Thermal Boundary Layer - Adiabatic Walls Pipe Flow
 

Hi All,

I am simulating the air flow in a simple straight pipe with adiabatic walls.

The conditions are as follows:

• Incompressible steady flow
• Inlet temperature = 450 C deg
• Inlet velocity = 100 m/s
• Outlet pressure = 1 atm

The problem should be very easy. Anyway, looking at the results, I see a high temperature gradient close to the wall surfaces, in direction normal to the wall (passing from 450 C of the core flow to 458 C at the wall prism layer).

First, I am a little rusty about this topic but, is it correct to have a thermal boundary layer in a problem like this with adiabatic walls?
I would say "yes" because total temperature should remains constant, thus a decrease of velocity at the wall implies an increase of temperature. Anyway, I am keen to listen others' opinion.

Second, if it is correct to have it, is such a high temperature change (Delta T = 8 C deg) a reasonable value for this problem?

Thanks.

Tommy

You should expect the adiabatic wall temperature to approach the stagnation temperature. What is the stagnation temperature for this case? 455 °C?

A thermal BL is possible with adiabatic wall, but you have to assess the normal component of the temperature gradient being resolved by the grid and verify it is zero.

Hi LuckyTran,

Yes, the stagnation temperature is 455°C.

I looked at the total temperature field close to the walls and the value is 458°C. This means that the temperature approaches the total temperature at the walls.

According to what you wrote this is correct and it answers my first question. Thank you.

Anyway, as far as I know the increase in the total temperature should not be present, I don't know if it has a possible physical explanation or it is a numerical error related to mesh and turbulence model.

Do you have any idea?

Tommy

Hi Professor Denaro,

Good to have another confirmation to my question, thanks.

I am not sure I understood the last sentence.

First, do you mean that I have to check if the temperature difference between the wall and the prism layer cells in contact with the wall to be zero (zeroGradient boundary condition)?

Secondly, how can I assess if the grid can solve the temperature gradient? By checking the yPlus?

Yes, the temperature contour should have a line that is normal to the wall of you have resolved correctly the BL. If Pr is O(1), the constraint for the dynamic BL applies also for thermal BL. Thus, at least 3-4 nodes at y+<1.

And are you including any viscous dissipation terms in your energy equation? What is in your TEqn.h or EEqn.h?

Yes, I am simulating a viscous incompressible steady flow.

I am using a pressure-based segregated solver and a k-omega SST turbulence model. Wall y+ < 1 everywhere (actually I have a value definitely too small for it, y+ <0.1).

I tried also to solve it with a compressible solver and to switch to k-epsilon turbulence model, but I have the same issue.

The only thing that worked was to coarsen the mesh in order to have y+>1. In that case I did not have that issue, but it was only because the mesh was not able to capture that tiny flow feature.

The first thing I would do is to check what happens without any turbulence model. But I have some doubts:


- incompressible flow model means Mach->0, if I remember well, the non-dimensional number for the dissipation would tend to zero.


- incompressible flow model means the pressure has no thermodinamic meaning. How do you couple your energy (temperature) equation with the momentum?


Again, check the adiabatic condition is really fulfilled.

Regarding the first point, I don't know what this means and implies. Do you mean that in an incompressible flow viscous dissipation tends to zero? Thus no losses are present?

About the second point, as far as I remember for incompressible flows the coupling is only between pressure and momentum. Temperature is calculated afterwards from the energy equation. But the energy equation does not affect the p-U coupling, it is a sort of "post-processing" calculation. I am not absolutely sure about it, so feel free to correct me if I am wrong.

Anyway, I perform some tests following your advice and then I will come back with the updates. Thanks.

Have a read of the page extracted from Kundu that confirms what I wrote about dissipation.

The incompressible flow model can be coupled to the temperature equation via the buoyancy term.

To be clear, I don't think it's a big issue that you have 3 deg higher than the total temperature. This is like a gentle breeze on a hurricane scale of disasters that can happen.

I bring up the viscous dissipation because with viscous dissipation, total enthalpy is constant but temperature increases due to the source term and that can explain why you have an extra 3 degrees. And if the term is off, then we know it's non-physical and can hunt down the numerical reasons.

Pressure-based segregated solver and viscous incompressible flow really does not answer my question if you are actually solving a compressible case or not and whether you have viscous dissipation source terms in your energy equation. That still needs to be checked. You can have a viscous momentum equation and no viscosity in your energy equation (and this is by far the most common approach to doing CFD). Especially, it sounds like you are using a commercial solver, and these are almost always a compressible solver.



If the energy equation doesn't affect the coupling then you wouldn't have a "segregated" solver. So while your intuition of how the problem should be solved is correct, what is actually be doing is not what you think.

Hi LuckyTran and Professor Denaro,

Yes, I totally agree that 3 degrees are negligible but I am curious to understand why I get this error for such a simple simulation.

I ran the simulation also with inviscid and laminar flow solvers and, for those cases, I don't have this issue. Thus, I guess the error comes from the turbulence model.

Regarding the solved equations, I am using STAR-CCM+ so I am not able to check which terms I have in the energy equation.

In the sentence you wrote, did you mean that temperature can increase due to viscous dissipation, not total temperature, right?

Tommy

Since you are using Star it does always include the viscous heat generation term. You can see the amount of this heat generation if you enable temporary storage. If you know the boundary layer thickness you can also compare it with an order of magnitude estimate to confirm, but it's faster to just get directly the number from Star. Turbulent flows have sharper velocity gradients, which is consistent with your issue that you only notice it for turbulent cases. We are splitting hairs over 3 degrees but one thing you can do is crank up and down the viscosity and/or conductivity or keep those constant and jack up the velocity.

I tried the tests you mentioned and the results are:

- Decreasing the viscosity or the velocity I am able to mitigate the issue, the more I decrease one of them the less the total temperature difference.

- Increasing the thermal conductivity gives the same result but if I decrease it, then I have a much higher temperature only in the first prism layer.

Considering a generic pipe flow problem, is it possible to have an increase in total temperature due to viscous losses?

(I don't think so, but I ask to be sure not to have started from a wrong idea).

Keep in mind we haven't ruled out numerical issues yet...

Total temperature is constant in the absence of external work implicitly assumes that the temperature rise due to viscous effects is negligible. With viscous effects, total enthalpy is constant.

You can make plots of all 4 to compare. Static temperature, total temperature, static enthalpy, and total enthalpy. If the total temperature and total enthalpy plots are everywhere constant then it is not due to viscous heating.

The total temperature evolution can be studied by means of the total enthalpy equation. You will see that DH/Dt, that is the variation of total enthalpy along the trajectory of a particle of fluid depends on reversible and irreversible work as well as on the thermal flux. Even in absence of such terms, the equation DH/Dt=0 must be associated to the uniform inflow condition to assume that H is homogeneous.


Note that when you solve a statistical system of equations like in RANS, the variable are not the classical one but the mean variable. A closure model introduces some more arbitrary term.

Hi everyone,

Sorry for the late update.

I tried different tests and I found out that the slight increase of total temperature within boundary layer is due to the velocity magnitude (100 m/s). If I decrease the velocity, e.g. to 20 m/s, the issue disappears.

If I switch from the incompressible air model to the compressible ideal gas one, then the issue is fixed also with the original velocity.

This difference (incompressible vs. compressible) is strange to me since the incompressible gas assumption should be fulfilled (Mach number is around 2.5). Anyway, it looks like the issue was caused by compressibility.

Thanks everybody for you help.

Tommy

Mach number around 2.5 ????

Pardon me, Mach number around 0.25.