Tutorial Structural Dynamic Analysis of a Cantilever Beam

## 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.

• The Full Method: This is the easiest method to use. All types of non-linearities are allowed. It is however very CPU intensive to go this route as full system matrices are used.

• The Reduced Method: This method reduces the system matrices to only consider the Master Degrees of Freedom (MDOFs). Because of the reduced size of the matrices, the calculations are much quicker. However, this method handles only linear problems (like our cantilever case).

• The Mode Superposition Method: This method requires a preliminary modal analysis, as factored mode shapes are summed to calculate the structure's response. It is the quickest of the three methods, but it requires a good deal of understanding of the problem at hand.

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

• Building the Model.
• Apply Loads and Obtain Reduced Solution.
• Review the Reduced Results. (View the response at desired locations.)
• Expand the Reduced Solution.
• Review the Expanded Results.
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.

### Applying Loads and Obtaining a Solution.

• Click open the Solution Menu and in New Analysis..., select Transient

• Then click on Analysis Options and select Reduced. Click on OK and another window will open up. Click on OK in that window.

• From the Solution Menu, click on Master DOFs -> (-User Selected-) Define and select all nodes except the left most node (at x=0). The following window will open, choose UY as the first dof in this window

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.

• From the Solution Menu, click on (-Loads-) Apply -> Displacement -> On nodes and select the left most node. Constrain all DOFs at this node.

• In the Solution Menu from the -Load Step Opts- section, select Time/Frequenc -> Time & Time Step.. and enter 0.001 at the time step size box. From the ANSYS rule of thumb, we should achieve accurate results up to 50 Hz with this time step size.

• In the Solution Menu, select Write LS File ... and enter 1 in the box. ANSYS will go ahead and save this load step in a file jobname.s01.

• Click on (-Solve-) Current LS

• Click on (-Loads-) Apply -> Force/Moment -> On nodes and select the right most node (at x=1). Enter a force in the FY direction of value 100 N.

• Click on Time/Frequenc -> Time & Time step .. and set a time of 0.001 for the end of the load step.

• In the Solution Menu, select Write LS File ... and enter 2 in the box. ANSYS will go ahead and save this load step in a file jobname.s02.

• Click on (-Solve-) Current LS

• Click on (-Loads-) Apply -> On nodes and select the right most node. Specify a force FY of value 0. This renews the force at the end of the beam to a value of 0.

• Click on Time/Frequenc -> Time & Time Step.. and enter 1 for the value of time at the end of the load step.

• In the Solution Menu, select Write LS File ... and enter 3 in the box. ANSYS will go ahead and save this load step in a file jobname.s03.

• Click on (-Solve-) Current LS

### Reviewing the Results

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

• Click on TimeHist Postprocessing from the ANSYS Main Menu and select Define Variables... select Add..

• A window will pop up inquiring on the type of variable; we want Nodal DOF results which is already selected so click on OK.

• The following dialog box will open up. Enter values as shown below (note UY has been selected).

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.

• At the ANSYS Input window enter
file,jobname,rdsp

Now that POST26 is directed towards that file, store the data.

• From the TimeHist Postprocessing window, select Store Data.. and click on OK in the window that pops up.

• Select Graph variables .. and select variable 2 as the first variable to plot..

You should see the following response.

• A few things to note in the response curve

• There are approximately 8 cycles in this window. This is the first mode of the cantilever beam and we have been able to capture it.

• We also see another response at a higher frequency. We may have captured some response at the second mode at 52 Hz of the beam. By the rule of thumb, the highest frequency we should be able to capture with our step size (0.001 s) is 50 Hz.

• Note that the response does not decay as it should not. We did not specify damping for our system.

### 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.

• Issue Finish from the ANSYS Main Menu and open up the Solution Menu.

• Select ExpansionPass... and switch it to ON in the window that pops open.

• In the -Load Step Opts- section select ExpansionPass -> Range of Solu's

• Solve Current LS

### 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
/NOPR
/TITLE,
_LSNUM= 1
BFUNIF,TEMP,_TINY
DELTIM, 1.000000000E-03
KBC, 1
TIME, 0.000000000E+00
TREF, 0.000000000E+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
ERESX,DEFA
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
/GOPR

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.