Part: PartDesign Pad(protuberanță)
|Part Design → Pad|
|Prezentat în versiune|
|A se vedea, de asemenea,|
Instrumentul Pad extrude o schiță într-un solid în direcția normală la planul schiței. Începând cu versiunea v0.17, fațete pe solid pot de de asemenea utilizate.
Sketch (A) shown on the left; end result after pad operation (B) on the right.
Cum se utilizează
- Select the sketch to be padded. In v0.17 and above, a face on the existing solid can alternatively be used.
- Press the button.
- Set the Pad parameters (see next section).
- Click .
When selecting a single sketch, it can have multiple enclosed profiles inside a larger one, for example a rectangle with two circles inside it. But the profiles may not intersect each other. introduced in version 0.20
Când se creează o protuberanță(Pad), vizualizarea Combo se comută automat în panoul Activități, afișând dialogul Parametri pad .
Tipul oferă cinci modalități diferite de a specifica lungimea la care va fi extrudat tamponul.
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.
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.
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.
Definește lungimea protuberanței. Unitățile multiple pot fi utilizate independent de preferințele unităților utilizatorului(m, cm, mm, nm, ft or ', in or ").
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:
- Face/Sketch normal The sketch or face is extruded along its normal. If you have selected several sketches or faces to be extruded, the normal of the first one will be used. introduced in version 0.20
- 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
Bifați caseta de selectare pentru a extinde jumătate din lungimea dată la fiecare parte a planului de schiță.
Reverses the direction of the pad.
Tapers the pad in the extrusion direction by the given angle. A positive angle means the outer pad border gets wider. This option is only available if Type is either Dimension or Two dimensions. Note that inner structures receive the opposite taper angle. This is done to facilitate the design of molds and molded parts.
- Sketches containing B-Splines often cannot be properly tapered. This is a limitation of the OpenCASCADE kernel that FreeCAD uses.
- For larger angles tapering will fail if the end face of the pad would have fewer edges than the start face/sketch.
Defines the length of the pad in the opposite extrusion direction. 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 if Type is Two dimensions.
2nd taper angle
Tapers the pad in the opposite extrusion direction by the given angle. A positive angle means the outer pad border gets wider. This option is only available if Type is Two dimensions. Note that inner structures receive the opposite taper angle. This is done to facilitate the design of molds and molded parts.
- DATERefine: 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.
- 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.