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.


  1. Define Analysis Type
  2. Define Master DOFs
  3. Constrain the Beam Solution Menu > Define Loads > Apply > Structural > Displacement > On nodes

    Fix the left most node (constrain all DOFs).

  4. Apply Loads
  5. 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.

    1. Load Step 1 - Initial Conditions

      1. Define Load Step

        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.

      2. Specify Time and Time Step Options

        • Select Solution > Load Step Opts > Time/Frequenc > Time - Time Step ..
          • set a time of 0 for the end of the load step (as shown below).
          • set [DELTIM] to 0.001. This will specify a time step size of 0.001 seconds to be used for this load step.

      3. Write Load Step File

        • Select Solution > Load Step Opts > Write LS File

          The following window will appear

        • Enter LSNUM = 1 as shown above and click 'OK'

          The load step will be saved in a file jobname.s01

    2. Load Step 2

      1. Define Load Step

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

      2. Specify Time and Time Step Options

        • Select Solution > Load Step Opts > Time/Frequenc > Time - Time Step .. and set a time of 0.001 for the end of the load step

      3. Write Load Step File Solution > Load Step Opts > Write LS File

        Enter LSNUM = 2

    3. Load Step 3

      1. Define Load Step

        • Select Solution > Define Loads > Delete > Structural > Force/Moment > On Nodes and delete the load at x=1.

      2. Specify Time and Time Step Options

        • Select Solution > Load Step Opts > Time/Frequenc > Time - Time Step .. and set a time of 1 for the end of the load step

      3. Write Load Step File Solution > Load Step Opts > Write LS File

        Enter LSNUM = 3

  6. Solve the System

To view the response of node 2 (UY) with time we must use the TimeHist PostProcessor (POST26).

  1. Define Variables

    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).

  2. List Stored Variables

  3. Plot UY vs. frequency

    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.

  1. Expand the solution

  2. Solve the System
  3. Solution > Solve > Current LS
    SOLVE

  4. Review 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.


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.


The above example was solved using a mixture of the Graphical User Interface (or GUI) and the command language interface of ANSYS. This problem has also been solved using the ANSYS command language interface that you may want to browse. Open the .HTML version, copy and paste the code into Notepad or a similar text editor and save it to your computer. Now go to 'File > Read input from...' and select the file. A .PDF version is also available for printing.