Parça Tasarım Tezgahı - Kalınlık ver
|Part Design → Create an additive feature → Pad|
|Introduced in version|
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 the sketch or face to be padded.
- Press the button.
- Set the Pad parameters, see the Options below.
- Click .
When creating a pad, the the Pad parameters dialog will be shown. It offers the following settings:
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 by default normal to the defining sketch plane. This can be changed by specifying another Direction. With the option Symmetric to plane the pad will extend half of the given length to either side of the 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). The directions can be switched 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 model that can be chosen by clicking on it.
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 "). This option is only available when Type is either Dimension or Two dimensions.
Offset to face
Offset from face at which the pad will end. This option is only available when Type is either To last, To first or Up to face.
You can select the direction of the extrusion:
- 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 and it becomes the direction vector for the extrusion. introduced in version 0.20
- Custom direction The sketch is extruded along a direction that can be specified via vector values. introduced in version 0.19
If checked, the pad direction will be shown. In case the pad uses a Custom direction, it can be changed. introduced in version 0.20
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
Symmetric to plane
Tick the checkbox to extrude half of the given length to either side of the sketch or plane.
Reverses the direction of the pad.
- VeriType: Type of ways how the pad will be extruded, see Options.
- VeriLength: Defines the length of the pad, see Options.
- VeriLength2: Second pad length in case the VeriType is TwoLengths, see Options.
- VeriUse 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.
- VeriDirection: introduced in version 0.19 Vector of the pad direction if VeriUse Custom Vector is used.
- VeriAlong Sketch Normal: introduced in version 0.20 If true, the pad length is measured along the sketch normal. Otherwise and if VeriUse Custom Vector is used, it is measured along the custom direction.
- VeriUp To Face: A face the pad will extrude up to, see Options.
- VeriOffset: Offset from face in which the pad will end. This is only taken into account if the VeriType option UpToLast, UpToFirst or UpToFace is used.
- VeriRefine: 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 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 a unresolved bug.