PartDesign Pad/ro

Start

Sets where the pad begins. By default the pad starts at the sketch or face used as its profile. introduced in 26.3

• Profile plane (default): the pad starts directly at the profile's sketch plane or face.
• Offset: the pad starts at a numerical distance from the profile, entered in the Start Offset field.
• Reference: the pad starts at a face, datum plane, or sketch selected with the Pick Reference button.

This is useful to create multiple features from a single master sketch without needing separate offset planes for each one.

Direction

You can select how the pad is created:

• One sided: the pad extends on one side of the face.
• Two sided: the pad extends on both sides of the face. Two sub-menus (Side 1 and Side 2) appear to define the pad for each side.
• Symmetric: the pad is symmetrical with respect to the original face.

To last

The pad will extend up to the last face of the support it encounters in its direction. If there is no support, an error message will appear.

To first

The pad will extend up to the first face of the support it encounters in its direction. If there is no support, an error message will appear.

Up to face

The pad will extend up to a face. Press the Select face button and select a face or a datum plane from the Body.

Two dimensions

This allows to enter a second length in which the pad should extend in the opposite direction. The directions can be switched by checking the Reversed option.

Up to shape

introduced in 1.0: The pad will extend up to the selected shape. Optionally press the Select shape button and select a shape. Leave the Select all faces checkbox enabled or disable it, press the Select faces button and select the faces up to which the pad should be created.

Offset to face

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

2nd length

Defines the length of the pad in the opposite direction. This option is only available if Type is Two dimensions.

Reverses the direction of the pad.

Direction

Direction/edge

You can select the direction of the extrusion:

• Sketch normal or Face normal: The sketch or face is extruded in the direction of its normal. If you have selected several sketches or faces to be extruded, the normal of the first one will be used.
• Select reference…: The sketch or face is extruded in the direction of a straight edge or a datum line selected from the Body.
• Custom direction: The sketch or face is extruded in the direction of the specified vector.

Show 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 or face normal, otherwise along the custom direction.

Taper angle

Tapers the pad in the extrusion direction by the given angle. A positive angle means the outer pad border gets wider. Note that inner structures receive the opposite taper angle. This is done to facilitate the design of molds and molded parts. This option is only available if Type is Dimension or Two dimensions.

2nd taper angle

Tapers the pad in the opposite extrusion direction by the given angle. See Taper angle. This option is only available if Type is Two dimensions.

Data

Pad

Part Design

• DateRefine (Bool): 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).

Sketch Based

• DateProfile (LinkSub)
• DateMidplane (Bool)
• DateReversed (Bool)
• DateAllow Multi Face (Bool)

Start

• DateStart Type (Enumeration): sets how the pad start is defined (Profile plane, Offset, Reference), see Options. introduced in 26.3
• DateStart Offset (Length): distance between the profile and the start of the pad. Only used if DateStart Type is Offset. introduced in 26.3
• DateStart Reference (LinkSub): a face, plane, or sketch the pad starts from. Only used if DateStart Type is Reference. introduced in 26.3

• Like all Part Design features, Pad creates a solid, thus the sketch must include a closed profile or it will fail with a Wire is not closed error.
• Sketches containing B-Splines often cannot be tapered properly. This is a limitation of the OpenCASCADE kernel that FreeCAD uses.
• For larger angles tapering will fail if the end face would have fewer edges than the start face/sketch.
• The algorithm used for To First and To Last is:
  • Create a line through the center 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 an unresolved bug.