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makeCAD/docs/book/src/guide/parameters.md
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Jackson Oursland ca4f3ed1a0 Book: getting started, sheet metal and import/export get pictures (#10732)
* Book: sketching step by step, with three clips and a numbered screenshot

The sketching page now opens with a first sketch in four steps: start a sketch on the Top
plane, draw a 60 x 40 rectangle and a 12 mm circle with typed values, dimension the circle
until the sketch is fully constrained, and finish. Each step has a short clip, and the last a
screenshot numbering the Sketch tools, a constraint, a dimension, the sketch's state and
Finish Sketch.

doc_shots.py gains what these needed: a setup that runs before recording, so a clip starts
where the last one ended; sketch framing; Enter sent as two input frames; and clips that keep
their pauses (hovering a plane).

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

* Book: the sketching page's general notes get a heading after Step by step

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

* Book: sketching adds Offset and Trim; the sketching figures again on 0.29.0

Two more clips after the sketching walkthrough: Offset draws the rectangle's outline 4 mm inside
it with one click (Chain), and Trim cuts a notch where a circle crosses the top side. All the
sketching figures are made again on SolidCraft 0.29.0, with the clips keeping a moment on each
result.

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

* Book: solid features step by step, with four clips

The solid features page now opens with the sketch from the sketching page made into an open
box in four steps, each with a short clip: extrude it 12 mm, shell it with the top open,
round its outer top edges, then make it 20 mm tall from the timeline while the shell and the
fillet rebuild. The panel table and what follows get a heading of their own.

doc_shots.py: the feature shots share their steps with the setups that lead up to the next
shot, and fail when a feature on the timeline carries a warning or an error, so no figure
shows one. Shell comes before Fillet for that reason: shelling through the rounds needed the
kernel's boolean retry. trim_idle.py takes --hold, the seconds of each idle stretch to keep
(default 0.1 as before); the doc clips keep 0.8 s, so a reader sees each result. The app gets
up to three minutes to answer on a busy machine.

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

* Book: features add Hole and Circular Pattern; the Parameters dialog, numbered

The features walkthrough gains two steps before the timeline edit: a 4 mm hole on the box's
floor, then Circular Pattern repeating it four times around the tube. The edit at the end now
rebuilds all of it. The parameters page gets a screenshot of the Parameters dialog numbering
apply as you go, user parameters, model parameters by feature, an expression and its value.
The features clips are made again on SolidCraft 0.29.0.

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

* Book: components and joints step by step, with three clips

The components and joints page now opens with a two-leaf hinge in three steps, each with a
short clip: the two bodies made into components from the Bodies folder's menu (the first one
grounded), a revolute joint on their barrel ends with Flip turning Leaf B the right way round,
and a drag that swings Leaf B about the hinge while grounded Leaf A stays put. What follows
gets a heading of its own.

doc_shots.py builds the leaves from commands, with Leaf B lifted and set back so the joint
visibly brings it into place.

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

* Book: assemblies add Drive Joints; the assembly clips again on 0.29.0

A fourth step drives the hinge with Drive Joints: the slider swings Leaf B while a ghost shows
where it started, and OK keeps the new angle. The assembly clips are made again on SolidCraft
0.29.0.

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

* Book: getting started, sheet metal and import/export get pictures

Getting started gains a section on the start page: a numbered screenshot (new design, open,
import, recent, samples, the File menu) and a clip opening a sample from it. Sheet metal opens
with a tray in three steps, each with a clip: a base flange from a sketched rectangle, edge
flanges from two top edges, and the flat pattern with its bends. Import and export opens with
the File menu, numbered.

Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>

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Co-authored-by: Claude Opus 5.5 <noreply@anthropic.com>
2026-11-05 06:31:44 +00:00

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Parameters and expressions

Every dimension and feature input is a model parameter (d1, d2, …). User parameters are ones you add yourself, with a unit, an expression and an optional comment. Change them in Change Parameters (parameters.change). The timeline rebuilds from the first feature that uses them.

When creating or editing a sketch dimension, its value editor shows its model parameter name (d1, d2, …). Click another driving dimension to use its name: when the value is just a number (such as 10 or 10 mm) the name replaces it; otherwise it goes in at the cursor, replacing selected text and keeping what you typed, so typing 10 + and clicking d1 gives 10 + d1. Add arithmetic such as / 2 to build a dependent dimension. Press Enter to apply the expression or Escape to cancel the edit. Add and edit user parameters through the existing Change Parameters command.

The Parameters dialog, numbered 1 to 5

1 Apply each change as you leave its field · 2 User parameters, and Add parameter · 3 Model parameters, grouped by the sketch or feature they belong to · 4 An expression · 5 The value it works out to

Naming a value as you type it

Any value input can name its value: type width = 40 (or #width = 40) for a dimension, a value box while drawing a shape (a line's length, a rectangle's width and height, a circle's diameter: the shape is drawn at that size and its dimension uses the parameter), an extrude distance, a fillet radius, a hole diameter, a sheet metal rule, a joint's offset and so on. SolidCraft adds the user parameter width with the expression 40, and the input uses width from then on, so editing it again shows width. A bare number reads as it would in that input (the design's units for a length, degrees for an angle), and the parameter keeps that unit. The right-hand side can be any expression, such as width = depth * 2. The command and its parameter are one undo step.

Editing a value that already has its own parameter (a dimension's d7, a feature input's) with height = 12 renames that parameter to height, references following, and sets it to 12; no other parameter is made. When the value is just a parameter's name (width), width = 50 sets that parameter instead. A name that is already taken, a unit, function or constant name, or a value that refers to itself is refused with the reason, and nothing changes. A parameter's own expression and a configuration cell can't define another parameter.

Scripts, the control channel and MCP tools take the same form in any expression parameter ("distance": "depth = 15"); the result names what it made in defined (the first name) and definitions ([{name, expression, unit}]).

In the MANAGE tab's PARAMETERS section, click Parameters to open the user and model parameter editor. The Configurations button in CONFIGURATIONS opens the configuration table; Configure remains in the dropdown for configuring columns.

Press Enter in the new parameter's name, expression or comment field to add it. Valid entries return focus to the name field for the next parameter; invalid entries remain editable. In expression fields, type a parameter or dimension name for autocomplete, or press Ctrl+Space to open suggestions, including in an empty field. Up/Down selects an autocomplete suggestion, Enter/Tab accepts it, and Escape dismisses the suggestions. Accepting a suggestion does not also submit the parameter. When what you typed is already a complete name (width), longer names such as width_extra stay listed without a selection: Enter applies what you typed, and Up/Down picks one of them first. A unit right after a number (10 mm) is left alone; anywhere else a unit is a prefix like any other, so rad followed by Enter gives radius.

With Preferences › Design › Step values with the arrow keys and the wheel on (it is off by default) and no suggestions open, Up/Down step a plain number in any value field (a dialog's rows, the value box beside the geometry, a sketch dimension, a parameter's expression) by 1 in the unit it is written in: 20 mm becomes 21 mm, 2,5 mm becomes 3,5 mm. Hold Shift for 10 or Alt/Option for 0.1. The mouse wheel over the focused field does the same, a step a notch, and the preview follows each step. An expression such as width / 2 is left as typed.

Expressions are unit-aware: 2 * width + 5 mm, angle / 2, sqrt(area), 1 in + 3 mm, using + - * / ^ %, parentheses, sin cos tan asin acos atan atan2 sinh cosh tanh asinh acosh atanh sqrt abs sign min max floor ceil round trunc mod exp ln log log10 pow hypot (log is base 10) and unit conversion. A number and the unit after it are one value: 10 mm / 2 mm is 5 and 90 deg / 1 rad is π/2, and a fraction of numbers before a unit is one value too (1/2 in is half an inch; after a / only written without spaces: 1 in / 1/2 in is 2, while width / 10 / 2 mm divides by 10 and then by 2 mm). A decimal comma works too: 2,5 mm is 2.5 mm, and -(width-0,5)/2 is -(width-0.5)/2 (directly in a function's parentheses the comma separates its arguments, so write max(2.5, 3) there). A mixed number is one value, as imperial sizes are written: 2 1/8" and 3 7/16 in are 2.125 in and 3.4375 in (a whole number, a space, then a proper fraction of whole numbers). A length where an angle is expected (or the other way round) is an error, not a silent conversion. Cycles are reported with their path (a → b → a), renaming a parameter updates every expression, dimension and feature input that uses it, and a parameter in use can't be deleted (the error lists its users).

The design's units (Document Settings in the browser: mm, cm, m, in or ft) set how a bare number or unitless arithmetic expression typed into a length field is read. In an inch design 0.25 and 1 / 4 mean 0.25 in. A new user parameter given no unit (parameters.add or parameters.import without unit) is a length in the design's units, as the Parameters dialog makes it: 40/2 is 20 in. Operation dialogs start with lengths in the design's units, including secondary distances, wall thicknesses, gaps, offsets and radii. Canvas handles and live sketch values use the same units as the operation. Angles, counts and scale factors keep their own units. Preferences selects the default units for new designs; existing designs use their own Document Settings.

Explicit units override that choice: 2 mm is still two millimetres in an inch design. Parameter expressions such as width / 2 remain driving expressions. Editing a saved feature preserves its physical size; an existing millimetre expression can still show mm so accepting an unchanged field cannot reinterpret it. Computed sizes and tolerances keep their full precision when written back into editable fields, independently of display precision.

Parameters export to and import from CSV or JSON (parameters.export, parameters.import). Configurations (config.*) keep a table of rows, each with its own parameter values and suppressed features, physical materials and body appearances, switched with config.activate. The table's Library picker selects material or appearance values. Choose Follow material to clear an appearance override. Custom looks retain their colour and opacity across activation, undo and save/reopen. See configuration commands and examples.

Checking a design across a parameter's range

Parameter Sweep (inspect.parameter_sweep) rebuilds a copy of the design at each of a parameter's values and reports what no longer holds, so a design meant to be driven by its parameters (one template, many sizes) can be checked before it is trusted. The design itself is not changed.

{"command": "inspect.parameter_sweep", "params": {"parameter": "Width", "from": 300, "to": 510, "steps": 21}}

values lists the values instead (numbers or expressions). For each value it gives the rebuild's time and what changed from the design as it is now: features that fail (failed) or warn (warned), joints whose origin is no longer found (joints_lost) or turned over on its own part (joints_flipped, more than 90°), sketch planes that turned over (sketches_flipped) and sketch solves that fail or only hold by flipping a triangle's turn or an offset's side (sketches_failed). summary counts the values that show each.