PartDesign Pad/ru

Выдавливание
Расположение в меню
Part Design → Аддитивные преобразования → Выдавливание
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Вырез

Описание

Инструмент Выдавливание вытягивает эскиз или грань твёрдого тела по прямой траектории.

Эскиз (А) показан слева; конечный результат после операции выдавливания (B) справа.

Применение

Опции

Тип

Размер

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.

К последнему

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.

К первому

До грани

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

Два размера

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 version 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.

Смещение к грани

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.

Длина

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.

2-я длина

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

Симметрично плоскости

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.

В обратную сторону

Меняет направление выдавливания на противоположное.

Направление

Направление/ребро

Вы можете выбрать направление экструзии:

• 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.

Показать направление

If checked, the pad direction will be shown. In case the pad uses a Custom direction, it can be changed.

Длина вдоль нормали эскиза

If checked, the pad length is measured along the sketch or face normal, otherwise along the custom direction.

Угол сужения

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.

2-й угол сужения

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.

Свойства

Data

Pad

• ДанныеType (Enumeration): Defines how the pad will be extruded, see Options.
• ДанныеLength (Length): Defines the length of the pad, see Options.
• ДанныеLength2 (Length): Second pad length in case the ДанныеType is TwoLengths, see Options.
• ДанныеUse Custom Vector (Bool): If checked, the pad direction will not be the normal vector of the sketch but the given vector, see Options.
• ДанныеDirection (Vector): Vector of the pad direction if ДанныеUse Custom Vector is used.
• ДанныеReference Axis (LinkSub)
• ДанныеAlong Sketch Normal (Bool): If true, the pad length is measured along the sketch normal. Otherwise and if ДанныеUse Custom Vector is used, it is measured along the custom direction.
• ДанныеUp To Face (LinkSub): A face the pad will extrude up to, see Options.
• ДанныеOffset (Length): Offset from face in which the pad will end. This is only taken into account if the ДанныеType option UpToLast, UpToFirst or UpToFace is used.
• ДанныеTaper Angle (Angle)
• ДанныеTaper Angle2 (Angle)

Part Design

• ДанныеRefine (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

• ДанныеProfile (LinkSub)
• ДанныеMidplane (Bool)
• ДанныеReversed (Bool)
• ДанныеAllow Multi Face (Bool)

Ограничения