[camille131]

Good evening,

I am a new CFD user, I have to simulate a burner with reactingFoam but I'm not sure of the fineness of my mesh.

The chamber is a cylinder 50 cm long and has a diameter of 20 cm
Since it is a axisymmetric problem, I try to simulate only a wedge of the cylinder of 5° and one cell thick.

I suppose the mesh is finner at the inlet and near the wall , and is coarser at the outlet.

but how many cells do I have to set? or either what is the necessary size of the smallest cell ?

- First if I use the RANS calculation ?
Is there a thumb rule like with LES simulation? h<30 n where h is the grid size and n is the kolmogorov length scale

Thank you in advance for you answer

Cam

[camille131]

Nobody can help me?

[Lieven]

Hi Camille,

The best way of determining the number of cells required, is by performing a grid sensitivity study.
Start by solving your problem on a coarse grid and systematically refine it. For each simulation, calculate a parameter that is of importance for you (something similar like the drag force on a cylinder). At a certain moment the parameter will stop changing with increasing number of cells and that's the number of cells you would want to use.

Have fun!

Cheers,

L

[camille131]

Hi Lieven,

Thank you very much for your answer, I'll try this and let you know.

So if I have to try simulation for différent meshes I have to know how long I have to simulate the case?

In laminar I think it is common to simulate a certain time to ensure we are in steady state such as 10 times the real time needed. Is it right? c.f. user guide U-22

In a first time I'm using RANS so does it has an impact ?
the velocity : U = 5.77 m/s
the chamber's length : L = 51e-2 m
so the time needed for the mix to run along the chamber : t = L/U = 0.088 seconds

so if I simulate 1 s it is far enough, is it?

And what if I use k-Epsilon model?
and then LES ?

Thank you for your help

Cam

[chegdan]

Just to add a little to what has been said. For RANS, in addition to grid size independence, your turbulence model will have some y+ value requirements. You will need to run a simulation, determine the y+ and then adjust the mesh appropriately (refining or even remeshing). Different turbulence models will need different y+ values.

[camille131]

Hi Dan,
thank you for you response.

So I 'd like to use the app here : http://www.cfd-online.com/Tools/yplus.php

but I'm not sur of all my parameters...

Input Freestream velocity: 5.77
[m/s] Density: 0.6709 (for CH4)
[kg/m3] Dynamic viscosity: 1.5e-5
[kg/ms] Boundary layer length: ?? don't know
[m] Desired Y+ value: ?? don't know
[]
Output Reynolds number: [] Estimated wall distance: [m]

So I don't know either the boundary layer length neither de desired Y+ value ?

And what will I do with the results? :-/

Sorry I m a bit lost...

[camille131]

I stil don't know how long do I have to simulate the case?

with combustion turned on TRUE and chemistry turned ON with laminar-RASModel in turbulenceProperties it took more than 1 day and 20 hours to run on 8 CPU in parallel and then fail at 1.4 seconds... :-/

[chegdan]

With problems that are in really complex systems, its best to stage your solution procedure to push towards an overall solution. Do cold flow, i.e. no temperature, no reactions, no radiation...just momentum. Then slowly make your simulation more complicated by adding turbulence, temperature, chemistry, etc. and you will move towards your final goal.

For y+, use the yPlusRAS utility in OpenFOAM. It is a post processing tool, so run your cold flow to steady-state and then get your yPlus values. Remesh were necessary, map the values from your old solution to your new mesh with mapFields and then continue until you get an appropriate yPlus value for that turbulence model. Once this is good....then move onto more complicated physics by adding temperature. Make sure to check you y+ when you move to new physics as it may change from the added transport effects.

[camille131]

Hi Dan,
thank you for the precisions.

I ll try to run my case in "cold flow" and then postProcess it with the yPlusRas utility for which I'll surely have some questions...

but for the moment then : I switch off turbulence, combustion and chemistry such that :

chemistryProperties
--> chemistry off;

combustionProperties
--> combustionModel PaSR<psiChemistryCombustionModel>;
active false;

tubulenceProperties
--> simulationType RASModel; --> RASProperties laminar;

You told also no temperature , so what does that mean in term of BC?

here is my T bcs , what should I change to run cold flow?

And how longdo I have to run the case to be in steady state ?

My chamber is a cylinder of 0.51 m long with 0.22 m of diameter and the initial velocity is 5.77 m/s. the inlet is a circle with 0.035 m diameter.

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 1 0 0 0];

internalField uniform 293;

boundaryField
{
inlet
{
type fixedValue;
value uniform 293;
}
leftWall
{
type wallHeatTransfer; // verifier av mes valeurs
Tinf uniform 293;
alphaWall uniform 20;
value uniform 293;

}
upWall
{
type wallHeatTransfer; // ou fixedGradient?
Tinf uniform 293;
alphaWall uniform 10;
value uniform 293;
}
outlet
{
type inletOutlet;
inletValue uniform 293;
value uniform 293;

}
frontAndBack
{
type wedge;
}
axis
{
type empty;
}
}

[chegdan]

As an optional method (preferred), you could use simpleFoam. A laminar or turbulent steady-state solver for isothermal, incompressible, non-reacting flows. The take that flow field and move back to your current solver.

[Lieven]

If you set if you set the RASProperties to laminar, you will probably never reach steady state. Wel ok, it depends on the Reynolds number (with very low Re you might reach a steady state) but since you want to use a RASModel I'm assuming the flow will be turbulent.

So my advice, either run the laminar-case for 100 timesteps or so and enable then the turbulence model (you can simply do this with the 'turbulence on/off' flag instead of changing the RASModel in RASProperties). This way you simply get a better initial velocity field for the turbulence model. Or alternatively, you can simply try to start your simulation with the RASModel enabled. I you don't set the time step too big, this will work as well...

Cheers,

L

[camille131]

Hello,
Well here is my case, http://dfiles.eu/files/y5fimgxvz


I ran it with icoFoam , no chemistry, no combustion an RASModel for turbulence.

- first I ran it also without transportProperties file but to use the yPlusRAS utilty, OF asked me this file. Then I added it with cinematic viscosity 1e-5 m²/s and transportModel Newtonian..

Now I check the yPlus files in each timeStep but it is value 0 everywhere.. so what am I suppose to understand?

is it because I have this message at each time step :

no nutkWallFunction patches

What Am I supposed to do to correct that?

In another case (ran with reactingFoam I tested YPlusRAs utility with -compressible option but OF told me at each time step :

no rho field

what am I supped to do for that case?

Thank you for your help

[chegdan]

There seems to be some miscommunication here

Your ultimate goal is to get a full simulation of a reacting flow in a chamber. In order to do that you will need a flow field, species transport, and possibly temperature field. In a previous post, I suggest you start with solving only momentum, and if the system is in a regime in which steady-state flow can be achieved, I would use simpleFoam. SimpleFoam is a steady state solver for isothermal flows. it can model both laminar and turbulent (using RANS) flows where the user defines what turbulence model to use e.g. laminar, kEpsilon, etc.

[camille131]

Sorry I am lost . I thought I had to use yPlusRAS utility on the simple case with only transport.

Isn't it ok for the case I just posted?