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Sketcher workbench icon

Introduction

The Sketcher workbench features "constraints", allowing 2D shapes to follow precise geometrical definitions in terms of length, angles, and relationships (horizontality, verticality, perpendicularity, etc.). A constraint solver calculates the constrained-extent of 2D geometry and allows interactive exploration of degrees-of-freedom of the sketch.

A fully constrained sketch

Basics of constraint sketching

To explain how the Sketcher works, it may be useful to compare it to the "traditional" way of 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 afterwards. 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?

Instead of dimensions, Constraints are used to limit the degrees of freedom of an object. For example, a line without constraints has 4 Degrees Of Freedom (abbreviated as " DOF "): it can be moved horizontally or vertically, it can be stretched, and it can be rotated.

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, thus leaving it with 3 degrees of freedom. Locking one of its points in relation to the origin will remove another 2 degrees 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. A complex Sketch with multiple objects will have a number of different solutions, and making it fully-constrained means that just one of these possible solutions has been reached based on the applied constraints.

There are two kinds of constraints: geometric and dimensional. They are detailed in the 'The tools' 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. Constraints 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. Unlike Sketcher elements, Draft objects don't use constraints; they are simple shapes defined at the moment of creation. Both Draft and Sketcher can be used for 2D geometry drawing, and 3D solid creation, although their preferred use is different; the Sketcher is normally used together with Part and PartDesign to create solids; Draft is normally used for simple planar drawings over a grid, as when drawing an architectural floor plan; in these situations Draft is mostly used together with the Arch Workbench. The tool Draft2Sketch converts a Draft object to a Sketch object, and vice versa; many tools that require a 2D element as input work with either type of object as an internal conversion is done automatically.

Sketching Workflow

A Sketch is always 2-dimensional (2D). To create a solid, a 2D Sketch of a single enclosed area is created and then either Padded or Revolved to add the 3rd dimension, creating a 3D solid from the 2D Sketch.

If a Sketch has segments that cross one another, places where a Point is not directly on a segment, or places where there are gaps between endpoints of adjacent segments, Pad or Revolve won't create a solid. Sometimes a Sketch which contains lines which cross one another will work for a simple operation such as Pad, but later operations such as Linear Pattern will fail. It is best to avoid crossing lines. The exception to this rule is that it doesn't apply to Construction (blue) Geometry.

Inside the enclosed area we can have smaller non-overlapping areas. These will become voids when the 3D solid is created.

Once a Sketch is fully constrained, the Sketch features will turn green; Construction Geometry will remain blue. It is usually "finished" at this point and suitable for use in creating a 3D solid. However, once the Sketch dialog is closed it may be worthwhile going to Part Workbench and running to ensure there are no features in the Sketch which may cause later problems.

The tools

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

General

• New sketch: Creates‎ a new sketch on a selected face or plane. If no face is selected while this tool is executed the user is prompted to select a plane from a pop-up window.
• View sketch: Sets the model view perpendicular to the sketch plane.
• Reorient sketch: Allows you to attach the sketch to one of the main planes.
• Validate sketch: Verify the tolerance of different points and adjust them.
• Stop operation: when in edit mode, stop the current operation, whether that is drawing, setting constraints, etc.

Sketcher geometries

These are tools for creating objects.

• Line: Draws a line segment between 2 points. Lines are infinite regarding certain constraints.
• Create an arc: This is an icon menu in the Sketcher toolbar that holds the following commands:
• Arc: Draws an arc segment from center, radius, start angle and end angle.
• Arc by 3 points: Draws an arc segment from two endpoints and another point on the circumference.
• Create a circle: This is an icon menu in the Sketcher toolbar that holds the following commands:
• Circle: Draws a circle from center and radius.
• Polyline (multiple-point line): Draws a line made of multiple line segments. Pressing the M key while drawing a Polyline toggles between the different polyline modes.
• Rectangle: Draws a rectangle from 2 opposite points.
• Create Regular Polygon : Draws a regular polygon by selecting the number of sides and picking two points: the center and one corner.
• Slot: Draws an oval by selecting the center of one semicircle and an endpoint of the other semicircle.
• Fillet: Makes a fillet between two lines joined at one point. Select both lines or click on the corner point, then activate the tool.
• Trimming: Trims a line, circle or arc with respect to the clicked point.
• Construction Mode: Toggles sketch geometry from/to construction mode. Construction geometry is shown in blue and is discarded outside of Sketch editing mode.

Sketcher constraints

Constraints are used to define lengths, set rules between sketch elements, and to lock the sketch along the vertical and horizontal axes. Some constraints require use of Helper constraints.

Geometric constraints

These constraints are not associated with numeric data.

• Coincident: Affixes a point onto (coincident with) one or more other points.
• Point On Object: Affixes a point onto another object such as a line, arc, or axis.
• Vertical: Constrains the selected lines or polyline elements to a true vertical orientation. More than one object can be selected before applying this constraint.
• Horizontal: Constrains the selected lines or polyline elements to a true horizontal orientation. More than one object can be selected before applying this constraint.
• Parallel: Constrains two or more lines parallel to one another.
• Perpendicular: Constrains two lines perpendicular to one another, or constrains a line perpendicular to an arc endpoint.
• Tangent: Creates a tangent constraint between two selected entities, or a co-linear constraint between two line segments. A line segment does not have to lie directly on an arc or circle to be constrained tangent to that arc or circle.
• Equal: Constrains two selected entities equal to one another. If used on circles or arcs their radii will be set equal.
• Symmetric: Constrains two points symmetrically about a line, or constrains the first two selected points symmetrically about a third selected point.

Dimensional constraints

These are constraints associated with numeric data, for which you can use the expressions. The data may be taken from a spreadsheet.

• Lock: Constrains the selected item by setting vertical and horizontal distances relative to the origin, thereby locking the location of that item. These constraint distances can be edited later.
• Horizontal distance: Fixes the horizontal distance between two points or line endpoints. If only one item is selected, the distance is set to the origin.
• Vertical distance: Fixes the vertical distance between 2 points or line endpoints. If only one item is selected, the distance is set to the origin.
• Distance: Defines the distance of a selected line by constraining its length, or defines the distance between two points by constraining the distance between them.
• Diameter: defines the diameter of a selected arc or circle by constraining the radius.
• Angle: Defines the internal angle between two selected lines.

Sketcher tools

• Show/Hide internal geometry: Recreates missing/deletes unneeded internal geometry of a selected ellipse, arc of ellipse/hyperbola/parabola or B-spline.

Best 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).
• If you have the possibility to choose between the Length constraint and the Horizontal or Vertical Distance constraints, prefer the latter. Horizontal and Vertical Distance constraints are computationally cheaper.
• In general, the best constraints to use are: Horizontal and Vertical Constraints; Horizontal and Vertical Length Constraints; Point-to-Point Tangency. If possible, limit the use of these: the general Length Constraint; Edge-to-Edge Tangency; Fix Point Onto a Line Constraint; Symmetry Constraint.
• If in doubt about the validity of a sketch once it is complete (features turn green), close the Sketcher dialog, switch to the Part Workbench and run .