CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)
-   -   some questions about the setting of a compressible case (https://www.cfd-online.com/Forums/openfoam/83950-some-questions-about-setting-compressible-case.html)

 xck1986 January 16, 2011 17:03

some questions about the setting of a compressible case

hi everyone,

I want to use rhoSimpleFoam to simulate a laval nozzel and I have some problems of OpenFoam setting.

1. in the 0 folder, there is a variable alphat. What mena this variable and how to calculate it?

2. Are the pressure and temeprature showed in ParaView totalpressure(temperature) or staticpressure(temperature)?

3. In the file thermophysicalProperties in constant folder, I have set the following for the air:

thermoType hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>;
mixture air 1 28.9 1007 0 1.84e-05 0.7;

But what means the value 0 1.84e-05 0.7 here?

4. For pressure I have set a totalpressure boundary condition for the inlet of the nozzel.

type totalPressure;
p0 uniform 203250;
U U;
phi phiv;
rho none;
psi psi;
gamma 1..4;
value uniform 203250;

What is the difference between p0 and value. I think p0 should be the total pressure but what means value uniform 203250, is it the static pressure?

Thanks a lot.

 nakul January 17, 2011 04:57

Hi,

1 Variable 'alphat' is turbulent thermal diffusivity. You need not worry about it. It is calculated during the run. So even if you delete it from 0 folder there wouldn't be any problem.

2. They are static values if at the point of interest fluid is in motion.

3. 1.85e-6 is value of viscosity coefficient needed because of "constTransport" and 0.7 is Prandtl No. (Refer the User Guide for details)

4. That "value" is where you specify the value of your Po. Just search this BC in this forum and you would find the necessary details.

 xck1986 January 17, 2011 09:53

Quote:
 Originally Posted by nakul (Post 290694) Hi, 1 Variable 'alphat' is turbulent thermal diffusivity. You need not worry about it. It is calculated during the run. So even if you delete it from 0 folder there wouldn't be any problem. 2. They are static values if at the point of interest fluid is in motion. 3. 1.85e-6 is value of viscosity coefficient needed because of "constTransport" and 0.7 is Prandtl No. (Refer the User Guide for details) 4. That "value" is where you specify the value of your Po. Just search this BC in this forum and you would find the necessary details.
Hi Nakul,

And still two questions are not clear for me:

1.In the file thermophysicalProperties,
thermoType hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>;
mixture air 1 28.9 1007 0 1.84e-05 0.7;

What means the value 0here?

2. Is it possible to visualise the Mach Number in ParaView? Do I need to also define the boundary and initial condition for Mach number in the 0 folder?

Thanks again!!!

 nakul January 20, 2011 05:27

Hi,

As I have told you earlier, if you go through user guide you will find that

1) "1007" is value of Cp and "0" is for heat of formation as required by the "hConstThermo" model.

2) Yes after the simulation ends just execute the command Mach and in each time directory a field called Mach would be created. After that you would be able to visualise Mach No. in paraView.

 camoesas September 26, 2011 05:18

HI,

I am trying to set up a compressible case with SST turbulence model. For that I am trying to understand the rhoPimpleFoam/ras/cavity tutorial. IŽd like to join in with some questions:

1) What is the variable 'R' ? And how to calculate it? (Edit: maybe Reynolds stress? Would match dimensions.)

2) Why do I have to set for an compressible case epsilon and mut (instead of nut)? Do I calculate mut this way: mut = nut * rho ? And do I calculate epsilon just like in an incompressible case?

thanks a lot

Camoesas

 nakul September 26, 2011 13:10

Hi,

1) Can you post the code snippet in which R is used? The code for the solver is located in applications folders of your OF directory!!

2) You have to provide BCs for turbulence parameters also. The parameters for which you provide value depend upon the turbulence model that you chose. You may read about OF's SST model on OF wiki (Turbulence Modelling Section). It would clear all your doubts regarding this model.

-Nakul

 camoesas September 27, 2011 11:40

Hey Nakul,

1) R is used in tutorials/compressible/rhoPimpleFoam/ras/cavity/0

2) I know I have to provide boundary conditions for turbulence parameters. But in a compressible case you just have to give k and omega for SST Model...

regards

 nakul September 27, 2011 14:24

Hi

1) Could you just post that file about 'R' here? I won't be having access to OF for few days so I can only reply by having a look at the details of this variable here?

2) If you have confirmed that only k and omega need to be specified, just specify these values in '0' folder. Other files (nut and mut) would be created automatically. You need not create them.

-Nakul

 camoesas October 4, 2011 06:22

HI Nakul,

Here's the 'R' file:

Code:

```/*--------------------------------*- C++ -*----------------------------------*\                                                                                                    | =========                |                                                |                                                                                                    | \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |                                                                                                    |  \\    /  O peration    | Version:  2.0.0                                |                                                                                                    |  \\  /    A nd          | Web:      www.OpenFOAM.com                      |                                                                                                    |    \\/    M anipulation  |                                                |                                                                                                    \*---------------------------------------------------------------------------*/                                                                                                    FoamFile                                                                                                                                                                            {                                                                                                                                                                                      version    2.0;                                                                                                                                                                    format      ascii;                                                                                                                                                                  class      volSymmTensorField;                                                                                                                                                    location    "0";                                                                                                                                                                    object      R;                                                                                                                                                                  }                                                                                                                                                                                  // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //                                                                                                                                                                                                                                                                                        dimensions      [ 0 2 -2 0 0 0 0 ];                                                                                                                                                                                                                                                                                                                                    internalField  uniform ( 0 0 0 0 0 0 );                                                                                                                                                                                                                                                                                                                                boundaryField                                                                                                                                                                      {                                                                                                                                                                                      movingWall                                                                                                                                                                          {                                                                                                                                                                                      type            kqRWallFunction;                                                                                                                                                    value          uniform ( 0 0 0 0 0 0 );                                                                                                                                        }                                                                                                                                                                                                                                                                                                                                                                      fixedWalls                                                                                                                                                                          {                                                                                                                                                                                      type            kqRWallFunction;         value          uniform ( 0 0 0 0 0 0 );     }     frontAndBack     {         type            empty;     } } // ************************************************************************* //```

 fcollonv October 7, 2011 17:56

Hi,

1) The 'R' is effectively the Reynolds stresses. It's there so if you choose a turbulent model transporting the reynolds stresses the case will run also. But if you the SST model, the solver won't even read 'R' because it isn't needed.
2) Concerning mut, nut (or in LES muSgs or nuSgs), the interest at the zero time folder is to determine which law of the wall, you want to apply. I actually don't know which one is chosen by default when mut/nut is not specified by the user.

Bye

Fred

 All times are GMT -4. The time now is 08:43.