Sketcher Workbench

The Sketcher Workbench is used to create 2D geometries intended for use in the Part Design Workbench and other workbenches. It features a constraint solver that allows sketching of geometry-constrained 2D shapes. Sketches are the basic building blocks of parametric 3D geometry creation.



Basics of constraint sketching
To explain how the Sketcher works, it may be useful to compare it to the "traditional" way of drafting.

Traditional Drafting
The traditional way of CAD drafting inherits from the old drawing board. Orthogonal (2D) views are drawn manually and intended for producing technical drawings (also known as blueprints). Objects are drawn precisely to the intended size or dimension. If you want to draw an horizontal line 100mm in length starting at (0,0), you activate the line tool, either click on the screen or input the (0,0) coordinates for the first point, then make a second click or input the second point coordinates at (100,0). Or you will draw your line without regard to its position, and move it afterward. When you've finished drawing your geometries, you add dimensions to them.

Constraint Sketching
The Sketcher moves away from this logic. Objects do not need to be drawn exactly as you intend to, because they will be defined later on by constraints. Objects can be drawn loosely, and as long as they are unconstrained, can be modified. They are in effect "floating" and can be moved, stretched, rotated, scaled, and so on. This gives great flexibility in the design process.

What are constraints?
Constraints are used to limit the [degrees of freedom] of an object. For example, a line without constraints has 4 degrees of freedom:
 * A sketch can only exist in a plane. Any single point defined on that plane can only have two degrees of freedom.
 * e.g. for the x-y plane: translational x and translational y.
 * (A point on a plane is not considered to have any rotational degrees of freedom since it is infinitesimally small and therefore its rotation is not defined.)
 * A line consists of two points joined, hence it can have 4 degrees of freedom on a plane:
 * Point 1 - translational x
 * Point 1 - translational y
 * Point 2 - translational x
 * Point 2 - translational y
 * Moving the two points variously in these 4 degrees of freedom will lead to the line experiencing movement horizontally or vertically, scaling of the line, and rotation of the line.

Applying a horizontal or vertical constraint, or an angle constraint (relative to another line or to one of the axes), will limit its capacity to rotate, leaving it with 2 degrees of freedom. Locking one of its points in relation to the origin will remove yet another degree of freedom. And applying a dimension constraint will remove the last degree of freedom. The line is then considered fully-constrained.

Multiple objects can be constrained between one another. Two lines can be joined through one of their points with the coincident point constraint. An angle can be set between them, or they can be set perpendicular. A line can be tangent to an arc or a circle, and so on.

There are two kinds of constraints: geometric and dimensional. They are detailed in section below.

What the Sketcher is not good for
The Sketcher is not intended for producing 2D blueprints. Once sketches are used to generate a solid feature, they are automatically hidden. Dimensions are only visible in Sketch edit mode.

If you only need to produce 2D views for print, and don't want to create 3D models, check out the Draft workbench (keep in mind though that the Draft workbench can also be useful to create 2D geometry not available in the Sketcher at this time, like B-Splines.)

Sketching Workflow
To be added

Good Practices
Every CAD user develops his own way of working over time, but there are some useful general principles to follow.


 * A series of simple sketches is easier to manage than a single complex one. For example, a first sketch can be created for the base 3D feature (either a pad or a revolve), while a second one can contain holes or cutouts (pockets). Some details can be left out, to be realized later on as 3D features. You can choose to avoid fillets in your sketch if there are too many, and add them as a 3D feature.
 * Always create a closed profile, or your sketch won't produce a solid, but rather a set of open faces. If you don't want some of the objects to be included in the solid creation, turn them to construction elements with the Construction Mode tool.
 * Use the auto constraints feature to limit the number of constraints you'll have to add manually.
 * As a general rule, apply geometric constraints first, then dimensional constraints, and lock your sketch last. But remember: rules are made to be broken. If you're having trouble manipulating your sketch, it may be useful to constrain a few objects first before completing your profile.
 * If possible, center your sketch to the origin (0,0) with the lock constraint. If your sketch is not symmetric, locate one of its points to the origin, or choose nice round numbers for the lock distances. In v0.12, external constraints (constraining the sketch to existing 3D geometry like edges or to other sketches) are not implemented. This means that to locate following sketches geometry to your first sketch, you'll need to set distances relative to your first sketch manually. A lock constraint of (25,75) from the origin is more easily remembered than (23.47,73.02).

The tools
The Sketcher Workbench tools are all located in the Sketcher menu that appears when you load the Sketcher Workbench.