Inventor ACU cheat sheet

The Application menu (top-left 'I' icon) holds file-level commands: New, Open, Save, Save As, Export, Print, and iProperties access.

The Quick Access Toolbar sits above the ribbon and can be customized by right-clicking any ribbon command and choosing Add to Quick Access Toolbar.

The ribbon is organized into tabs (Sketch, Model, Annotate, Inspect, Tools, Manage, View, Environments); each tab contains panels of related commands.

The browser (model tree) at the left shows feature history in creation order; the End of Part marker can be dragged upward to roll the model back to an earlier state.

A part file uses .ipt, an assembly uses .iam, a drawing uses .idw (or .dwg), and a presentation uses .ipn.

Project files (.ipj) define search paths for libraries, workgroups, and content center; the active project controls where files are resolved from.

ViewCube, SteeringWheels, and the navigation bar control orientation and zoom; F4 toggles orthographic/perspective and F6 returns to isometric home view.

iProperties (Summary, Project, Status, Custom) store metadata such as part number, description, and material that propagate to drawings and bills of materials.

Application Options (Tools tab) set global behavior such as undo count, sketch snap, and auto-save interval; Document Settings apply only to the current file.

A sketch must be attached to a work plane or planar face; unconsumed sketches remain visible in the browser and can be reused by later features.

Fully constrained geometry displays black; under-constrained geometry is blue; selected is red. The status bar shows remaining degrees of freedom.

Geometric constraints include coincident, collinear, concentric, parallel, perpendicular, horizontal, vertical, tangent, equal, symmetric, and fix.

Dimensional constraints include linear, angular, radial, diameter, and ordinate dimensions; driven (reference) dimensions display in parentheses and cannot drive geometry.

The constraint inference priority follows proximity - hold Ctrl while sketching to suppress automatic constraints, or use the Constraint Settings dialog to limit inference.

Construction geometry (toggled with the Q key or the format toggle) is ignored by profiles but usable as references for constraints and symmetry.

Sketch Doctor (Sketch tab, right-click) locates open loops, duplicate points, and overlapping geometry that prevent a profile from being extruded or revolved.

Pattern and Mirror in the sketch create constrained copies of sketch geometry; Trim (with Extend option) and Offset are sketch-modify tools, not model features.

Auto Dimension (Sketch tab) applies the dimensions needed to reach a fully constrained state based on remaining degrees of freedom.

Sketched features include Extrude, Revolve, Sweep, Loft, and Rib; placed features include Hole, Fillet, Chamfer, Shell, Draft, Thread, and Pattern.

Extrude options: Distance, Symmetric, Two Directions, To Next, To Face, To a Work Plane, and Through All; Join, Cut, Intersect, and New Solid define the boolean result.

Fillet (constant radius, variable, face) and Chamfer (distance, distance-angle, two distances) are edge features; the order of fillets affects the result on complex corners.

Hole command supports drilled, counterbore, countersink, spotface, and tapped holes; hole placement uses a sketch of points and can terminate by distance, through all, or to a face.

Pattern features include Rectangular, Circular, Mirror, and Sketch-driven; pattern occurrence counts and spacing can be suppressed per instance via the pattern dialog.

A work feature (plane, axis, point) is created by choosing references such as an offset face, a face plus an edge, or three points; work planes are consumed by features that use them.

The End of Part marker rolls the model back; features below the marker are temporarily suppressed so you can add a feature in the middle of the history.

Parameters (fx) drive dimensions by name and can be linked to a spreadsheet; user parameters can be exported to drawings and referenced in other dimensions.

Assembly constraints: Mate (faces flush or mated), Angle, Tangent, Insert (aligns two circular edges and mates faces), and Symmetry; each constraint removes degrees of freedom.

A grounded component (default: first placed part) has all degrees of freedom removed; the ground status can be toggled with the Grounded button in the Assemble tab.

Degrees of freedom remaining in an assembly are shown in the status bar; a fully constrained assembly shows zero and the component icon changes color.

Bills of materials are driven by the assembly structure: part number, quantity, and structure (normal, inseparable, purchased) come from iProperties and component settings.

Drawing views include Base, Projected, Auxiliary, Section, Detail, Break, and Overlay; a projected view inherits alignment from the parent view.

A section view is defined by a section line sketched in the parent view; the view direction and depth are set in the Section View dialog.

Dimensions in a drawing can be retrieved (Retrieve Dimensions) from the model's sketch dimensions, or placed manually; model dimensions are associative to the part.

A parts list is placed from the Annotate tab and references a view's BOM; balloons attach to the parts list item numbers and can be renumbered.