|Structural Dynamic Analysis of a Cantilever Beam|
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
For an explanation on Master DOFs, see the section on Using the Reduced Method for modal analysis.
We will now begin applying the loads. We will define our impulse load using Load Steps. The following time history curve shows our load steps and time steps. Note that for the reduced method, a constant time step is required throughout the time range.
We can define each load step (load and time at the end of load segment) and save them in a file for future solution purposes. This is highly recommended especially when we have many load steps and we wish to re-run our solution.
We can also solve for each load step after we define it. We will go ahead and save each load step in a file for later use, at the same time solve for each load step after we are done defining it.
Thus far we have only pointed the variables to the results we would like to see. We now have to store the data under the variable names into memory.
By default, POST26 looks for the results file (jobname.rst) to read the results from. We don't have this file yet because we have not performed an expansion pass. We need to direct POST26 to another file named jobname.rdsp to get the results for node 2.
Now that POST26 is directed towards that file, store the data.
You should see the following response.
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.
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
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
Back to the ANSYS Tutorials Page
If you have any questions, comments, or suggestions, please contact Amir Muradali.