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The Pad tool extrudes a sketch or a face of a solid along a straight path.
Sketch (A) shown on the left; end result after pad operation (B) on the right.
- Select a single sketch or one or more faces from the Body.
- Press the
Pad button. - Set the Pad parameters, see Options below.
- Press the OK button.
When creating a pad, or after double-clicking an existing pad in the Tree view, the Pad parameters task panel is shown. It offers the following settings:
Type offers five different ways of specifying the length of the pad:
Enter a numeric value for the Length of the pad. With the option Symmetric to plane the pad will extend half the given length to either side of the sketch or face.
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.
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.
The pad will extend up to a face. Press the Select face button and select a face or a datum plane from the Body.
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.
(v1.0)
: 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 from face at which the pad will end. This option is only available if Type is To last, To first or Up to face.
Defines the length of the pad. This option is only available if Type is Dimension or Two dimensions. The length is measured along the direction vector, or along the normal of the sketch or face. Negative values are not possible. Use the Reversed option instead.
Defines the length of the pad in the opposite direction. This option is only available if Type is Two dimensions.
Check this option to extrude half the given length to either side of the sketch or face. This option is only available if Type is Dimension.
Reverses the direction of the pad.
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.
If checked, the pad direction will be shown. In case the pad uses a Custom direction, it can be changed.
If checked, the pad length is measured along the sketch or face normal, otherwise along the custom direction.
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.
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.
{{TitleProperty|Pad}}
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Type|Enumeration: Defines how the pad will be extruded, see Options.
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Length|Length: Defines the length of the pad, see Options.
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Length2|Length: Second pad length in case the Type is TwoLengths, see Options.
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Use Custom Vector|Bool: If checked, the pad direction will not be the normal vector of the sketch but the given vector, see Options.
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Direction|Vector: Vector of the pad direction if Use Custom Vector is used.
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Reference Axis|LinkSub
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Along Sketch Normal|Bool: If true, the pad length is measured along the sketch normal. Otherwise and if Use Custom Vector is used, it is measured along the custom direction.
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Up To Face|LinkSub: A face the pad will extrude up to, see Options.
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Offset|Length: Offset from face in which the pad will end. This is only taken into account if the Type option UpToLast, UpToFirst or UpToFace is used.
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Taper Angle|Angle
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Taper Angle2|Angle
{{TitleProperty|Part Design}}
- Refine|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).
{{TitleProperty|Sketch Based}}
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Profile|LinkSub
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Midplane|Bool
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Reversed|Bool
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Allow Multi Face|Bool
- 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.
- 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.
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