[ANSYS] Tutorial
Structural Dynamic Analysis of a Cantilever Beam

written by: Amir Muradali

Transient Dynamic Analysis

Transient dynamic analysis is a technique used to determine the dynamic response of a structure under a time-varying load.

The time frame for this type of analysis is such that inertia or damping effects of the structure are considered to be important. Cases where such effects play a major role are under step or impulse loading conditions, for example, where there is a sharp load change in a fraction of time.

If inertia effects are negligible for the loading conditions being considered, a static analysis may be used instead.

For our case, we will impact the end of the beam with an impulse force and view the response at the location of impact.

Since an ideal impulse force excites all modes of a structure, the response of the beam should contain all mode frequencies. However, we cannot produce an ideal impulse force numerically. We have to apply a load over a discrete amount of time dt.

After the application of the load, we track the response of the beam at discrete time points for as long as we like (depending on what it is that we are looking for in the response).

The size of the time step is governed by the maximum mode frequency of the structure we wish to capture. The smaller the time step, the higher the mode frequency we will capture. The rule of thumb in ANSYS is

time_step = 1 / 20f

where f is the highest mode frequency we wish to capture. In other words, we must resolve our step size such that we will have 20 discrete points per period of the highest mode frequency.

It should be noted that a transient analysis is more involved than a static or harmonic analysis. It requires a good understanding of the dynamic behavior of a structure. A modal analysis of the structure should be initially performed to provide information about the structure's dynamic behavior.

In ANSYS, transient dynamic analysis can be carried out using 3 methods.

We will use the Reduced Method for conducting our transient analysis. The steps involved in using this method are

Usually one need not go further than Reviewing the Reduced Results. However if stresses and forces are of interest than, we would have to Expand the Reduced Solution.

Building the Model - If not already completed, link to this section to build the model.

Applying Loads and Obtaining a Solution.

Reviewing the Results

We will view the response of node 2 (UY). This is only possible in TimeHist PostProcessing (POST26).

Expanding the Solution

For most problems, one need not go further than Reviewing the Reduced Results as the response of the structure is of utmost interest in transient dynamic analysis.

However, if stresses and forces are of interest, we would have to expand the reduced solution.

Let's say we are interested in the beam's behaviour at peak responses. We should then expand a few or all solutions around one peak (or dip). We will expand 10 solutions within the range of 0.08 and 0.11 seconds.

Reviewing the results in POST1

Review the results using either General Postprocessing (POST1) or TimeHist Postprocessing (POST26). For this case, we can view the deformed shape at each of the 10 solutions we expanded.

Damped Response of the Cantilever Beam

We did not specify damping in our transient analysis of the beam. We specify damping at the same time we specify our time & time steps for each load step.

We will now re-run our transient analysis, but now we will consider damping. Here is where the use of load step files comes in handy. We can easily change a few values in these files and re-run our whole solution from these load case files.

Open up the first load step file (jobname.s01) for editing. The file should look like the following..

/COM,ANSYS REVISION 5.2 14:33:39 01/30/1998
DELTIM, 1.000000000E-03
KBC, 1
TIME, 0.000000000E+00
TREF, 0.000000000E+00
ALPHAD, 0.000000000E+00
BETAD, 0.00000000E+00
DMPRAT, 0.000000000E+00
TINTP,R5.0, 5.000000000E-03,,,
TINTP,R5.0, .500000000 , .500000000 , .200000000
NCNV, 1, 0.000000000E+00, 0, 0.000000000E+00, 0.000000000E+00
ACEL, 0.000000000E+00, 0.000000000E+00, 0.000000000E+00
OMEGA, 0.000000000E+00, 0.000000000E+00, 0.000000000E+00, 0
DOMEGA, 0.000000000E+00, 0.000000000E+00, 0.000000000E+00
CGLOC, 0.000000000E+00, 0.000000000E+00, 0.000000000E+00
CGOMEGA, 0.000000000E+00, 0.000000000E+00, 0.000000000E+00
DCGOMG, 0.000000000E+00, 0.000000000E+00, 0.000000000E+00

D, 1,UX , 0.000000000E+00, 0.000000000E+00
D, 1,UY , 0.000000000E+00, 0.000000000E+00
D, 1,ROTZ, 0.000000000E+00, 0.000000000E+00

Change the damping value BETAD from 0 to 0.01 in all three load step files.

We will have to re-run the job for the new load step files. From the Utility Menu go to file and select Clear and Start New.

Repeat the steps shown above up to the point where we select MDOFs. After selecting MDOFs, simply go to (-Solve-) From LS files ... and in the window that opens up select files from 1 to 3 in steps of 1.

After the results have been calculated, plot up the response at node 2 in POST26. The damped response should look like the following

Go Back to the introductory page for Dynamic Analysis.

Back to the ANSYS Tutorials Page

If you have any questions, comments, or suggestions, please contact Amir Muradali.