CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Main CFD Forum (https://www.cfd-online.com/Forums/main/)
-   -   Time step independence study for transient CFD simulation (https://www.cfd-online.com/Forums/main/118746-time-step-independence-study-transient-cfd-simulation.html)

 Anna Tian June 3, 2013 12:35

Time step independence study for transient CFD simulation

Hi

I'm a beginner of transient CFD simulation. I'm wondering what are the typical approaches(steps) of the time step independence study for the transient simulation? Any good summary or paper on that? How to quantity the time step dependency? What is the criteria of the time step independency?

 Far June 3, 2013 12:48

Take a representative time step for your case. Simulate it and decrease time step by half. Again simulate and compare your results. If your results haven't changed much, you have achieved time independence :cool:

 cfdnewbie June 3, 2013 15:09

I would suggest a more stringent approach. Choose your spatial discretization fine enough to guarantee your spatial errors is magnitudes below your temporal error. Then do a temporal convergence study and check the order of convergence of your temporal integration. This will show you whether you are in the sufficiently resolved regime and converging towards time independence.

 Far June 3, 2013 15:15

This would put a strict limit on time step choice. This choice would be better for LES !!!!

 JBeilke June 3, 2013 15:15

Quote:
 Originally Posted by Far (Post 431723) Take a representative time step for your case. Simulate it and decrease time step by half. Again simulate and compare your results. If your results haven't changed much, you have achieved time independence :cool:

This is only half true.

Since the time-step-size and cell-size are connected via Courant number you can only say that the solution is time-step indpendend for the current mesh-size. And you don't know what this means unless you perform a study for mesh independence :-)

 cfdnewbie June 3, 2013 15:22

Could be please explain why you think this would put a strict limit on the time step?

 JBeilke June 3, 2013 15:53

Quote:
 Originally Posted by cfdnewbie (Post 431750) ... Choose your spatial discretization fine enough to guarantee your spatial errors is magnitudes below your temporal error.
That's probably possible for academic problems but usually wishful thinking in the real world.

 cfdnewbie June 3, 2013 16:08

True, but since she asked about how to quantify the temporal accuracy and the criteria, it never hurts to take a look at the most stringent and correct way.

 immortality June 3, 2013 17:30

hi dear Anna
I didn't know i have to do a time step dependence study as well as grid independence.
Then i should set time step constant and don't use maxCo,right?
Thanks.

 FMDenaro June 4, 2013 04:01

My opinion is that one should see the structure of the local truncation error. It is done by a combination of power of time step and spatial step, a rigorous theoretical estimation of the consistence of any scheme requires that the local truncation error goes to zero for dt and h going simultaneously to zero (with dt/h = constant). The convergence slope gives the accuracy of the scheme.
However, if you want to check only the temporal part of the scheme there is only a way, fix the smallest possible value for the spatial resolution (so that you can assume disregardable contribution of the spatial errro in the local truncatio error) and do the convergence test.
Of course, similarly you can work by fixing the smallest time step and study the convergence by reducing the space size.

 JBeilke June 6, 2013 05:36

I tried to describe a slightly more practical approach in my dissertation.

There I did the simulation of a side-channel-fan with sliding mesh and pressure bc at inlet and outlet. The resulting integral quantities are the mass flow and the impeller torque.

It turned out, that the impeller torque was much more sensible to a change in the time step size than the mass flow. So I decided to take
• the average value of the impeller torque and
• the smoothness of the curve over the time
as a criterion.

 immortality June 6, 2013 07:20

Hi Joern
how could describe the more effect of time step on calculated torque?:)

 chandrasekhar April 10, 2014 14:05

Hi
i would like to know how to ensure grid independence for a transient case(i.e how to check if a given transient case is grid independent or not). i know that i have to compare the velocity field (say) of the two meshes at the same locations for each time step, but i don't know how would do it in software like ansys fluent. any help on this would be appreciated. Many thanks for replying.

with regards
Chandra Sekhar

 immortality April 11, 2014 07:14

Hi Chandrasekhar
I've done it in openFoam, so you know the theory and want to know how to draw graphs of data you've obtaind from Fluent,right? I think you have to use the data and use a software like gnuplot for working on them and plotting but don't know the details about extracting the data in Fluent because its 3-4 years I haven't work with Fluent, others helps are appreciated!

 chandrasekhar April 11, 2014 11:58

Hi
thanks a lot for the reply. i have a doubt in the theory part itself. this is what i think i should do for checking grid independence- first run the cases with two meshes; then check velocity, pressure and temperature fields of the two cases at same locations; see error and decide. do i have to calculate all the three fields and compare the error or any one of them is sufficient. also do i have to check error over the whole domain or at certain locations is enough. Any help on this would be much appreciated. Many thanks for replying.

with regards

Quote:
 Originally Posted by immortality (Post 485433) Hi Chandrasekhar I've done it in openFoam, so you know the theory and want to know how to draw graphs of data you've obtaind from Fluent,right? I think you have to use the data and use a software like gnuplot for working on them and plotting but don't know the details about extracting the data in Fluent because its 3-4 years I haven't work with Fluent, others helps are appreciated!

 immortality April 11, 2014 23:36

Hi dear Chandrasekhar,
at first you should test some runs with different time steps, maybe 3-4 time steps that each one be around half or double in order from another , for example 1e-8,2e-8,5e-8,1e-9 or other numbers depending on how transient is your model. start from a bigger value and reduce it and see how results of velocity (especially) changes then select the value of time step that results doesn't change a lot at that time step compare to the smaller one. this way you can reduce the role of time step in numerical error to minimum and focus on the grid.
for grid independence do the same procedure of time step for the same location (the location that the most changes in fields or the most phenomena occurs there if there is such place in your CFD problem). and velocity is more important it doesn't have a specified rule, I saw in a thesis that only velocity was compared and I myself compared both velocity and pressure for more accuracy in two graphs. depends on your problem,whats the subject you are working on?

 DrAkram April 12, 2014 03:56

The suggested time steps seem rather short 1 - 80 nsec, may be important to see if the physical phenomena have that kind of time scales and the corresponding space step still keeps the model within continuum limits! :confused:

 chandrasekhar April 12, 2014 10:38

Hi immortality
thanks for your reply. i will try doing what you have said and see the results. the case i am working on is as follows- karman vortex shedding over a circular cylinder(in 2d). the problem is transient one. i am simulating this problem on ansys fluent. my friend is simulating the same problem on open foam and we are comparing the results.

with regards

 immortality April 13, 2014 06:22

Quote:
 Originally Posted by DrAkram (Post 485615) The suggested time steps seem rather short 1 - 80 nsec, may be important to see if the physical phenomena have that kind of time scales and the corresponding space step still keeps the model within continuum limits! :confused:
Hi,
I didn't suggest anything, what I said was only an example from the problem I was working on that was very transient in a very narrow tube.:)

 All times are GMT -4. The time now is 12:34.