
[Sponsors] 
July 15, 1999, 12:50 
Multiphase models in CFX

#1 
Guest
Posts: n/a

Hi there,
I am using CFX to simulate the mixing of two gases (air and methane) inside a furnace using an isothermal model. The geometry of the furnace is quite simple (close to a rectangular box). There are two inlets: one central circular inlet for methane and an annular non swirling inlet for air. Now, the CFX User Guide advices the use of an homogeneous model for the turbulence of nondispersed cases (like my case!). This model assumes the solutions fields for each phase identical. When setting K and Epsilon I use the mean inlet velocity. Is it sensible to use those?? For the momentum I chose the multifluid model because they will have different velocity fields. Moreover I specified the mixture model to be used, which assumes both phases symmetrically and it is said to be appropriate for a calculation of nondispersed twophase flow. The problem arises when running the solver, where neither converges nor diverges. Eventually it seems to converge but at a very slow pace. So far I've only runned it for a maximum of 1000 iterations. Should I expect an extremely slower convergence for my case??? And what about the mass residuals for my two phases? In the residual plot I can only get track of one mass phase residual. Why is that?? And what values to specify for the mixture model parameters (drag coefficient and interfacial length scale)? Does anyone understand anything of what I've been writing??? Have you worked in a similar problem?? If yes, please give me a hand! All comments are welcome! Thank you Sara 

July 15, 1999, 16:37 
Re: Multiphase models in CFX

#2 
Guest
Posts: n/a

Hi, Sara.
>Does anyone understand anything of what I've been writing? Khgm, I am not sure about me >I am using CFX Is CFX one of those commerical solvers used without understanding what they (the solvers) are doing ? In reading the rest please keep in mind that I have no idea what CFX is. > mixing of two gases (air and methane) inside a furnace using an isothermal model. >For the momentum I chose the multifluid model because they will have different velocity fields. Well, no. Multifluid model assumes that it makes sense to think about two velocities at the same point in space. This is the case if there are, say, heavy dust particles moving through the air, and these particles are modeled as a fluid. Now, both particles and molecules may have a chaotic component of velocity (represented by diffusion and/or viscous terms in the equations) and mean component of velocity, for which those equations are written for. Naturally, particles can have one mean velocity and air can have another (consider rain drops as particles, for example). For gas mixture, allthough gases will diffuse through each other, this motion is of a chaotic nature, and is governed by a convectiondiffusion equation for concentration: the mean velocities of mixed gas components are almost the same, and the difference certainly should be neglected in the momentum equation. Read the manual for CFX if there is one, it might be there is something there. >And what values to specify for the mixture model parameters (drag coefficient and interfacial length scale)? Drag coefficient is for a particle moving through an air, like a body, this is quite ordinary parameter for dasty gas flow, but not for gas mixing. So, most probably you should forget about multifluid model, drag, lengthscale etc. in your case. Hope this helps. Sergei 

July 16, 1999, 10:16 
Re: Multiphase models in CFX

#3 
Guest
Posts: n/a

Hi Sara,
As Sergei mentioned, twophase flow model refers to (e.g.) dust particle moving in a gas, with drag forces and other things maybe. What you want to do is different. In all the domain you need to have specified the fraction of each gas by weigth, e.g. X represents the Oxygen (in the air), Y represents the fraction of Nitrogen (air) and Z the fraction of Methane. XY and Z will then enter the equation of state through the mean molecular weight, etc.. The next step will be to solve the diffusion equations for the different gas (XY and Z). For the rest there is only ONE FLOW, with its density and velocities (NavierStokes equations). Where the Methane is injected there will be an initial (and boundary) condition for the velocities and density, and where the air is injected some other condition for the density and velocity (in a different region of the computational domain). If the rest of the chamber is empty, then in between the two gases, initially the density and velocity are set to a very small value. Once the gases interact there will be only one flow. To follow where the methane 'is', one needs to solve for the fraction of the different gases using the diffusion equations. I am also not familiar with CFX. Cheers, Patrick 

July 19, 1999, 07:59 
Re: Multiphase models in CFX

#4 
Guest
Posts: n/a

Hi Sara
I am new in CFX but i think your problem is not a multiphase problem but a single phase multi component flow. In the CFX Examples Manual you can check Reference Example 10. It deals with CO2 and air in a box. I hope it helps Zoltan Turzo 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Multi phase flow  skatun  CFX  6  July 28, 2014 06:37 
Conformal Mesh in Multi Phase Flows  ziyasaydam  STARCCM+  2  March 16, 2010 16:29 
regarding multi phase flows  srikanth  Main CFD Forum  1  January 26, 2006 03:49 
Multi Phase option problem....  Christos Sfyris  Siemens  1  May 22, 2003 07:53 
Two phase flow models  Atholl  Main CFD Forum  2  May 7, 2002 03:49 