Register Blogs Members List Search Today's Posts Mark Forums Read

 June 23, 2004, 13:43 Advection Time #1 Anne Guest   Posts: n/a Hi CFX Family, What is the implication or physical meaning of advection time (of say, water) in a stirred tank? Can this influence the choice of time step? Thanks anne

 June 23, 2004, 14:57 Re: Advection Time #2 Robin Guest   Posts: n/a Anne, What you really want to know is the physical timescale, advection time is one such timescale, but there are others. Basically, the physical timescale is the average time it takes for a change in one region of the domain to propegate throughout the entire domain. In terms of convergence, consider that if a change occurs and you timestep is set to be 1/10th of the physical timescale, the solver will require at least 10 iterations to propegate it's effects (and perhaps a few more for the non-linearities to settle down). If you choose a timestep which is 1/100th of your physical timescale, you need 100 iterations, and so on. So armed with this knowledge, what would you consider to be the physical timescale for a stirred tank? Regards, Robin

 June 24, 2004, 12:21 Re: Advection Time #4 Robin Guest   Posts: n/a Hi Anne, What I previously stated only applies to a steady state simulation, the timestep requirements of a transient simulation are altogether different. For a steady state, the transient terms in the equations cancel out when the solution has converged, since the solution is no longer changing (hence it has reached a steady state). When you run a transient simulation, however, you are trying to simulate the changes in time accurately and therefore need a timestep small enough to do so. Determining the right timestep can depend on a lot of factors, but probably the best way is by looking at what the code is doing. When you solve a transient simulation, the solver will perform a series of coefficient loops in order to converge the non-linear equations within the timestep, after which it advances the solution in time. Generally, you shouldn't require more than 3 to 6 coefficient loops to converge to a MAX residual of .001, or else your timestep is too large. When you start your run, you may find the solver requires more coefficient loops while it is getting over the initial guess. After 10 or 20 timesteps, the initial transients should have settled out and the solver will behave better. If you find you are still using too many coefficient loops, reduce your timestep, if too few, increase it. If you are interested, there is example code in the User FORTRAN documentation for a Junction Box routine which will do this automatically for you. Best regards, Robin

 June 29, 2004, 04:55 Re: Advection Time #5 Anne Guest   Posts: n/a Hi Robin, Thanks for such a lengthy explanation. There are some other CFD artefacts that may be implicitly relevant to our subject matter. When I run a steady state simulation (say frozen rotor), is the transient term set to zero automatically right from the beginning? What i THINK is that a TRS with a very 'big' time step is implicitly a steady state simulation (not necessarily a frozen rotor). However, I fail to connect the physical time scale and advection time with the time steps (either in TRS or frozen rotor). Many thanks for your time. anne

 June 29, 2004, 05:12 Re: Advection Time #6 Jeff Guest   Posts: n/a Anne, I can throw some personal experience in here on mixing tanks. Perhaps this can relate to what you are after. To acurately capture the transient startup, you need to look at cell width in the theta direction divided by tip speed. That is, the impeller shouldn't travel more than a cell width in one time step, or you won't accuately capture the transients. Using this method, experience shows at least 20 full revolutions of the impeller to get to a final steady state (which is an oscillating condition as impellers move past the baffles). If the startup is not of concern, frozen rotor can be done to get the fluid moving, before switching to a true transient impeller. This get's you a LOT closer to steady state and can cut down on the revolutions required. The step size here can be larger, but some fraction of the symmetry on the impeller. I don't know if this helps with your question, but it may help with your solution. Jeff

 June 29, 2004, 05:17 Re: Advection Time #7 ioana Guest   Posts: n/a Hello, Like Anne I encounter difficulties with the Physical time scale. I am simulating a fire and now I am trying to use the Flamelet model (I have just loaded the file supplied in the library Reaction.fll for methane air/flames at 1 bar and t = 298 K as I considered that it is very close from mine (methane is injected at t=302.27)- can this be the cause for the lack of convergence??; I did this because I want to see if I get diff results when comparing to others combustion models and if it worth starting with Chemkin). Anyway I have problems with convergence I have tried to calculate the physical time scale the formulas form help (dt=L/2U= 2.42; I haven't used the second one because I don't know what the"leghtscale associated with the vertical temp gradient" is). The physical timescale that I had obtained is bigger than the Advection Time Scale, so it does not work. I have tried different values: 0.00625 s, 0.0125 are too small, so I increased to 0.01875 is too big. Anyway the fact is when using 0.01875 after 2000 iteration I canot get convergence. Any advice is welcome Ioana

 June 29, 2004, 13:49 Re: Advection Time #8 Wu Jiurong Guest   Posts: n/a Dear Robin: Can you tell me where i can find such an example code in the User FORTRAN documentation for a Junction Box routine which will adjust the time step automatically in the transient simulation? Best Regards!

 June 29, 2004, 18:22 Re: Advection Time #9 Glenn Horrocks Guest   Posts: n/a Hi Anne, I don't think TRS with a big timestep is equivalent to a steady state simulation. TRS is a time accurate simulation which will show the full evolution of the flow; steady state will only show the final result of a steady flow. If you are running a TRS simulation and it has evolved to the steady state solution, then it won't matter what time step size you use as the transient term drops out anyway. Is this what you mean? Glenn

 June 30, 2004, 04:15 Re: Advection Time #10 Anne Guest   Posts: n/a Hi Glenn, Thanks for the correction . For a stirred tank we are discussing here, what i noticed was that when i took a time step equal or greater than one revolution time, the convergence was similar to that of a steady state assumption. That led me to think they way i did. I would be hesitant to use the word equivalent because that may imply that we are equating a TRS to steady state (or frozen rotor), the mathematics involved is certainly differrent. Things that behave in a similar fashion (implicit behaviour) may not be equivalent. Sorry, if i used wrong words. But Glenn/Jeff/Ioana, what is the physical meaning of advection time in a transient flow in a stirred tank? kind regards anne

 June 30, 2004, 16:03 Re: Advection Time #11 KKA Guest   Posts: n/a Hi Wu (is Wu your first name?) Go to the user manual, (the pdf folder), click on the master directory then expand the Solver Modelling Link, you'll find the User Fortran, there you'll find the code he was talking about!!! Regards!!

 July 10, 2004, 08:38 Re: Advection Time #13 Ben Guest   Posts: n/a Hi Robin, This is a very generous response considering the depth of explanation and the time taken to type this down. Let me go thro is slowy and try to get all that you have put down here. Thanks a million Robin. Regards, annne

 July 10, 2004, 08:53 Re: Advection Time #14 anne Guest   Posts: n/a Sorry Robin, I used one of my CFD student's profile in the above posting. However the words remain the same. Regards, Anne

 March 1, 2018, 06:17 Advection time #15 New Member   pnr Join Date: Oct 2017 Posts: 3 Rep Power: 8 Hi Robbin, If there different domains, say two stationary and one rotating regions and each has different Advection time and usually rotating region has very less Advection time. So which one to be considered for physical time scale . please elaborate. Thanks, Regards PNR

 March 1, 2018, 16:53 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,729 Rep Power: 143 Robin has not been seen on the forum for decades, sadly. This is a 14 year old thread..... Advection time should be the time taken for the flow to pass through the entire flow path. This may cover multiple domains, some big some small. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Lord Kelvin OpenFOAM Running, Solving & CFD 8 March 28, 2016 11:08 xujjun CFX 9 June 9, 2009 07:59 lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 14:09 Atit Koonsrisuk CFX 1 June 11, 2007 05:37 özgür FLUENT 8 January 6, 2004 08:23

All times are GMT -4. The time now is 08:19.