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, …). Double-click another dimension to edit it: the current value is applied, as Enter does (if it is not valid, the box stays open with its error), and the clicked dimension opens with its value selected. Single-click another driving dimension to insert 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. The name goes in a moment after the click, once it is clear the click was not the first of a double-click. 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.

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.

The Filter box lists the parameters whose name, expression, comment or group contains what you type, in any case. It also finds a name by the starts of its words, in order: toodia, toofla and outdia all find tooth_outward_flange_diameter. Underscores, hyphens and camelCase (boltHoleDepth) separate the words. Autocomplete offers parameters the same way.

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. One is the exception: a new Solid Fillet’s radius opens at the 2 mm the tool ships with, shown in the design’s units (“0.07874 in” in an inch design), because a radius is bound by the faces beside its edges. 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). In a CSV, a value that a spreadsheet would run as a formula is written with a ' before it, so the spreadsheet shows it as text. That is a value that starts with =, +, - or @, their full-width forms, a tab or a line break, after any spaces and '; a plain number such as -5 is left as it is. The import takes the ' off again. A spreadsheet that saves the file again as CSV can drop the ' (Excel does), so export again from SolidCraft instead of passing that file on. Earlier versions of SolidCraft wrote every value unchanged, so in a CSV from one of them, a value whose first character really was a ' typed before a formula character ('=x) now imports without it (=x). 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.

Use Compare Parameter Variants when several parameters must change together. Each named variant starts from the same open design, so values from one variant never carry over to the next. For example, compare a pair of bracket sizes:

{"command": "inspect.parameter_variants", "params": {"variants": [
  {"name": "Compact", "set": {"Width": "40 mm", "Thickness": "4 mm"}},
  {"name": "Wide", "set": {"Width": "60 mm", "Thickness": "6 mm"}}
]}}

The command accepts up to 12 variants with up to 16 existing parameters each. It returns the baseline’s volume, mass and body counts, then one result per variant in input order. The result reports new feature, joint or sketch regressions using the same checks as Parameter Sweep. A refused expression is an error for that variant; later variants still run. A variant with a rebuild regression has no metrics. Open bodies do not count toward volume or mass. The design and its undo history are unchanged.