Pocket

 

 

 

 

This command allows you to create a pocket on the part having the same shape as the profile used.

 

Creation Stages / Use:

 

Click the icon or select Shape > Pocket... from the drop-down menu (or Modeling > Shape > Pocket... in the assembly document).

 

  1. Select the shape to modify.

  2. Select the section to use to generate the pocket. A sketch can be created on the fly by using the "+".

  3. Define, if need be, the recess direction of the pocket (normal to the section by default)

  4. Define the bound of the bottom of the pocket (see available options for the different available modes)

 

 

If the section is opened, you should first use the Offset command before using this command.

 

 

  • Click on yellow handles to dynamically and quickly modify heights and the draft of the pocket.

  • Double click on a handle to enter heights or the draft angle.

  • Click on "+" to be able to create a sketch "on the fly".

 

 

Available Options:

 

 

You can define the bottom of the pocket in several ways:

  • Depth: enter the value for the depth of the pocket, measured in relation to the section.

  • Point: define a point for the bound of the bottom of the pocket.

  • Plane: select a trimming plane of the bottom of the pocket.

  • Surface: select a surface (flat or curve) to trim the pocket bottom.

  • Face set: select a face of the shape to trim the pocket with this face and all its adjacent faces.

  • Shape: select a shape against which the pocket must be trimmed

  • Through: the pocket traverses through a first thickness of the part in the defined direction.

  • Through all: the pocket traverses the part in its entirety in the defined direction, even if it countersinks a first time in the area without material.

  • Though all on both directions: the pocket traverses the entirety of the part on both sides of the section

  • In place: the section defines the bottom of the pocket that countersinks on the exterior of the part in the defined direction.

 

 

By checking this box, you will be able to add a draft on all lateral faces of the pocket.

 

 

For limits like Point, Plane, Surface, Face set, Shape, it is possible to add an offset.

 

Example of an offset limit regarding the surface.

 

 

This option allows you to make the pocket countersink on the material of the part located above the section. This option should be active when the pocket section is mounted on a portion of the part and the area above it must be removed. By activating this option, TopSolid removes the material found directly above and in contact with the section, until it falls off.

 

 

 

 

Blend: allows to add a fillet or a chamfer on the upper edge of the pocket. It is the edge between the reference face and the pocket.

  • None: the upper edge has no fillet or chamfer.

  • Chamfer: enter the value for the both sides of the chamfer.

  • Fillet: enter the value of the radius. The "rounded corners" check box allows you to obtain a rounded connection between the fillets arriving at a sharp angle.

 

Fillets: allows you to add fillets.

  • Bottom radius: on the edges of the bottom of the pocket.

  • Vertical fillets: same value on the lateral edges of the pocket.

  • Internal/external vertical fillets: different fillet values on the lateral edges of the pocket between internal and external radii.

 

 

 

This option allows you to make the pocket on the other planar face, this face must be parallel to the definition plane of the sketch.

The depth of the pocket is therefore calculated in relation to the reference plane and not in relation to the sketch.

 

Sketch

 

Pocket

 

Reference plane

 

 

 

Entry point : Once the machining process defined, it is possible to activate this option in order to defined entry points  positions for this machining.

Give the diameter value and select the points to define as entry point positions.

The entry points can be displayed/hidden into the graphic area by using the display mode Create MF available in the Edition menu or on the Home Tab icon bar.