CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Particle injection boundary condition (http://www.cfd-online.com/Forums/cfx/68388-particle-injection-boundary-condition.html)

fjalil September 17, 2009 09:56

Particle injection boundary condition
 
Hi. I'm modelling a multiphase flow problem with particle tracking. The problem consists on a channel or launder where ther is water flowing in the bottom, and air on top (a typical open channel). For the inlet boundary condition I had to use a step function in order to say that water enters on the bottom and air on top. The thing is, now I have to inject particles with the water. I want to use the option of uniform injection, but I don't know how to say that the uniform injection is only at the bottom part of the inlet (in the water step part).

Another question I have of the same problem is how can I say that the injection occurs after, say, 20 seconds, instead of using the default setting that the injection occurs at the beginning of the simulation.

Thank you very much.

Regards,

Francisca Jalil

John September 17, 2009 12:01

You can multiply your injetction quanitity with the volume fraction of water.

for your second question, a step function can be used to control the injection time

fjalil September 21, 2009 14:56

Still a doubt
 
Quote:

Originally Posted by John (Post 229787)
You can multiply your injetction quanitity with the volume fraction of water.

for your second question, a step function can be used to control the injection time


Hi, sorry, but I didn't really get the answers. In the first part, what do you mean with injection quantity? Do you mean the Number Rate ( I'm running a transient simulation)? I tried multipliying that value but I had an error:

"The parameter 'Number per Unit Time' in object '/FLOW/DOMAIN:Domain 1/BOUNDARY:Entrada/FLUID:Particulas fully coupled/BOUNDARY CONDITIONS/PARTICLE POSITION/NUMBER OF POSITIONS' is defined to be "Single Valued" but it depends on the following field valued variables: z."

In the second part, where should this function be written?

Thanks

Francisca

ckleanth September 21, 2009 19:44

you cannot perform a lagrangian eulerian simulation with multiphase.

instead you can can use the Eulerian-Eulerian multiphase model but you wont have the individual particle tracks. you might want to ask your self is the tracks important to your simulation, does the particles affect the flow? can you simplify it even more by using a passive scalar?

John September 21, 2009 20:40

Quote:

Originally Posted by fjalil (Post 230044)
Hi, sorry, but I didn't really get the answers. In the first part, what do you mean with injection quantity? Do you mean the Number Rate ( I'm running a transient simulation)? I tried multipliying that value but I had an error:

"The parameter 'Number per Unit Time' in object '/FLOW/DOMAIN:Domain 1/BOUNDARY:Entrada/FLUID:Particulas fully coupled/BOUNDARY CONDITIONS/PARTICLE POSITION/NUMBER OF POSITIONS' is defined to be "Single Valued" but it depends on the following field valued variables: z."

In the second part, where should this function be written?

Thanks

Francisca



For Question 2: you can inject particles within 0.1second as follows:
particle mass flow [kg s^-1]*step( (t-0.09[s])/0.01[s] )*step( (0.011[s]-t)/0.01[s])

John September 22, 2009 22:42

Quote:

Originally Posted by ckleanth (Post 230068)
you cannot perform a lagrangian eulerian simulation with multiphase.

instead you can can use the Eulerian-Eulerian multiphase model but you wont have the individual particle tracks. you might want to ask your self is the tracks important to your simulation, does the particles affect the flow? can you simplify it even more by using a passive scalar?

C


Read the help file again, I did not find words clearly showing that particle tracking can not be used for Eulerian-eulerian problem. This needs to be clarified by CFX technical support.

But I do know that CFX allows you to DEFINE particle tracking for eulerian-eulerian cases. Of course, you can only inject particles in the continuous phase, which could be tricky for free surface problems.

ckleanth September 23, 2009 02:54

Quote:

Originally Posted by John (Post 230210)
C


Read the help file again, I did not find words clearly showing that particle tracking can not be used for Eulerian-eulerian problem. This needs to be clarified by CFX technical support.

But I do know that CFX allows you to DEFINE particle tracking for eulerian-eulerian cases. Of course, you can only inject particles in the continuous phase, which could be tricky for free surface problems.

you missed the word "multiphase"... as I said, lagrangian eulerian simulation and multiphase (with two continuous phases as in a free surface problem) is not supported. perhaps I could had been more precise

John September 23, 2009 08:38

Quote:

Originally Posted by ckleanth (Post 230229)
you missed the word "multiphase"... as I said, lagrangian eulerian simulation and multiphase (with two continuous phases as in a free surface problem) is not supported. perhaps I could had been more precise

Thanks for clarify this. Two more questions regarding this:

1. One of my previous application case in version 10 was to do a particle tracking for a gas-liquid system in which liquid is the only continous phase. There is a degassing boundary in the model. I remember that particles can pass the degassing BC which should not happen in reality. What I did was to change the BC to wall when performing particle tracking. Is there a better way to do it?

2. Does CFX post have capacity to show histogram of particle tracking results at outlet. For example, if I inject 1000 particles, can CFX post show the distribution of retention time of particles?

Regards,
John

ckleanth September 23, 2009 09:40

1) have no idea, it seems to me its problem dependent and I never came across this issue
2) yes its a hidden feature (but not in post, cfx can provide particle disrtibution that hits a wall or exit a boundary), please ask ansys support on how to enable it


All times are GMT -4. The time now is 17:11.