PartDesign Pad

Introduction
'Pad a selected sketch' - This tool takes a selected sketch as its input (the 'defining sketch'), and produces with it a 'pad'. A pad is essentially an extrusion of a sketch. For example, if a sketch were made of two concentric circles, and the pad tool were subsequently used on this sketch, the result would be a cylinder:

Options
When creating a pad, the 'pad parameters' dialogue offers five different ways of specifying the length to which the pad will be extruded



Dimension
Enter a numeric value for the length of the pad. The default direction for extrusion is away (outside of) the support, but it can be changed by ticking the Reversed option. Extrusions occur normal to the defining sketch plane. With the option Symmetric to plane the pad will extend half of the given length to either side of the sketch plane. Negative dimensions are not possible. Use the Reversed option instead.

Two dimensions
This allows to enter a second length in which the pad should extend in the opposite direction (into the support). Again can be changed by ticking the Reversed option.

To last
The pad will extrude up to the last face of the support in the extrusion direction. If there is no support, an error message will appear.

To first
The pad will extrude up to the first face of the support in the extrusion direction. If there is no support, an error message will appear.

Up to face
The pad will extrude up to a face in the support that can be chosen by clicking on it. If there is no support, no selections will be accepted.
 * }

Limitations

 * The algorithm used for To First and To Last is:
 * Create a line through the centre of gravity of the sketch
 * Find all faces of the support cut by this line
 * Choose the face where the intersection point is nearest/furthest from the sketch
 * This means that the face that is found might not always be what you expected. If you run into this problem, use the Up to face type instead, and pick the face you want.
 * For the very special case of extrusion to a concave surface, where the sketch is larger than this surface, extrusion will fail. This is a unresolved bug.
 * There is no automatic cleanup, e.g. of adjacent planar surfaces into a single surface. You can fix this manually in the Part workbench with Refine shape.