Structural Dynamic Analysis of a Cantilever Beam

written by: Amir Muradali

The purpose of this tutorial is to explore the dynamic analysis capabilities of ANSYS. These capabilities include

Modal Analysis: Determining the mode frequencies and mode shapes of structures.

Harmonic Analysis: Analysing the steady-state behavior of a structure subject to cyclic loads.

Transient Analysis: Determining the dynamic response of a structure under more general time-dependant loads.

Spectral Analysis: Studying the response of structures under the action of loads with known "spectra" (eg. random loading conditions).

The ANSYS version 5.2 was used to develop this tutorial.Introducing the Problem

A full dynamic analysis will be done for the cantilever beam shown below. The beam has a square cross section and is made of steel. 

ANSYS Structural Dynamic Modelling Tutorials

Building the Model

We will model a cantilever beam with Beam2D Elastic elements.Select Preprocessor from the ANSYS Main Menu . We will follow the order presented in the Preprocessor Menu beginning with selecting the element type.

Choosing Element type: Element type -> Choose Beam 2D Elastic element. 

Setting Constants for Chosen Element type: Real constants -> enter cross-sectional properties (of the beam) in the dialog box as shown below. 

Specifying Material Properties for Chosen Element type: Material Properties -> enter material properties as shown below 

Note: For dynamic analysis, both the stiffness and the material density have to be specified. 

Creating the Geometry of Cantilever: Modelling -> Create -> Keypoints -> In Active CS.. -> specify 2 keypoints (the ends of the cantilever beam) as follows: 

keypoint

x

y

z

1

0

0

0

2

1

0

0

Join the two keypoints with a line. Modelling -> Create -> Lines -> Straight line -> Click on both keypoints. 

Setting Meshing Options: Meshing -> Shape & Size -> for picked lines -> select the line and then specify 10 element divisions in the dialog box that pops up. 

Meshing the line: Meshing -> mesh -> lines -> pick the line and click OK.

Dynamic Analysis

We are now ready to perform full dynamic analysis on the beam.

Modal Analysis of a Cantilever Beam

We are going to determine the first 5 modes and the respective frequencies of the cantilever beam.Modal Analysis in ANSYS is done in 4 steps:

Building the model (Preprocessing)

Applying loads and obtaining solution (Solution)

Expanding the modes (Solution)

Reviewing the results (Post Processing)

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

Applying Loads and Obtaining a Solution

Open the Solution menu from the ANSYS Main Menu.

Choosing Analysis type: New Analysis ... -> Modal 

Setting Options for Chosen Analysis type: Analysis options.. -> The following dialog box will open up 

Select the Subspace method and enter 5 at No. of modes to extract as shown above and click on OK.

Note that the default mode extraction method chosen is the Reduced Method. This is the fastest method as it reduces the system matrices to only consider the Master Degrees of Freedom (see below) and is the only other option applicable for this problem. The Subspace Method on the other hand extracts modes for all DOF's. It is more exact and easier to use, however it also takes long to compute (especially when the geometry of the problem is increased).

The following window will then open up requesting for options for the Subspace method. For a better understanding of these options see the Commands manual. For this problem, we will live with the default options so click on OK. 

Applying constraints: Loads -> apply -> displacements -> Constrain the left most node in all DOF (specify a displacement value of 0). 

Obtaining the solution: Select Solve -> Current LS 

When ANSYS has completed the solution, close the Solution menu and issue FINISH at the bottom of the ANSYS Main Menu .

Expanding the Modes

This is when the mode shapes are written to the results files for review in the post processing stage. 

Open the Solution menu again. 

Select expansion pass... -> Switch EXPASS to "ON" 

Setting Options for Expansion Pass: -load step opts - expansion pass -> We want the first 5 modes, so fill in the dialog box as shown. 

Solving: Solve -> Current LS 

After ANSYS has finished expanding the modes, close the Solution menu.

Reviewing the Results (Post Processing)

Open up the General Post Processing menu. We will first verify that 5 modes have been extracted, and will also compare these values to theoretical values.Listing Results: list results -> results summary -> You should see the following window pop up. Note you can either print this list or save it to a file. 

Comparing to Theory: The following table compares the mode frequencies in Hz predicted by theory and ANSYS. 

Mode

Theory

ANSYS

1

8.311

8.302

2

51.94

52.02

3

145.68

145.67

4

285.69

285.57

5

472.22

472.64

Note: To obtain accurate higher mode frequencies, this mesh would have to be refined even more (i.e. instead of 10 elements, we would have to model the cantilever using 15 or more elements depending upon the highest mode frequency of interest).

To view the first mode shape, select - read results - First Set (1st Mode) from the Post Processing menu.

To view the deformed shape, select plot results -> Deformed shape

To animate the mode shape, select Plot Ctrls from the ANSYS Utility Menu (Blue menu at the top). Then select Animate -> Mode Shape 

To view the next mode shape, select - read results - Next Set from the Post Processing . You can then view the mode shape or animate it using the same procedure as above. 

The first four mode shapes should look like the following: 

The animated mode shapes are shown below. 

Mode 1 

Mode 2 

Mode 3 

Mode 4 

Using the Reduced Method for Modal Analysis

This method employs the use of Master Degrees of Freedom. These are degrees of freedom that govern the dynamic characteristics of a structure. For example, the Master Degrees of Freedom for the bending modes of cantilever beam are 

For this option, a detailed understanding of the dynamic behavior of a structure is required. However, going this route means a smaller (reduced) stiffness matrix, and thus faster calculations.

The steps for using this option are quite simple.

Instead of specifying the Subspace method, select the Reduced method and specify 5 modes for extraction. 

Click OK and another window should open up for options for the Reduced method. We already specified 5 modes to be extracted, however we could also specify a frequency range within which all modes of interest lie. This window looks like the following 

Note: For this example both the number of modes and frequency range was specified. ANSYS then extracts the minimum number of modes between the two. 

Select Master DOF -> -User Selected- Define -> Select all nodes except the left most node (to be constrained later). Then select UY as the 1st degree of freedom (shown below). 

After we have selected our MDOFs we can now apply constraints and obtain the solution using the same steps as shown in the example above.

Modal Analysis of a Clamped Plate

Here is another problem for which the first 8 modes were calculated. The clamped plate is shown below together with the material properties. 

See if you can obtain the first 8 modes of this structure. These modes should look like the following. The contours represent relative stress distribution.

Modes 1 to 4

Modes 5 to 8

The first 8 mode frequencies are

Harmonic Analysis of a Cantilever Beam

For this problem, we will conduct a harmonic forced response test on a cantilever beam. We will do this by applying a cyclic load (harmonic) at the end of the beam and observing the response at that location. The frequency of the load will be varied from 1 - 100 Hz. The figure below depicts the beam with the application of the load. 

ANSYS provides 3 methods for conducting a harmonic analysis. These 3 methods are the Full , Reduced and Modal Superposition methods.

This example demonstrates the Full method because it is simple and easy to use as compared to the other two methods. However, this method makes use of the full stiffness and mass matrices and thus is the slower and costlier option.

There are 3 steps involved for the Full Harmonic Response Analysis of a structure. These steps are:

Building the Model

Applying Loads and Constraints

Reviewing the Results

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

Applying Loads and Constraints

Open up the Solution Menu, and select New Analysis...-> HarmonicClick on Analysis Options... The following window will open showing the methods available for harmonic analysis. Select Full. 

We will now constrain the beam and apply a harmonic load at the end of the beam.Applying Constrains: Click Apply -> Displacement -> On Nodes and click on the node at x=0. Constrain all the degrees of freedom at this node. 

Applying Load: From the Apply menu, click on Force/Moment -> On Nodes and click the node at x=1. Apply a load in the Y direction with a real value of 100 and an imaginary value of 0. 

Note: By specifying a real and imaginary value of the load we are providing information on magnitude and phase of the load. In this case the magnitude of the load is 100 N and its phase is 0. Phase information is important when you have two or more cyclic loads being applied to the structure as these loads could be in or out of phase. For harmonic analysis, all loads applied to a structure must have the SAME FREQUENCY.

We have not yet set the frequency of the load. For harmonic analysis we can observe the structural response to a load over a range of frequencies.To do this, select Time/Frequency below the -Load Step Opts- (Solution Menu). Select Freq & Substeps... and specify a frequency range of 0 - 100Hz with 100 substeps. 

By doing this we will be subjecting the beam to loads at 1 Hz, 2 Hz, 3 Hz, ..... 100 Hz. We will specify a stepped boundary condition (KBC) as this will ensure that the same amplitude (100 N) will be applyed for each of the frequencies. The ramped option, on the other hand, would ramp up the amplitude where at 1 Hz the amplitude would be 1 N and at 100 Hz the amplitude would be 100 N.

You should see the following in the ANSYS Graphics window

We can now solve the problem. -Solve- Current LS

Reviewing the Results

We want to observe the response at x=1 (where the load was applyed) as a function of frequency. We cannot do this with General PostProcessing (POST1), rather we must use TimeHist PostProcessing (POST26). POST26 is mainly used to observe certain variables as a function of either time or frequency.Enter POST26 by selecting TimeHist Postprocessing from the ANSYS Main Menu.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 will be 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 List -> nodes from the Utility Menu).

Select Define Variables... and the following window should pop up. 

Select Add.. from this window and the following window should appear 

We are interested in the Nodal DOF solution at node 2, so click OK. For stresses, we would have to select Element Results in this window.

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.

Click on Store Data.. in the TimeHist PostProcessing menu. 

The following dialog box will appear. By default the merge with existing data option will be selected. We don't have any data stored in memory so we could just click on OK. However, change the option to Replace. This will erase all of the previously "stored" data in the memory. This option was chosen for demonstration purposes because numerous results from an ANSYS job may be of interest, however, only a limited number of variables can be stored in memory. 

We now should have 2 variables in memory, frequency (1) and UY at node 2 (2).

To view these variables select List Variables... and set variable 1 as the first variable to list and variable 2 as the second. You should see the following window with the values of both variables listed. 

Note that by default ANSYS names variable number 1 as Time, whether the variable is time or frequency.

We now want to plot UY vs. frequency. To do this select Graph Variables.. and select variable 2 as the first variable to plot. You should see the following figure. 

Note that we get peaks at the right frequencies (from the modal analysis) at approximately 8.3 and 51 Hz.

To get a better view of the response, we should be viewing the log scale of UY. To do this enter the following in the ANSYS Input Window/gropt,logy,1

/replot

You should now see the following 

This is the response at node 2 for the cyclic load applied at this node from 0 - 100 Hz.

Harmonic Analysis using the Reduced and Modal Superposition Methods.

These other methods available for harmonic analysis are a bit more involved and require a good physical understanding of the problem at hand.The Reduced Method employs the use of Master Degrees of Freedom. The dynamic behavior of the structure should be known before assumptions can be made as to which degrees of freedom can be assigned as MDOF. The steps involved in using this method are

Building the Model (Preprocessing).

Selecting MDOFs and Applying the Loads and Constraints (Solution).

Expanding the Solution or Performing an Expansion Pass (Solution).

Reviewing the Results (TimeHist Postprocessing).

The Modal Superposition Method is the fastest of the three methods. It however involves several steps including doing a Modal Analysis on the structure. These steps areBuilding the Model (Preprocessing).

Applying Constraints and Calculating the Modes (Solution).

Applying Loads and Obtaining the Harmonic Solution (Solution).

Performing an Expansion Pass (Solution).

Reviewing the Results (TimeHist Postprocessing).

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. 

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

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.

Load Step 1 

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

Load Step 2 

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

Load Step 3 

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

Good @Mahmoud 

Respected sir,

The field approached by you is very interesting and also vast, so more research can be done in this regard. It's very interesting topic.Solution of Finite Element Problem by using ANSYS In general, a finite element solution may be broken into the following three stages. This is a general guideline that can be used for setting up any finite element analysis. 1) Preprocessing 2) Solution 3) Post processing. The following article link may help you for your kind information.

https://www.researchgate.net/publication/301348952_Licensed_Under_Creative_Commons_Attribution_CC_BY_Investigation_on_Mode_-_I_Fracture_Parameters_Using_Steel_Fibers_in_High_Strength_Concrete

Article Licensed Under Creative Commons Attribution CC BY Investigat...

Thanks a lot Mahmoud Fathy Moubark and Brahma Chari J Kanneganti

I really appreciate your help.

Best regards,