ScalarTransportFoam for RTD calculations
 

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

scalarTransportFoam could work in your case, as the scalar is purely passive. But you need to modify scalarTransportFoam to use the turbulent diffusivity (alphaEff) from the turbulence model to do that, as your flow is turbulent.

hi Flavio

Thanks for the information, My mentor was also explaining the same.

I think this can be done by changing the laplacian term in the scalarTransportFoam solver from as follows

fvm::laplacian(DT, T) to fvm::laplacian(turbulence->alphaEff(), T)

I will do the necessary change the post the result if I am successful.

If anybody has any other suggestion please post.

Thanks
santhosh

little update
 

As above suggested I have changed the scalarTransportFoam as follows

laplacian(DT, T) is replaced by laplacian(turbulence->nut() + DT, T) ( simply I took help from simpleFoam solver for other stuff in createFields etc..)

Where in transport propertied I have provided with Viscosity for DT entry.
I have not seen any further improvement. I am looking for other possibilities to improve the solution.

Will post back if I get any good results.

Thanks for help
Santhosh.

valildation paper
 

Following is the link for the Article which I am trying to validate. You can freely download from the site. Intersted people may try it.
http://www.journalarchive.jst.go.jp/...startpage=1228

Thanks
Santhosh

Fluent comparision
 

Hi,

I have tested scalarTransportFoam in openFOAM with UDS approach in fluent.
The results are completely different.

I have converted the OpenFOAM developed velocity profile (using foamDataToFluent), and used UDS in fluent to get the RTD curve

I am attaching the results of results. (fluent developed scalar contour with RTD curve, OF developed scalar countour along the RTD cure)

Hi Santhosh,

have you compared the velocity and turbulence (k and epsilon) profiles you got with Fluent and OpenFoam? It appears that you have different solutions there.

Hi,

Actually I have taken the steady state solution from openFOAM only.
I have converted the openFOAM flow fields to Fluent and did transient study for RTD comparison. So there is no confusion regarding initial velocity fields. (In this comparison exercise I am not taking turbulent diffusion into consideration)

What I shown in the figures are Scalar field contour at the end of the transient run and corresponding RTD curves in both fluent and OpenFOAM.

To my knowledge scalarTransport equation is so plain and simple and OpenFOAM implementation is robust even for very complex non linear terms.
What puzzling me is that huge difference in results of fluent and openFOAM for simple Scalar transport equation solver.

If anybody used scalarTransportFoam for RTD calculation help me. I also thinking of using Lagrangian approach for it ,but I am not clear how to proceed in that direction.

Thanks
Santhosh

Hi Santhosh,

Your approach seems to be correct, I have now no idea what is going wrong.

My only comment is that, if you are using nut() in the scalar equation, the turbulent diffusion effects are being taken into account.

Thanks flavio for your help. I will try other option and will post back once I validated the results.

--Santhosh

Hi,

I don't understand what you did actually. Did you add a scalar transport equation to simpleFoam, or do you get a steady solution from simpleFoam and then run scalarTransportFoam on it?
If you do the latter, it is not correct to use turbulence->nut(), and the procedure is a lot simpler, since it is enough to read in scalarTransportFoam the field of the turbulent viscosity associated with the velocity field already provided as input, and use the appropriate effective diffusivity.

Best,
Alberto

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,

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..

Dear Santhosh,

I had a look to your thread just now, maybe I am too late to help. Actually, it is difficult to say why your solutions are so different. But for me they appears too different to be the solution of the same problem. Just to suggest a possible cause, have you double checked that domain dimensions are the same ? How did you built the mesh ?
At the beginning of the blockMeshDict, a line allows to control the scale factor. To write coordinates in mm and properly scale the mesh to meters:
convertToMeters 1e-03;
A look to the velocity fields and magnitude could help to understand if a wrong mesh scaling is occurring.

My best regards,

Franco

Hi Franko,

Thanks for the reply. Your suggestion very important that people usually forget to scale. In my case I have created mesh from third party software and properly scaled down after import.

Anyways to avoid any ambiguity in comparision I have exported the steady state results of OpenFOAM to Fluent and did scalarTransport steady in fluend as I discussed in Thread-6 of this post. you can see the results also there.

Now I am doing fresh run of complete case again with another standard benchmark problem. Now I got enough expertize that I can do this very easily.
I will post back with results soon. (This new one also eliminate if any simple mistakes I have done previously)

Regards
Santhosh.

RANS and Scalar Mixing
 

Hello Fellow Foamers,

I'm doing some RTD calculations an a fairly complicated geometry that I have a steady state flow field determined from simpleFoam. Now I am performing RTD calculations with a step input of tracer into the domain. That is the ultimate goal, however on some simple cases I'm having some issues. First of all I have my solver, which is a scalarTransportFoam derived solver to include a turbulent mass diffusivity.

solve
(
fvm::ddt(C)
+ fvm::div(phi, C)
- fvm::laplacian(D, C)
- fvm::laplacian(Dturbulent, C)
);

where Dturbulent is related to the nut field through an assumed value of turbulent Schmidt number (suggested in both Fluent and a book by Fox "computational models for turbulent reacting flows").

My problem is that the scalar is unbound even if I use the bounded schemes in fvSchemes (see attached). I see values higher than 1 (injection C = 1). I have altered the Peclet number utility to use Deff=D+Dturbulent and there are some values that are still >>2 (suggested value from Ferziger and Peric "Computational Methods for Fluid Dynamics" in eqn 6.33). I understand that the Pe rule was for a different scheme.

My questions are:
1) is this a problem with my schemes?
2) is there some other addition to the model I need (i.e. include ensemble averaging...if its not already in the solver)?
3) refine my mesh to be more Peclet Number friendly? if so how can I refine only the cells that have a terrible peclet number?

I have included a link (http://students.cec.wustl.edu/~dc3/) to the solver, test case, and sample utility that one would need to do exactly what I am doing. I am using OpenFOAM-1.5-dev on Ubuntu 9.10 amd64. Waiting for a reply and thanks in advance.


Dan

Correct me if I'm wrong
 

Just following up a little bit on my previous post, however I'm still not clear on why this works.

was unbounded even with the bounded schemes. However, when I added another term to the equation:

it was bounded just fine. I found this by looking at the SpalartAllmaras.C file and from this post (http://www.cfd-online.com/Forums/ope...silon-eqn.html).

The explanation was not that clear to me, but I will try and look at it some more today and make some sense of it. if anyone can explain (or clarifiy the post where it came from) I would greatly appreciate it.

Dan

Now I understand
 

Like Jasak said in the post (http://www.cfd-online.com/Forums/ope...silon-eqn.html) the

For continuity to be satisfied div(U) = 0 and we assume is zero. However, for incomplete convergence (see cited post above)...this term is not zero. Therefore we need to move C(div(U)) to account for incomplete convergence that would otherwise be zero.

A very loose explanation, but it worked and has a physical/numerical significance.

Hello Foamers,

I found this Thread which is closely related to my current problem and it encouraged me to ask some questions-

I'd like to simulate smoke propagation. The smoke can be treated as massless. The idea is to first generate a flow field for every timestep with all the necessary phyics, and then to apply scalarTransportFoam after every timestep, where the smoke is representing my scalar.

As I have no programming experience jet regarding openFoam solvers - how can I adopt the current "scalarTransportFoam" with "T" as scalar to i.e
"smokeTransportFoam" with "smoke" as scalar.

Any hints?

Thanks a lot in advance,
Tony

You need not to create any separate solver, just existing scalarTransportFoam with T as your smoke. Just you need to give the proper diffusivity value. In case your case involves turbulence, you need to change the solver in order to account for turbulence diffusivity. Check the above posts do it.

Sorry for late update, I got excellent results with scalarTransportFoam for RTD calculations very closely matching with experiment.

Regards,
Santhosh

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

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.

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

turbulence model needs to be included
 

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.

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.

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?

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.

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

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!

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

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

@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 :D

Thank you very much again Daniel it was fixed.

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

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


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"

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.

hie Santoo
 

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::option) 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::option) 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::option) 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.