How to set up BCs for k epsilon model
 

Hi,

I started to use OpenFOAM 2 weeks ago and as an exercise I would like to simulate the "elbow"-tutorial of Fluent's tutorial guide.
http://193.204.76.120/fluent6.2/help/html/tg/node12.htm

I set up the BCs for U and p, however I do not know how to define the BCs for k and epsilon. First of all, I calculated k according to

k = 1/2 * (u'_x² + u'_y² + u'_z²)

Since the elbow geometry has 2 inlets, I calculated two k, one for each inlet:

k_1 = 0.02 m² s¯²
k_2 = 0.5 m² s¯²

Now, I'd like to set the k file in the /0 directory. However, I don't know which patch field types I shoud use for the different patches. Should I use 'fixedValue' at the inlets and set the internal field to uniform 0 ? At the walls and the outlet I'd then apply a 'zeroGradient'.

I calculated epsilon to be

eps_1 = 0.01641 m² s¯³
eps_2 = 2.05122 m² s¯³

for the two inlets.
Here I though of using 'fixedValue' at the inlets, 'zeroGradient' at the walls and the outlet and setting the internal field uniformly to a value between eps_1 and eps_2, for instance to 1.

Was my choice okay, or do you have any suggestions?


Bye,

Julian

Hi and welcome to the daily fight against the elements (of OpenFOAM),

the BC should be

inlet:
U: fixed value
p: zero gradient
k/eps/omega: value

outlet:
U: zero ngradient
p: fixed value (0)
k/eps/omega: zero gradient

walls:
U: fixed value
p: zero gradient
k/eps/omega: zero gradient

the internal field value you can set the same as the inlet value, sometimes it helps starting the calculation. but mostly it seems to be so unimportant.

Anyway it will be overwritten after the first timestep.

The values for epsilon and k also seem to be uninteresting. just give a k intensity and it will calculate its values itself.

Hi,

thank you very much for the answer!

Just another short (greenhorn) question:
In which file do I have to define the 'k intensity' (by 'k intensity' you mean 'turbulence intensity', don't you)?
In case I define just the 'k intensity', will I have to initialise the internal field for k/epsilon with 0 and set the patch types to 'zeroGradient'.


cheers,

Julian

I generally use settings similar to what you find in the tutorials/compressible/rhoPorousSimpleFoam/angledDuctImplicit/0/

inlet:
U: flowRateInletVelocity
p: zeroGradient
k: turbulentIntensityKineticEnergyInlet
epsilon: turbulentMixingLengthDissipationRateInlet
omega: turbulentMixingLengthFrequencyInlet

outlet:
U: inletOutlet
p: fixedValue
k/epsilon/omega: inletOutlet

It is 'mostly' irrevelant which values you take for the initial k/epsilon/omega fields, but initializing with zero for things like epsilon is likely to be a bad idea (== no dissipation and/or divide-by-zero problems).

Using an inletOutlet for the outlets also seems to be a good idea. It works the same as a normal outflow, but if the flow happens to reverse, you have a defined boundary condition.

Remeber that the pressure is NOT relative in compresssible cases (ie, zero would be really bad idea). After making a transcription error once (Pa vs. bar), I always use the OpenFOAM dictionary expansion function. For example in 0/p:

internalField uniform 1.0e5;
boundaryField
{
...
outlet
{
type fixedValue;
value $internalField;
}
}


/mark

Dear Olesen

I have a question:
What does "$internalField" means (as a defined value for the outlet)? Does it mean that the value for the surface is the one of the cells that shares with the fluid? Or it takes another value? Thanks a lot

Juanma

None of the above. The "$internalField" is simply a dictionary expansion.
In this example,

The "$internalField" would expand to "uniform 1.0e5" (your initialization field itself). At later time steps, the value will be filled in with what OpenFOAM has calculated for the those boundary faces. For most cases it is only needed to ensure that the field is properly initialized and that the post-processing works correctly.

If you are playing about with using the dictionary variables, the utility "expandDictionary" can come in quite handy to verify that your dictionaries are actually getting expanded as desired.

Thanks for the quick reply!

I understand what you mean but, thinking in the initialization of the case for 0/k and 0/epsilon, if the inlet is defined as fixedValue for these variables, it will maintain the same value for all the iterations and depending on the definition for the others variables (i.e. p as fixedValue and U as zeroGradient) It would be better not to set the the turbulent variables as "fixedValue" but as "calculated". Is that true? Is there any problem to initialize k and epsilon as calculated at the inlet? Thanks again.

Juanma

But k/epsilon aren't 'calculated' at the inlet boundary. If you do this, your equations will be underspecified. Specifying the turbulent intensity and mixing length with the respective boundary condition types makes more sense. They'll need a'value' entry though (as previously described) to have properly initialized fields for the time 0.

hello All,
What would be better choice for specifying turbulence parameters??? "fixedValue" or "calculated through turbulent intensity and mixing length like turbulentIntensityKineticEnergyInletlike" ???

I suppose this should not matter as far as i am giving same BC for k and eps and omega etc.

i have same problem.
please tell me how and where can i define turbulent intensity ( i want 5%) for inlet velocity.
Regards.

Put this in "/0/k" file for inlet. 0.05 corresponds to 5%. The value is actual value of k that you can calculate from 5% Turb intensity. I am not sure whether it is significant or nor, but i think its better to use appropriate value nevertheless.

Thanks Nilesh,
You mean it is not necessary to define anything in 0/u file. if no, what is the meaning of this phrase? :
Best regards.

I have never used turbulentInlet as such, but i am guessing that you specify the turbulence in terms of fluctuating velocity (as in u+u'). I have no idea how exactly this BC works. You can specify turbulence this way as well, no doubt, but i think this is much specific way than giving turbulent intensity, which is approximate guess generally speaking. And if i am not wrong, turbulentInlet is not meant for RANS. It makes sense to use it for LES/DNS. In RANS we always solve equations for mean values and not for fluctuating part of any variable.

Even though you specify turbulence in "/0/u" file, still you need to initialize k and epsilon/omega in respective files. So to me specifying turbulence in k file makes more sense. I can't think of a way for calculating velocity fluctuations for specifying turbulence. How would you know what values to give?? At least i have never seen specifying turbulence with velocity fluctuations.

This is the description of turbulentInlet BC given in source code.

Description
Generate a fluctuating inlet condition by adding a random component
to a reference (mean) field.
Input:
referenceField
Mean field.
fluctuationScale
RMS fluctuation, provided as the fraction of the mean field.
alpha
temporal correlation factor;
the fraction of the new random component added to the previous
time-step (defaults to 0.1).

Thanks,
as you mentioned turbulentInlet is for LES/DNS. i searched in tut files and not found this inlet type for RAS.
i will add intensity to k and compare results with benchmark.
Best.

The BC settings are not correct. k-epsilon needs wall treatment. I don't if the other settings are oke !

It depends on your y+.

If your mesh be refined near wall and yPlus value be less than ~5 you don't need to use wallFunction and zeroGradient is the correct choice.

Best,

Hello Maysam,

That's right. Under a certain threshold for y+ the mesh can reproduce reasonably the growth of the boundary layer. BUT, I try to define k and epsilon as a zeroGradient and OF renames my k and epsilon files (as *.org) and writes a new ones with the wallFunctions inside the patch of the wall. Any suggestion?

Thanks in advance,
Juanma

I am running k-epsilon model with the simpleFoam solver, but the results are not converging. The initial residual for pressure remains the same after some value, in this case 0.002. :confused:

BC:
U file
inlet freestream value()
outlet zeroGradient
wall fixedValue

p file
inlet freestreamPressure
outlet zeroGradient
wall zeroGradient

k file
inlet fixedValue (20)
outlet zeroGradient
wall kqRWallFunction (20)

epsilon file
inlet fixedValue (50)
outlet zeroGradient
wall epsilonWallfunction (50)

nut file
inlet freestream (0)
outlet zeroGradient
wall nutWallFunction (0)

Can someone point out the wrong BC, please.

is there nobody on the forum with k-epsilon-openfoam experience ? :(

Hi Juan, I didn't face your problem before.
Hi Eren, I have doubt about using free stream for both U and P. I haven't used this boundary too.
Try using fixed value for U and zeroGradient for P and nut if possible in your case. i suggest to use settings same as tutorial settings.

Any other suggestions for these two problems will be appreciated.

Other possible for convergence problem of simpleFoam is running an unsteady case with this steady solver.

i had this experience. Switching to pisoFoam solved my problem.

How important is the initial values for k and epsilon. I know that it doesn't require exact values but what is maximum variation ? Or is it enough if it converges well with the right yPlus values.

Initial values are not important and your solution is independent on them but, you should set them exactly in boundaries.

This sounds as a contradiction !

I don't see any contradiction. what is set in 0 folder is not initial condition only. you should set also boundary condition in this folder. if you see e.g case/0/U what is written after "Internal field" is initial value and after "Boundary field" is boundary condition. boundary condition effects solution in next iterations but initial value doesn't.

Thank you ! I overlooked that. I have set that correct and now I have almost the same Cl. Only Cd is almost 2 times higher , y+ lies between 14-40 , average 29.5 . This is also not too bad.

Do you know what the cause of much higher Cd is ?

This seems to have worked for me. Internal flow,compressible:

SDuctOutlet
{

type inletOutlet;
inletValue uniform 200;
value uniform 200;
}
SDuctInlet
{
type compressible::turbulentMixingLengthDissipationRate Inlet;
mixingLength 0.005;
value uniform 200;
}
vol1face4
{
type compressible::epsilonWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0;
}


however...what should I do for freestream conditions parallel to the flow?
I have thins and I'm sure it's wrong

rightZmax
{type compressible::turbulentMixingLengthDissipationRate Inlet;
mixingLength 0.005;
value uniform 200;
}

Hi,
I tried to use those boundary conditions for my model.
I use a k epsilon turbulence model, and the simpleFoam (steady) solver.
At the inlet I fixed the value 1.5 for k since my flow's velocity is 10m/s et my turbulent intensity is 10%.

When I look at the k field and the epsilon field, they seem to be far from true as you can see in the picture I enclosed.

I think that this problem is related to the boundary condition at the outlet.
Do you have an idea about what could be the problem ?

Thx for all !

Similar Problem
 

I have a similar type of problem too. Why can not we set k=0 at wall boundaries. According to theory all the velocity fluctuations are zero at the wall boundaries hence k should be 0.

I gave this BC in one of my simulations and couldn't see k=0 at the wall in post processed results. Have attached the figure.

Please help me to figure this out.

I just forgot to tell that I found what was my problem : I has inverted my inlet boundary conditions with my outlet boundary conditions.
However, for your case, it seems like you have fixed a k value at the inlet and put zero gradient at the outlet.
Maybe you should try to see if your velocity boundary conditions are OK.

For your second question : there is no reason why k would be zero at the wall because the boundary condition is zeroGradient.
You use this boundary condition when you work with a wall function (see simpleFoam/pitzDaily tutorial for example). And when you don't use wall function, you can put a value near 0 on the wall. For example you can see the lowRekEpsilon model LaunderSharma tutorials.

It does not answer your question but it shows that these boundary conditions are classical.
The reason why we use zero gradient when we have a wall function was explained in another thread here : what i understood was that on the first cell the wall function creates a profile of k, espilon, U ... You do not see that because on your simulation there is only one value in one cell. But you should not actually worry about it.
This is all I know on the subject and there must be a lot of things I do not understand, so be careful with what i said !

BC for k
 

Thanks for your reply.

It seems that I have not expressed my question clearly in the previous post. I am very sorry about that.

The boundary conditions are exactly same for U and p as in your post on Jan 15 2013.

For k and epsilon I put
fixedValue condition at the inlet
zeroGradient condition at the outlet

And at the walls

for k , type fixedValue;
value uniform 0;

and for epsilon,
type zeroGradient;

for these conditions I got above diagram for k. You can see that I have explicitly set k=0 at the wall.

That is the problem I have. Why doesn't the diagram show k=0. Is it a wrong BC for the k-epsilon model.

Please give me a clue. Once again thank you in advance.

Hi,
Could you tell me if you use wall function ?
Maybe you should try to avoid using wall function for your case as you want to fix a value for k (which means not setting the BC nutWallFunction for nut).
Tell me if it helped.

Hi Julian,
Can you please share your files for the elbow tutorial if you still have them?
I am also trying to simulate the elbow tutorial with turbulence but not able to get turbulence and everything just looks laminar.

setting of omega BC"s
 

helo
I am trying to set up a case using rhopimplefoam solver and the kOmegaSST turbulance model model but I have difficulties defining the boundary conditions for omega.

in my case i have inlet , axis , upperwall, outlet so hw to define BC's for that ?

what Eren?you have set both p and U in inlet by values and both zeroGradient in outlet?
that's wrong obviously.
you should set p be value in outlet and whether p or U be value in inlet and the other be zeroGradient in inlet. k and epsilon seems be correct.

Boundary Conditions
 

Hello Everyone,

I see that you are quit familiar with all the BCs settings.

I have a question for you all about the settings of U,P,k,epsilon and nut. I am trying to model a 3D free surface flow (flow goes in [inlet] and the same flow goes out [outlet]) and I'm having a hard time setting boundary conditions for allthe U,P... .

I tried to follow some instructions suggested in this threads but I didn't really find what I need. So (as you can see in the pictures attached) I need to have in the Inlet a flow condition and outlet flow condition too. For the walls (k, Epsilon and nut) I used respectively :

- kqRWallFunction uniforme 1;
- epsilonWallFunction uniform 200;
- nutkWallFunction uniform 0;
(I copied the values from a tutorial)

I am using a simpleFoam solver with RASModel ---> kEpsilon

Can someone help me with th BCs it's the first time that I have to do the settings so I'm a little bit lost :confused:

Thank you

Dadou

Dadou: I can't see the attachments.

I Apparently it didn't work.

And Now ?

three things:

did you actually type "uniforme" in the input file?

try to set your free surface like freestream in the motorbike tutorial.

if no typos in the file, I would suggest a K-omega model, look into the forums for definitions and initial conditions settings.