[alfa_8C]

Hello Santhosh,

thanx a lot for your quick reply!

The flow field I provide for applying scalarTransportFoam on is the result of a thermal simulation where the variable T ist already used for the Temperature. Even if scalarTransportFoam only needes the p and U filed and in that simulation the variable T can be regarded as a free one, later, in the postprocessing, I'd like to distinct the T for temperature and T for smoke. Obviously it is possible to rename the scalarFiled T generated by scalarTransportFoam - in my case into "smoke". But it would be far more elegant to rename the variable directly within the solver.

Do you think it is a big deal to do that?

Best regards
Tony

[santoo_cfd]

It is very simple...To have more Idea go through following link...
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

If you dont have patience, just copy scalarTransportFoam to your directory and rename variable T to whatever you want, change the name of solver in Make directory of your choice and create a new solver.

I suggest you to spend little more time in learning basic stuff in OpenFOAM, you will find your life easier in your further work.

Santhosh.

[alfa_8C]

Hello Santhosh,

changing the variable Name within scalarTransportFoam worked without any problems.

Now I am following your suggestion, to implement turbulence in my new, from scalarTransportFoam derived solver. I'm trying to do so following the posts of the present thread. But I'm struggling with compiling.

This is how the changes in my .C file from the Make directory looks like (changed strings in red):

for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++)
{
solve
(
fvm::ddt(Smoke)
+ fvm::div(phi, Smoke)
- fvm::laplacian(turbulence->mut() + DSmoke, Smoke)
);

I didn't change anything else - most probably I have to, but I don't know where and what.

The error message I receive is the following:
smokeTurbulentTransportFoam.C:65: error: ‘turbulence’ was not declared in this scope

Any idea how to solve this?

Tony

[chegdan]

The error message I receive is the following:
smokeTurbulentTransportFoam.C:65: error: ‘turbulence’ was not declared in this scope

This error message is because your turbulence model was not defined in your solver. This will take some additional steps, so you should look a the simpleFoam solver and see how they have added a RAS turbulence model to the solver. This means that you will have to also have additional dict files with the RAS model you want and some constants in your caseName/constant folder. Again, have a look at the simpleFoam tutorials to see how those look.

[shyam]

Hi Santhoosh,
Any logic behind increasing the diffusivity from 1e-6 (fluent) to 100 (openfoam).

[alberto]

Originally Posted by shyam

Hi Santhoosh,
Any logic behind increasing the diffusivity from 1e-6 (fluent) to 100 (openfoam).

Do you notice this in your results? One of the most common mistakes is not considering the proper term in the equation. In other words the turbulent diffusivity you have to consider is nut/Sc, being Sc the turbulent Schmidt number.

[shyam]

Do you notice this in your results? One of the most common mistakes is not considering the proper term in the equation. In other words the turbulent diffusivity you have to consider is nut/Sc, being Sc the turbulent Schmidt number.

Alberto,

Evening using nut/Sc as the turbulent diffusivity does not help to reproduce the results I have predicted from fluent. in fact in fluent i have made the Sc value very high 10000000 so as to neglect the turbulent diffusivity. the molecular diffusivity value was set to 10e-12. i am using the same parameters in openfoam but the results are way off. any comments or suggestion?

[santoo_cfd]

Originally Posted by shyam

Hi Santhoosh,
Any logic behind increasing the diffusivity from 1e-6 (fluent) to 100 (openfoam).

There is no logic in doing this and it is wrong to do it. Please don't do it as it is not the reason for wrong results in OpenFOAM.

Results between OpenFOAM and Fluent were not matching because of human error of not scaling down the mesh converted to OpenFOAM.

scalarTransportFoam in OpenFOAM works pretty fine as it is. As I have mentioned earlier, turbulence effect can be included by adding turbulent diffusivity.

Sorry for the confusion, if any, in above posts.

[jeicek]

Originally Posted by santoo_cfd

Hi Alberto,

Thanks for the information, Actually I was busy with other work thus late in reply.

Now, I have done another simulation run as per your suggestion. I changed the createFields in scalarTransportFoam to read nut values directly. I have added this to Diffusivity values. i.e, laplacian(DT+nut, phi).
(Here, nut is read from 0 directory which I got from steady state run using simpleFoam)

The problem is still I am unable to get the results as that of fluent.

Regards
Santhosh.

Hi guys,

Santoo I do the same case. can u plz explaine how should I do these modificarions? I mean shall I creat new solver or change the source code? I m not good in c++

thanks in advanced

[chegdan]

Greetings! Have you read this thread fully and noticed the post

http://www.cfd-online.com/Forums/ope...tml#post280210

that outlined the equation to be used? The c++ is actually not too painful and if you aren't good its really a great place to start. I would look at the equation from that particular post; decide what information you need i.e. velocity, turbulence schmidt number, nut; take a look at other solvers like solvers/basic/scalarTransportFoam or even icoFoam for inspiration; write your solver and then compile. If you are having issues compiling things then I would take the time to start with learning how to compile OpenFOAM on your own. These days it has become easier and easier to compile using instructions like these or these, depending on if you are using standard or foam extend. Good luck!

[jeicek]

Originally Posted by santoo_cfd

Hi

I want to get the RTD (Residence time distribution) of for steel industry application. The procedure I followed is as follows,
Methodology:
1. Steady state - I ran simpleFoam to get the initial velocity Field. I ensured 5 orders of residue fall
2. Tracer Injection - I used to velocity field from the simpleFoam and used scalarTransportFoam for passsive scalar injection. ( Traced inlet boundary set to 1 for 0.129 sec)
3. RTD study - I monitored the tracer concentration at the outlet for 1000 secs using scalarTransportFoam.

Problems

1. RTD curve is not matching either with fluent or experiment.
2. I have some confusion regarding the use of slip boundary condition in OpenFOAM. Is it similar the boundary we set in Fluent ( I mean we set shear stess =0 for wall with slip).
3. Is it right to use scalarTransportFoam or should I need scalarTranportFoam with turbulence added to it? ( As flow regime is turbulent, I used k-epsilon in simpleFoam)

Any kind of suggestion u think of, I am ready to try and post back.

Thanks
Santhosh

Hi dude,
Can u help me? how should I monitor the concentration at the outle in order to plot the RTD?

[chegdan]

For monitoring at the outlet, you probably want mixing-cup average. I generally use the tool

simpleFunctionObjects

which is part of

swak4Foam


and use the patchMassFlowAveraged function for mixing-cup average. Again, you will need to be able to compile this tool.

[jeicek]

Originally Posted by chegdan

For monitoring at the outlet, you probably want mixing-cup average. I generally use the tool

simpleFunctionObjects

which is part of

swak4Foam


and use the patchMassFlowAveraged function for mixing-cup average. Again, you will need to be able to compile this tool.

Daniel thank you very much for fast reply. I went through the Contrib/swak4Foam wiki page:
http://openfoamwiki.net/index.php/Contrib/swak4Foam

So as far I understood in order to use functionobject ( in our case PatchMassFlowAveraged) we need to install (compile) the swak4Foam. But I typed the command wmake all but it has taken very long about 17 hours and still compiling (and my space is about 28 GB)?!! Shall I wait still?? everything is correct??
Thanks in advance

[chegdan]

@jeicek

Cancel the compilation, it should not take that long. A few questions for you:

• What operating system are you using?
• Is there a log file associate with your compilation and are there any errors?
• what version of OpenFOAM are you using?
• have you compiled OpenFOAM before i.e. do you have all the necessary external libraries to compile OpenFOAM code?
• can you compile a simple solver like this one here?

It may be best to find threads related to swak4Foam compilation and post there, or start an entirely new thread about your overall goal (in the programming and development sub-forum?). When that happens, post a link here leading others their that may need similar help (a link not asking for help, but informing others that there is a new thread and what the topic is) and I will follow that and answer questions over there. Try to formulate a good post so others will join according to http://www.cfd-online.com/Forums/ope...-get-help.html .I will see you there at your new post

[jeicek]

Originally Posted by chegdan

@jeicek

Cancel the compilation, it should not take that long. A few questions for you:

• What operating system are you using?
• Is there a log file associate with your compilation and are there any errors?
• what version of OpenFOAM are you using?
• have you compiled OpenFOAM before i.e. do you have all the necessary external libraries to compile OpenFOAM code?
• can you compile a simple solver like this one here?

It may be best to find threads related to swak4Foam compilation and post there, or start an entirely new thread about your overall goal (in the programming and development sub-forum?). When that happens, post a link here leading others their that may need similar help (a link not asking for help, but informing others that there is a new thread and what the topic is) and I will follow that and answer questions over there. Try to formulate a good post so others will join according to http://www.cfd-online.com/Forums/ope...-get-help.html .I will see you there at your new post

Thank you very much again Daniel it was fixed.

[mwmalkawi]

RTD with DT of 100 so did it work fo rth eother modles in seeting diffusion to 100?

Originally Posted by santoo_cfd

Hi,

I revisited the case and think that I have solved the problem. The trick (ofcourse not) is that I have increased the Diffusivity value to 100 and I got similar RTD pattern I obtained with Fluent with corresponding diffusivity of 1e-6.

Apart, The steady state velocity profile I got with simpleFoam are in excellent agreement with Fluent and experimental observation.

So, I thought the normalization of Diffusity values the solver does is different in OpenFOAM and Fluent.

Anyway Now I will do some other parameter study in openFOAM to get more insight.

Thanks to Dr.Eelco from TATA Corus in helping me to get confidence in this exercise.

Thanks all the contributors to this thread.

I will post back with other results soon.


Santhosh..

RTD with DT of 100 so did it work fo rth eother modles in seeting diffusion to 100

[amuzeshi]

Originally Posted by mwmalkawi

RTD with DT of 100 so did it work fo rth eother modles in seeting diffusion to 100?

You have alittle typo;
"with DT of 100 so did it work for the other modles..." rather than "with DT of 100 so did it work fo rth eother modles".

I also don't understand what do you mean by "seeting diffusion to 100"

[otaolafr]

hello everybody,
I have a doubt with the usage of the scalarTransportFoam to calculate the RTD,
as i have read several threads, there is a lot of people using it for this, with the need of modification in case that our case that the flow is turbulent. my doubt is in respect to the dimensions of T and D. normally D it should m2/s and T it is a concentration normalized, so it should be adimensional, but in the T file it has unit (K). shouldn't this disrupt the units of the equation?

thanks in advance,
franco

[amuzeshi]

Originally Posted by otaolafr

hello everybody,
I have a doubt with the usage of the scalarTransportFoam to calculate the RTD,
as i have read several threads, there is a lot of people using it for this, with the need of modification in case that our case that the flow is turbulent. my doubt is in respect to the dimensions of T and D. normally D it should m2/s and T it is a concentration normalized, so it should be adimensional, but in the T file it has unit (K). shouldn't this disrupt the units of the equation?

thanks in advance,
franco

Hello,
"Disruption" occurs when the dimensions of the terms (convection, diffusion, ...) are inconsistent. Setting an arbitrary unit for field T causes no inconsistency.

[Lucky]

Originally Posted by santoo_cfd

Hi Alberto,

Thanks for the information, Actually I was busy with other work thus late in reply.

Now, I have done another simulation run as per your suggestion. I changed the createFields in scalarTransportFoam to read nut values directly. I have added this to Diffusivity values. i.e, laplacian(DT+nut, phi).
(Here, nut is read from 0 directory which I got from steady state run using simpleFoam)

The problem is still I am unable to get the results as that of fluent.

Regards
Santhosh.

I know it has been about a decade since you posted this but i have tried what you are suggesting and i keep getting funny errors here are the edits i did.


i added this chunk in the createFields.H in scalarTransportFoam:


Info<< "Reading field nut\n" << endl;

volScalarField nut
(
IOobject
(
"nut",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);


In the fvShemes i did this'


laplacianSchemes
{
default none;
//laplacian(DT,T) Gauss linear corrected;
laplacian(DT+nut,phi) Gauss linear corrected;
}



i am getting the following error:
[1]
[1]
[1] --> FOAM FATAL IO ERROR: (openfoam-2106)
[1] Entry 'laplacian(DT,T)' not found in dictionary "stream.laplacianSchemes"
[1]
[1]
[1] file: stream.laplacianSchemes at line 0.
[1]
[1] From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType:ption) const
[1] in file db/dictionary/dictionary.C at line 413.
[1]
FOAM parallel run exiting
[1]
[0]
[0]
[0] --> FOAM FATAL IO ERROR: (openfoam-2106)
[0] Entry 'laplacian(DT,T)' not found in dictionary "/home/lka62/Documents/oF2106/1000/10/scalarT/system/fvSchemes.laplacianSchemes"
[0]
[0]
[0] file: /home/lka62/Documents/oF2106/1000/10/scalarT/system/fvSchemes.laplacianSchemes at line 35 to 37.
[0]
[0] From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType:ption) const
[0] in file db/dictionary/dictionary.C at line 413.
[0]
FOAM parallel run exiting
[0]
[2]
[2]
[2] --> FOAM FATAL IO ERROR: (openfoam-2106)
[2] Entry 'laplacian(DT,T)' not found in dictionary "stream.laplacianSchemes"
[2]
[2]
[2] file: stream.laplacianSchemes at line 0.
[2]
[2] From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType:ption) const
[2] in file db/dictionary/dictionary.C at line 413.
[2]
FOAM parallel run exiting





what am i doing wrong, its a simulation of flow in porous media and i am using the results from simpleFoam.