How a design is built

SolidCraft is a parametric, history-based modeller. You don’t shape geometry directly: you describe the steps that make it, and SolidCraft computes the result from those steps. Change a step or a value and everything after it is computed again. This page explains that idea and the usual ways of working with it. The pages after it cover each tool in detail; the glossary defines most of the terms used here.

The idea in one paragraph

A design holds a timeline: an ordered list of features. Most parts start with a sketch, a 2D drawing on a plane, held in shape by constraints and dimensions. A feature such as Extrude or Revolve turns the sketch’s closed regions into a solid body; later features add to it, cut into it or finish it (holes, fillets, shells). Every dimension and feature input is a parameter, so a size can be changed at any time, and the timeline rebuilds from the first feature that uses it.

sketch (plane + constraints + dimensions)
   └─ feature (extrude, revolve, …)  →  body
         └─ more features (holes, fillets, patterns, shell, …)
               └─ change a parameter  →  the timeline rebuilds

Principles that make a design easy to change

• Capture intent, not just shape. A hole “centred on the face” or “10 mm from that edge” stays right when the part grows; a hole placed by eye doesn’t. Use constraints and dimensions for what matters, and name the important values as parameters (type width = 40 in any value box: see Parameters and expressions).
• Fully constrain sketches. Under-constrained sketch geometry is drawn blue and the Sketch Palette shows how many degrees of freedom are left; once none are, the geometry changes colour (white in the default dark theme) and the status reads Fully constrained (see Sketching and constraints). A fully constrained sketch changes only the way you tell it to.
• Keep sketches simple, let features do the work. A rectangle and an extrude, then a fillet, is easier to change than one sketch that draws the rounded outline. Holes, patterns, mirrors, fillets and chamfers are features of their own for the same reason.
• Build in a sensible order. The base shape first, then the features that add and cut, then the finishing features (fillets, chamfers, shell, draft). Features depend on the ones before them, so an early change ripples forward.
• Sketch on stable references. An origin plane (XY, XZ, YZ, or Top, Front, Right) or a construction plane changes less than a face that a later edit may remove.

The timeline is the design

The timeline, the History strip along the bottom of the window, lists every feature in the order it is computed. Each feature can be edited (double-click), suppressed, renamed, reordered when nothing it depends on moves after it, and deleted; deleting asks first when other features depend on it.

Drag the rollback marker back to see the design as it was at an earlier step. Features after the marker are kept, not deleted, and a new feature is added at the marker. This is how you add something early in the design (a sketch the later features should use) without rebuilding the rest.

The timeline is not the undo history: Undo and Redo move back and forth through what you did; the timeline is what the design is made of.

Bodies and components

A body is one connected solid or surface shape. A design can hold many bodies, and features can make a new body, join or cut existing ones, or intersect them.

A component groups bodies, sketches and construction geometry, with its own origin, and can be placed more than once; each placement is an occurrence. Editing a component changes every occurrence of it; moving an occurrence moves only that copy. The active component (the radio button in the browser) receives new sketches and features.

Two ways of working follow from this:

• One part, several bodies. For a single part, or a few parts that are designed against each other, model bodies in one design. Bodies are quick to make and to combine, split or cut with each other.
• Components and joints. When parts are separate pieces (they move, repeat, or go on a bill of materials), make them components: New Component, or Create Components from Bodies to turn bodies you already modelled into components. Then connect them with joints (rigid, revolute, slider, cylindrical, pin-slot, planar, ball) and drive the motion. See Components and joints.

Starting with bodies and turning them into components later is a common path: it keeps the early design quick and makes the assembly when its structure is clear.

Common workflows

Everything you click is a command with named parameters, and the toolbar, scripts, the CLI and AI agents all run the same commands. A design built in the window can be turned into a script with solidcraft-cli script, which rebuilds it without the window (designs with components or joints are not supported there yet).

Terms if you come from another CAD program

Other programs use other words for the same ideas. SolidCraft uses one term for each:

The full list, with what each term must not be confused with, is in the glossary.

Finding help

• Help (?) › Documentation in the title bar opens this manual.
• Help (?) › Keyboard Shortcuts lists the shortcuts; see also Keyboard shortcuts.
• The command reference describes every command and its parameters.
• Report a bug, in the title bar, drafts an issue report with the details the maintainers need, for you to review and file on GitHub; the app doesn’t send anything itself.
• Questions and ideas: the Discord and the issue tracker.