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PartDesign Groove

Ubicación en el Menú
PartDesign → Groove
Entornos de trabajo
Diseño de Piezas, Complete
Atajo de teclado por defecto
Ninguno
Introducido en versión
-
Ver también
Ninguno

The PartDesign Groove tool creates a solid in the active Body by revolving a sketch, a 2D object, or one or more faces about a given axis. Its shape is combined with the existing solid through a subtraction or (introduced in 26.3) common boolean operation.

Introduccióin

Esta herramienta revoluciona un croquis seleccionado o un objeto 2D alrededor de un eje indicado, cortando material del soporte. Por ejemplo, la imagen muestra un corte de muesca que se elimina del eje.

Above: sketch (A) is revolved around axis (B); resulting groove on solid (C) is shown right.

Usage

  1. Select a single sketch or similar 2D object, or one or more faces from a single sketch or other object, or from the Body itself.
  2. There are several ways to invoke the tool:
    • Press the   Groove button.
    • Select the Part Design → Subtractive Features →   Groove option from the menu.
  3. The task panel opens.
  4. Set the parameters, see Options below. introduced in 1.1: If the Show interactive draggers when editing features preference is selected (default), angle parameters can be adjusted with interactive gizmos in the 3D View.
  5. Press the OK button to close the task panel and finish the tool.
  6. A Groove feature appears under the active Body.

Editing

The Groove can be edited after its creation in two ways:

  • Double-clicking it in the Tree View, or by right-clicking and selecting Edit Groove in the context menu; this brings up the task panel and (introduced in 1.1) the interactive gizmos (if enabled).
  • Via the Property View.

Opciones

 

Cuando se crea una ranura, los parámetros del letrero de diálogo de 'ranura' ofrece varios parámetro especificando como debería revolucionarse. Tienen exactamente el mismo significado que para la operación de revolución.

The task panel offers the following settings:

 

Start

introduced in 26.3

Sets the angular starting position of the groove around the axis. By default the groove starts at the sketch or face used as its profile.

  • Profile plane (default): the groove starts directly at the profile's sketch plane or face.
  • Offset: the groove starts at an angular offset from the profile, entered in the Offset field.
  • Reference: the groove starts at a face, datum plane, or sketch selected with the Pick Reference button.

Direction

introduced in 26.3

Sets the direction(s) of the groove:

  • One sided: the groove extends on one side of the sketch or face.
  • Two sided: the groove extends on both sides of the sketch or face. Two sub-menus (Side 1 and Side 2) appear to define the groove for each side.
  • Symmetric: the groove is symmetrical with respect to the original sketch or face.

Axis

Specifies the axis of the groove:

  • Vertical sketch axis: selects the vertical sketch axis.
  • Horizontal sketch axis: selects the horizontal sketch axis.
  • Construction line: selects a construction line from the sketch used by the groove. The dropdown list will contain an entry for each construction line. The first construction line will be labelled Construction line 1.
  • Base (X/Y/Z)-axis: selects the X-, Y- or Z-axis of the Body's origin.
  • Select reference…: allows the selection of a straight edge or a datum line from the Body.

Note that when changing the axis, the Reversed option may be (un)checked automatically.

Type

introduced in 1.0

For Side 1 and Side 2 if applicable.

Offers four ways to specify the angle of the groove:

  • Angle: enter a numeric value for the Angle of the groove. With the Direction option Symmetric the groove will extend half the given angle to either side of the sketch or face.
  • Through all: the groove will extend up to the last face of the support it encounters in its direction. With the Direction option Symmetric the groove will extend through all material in both directions.
  • To first: the groove will extend up to the first face of the support it encounters in its direction.
  • Up to face: the groove will extend up to a face. Press the Face button and select a face or a datum plane from the Body.

Angle

For Side 1 and Side 2 if applicable.

Defines the angle of the groove. This option is only available if Type (for the same side) is Angle. Angles larger than 360° are not possible.

Project selected axis to profile plane

introduced in 26.3

Projects the selected axis onto the profile plane if the profile is planar (only available for planar profiles). When unchecked (default), the axis is used in its original position and direction.

Reversed

Reverses the direction of the groove.

Operation

introduced in 26.3

Sets the boolean operation used to combine the groove with the base solid.

  • Subtraction (default): the groove removes the revolved volume from the base solid, as in previous versions.
  • Common: the groove keeps only the volume shared between the revolved profile and the base solid, discarding everything else.

Recompute on change

This option should be checked if Show final result or Show preview overlay is checked.

Show final result

If checked the cumulative result of the previous features and the current operation is shown.

Show preview overlay

If checked the result of the current operation is shown as an overlay.

Properties

See also: Property View.

A PartDesign Groove object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:

Data

Groove

  • DatosSide Type (Enumeration): One side, Two sides or Symmetric. introduced in 26.3
  • Datos (ReadOnly)Base (Vector): The axis base point derived from the DatosReference Axis.
  • Datos (ReadOnly)Axis (Vector): The axis vector derived from the DatosReference Axis.
  • DatosProject Axis (Bool): If checked, the DatosReference Axis is projected onto the profile plane. introduced in 26.3
  • DatosReference Axis (LinkSub): Reference to the axis of the groove.

Part Design

See PartDesign Pocket.

Side1

  • DatosType (Enumeration): Angle, ThroughAll, UpToFirst or UpToFace. Do not use ?TwoAngles. Defines how the groove will end.
  • DatosAngle (Angle): The angle of the groove.
  • DatosUp To Face (LinkSub): Face where the groove will end.
  • DatosUp To Shape (LinkSubList): Not used.

Side2

The properties in this group are only editable if DatosSide Type is Two sides. See the Side1 group for more information about the properties.

Sketch Based

See PartDesign Pad.

Start

See PartDesign Pad.