Line Law of Face Extension

Surface creation

To create a surface, choose two geometrical elements: Face and Guides.

Face. The initial face can belong to the surface or a solid body.

Guides. The initial face must lie within the face, can be comprised of several elements and either be smooth or have fractures. The directrix can be closed.

The surface being built is determined by two main features: Height and Angle.

Height. Determines the generatrix length set by the distance from the directrix to the free edge of the surface.

Angle. Determines the angle between the generatrix and the normal to the initial face built at the point lying at the directrix.

1 – Guides 2 – surface free edge 3 – Height 4 – Angle

Breakage processing

In case the directrix is not smoothly joint and has fractures, the surface being built can have breakages or self-intersections. To deal with such cases there is a special option Extend for fracture processing in the command. In this case the surfaces are extended to intersection or vice versa, cut along the intersection line. In case there is no need for such processing, select the Split variant.

There is the third processing variant: Round. In this case the breakage section will be filled with a surface whose cross-section is a circular arc tangent to the surfaces.

If there is no breakage section, i.e. the planes were “cut” along the intersection line, the option Round is not available.

In case the directrix has fractures and lies at an uneven face, the Angle parameter can only be equal to zero. In all other cases the Angle parameter can have any value.

Building a body

General parameters

Thickness can be added to the surface being created. In this case the surface will be pushed along the normal at a given value. The pushing value of the surface is determined by Offset parameter. Pushing variants can be selected from Thickness list. By default variant No is selected, i.e. the system builds a surface by default.

Roundings

In case the initial face belongs to a solid body, users can create grooves representing the trace of a mill with the help of Law Extension command. To do it you need to build the surface inwards the body: select Inside variant in Extension parameter. The groove thickness relative to the directrix is set by thickness adding variants and Offset parameter value. To get the obtained body subtracted from the body containing the initial face, select the Boolean operation Subtraction variant. End edges or faces can be rounded which imitates the mill trace. To do this, select the rounding variant: Edges or Faces. If you select Faces variant, end faces will be cylindrical surfaces with a radius equal to half the thickness of the groove obtained.

If the directrix has fractures, they can be processed when creating the body. Select the Round variant in the Kinks parameter. In this case a rounding will be created at the external body bend which is equal to half the body thickness. In case the Edges variant is selected in the Rounding parameter, the external body bend will be rounded with a radius specified in the Radius field. The options listed enable users to imitate a mill with a given diameter creating a groove.

 

It is possible to define Height and Angle via a graph depending on a guide length.

Clicking the button invokes a graph type selection dialog. Then the graph can be edited using the T-FLEX CAD Graph editor.

Topics in this section:

•Solid Body Creation when Extending Face by Line Law

•Surface Creation when Extending Face by Line Law