
[Sponsors] 
Time step independence study for transient CFD simulation 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 3, 2013, 12:35 
Time step independence study for transient CFD simulation

#1 
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 15 
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?
__________________
Best regards, Meimei 

June 3, 2013, 12:48 

#2 
Super Moderator

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


June 3, 2013, 15:09 

#3 
Senior Member
cfdnewbie
Join Date: Mar 2010
Posts: 557
Rep Power: 20 
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.


June 3, 2013, 15:15 

#5  
Senior Member
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 503
Rep Power: 20 
Quote:
This is only half true. Since the timestepsize and cellsize are connected via Courant number you can only say that the solution is timestep indpendend for the current meshsize. And you don't know what this means unless you perform a study for mesh independence :) 

June 3, 2013, 15:22 

#6 
Senior Member
cfdnewbie
Join Date: Mar 2010
Posts: 557
Rep Power: 20 
Could be please explain why you think this would put a strict limit on the time step?


June 3, 2013, 15:53 

#7 
Senior Member
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 503
Rep Power: 20 

June 3, 2013, 16:08 

#8 
Senior Member
cfdnewbie
Join Date: Mar 2010
Posts: 557
Rep Power: 20 
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.


June 3, 2013, 17:30 

#9 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 26 
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? I'll be glad if you let me know your experience. Thanks.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

June 4, 2013, 04:01 

#10 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71 
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. 

June 6, 2013, 05:36 

#11 
Senior Member
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 503
Rep Power: 20 
I tried to describe a slightly more practical approach in my dissertation.
There I did the simulation of a sidechannelfan 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


June 6, 2013, 07:20 

#12 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 26 
Hi Joern
how could describe the more effect of time step on calculated torque?
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

April 10, 2014, 14:05 

#13 
New Member
Chandrasekhar
Join Date: Oct 2013
Location: new jersey
Posts: 24
Rep Power: 12 
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 

April 11, 2014, 07:14 

#14 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 26 
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 34 years I haven't work with Fluent, others helps are appreciated!
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

April 11, 2014, 11:58 

#15  
New Member
Chandrasekhar
Join Date: Oct 2013
Location: new jersey
Posts: 24
Rep Power: 12 
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:


April 11, 2014, 23:36 

#16 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 26 
Hi dear Chandrasekhar,
at first you should test some runs with different time steps, maybe 34 time steps that each one be around half or double in order from another , for example 1e8,2e8,5e8,1e9 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? ask me if you had any question
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

April 12, 2014, 03:56 

#17 
New Member

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!


April 12, 2014, 10:38 

#18 
New Member
Chandrasekhar
Join Date: Oct 2013
Location: new jersey
Posts: 24
Rep Power: 12 
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 

April 13, 2014, 06:22 

#19  
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 26 
Quote:
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.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

October 21, 2021, 14:43 

#20  
Member
Join Date: Sep 2018
Posts: 53
Rep Power: 7 
Quote:


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Superlinear speedup in OpenFOAM 13  msrinath80  OpenFOAM Running, Solving & CFD  18  March 3, 2015 05:36 
directMapped problem  panda60  OpenFOAM Bugs  4  July 8, 2010 10:23 
Time step in transient simulation  shib  FLUENT  0  June 17, 2010 13:07 
calculation diverge after continue to run  zhajingjing  OpenFOAM  0  April 28, 2010 04:35 
IcoFoam parallel woes  msrinath80  OpenFOAM Running, Solving & CFD  9  July 22, 2007 02:58 