|Part Design → Create an additive feature → Pad|
|Introduced in version|
The v0.17 and above faces on the solid can also be used.tool extrudes a sketch into a solid in a direction normal to the sketch plane. As of
Sketch (A) shown on the left; end result after pad operation (B) on the right.
Note: version 0.16 and below 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.
- Select the sketch to be padded. Note: As of v0.17 and above a face on the existing solid can alternatively be used.
- Press the button.
- Set the Pad parameters, see the Options below.
- Click .
When creating a pad, the Combo view automatically switches to the Tasks pane, showing the Pad parameters dialog.
Type offers five different ways of specifying the length to which the pad will be extruded.
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.
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.
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.
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.
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 ").
Use custom direction
introduced in version 0.19 If checked, the pad direction will not be the normal vector of the sketch but the given vector. The pad length is however set according to the normal vector direction.
Length along sketch normal
If checked, the pad length is measured along the sketch normal, otherwise along the custom direction. introduced in version 0.20
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.
Reverses the direction of the pad.
- DataType: Type of ways how the pad will be extruded, see Options.
- DataLength: Defines the length of the pad, see Options.
- DataLength2: Second pad length in case the DataType option TwoLengths is used, see Options.
- DataUse Custom Vector: introduced in version 0.19 If checked, the pad direction will not be the normal vector of the sketch but the given vector, see Options.
- DataDirection: introduced in version 0.19 Vector of the pad direction if DataUse Custom Vector is used.
- DataAlong Sketch Normal: introduced in version 0.20 If true, the pad length is measured along the sketch normal. Otherwise and if DataUse Custom Vector is used, it is measured along the custom direction.
- DataUp To Face: A face the pad will extrude up to, see Options.
- DataOffset: Offset from face in which the pad will end. This is only taken into account if the DataType option UpToLast, UpToFirst or UpToFace is used.
- DataRefine: v0.17 and above 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.
- 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.
- version 0.16 and below 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 (which creates an unlinked, non-parametric solid) or with the from the OpenSCAD Workbench which creates a parametric feature.