When your model contains parts that contact
each other, you can specify that one or more of the parts is rigid. A rigid
part represents a part that is so much stiffer than the rest of the model that
its deformation can be considered negligible.
In contrast to a part that you define as rigid, a part that you define as
deformable can deform during contact with either a rigid part or another
deformable part. For example, a model of a metal stamping process might use a
deformable part to model the blank and rigid parts to model the mold and die,
as shown in
Figure 1.
In this example the mold is constrained to have no motion, and the die moves
through a prescribed path during the stamping process. You control the motion
of rigid parts by selecting a rigid body reference point and constraining or
prescribing its motion. For more information, see
The reference point.
Computational efficiency is the principal advantage of rigid parts over
deformable parts. During the analysis element-level calculations are not
performed for rigid parts. Although some computational effort is required to
update the motion of the rigid body and to assemble concentrated and
distributed loads, the motion of the rigid body is determined completely by the
reference point. To change the type of a part from deformable to rigid and vice
versa, you can click mouse button 3 on the part in the
Model Tree
and select Edit from the menu that appears. For more
information, see
What is the difference between a rigid part and a rigid body constraint?
and
Display bodies.
You can choose between two kinds of rigid parts:
Discrete rigid
parts
A part that you declared to be a discrete rigid part can be any arbitrary
three-dimensional, two-dimensional, or axisymmetric shape. Therefore, you can
use all the
Part module
feature tools—solids, shells, wires, cuts, and blends—to create a discrete
rigid part. However, only discrete rigid parts containing shells and wires can
be meshed with rigid elements in the
Mesh module.
If you try to create an instance of a solid discrete rigid part in the
Assembly module,
Abaqus/CAE
displays an error message; you must return to the
Part module
and convert the faces of the solid to shells.
Analytical rigid
parts
An analytical rigid part is similar to a discrete rigid part in that it is
used to represent a rigid part in a contact analysis. If possible, you should
use an analytical rigid part when describing a rigid part because it is
computationally less expensive than a discrete rigid part. The shape of an
analytical rigid part is not arbitrary, and the profile must be smooth. You can
use only the following methods to create an analytical rigid part:
You can sketch the two-dimensional profile of the part and revolve the
profile around an axis of symmetry to form a three-dimensional revolved
analytical rigid part, as shown in
Figure 2.
You can sketch the two-dimensional profile of the part and extrude the
profile infinitely to form a three-dimensional extruded analytical rigid part.
Although
Abaqus/CAE
considers that the extrusion extends to infinity, the
Part module
displays a three-dimensional extruded analytical rigid part with a depth that
you specify, as shown in
Figure 3.
You can sketch the profile of a planar two-dimensional analytical rigid
part, as shown in
Figure 4.
You can sketch the profile of an axisymmetric two-dimensional analytical
rigid part, as shown in
Figure 5.
You can import a part from a file containing geometry stored in a
third-party format and define it to be either a deformable or a discrete rigid
part; however, you cannot define an imported part to be an analytical rigid
part. As an alternative, you can import the geometry of the analytical rigid
part into a sketch. You can then create a new analytical rigid part and copy
the imported sketch into the
Sketcher toolset.
A rigid part in
Abaqus/CAE
is equivalent to a rigid surface in an
Abaqus/Standard
or
Abaqus/Explicit
analysis. For more information, see the following: