This document provides an overview of dynamic modeling and analysis in ABAQUS. It discusses starting ABAQUS/CAE, the differences between implicit and explicit dynamic analysis, and provides an example of modeling a beam undergoing forced vibration. It also demonstrates modeling contact between a block and plate, where the block is partially bonded to the plate, and applying a periodic pressure load to analyze the dynamic response. Issues with the initial model formulation are discussed and resolved.

1. AE4131
ABAQUS Lecture
Part V
Patrick Roberts
gt0398b@prism.gatech.edu
x5-2773
Weber 201

2. Starting ABAQUS CAE
You can start ABAQUS CAE from the start
menu or with a command line by typing
abaqus cae
TIP: You should start ABAQUS CAE via
command line from the directory you want
your results files to end up.

3. Dynamics
• We have seen how we can compute and
view the results of static loading on 1D, 2D
and 3D models.
• We may also be interested in how a model
moves as a function of time or dynamic
modeling.
• Reason: Stresses and displacements can
be greater in a dynamic model than a static
model.

4. The Beam
Example: Let’s look at a 3D beam that has dimensions of
1m length, 0.1 m height, and 0.2 m width.

5. Material Properties
• We used standard 2014-T6 aluminum alloy
properties which are:
– Density: 174 lbm/ft3 (2800 kg/m3)
– Young’s modulus : 10,400,000. psi (72 GPa)
– Poison’s ratio: 0.33

6. The Step Module
Under the General procedure type there are
two basic types of dynamic analysis; implicit
and explicit.
– ABAQUS/Standard uses the implicit Hilber-Hughes-
Taylor operator for integration of the equations of
motion. This offers the use of all elements in
ABAQUS but can be slower than Explicit.
– ABAQUS/Explicit uses the central-difference operator.
In an implicit dynamic analysis the integration
operator matrix must be inverted and a set of
nonlinear equilibrium equations must be solved at
each time increment.

7. ABAQUS Explicit
ABAQUS/Explicit offers fewer element types than
ABAQUS/Standard. For example, only first-order,
displacement method elements (4-node quadrilaterals, 8-
node bricks, etc.) and modified second-order elements are
used, and each degree of freedom in the model must have
mass or rotary inertia associated with it. However, the
method provided in ABAQUS/Explicit has some important
advantages:
1. The analysis cost rises only linearly with problem size, whereas the cost
of solving the nonlinear equations associated with implicit integration
rises more rapidly than linearly with problem size. Therefore,
ABAQUS/Explicit is attractive for very large problems.
2. The explicit integration method is more efficient than the implicit
integration method for solving extremely discontinuous events or
processes.
3. It is possible to solve complicated, very general, three-dimensional
contact problems with deformable bodies in ABAQUS/Explicit.
4. Problems involving stress wave propagation can be far more efficient
computationally in ABAQUS/Explicit than in ABAQUS/Standard.

8. Dynamics
For our modeling we will use ABAQUS
Standard (implicit).
– Edit Step Dialog
• Basic tab:
– Time period : 5
• Incrementation tab:
– Type : fixed;
– Maximum number of increments : 50000;
– Increment size: 0.0001;
– Check: Suppress half-step residual calculation.
– Monitor the displacement of a node in the transverse
direction.

9. The loading
We apply a 5 Newton load to the top two corners of the
beam at the free end.

10. Running the model
The model may take some time to run. You
should monitor the model as it runs. If there
is a problem it’s important you see how the
problem manifests itself.

11. Results

12. Results
What we see is an initial transient region
then the oscillation settles to a steady state
with a bias from 0 of about 0.65. Because
there is no damping the energy cannot
dissipate so it will oscillate about this point at
that amplitude forever. Numerical errors can
often appear as “artificial” damping (usually
negative damping which causes exponential
growth)

13. Dynamic modeling with contact
analysis
• Contact/noncontact analysis is studied
extensively in finite element modeling.
• Any time two or more parts come in
contact the nature of the contact surfaces
must be defined.

14. Example problem
In our example we consider a block bonded
onto a plate. There is a circular area in the
center that is not bonded. We want to model
how this non-bonded area effects the
dynamic response of the block when there is
a periodic pressure load applied on the
bottom of the plate.

15. Part module
Block dimensions:
• Length = 6 inches (0.1524 m)
• Width = 6 inches (0.1524 m)
• Height = 3 inches (0.0762 m)
Plate dimensions:
• Length = 12 inches (0.3048 m)
• Width = 12 inches (0.3048 m)
• Height = 0.375 inch (0.009525 m)

16. Property module
Block material:
• Density = 12 lb/ft3 (192 kg/m3)
• Young’s modulus = 29 x 106 psi (200 GPa)
• Poisons ratio = 0.33
Plate material:
• Density = 174. lb/ft3 (2800 kg/m3)
• Young’s modulus = 10,400,000 psi (72 GPa)
• Poisons ratio = 0.33

17. Assembly module
• When you create each instance make sure
to auto offset.
• To place the tile correctly use datum points
on the center of the bottom of the block
and the top of the plate.
• Translate the block so it is centered on the
top of the plate.

18. Assembly Module

19. Step Module
• Create a dynamic step just like in our
beam example.
• Monitor one corner of the block in the
transverse direction.

20. Interaction Module
• This is the module you will define the contact
surfaces.
• Two types of contact for this model:
– Tied (for areas that are perfectly bonded) and
– NoFric (for those areas not bonded).
• We will create a circular partition on the center of
the contact surface of the block and plate with a
radius of 0.03 m.
• Under View you will see an option of Assembly
Display Options. Go to the Instance tab. You
can use this to turn on/off views of parts.

21. Interaction Module
• ABAQUS/Standard defines contact between two bodies in
terms of two surfaces that may interact; these surfaces are
called a “contact pair.” ABAQUS/Standard defines “self-
contact” in terms of a single surface.
• The order in which the two surfaces are specified on the
*CONTACT PAIR option is critical because of the manner in
which surface interactions are discretized. For each node on
the first surface (the “slave” surface) ABAQUS/Standard
attempts to find the closest point on the second surface (the
“master” surface) of the contact pair where the master
surface's normal passes through the node on the slave
surface. The interaction is then discretized between the point
on the master surface and the slave node.
• We will use the plate as the Master surface and the block as
the slave surface.
(From the ABAQUS documentation)

22. Interaction Module
• Inside the circle on both parts we need to define
the NoFriction contact definition. Go to
Interaction, Manager, Create and give it a name;
Step is Initial, Surface-to-Surface contact, pick
the master and slave surface.
• Outside the circle on both parts we need to
define tied contact. Go to Constraint and pick
Tie from the list. Choose each surface outside
the circle.

23. Load Module
• Fully constrain the four sides of the plate.
• We want to have a periodic pressure
applied to the bottom of the plate of 10 Hz
(62.8 rad/s) and a magnitude of 5.

24. Defining Periodic loading
These are constants that are defined on the data lines of
*AMPLITUDE
(From the ABAQUS documentation)

25. Defining Periodic loading
Go to Tools, Amplitude, Create, give it a
name and choose Periodic. Add the
values as seen in the next slide.

26. Load Module

27. Load Module
• Define a pressure load on the bottom of
the plate with a magnitude of 5. When you
get to Amplitude pick the periodic
amplitude you just defined.

28. Mesh Module
When choosing which parts mesh controls,
element type, seed and mesh instance
hold down the Shift key and choose both
parts.

29. Job Module
1. Submit the job and watch for Warnings.
2. We immediately see zero pivot and
overconstraint warnings.
3. Notice that the nodes in question have
been placed in node sets.
4. Kill the job.
5. Go into Results.

30. Visualization module
ABAQUS helps you locate problems by assigning
nodes or elements to sets so you can view them
in the Visualization module.
Turn on Node labeling
Create a Display group. When you choose Node
Sets you will see a list of sets the system
created when it had problems. Pick one and you
will see they are near the perimeter of the circle
we created.

31. The problem
All attributes of a node are defined by the
elements that are attached to them. The
nodes along the perimeter of the circle are
connected to elements with two different
contact surface definitions. Therefore,
ABAQUS doesn’t know which rule set to
apply to these nodes.

32. The Solution
• Go back and delete all the tied contact
surface definitions.
• Add a circle that has a radius of 0.035. It
should look like

33. The Solution
• The area inside the inner circle is already
defined as NoFriction. Define the area
outside the outer circle as Tied contact.
The area between the two surfaces are
undefined. This way a node has at most
one contact surface definition.
• Now rerun the model.

34. The Results
This model takes
quite some time
to run. The
important item to
notice is no more
warnings. The
results should be
compared with
theory.

35. The Conclusion
• Dynamic modeling in ABAQUS is very
easy and can provide very meaningful
results.
• Check results against established theory
to confirm what the software is calculating.
• Take the time to understand all the
dynamic procedures in ABAQUS to
choose the best one for your analysis.