PartDesign Pad

Description
The tool extrudes a sketch into a solid in a direction normal to the sketch plane. As of faces on the solid can also be used.



Sketch (A) shown on the left; end result after pad operation (B) on the right.

Note: If the selected sketch is mapped to the face of an existing solid or another Part Design feature, the pad will be fused to it.

Usage

 * 1) Select the sketch to be padded. Note: As of  a face on the existing solid can alternatively be used.
 * 2) Press the  button.
 * 3) Set the Pad parameters, see the Options below.
 * 4) Click.

Options
When creating a pad, the Combo view automatically switches to the Tasks pane, showing the Pad parameters dialog.



Type
Type 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.

Length
Defines the length of the pad. Multiple units can be used independently of the user's units preferences (m, cm, mm, nm, ft or ', in or ").

Direction/edge
You can select the direction of the padding:


 * Sketch normal The sketch is extruded along its normal
 * Select reference... The sketch is extruded along an edge of the 3D model. When this is method selected, you can click on any edge in the 3D model. This becomes then the direction vector for the padding.
 * Custom direction The sketch is extruded along a direction that can be specified via vector values.

Show custom direction
If checked, the pad direction will be shown. In case the pad uses a Custom direction, it can be changed.

Length along sketch normal
If checked, the pad length is measured along the sketch normal, otherwise along the custom direction.

Offset to face
Offset from face in which the pad will end. This option is only available when Type is either To last, To first or Up to face.

Symmetric to plane
Tick the checkbox to extend half of the given length to either side of the sketch plane.

Reversed
Reverses the direction of the pad.

Properties

 * : Type of ways how the pad will be extruded, see Options.
 * : Defines the length of the pad, see Options.
 * : Second pad length in case the option TwoLengths is used, see Options.
 * : If checked, the pad direction will not be the normal vector of the sketch but the given vector, see Options.
 * : Vector of the pad direction if  is used.
 * : If true, the pad length is measured along the sketch normal. Otherwise and if  is used, it is measured along the custom direction.
 * : A face the pad will extrude up to, see Options.
 * : Offset from face in which the pad will end. This is only taken into account if the option UpToLast, UpToFirst or UpToFace is used.
 * : true or false. Cleans up residual edges left after the operation. This property is initially set according to the user's settings (found in Preferences → Part design → General → Model settings). It can be manually changed afterwards. This property will be saved with the FreeCAD document.

Limitations

 * Like all Part Design features, Pad creates a solid, thus the sketch must include a closed profile or it will fail with a Failed to validate broken face error. There can be multiple enclosed profiles inside a larger one, provided none intersect each other (for example, a rectangle with two circles inside it).
 * 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 [[Image:Workbench_Part.svg|16px]] Part workbench with (which creates an unlinked, non-parametric solid) or with the  from the [[Image:Workbench_OpenSCAD.svg|16px]] OpenSCAD Workbench which creates a parametric feature.