Sketch

The command can be called in one of the following ways:

The command is used for creating graphic lines independent of construction elements. Optionally, you can link created line to a 2D node using object snapping.

Parametrization of Sketch

With the help of a sketch, you can create a non-parametric drawing, a parametric drawing or a combination of the both. Non-parametric drawings do not share the advantage of parametric drawings in the effective dimensions modification. However, in certain cases, creating such drawings is faster, requires less resources for constructions calculation and can bring certain benefits, when large modifications are not expected. Parametric drawings are created by applying constraints and driving dimensions to sketch lines. Sketching with constraints can be used either as an independent way of creating parametric drawings, or in combination with the classic for T-FLEX CAD parametrization based on the construction lines. Parametrization based on sketching with constraints makes it possible to eliminate dependence on the order of the constructions, giving the user more freedom. If you remove constraints, the parametric sketch becomes non-parametric. Conversely, after creating a nonparametric sketch, you can apply constraints to it, thus making a drawing or some of its parts parametric.

Object snappings define positions of sketch lines only at the moment of line creation. It doesn't result in creating associative link between created line and object of snapping (except snapping to a 2D node). Sketch lines stay independent of each other, until you apply constraints. Therefore, lines, that were initially visually connected (e.g. sides of a polygon), may change their relative positions upon further changes of the drawing.

If you want to create associative links between sketch lines, so that their geometrical relations to be kept upon further changes of the drawing, you have to apply constraints (parametrize the sketch) or snap characteristic points of lines to 2D nodes.

During sketch creation, the automatic constraints creation and automatic dimensions creation modes can be enabled in the snapping toolbar. If you combine the automatic dimensions creation with the driving dimensions creation mode (available in the ribbon), then driving dimensions will be automatically created.

After creating a sketch you can apply constraints and driving dimensions either manually using the Constraint and Dimension commands, or automatically using the Find and Infer Constraints command.

Any line of the sketch can be made auxiliary. Auxiliary lines are displayed in drawing window and participate in parametrization, but they're non-printable.

Automenu options

Different automenu options are used for creating different types of lines and performing some actions with existing lines. Descriptions of using certain options can be found in separate sections of the help system. In order to open a description of a certain option, follow the link in the option's name below.

Upon calling the command, following options are available in the automenu:

This option is active by default. In result, the ending point of the previous line, arc or spline is automatically used as the starting point of the current line or arc. The option takes effect only, when creating a line or an arc. When creating other sketch elements, the option is present in the automenu, but has no effect.

Continuous creation doesn't create associative links between connected lines. If you move such line later, its starting and ending points will be disconnected from other lines. In order to keep the connection between lines, upon further changes in the sketch geometry, use constraints (parametrize the sketch).

Most of the sketch options may also be called directly from the ribbon:

The Symmetry option is only available in the ribbon.

Both in the automenu and in the ribbon, similar options are grouped into drop-down lists. There are differences in grouping between the automenu and the ribbon.

Topics in this section:

•Point

•Line

•Circular Arc

•Circle

•Rectangle

•Polygon

•Parallelogram

•Slot

•Ellipse and Elliptical Arc

•Spline and Polyline

•Axis Lines

•Chamfer and Fillet

•Modifying Sketch Lines

•Offset

•Symmetry

•Sketch Line Parameters

•Edit Sketch

See Also:

•Auxiliary Lines