Dear all, I'm simulating he
 

Dear all,

I'm simulating heat trasfer to water at pressures higher than critical (22.1MPa) and in this region, the results are extremely sensitive to the accuracy of thermo-physical properties implemented. Therefore their correct implementation is of a critical importance for me. New IAPWS-IF97 water properties standard functions shows a very high accuracy and therefore i would like to have them implemented to OpenFOAM.
Basically, when hThermo model with pureMixture, sutherlandTransport, specieThermo, janafThermo, perfectGas is used as a template, methods in sutherlandTransport, janafThermo and perfectGas equations can be overloaded for this purpose.
My question is: when i create new transport, thermo and equationOfState clases, how do i link them to the rest of the code, so for example buoyantSimpleFoam would use them in the following form, let's say:
hThermo<puremixture<iapwstransport<speciethermo<ia pwsthermo<waterrealgas>>>>>

Thank you in advance

David

Hi David, I've been discuss
 

Hi David,

I've been discussing this with both Henry and also Niklas Nordin who's responsible for much of the thermodynamics structure in OF. It seems from these discussions that one way to implement a full thermodynamics package like the IAPWS-IF97 for water and steam which return both transport and thermo properties is by introducing the following classes:

IAPWSgas in addition to perfectGas
IAPWSthermo in addition to hConstThermo/janafThermo
IAPWStransport in addition to constTransport/sutherlandTtransport

then we have the following thermoType (through changes in basicThermos.C)

hThermo<puremixture<iapwstransport<speciethermo<ia pwsthermo<iapwsgas>>>>>

For multiphase flows it might help with a waterSteamMixture class to help with voidfraction dependent properties but this is probably best implemented on application level together with the interface functions.

We currently have all necessary IAPWS functions written in OpenFOAM syntax for implementation in the new classes.

Niklas recently implemented Peng-Robinson equation of state which also might be helpful.

Any new ideas would be much appreciated.

//Eric

Hi all, if you are interested:
 

Hi all, if you are interested:
I found IAPWS'97 properties as C++ library (FreeSteam) in www.sourceforge.net

I have already adpated this library to OpenFoam 1.4(but it really slows down the calculation process)

If someone needs more information, please, write to my e-mail:
mkraposhin@inbox.ru

SORRY FOR BAD ENGLISH

Dear All, Does anyone know
 

Dear All,

Does anyone know what definition of compressibility does OpenFoam use? I found that perfectGas psi() function returns 1.0/(R()*T). Assuming that compressibility is defined as psi=(-1/rho)*(drho/dT) at constant pressure, psi function should return 1.0/T.
I need the exact defintion in order to apply the compressibity for water in the correct way.
Thank you so much in advance,

David

Hi my impression is that psi=
 

Hi
my impression is that psi=rho/p.

PerfectGasI.H, line 48:
//- Return compressibility rho/p [s^2/m^2]

This is in agreement with basicThermo.H, line 205

//- Density [kg/m^3]
tmp<volscalarfield> rho() const
{
return p_*psi();
}

It would be very interesting to hear about your progress in implementing IAPWS-IF97.

Henrik

Thank you Henrik, So the de
 

Thank you Henrik,

So the definition of compressibility is psi=drho/dp at constant temperature which gives exactly rho/p for an ideal gas. Please could anyone confirm that i'm right?
In that case the density which is returned by basicThermo.H, line 205 (see below) is valid only if we use ideal gas approximation. Am i right?

//-Density [kg/m^3]
tmp<volscalarfield> rho() const
{
return p_*psi();
}

Thank you,

David

hmm, thread started a year ago
 

hmm, thread started a year ago...
is there anything new on freesteam/OpenFOAM integration? I'd like to try

Maxim, The issue which i poi
 

Maxim,
The issue which i pointed in the message above, Friday Aug-29 must be solved before you try anything.

David

Hi David I absence of input f
 

Hi David
I absence of input from people who actually know things, allow me to speculate. Unfortunately my knowledge of c++ is rudimentary, so I can't offer any solutions. However, the problem seems to be two-fold:

1. rho is not stored explicity by basicThermo, but constructed as p*psi. Can this be avoided by having basicThermo fetch the density directly from the equation of state, thereby bypassing psi in the calculation of density?

2. The second problem is that psi itself is called from various bits of the source code. I guess that means that we still need a proper definition of psi, even if the density may be possible to calculate even without using psi.

Best Regards
Henrik

Hej Henrik, I absolutely ag
 

Hej Henrik,

I absolutely agree with your points. Rho should be fetched from the equation of state, i am just wondering why OpenFoam doesn't do it this way. And i also agree that psi must be correctly implemented into the equation of state ( in the form: psi=drho/dp at constant temperature).

What i did until now is that i took the water properties, IAPWS-IF97 as implemented in matlab functions of XSteam and use them instead of mu(), kappa(), alpha(), cp(), h(), rho() and psi() functions in thermo, transport and equationOfState objects (one MSc student of Eric Lillberg helped with coding).
These functions differs in different regions of phase diagram, resulting into quite an ugly piece of code. Moreover, when the functions are called directly, they slows down the CFD calculation rapidly.
That's why i decided to use an other approach. Here i call the XSteam functions only when the contructor of thermo, transport or equationOfState is called and create the tables where user specifies the minimum and maximum temperature, number of points and reference pressure. Then all the points are generated at the begining of calculation (which takes around 1-2 minutes depending on the number of points) and during the run-time functions mu(), kappa() etc... use just the linear interpolation between two nearest points depending on the temperature. This approach is really fast and could be quite precise, depending on the size of your lookup table.
I quickly wrote the code (except psi(), which is not defined by XSteam IAPWS functions) and as i remember it runs quite ok. Later i gave up my work on that because i didn't need water properties anymore and didn't even have time for that. If you are interested we can try to make it work and finally solve the issue of water properties, however i warn you, the code at this stage is quite ugly (i just cannot manage to make all the indentations, comments etc..)

David

Hi David Your work is very in
 

Hi David
Your work is very interesting, but for my current projects the full IAPWS-IF97 is probably over-kill. Instead I have tried to write dedicated equations of state (e.g. rho as a polynomial function of T) to use mainly for flow of liquid water. To that end I still need to understand the function of psi. If you get any further with this, please let me know.

Henrik

Dear Henrik,
I am facing exactly same problem now. Please share your valuable thoughts if you have found solution of above 2 problems ?

Best Regards,
JM

IAPWS 97 Properties, liquid Sodium (Na), properties, Bismuth-Led (BiPb) properties
 

Dear friends, here is link to water, Na and BiPb properties

http://www.os-cfd.ru/mamb/index.php?...1a69&no_html=1

Thankyou very much Matvej !!

JM

I am starting to investigate how to implement the water properties into openfoam at supercritical pressures. In IAPWS-97, the properties, such as specific heat capacity, are functions of density and temperature in the region 3 which includes the critical point. This does not agree with the style of thermalphysical model in OpenFOAM. Is there any smart solution for this?

Thanks in advance.

I am keep going with the implementation of IAPWS-IF97 in OpenFOAM. My approach consists of the following steps.

1) build the interpolation table at constant pressure with T as the abscissa.
The table is generated with the aid of freesteam which can generate all the properties I need, such as density, enthalpy, entropy, heat capacity, conductivity and dynamic viscosity etc.

2) interpolate the properties according to T

The multi-layer implementation in my approach is
hPsiThermo<pureMixture<iapwsTransport<specieThermo <iapwsThermo<iapwsEOS>>>>>

This implementation is defined in thermophysicalModels/basic/psiThermo/hPsiThermo/hPsiThermos.H
with
makeBasicPsiThermo
(
hPsiThermo,
pureMixture,
iapwsTransport,
iapwsThermo,
iapwsEOS
);

A basicMixture is also defined in
thermophysicalModels/basic/mixtures/basicMixture/basicMixtures.C
with
makeBasicMixture
(
pureMixture,
iapwsTransport,
iapwsThermo,
iapwsEOS
);

However, the above-mentioned modifications doesnot make the implementation work. When I try to test the implementation with the tutorial case, buoyantCavity, I got the error
buoyantSimpleFoam: symbol lookup error: /home/jinbiao/OpenFOAM/OpenFOAM-2.0.1/platforms/linuxGccDPOpt/lib/libbasicThermophysicalModels.so: undefined symbol: _ZN4Foam14iapwsTransportINS_12specieThermoINS_11iapwsThermoINS_8iapwsEOSEEEEEEC1ERKNS_10dictionaryE

There seems something wrong with the dictionary lookup. The exact problem is still to be debugged.

Best,

Hello,

have you correctly included all libraries and paths for IAPWS-IF97? You should double check that.

Do you plan to make your code available?

Markus

Markus,

Thanks for your reply. I am also thinking about that there may be some mistakes in library linking. The implementation of thermophysical property in OF is complicated. I do not fully understand what is wrong.

I will consider to make my code available. But I donot how to do that. Should I add to the OpenFOAM-2.0.1-extend for example?

Hi,

maybe the libbasicThermophysicalModels is missing the link to the IAPWS-IF97 library.

And yes. The extend project is a good place. You can create an own account or have it put by another member.

Markus

Hi Markus,

I have solved the problem. I missed the line which includes the iapwsThermo.C file into iapwsThermo.H. And the same mistake in iapwsTransport.H. These files are not complied in the libspecie. Instead they were included in files like basicMixtures.C and consequently compiled in libbasicThermophysicalModels.

So the .C file should be included in the header files so that the libbasicThermophysicalModels can properly linked to them.

Now I am testing the implementation. I will try to create an account in the extend project soon. If the testing is good, I will share it.

Best,

Hi JinBao,

Christan Lucas at the TU Braunschweig has done some work on real gas thermodynamics which might find helpful. It includes implementations of aungierRedlichKwong, pengRobinson, redlichKwong, soaveRedlichKwong EOS.

Please checkout the feature/fullyIntegratedRealGasThermo branch on extend.

... and, yes, your contribution is more than welcome.

Best Regards,

Henrik

Hi Henrik, Thank you for the helpful information. Christan Lucas's approach is very interesting. I will try to apply it in my calculation. Christan Lucas provided the tutorial for CO2. I am not sure the library will work for water. I will share my experience here after I try it.

I am also trying to get a successful calculation with my own property library. Thanks again.

Regards,

Hi, JinBiao:

I am doing something with OpenFOAM using some real gas model.

I want to know where do you fine the "Christan Lucas provided the tutorial for CO2."

thank you

Hi,

you can find my code in the OpenFOAM extend on sourceforge. See link:

http://openfoam-extend.git.sourcefor...-ext;a=summary

Have a look at feature/fullyIntegratedRealGasThermo.

Best Regards
Christian

Hi Haomin,

I hope you have already get what you need. Because I am playing with water, I had no further experience with Lucas's library. But the structure of Lucas's implementation looks very good. Much better than I can do.

Good luck and enjoy it.

Regards,

Jinbiao

Hi Jinbiao,

I forgot to ask you, is your IAPWS-IF97 implementation working? Did you implement it yourself or are you using external libraries like freeSteam.

Best Regards,
Christian

Supercritical water properties in FLUENT
 

turbulent flow
 

hello, I'm just learning openFoam. could you tell me how can I simulate a turbulent flow? I know the icoFoam solver is only for laminar flow.
Thanks a lot,
Diego

Christian,

Would you mind explaining how to download and install your IAPWS implementation? Can it also be used in version 2.1.1 or only in 1.6?

Christian,

I am not very familiar with git, so I would appreciate your help. I have downloaded OpenFOAM-1.6 ext using

If I look for “src/thermophsicalModels/externalMedia” at this point, the externalMedia directory doesn't seem to exist. I'm guessing this is because I need to do something with the branches. I have tried
But after executing this command, I still don't see an externalMedia directory. Can you please explain what I need to do next? Thanks.

Hi,

try

git checkout -b feature/fullyIntegratetedRealGasThermo origin/feature/fullyIntegradetedRealGasThermo

maybe you need to use
git pull
afterwards

Regards,
Christian

Hi Chris,

can you please explain step by step how to get the branch?

Is the right one

feature/fullyIntegradetedRealGasThermo

or

origin/feature/fullyIntegradetedRealGasThermo?

I got the following messages:

>git checkout -b feature/fullyIntegradetedRealGasThermo origin/feature/fullyIntegradetedRealGasThermo

fatal: git checkout: updating paths is incompatible with switching branches.
Did you intend to checkout 'origin/feature/fullyIntegradetedRealGasThermo' which can not be resolved as commit?


>git pull
You asked me to pull without telling me which branch you
want to merge with, and 'branch.origin/feature/realGasThermo.merge' in
your configuration file does not tell me, either. Please
specify which branch you want to use on the command line and
try again (e.g. 'git pull <repository> <refspec>').
See git-pull(1) for details.

If you often merge with the same branch, you may want to
use something like the following in your configuration file:
[branch "origin/feature/realGasThermo"]
remote = <nickname>
merge = <remote-ref>

[remote "<nickname>"]
url = <url>
fetch = <refspec>

See git-config(1) for details.


Thanks a lot. Markus

Hi,

Follow this explanation (this is what I did)

http://gugod.org/2008/12/git-checkout-remote-branch/

Have a look at

http://openfoam-extend.git.sourceforge.net/git/gitweb.cgi?p=openfoam-extend/OpenFOAM-1.6-ext;a=summary

you can find the name of the branch, the changes in the branch ... there. The name is:


feature/fullyIntegratedRealGasThermo

Kind Regards,
Christian

Hi Chris,

you are right. So that is what I did (again):

Ok thanks for your patience.

Markus

Hi,

if you have the time, I would like to get a response regarding the code (problems, suggestions, ...)

Regards,
Christian

Hi everyone,

I'm trying to install freesteam and I had some problems with it. Does anybody have a tutorial in how to install the freesteam package?

Chris Lucas,
Is it possible to simulate superheated steam and supercooled steam using your code?

Best regards,
Felipe Magazoni

Hi,

have a look at the freesteam page, you can find the limits, in which the code works, there. The code works with superheated and subcooled steam.

Have you looked at the README file in the tutorial case I provided for freesteam (in OpenFOAM/tutorials/compressible/rhoPisoFOAM/RAS/IAPWS97_pipe)?

Have you installed all the required components for freesteam as stated in the README file in freesteam?

Could you post the error?

Kind Regards,
Christian

Hi Chris Lucas, thanks for help me.

Now, the freesteam package is correctly installed, but I installed it in the folder '/opt/freesteam'. The libfreesteam.so is not in a folder where OpenFOAM finds ($WM_PROJECT_DIR/lib/linux64GccDPOpt). Must I install the freesteam package in another folder?

After I tried to compile the IAPWS package and there are some errors,

Best regards,
Felipe Magazoni