = 1000 / N

scale	name	mm/ft	mm/m	1.8 m person	2.4 m storey	std gauge 1435
1:16	large scale, ⅝″ rolling stock, 112 mm figures	19.05	62.5	112	150	89.7
1:22.5	G (LGB; on 45 mm track)	13.5	44.4	80	107	63.8
1:24	½″ scale, dolls' house	12.7	41.7	75	100	59.8
1:32	Gauge 1 (45 mm) · 54 mm figures	9.53	31.3	56	75	44.8
1:35	Tamiya armour	8.71	28.6	51	69	41.0
1:43.5 · 1:45 · 1:48	O gauge (32 mm): UK · Europe · US	6.35 (US)	20.8	37.5	50	29.9
1:56	28 mm wargames	5.44	17.9	32	43	25.6
1:64	S gauge (22.4 mm) · Hot Wheels	4.76	15.6	28	37.5	22.4
1:72	Airfix · 20 mm figures	4.23	13.9	25	33.3	19.9
1:76.2	OO (UK, on 16.5 mm)	4.00	13.1	23.6	31.5	18.8
1:87	HO (16.5 mm; NMRA 3.5 mm/ft = 1:87.1)	3.50	11.5	20.7	27.6	16.5
1:100	15 mm wargames · single-building architecture	3.05	10.0	18	24	14.3
1:120	TT (12 mm)	2.54	8.33	15	20	12.0
1:144	aircraft · Dragon armour	2.12	6.94	12.5	16.7	10.0
1:160	N (9 mm; UK N 1:148, Japan 1:150) · 10 mm wargames	1.91	6.25	11.2	15	8.97
1:200	city-block architecture · large ships	1.52	5.00	9.0	12	7.17
1:220	Z (6.5 mm)	1.39	4.55	8.2	10.9	6.52
1:285 / 1:300	6 mm micro-armour	1.07	3.51	6.3	8.4	5.04
1:350	full-hull ship display standard	0.87	2.86	5.1	6.9	4.10
1:400	Heller ships · airliners	0.76	2.50	4.5	6.0	3.59
1:500	site-plan architecture	0.61	2.00	3.6	4.8	2.87
1:600	Airfix warships (1959)	0.51	1.67	3.0	4.0	2.39
1:700	waterline ships (1971 series)	0.44	1.43	2.6	3.4	2.05

Converting a model built at 1:A to 1:B: scale by A / B — HO → N is 87/160 = 54.4 %, HO → O(US) 181 %, 28 mm → 6 mm is 56/285 = 19.6 %. Figures are named by foot-to-eye height, so "28 mm" is nearer 32 mm to the top of the head.

What survives the nozzle

0.2 mm nozzle · real detail at scale, mm

≥ 0.45 stands as a wall (two perimeters) · 0.22–0.45 prints as a single line only · < 0.22 does not print — engrave it, paint it, or leave it out. A 0.2 mm nozzle lays a 0.22 mm line; a step needs two layers (0.1 mm at 0.05).

scale	65 mm brick course	40 mm mullion	25 mm rivet	12 mm handrail	300 mm wall	1 m
1:16	4.06	2.50	1.56	0.75	18.8	62.5
1:24	2.71	1.67	1.04	0.50	12.5	41.7
1:32	2.03	1.25	0.78	0.38	9.38	31.2
1:48	1.35	0.83	0.52	0.25	6.25	20.8
1:64	1.02	0.62	0.39	0.19	4.69	15.6
1:72	0.90	0.56	0.35	0.17	4.17	13.9
1:87	0.75	0.46	0.29	0.14	3.45	11.5
1:100	0.65	0.40	0.25	0.12	3.00	10.0
1:144	0.45	0.28	0.17	0.08	2.08	6.94
1:160	0.41	0.25	0.16	0.07	1.88	6.25
1:220	0.30	0.18	0.11	0.05	1.36	4.55
1:350	0.19	0.11	0.07	0.03	0.86	2.86
1:600	0.11	0.07	0.04	0.02	0.50	1.67

Read it against the nozzle: under one line width nothing exists; under two nothing stands as a wall; under two layers nothing shows as a step. With the 0.2 mm nozzle brick courses stay engravable to about 1:144, mullions print as lines down to 1:160 and as walls to 1:87, rivets are real at 1:32 and single-line dots to 1:100, and handrails are wire below 1:48. A 300 mm wall is a healthy 3.4 mm at HO and still a printable 0.5 mm at 1:600, where a building is a massing block with floor lines every 4 mm.

Per-scale strategy

what to model, what to leave to paint or wire

1:16 – 1:32	0.2 nozzle at 0.15 layers (or a 0.4 at 0.2 for speed). Model everything: rivets 0.8–1.5 mm, bricks, mullions 1.2–2.5 mm, planking. Walls 0.9–1.2 mm. Colour boundaries work at any feature you can draw.
1:48 – 1:72	0.2 at 0.10–0.15. Bricks as 0.2 mm engraved lines; mullions 0.5–0.8 mm; rivets 0.5 mm domes; walls 0.7–0.9 mm. Colour: roofs, trim, lettering ≥ 5 mm.
1:87 – 1:100	0.2 at 0.07–0.10. Mullions 0.45 mm; brick as 0.22 mm mortar lines 0.1 deep on flat-printed walls; rivets as 0.25 mm single-line dots or none; window frames as separate flat parts; walls 0.7 mm. Colour: wall / roof / trim bodies; lettering ≥ 3 mm.
1:144 – 1:220	0.2 at 0.05–0.07. Massing, openings, cornices, chimneys; mullions as single 0.22 mm lines; floor lines engraved 0.1 mm; walls 0.45–0.7 mm. Figures and sub-0.2 mm detail are a resin printer's job.
1:285 – 1:700	0.2 at 0.05–0.07. Massing only: hull, superstructure blocks, building blocks. Anything under 0.15 m real is omitted or drawn as a colour patch. Print hulls upright or on the waterline; barrels, masts and railings are wire or bought.

Setting up the design

one parameter, three habits

1 · the parameterChange Parameters › s = 1/87 (No Units) — and wall, detail, clr, layer as absolute floors (§06) 2 · reference materialInsert › Canvas on the front/side/plan planes → right-click › Calibrate two known points… and type the scaled distance (2400 mm * s), so the canvas is already at model size 3 · prototype dimensionsevery sketch dimension typed as real * s: 9.1 m * s for a boxcar, 2.7 m * s a storey, 1435 mm * s the gauge 4 · print-limited dimensionstyped as the floor: wall, detail, peg + 2*clr, 3 * layer — never multiplied by s 5 · the checkchange s to 1/160, ⌘B, and look: prototype geometry shrank, walls and pegs did not, the timeline stayed green

Fusion has no drawing scale. It models at 1:1 in whatever the numbers say. Modify › Scale is a feature that scales bodies (sketches need Sketch › Modify › Sketch Scale separately) and the factor lands in Change Parameters as a model parameter you can edit later. Use it for the 1:1-then-shrink workflow or for re-scaling a downloaded model; use s for anything you will maintain.

Subjects

the feature recipe for each

Building	One component per wall (print flat, detail face up — XY detail at full nozzle resolution, no supports, brick courses as one-layer engraving) or one shelled box printed upright (brick relief at layer resolution, Z lines on the walls). Offset plane per storey; window = sketch + Cut patterned by `bays`; frames and doors as separate flat bodies in their own colour; roof its own component with a peg registration; chimneys and cornices joined to what they sit on. Shell 0.9–1.2 mm, bottom face removed.
Rolling stock	Body shell as a shelled box or Loft (ends, tumblehome); underframe separate; Emboss for rivets and panel lines (0.15 mm proud at HO — or skip); doors and ladders as bodies of their own colour; couplers and wheels are commercial parts — model the pocket to NEM/Kadee dimensions with `clr`.
Ship	Half-hull Loft of station sections with sheer and keel rails, Mirror, Stitch; Split Body at the waterline (colour and print seam); deck and superstructure as stacked bodies; print the hull upright on its transom or on the waterline plane; masts and barrels as wire holes (`0.5 mm + clr`).
Vehicle	Body as a Form (T-spline) or Loft from a calibrated three-view canvas; Split Body at the belt line for two-tone paint; wheels as Revolve + Circular Pattern; print body upside-down on its roof or on a flat face with organic supports.
Figure	Form workspace, symmetry on; one body, one colour, 0.2 nozzle, organic supports at a 15–20° threshold. Below 20 mm tall, resin.
Terrain and bases	Big and coarse: 0.6–0.8 mm tool on the INDX, 0.3 mm layers, Rectangular Pattern of a hexagon for grid bases, Emboss with an image (Texture Extrude on a mesh) for ground.

Tracing plans and photos

Canvas · SVG · DXF

Canvas — Insert › Canvas → pick a plane → image. Browser › Canvases › right-click › Calibrate: two clicks and the true (scaled) distance. Edit Canvas for opacity, flip and Display Through. Put the side view on XZ, the end on YZ, the plan on XY, each calibrated on the same known length, and the three trace sketches line up.
Insert SVG — logos, laser-kit drawings; must be paths (convert strokes to paths first); scale on insert or with Sketch Scale; thousands of tiny segments make Extrude slow — simplify first.
Insert DXF — plan drawings from the railway press or an architect; layers become sketches; set the unit.
Fit Point Spline through a traced outline, then Control Point Spline to fair it; fewer points, truer curve. Dimension a couple of key points to the origin so the trace is anchored.
Measure the prototype, not the drawing: a wheelbase or a door height you know beats the plan's scale bar.

Feature limits

0.2 mm nozzle · (0.4 mm in brackets)

feature	minimum	comfortable
single-line wall	0.22 (0.45)	needs Arachne or Detect thin walls; fragile
free-standing wall	0.45 (0.9)	0.7 mm = 3 perimeters; multiples of 0.22 avoid gap fill
raised detail	0.25 wide × 0.15 high (0.5 × 0.3)	0.5 wide × 0.3 high
engraved detail	0.25 wide × 0.1 deep (0.5 × 0.2)	0.5 × 0.2; one layer deep for mortar lines
text, bold sans	2 mm cap (3 mm)	3–4 mm; stroke ≥ 0.45 mm
hole, vertical	0.3 mm	1 mm to be round; add 0.1–0.2 mm to the diameter
hole, horizontal	1 mm	teardrop the top, or +0.2 mm; sags otherwise
peg	2 mm vertical	3 mm; horizontal pegs snap across layers
slot or gap	0.5 mm	0.6 mm for a hinge
unsupported overhang	45°	55–60° in cooled PLA; chamfer instead of fillet underneath
bridge	—	PLA 50–60 mm, PETG 40; a lintel is a bridge
layer height	≤ 80 % of nozzle = 0.16	0.07–0.10 for detail, 0.15 for speed; a 0.4 or 0.6 tool for bases
XY accuracy	±0.1 best	±0.3 typical — design fits in 0.1 mm steps

Z is finer than XY

put the detail where the resolution is

A layer is 0.05–0.15 mm; a line is 0.22 mm on the 0.2 nozzle, 0.45 on a 0.4. Detail that varies with height — courses, weatherboards, corrugations, steps — resolves 2–8× finer than detail that varies across the bed. Two consequences:

Print walls flat, detail face up, when the detail is in the plane of the wall (window surrounds, signs, one-layer engraved mortar): every edge is at nozzle width, the top face is smooth, nothing needs support, and the wall is a separate part in its own colour if you like.
Print walls upright when the detail is relief that runs horizontally (brick courses, clapboard, corrugated iron): the courses come out at layer resolution and the layer lines are the texture.

Fusion side: model each wall as its own body in its own component so it can be oriented independently; a shared registration peg keeps the corners true.

Orientation and splitting

decide in CAD, not in the slicer

largest flat face downbuildings on their base; roofs on their flat underside; vehicles on the roof, or Split Body so a flat face exists split where the overhang startsModify › Split Body at the eaves, the belt line, the waterline — two clean prints beat one supported one split for the bedCORE One bed is 250 × 220 × 270 mm; a 1:87 station platform is longer — split with pegs every 200 mm chamfer, do not fillet, belowa 45° chamfer under a sill or ledge is self-supporting; a fillet there needs support bottom-edge chamfer0.3–0.5 mm on any face that mates — elephant foot never fights the fit no tiny footprintsa 0.5 mm chimney standing alone on the bed will not stick; give it a base flange or a brim

Walls, shells and infill

what the slicer will make of your solid

A solid body becomes perimeters (2 by default, 0.22 mm each on the 0.2 nozzle), top and bottom solid layers, and sparse infill in between. So:

Shell a building to wall = 0.45–0.9 mm (two to four perimeters) with the bottom face removed: the slicer prints the walls as perimeters only, no infill, and the print is light and quick. Interiors visible through windows get an inner wall of their own colour if you want.
Solid small parts (chimneys, figures, wheels): let infill happen; 15 % gyroid.
A wall of whole perimeters prints cleanest — 0.45, 0.67, 0.9 mm on the 0.2 nozzle; 0.5 mm leaves a sliver the slicer fills badly. Make wall a multiple of 0.22.
Bosses and ribs (Rib, Web) at 0.45–0.7 mm brace a shelled roof without adding infill.

Registration, fits and assembly

so the kit goes together without filing

Peg and socket	Peg 2–3 mm dia, socket `peg + 2*clr`, 0.5 mm lead-in chamfer on both. Make the peg on the part where it points up.
Rebate corners	Walls meet on a stepped rebate (half thickness each) rather than a butt or mitre; glue area doubles and the corner squares itself.
Tabs and slots	A 0.9 mm tab into a 1.1 mm slot (0.2 mm total clearance); print the slotted part flat so the slot is an XY feature.
Combine Cut, Keep Tools	Model the peg on part A, Combine Cut it from part B with Keep Tools, then Offset Face the socket by `clr`. Exact fit, one edit.
Test coupon	Print one peg/socket pair at three clearances before printing a kit. Calibrate `clr`, then never think about it again.

Checking before export

two minutes that save a print

Section Analysis through the thinnest wall; Measure I the smallest positive detail and the smallest gap. Anything under the table above: thicken, or delete.
Interference between the bodies of one component: colour bodies must report zero.
Display Component Colors ⇧N: one glance shows which bodies are which.
Hide reference meshes, canvases and mould tools; Save As Mesh exports what is visible.
Look at the model from below (ViewCube Bottom): the face that goes on the bed should be flat and unbroken.

What the INDX is

CORE One + Bondtech passive toolchanger

The INDX is a conversion kit for the Prusa CORE One / CORE One+: one Smart Head on the gantry carries the extruder drive, an induction coil and a load cell; each of the four or eight tools is a passive nozzle-and-filament-path with no heater, motor or wiring, parked in docks on the front panel. The head picks a tool, induction-heats its nozzle in seconds, prints, and parks it. A change takes roughly 12–16 s and purges about 13 mg into a wastebin, so there is no wipe tower in the official profiles. Tool XY offsets are measured by an eddy-current sensor at the start of every print. Firmware Buddy 6.6.0+; the slicer is PrusaSlicer 2.9.6 with the INDX printer profile installed through Configuration › Configuration Wizard (an online update, not bundled). Tools print in ascending number order and Tools Mapping is not available on INDX: load spools to match the tool numbers you sliced with.

nozzle	type	use
0.4 CHT hardened	ships in the kit	bases, infill, the only size the official profiles cover
0.5 · 0.6 · 0.8 · 1.0 CHT	optional	bases, terrain, big shells
0.25 · 0.4 standard	optional	0.25 is the finest INDX tool Bondtech lists — no 0.2 mm INDX nozzle exists at the time of writing; 0.2 mm work stays on the plain Nextruder, or treat a 0.25 tool as the fine one and read this sheet's 0.2 figures as 0.28 mm lines

Mixed nozzle sizes per tool are physically fine but "experimental" in 2.9.6 (put the fine nozzle on Tool 1, widths to auto, and read the experimental-nozzles article first). PrusaSlicer 3.0 alpha handles per-tool nozzles properly but is an alpha — slice real work in 2.9.6.

The rule: one body per colour, no overlaps

why

PrusaSlicer assigns an extruder per object part. Where two parts overlap, which tool wins is undefined; where they leave a gap, the slicer prints a gap. So the bodies must form an exact partition: the red roof body ends on the same face where the white wall body begins. Fusion gives you that for free when both bodies come from one solid split in two, because the halves share the face exactly and the export triangulates it identically on both sides.

split at a plane or sketch — waterline, storey line, bandModify › Split Body · body + splitting tool (offset plane, sketch, surface) · Extend splitting tool carve one colour out of another — inlay, lettering, window framesmodel the detail as a New Body overlapping the base → Modify › Combine · target base · tool detail · Cut · Keep Tools ✓ raised detail of a second colour — trim, rivets, lampsExtrude / Emboss as New Body starting exactly on the base face (Start › Object); do not Join a face's colour without volume (paint in slicer)skip CAD; paint in PrusaSlicer (§11) — or Split Face for the preview only checkInspect › Interference on the bodies of the component → must report nothing; Section Analysis through the boundary

Keep every colour body in the same component. Their positions are then shared and one Save As Mesh › One File exports the whole part as one 3MF with the bodies as parts.

Name and colour the bodies

Browser › Bodies

Fusion writes each body into the 3MF as an object with the body name, and PrusaSlicer shows that name in its Object list. Name bodies by role and filament: walls-cream, roof-red, trim-white, glass-clear. Give each an Appearance (A) in the filament colour so the Fusion canvas previews the print — PrusaSlicer ignores 3MF colours from CAD, but the preview stops you exporting a roof that is still white.

Give every colour body a different Appearance. Fusion's 3MF writer has been seen merging bodies that share an appearance into one mesh; distinct appearances keep them distinct, and doubles as the visual key. If a 3MF ever arrives merged or scattered, export One File Per Body as STL and multi-select the files in PrusaSlicer — bodies from one design share an origin, so they land registered.

Prefix names with the tool number when a design is settled — T1-walls, T2-roof — and the slicer step becomes press 1, press 2.

How thin can a colour be?

0.2 mm nozzle · 0.4 in brackets

feature	minimum	why
a coloured line or stroke	0.25 mm (0.5)	one extrusion line is 0.22 mm (0.45); Arachne drops anything under ~25 % of the nozzle
a proper two-perimeter stroke	0.45 mm (0.9)	two lines side by side, room for infill between them
gap between two colours (if not touching)	0.22 mm (0.45)	otherwise they fuse into one
colour band or inlay depth (Z)	2 layers, whole layers	one top layer over one interface layer; use `n * layer`
raised second-colour detail	0.3–0.8 mm proud	reads at arm's length; a single 0.1 mm layer disappears
lettering (bold sans)	2–3 mm cap height (5–6)	each stroke at least two lines wide
text stroke	≥ 0.45 mm (0.9)	so each letter is two perimeters

XY size compensation is applied per object in PrusaSlicer, so with separate colour parts it opens a hairline at the boundary — leave it at 0 for multi-colour objects. Same-material colours (PLA on PLA) bond on their own; for PLA + PETG or TPU inserts turn on Use beam interlocking in the slicer.

Patterns for models

recipes

Two-tone hull	hull solid → Offset Plane at the waterline → Split Body → name `hull-black` / `hull-red`. Boot-topping: split twice.
Brick building with stone quoins and a slate roof	walls body; quoins as a New Body extruded from the wall face (Start › Object) → Combine Cut keep tools; roof as its own body sitting on the top face; window frames extruded proud as a fourth body.
Lettering on a wagon side	Sketch › Text on a tangent plane → Extrude `2layer` into the side as New Body* → Combine › Cut, Keep Tools → letters become `lettering-white`. Inlay prints flush; raised lettering prints proud and reads better at 1:87.
Window glazing	Model the glass as a body 2 layers thick inside the frame; print with a clear or light filament on its own tool; no assembly.
Coloured roof tiles / corrugation	Keep it one colour and let geometry do the texture: Pattern on Path or Rectangular Pattern of a small cut. Colour changes cost tool changes per layer; texture costs nothing.
Trackwork	Rails and sleepers as two bodies from one Sweep + Pattern; rail head ≥ 0.45 mm wide at any scale.
Figures and vehicles (1:87 and down)	One body, one tool. Sub-millimetre colour regions do not print. Paint.

Budgeting tool changes

time, not filament

Each change is about 15 s. A layer that touches four colours changes tools three or four times; a 200-layer building with four colours on every layer is ~12,000 s of changes — over three hours added. Waste is negligible (13 mg per change), time is not.

Stack colours in Z where you can: a coloured base band, then walls, then roof — each layer touches one or two tools.
Bring the same-colour details together in one body (all white trim on the whole building is one body, not thirty).
Print the roof separately if it is a different colour and sits on a flat face: a peg joint costs nothing and saves a change on every layer of the walls.
PrusaSlicer's preview (Tool changes legend and the time estimate per feature) shows the cost before you commit.

Save As Mesh

right-click a body or component in the Browser

Selection	Right-click the component to export every visible body in it; a single body exports only itself. Hidden bodies are skipped — hide the reference mesh and the mould tools first.
Format	3MF (carries units, body names and positions) · STL binary / ASCII (unitless, one shell) · OBJ.
Unit Type	Millimeter. 3MF records it; STL does not, and PrusaSlicer will ask "…seems to be defined in inches" for anything tiny — answer No for a genuinely small mm model.
Structure	One File for a multi-colour part (bodies become parts of one object, positions kept) · One File Per Body for a kit of separate prints (files are named `design_body`).
Refinement	Low · Medium · High · Custom: Surface Deviation (how far a facet may sit from the true surface), Normal Deviation (angle between adjacent facets), Max Edge Length, Aspect Ratio. Preview Mesh shows the triangle count.
Send to 3D Print Utility	Optional; Custom lets you pick PrusaSlicer.app. The macOS picker sometimes refuses to show it — untick, save the 3MF and open it from the slicer instead. Nothing is lost.

Refinement for small models

"High" is tuned for parts in the tens of millimetres. A 1:160 dome 6 mm across shows facets at High; set Custom, surface deviation 0.005 mm, normal deviation 5° and the curves come out smooth at any cost in file size the slicer will not notice. Flat-sided buildings are indifferent to refinement.

Utilities › Make › 3D Print is the same dialog with an extra choice: continue in the Manufacture workspace's Additive setup instead of exporting. For a Prusa, export.

Into PrusaSlicer

2.9.6 · CORE One INDX profile selected first

1 · printerSidebar › Printer: Original Prusa CORE One INDX (from the Configuration Wizard's online update); Filament rows for tools 1–8, click each colour swatch to set the preview colour 2 · import⌘I Import STL/3MF… or drag the 3MF in → Multi-part object detected — "…should the file be loaded as a single object having multiple parts?" → Yes if it did not ask(the prompt is a heuristic and needs a multi-extruder printer active) select every object › right-click › Merge — parts keep their positions 3 · assign toolsObject list › expand the object › click a part's Extruder swatch, or select the part and press 1–8, or right-click › Change extruder 4 · checkSlice → preview legend by Tool; look at the time estimate and the tool-change count 5 · exportExport G-code (.bgcode) → USB, or Send to printer via PrusaLink / Prusa Connect

PrusaSlicer's own 3MF project (File › Save Project) is the file to keep: it stores parts, tool assignments, painting, modifiers and all three profiles. Re-importing a Fusion 3MF starts the assignment from scratch.

Colour without CAD bodies

painting, modifiers, layer changes

Multimaterial painting `N`	Left toolbar. First/Second colour on left/right mouse; Brush (sphere/circle, size), Smart fill (stops at a sharp edge; angle threshold), Bucket fill, Height range; clipping plane to reach inside. Stored on triangles, so it survives save and reload. Best for faces of a single body — a coloured door in a wall body.
Segmentation settings	Print Settings › Multiple Extruders › Advanced: Interface shells, Maximum width of a segmented region (paint as a skin N mm deep instead of solid), Interlocking depth of a segmented region.
Modifiers	Right-click › Add modifier › Box / Cylinder / Sphere / Slab / Text / SVG; set its extruder → the intersection with the model prints in that tool. A modifier box across a hull is a two-minute waterline.
Height range modifier	"Layers" under the object › + a range › cog › extruder. Colour bands by height.
Colour change at a layer	Layer slider › + → M600 / Add extruder change on a multi-tool printer. A lettered sign in two colours with one body.

Painting ignores XY size compensation and can merge thin features into the neighbouring colour; keep painted regions ≥ 0.45 mm wide or enable Detect thin walls.

Multiple Extruders settings

Print Settings tab

Perimeter · Infill · Solid infill extruder	0 = current tool (no extra change). Set infill to a cheap colour only if the walls are opaque — two perimeters of light PLA show a dark infill.
Support material / interface extruder	0 keeps supports in the current tool. A dedicated tool with breakaway or soluble filament for the interface is where an 8-tool head pays for itself on figures and overhangs.
Wipe tower	Leave as the INDX profile sets it (off or tiny — purging goes to the wastebin). If a profile turns it on: position, width, No sparse layers, per-object Wipe into this object's infill.
Ooze prevention	Temperature drop for idle tools. Passive INDX tools cool on the dock, so the profile's default is what you want.
Use beam interlocking	Cross-hatched beams across a material boundary so PLA + PETG or TPU hold. Off for same-material colour work; incompatible with a non-zero Maximum width of a segmented region.
Purging volumes…	Right panel button. INDX purges 13 mg per change by design; only raise it for dark-to-light changes that show ghosting.
Label objects	Output options; writes part names into G-code so the printer's Cancel object works.

Small-model slicer settings

the ones that change the result

Layer height	0.07–0.10 mm on the 0.2 nozzle for detail, 0.15 for speed (keep under 80 % of the nozzle, 0.16). First layer 0.15. Variable layer height (toolbar) thins layers only across domes and slopes — but not with Organic supports.
Perimeters	2, or 3 for tiny strong parts; Extra perimeters on overhangs on.
Arachne	Default generator. Minimum feature size 25 % of nozzle = 0.05 mm on the 0.2 (drop to 10 % if hairline detail vanishes); Minimum perimeter width 85 % = 0.17 mm.
Slice gap closing radius	0.049 default; 0.1 if a split-body model shows hairline gaps between colours.
Elephant foot	~0.2 mm in Prusa profiles; drop to 0–0.1 mm on parts with footprints under ~2 mm or the first layer vanishes.
Supports	Organic for figures and overhangs; paint enforcers/blockers with `L`; support on build plate only for buildings.
Cooling	Slow down if layer time below 15 s — small layers otherwise melt; tool changes add natural cooling on the INDX.
Scale · Place on face	Object manipulation panel: % or absolute size, per axis or locked; `F` place on face (scale up first on very small parts — it misbehaves on tiny faces).
Brim	Per-object via Add settings › Skirt and brim; outer brim 3 mm on tall thin models.

Scripts and Add-Ins

⇧S · Utilities › Add-Ins

where scripts live on this Mac ~/Library/Application Support/Autodesk/Autodesk Fusion 360/API/Scripts/<Name>/<Name>.py + .manifest ~/Library/Application Support/Autodesk/Autodesk Fusion 360/API/AddIns/ add-ins: same shape, can Run on Startup the dialog Create (name, Python or C++, script or add-in) · Run · Edit (opens VS Code with the Fusion debugger extension) · Details ▸ Full Path interpreter Fusion's own Python 3.14 inside the app bundle; adsk.core, adsk.fusion, adsk.cam are only importable there units in the API centimetres and radians, always — ValueInput.createByString('12 mm') converts for you

Text Commands (⌥⌘C) is a one-line Python console for poking at app.activeProduct. The Fusion App Store has community add-ins; AnyShortcut gives hotkeys to commands that lack them.

A script that builds and exports

skeleton

import adsk.core, adsk.fusion, traceback def run(context): app = adsk.core.Application.get(); ui = app.userInterface try: design = adsk.fusion.Design.cast(app.activeProduct) root = design.rootComponent s = design.userParameters.add('s', adsk.core.ValueInput.createByString('1/87'), '', 'scale') sk = root.sketches.add(root.xYConstructionPlane) sk.sketchCurves.sketchLines.addTwoPointRectangle( adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(12.0*s.value, 8.0*s.value, 0)) # metres → cm × s prof = sk.profiles.item(0) ext = root.features.extrudeFeatures inp = ext.createInput(prof, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) inp.setDistanceExtent(False, adsk.core.ValueInput.createByString('3.2 m * s')) body = ext.add(inp).bodies.item(0); body.name = 'walls-cream' em = design.exportManager o = em.createC3MFExportOptions(root, '/Users/you/Desktop/house.3mf') # or createSTLExportOptions(body, path) o.meshRefinement = adsk.fusion.MeshRefinementSettings.MeshRefinementHigh em.execute(o) except: if ui: ui.messageBox('Failed:\n' + traceback.format_exc())

Other entry points: root.occurrences.addNewComponent(adsk.core.Matrix3D.create()) for a component, root.bRepBodies, root.features.combineFeatures / splitBodyFeatures for the colour split, design.allParameters, ui.selectEntity(prompt, filter) to ask for a pick, app.log() for the text-commands window. Setting meshRefinement resets the four custom deviation values — set it first, then override surfaceDeviation (cm).

Autodesk Assistant

⇧H · the button top-right

A docked chat panel that knows the open design. It answers how-do-I questions, runs commands and changes preferences, and — the useful part for this workflow — writes and executes Fusion API Python from a description: "split the body hull at the plane Waterline and name the halves hull-black and hull-red", "pattern the window cut 6 times at bay_pitch", "export every body in the active component as one 3MF at high refinement". It shows the script before running it. Treat it as a script author whose output you read: it is fast at the boring parametric plumbing and confidently wrong about your intent.

Personal-plan availability of the Assistant's script-execution actions has moved over 2026; if the button offers only Q&A, the API route above still works.

Headless companions

when Fusion is the wrong tool

Fusion has no headless mode — a script needs the application open. For a prompt-to-print chain the design stage can instead be CadQuery or OpenSCAD (code in, STL/3MF out, no clicks), with PrusaSlicer's command line doing the slicing:

"/Applications/Original Prusa Drivers/PrusaSlicer.app/Contents/MacOS/PrusaSlicer" --load printer.ini --load print.ini --load filament.ini --center 125,110 --export-gcode -o part.bgcode part.3mf

The CLI slices one bed per run, cannot paint or assign tools per part (that lives in the saved project 3MF), and its auto-arrange has crashed on this platform — use the GUI for multi-colour and multi-part work, the CLI for repeat single-tool parts.

Sketch › Create

SKETCH tab

Line LCreates lines and arcs.

2-Point Rectangle RCreates a rectangle using two points for the diagonal corners.

Center Diameter Circle CCreates a circle using a center point and diameter.

Fit Point SplineCreates a spline through the selected fit points.

MirrorMirrors the selected sketch curves about a selected sketch line.

Sketch Dimension DCreate sketch dimensions for sketch geometries. Use dimensions to control the size or position of sketch objects.

Midpoint LineCreates a line that is symmetrical from the midpoint.

3-Point RectangleCreates a rectangle using three points to define width, direction, and height.

Center RectangleCreates a rectangle using two points to define the center and one corner.

2-Point CircleCreates a circle defined by two points.

3-Point CircleCreates a circle defined by three points.

2-Tangent CircleCreates a circle tangent to two sketch lines.

3-Tangent CircleCreates a circle tangent to three sketch lines.

3-Point ArcCreates an arc using three points.

Center Point ArcCreates an arc using three points.

Tangent ArcCreates an arc with tangency.

Arc by LengthArc from a start point, direction and arc length.

Arc by Center & AngleArc from a center point, a start point and a sweep angle.

Circumscribed PolygonCreates a polygon using the center point and the midpoint of one edge.

Inscribed PolygonCreates a polygon using the center point and a vertex.

Edge PolygonCreates a polygon by defining a single edge and the position of the polygon.

EllipseCreates an ellipse defined by a center point, major axis and a point on the ellipse.

Center to Center SlotCreates a linear slot defined by placement and distance of slot arc centers, and by slot width.

Overall SlotCreates a linear slot defined by orientation, length and width.

Center Point SlotCreates a linear slot defined by a center point, location of slot arc centers, and by slot width.

3-Point Arc SlotCreates an arc slot defined by a three point center arc and slot width.

Center Point Arc SlotCreates an arc slot defined by a center point, two point center arc and slot width.

Center Radius SlotArc slot defined by a center point, radius, start and end, and slot width.

Control Point SplineCreates a spline driven by the selected control points.

Control Point Spline (degree 5)Creates a spline driven by the selected control points.

Coil (sketch)Sketch a 2D spiral (planar coil) by center, revolutions and pitch.

Conic CurveCreates a curve driven by endpoints and Rho value. Depending on the Rho value, the curve can be elliptical, parabolic, or hyperbolic.

PointCreates an individual sketch point to use as reference geometry.

TextCreates text inside a rectangular frame or along a selected path, which you can use as a profile to create 3D geometry.

Fit Curves to Mesh SectionFits lines, arcs and splines to a mesh section sketch so the mesh outline becomes editable sketch geometry.

Circular PatternDuplicates selected sketch curves in an arc or circular pattern.

Rectangular PatternDuplicates sketch curves in rows and columns.

Project PProjects the body silhouette, edges, work geometries and sketch curves into the active sketch plane.

IntersectProjects the points, model edges, work geometries, and sketch curves that intersect the active sketch plane.

Spun ProfileRotates selected geometry around a specified axis and projects a 2D spun profile on to the active sketch plane.

Include 3D GeometryInclude edges, work geometry, and sketch curves into the current sketch.

Project to SurfaceProject sketch geometry, edge, vertex, or workpoint to selected faces.

Intersection CurveCreates a 3D sketch curve from intersecting geometry.

Isoparametric CurveCreates smooth curves along a face in the U or V direction.

Sketch › Modify

SKETCH tab

Sketch FilletPlaces an arc of a specified radius at the intersection of two lines or arcs.

Trim TTrims a sketch curve to the nearest intersecting curve or boundary geometry.

Offset OCopies the selected sketch curves a specified distance from the original curves.

Blend CurveCreates a tangent or curvature continuous blend curve between the endpoints of two sketch curves or edges.

Chamfer · equal distanceCreates a chamfer at the vertex, intersection, or apparent intersection of two lines in a sketch, based on an equal distance to each side.

Chamfer · distance & angleCreates a chamfer at the vertex, intersection, or apparent intersection of two lines in a sketch, based on a single distance and an angle.

Chamfer · two distancesCreates a chamfer at the vertex, intersection, or apparent intersection of two lines in a sketch, based on a different distance to each side.

ExtendExtends a curve to the nearest intersecting curve or boundary geometry.

BreakBreaks a sketch entity into two or more segments where it intersects other sketch entities.

Sketch ScaleScales sketch geometry.

Move MMoves the selected face, body, sketch, or construction geometry a specified distance or angle.

Change ParametersDisplays the Parameters dialog, where you can create and manage equations and relationships to control the size of objects.

Sketch › Constraints

SKETCH tab

AutoConstrain (AI)Generates options using AI technology to automatically dimension and constrain your sketch. Review the proposals and select the one that best suits your needs.

AutoConstrain from datumPlace a datum point to align the constraints and dimensions to, then AI technology automatically generates options with dimension and constraints added your sketch.

Horizontal / VerticalConstrains a single line, or two points, to lie on either the vertical or horizontal axis, whichever is closer to the current alignment.

CoincidentConstrains the position of two points or a point and a line or curve together.

TangentConstrains a curve and another object so that they touch at a single point but never cross each other.

EqualConstrains similar objects so that their sizes are identical. When the size of one object changes, the others adjust, too.

ParallelConstrains two lines so that they extend in the same direction and never intersect.

PerpendicularConstrains two objects so that they lie perpendicular (at a 90-degree angle) to each other.

Fix / UnFixLocks the size and location of a point or object.

MidpointConstrains a point or object to the midpoint of another object.

ConcentricConstrains two or more arcs, circles, or ellipses to the same center point.

CollinearConstrains two or more objects so that they share a common line.

SymmetryConstrains two or more objects so that they are symmetrical (identical to each other in relation to a common axis).

Curvature (G2)Constrains two or more objects to create a smooth, continuous curvature between them (G2 continuity).

Polygon constraintConstrains a closed sketch profile with sides of the same length and equal angles as a regular polygon.

Solid › Create

SOLID tab

Create SketchEnters Sketch mode, where you create geometric profiles that define the foundation of a design. Then use commands like Extrude, Revolve, and Loft to create 3D bodies from sketches.

Create FormEnters Form mode and inserts a form feature into the timeline. Use form tools to create and edit history-free bodies by pushing and pulling on vertices, edges, and faces.

DerivePushes and links design features from the active design into a new or existing design.

Automated ModelingGenerates design alternatives between geometries in space that you want to connect.

Extrude EAdds depth to open or closed sketch profiles or faces.

RevolveRevolves a sketch profile or planar face around a selected axis.

SweepSweeps a sketch profile, planar face, or a solid body along a selected path.

LoftCreates a transitional shape between two or more sketch profiles or planar faces.

RibCreates a thin feature from an open sketch profile, extruded to the nearest faces on a solid body. The rib feature is extruded in a direction parallel to the sketch plane.

WebCreates a thin feature from an open sketch profile, extruded to the nearest faces on a solid body. The web feature is extruded in a direction perpendicular to the sketch plane.

EmbossRaises or recesses a sketch profile relative to faces on a solid body by a specified depth and direction.

Hole HCreates a hole based on user-specified values and selections.

ThreadAdd internal or external threads to cylindrical geometry. Threads can be cosmetic or modeled on the geometry.

BoxCreates a solid box.

CylinderCreates a solid cylinder.

SphereCreates a solid body sphere.

TorusCreates a solid torus.

CoilCreates a solid coil.

PipeCreates a solid pipe that follows a selected path.

Stock ModelCreates a solid component around a selected component, body, or set of bodies.

Rectangular PatternDuplicates faces, bodies, features, or components in a design and distributes them along linear axes in rows and columns to create a rectangular pattern.

Circular PatternDuplicates faces, bodies, features, or components in a design and distributes them around a linear axis to create a circular pattern.

Pattern on PathDuplicates faces, bodies, features, or components in a design and distributes them to create a pattern along a specific path.

Geometric PatternCreates a pattern with size and distribution gradients across a face on a solid body.

MirrorCreates a copy of selected faces, bodies, features, or components, mirrored across a plane.

ThickenAdds thickness to surface faces to create a solid body.

Boundary FillCreates, joins or removes volumes using bounding volumes formed by tool selections.

Find FeaturesIdentifies features in a body. Recognized features are listed in the browser.

Fluid VolumeCreates the surrounding volume from selected bodies. Surrounding volume can be internal or external to the bodies. The surrounding volume is created in a new component.

Create Base FeatureEnters direct editing mode and inserts a history-free feature in the timeline. Actions performed while in the Base Feature are not recorded in the timeline.

Joint OriginPositions a joint origin on a component. Joint origins define the geometry used to relate a joint's components.

Solid › Modify

SOLID tab

Press Pull QModifies the selected geometry using offset, extrude, or fillet commands. The operation depends on the geometry selected.

Edit FaceConverts the selected face to T-Spline faces, edges, and vertices for modification.

Fillet FRounds the edges of a solid body by adding material to interior edges and removing material from exterior edges.

ChamferBevels the edges of a solid or surface body by removing material from exterior edges or adding material to interior edges.

ShellOffsets the walls of a solid body to create a hollow cavity with walls of a specified thickness.

DraftApplies a fixed or parting line draft angle to planar faces.

ScaleScales sketch objects, bodies, or components.

CombineJoins, cuts, or intersects two or more solid bodies to create a single solid body.

Offset FacesShifts the selected face or faces in a positive or negative direction.

Replace FaceReplaces one or more part faces with different face. The new face must completely intersect the part.

Split FaceDivides faces using a selected profile, face, or plane as the cutting tool.

Split BodyCreates new bodies by dividing selected bodies using a profile, face, or plane.

Silhouette SplitSplits a body using surfaces generated from its silhouette curves.

Move MMoves the selected face, body, sketch, or construction geometry a specified distance or angle.

AlignMoves an object (component, body, sketch, work geometry) by aligning geometry selected from the object with geometry selected elsewhere.

Delete ⌫Permanently deletes selected objects, and everything related to them, from the design. Does not create a feature in the timeline. Deleted objects cannot be restored parametrically.

RemoveDeletes selected components or bodies from the design and preserves the operation as a feature in the timeline. Removed objects can be restored parametrically.

ArrangeQuickly arrange items on a plane or sketch for manufacturing.

Remove FeaturesAutomatically deletes features from selected objects.

Remove FacesDeletes selected faces.

Replace with PrimitivesReplaces selected objects with primitive shapes.

Physical MaterialAssigns physical materials to components and bodies in a design to control their thermal, mechanical, strength, and advanced engineering properties, as well as their appearance.

Appearance AAssigns appearances to components, bodies, or faces in a design to override the color and texture of their physical materials, without affecting physical engineering properties.

Manage MaterialsOpens the Material Browser, where you can manage physical materials and appearances in user-defined material libraries.

Change ParametersDisplays the Parameters dialog, where you can create and manage equations and relationships to control the size of objects.

Compute All ⌘BComputes all of the parameters, features, and assembly relationships in a design.

Compute UnresolvedComputes only the features related to unresolved external components in the assembly.

Convert (T-Spline → BRep)Converts a T-Spline form body into a solid or surface BRep body (or the reverse) so solid tools can be used on it.

Assemble

SOLID tab

Insert into Current DesignInserts the selected component into the current design.

New ComponentCreates a new internal or external component in the assembly.

Duplicate with JointsDuplicates components in an assembly and the joints attached to them.

Constrain ComponentsPositions components with mate-style relationships (planar, concentric, tangent) instead of joints.

Joint JPosition components relative to each other in an assembly, then defines the relative motion between them.

As-Built Joint ⇧JCreates a Joint relationship between two components in their current position and defines their relative motion.

Rigid GroupLocks the relative position of the selected components. The components are treated as a single object when moved or when joints are applied.

Tangent RelationshipCreates a tangent relationship between a face on a body in one component and a set of connected faces on a body in another component within an assembly.

Drive JointsSpecify the rotation angle or distance value for joint degrees of freedom.

Motion LinkDefines rotational and translational relationship between joint degrees of freedom.

Motion StudyPerforms kinematic motion analysis based on joints.

Enable Contact SetsActivates contact analysis between components in contact sets. Contact sets are managed in the browser.

Enable All ContactActivates contact analysis for all components.

Disable ContactTurns off contact analysis for all component.

New Contact SetCreates a contact set between selected components.

Configure

SOLID tab · not on Personal

ConfigureOpens the Configuration Table, enters Configuration Mode, and highlights configurable features and objects in the Timeline and Browser.

Show Configure panelShows or hides the Configure dialog without entering Configuration Mode.

Configuration RulesCreates logical Configuration Rules that drive or limit configured aspect values in a Configured Design, to ensure only valid configurations can be created.

Construct

planes · axes · points

Coordinate SystemCreates a custom coordinate system that you can reference in assembly relationships, manufacturing setups or other downstream workflows.

OffsetCreates a Construction Plane that is offset from the selected face or plane.

Plane At AngleCreates a Construction Plane through an edge, axis, or line at a specific angle.

Tangent PlaneCreates a Construction Plane that is tangent to a face.

MidplaneCreates a Construction Plane at the midpoint between two faces or planes.

Perpendicular PlaneCreates a Construction Plane that is perpendicular to a plane or face.

Plane Through Two EdgesCreates a Construction Plane that passes through two edges or axes.

Plane Through Three PointsCreates a Construction Plane that passes through three points or vertices.

Plane along PathCreates a Construction Plane normal to an edge or sketch line.

Axis Through Cylinder/Cone/TorusCreates a Construction Axis through the center of a cylinder, cone or torus.

Axis Perpendicular At PointCreates a Construction Axis that is perpendicular to a face and passes through a specific point.

Axis Through Two PlanesCreates a Construction Axis coincident with the intersection of two faces or planes.

Axis Through Two PointsCreates a Construction Axis that passes through two points or vertices.

Axis Through EdgeCreates a Construction Axis along a linear edge or sketch curve.

Point At VertexCreates a Construction Point at an existing point or vertex.

Point Through Two EdgesCreates a Construction Point at the intersection or extended intersection of two edges.

Point Through Three PlanesCreates a Construction Point at the intersection or extended intersection of three non-parallel planes or faces.

Point At Center Of Circle/Sphere/TorusCreates a Construction Point at the center of a circle, sphere, or torus.

Point At Edge And PlaneCreates a Construction Point at the intersection of a linear edge, sketch line, or axis with a face or plane.

Point Along PathCreates a Construction Point at a specific distance along the path.

Inspect

SOLID tab

HistoryDisplays the version history of the selected component.

Change SummaryDisplays a list of changes made to the current assembly and its external references.

Measure IMeasures the distance, angle, area, or position of selected objects.

InterferenceReports the interference between selected solid bodies or components.

Find Similar ComponentsFinds components in your hub that are similar to those in the active design.

Curvature CombDisplays a comb with sample points along selected edges of a body to help you analyze the curvature of a surface.

Zebra AnalysisDisplays alternating black and white stripes on a body to help you analyze the curvature of a surface.

Draft AnalysisDisplays a color gradient on the faces of selected bodies to help evaluate the manufacturability of your design.

Curvature Map AnalysisDisplays a color gradient on bodies to help you analyze areas of high and low surface curvature.

Isocurve AnalysisApplies UV mapping and curvature combs to analyze the quality of a surface.

Accessibility AnalysisUsed to colorize an object based on whether or not certain parts of the object are accessible from a particular plane.

Minimum Radius AnalysisDisplays colors on the model that represent the minimum radius for the curvature of the concave faces.

Section AnalysisCreates a view that cuts through all visible objects in a design to reveal interior details and obscured features.

Center of MassDisplays a center mark glyph at the center of mass for the selected objects.

Degree of FreedomDisplays Degree of Freedom of each component in the Assembly.

Assembly StatisticsDisplays Assembly Statistics of the Assembly.

Display Component Colors ⇧NDisplays each component in an assembly as a different color to make them easier to differentiate. Hides physical materials and appearances.

Display Face Groups ⇧FDisplay face groups on mesh bodies to make them easier to work with. Hides component colors, physical materials and appearances.

Graph ViewShows how data elements connect in a visual graph.

Insert

SOLID tab

DecalPlaces an image on a selected face as a cosmetic decal.

CanvasPlaces an image on a planar face or sketch plane.

Insert T-Spline (.tsm)Inserts a saved T-Spline body (.tsm) into the active form.

Insert SVGImports an SVG file into the active sketch.

Insert DXFInserts geometry from a DXF file into the active sketch.

Insert MeshInserts an existing STL, OBJ, or 3MF file as a mesh body into the active component in a design.

FastenersInserts a fastener into the active document.

Insert DerivePulls and links design features from another design into the active design. When you update the derived features in the original design, the changes are reflected in the destination design.

Insert McMaster-Carr ComponentInsert a McMaster-Carr Component into the active document.

Select

SOLID tab

SelectSelection is always active and the active selection mode displays here.

Window Select 1Selects objects enclosed in a rectangular selection area.

Freeform Select 2Selects objects enclosed in an irregular (lasso) selection area.

Paint Select 3Press and hold the left mouse button and move across objects to select them.

Select by NameSelects bodies or components by the name used in the Browser.

Select by BoundarySelects objects using a boundary shape you choose.

Select by SizeSelects bodies or components within a size range that you specify.

Invert SelectionSwitches the selection state of all objects.

Seed & Boundary FacesAutomatically creates a selection set that includes faces on a solid or surface body that are located between a set of boundary objects and a seed object.

Component DragEnables or disables the movement of components by dragging in the canvas.

Body PrioritySets the selection filter to Bodies, and prevents selection of other object types.

Face PrioritySets the selection filter to Body Faces, and prevents selection of other object types.

Edge PrioritySets the selection filter to Body Edges, and prevents selection of other object types.

Component PrioritySets the selection filter to Components, and prevents selection of other object types.

Selection FiltersSpecifies which object types can be selected.

Position

SOLID tab

Capture PositionCaptures the positions of recently moved/rotated components as an event in your timeline. This information is used by geometry and assemble commands.

Revert PositionReturns the components to the previous position and rotation.

Surface › Create

SURFACE tab · beyond Solid

New ComponentCreates a new internal or external component in the assembly.

ExtrudeAdds depth to open or closed sketch profiles or planar faces.

Revolve (surface)Revolves a sketch profile or edge around an axis to create a surface body.

Sweep (surface)Sweeps a profile or edge along a path (optionally with a guide rail) to create a surface body.

LoftCreates a smooth shape that transitions between two or more sketch profiles or faces.

PatchFills a closed loop of edges or sketch curves with a surface; continuity options (connected, tangent, curvature).

RuledCreates a ruled surface from edges at a distance and angle — the fast way to make draft walls or flanges.

Offset (surface)Copies faces a set distance from the originals as a new surface body (distance 0 = a copy).

BoxCreates a surface body box.

CylinderCreates a surface body cylinder.

SphereCreates a surface sphere.

TorusCreates a surface torus.

CoilCreates a surface coil.

PipeCreates a surface pipe that follows a selected path.

Surface › Modify

SURFACE tab · beyond Solid

TrimRemoves the part of a surface on one side of a cutting sketch, surface or plane.

UntrimRestores trimmed regions of a surface, removing holes or extending the edges.

ExtendEnlarges a surface by extending its edges a specified distance.

StitchJoins touching surfaces into one surface body; if they close a volume the result becomes a solid.

UnstitchSeparates a stitched surface body (or a solid) into individual surfaces.

MergeMerges adjacent faces of a surface body into a single face.

Reverse NormalFlips the normal direction of a surface, which decides which side Thicken and Offset grow from.

Form › Create

FORM tab (T-Splines)

New ComponentCreates a new internal or external component in the assembly.

BoxT-Spline box; set the face counts per side before you place it.

PlaneFlat T-Spline plane with a chosen face grid — the start for panels and hull halves.

CylinderT-Spline cylinder with face counts around and along.

SphereT-Spline sphere; a quadball usually gives a cleaner topology.

TorusT-Spline torus.

QuadballSphere built from six quad patches — no poles, so it edits smoothly.

PipeT-Spline pipe along a path or edges, with per-section diameters.

FaceDraws new T-Spline faces by clicking points, or by extending existing edges.

ExtrudeExtrudes sketch curves or T-Spline edges into a T-Spline surface.

RevolveRevolves a sketch profile into a T-Spline body.

SweepSweeps a profile along a path as a T-Spline body.

LoftCreates a transitional shape between two or more sketch profiles or planar faces.

Form › Modify

FORM tab

Edit FormThe main form tool: drag, rotate and scale vertices, edges and faces with the manipulator (Alt-drag extrudes).

Edit by CurveReshapes a T-Spline by editing a curve that its selected edges follow.

Insert EdgeAdds an edge loop next to a selected edge, adding control where you need detail.

SubdivideSubdivides selected faces into more faces (simple or exact).

Insert PointInserts vertices on edges or faces.

Merge EdgeJoins two open edge loops of the same body into one continuous surface.

BridgeConnects two sets of faces or edges with a tube of new faces.

Fill HoleCloses an open edge loop with a fill star, a collapsed vertex or a single face.

Erase and FillDeletes selected faces and refills the hole smoothly — removes detail without leaving a gap.

Weld VerticesMerges two vertices into one.

UnWeld EdgesSplits the body along selected edges.

CreaseMakes edges sharp; the surface is no longer smooth across them.

UnCreaseReturns creased edges to smooth.

Bevel EdgeAdds parallel edges either side of a selection to tighten a corner while keeping it smooth.

Slide EdgeMoves an edge loop along the surface between its neighbours.

SmoothAverages vertex positions to smooth a region.

CylindrifyPulls a selected loop of faces onto a cylinder.

PullSnaps vertices onto a target body or surface.

FlattenMoves selected vertices onto a common plane.

StraightenPuts selected vertices on a straight line.

MatchMatches a T-Spline edge to a sketch curve or BRep edge with position, tangent or curvature continuity.

InterpolateMoves vertices onto the smooth surface so control points sit on the shape itself.

ThickenGives an open T-Spline surface a wall thickness (sharp or soft edges).

FreezeLocks selected faces so edits elsewhere cannot move them.

UnFreezeUnlocks frozen faces.

Form › Symmetry

FORM tab

Mirror - InternalMakes an existing body symmetric about a plane through it; edits on one side mirror to the other.

Circular - InternalRadial symmetry within an existing body.

Mirror - DuplicateDuplicates a body as a mirrored copy that stays linked to it.

Circular - DuplicateDuplicates a body around an axis as linked copies.

Clear SymmetryRemoves symmetry from the body.

Isolate SymmetryShows only one symmetric portion while editing.

Form › Utilities

FORM tab

Display Mode (box / smooth)Switches between box (control cage), control frame and smooth display.

Repair BodyFinds and fixes T-Spline errors (star points, T-points) that block conversion to a solid.

Make UniformRe-spaces control points evenly; use before Convert if the body fails.

Cap SettingsSets how open ends of primitives are capped.

Mesh › Create

MESH tab

Insert MeshInserts an existing STL, OBJ, or 3MF file as a mesh body into the active component in a design.

TessellateConverts an existing solid or surface body into a mesh body.

Create Mesh Section SketchCreates a sketch that contains a section line where a plane intersects a mesh body.

Create Mesh (empty base feature)Creates an empty Mesh Base Feature.

Mesh › Prepare

MESH tab

RepairRepairs a mesh body to prepare it for further design and manufacturing operations.

Generate Face GroupsAutomatically generates face groups on a mesh body using the normal angles between faces to determine the boundaries of each face group.

Combine Face GroupsCombines two or more adjacent face groups on a mesh body.

Create Face GroupCreates a face group from a selection of faces on a mesh body.

Mesh › Modify

MESH tab

Direct EditCreates a mesh base feature that you can edit directly.

RemeshRefines or coarsens faces on a mesh body or face groups.

ReduceReduces the number of faces on a mesh body to minimize complexity.

Plane CutUses a plane to trim or split a mesh body.

Shell (mesh)Hollows the interior of a mesh body.

Combine (mesh)Joins, intersects, cuts, or merges two or more mesh bodies to create a single mesh body.

SmoothSmooths rough or creased regions on a mesh body.

Smooth BoundarySmooths the boundary edges of a mesh body.

Reverse NormalReverses the normal direction of selected faces on a mesh body.

Erase And FillRemoves and replaces faces on a mesh body to fill holes and repair regions.

BridgeBridges two regions of a mesh body by creating connecting geometry between them.

Mesh AlignAligns a face on a mesh body to a plane with one transformation.

Attract to ReferenceAttracts selected faces on a mesh body towards a reference mesh body.

Texture ExtrudeUses an image to add surface texture to a mesh body.

SeparateSeparates regions of a mesh body into independent mesh bodies.

Scale MeshScales mesh bodies from a reference point.

RemoveRemove meshes

Convert MeshConverts a mesh body to a solid or surface body.

Convert To Quad MeshConverts a mesh body or face groups with triangular faces to a mesh body or face groups with quad faces.

Utilities › Make

UTILITIES tab

3D PrintPrepares solid or mesh bodies to be 3D printed directly from Fusion's Manufacture workspace or from an external application.

Utilities › Add-ins

UTILITIES tab

Scripts and Add-Ins ⇧SManage Scripts and Add-Ins

Fusion App StoreOpens the Autodesk App Store for Fusion add-ins.

Join ate the colour body

Operation

Extrude and the primitives default to Join whenever the new shape touches an existing body. The roof merges into the walls, you export one body, and the slicer has nothing to assign. Check the Operation drop-down on every colour feature; it should read New Body. If it already happened: roll back, or Split Body along the face that used to be the boundary.

Bodies in the root, not the component

activation

Sketching without activating the part's component puts the sketch and the body in the root. Everything still works until you pattern, joint or export the component and half of it is missing. Watch the radio button in the browser; drag stray bodies onto the component to move them.

Scale scaled the walls

Modify › Scale

Scaling a 1:1 building by 1/87 turns a 300 mm wall into 3.4 mm (fine) and a 20 mm window mullion into 0.23 mm (one hair of a line on the 0.2 nozzle, nothing on a 0.4). Nothing warns you; the slicer simply drops the feature. Either model at scale with max(real * s; 0.25 mm) floors, or after scaling run Inspect › Measure over every thin feature.

Fillet failed after an edit

red timeline

Fillets and chamfers reference edges; when an earlier feature moves or removes those edges the fillet goes red and everything after it may too. Put fillets last in the timeline, prefer Tangent Chain selections (fewer explicit edges), and when one breaks, edit it and reselect rather than deleting it.

The slicer did not ask about parts

Multi-part object detected

The "single object having multiple parts" prompt only appears with a multi-extruder printer profile active, and even then it is a heuristic — same-size stacked bodies can slip through as separate objects. Select all, right-click, Merge. Or export One File Per Body and multi-select the files on import, which asks reliably.

PrusaSlicer ignored the colours

3MF appearances

Fusion writes appearance colours into the 3MF; PrusaSlicer 2.9 reads geometry and names only. Colours in Fusion are for your preview. Tools are assigned in the Object list, and only PrusaSlicer's own project 3MF stores them.

Two bodies became one part

shared appearance

Bodies that share the same Appearance can come out of Fusion's 3MF export merged into a single mesh, so two colour regions arrive in PrusaSlicer as one part. Give each colour body its own appearance before exporting, or fall back to one STL per body.

Overlapping colour bodies

undefined precedence

Two parts occupying the same volume with different tools: which prints is not specified and can change between slices. Make the bodies a partition — Split Body, or Combine Cut with Keep Tools — and run Interference before export. A hairline gap is the mirror problem: the slicer prints it as a gap; raise Slice gap closing radius or fix the split.

Inches? No.

STL units

STL has no units. A 15 mm N-scale hut looks like a 0.6 in object to PrusaSlicer, which offers to multiply by 25.4. Say No — or export 3MF, which carries millimetres and never asks.

High refinement is not high enough

tiny curves

Refinement presets are tuned for parts tens of millimetres across. A 6 mm dome at "High" prints visibly faceted at 0.1 mm layers. Custom: surface deviation 0.005 mm, normal deviation 5°.

The 10-document wall

Personal

The eleventh editable design refuses to save. The limit is per hub, not per open tab; flip finished designs to Read-only in the Data Panel (they still open and export), keep a kit as one design with many components, and export .f3d archives to disk as the only offline backup you have.

Send to 3D Print Utility cannot see PrusaSlicer

macOS file picker

A long-standing Mac bug hides PrusaSlicer.app from the Custom-utility picker. Untick Send to 3D Print Utility, save the 3MF, and open it from PrusaSlicer or with open -a PrusaSlicer part.3mf. The utility only launches the app with the file anyway.

Tool numbers are the tool numbers

no Tools Mapping on INDX

The XL lets you remap extruders on the printer's screen before a print; the INDX does not. What you assigned as Tool 3 in PrusaSlicer prints from dock 3. Load the spools to match, and put the fine nozzle on Tool 1 if you mix sizes — tools print in ascending order.

Faceted convert of a big mesh

Mesh › Convert

Converting a 500 k-triangle STL faceted gives a body with 500 k faces; every later fillet, section and export crawls. Reduce first, convert only what you must Boolean, and keep the original mesh as a hidden reference.

Fusion parametric CAD for scale models that print in colour

01 · Fusion in One Page

Five ideas that carry the rest of the sheet

The order a professional actually works

Promoting what you already drew

02 · Navigation & Hotkeys

Sketch

03 · Sketch

04 · Solid Modelling

05 · Components, Joints & Timeline

06 · Parameters & Design Intent

07 · Surface, Form & Mesh

A hull in five features

08 · Scale Modelling

09 · Designing for the Nozzle

10 · Multi-Colour for INDX

11 · Export & Slice

Refinement for small models

12 · Scripts, API & Assistant

13 · Command Index

14 · Traps