- 429 Views
- Uploaded on

Download Presentation
## PowerPoint Slideshow about 'AE4131 ABAQUS Lecture Part V' - albert

**An Image/Link below is provided (as is) to download presentation**

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.

- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -

Presentation Transcript

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.

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.

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.

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

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.

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:

- 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.
- The explicit integration method is more efficient than the implicit integration method for solving extremely discontinuous events or processes.
- It is possible to solve complicated, very general, three-dimensional contact problems with deformable bodies in ABAQUS/Explicit.
- Problems involving stress wave propagation can be far more efficient computationally in ABAQUS/Explicit than in ABAQUS/Standard.

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.

The loading

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

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.

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)

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.

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.

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)

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

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.

Step Module

- Create a dynamic step just like in our beam example.
- Monitor one corner of the block in the transverse direction.

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.

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)

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.

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.

Defining Periodic loading

These are constants that are defined on the data lines of *AMPLITUDE

(From the ABAQUS documentation)

Defining Periodic loading

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

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.

Mesh Module

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

Job Module

- Submit the job and watch for Warnings.
- We immediately see zero pivot and overconstraint warnings.
- Notice that the nodes in question have been placed in node sets.
- Kill the job.
- Go into Results.

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.

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.

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

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.

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.

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.

Download Presentation

Connecting to Server..