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Point-level selection

bearcad.select normally targets a whole element. Point-level selection targets an individual vertex instead — a line endpoint or a circle's center — using the same point numbering the interactive Constraint tool uses.

Selecting a line endpoint​

bearcad.select{ kind = "line", index = 0, ["end"] = "start" }  -- or "end"

Selecting a rectangle corner​

A rect is four separate lines, so a corner is a line endpoint. Lines run counterclockwise from the (x, y) origin corner — 0 bottom, 1 right, 2 top, 3 left — and each corner is the start of the line with the same number:

bearcad.select{ kind = "line", index = 2, ["end"] = "start" }  -- the third corner (top-right)

Selecting a circle's center​

kind = "circle" alone selects the whole circle. Pass point = true for its center:

bearcad.select{ kind = "circle", index = 0, point = true }

Selecting a text's anchor​

A sketch text has nine anchor points — box corners, edge midpoints, center. Pass anchor to select one (without it, sketch_text selects the whole text):

bearcad.select{ kind = "sketch_text", index = 0, anchor = "center" }  -- or "top_left", …

Constraining an anchor translates the whole text to satisfy it; rotation and size never change.

Selecting a face's own vertex or edge​

While a sketch is open directly on a body's face (an extrusion cap or side wall), that face's boundary loop is selectable, so the sketch can be constrained against the face it's drawn on:

bearcad.select{
    kind = "face",
    face = { kind = "extrude_cap", extrusion = 0, profile = "polygon", profile_lines = { 0, 1, 2, 3 }, top = true },
    index = 2,
}

face takes the same table shape as bearcad.begin_sketch; index numbers the boundary loop. This selects the vertex; add edge = true for the edge from that corner to the next:

bearcad.select{
    kind = "face",
    face = { kind = "extrude_side", extrusion = 0, profile = "polygon", profile_lines = { 0, 1, 2, 3 }, edge = 0 },
    index = 0,
    edge = true,
}

Both are fixed by the body's geometry — not draggable — but plug into Coincident, Midpoint, and distance constraints like any sketch point/line. Only the sketch's own face is pickable; imported STL/STEP bodies have no analytic boundary to reference.

Selecting the origin and its axes​

Constrain a point onto an axis (pins that coordinate to 0) or onto the origin:

bearcad.line{ x = 5, y = 5, x1 = 12, y1 = 8 }
bearcad.select{ kind = "line", index = 0, ["end"] = "start" }
bearcad.select({ kind = "axis", axis = "x" }, true)   -- add the X axis
bearcad.add_geometric_constraint("coincident")         -- start point now sits on the X axis

bearcad.select{ kind = "line", index = 0, ["end"] = "end" }
bearcad.select({ kind = "origin" }, true)              -- add the origin
bearcad.add_geometric_constraint("coincident")         -- end point now sits on the origin

Interactively, dragging a point near an axis or the origin snaps it on and adds the same constraint.

Making two lines collinear​

Select two lines and apply Coincident:

bearcad.select{ kind = "line", index = 0 }
bearcad.select({ kind = "line", index = 1 }, true)
bearcad.add_geometric_constraint("coincident")         -- the two lines are now collinear

Additive selection​

Pass true as the second argument to add to the current selection instead of replacing it:

bearcad.select({ kind = "line", index = 1 }, true)

Worked example: closing a polygon loop purely from a script​

bearcad.new()
bearcad.line{ x = 0, y = 0, x1 = 10, y1 = 0, name = "a" }
bearcad.line{ x = 20, y = 0, x1 = 30, y1 = 0, name = "b" }

bearcad.select{ kind = "line", index = 0, ["end"] = "end" }
bearcad.select({ kind = "line", index = 1, ["end"] = "start" }, true)
bearcad.add_geometric_constraint("coincident")

Combine with bearcad.extrude{ polygon = {...} } to build and extrude an arbitrary closed profile without any GUI interaction.