When you run unsteady simulations you need to let the results reach a statistically steady state. The way you decide whether you reached a statistically steady state is by observing time histories of various flow quantities and make sure the transient behavior is no longer there, I.e there is a repeating pattern in the time history. If it is random, you should see a band of nearly white noise. The other thing you need to have is a long enough time sample to average over, after removing the transient. 

I have found out a very interesting way to do this averaging if I am using ANSYS FLUENT as my CFD tool. All you need to do is run your simulation in unsteady state as per your choice of time step. Save the data files at each time step. Once all your simulations are over, you extrapolate the field data as save them as separate text files. This way we can generate as many files we want. Now I have written a small code for averaging these fluent files. It reads in these files sequentially and then creates a "average.txt" file. Once this average file is ready, we read it back in Fluent by interpolating. Now I have the averaged field in my domain to work further on it.

Hi all , i have the same broblem with Mr Rizwan . the answer of Mr Rajeev is interesting if it's possible i would more explanation about the code that you are developed and how we can interpolate in Fluent ? 

Fluent has a feature called file - interpolate. Look under the File Menu. You can select the domain on which you want to interpolate. Then you can interpolate the fields of interest. Normally it creates a file which can be opened in Wordpad and you can see its structure.

I am enclosing the structure of an input file for your ready reference

2

3

182125

6

pressure

x-velocity

y-velocity

z-velocity

k

epsilon

-1.71295

-1.7132

-1.71341

-1.71358

-1.71386

-1.71412

-1.7141

-1.71385

Explanation:

2 in first line is the domain id

3 stands for 3d simulation

182125 stands for the mesh size or the number of data points in each field

6 stands for the no of fields it stores

next six words are the fields

Now the data set below as seen here has 182125 x - locations

Next 182125 will be y-locations

And likewise till you complete the 3 locations and the six fields

All you need to do is extract such series of files. I am attaching a sample file here

Hi Rishad,

How many data points do you have in a cycle. Is it difficult to read that into matlab or excel and, for starters, use the trapezoidal rule of integrating discrete data points?

Best Regards

One of the more perplexing issues is determining if the transient data is eliminated from your data when computing the mean. The best way I've seen this done is to compute two quantities. The first is an RMS (root mean square) of whatever parameter you are targeting. The second is to perform a Fast Fourier Transform (FFT) analysis of the data. To do the FFT, you'll want to use multiple segments of the data that over lap. In theory, if the window size is sufficiently sized, there will be very little variance between each window. I recommend looking at Welch's method for windowing. Simply take your time accurate data set (preferably second order accurate in time) and divide it into windows of equal size. If you have 100,000 time steps, try 25,000 time steps each, where the first window is 1-25k, the second is 12.5k-37.5k, the third is 25k-50k, the fourth is 37.5k-62.5k, etc. up to 100k. That should give you 7 windows of data. Perform an FFT on each window, then sum and average each FFT together to get one window. As you add each window and then average, if the frequency signature changes considerably, then you have not eliminated the transients. Continue to run the software until the window averaging of the FFTs converge to a constant signature. Then you have a sufficient number of time steps to compute the RMS without transient data.

To :

Stephen J Alter

Thank you sir for your time. I'm following your instructions.

regards

To:

Rajeev Kumar Singh

Thank you sir. I've also found the data sampling feature in fluent. It provides time averaging facility for the parameters. It works.

Dear Mr Frendi, since your answer is the very first one, I like to comment that it is very often neither possible nor aimed to receive a steady state in a transient simulation. It strongly depend on the case one is exploring. For instance, investigating turbulence under time varying BCs - how can one expect steady state? The question is clearly about averaging time varying data.

I am simulating an unsteady combustion using Fluent ; and i need to export some result of (radial temperature , mole fraction of species) of every time step and make the average of all this result .tille now i am saving my calculation every time step and export my result every time steps and calculate the average using exel , but this methode take a lot off time .

second question ; how many data result should i make the average of it (how many time step )

thank you

Hi Benmenine 

You can check the time averaging options prior to running the iterations. Once the option is checked, Fluent will do the calculations for you, and you can also provide the time stepping intervals.

As for your second question, it really depends on the nature of your problem and the solution behaviour. Once you do this for few cases, you can get a clear idea on how far you need to go.

Thanks

Hi Muhammad Rizwanur

How i control the start and the end of time average (Tstart=100 s and Tend=200 s) and what is meant by sampling interval ?

if i have time step=0.01 sec and want to make average from T=100 sec to 200 sec@Muhammad Rizwanur Rahman

Hi Zein

Long since I used this time sampling and currently not in the field of CFD. So far I can reconnect, fluent offers you to tick a check box to provide the sampling interval and other necessary details, i.e., internal iterations etc. For further control and input, writing a macro can help. Anyway, I am guessing from my memory so not sure indeed. I believe, Ansys support team is quiet responsive. also you can connect with current users through the forums.

Stephen J Alter

Although an old thread, I found it very relevant to what I need in my study on the wake of a rectangular cylinder in the vicinity of free surface. So I'm hoping I'll have a chance to have your comment on the following.

My study is aimed at investigating the stability of floating rectangular cylinders against hydrodynamic forces and torques. The CFD simulations are performed using Ansys CFX.

What visualization and post-processing of the results reveals is highly varying drag and lift time histories, perhaps corresponding to the complex wake patterns that seem to be non-periodic, i.e. no matter for how many timesteps I run the simulation, I'm not able to ensure, via visual inspection, the transient behavior fades away.

The procedure you suggested might be useful to me. However, I was wondering if there's any standard method of doing that. Could you please cite any reference?