starting off with OpenFOAM

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 7, 2011, 07:31 starting off with OpenFOAM #1 New Member   Sibusiso Mavuso Join Date: Jul 2010 Location: South Africa/Pretoria Posts: 21 Rep Power: 9 HI GUYS I am a new user of OpenFOAM and would like to solve an unsteady energy equation for a compressible gas through a porous media. I have basic knowledge of C++ prograqming, please help. thanx in advance

 February 8, 2011, 03:24 #2 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 10 Hi semaviso, have a look into the rhoReactingFoam application to see how its done there. This is the general way to go. Look whether theres something you need. Best Kathrin

 February 16, 2011, 09:21 #3 New Member   Sibusiso Mavuso Join Date: Jul 2010 Location: South Africa/Pretoria Posts: 21 Rep Power: 9 thanx Kathrin I checked it out and now I want to understand the meaning of: 00008 volScalarField rUA = 1.0/UEqn.A(); 00009 U = rUA*UEqn.H(); from rhoReactingFoam/pEqn.H How can I write Darcy's formula (U_gas = (-permK/mu)*grad(p) ) U_gas being the gas flux or velocity in m/s in OpenFOAM to use with the mass transport equation. thanx again for your help.

 February 16, 2011, 10:48 #4 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 10 1. Question This is part of the pressure velocity coupling see: http://powerlab.fsb.hr/ped/kturbo/Op...jeJasakPhD.pdf for details. What is done: UEqn.A() gives you the central coefficient of the the fvMatrix (fv=finiteVolume) UEqn. UEqn.H() gives you the H operator which is basically H(UEqn)=source(UEqn)-diagonal(UEqn)U in that way the velocity is evaluated by U = rUA*UEqn.H(); ok? 2. Question I'm not really sure what your trying to do. Can you specify a little? Do you want to use your U_gas in the continuity equation? Why? Best Kathrin

 February 16, 2011, 17:37 #5 Senior Member   Cyprien Join Date: Feb 2010 Location: Stanford University Posts: 262 Rep Power: 11 Hi semaviso! There are several way to solve your problem: - either your add a source term in an existing momentum equation (for example rhoReactingFoam as suggested by Kathrin, or may be rhoPisoFoam will be easier to begin) : Code: ``` fvVectorMatrix UEqn ( fvm::ddt(rho, U) + fvm::div(phi, U) + turbulence->divDevRhoReff(U) == rho*g - fvm::Sp(mu/K,U) );``` or you code your own porous media solver. For a incompressible flow, you have to solve the following diffusion equation on P variable : Code: ```solve ( fvm::laplacian(-K/mu,P) );``` It is not very difficult to adapt this porous solver to compressible flow (Darcy's law replaced within continuity equation). Regards, Cyp Last edited by Cyp; February 17, 2011 at 06:44.

 February 17, 2011, 03:40 #6 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 10 Maybe you want to have a look into rhoPorousFoam. I never worked with it. But it sounds promising. Best Kathrin

 February 22, 2011, 09:21 #7 New Member   Sibusiso Mavuso Join Date: Jul 2010 Location: South Africa/Pretoria Posts: 21 Rep Power: 9 thanx guys it worked. another question is, how do I add a source term to an energy balance equation if the source term is as follows: [deltaH - T(Cp_ss - Cp_s)] deltaH : Heart of reaction Cp_ss : saturated solid (porous media) heat capacity Cp_s : solid (porous media) heat capacity

 February 23, 2011, 03:10 #8 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 10 Which variable are you solving for in your energy equation T or h? Best Kathrin

 February 24, 2011, 04:09 #9 New Member   Sibusiso Mavuso Join Date: Jul 2010 Location: South Africa/Pretoria Posts: 21 Rep Power: 9 Hi Kathrin I want "T" but I had used the energy equation with "h". since h = Cp*T. thanx in advance

 February 25, 2011, 05:07 #10 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 10 could you post the equation you have? Do you reconstruct the Temperature from the energy? Best Kathrin

 February 25, 2011, 05:38 #11 New Member   Sibusiso Mavuso Join Date: Jul 2010 Location: South Africa/Pretoria Posts: 21 Rep Power: 9 the equation is from http://onlinelibrary.wiley.com/doi/10.1002/er.919/pdf equation 1 of this publication. I have decided to use h becouse i found a lot of hEqn.H file that I think have something almost similar to this equation.

 February 25, 2011, 05:47 #12 Senior Member   Cyprien Join Date: Feb 2010 Location: Stanford University Posts: 262 Rep Power: 11 Hi semaviso! You should try something like that: Code: ```fvm::ddt(rho*Cpg,T) +fvm::div(phi,T) -fvm::laplacian(lambda,T) == fvm::Sp(m_dot*(Cpg-Cps),T) -m_dot*dH0``` where the flux phi is defined as: Code: `surfaceScalarField phi = rho*Cpg*linearInterpolate(U)&mesh.Sf();` (if rho or Cpg are volScalarField, you must use: Code: `surfaceScalarField phi = fvc::interpolate(rho)*fvc::interpolate(Cpg)*linearInterpolate(U)&mesh.Sf();` Best Regards, Cyp

 August 2, 2011, 07:50 #13 New Member   Sibusiso Mavuso Join Date: Jul 2010 Location: South Africa/Pretoria Posts: 21 Rep Power: 9 thank you a lot, I have been tryin to modify the porousExplicitSourceReactingParcelFoam to solve for a compressible gas inside a porous reactor. Regards, SBU

 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 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36 wyldckat OpenFOAM Announcements from Other Sources 3 September 8, 2010 06:25 pete Site News & Announcements 0 June 29, 2009 05:56 mbeaudoin OpenFOAM 16 October 9, 2007 09:33 oseen OpenFOAM Installation 9 August 26, 2007 13:50

All times are GMT -4. The time now is 16:56.