CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Ammonium gas in the air (http://www.cfd-online.com/Forums/openfoam-solving/58007-ammonium-gas-air.html)

christian June 9, 2008 03:34

I'm investigating the potentia
 
I'm investigating the potential of predicting the traveling of ammonium gas in air. From one building ammonium gas is released into the open, what will be the concentration at the air inlet of an adjacent building? This is what I'm hoping to simulate. What would you suggest me in general terms? What solver?

christian June 9, 2008 04:25

Hi Dragos, Thank you for th
 
Hi Dragos,

Thank you for the answer. Can I contact you on some e-mail address? I tried the lth address but it didn't work. Should I go with the yahoo address?

Best regards,
Christian Svensson

dmoroian June 9, 2008 05:05

Uh, the lth address is no long
 
Uh, the lth address is no longer valid (since 2005). You can contact me on the yahoo address, though.

Dragos

christian June 12, 2008 11:04

When talking to people I'm giv
 
When talking to people I'm given the advice to use a scalar transport for the ammonium gas. But the density of the ammonium gas is only 60 of the density of air. I want to account for this.

I guess a way could be to use some kind of solver where I calculate the density of each cell based on the mass balance between air and ammonium.

But this is not true. If a cell consists of 50 % air and 50 % ammonium, the ammonium should travel upwards compared to the air due to it weighs less. But since there are not two phases when using the scalar transport approach, the entire cell containment will travel upwards due to its smaller weight compared to a cell with 100 % air.

sradl June 12, 2008 11:23

Dear Christian, you are fac
 
Dear Christian,

you are facing a hard problem, if you want to couple the species transport solver to the flow solver, as you have to run transient and the coupling will lead to instabilities if your time step is too big.

I not fully agree with your view on the "50% air and 50% ammonium" thought experiment: gases mix in a homogeneous fashion, so both air and ammonium will rise. You will already account for the force separating the two gases if you calculate the density as a function of the local gas composition.

Maybe you think of the problem that you'll have when your mesh is too coarse: numerical diffusion will smear out the concentration field and make the result unrealistic, e.g., too much mixing. I'd suggest to test the influence of the mesh size in detail.

br
Stefan Radl

christian June 12, 2008 11:51

Thank you for your input Stefa
 
Thank you for your input Stefan.

I seem to have three choices:

1) Use scalar transport to account for the ammonium gas. This means that I assume that the ammounium gas doesn't affect the flow (of air). When can expect this assumption to fail? I have little knowledge within this area. What if air flows in a horisontal pipe and ammonium is injected in a small area around the center of the inlet. It would diffuse as it travels downwards. I assume this diffusion coefficient is to be input in the scalar transport model? But what about the fact that the ammonium gas only weighs 60 % of the air. Wouldn't that make the ammonium wanna travel upwards?

2) Do the same as (1) but recalculate the density in each cell based on the scalar fraction.

3) Use rasInterFoam to account for the two phases of different density and viscosity. Does rasInterFoam solve for the position of the phase change or does it solve for a phase factor (0-1) in each cell? I'm a novice as I said before.

I'm grateful for any help from anyone.

alberto June 12, 2008 22:49

Dear Christian, to answer
 
Dear Christian,

to answer your questions in your last message:

1) The diffusion coefficient, if the flow is turbulent, depends more on fluctuations than on molecular diffusions, and it is defined, in a RANS approach, as the ratio between the turbulent viscosity and the turbulent Schmidt number (Sc). You can find the value of Sc in the literature (tell me if you need references). The default value in many commercial packages is set to 0.7.

2) I suggested you by e-mail, give a look at the ventilation and heat transfer solvers for this approach. Of course, the simulation will be time-dependent.

3) I disagree with this approach. A gas mixture _is_not_ a multiphase flow. Gases mixes in all proportions, constituting a single phase. As a consequence, in a cell, only the gas mixture exists as a single entity, and not two separate entities (phases). So you have a single density and a single viscosity (assume it constant in your case).

Anyway, before going the complex way, I would like to know what is the concentration of ammonium you want to consider.

With kind regards,
Alberto

christian June 13, 2008 02:05

Thank you for the answers and
 
Thank you for the answers and the discussion.

I will know the concentration entering my domain next week. But the ammonium gas is released from one building, into the open. It will then travel somehow depending on the wind and position of adjecent buildings. An air intake is placed on one of those adjacent buildings. I need to find the maximum concentration of ammonium gas at this air intake. So the ammonium concentration will be very low, but even a very low concentration is dangerous to humans. However, this very low concentration is good from a modelling point of view. The ammonium gas will not affect the flow of air (in the open, the wind) and could be modelled as a passive scalar from that point of view. My concern is the different density of ammonium compared to air even though the concentration is low. The densities are different and I assume it doesn't matter that the concentration is very low. I still need to predict the way the ammonium gas travels.

For buoyant flows one can tell if buoyancy effects can be neglected by checking if Gr/Re^2 << 1. I assume one could do the corresponding in this case for the gravitational effect. I haven't had time to think this through yet but any input is welcome.

I don't believe there will be any temperature differences.

Grateful regards,
Christian

niklas June 13, 2008 04:53

Hey, Here's a small case I
 
Hey,

Here's a small case I just set up to demonstrate how you could do this using dieselFoam.

http://files.nequam.se/ammo.tgz

The gravity is downwards and a small inlet of NH3 is placed at the bottom left and a small outlet at the upper right.
Here's a movie that shows you the result.

http://files.nequam.se/nh3Room.avi

I've plotted rho and NH3 concentration.

lara_areis February 3, 2009 11:18

Dear all I am quite new in
 
Dear all

I am quite new in CFD and OpenFoam.
I am trying to simulate de dispersion of gas pollutants in the the atmosphere using dieselFoam, with chemistry off.
I used the ammonia case that Niklas Nordin post on the forum as a build up point. I have changed the mesh to a much simpler case in witch the inlet is the whole left wall. It seems as though I have been having some problem with the injectorProperties. What I wanted to know to be able to continue is what is really the function of the injectorProperties? Do these properties control the entrance of the pollutants at the inlet? or can I simply define a velocity boundary condition and a concentration at the inlet, and not use the injectorProperties?

Thank you in advance
Best regards

Lara

hsieh February 3, 2009 14:22

Hi, Niklas, I tried to run
 
Hi, Niklas,

I tried to run your ammo.tgz using dieselFoam in OF-1.5, but, got error. Something like: "unknown variable name "FOAM_ROOT". Do you have any idea how to fix this? Thanks!

Pei

hsieh February 3, 2009 14:41

Hi, Problem solved. I had
 
Hi,

Problem solved. I had to edit thermophysicalProperties under constant.

Pei

mahaputra May 19, 2009 09:45

Co2 + h2o
 
1 Attachment(s)
Dear Mr. Niklas Nordin


I try to modify ammo case for my condenser problem


but the result really not satisfied and looks strange. All of the CO2 flows down to the bottomOutlet. none goes up to the topOutlet.


in the inlet i try to define mixture of CO2 + H2O vapor (0.9 + 0.1).

and in the internal field, i initialize with air (N2 + O2)

N2 = 0.766
O2 = 0.233


my expectation is, i can see the behaviour of the mixture inside my condenser, and the effect of the cooling. the a partial of water vapor will flow down , and most of the CO2 will flow up.

here i attach the movie of CO2 fraction.


i really need any comment and help



--
--
Regards



Nugroho Adi Sasongko

mahaputra May 19, 2009 09:50

Oh ya

for my case, the gravity is negative y

g g [0 1 -2 0 0 0 0] (0 -9.81 0);


so, setting of the environmentalProperties is correct


please give me some comment and help

mahaputra May 21, 2009 10:01

Hei?


Nobody can answer my question?

at least just a comment? please





my T inlet = 363 K
and T internal field is = 300 K

it sould be some amount of my CO2 with go up to the topOutlet.

but i really dont know, whats wrong with my case

:(

mahaputra May 21, 2009 10:03

it sould be some amount of my CO2 goes up to the topOutlet.

nikolay_k January 12, 2011 12:51

Hello mahaputra.
Could you please update us on that problem? I'm onto a similar task and I was wondering, whether assuming that gravity acted downwards (setting a positive value for g) helped to solve your case...
Thank you.

wmrlak September 4, 2014 13:59

Quote:

Originally Posted by alberto (Post 200487)
Dear Christian,

to answer your questions in your last message:

1) The diffusion coefficient, if the flow is turbulent, depends more on fluctuations than on molecular diffusions, and it is defined, in a RANS approach, as the ratio between the turbulent viscosity and the turbulent Schmidt number (Sc). You can find the value of Sc in the literature (tell me if you need references). The default value in many commercial packages is set to 0.7.

2) I suggested you by e-mail, give a look at the ventilation and heat transfer solvers for this approach. Of course, the simulation will be time-dependent.

3) I disagree with this approach. A gas mixture _is_not_ a multiphase flow. Gases mixes in all proportions, constituting a single phase. As a consequence, in a cell, only the gas mixture exists as a single entity, and not two separate entities (phases). So you have a single density and a single viscosity (assume it constant in your case).

Anyway, before going the complex way, I would like to know what is the concentration of ammonium you want to consider.

With kind regards,
Alberto

Hello,
This is quite an old thread but could you please send your suggestions to me too? I am dealing with a similar problem.

Thank you in advance


All times are GMT -4. The time now is 06:42.