# Solving transport equations with known velocity field

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 August 6, 2012, 05:20 Solving transport equations with known velocity field #1 Senior Member     Mojtaba Amiraslanpour Join Date: Jun 2011 Location: Zanjan, Iran Posts: 287 Rep Power: 8 Hi. 1) I want to solve 2 transport equations with known velocity field. First i want to solve coupled equations of momentum, energy and mass conservation to compute velocity field and pressure and also temperature. after solving these equations and by known velocity field i want to solve 2 other transport equations. How can i do that in openFoam? 2) my second question is that is there anyway to include heat transfer coefficient in openfoam? or it will be computed automatically? if yes, then how can I find it? 3) I am modeling a room with heat sources which both natural convection and forced convection are significant. my case is incompressible. which solver do u suggest to use and how can i see the effects of forced convection? Regards Mojtaba ~

August 6, 2012, 05:49
#2
Senior Member

Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 584
Rep Power: 20
Quote:
 Originally Posted by Mojtaba.a Hi. 1) I want to solve 2 transport equations with known velocity field. First i want to solve coupled equations of momentum, energy and mass conservation to compute velocity field and pressure and also temperature. after solving these equations and by known velocity field i want to solve 2 other transport equations. How can i do that in openFoam? 2) my second question is that is there anyway to include heat transfer coefficient in openfoam? or it will be computed automatically? if yes, then how can I find it? 3) I am modeling a room with heat sources which both natural convection and forced convection are significant. my case is incompressible. which solver do u suggest to use and how can i see the effects of forced convection? Regards Mojtaba ~
1. Yes, have a look at (http://openfoamwiki.net/index.php/ScalarTransportFoam).

2. Not sure

3. buoyantBoussinesqSimplFoam?

Give the forum a good search for passive scalar transport, natural convection, buoyancy,.... This will answer all of your questions. Hopefully this will get you started.
__________________
Dan

Find me on twitter @dancombest and LinkedIn

August 6, 2012, 06:08
#3
Senior Member

Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 287
Rep Power: 8
Quote:
 Originally Posted by chegdan 1. Yes, have a look at (http://openfoamwiki.net/index.php/ScalarTransportFoam). 2. Not sure 3. buoyantBoussinesqSimplFoam? Give the forum a good search for passive scalar transport, natural convection, buoyancy,.... This will answer all of your questions. Hopefully this will get you started.
Thank you for your quick answer chegdan.
1) well i have already seen that tutorials. i want to know how can i solve transport equation after finishing solving for U,p and T. is it possible?

regards

Last edited by Mojtaba.a; August 6, 2012 at 06:38.

 August 6, 2012, 06:27 #4 Senior Member     Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 584 Rep Power: 20 Yes, its possible. You will need to add your volScalarField for your scalar, formulate the implicit equation and then solve it as usual. If it is strongly coupled with the momentum equation (active) you can solve it inside the PISO/SIMPLE loop and if its a passive scalar (one-way coupled) you can solve it at the end of the time-step. Mojtaba.a likes this. __________________ Dan Find me on twitter @dancombest and LinkedIn

August 6, 2012, 06:42
#5
Senior Member

Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 287
Rep Power: 8
Quote:
 Originally Posted by chegdan Yes, its possible. You will need to add your volScalarField for your scalar, formulate the implicit equation and then solve it as usual. If it is strongly coupled with the momentum equation (active) you can solve it inside the PISO/SIMPLE loop and if its a passive scalar (one-way coupled) you can solve it at the end of the time-step.
Here is the source code for buoyantBoussinesqSimpleFoam:

Quote:
 while (simple.loop()) { Info<< "Time = " << runTime.timeName() << nl << endl; p_rgh.storePrevIter(); // Pressure-velocity SIMPLE corrector { #include "UEqn.H" #include "TEqn.H" #include "pEqn.H" } turbulence->correct(); runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; }
By "end of the time step" you mean where?

August 6, 2012, 07:24
#6
Senior Member

Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 584
Rep Power: 20
Quote:
 Originally Posted by Mojtaba.a By "end of the time step" you mean where?
Code:
```while (simple.loop())
{
Info<< "Time = " << runTime.timeName() << nl << endl;

p_rgh.storePrevIter();

// Pressure-velocity SIMPLE corrector
{
#include "UEqn.H"
#include "TEqn.H"
//<--here for active scalar
#include "pEqn.H"
}

turbulence->correct();
//<-- here for passive scalar that depends on turbulence

runTime.write();

Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
<< " ClockTime = " << runTime.elapsedClockTime() << " s"
<< nl << endl;
}```
You could try it in several places, compare execution time and solution and see which one is best. Good luck
__________________
Dan

Find me on twitter @dancombest and LinkedIn

August 6, 2012, 07:43
#7
Senior Member

Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 287
Rep Power: 8
Quote:
 Originally Posted by chegdan Code: ```while (simple.loop()) { Info<< "Time = " << runTime.timeName() << nl << endl; p_rgh.storePrevIter(); // Pressure-velocity SIMPLE corrector { #include "UEqn.H" #include "TEqn.H" //<--here for active scalar #include "pEqn.H" } turbulence->correct(); //<-- here for passive scalar that depends on turbulence runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; }``` You could try it in several places, compare execution time and solution and see which one is best. Good luck
I understand it now,
Thanks chegdan ~

 Tags heat transsfer, hvac, room, transport equation

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post CKH OpenFOAM Running, Solving & CFD 12 March 21, 2016 14:05 Unseen OpenFOAM Running, Solving & CFD 7 April 16, 2014 03:38 Artex85 OpenFOAM Running, Solving & CFD 9 January 3, 2012 09:06 renyun0511 OpenFOAM Running, Solving & CFD 0 November 19, 2009 03:11 barath.ezhilan OpenFOAM 13 July 16, 2009 05:55

All times are GMT -4. The time now is 23:05.

 Contact Us - CFD Online - Top