solvecraft/docs/frames.md

Frames and weldments

Frames and weldments (#4003) are structural members (tube, angle, channel, beam, an aluminium extrusion of your own) laid along the lines of a frame sketch. This page covers what has landed: members and their profiles. Corners, trims, end caps, gussets, welds and the cut list follow.

The workflow

1. Sketch the frame: lines in a sketch, or a 3D sketch for a frame that leaves one plane (sketch.options sketch_3d: true, then sketch.line3d). Drive the sizes with parameters as usual; members follow.
2. Choose a profile: a built-in one from its dimensions (below), or your own drawn in a sketch (a vendor's extrusion: insert their DXF with sketch.insert_dxf). A profile sketch's origin is the point that sits on each line, and its x and y are the profile's.
3. Add members: Frame Member (WELDMENTS › CREATE, frame.member) makes one body per line, square to it, from its start to its end. Repeat with another profile for the next group of lines.

{"command": "frame.member", "params": {"sketch": "Frame", "profile": {"kind": "rect_tube", "width": 40, "height": 40, "wall": 3}}}
{"command": "frame.member", "params": {"sketch": "Frame", "lines": ["l5", "l6"], "profile_sketch": "45x45 section", "anchor": "bottom_left", "angle": "90 deg"}}

Members are ordinary bodies: mirror, pattern, move, drill and combine them with the usual commands. Where members meet they overlap until corner treatments land.

The Weldments ribbon tab gathers the frame commands: New Sketch, Frame Member and Parameters. Like Sheet Metal it is always there, and it selects itself when a frame member is the selected body (or the last body of the active component).

The Frame Member dialog

• Lines: pick the frame sketch's lines in the view (2D or 3D sketch lines). All Lines makes a member on every line of that sketch instead, including lines drawn later.
• Section (optional): pick the section's region in another sketch (the ring between two circles makes a tube). With nothing picked, Profile chooses a built-in profile and its dimensions follow; optional ones left empty take their defaults.
• Anchor, Angle and Mirror place the section on each line, as below. Name names the members (default: after the profile).
• The preview shows the members as you change the values. Edit Feature reopens the dialog with the feature's values; the members keep their names through the edit, and a new Name renames them all. A member made with a whole profile sketch keeps it (the Section row shows the sketch; untick it for a built-in profile).

frame.member

• sketch: the frame sketch. lines: the curve ids to lay members on (2D lines or 3D sketch lines), each once; left out, every straight line drawn in the sketch: not construction, not projected or otherwise linked (a sketch on a face projects the face's edges; they are references, not members), and with a length.
• profile (a built-in profile) or profile_sketch (a sketch), one of them. A profile sketch's section is its material as nested loops alternate (an outline is material, a loop inside it a hole, a loop inside that material again), so two circles make a tube; pick other regions with profiles as solid.extrude takes them. Like solid.extrude, only what was drawn counts: projected edges are left out unless the drawn curves make no profile. It must be one piece.
• anchor: the profile point on the line: origin (the default: a built-in profile's centre, a profile sketch's origin), center (of its bounding box), centroid, or a corner or edge middle of its bounding box (bottom_left, top…).
• Orientation: the profile's y points up (world +Z) as far as the line allows and its x is square to the line and to y (x × y runs along the line, so on a line along +X the profile's x is world +Y); a vertical member's x is world +X. angle (an angle expression) turns the profile about the line, counter-clockwise looking back from the line's end; mirror mirrors it across its y axis first. A line leaning less than 10⁻⁶ rad from vertical counts as vertical, so rounding in a 3D sketch never turns a post a quarter turn.
• Bodies are named after body_name, or the profile (Rect Tube 40x40x3) or the profile sketch, then numbered on past names already taken ((2), (3)…). Each member's name is kept with its line (the feature's names), so deleting or adding a line, or deleting another feature, leaves the other members' names alone; body.rename renames a member on its line. names ({line id: name}) gives names to keep, as Edit Feature (timeline.redefine) passes them unless the edit changes body_name.

Every built-in profile is SolidCraft's own parametric definition, built in code (solidcraft_doc::frame). SolidCraft ships no vendor's or standard's size table: you give the dimensions of the stock you buy. Any other section, a vendor's aluminium extrusion for example, comes from a sketch: draw it or insert the vendor's DXF.

Built-in profiles

A profile is JSON with a kind and its dimensions, each a number in the design's units or a length expression over its parameters ("tube_wall", "2 in"): a member follows a parameter change like any feature. Dimensions marked optional default from the profile's size when left out, made smaller where a thick section leaves less room for a radius; frame.profile.properties returns the profile in millimetres with every default written out.

Kind	Required	Optional (default)
bar	width, height	corner_radius (0)
round_bar	diameter
rect_tube	width, height, wall	outer_radius (2 × wall; inner radius is outer − wall)
round_tube	diameter, wall
angle	width (leg along x), height (leg along y), thickness	root_radius (thickness), toe_radius (thickness / 2); together at most the shorter leg's inside length
channel	height, width (flange length), web, flange (thicknesses)	root_radius (web, at most the room in a flange and half the web's inside height), toe_radius (0)
i_beam	height, width, web, flange	root_radius (web, at most the room in a flange and half the web's inside height)

The profile's bounding box is centred on its origin, x across and y up. Angles have their heel at the bottom left; channels open towards +x.

Dimensions are refused, with the dimension named, when they are not finite, are outside 0.01 mm–10 m (radii: 0, or 0.01 mm–10 m), or do not fit: a wall of half the tube or more, a radius given larger than the room for it.

Commands

• frame.profile.list: every kind, its dimensions and a working example.
• frame.profile.properties {profile, density?}: the section, worked out exactly from its lines and arcs: area (mm²), centroid (mm from the bounding box centre), ixx, iyy, ixy (mm⁴ about the centroid), width, height; with density (kg/m³), mass_per_m (kg/m).
• frame.profile.insert {profile, at?, anchor?, angle?, fixed?, sketch?}: draws the profile into the sketch being edited, its anchor point (center, centroid, or a corner or edge middle of the bounding box such as bottom_left) on at, turned by angle radians. The curves are locked (fixed, default true) so solving the sketch keeps the shape. The outline and each hole are separate sketch regions: extrude the material region (pick it with profiles: [{point}]).

{"command": "frame.profile.insert", "params": {"profile": {"kind": "rect_tube", "width": 40, "height": 40, "wall": 3}, "at": [0, 0], "anchor": "bottom_left"}}