Creating a pocket consists of extruding a profile or a surface
and removing the material resulting from the extrusion. The
app
lets you choose the limits of creation as well as the direction of extrusion.
Pocket Definition Options
This section describes various options available in the Pocket.x
dialog box.
In this dialog box, you can define a pocket using the following
options:
Type
You can define a specific depth for your pocket using
Dimension or set one of following options:
Up to next: The Extrusion stops at the first face that the app detects while performing the operation.
Profile
Result
Up to last: The Extrusion stops at the
last face that the
app
detects while performing the operation.
Up to plane: The Extrusion stops at the
selected Plane while performing the operation.
Up to surface: The Extrusion stops at the
selected surface while performing the operation. If the surface cuts the
extruding profile, partially,
app
continues the extrusion for the uncut portion of the profile.
If you want to use Up to plane or Up to
surface, you can then define an offset between the limit plane (or
surface) and the bottom of the pocket. For more information, see .
If you have chosen to work in a hybrid design environment, the geometrical elements created
on the fly via the contextual commands mentioned above are aggregated into sketch-based features.
If you set
Up to plane, contextual commands creating new
planes you may need are then available from the Limit
box:
Insert Wireframe > Create Plane:
Insert Wireframe > XY Plane: The XY
plane of the current coordinate system
origin (0,0,0) becomes the limit.
Insert Wireframe > YZ Plane: The YZ
plane of the current coordinate system origin (0,0,0) becomes the limit.
Insert Wireframe > ZX Plane: The ZX
plane of the current coordinate system origin (0,0,0) becomes the limit.
If you set
Up to surface, contextual commands creating
new surfaces you may need are then available from the
Limit box:
Insert Operations > Create Join: Joins surfaces or curves.
If you create any of these elements, the
app
then displays the corresponding icon in front of the Reference
box. Clicking this icon enables you to edit the element.
About Profiles
This section provides information on the profiles used to create a pocket.
You can:
Use profiles sketched in the Sketcher
app
or planar geometrical elements created in the
Generative Shape Designapp
(except for lines).
Create pockets from open profiles provided existing geometry can
trim the pockets.
Create pockets from sketches including several closed profiles.
These profiles must not intersect. In the following example, the initial sketch
is made of eight profiles. Applying the
Pocket command on this sketch lets you create
eight pockets:
Select diverse elements constituting a sketch.
Instead of selecting profiles, you can select surfaces created in Generative Shape Design, non-planar faces and even V4.
If you can click the
Pocket command with no profile previously
defined, just click the icon
to access
the Sketcher
app
and sketch the profile you need.
If you are not satisfied with the profile you selected, note that
you can:
Click the
Selection box and select another
sketch.
Use any of these creation contextual commands available from the
Selection box:
Insert Wireframe > Create Sketch:
Opens the Sketcher app after selecting any plane, and lets you sketch the
profile you need as explained in the Sketcher User's
Guide.
Insert Surfaces > Create Fill:
Creates fill surfaces between the boundary segments. For
more information, see Generative Shape Design User's Guide: Creating Surfaces: Creating Fill
Surfaces.
Insert Operations > Create Join:
Joins surfaces or curves. For more information, see
Generative Shape Design User's Guide: Performing Operations on Shape
Geometry: Joining Surfaces or Curves.
Insert Operations > Create Extract:
Generates separate elements from unconnected sub-elements.
For more information, see Generative Shape Design User's Guide: Performing Operations on Shape
Geometry: Extracting Geometry: Extracting
Elements.
If you create any of these elements, the app displays the corresponding icon in front of the box. Clicking
this icon enables you to edit the element.
If you have chosen to work in a hybrid design environment, the
elements created on the fly via the contextual commands mentioned
above are aggregated into sketch-based features.
About Directions
You can define a direction while creating a pocket.
Note that:
By default, if you extrude a profile, the
app
extrudes normal to the plane used to create the profile.
To specify another direction, Select a new creation direction in the geometry in the
Direction box.
Important:
The option to select the direction which is not normal to the profile is
only available in the MDG role. In the restricted TDD license, a pocket
will be created in the direction normal to the profile.
When copying and pasting a pocket using the As specified in Part document
option , note that if the extrusion direction used does not belong to the
same body as the pocket, this direction is not taken
into account by the Copy and Paste
commands.
If you extrude a surface, you need to select an element defining
the direction because there is no default direction.
to access
the Sketcher
app
and sketch the profile you need.