Parameters & units

Parameters are named values like leg = 50mm that any value field can reference. Change the value and everything built on it rebuilds.

The Parameters pane

The Parameters pane lists every parameter. While a row's field is focused, the Elements pane highlights everything that uses that parameter — and hovering a row (or focusing its fields) also glows those users green in the 3D view: the dimensions referencing it, the geometry they drive, and any body whose extrude distance uses it.

Each row's eyeball marks the parameter primary (eye open) or secondary (closed). Primary parameters are the knobs someone importing this file is meant to change; secondary ones are internals. Nothing is blocked either way. A new parameter starts primary when its value is a plain number and secondary when it's an expression; the toggle is yours after that.

An imported unit's parameters

Select a unit instance and its parameters lead the pane under the instance's name — primary knobs first, with an Internals eye that reveals the secondary ones. Click a value to type a new one: the edit is an override on that one instance — the part's file and its other instances never change. Overridden values read gold; the ✕ beside one goes back to the part's own value.

bearcad.unit_override{ instance = 0, name = "width", value = "20" }
bearcad.unit_override{ instance = 0, name = "width" }   -- back to the part's value

Expressions

Every value input accepts an expression, not just a number:

• Arithmetic: + - * / and parentheses — leg / 2 + 5.
• Functions: max, min (any number of arguments, or one [a, b, c] array), abs, floor, ceil/ceiling, and round — max(w, 20), min([leg, arm, 40]), ceil(span / step).
• A unit instance's parameters, qualified by the instance name: bracket.width. Backticks wrap a single name where it has spaces — `left bracket`.width. The value is the instance's override where one is set, otherwise the part's own. One level only: a nested unit's internals aren't reachable.
• Parameter names, including inside other parameters' expressions: A + 5in.
• Mixed units: 3mm + 2in evaluates correctly. Lengths take mm, cm, m, in, ft; angles take deg, rad. A bare number is millimetres (degrees in angle fields).

The text you type is stored verbatim — reopen the field and 3mm + 2in is still there. Whenever what you typed isn't literally the resulting value, the field shows the computed result beside it — 1in shows = 25.4 mm, a bare 10 shows = 10.0 mm.

While typing a name, autocomplete offers matching parameters: Space/Tab completes, Enter completes and commits. Unit instances complete too: typing fo offers foo (backticked when the name has spaces), and foo. offers that instance's parameters — primary knobs first.

Creating parameters inline

Typing name=value in any value field — width=20mm in an extrude-distance field, say — creates that parameter on the spot and binds the field to it. A bare name= reuses an existing parameter; name=value redefines it.

Derived parameters

A derived parameter's value comes from measuring geometry. The Dimension tool in 3D mode records one from the selection with its Derive parameter button. Valid selections:

• One line or edge — its length (also on right-click: Create parameter from length).
• Two points — the distance between them (2D or 3D).
• Two parallel lines — the distance between them.
• Two non-parallel lines in the same plane — the angle between them.
• One body edge — its length.
• Two body corners — the distance between them, on one body or across two.

Derived values are read-only in the pane — a lock icon sits left of the name (hover it to see what's measured), while the name itself stays editable — and re-measure as the geometry changes. Focusing a derived parameter's row highlights the geometry that defines it; clicking into its name field draws that source geometry in green in the 3D view.

bearcad.derive_parameter{ kind = "line_length", a = 0, name = "leg" }
bearcad.derive_parameter{ kind = "line_distance", a = 0, b = 1 }
bearcad.derive_parameter{ kind = "line_angle", a = 0, b = 2 }
bearcad.derive_parameter{ kind = "point_distance",
  a = { kind = "line", index = 0, ["end"] = "start" },
  b = { kind = "line", index = 0, ["end"] = "end" } }
-- Body geometry: a/b are mm points anywhere on the picked edge's ends or the corners.
bearcad.derive_parameter{ kind = "body_edge_length", body = 0, a = {0, 0, 0}, b = {30, 0, 0} }
bearcad.derive_parameter{ kind = "body_vertex_distance", body = 0,
  a = {0, 0, 0}, b = {30, 40, 0} }

Display units

The Context pane's Default units section (Select tool, nothing selected) sets the document-wide length and angle units used for dimension labels and the Elements pane. With exactly one sketch selected it becomes Sketch units — a per-sketch override, with a Follow document entry per axis to inherit the default again.

Scripting

bearcad.parameter("add", "A", "5mm")
bearcad.parameter("value", 0, "A + 5in")     -- edit parameter 0's expression
bearcad.parameter("name", 0, "Len")
bearcad.parameter("primary", 0, true)        -- eye open / closed
bearcad.parameter("delete", 0)
assert(bearcad.parameter("get", "A") == 5)   -- evaluated (mm / radians)
bearcad.parameter("get_expression", "A")     -- "5mm", as typed

bearcad.set_units{ length = "in", angle = "deg" }          -- document defaults
bearcad.set_units{ sketch = 0, length = "mm" }             -- per-sketch override

Sizes in scripting calls accept expression strings too — see Declarative modeling.