[cfdEng_]

Background: My goal is to study flow over an isothermal plate covered with hemispherical wall features. The far-field temperature is equal to 0.9*Wall_Temperature.

Problem: To simulate an "infinite" domain, I impose periodic BC sideways and I would need flow recirculation from exit to inlet. I am running LES so I have to recirculate Density*Velocity at every time-step.

Question: Would you have any practical suggestions on how to do it?

Thank you.

[vinerm]

What do you mean by Flow Recirculation? If it implies translational periodicity, then you can make inlet and outlet periodic, just like your side walls.

[cfdEng_]

Originally Posted by vinerm

What do you mean by Flow Recirculation? If it implies translational periodicity, then you can make inlet and outlet periodic, just like your side walls.

Ideally, I would like to simulate an infinitely long domain so that the flow field is not affected by the entrance effect.

I don't think I can simply impose translational periodicity between inlet and outlet. The fluid experiences a total pressure drop throughout the domain.

[vinerm]

For modeling an infinitely long domain, translational periodicity is the most suitable condition. Translational periodicity allows user to specify either mass flow rate, which, of course, stays constant along the length or the pressure drop per unit length. So, you can specify one and Fluent will calculate the other. Other alternative is to make it really, really long.

[cfdEng_]

Originally Posted by vinerm

For modeling an infinitely long domain, translational periodicity is the most suitable condition. Translational periodicity allows user to specify either mass flow rate, which, of course, stays constant along the length or the pressure drop per unit length. So, you can specify one and Fluent will calculate the other. Other alternative is to make it really, really long.

Thank you very much, that was very useful. I would have one more related question.

In my case, I have two periodic BCs: side walls and inlet-outlet. Thus, I need to set the pressure drop to 0 sideways (periodic side walls), and to a specified value in the flow direction (inlet-outlet). However, through the GUI, I can only define a single pressure drop value that is applied to all periodic BCs.

Do you know how can I impose a specified pressure drop from inlet to outlet and a 0 pressure drop sideways?

Thank you in advance.

[vinerm]

I am afraid that's not possible. However, if there is not cross flow, then you can use symmetry condition for the side wall. If there is cross flow, then you have no choice but to either make the domain very long or use a UDF.

[cfdEng_]

Thank you for your answer.

[LuckyTran]

You use the periodic BC for the inlet and outlet.

For the sides, you use a periodic interface.

[vinerm]

It won't matter whether you use interface to create translational periodic boundary or directly create it via TUI. The periodic conditions apply to all translational boundaries.

[cfdEng_]

Thank you for the explanation.

According to the FLUENT user's guide, the actual temperature field is not periodic; nevertheless, the scaled temperature (theta) obeys the periodic condition. (Link: https://www.afs.enea.it/project/nept...4.htm#eq16.4.4).

Question 1: if the scaled temperature at the inlet is equal to the scaled temperature at the exit, and we specify Tbulk and Twall, how can the actual temperature not be periodic? (see eq. 13.4-1 from the user's guide)

Question 2: is the 1st Law of Thermodynamics satisfied by such a periodic heat transfer solution?

[vinerm]

The periodicity definition is nothing but a way of saying that the profile is independent of axial location. While the temperature field changes, the profile defined with transformation of variable to maintains its value. This does not imply that T has to maintain its value; it only has to maintain its profile, which is true for a developed flow. Apparently, that is the definition of the developed flow - no variation of profile along the axial direction. T (also ) will still be function of radial or wall normal direction but not of the direction along the wall.

This has no conflict with first law of thermodynamics since the heat flow depends on gradient and gradient is nothing but mathematical description of profile; similar profile implies similar heat flow.

[cfdEng_]

Originally Posted by vinerm

The periodicity definition is nothing but a way of saying that the profile is independent of axial location. While the temperature field changes, the profile defined with transformation of variable to maintains its value. This does not imply that T has to maintain its value; it only has to maintain its profile, which is true for a developed flow. Apparently, that is the definition of the developed flow - no variation of profile along the axial direction. T (also ) will still be function of radial or wall normal direction but not of the direction along the wall.

Thank you very much for your answer. I am still not 100% sure about what happens to Density.

Question: pressure-based solvers calculate Density from the equation of state: it is a function of the local temperature. Nevertheless, in our case, continuity has to be respected between inlet and outlet and velocity is directly periodic (Uin=Uout). Therefore, it seems we would end up with two requirements for Density. How can that be the case?

Thank you in advance.

[vinerm]

Only for incompressible flows average velocity at inlet is equal to average velocity at outlet. It is a special case of real scenario. In reality, it is not the velocity but mass flow rate that is equal. So, it is the area integral of the product of density and velocity that remain same not the velocity itself.

[cfdEng_]

Originally Posted by vinerm

Only for incompressible flows average velocity at inlet is equal to average velocity at outlet. It is a special case of real scenario. In reality, it is not the velocity but mass flow rate that is equal. So, it is the area integral of the product of density and velocity that remain same not the velocity itself.

So if I understood correctly, by applying FLUENT's periodic inlet BC to compressible flows:

1. (rho*V)in = (rho*V)out
2. Temperature follows the treatment discussed previously
3. rho is calculated through the equation of state
4. V is derived from continuity

Am I right?

Thank you very much for your helpfulness.

[vinerm]

Yes, that is correct.

[cfdEng_]

Thank you very much for your helpfulness. I would like to ask another question if possible.

Background: My geometry is a duct with a squared section. As you suggested, I imposed periodic BC from inlet to outlet and symmetry BC to the sidewalls and the top surface. The bottom surface is a no-slip wall with uniform wall temperature, Twall=0.9*Tbulk.

Question: By simulating a hot flow over a cold plate I would expect to have a "parabolic" temperature profile where Tmin=Twall and Tmax=Tfreestream. However, I get a hot core with cold walls. How could I fix this problem and impose Tfreestream=Tmax?

[vinerm]

Any particular reason for expecting a parabolic profile? Top should not be symmetric, however, you can define it as free-slip wall.

[cfdEng_]

Originally Posted by vinerm

Any particular reason for expecting a parabolic profile? Top should not be symmetric, however, you can define it as free-slip wall.

Thank you for your reply.

I want to simulate forced convection of warm air over a cold plate, hence Tfreestream=Ttop=Tmax and Twall=Tmin. By contrast, I am getting a hot core with cold air close to the sidewalls and the top surface.

[vinerm]

Maximum temperature at the top and lowest at the bottom do not imply parabolic profile in between. That is defined by flow structure. If it is laminar flow, then you can expect parabolic profile, else, it would have very high gradient close to the wall and almost plug flow like structure outside. But if you are getting low temperature at the top, then that is due to wrong boundary condition on the top. So, check your thermal boundary condition.

[cfdEng_]

I am running a low-speed laminar simulation. At the top surface, I have simply set heat flux=0. Should I adopt a different thermal BC?