|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Abhinav Sharma
Join Date: Sep 2010
Posts: 28
Rep Power: 15 ![]() |
Hello Foamers,
I've set up my flow field model using both LES and RAS ( run with pisoFoam) for a urban street canyon, and would like to introduce scaler transport model to simulate pollutant dispersion. I understand that ScalarTransportFoam can be used here, however i will need to modify the code to introduce a source term (i've been following this tutorial) I'm not quite clear as to how to go about the entire process, ie to link the modified code after introducing the changes , to my wind field output data(output of pisoFoam run). I'm not very thorough with C ++ hoping to get familiarized with it as soon as possible! Thank you in advance! Regards, Abhinav Last edited by asharma; January 3, 2011 at 06:01. |
|
![]() |
![]() |
![]() |
![]() |
#2 |
New Member
Abhinav Sharma
Join Date: Sep 2010
Posts: 28
Rep Power: 15 ![]() |
I've been trying to implement a source term to scalerTransportForm coupling it to my pisoFoam solver and have attempted to include a source term as mentioned in the tutorial(mentioned above) as follows where my T is my scaler field and my source "source":-
Code:
solve ( fvm::ddt(T) + fvm::div(phi, T) - fvm::laplacian(DT, T) == source ); Code:
for (int corr=0; corr<nCorr; corr++) { #include "TEqn.H" Code:
Info<< "Reading field T\n" << endl; volScalarField T ( IOobject ( "T", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); Info<< " Reading source" << endl; volScalarField source ( IOobject ( "source", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::NO_WRITE ), mesh ); Regards, Abhinav |
|
![]() |
![]() |
![]() |
![]() |
#3 |
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 24 ![]() |
Abhinav, the kind of source you're using is passive, i.e. it doesn't depend on the values of T. Nevertheless this doesn't imply that this source have to be spatially constant. In the way you're defined it, it can be a completely spatially variable source. Other way is to define the source value in the transportProperties dictionary and then use:
Code:
solve ( fvm::ddt(T) + fvm::div(phi, T) - fvm::laplacian(DT, T) == sourceValue ); Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar |
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Abhinav Sharma
Join Date: Sep 2010
Posts: 28
Rep Power: 15 ![]() |
Thank you Santiago!
Yes i understand i'm using a passive source here, which is exactly what i want. However i'm getting a little confused on how to specify my source to a specific region in my geometry where i want my scaler T to get generated and subsequently dispersed with the prevailing wind flow regime. Is there a way to do that? Pardon me if my question seems silly! Thanks, Regards, Abhinav |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 24 ![]() |
Abhinav, your question is how to set the values of the source across the domain? If it's the case you have swak4Foam (http://openfoamwiki.net/index.php/Contrib/swak4Foam) to do so.
Regards
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar |
|
![]() |
![]() |
![]() |
![]() |
#6 | |
Member
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17 ![]() |
Quote:
and set the values at the appropriate regions of the mesh using setFields or funkySetFields, or, in especially customized cases, assign the values straight in the code, e.g. point by point, like this: Code:
source[mesh.findCell (point (x,y,z))] = value_at_xyz; |
||
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
Abhinav Sharma
Join Date: Sep 2010
Posts: 28
Rep Power: 15 ![]() |
Hi Robertas and Santiago,
Thanks for the help! I'm pretty sure as to how to go about it now... Regards, Abhinav |
|
![]() |
![]() |
![]() |
![]() |
#8 |
New Member
Abhinav Sharma
Join Date: Sep 2010
Posts: 28
Rep Power: 15 ![]() |
Robertas , if i were to assign values straight in the code like you've mentioned, where(which file) am i suppose to add the code to?
|
|
![]() |
![]() |
![]() |
![]() |
#9 | |
Member
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17 ![]() |
Quote:
overall structure of the solver is like this: Code:
// Initialization goes here; // main loop: while ( runTime.run() ) { // solution steps for equations (depend on the particular solver): #include "UEqn.H" ... // other equations, as/if needed // output data and such... } // wrap up the values should be assigned inside the main loop; but then you'll probably want to define a separate function for calculating the field values, and this function can be located in a separate file, like Code:
// in the file "updateSource.h" void updateSource (volScalarField& Q); Code:
// in the file "updateSource.cpp" void updateSource (volScalarField& Q) { // the required assignments go here } Code:
#include "updateSource.h" // Initialization goes here; // main loop: while ( runTime.run() ) { // update source fields updateSource (Q); // solution steps for equations (depend on the particular solver): #include "UEqn.H" ... // other equations, as/if needed // output data and such... } // wrap up |
||
![]() |
![]() |
![]() |
![]() |
#10 | |
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 0 ![]() ![]() |
Quote:
http://www.cfd-online.com/Forums/ope...culations.html I had a similar question a while back and I give a snippet of code that has worked very well. If the code on that thread is used, then the difficult part is to estimate the turbulent mass diffusivity of the pollutant. Usually this is estimated with a constant global turbulent schmidt number (turbulent viscosity/ turbulent mass diffusivity) equal to 0.7 (from fluent documentation). There are some other nuances of that are covered in posts 17 and 18 in the provided link. Basically the gradient diffusion hypothesis is used to approximate the scalar-flux <u'\phi'> term produced during reynolds averaging. For an LES approach, the methods are a little different that could employ a subgrid scalar flux relationship. I hope this helps. Dan |
||
![]() |
![]() |
![]() |
![]() |
#11 |
New Member
Abhinav Sharma
Join Date: Sep 2010
Posts: 28
Rep Power: 15 ![]() |
Thank you Robertas and Dan,
I apologies for the late reply as i was busy with some related but different work. Yes i see the importance of modeling scaler transport in a turbulent field to be addressed here, it was also pointed out by my mentor. I've used funkysetfields to define specific patches where i would like to introduce my scaler (i found it more convenient then manually entering the points), moreover i believe usage of a source term is not apt for my particular application(?). Actually i require a constant source of scaler to be introduced in my domain at a specified location, corresponding to emissions from vehicles passing through my street canyon. Would it be reasonable to assume a constant scaler concentration at points where i have assumed vehicle to pass, and allow scaler transport foam to calculate the dispersion with the turbulent diffusivity (by adding nut term to DT) accounted for?... |
|
![]() |
![]() |
![]() |
![]() |
#12 | |
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 0 ![]() ![]() |
Quote:
Dan |
||
![]() |
![]() |
![]() |
![]() |
#13 |
Member
Chris Harding
Join Date: Dec 2016
Posts: 76
Rep Power: 9 ![]() |
Hello,
The link to the tutorial is: http://cfd.at/downloads/FoamTutV4_10-ExampleTen.pdf I am confused about the sudden need for a T-file in section 3.2.0. I found a T file, but now errors told me that I need DT in transport properties and I don't know how to do that. IN fact, I am new and have never used the T-file or DT specification. If the above link does not work, try: https://wiki.openfoam.com/T-junction...and_colleagues and download PDF. Can someone help walk me through the addition of a T-File, etc. Remember, I am new and why I am taking these tutorials. |
|
![]() |
![]() |
![]() |
![]() |
#14 |
Member
Chris Harding
Join Date: Dec 2016
Posts: 76
Rep Power: 9 ![]() |
Hello,
I got the scalarTransportFoam to run, but it only ran when I disabled "streamlines" and altered fvSchemes and fvSolution with example data from "Basic" pitzdaily. My results look the same as the tutorial results, but there doesn't seem to be any calculation going on in my case. It appears that it immediately jumps to the correct result at 1st calculation. Maybe it is because diffusion is set at 0.01. (I just changed the diffusion to 1e-04 and it still jumped within 10 seconds to an analysis that stayed the same the whole time). I need to get this correct. I would like to use "streamlines" so that I can use vtk. I want to do a Residence Time Distribution analysis. |
|
![]() |
![]() |
![]() |
![]() |
#15 | ||
Senior Member
Robert
Join Date: May 2015
Location: Bremen, GER
Posts: 292
Rep Power: 12 ![]() |
Hello Chris,
since you got your solver to work, i suppose that you understood the the T-file is the transported species of your simulation. Like any other variable (p,U,nut,...) it needs its own file in your 0-folder. Dt is the diffusion coefficient. The parameter determines how diffusive your transport species behaves (also see Peclet number). Quote:
Read up about the Peclet number and about what advective and diffusive transport are. To get a more advective transport, try further reducing the diffusion coefficient. Don't set it to 0. This works in OpenFoam but the results are not comparable. You need a diffusion coefficient to get meaningful results. Quote:
__________________
If you liked my answer to your question, please consider leaving a "Like" in return ![]() |
|||
![]() |
![]() |
![]() |
![]() |
#16 | |
Member
Chris Harding
Join Date: Dec 2016
Posts: 76
Rep Power: 9 ![]() |
Quote:
Apparently, the solver for diffusion were happy with this velocity data because it converged immediately. |
||
![]() |
![]() |
![]() |
![]() |
#17 |
Member
Rosario Arnau
Join Date: Feb 2017
Location: Spain
Posts: 57
Rep Power: 9 ![]() |
Hi foamers,
I know this is an old post but I have a question about scalars/concentration at scalarTransportFoam solver. I'have seen that there are some experts at this threat so hope one of you can help me: In my case I have two inlets (Inlet 1 and RecirculationInt) and two outlets (Outlet and RecirculationOutlet). The flow enters the domain by the Inlet and exits through Outlet but, the flow that enters through Inlet and RecirculationInlet exits the domain through RecirculationOutlet so that the flows going in and out are: Inlet Flow= Q1 +Q2 RecirculationInlet= Q3 Outlet= -Q1 RecirculationOutlet= -(Q2+Q3) Now I need to introduce an scalar so that the concentration that goes out through RecirculationOutlet need to enter again in the domain in order to avoid lossing my scalar concentration. I'm able to calculate the surface concentration of the patch throughout: Code:
{ Recirc_T { type surfaceFieldValue; operation areaIntegrate; libs ("libfieldFunctionObjects.so"); writeArea yes; regionType patch; surfaceFormat foam; name RecirculationOutlet; enabled true; writeControl writeTime; //writeControl timeStep; //Output every timestep //writeInterval 1; //Cada timestep, guarda valor valueOutput true; log false; writeFields no; fields ( T) } Thanks! Last edited by rarnaunot; August 21, 2020 at 10:41. Reason: typo |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
ScalarTransportFoam for RTD calculations | santoo_cfd | OpenFOAM Running, Solving & CFD | 39 | July 12, 2021 01:15 |
Problem with scalarTransportFoam illistrated using pitzDaily tutorial | mlawson | OpenFOAM | 2 | January 18, 2011 13:39 |
High number of iterations (scalarTransportFoam) | Frithjof | OpenFOAM Running, Solving & CFD | 0 | December 8, 2010 04:44 |
Modified scalarTransportFoam, but result is not right , need help | panda60 | OpenFOAM | 2 | December 2, 2009 19:50 |
flux seems not conserved in my modified scalarTransportFoam | danielr | OpenFOAM Running, Solving & CFD | 3 | October 5, 2009 16:05 |