[Peter023]

Hello everyone,

I'm doing some particle transport and settling simulations using the Fluent 6xxx and a scalar with UDS. For the scalar mass flux, an UDF is employed and the flux is set in boundary conditions for each surface (UDS > Specified Flux).

My problem now is to set the UDS concentration at the each boundary (surface) to zero and make the surface as a perfect sink for the UD scalar.

Does anybody know how to resolve this problem ?

Thanks in advance.

[sgrshukla]

Hello Petr,
I am doing similar work right now, my problem is to Give zero flux every where except the floor where i consider the source of the concentration.

I defined User defined scalar and applied the boundaries, I want to measure concentration at different points in space at different time(Transient), If you could help me regarding this would be lot helpful to me ..


thanks in advance,
Sagar

[sgrshukla]

Originally Posted by Peter023

Hello everyone,

I'm doing some particle transport and settling simulations using the Fluent 6xxx and a scalar with UDS. For the scalar mass flux, an UDF is employed and the flux is set in boundary conditions for each surface (UDS > Specified Flux).

My problem now is to set the UDS concentration at the each boundary (surface) to zero and make the surface as a perfect sink for the UD scalar.

Does anybody know how to resolve this problem ?

Thanks in advance.

Can we use negative flux for sink ??

[Peter023]

Hello sgrshukla:

the solution of this problem is less complicated than it looks at the first sight.

Firstly, you must know how do you want to specify your particle/gas mass flux towards the surfaces or whether you have specified source term in the Fluid Zone. If you have specified the mass flux in Boundary Conditions panel, you can not set the zero value at the boundary at the same time. In this case you can resolve the problem by Fluid Zone near the boundary, i.e. to set the UDS concentration to zero in the Fluid Zone near the boundary which you must create first in your model. The only problem is, that you may get an unrealistic results.

The other way is to reverse the sign of the calculated mass flux in your UDF. The scalar will be drawn out from the calculation domain and the effect will be similar as in the Fluid Zone case.

The last way I successfully used is to set the UDS concentration of the scalar at the boundary. For example you can take the UDS concentration at the first cell C_UDSI(c,t,0) and multiply this number by a constant or use some more complicated equation. This works very well in my case and by this way I could get a good results for particle distribution (Drift Flux model). The core of the drift flux model is implemented in the source term for the fluid zone.

Unsteady solution is then very easy to get, just iterate steady state model without UDS, after convergence reached just switch you simulation to unsteady with the :Frozen Flux definition: and in the solution panel select only UDS to be solved.

That's it.

Hope it will be helpful.

Regards
Peter.

[kingjewel1]

Originally Posted by Peter023

Hello sgrshukla:

the solution of this problem is less complicated than it looks at the first sight

The other way is to reverse the sign of the calculated mass flux in your UDF. The scalar will be drawn out from the calculation domain and the effect will be similar as in the Fluid Zone case.

That's it.

Hope it will be helpful.

Regards
Peter.

Hi Peter,

You're obviously an expert in your field. Would you mind just clarifying quickly the bold. Must a UDF be used to extract a UDS from the fluid zone? Can it not be done directly through the GUI in boundary conditions?

I'd extremely appreciate your response

[Peter023]

Hello kingjewel1,

the problem of the UDS scalar trasport as particles trasport is that we need to implement gravity and other body forces on this scalar, i.e. to adopt a suitable mathematical model. In this case the model is known as the Drift Flux Model defined in an UDF. So, in Fluent, we define the behaviour of our model via zones' or faces' UDS definitions (specified flux+UDF) and therefore we cannot set a numerical value anymore. This option is simply occupied by our own UDS. Moreover, the UDS flux, which must go out of the domain (settling effect of particles), is not constant and depends on overall UDS concentration (density) in whole computational domain.

For more info, please read some papers about 'Drift flux model': http://www.sciencedirect.com/science

To sum up: the is no need to use an UDF to extract the UDS from the domain if the 'extraction rate' (sink) is constant and there is no other model employed. But it is neccessary to consider accuracy of the solution and agreement with the measured data.

Hope it'll be helpful.

Pete.

[bkk]

hello everyone,
great posts and questions so far. Some have been quite useful. In particular I have a question regarding the use of the UDS as a concentration flowing in a tube. I have assigned the inlet surface the UDS concentration value. However, for the outflow, I wanted to assign a zero axial gradiant. The outlet surface boundary condition is outlet, pressure, exhaust. I wasn't sure if I assign 0 for the flux it would impede the concentration from flowing or whether the program was 'smart' and consider it a stress-free condition. Secondly, if the first (i) condition is true, would I need to write a UDF to choose which states that the gradient of the concentration is zero. If so, suggestions on how, e.g. which command (define_adjust, define_profile, etc)?
Thank you so much.

[hem233]

Hello bkk,
Have you solved the problem on how to specify boundary condition at the outlet for UDS concentration, if so then how have you done it?
Please, help of any kind is appreciated.

Thanks.

[randolph]

Originally Posted by Peter023

Hello sgrshukla:

the solution of this problem is less complicated than it looks at the first sight.

Firstly, you must know how do you want to specify your particle/gas mass flux towards the surfaces or whether you have specified source term in the Fluid Zone. If you have specified the mass flux in Boundary Conditions panel, you can not set the zero value at the boundary at the same time. In this case you can resolve the problem by Fluid Zone near the boundary, i.e. to set the UDS concentration to zero in the Fluid Zone near the boundary which you must create first in your model. The only problem is, that you may get an unrealistic results.

The other way is to reverse the sign of the calculated mass flux in your UDF. The scalar will be drawn out from the calculation domain and the effect will be similar as in the Fluid Zone case.

The last way I successfully used is to set the UDS concentration of the scalar at the boundary. For example you can take the UDS concentration at the first cell C_UDSI(c,t,0) and multiply this number by a constant or use some more complicated equation. This works very well in my case and by this way I could get a good results for particle distribution (Drift Flux model). The core of the drift flux model is implemented in the source term for the fluid zone.

Unsteady solution is then very easy to get, just iterate steady state model without UDS, after convergence reached just switch you simulation to unsteady with the :Frozen Flux definition: and in the solution panel select only UDS to be solved.

That's it.

Hope it will be helpful.

Regards
Peter.

_________________

Hi,

I always wonder what is the most realistic condition for the net deposition simulation. perfect sink (zero con.) or no flux (zero grad.)?

Thanks,
Rdf