This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to show the steps involved to perform a simple transient 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. Therefore, 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. 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.
The simple cantilever beam is used in all of the Dynamic Analysis Tutorials. If you haven't created the model in ANSYS, please use the links below. Both the command line codes and the GUI commands are shown in the respective links.
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.
Fix the left most node (constrain all DOFs).
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.
We need to establish initial conditions (the condition at Time = 0). Since the equations for a transient dynamic analysis are of second order, two sets of initial conditions are required; initial displacement and initial velocity. However, both default to zero. Therefore, for this example we can skip this step.
The following window will appear
The load step will be saved in a file jobname.s01
Enter LSNUM = 2
Enter LSNUM = 3
The following window will appear.
To view the response of node 2 (UY) with time we must use the TimeHist PostProcessor (POST26).
In here we have to define variables that we want to see plotted. By default, Variable 1 is assigned either Time or Frequency. In our case it is assigned Frequency. We want to see the displacement UY at the node at x=1, which is node #2. (To get a list of nodes and their attributes, select Utility Menu > List > nodes).
The following window will appear listing the data:
The following graph should be plotted in the main ANSYS window.
A few things to note in the response curve
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.
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.
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.
/COM,ANSYS RELEASE 5.7.1 UP20010418 14:44:02 08/20/2001 /NOPR /TITLE, Dynamic Analysis _LSNUM= 1 ANTYPE, 4 TRNOPT,REDU,,DAMP BFUNIF,TEMP,_TINY DELTIM, 1.000000000E-03 TIME, 0.00000000 TREF, 0.00000000 ALPHAD, 0.00000000 BETAD, 0.00000000 DMPRAT, 0.00000000 TINTP,R5.0, 5.000000000E-03,,, TINTP,R5.0, -1.00000000 , 0.500000000 , -1.00000000 NCNV, 1, 0.00000000 , 0, 0.00000000 , 0.00000000 ERESX,DEFA ACEL, 0.00000000 , 0.00000000 , 0.00000000 OMEGA, 0.00000000 , 0.00000000 , 0.00000000 , 0 DOMEGA, 0.00000000 , 0.00000000 , 0.00000000 CGLOC, 0.00000000 , 0.00000000 , 0.00000000 CGOMEGA, 0.00000000 , 0.00000000 , 0.00000000 DCGOMG, 0.00000000 , 0.00000000 , 0.00000000 D, 1,UX , 0.00000000 , 0.00000000 D, 1,UY , 0.00000000 , 0.00000000 D, 1,ROTZ, 0.00000000 , 0.00000000 /GOPR