Hi friends, First i will define the pysics of problem. We are trying to model the REACTOR with two phases Liq and Gas. But to avoid the complications to solver, we are modeling the 2-phase system as SINGLE PHASE (liq) system with Liq-Gas interface replaced by Free-slip wall. The mass transfer between Liq and Gas can be given as Mass-flux for species. When the species (like Hydrogen, CO2, CH4) transfer from liquid to gas phase (here flux@freewall) the partial pressure of speices in Gas phase changes. To account for this we are defining PARTIAL PRESSURES AS ADDITIONAL VARIABLES.

The partial pressures (additional variables) are changing with time. Which is function of Conc in liquid phase as well as the partial pressure in gas phase.

I want to know whether we can model PP of species as additional variables? If we can then there is difficulty whether to define it as transport equation or algebraic equation? If we define transport equation then variables will be transported and present in Liq phase, which is not realistic. And if we define algebraic equation then how to model the variation with time?

Can somebody give insights to the problem? I will be greatfull.

Thanks in advance Tuks

Hi,

If I understood well, you have, for the Hydrogen, a variable <font color="green">PP of Hydrogen at Gas</font> and another variable <font color="green">Concentration of Hydrogen at Liquid</font>. Both are simple variables, this is <font color="green">Concentration of Hydrogen at Liquid</font> is constant for the whole liquid. Am I right?

If I am right, I think you could define in Pre both variables as Transport Equations (set the Diffusivity to zero), then after applying the domain settings, right click on the Fluid Models object within the domain and select "Edit in Command Editor". In the command editor, under the ADDITIONAL VARIABLE object, replace "Transport Equation" with "Poisson Equation". ( http://www.cfd-online.com/Forum/cfx_....cgi?read=7829 )

Define the whole liquid domain as a Subdomain. In the Subdomain you can define source terms (positive or negative) for each additional variable.

Each variable will then be calculated at every mesh node, but they will have the same value at all the nodes.I've never worked with Fortran in CFX, but this could perhaps be done in User Fortran avoiding the need to calculate each variable at every nodes.

P.S.: I don't know why, but the Poisson Equation isn't described in the Documentation and it isn't possible to set it directly in Pre. However, in the Solver Manager editing the def file (Flow - Domain - Fluid Models - Additional Variable) you have access to it. You'll find more information about the Poisson Equation, if in the CFX-Comunity forum you search for it.

Hope this helps.

Rui

If you have access to the CFX-Community forum, take a look at these topics:

http://www-waterloo.ansys.com/commun...p?TOPIC_ID=744

http://www-waterloo.ansys.com/commun...p?TOPIC_ID=968

Hi Rui,

I thak you for your advice. You have quite understood the problem but the concentration of species in liquid (domain) is not constant throughout, it varies with space. And also i think poisson equation will not work since we have to solve for variation of additional variable with time. We can imagine that some species dissolved in liquid are transfering from liqid to gas (defined as freeslip wall). The species transfer is function of conc in liquid as well as time. This tranfer changes the partial pressure (additional variable) in gas phase. The equation is as follows.

dPi/dt = (Ni*Vliq*RT*Ptotal - Gtotal*Pi)/Vgas

Ni = Kla*(Ciliq - Pi/Hi) and Gtotal = sum(Ni) *Vliq*RT

Where, Pi, Ni - partial pressure and mass transfer from liq.

Hi - Henry's constant for species 'i'

Vgas, RT - Gas phase volume (constant), gas constant multiplied by temperature.

Ptotal = total pressure in gas phase = sum(Pi).

HOW TO SOLVE THE FIRST EQUATION? It contains the concentration in liquid phase Still if you are not clear about the physics then, can you please give me your 'emalid'

Thank you once again for your kind advice.

Regards Tuks

Hi,

You're right, Poisson equation won't work, it should be Diffusive Transport Equation

Poisson Eq.: <font color="blue">d/d_x( k * d/d_x(phi) ) + S = 0</font>

Diffusive Transport Eq.: <font color="blue">d/d_t( rho * phi ) = d/d_x( k * d/d_x(phi) ) + S</font>

• (I think this is correct, but it isn't described in the Documentation)

So if you want to solve your 1st equation, you should select the Diffusive Transport Equation, define k=0 and S=(Ni*Vliq*RT*Ptotal - Gtotal*Pi)/Vgas. Note that k is the effective diffusivity, if the flow isn't laminar it is different from the kinematic diffusivity. For the Transport Equation, if you want to set the effective diffusivity to zero, you have to leave the Kinematic Diffusivity box unchecked. I suppose it's the same for the Diffusive Transport Equation, but it isn't described in the Documentation.

I'm not sure if this helps,

Rui