The techniques described in this section deal with random vibration induced fatigue, which is calculated from random vibration and/or frequency response FE analysis results. A Power Spectral Density Function (PSDF or PSD) is the most common way of representing the loadings or responses in the frequency domain. The transformation between time domain, i.e., the time history of the loading, and the frequency domain, i.e., a PSD, should not trouble the reader. The PSD simply shows the frequency content of the time signal and is an alternative way of specifying the time signal. It is obtained by utilizing the Fast Fourier Transform (FFT). Figure 14‑1 shows this equivalence for a typical structural response signal.

Transforming from the frequency domain to the time domain is also a relatively easy task which can be done using the Inverse Fourier Transform (IFT). However, when transforming in this direction the random phase angles attributable to each frequency component (which have not been kept when converting to the frequency domain) have to be generated or re-generated. This can be done such that a statistically equivalent signal can be reproduced.

It is not the intention of this manual to teach the user all there is to know about random vibration. For those unfamiliar with random vibration techniques, refer to Vibration Fatigue Theory (p. 674) in the MSC Fatigue User’s Guide.

These are some of the terms you might come across when going through the Vibration Fatigue example:

All of these terms are defined in Appendix A, Glossary Terms.

This section provides a brief summary of techniques for computing fatigue life, or damage, from a PSD of stress or strain. These fall into two broad categories: those that estimate fatigue life directly and those that compute rainflow cycle PDFs as an intermediate stage. All of the approaches have now been brought together in MSC Fatigue.

The general Fatigue Damage equation for the Frequency Domain is shown below. P(S) is obtained with the appropriate vibration fatigue modeler instead of with rainflow cycle counting used in the time-based approach. Refer to the MSC Fatigue 2005 QuickStart Guide MSC Fatigue User’s Guide.

 

To obtain a time history of stress or strain response, either a steady state or transient analysis would be required. For the random response history indicated this would obviously be a transient analysis. In the frequency domain a transfer function would first be computed for the structural model. This is completely independent of the input loading and is a fundamental characteristic of the system, or model. The PSD response caused by any PSD of input loading is then obtained by multiplying the transfer function by the input loading PSD. Further response PSDs caused by additional PSDs of input loading can then be calculated with a trivial amount of computing time. An essential requirement of a structural analysis in the frequency domain is that it results in a PSD which is equivalent to the time history obtained using the transient approach. The rest of the design process is then concerned with using the vibration fatigue tools to compute fatigue life directly from these PSDs of stress. These tools either estimate rainflow histograms (or PDFs), or fatigue life directly. These are shown schematically in the dashed box in the figure above under the heading fatigue modeler. This is intended to show that the time and frequency domain processes are actually very similar. The only differences being the structural analysis approach used (time or frequency domain) and the fact that a fatigue modeler is required to transform from a PSD of stress to the rainflow cycle histogram. In this context the vibration fatigue modeler can be envisaged as just another form of rainflow cycle counting.

A simple bracket, shown to the left, is subject to random vibration excitations defined by loading power spectral density (PSD) functions, which induce serious fatigue damage around the attachment location (the circular hole). The bracket is subject to three input loads, a vertical and horizontal force and a twisting moment, at the far end of the slot. The model is constrained around the circular hole. A random vibration analysis is performed by combining FE frequency response analysis results using three unit loads combined with the loading input PSDs. Fatigue damage is calculated due to each independently and all three simultaneously.

Open a new database and call it bracket.db. Press the Import toggle switch (Analysis in MSC Patran) on the main form. When the form appears, set the Action to Access Results, the Object to Read Output2, and the Method to Both; then, press the Select Results File button and select the file bs_fresp_v.op2. Click the Apply button to read in the file. Now set the Method to Result Entities and select the file bs_fresp_h.op2. Click Apply. Repeat for the bs_fresp_t.op2 file.

Now set the General Setup Parameters as follows:

Open the Solution Params... form. Set the parameters as follows:

Click OK to proceed and close the form.

Open the Material Info... form. This form is used to assign material and other information to regions of the model. In fact it is identical to the time domain S-N material set up form which you should be familiar with from previous exercises.

The Material Info... form and spreadsheet should then be filled in as follows:

Accept the defaults for anything else on the form and close the form by clicking the OK button when finished.

Open the Loading Info... form. Before completing this form we need loading input PSDs. These PSDs will be created from the time signals we used in the pseudo-static runs. On the Loading Info... form press the PSD Manager button. This will spawn PTIME, the loading database manager.

When PTIME appears, select Add an entry... | creaTe psd from time. This will spawn a utility module called MASD for creating auto spectral density functions. This module has multiple functions which are beyond the scope of this text. We wish only to create a Power Spectral Density function from a time series using MASD. A number of screens will be presented to you. Accept the defaults for all items except those indicated below:

Repeat these steps for the other two time histories creating 8d_44-50.psd and 9d_44-50.psd for the horizontal and twist loads respectively. Then quit from PTIME. The original signals and their corresponding PSDs are shown below.

Once the PSDs are created you can proceed to fill out the appropriate information on the
Loading Info... form:

The Loading Info... form is now complete. Click the OK button to accept the form. Before going on, however, a word or two on loading input PSDs is appropriate.

Vibration fatigue analysis makes certain assumptions of loading input. Those assumptions are that the signal is random, stationary and gaussian in nature. Random means that the signal contains no deterministically dominant event such as a spike occurring occasionally or a superimposed dominating sine wave. Truly random signals can only be characterized by their statistics such as root mean square (rms) and mean levels.

Stationary means that those statistics are not changing significantly with time. Any section of the signal should show very close statistical agreement.

Gaussian means that the peak and amplitude probability density function are gaussian in nature or follow a bell shaped curve as shown here. If you draw tram lines through a signal and count the number of times the signal passes through it and plot that as a density function it is gaussian if it follows a bell shape. An example of a non-gaussian signal is a pure sine wave. However adding multiple sine wave together quickly becomes gaussian.

Open the Job Control... form and set the Action to Full Analysis and click the Apply button to submit the job. Change the Action to Monitor Job and click the Apply button occasionally to monitor the job. This analysis will create the usual files: the job parameter file, bs_fresp_v.fin, the fatigue input file, bs_fresp_v.fes, and the fatigue results file, bs_fresp_v.fef. Also a message and status file are created (bs_fresp_v.msg, bs_fresp_v.sta). Unlike a standard time domain solution there is no intermediate rainflow count file, bs_fresp_v.fpp.

When the job is complete open the Results... form and with the Action set to Read Results, click the Apply button. This will read the results into the database for later viewing.

Now that you have seen how to set up the vertical load vibration analysis job you can repeat the setup procedures for the other two single input load (horizontal and twist loads). For the three single load input jobs you can follow the table below for Vibration analysis. Use default values if parameters are not specified.

Again, after each fatigue analysis is finished, read the results into the database under the Results form in the main MSC Fatigue form with the Action set to Read Results.

When each of these jobs is done we can now set up a multiple load input job with all three loads acting simultaneously. It is at this point however, that we have to decide whether the individual load inputs are correlated or uncorrelated. Simultaneously acting loads are said to be fully correlated if, in the time domain, the peaks and valleys from each signal occur simultaneously. This is normally the case for random load signals. Fully uncorrelated signals have the opposite true. Peaks and valleys do not occur at the same time and may cause a cancelling effect. Thus you would expect correlated loads to be more damaging than uncorrelated loads.

Since we are dealing with correlated loads, we need some way of determining the cross-correlation PSDs that will relate one input load PSD to another. If you have the original time series, this can be done with a MSC Fatigue module called MFRA (frequency response analysis). Start MFRA from a system prompt by typing mfra, or by selecting it from the Tools | Fatigue Utilities | Advanced Loading Utilities pull-down menu in Pre & Post or the Tools |MSC Fatigue | Advanced Loading Utilities pull-down menu in MSC Patran.

To get cross PSDs from MFRA follow these instructions after selecting Transfer Function Analysis from the main menu (use the defaults if not specified):

Repeat this process to correlate 7d_44-50.dac with 9d_44-50.dac and 8d_44-50.dac with 9d_44-50.dac and use the output file names of 7-9d_44-50 and 8-9d_44-50 for the two respectively. Exit from MFRA when you are finished or you may plot the results using Results Display on the main menu of MFRA.

You will have in your directory three files called 7-8d_44-50.sxy, 7-9d_44-50.sxy and 8-9d_44-50.sxy. These are the cross PSD terms. Next, invoke PTIME and load these three new PSD files in using the Add an entry | Load file option so that they exist and are known in the PTIME database. Use a wild card to specify all three at the same time, i.e., *.sxy. Accept all defaults and click OK. Exit from PTIME when you are finished.

One last step must be performed before the Loading Info... form can be properly filled for a multiple input load job. We must create a matrix file that relates the cross PSD terms with the input load PSDs. There are two ways to do this. Since we want to look at the effect of both uncorrelated loads and correlated loads we will introduce you to both methods by creating two matrix files.

Perhaps the easiest method is to manually create the file and then load it into PTIME. Create a file using any editor that looks like this in your working directory and call it cor789.pmx:

3
7d_44-50.psd 	7-8d_44-50.sxy 	7-9d_44-50.sxy 
7-8d_44-50.sxy 	8d_44-50.psd 	8-9d_44-50.sxy 
7-9d_44-50.sxy 	8-9d_44-50.sxy 	9d_44-50.psd 

Note that the contents of this file are the names of the input load PSD files on the diagonal terms and the names of the cross PSD files on the off-diagonal terms. The first line indicates that there are three input loads and therefore the matrix is to be 3x3.

This file can be loaded into PTIME by using the option Add an entry | ASCII convert + load. Once in this option do the following:

The second method is a direct method within PTIME. Use the option Add an entry | Psd matrix. Follow these instructions:

If you look at the contents of the second file it should look like this:

3
7d_44-50.psd 	NONE 	NONE 
NONE 	8d_44-50.psd 	NONE 
NONE 	NONE 	9d_44-50.psd 

Finally you can return to the Loading Info... form and set the job up for a multiple input load analysis.

Close down the Loading Info... form. Go to the General Setup Parameters and give the job the name bs_fresp_vth_c and the title correlated loads. Submit the job as you did for the single load input jobs and when the job is complete read the result into the database as done before.

Run one last job before investigating the results. Go into the Loading Info... form and change the matrix PSD file to UNCOR789.PMX. Give it the jobname bs_fresp_vth_u with the title uncorrelated loads and submit the job and read the result when finished.

Do not forget to read the results in from these two jobs.

Perhaps the most obvious thing to do first is to make contour plots of fatigue life from the various jobs run so far. All of the fatigue analyses should have been run and the results imported into the database, so open the Results application switch on the main menu bar (remember not to confuse this with the Results... button on the main MSC Fatigue form).

When the Results application appears, make sure the Object is set to Quick Plot. You will see many Result Cases in the top listbox. Scroll all the way down to the bottom and select the Result Case that corresponds to the vibration fatigue analysis called Vibration Analysis, bs_fresp_vfef. Select Log of Life (Seconds) and click the Apply button to produce a plot. The plot is shown below.

Let us now investigate the design optimization (sensitivity) capabilities of the vibration fatigue analysis. This is analogous to those capabilities in the S-N and strain-life analyzer FEFAT. The design optimization feature can be invoked directly from the Results... form with the Action set to Optimize or from FEVIB started at the system prompt by typing fevib and then entering the Design optimization menu pick.

Do this with any of the vibration fatigue jobs completed thus far.

After specifying a jobname, if necessary, and selecting a node of interest and supplying a design life, the program will proceed to a summary report screen reporting the same life as the global analysis. When the summary report is closed you are placed in the main menu of the design optimization mode. The operation is identical to that of FEFAT’s design optimization mode and is therefore left to you to investigate its many options.

The only unique option to FEVIB’s design optimization mode is its ability to calculate life due to all the analysis methods (Dirlik, Narrow Band, etc.). This is done under Sensitivity analysis | Analysis methods (all).

To see the statistical nature of the vibration analysis, you may want to plot the rainflow cycle count histogram, which is really a probability density function of rainflow ranges. In order to plot the histogram you will need to do the following from the Design Optimization main menu:

As a last exercise before we go on to the second model of the bracket, let us look at another feature of the vibration fatigue analysis module FEVIB. Again invoke FEVIB from the system prompt and this time select the Output power spectrum option. Or on the Results... form set the Action to Extract PSD and click Apply.

Supply a jobname if necessary. The job we want to extract a PSD from is the multi-input correlated load case, bs_fresp_vth_c at Node 72. Do the following after supplying the proper jobname:

At this point you are presented with three options for displaying different types of plots. Plot each one of them separately. The first is the stress response PSD as calculated by FEVIB at Node 72. This is, of course, calculated by multiplying the input PSD by the Transfer Function. For multiple inputs this becomes a matrix operation.

The second plot (angular deviation v. Load case) shows the total angular spread of the principal stress axes for each load case. The solid red line is plotted through the median value at each load case. The yellow error bars indicates the total deviation for each load case; the first load case being the first yellow error bar, the second, the second load case, and the third, the third load case, from left to right.

 

The third plot (angular deviation v Load Frequency) shows how the principal stress axes change with respect to frequency for each load case - actually three different plots.

The angle vs. frequency plot for the vertical load case shows a total angular deviation of the principal stress axes of only about two degrees according to the y-axis labels. The horizontal load case is very small, almost zero, and the twist shows a total of about 20 degrees. These corresponds to the single yellow error bars on the angle vs. load case plot for each load case. The yellow error bars on the angle vs. frequency plots indicate how the stress axes change due to differential damping at each frequency. In other words, it represents how the principal stress axes change subject to a sine wave load input at that frequency.

All angle spreads reported on these plots are relative to an arbitrarily selected angle. The angle vs. load case plot shows the angles relative to each other. You can see that there is about a 45 degree difference between the vertical load case and the horizontal and twist load cases, these two being very similar. This is as expected also in that the horizontal and twist loads are inducing a shear state at Node 72 whereas the vertical load case is not. This is confirmed by plotting the principal stress at Node 72 using the Results application.

These angular spread plots are characteristics of the model. To see whether or not there may be a problem with stationarity of the principal stress axes, you must look at the regions of interest on the response PSD (between zero and 25 Hz) and the corresponding frequency locations on the stationarity plots. For all three load cases, there is little movement of the stress axes in this region.