[hunger]

Hi everybody!

I want to simulate humidification of dry air with water vapour. The geometry can more or less be seen as some kind of T-junction, but the water inlet is very small compared to the air inlet.

First, I run a steady state simulation with simpleFoam to calculate the flow field. Here I make sure to get a converged solution and mass is conserved.
When I run scalarTransportFoam (also in steady state), mass conservation of the passive scalar is not given anymore.

I have tried different OpenFOAM versions (of4x, of240), the results are the same.
I found out that the diffusion coefficient has an influence on the result, i.e. the bigger "DT", the bigger is the difference between inlet and outlet massflow of the passive scalar. The result also gets better when I increase the inlet massflow with which the passive scalar is transported into the domain.
Therefore I thought that the difference might be due to diffusion of the passive scalar at the inlet (I am using a fixedValue BC at the inlet and a inletOutlet BC at the outlet). I know that in FLUENT one can switch off inlet diffusion at the inlet when calculating multispecies flow.

Has anybody made the same experience using scalarTransportFoam and can give me any hint? E.g. are there more suitable BC to use? Or does scalarTransportFoam in general run into problems, if the massflow of the passive scalar is very small compared to the main fluid flow?

Best regards
Harald

[Tobi]

Hey all,

this thread is already very old but there might be some people who are still interested in the answer of the question.


Generally, the scalarTransportFoam does not have any problems with that type of calculation and the phenomenon one sees here is purely a mathematical problem.

The problem our questioner encountered is as follows:

• We transport the scalar based on the fluxes and based on the diffusion
• Now, lets imagine a more realistic scenario based on the energy equation.
  • Imagine we have a small room in which one wall does have a hot surface included
  • We set the temperature to a fixed value here
  • The driving force for the energy exchange is the diffusion as the velocity is almost zero (viscouse sub-layer).
  • However, we can increase the energy exchange by putting a fan infront of the hot area.
  • What changes is that we take the energy away by convection and in addition we increase the diffusion coefficient namely the thermal diffusivity based on the turbulence which also increases the close-to-the-walls diffusivity
• However, this might be wrong in particular cases. E.g., imagine the temperature at the surface... it is constant and will not reduce even though we would take billions of joules away - its a matter of the boundary condition

Regarding the question asked here, the main problem is as follows:

• Small convection that transport the scalar into the domain
• Large influence of, e.g., cross flows that influence the diffusion based on turbulence

Hence, if the flux through an inlet is very very small, but for any reason there is a cross flow that introduce high turbulence close to that patch, the diffusion coefficient at the patch (or close to it) increases based on the turbulence models. The result is that we have an increased diffusion transport which is mathematically correct but probably not physical.

If we would imagine a tracer gas that is injected into a pipe, the inlet should not be added directly at the pipe-wall. We should include a small intake pipe section for the tracer gas in order to avoid the increase of diffusion at the inlet patch. Just imagine what happens here? The turbulence will take out the tracer gas maybe a few millimeters or centimeters from the added small intake pipe but will not influence the inlet patch. Hence, no artificial diffusion will increase any transport here.

I hope that my explanation is understandable.
If you are involved in that topic, its clear, if not, it is sometimes hard to understand.


Summary

• Inlet patches that do have small fluxes (transport through the flow) of any quantity but might be influenced by the internal flow based on turbulence should be exteneded in order to avoid artificial diffusion (which is physical correct but not in terms of the underlying mathematical description - boundary conditions)

Hence, for such purposes, Fluent offers the inlet-diffusion to be turned on or of. However, this does not only hold for species transport (as it is written in the fluent user guide).

Example: HVAC simulation with textile pipes which have 5 mm/s outflow. The surrounding air flow has 10 m/s - so high turbulent. However, the surface of the textile pipes are very large and the turbulence of the surrounding are is high too. If someone sets the surface temperature of the textile pipes to a fixed value (which is reasonable), you have one problem: The additional turbulence of the surrounding air increases the diffusion coefficient within the energy equation which increases the heat exchange at the large textile surface. Everything is physically and mathematically correct regarding the boundary conditions but it is not correct in terms of reality as the surface tempreature will change respectively. Hence a fixed value of the temperature in combination with the diffusion and a small flux will probably lead to wrong results.