CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

 osimonsimon November 6, 2006 17:17

Hi, this problem bothered me f

Hi, this problem bothered me for a while and I really couldn't find a way to figure it out. Basically I am running a 3D simulation using simpleFoam. The model is like a room with multiply inlets (nine) and oulets (two). All of them are velocity inlets(outlets), i.e. the velocity is known at all these boundaries. I followed the tutorial to calculate the initial k and Epsilon at time "0" for all the boundaries. And also set the value for the internal field by guessing a number within the range (between min and max of k(or Epsilon)). I found that the convergence is GREATLY depended on the initial guess of k and Epsilon for the internalField and very sensitive to them. The flow field is also stongly depended on the initial guess of k and epsilon. I've tried a lot of combinations and still have problems getting expected convergence.

Does anyone have any suggestions to this kind of problem? This problem holds me up for quite a while and it is killing me... Please help! Thank you a bunch!

 eugene November 7, 2006 06:05

Well I am surprised you get an

Well I am surprised you get any convergance at all seeing as you have specified the velocity on all boundaries. The system is over-specified. Try making (at least one of) the outlet velocities zeroGradient.

At convergance simpleFoam results should be more-or-less independant of the starting conditions.

 osimonsimon November 7, 2006 09:27

Thanks Eugene. Sorry I forgot

Thanks Eugene. Sorry I forgot to mention that there is an outlet that is velocity zeroGradient and zero pressure.

 eugene November 7, 2006 12:24

As long as your boundary condi

As long as your boundary conditions are the same, the flow should converge to an identical solution independent from the initial conditions. Of course convegence will be affected by the initial conditions, this is normal.

Specifiying a fixed value outlet velocity is not a very good idea even if you have zeroGradient on one of the oulet boundaries. What we really need is some kind of flow split boundary if the mean outlet mass flow distribution is known. This is doable, but has not been implemented to date.

Also, make sure your k and epsilon are zero gradient on the fixed value outflow boundaries. Check that you have no inflow at your zero-gradient outflow boundary, this tends to cause a lot of stability problems. Typically you should run potentialFlow to get a reasonable initial guess for velocity, and use the inletOutlet boundary with inletValue set to (0 0 0) to prevent inflow.

We are working on a more sensible way to specify the initial conditions, but for the time being you have to provide it. For turbulence properties I typically use the values calculated from turb intensity, velocity and lengthscale at the inlet to populate the internal domain.

 olesen November 8, 2006 02:48

I can't promise that it will s

I can't promise that it will solve your initialization problems, but you could try using this http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif setKepsilon.tar.gz utility for setting tke and epsilon based on turbulent intensity and length scale. The initial epsilon values seem to cause most of the stability problems.

 osimonsimon November 8, 2006 11:58

Thanks Eugene and Thanks Mark!

Thanks Eugene and Thanks Mark! I really appreciate your help!!

Eugene, thanks for your advise. They do improve the convergence but not much. I changed the k and epsilon to zero gradient on the fixed value outlow boundaries. And no inflow was observed. I was using the same method calculating the initial value of k and epsilon at inlets. For the internal Field, I just pick one a value from those on the inlets. Now I just change these two values (initial valuce of k and epsilon for internal field) and the convergence varies a lot. Some times it getting singularity solutions; sometimes it blows up (continuity); sometimes it converges to 1e-6 for all the variables, but the k is around 3~12 and epsilon is around 20~30, something like that...I am really confused about this. Any comments about these?

Again, thanks very much for you guys' help!

 olesen November 9, 2006 02:48

I just downloaded the utility from the server without a hitch, but the downloaded filenames are indeed a bit odd. In this case it is 'setKepsilon_tar-3364.unk', but the file command reveals that it really is a gzip'd tar file. Just rename and you should be fine.

 osimonsimon November 9, 2006 10:43

Yep, you are right. It works.

Yep, you are right. It works. I will try this out. THanks a lot, Mark!

 chegdan April 23, 2008 19:05

Does anyone have a good source

Does anyone have a good source explaining what the inlet conditions for k and epsilon should be or how they should be calculated? I'm running a case in simpleFoam of a turbulent reactor (using the k-epsilon model) and I have no idea what the inlet value of k and epsilon should be. Thoughts?

 ryan_m April 23, 2008 19:44

Hey, Try the Fluent online

Hey,

Try the Fluent online user manual:

http://jullio.pe.kr/fluent6.1/help/h....htm#ke-params

It got some pretty simple equations to use for determining turbulent inlet conditions.

Cheers

 olesen April 24, 2008 02:52

That's where the two following

That's where the two following bc types should be useful:

Calculate turbulent kinetic energy from the intensity provided as a fraction of the mean velocity.
Example of the boundary condition specification:
inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05; // 5% turbulence
value uniform 1; // placeholder
}

Calculate epsilon via the mixing length [m].
Example of the boundary condition specification:
inlet
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.005; // 5 mm
value uniform 200; // placeholder
}

... assuming, of course, that you have an idea of which intensity and length scales might be relevant for your case.

 All times are GMT -4. The time now is 23:21.