[GaspA]

Hello everyone,

I come to you in order to understand and solve the problem that concerns me. I simulate the fluid flow in a tube heat exchanger. Only the fluid part (oil) is simulated. It is therefore the flow around the tubes of the exchanger.

I want to solve the fluid equations and those of the thermal to evaluate in a comparative way the efficiency of cooling of several geometries.

The key points are:

+ Openfoam version: V8.0
+ Solver: buoyantSimpleFoam/simpleFoam/potentialFoam
+ Fluid: oil
+ Mesh: approx 90 million tetra elements, with boundary layer, generated with Ansys Meshing
+ Mesh quality: max nonOrthAngle: 80 deg, max skweness: 2.7, Mesh Ok with checkMesh.
+ RAS model: kOmegaSST
+ Parallel computing: 2x 24 CPU AMD EPYC 7352 (without SMT)


Since the tubes are very close together and the flow between these tubes must be calculated, the mesh size is extremely small, about 0.7 mm. This, together with the viscosity of the oil and the very low flow velocities (from 0.1 to 1.5 m/s) generate very, very low y+ values: an example: average over a surface, 5e-5....

The calculation runs very well in simpleFoam with an initialization with potentialFoam. Which gives the above results.

The parameters used for the calculation with simpleFoam are:

+ div(phi, U) Gauss limitedLinearV 1
+ div(phi, k) Gauss limitedLinear 1
+ div(phi, omega) bounded Gauss limitedLinear 1
+ grad(iii) cellLimited leastSquares 1
+ GAMG Solver for p and smoothSolver for U, k and omega

The results seem quite logical and the convergence is going very well. A test without a turbulence model also works very well. This last calculation was made because the flow is mainly laminar.

However, when a test is made with buoyantSimpleFoam, despite an initialization of U with potentialFoam, the calculation diverges slowly.
This can be observed very well on the pressure residues and mainly on the 'time step continuity errors'.

For the tests with buoyantSimpleFoam, the characteristics were as follows:

+ Same as simpleFoam
+ div(phi,K|R|T) bounded Gauss upwind
+ GAMG solver for k with DILUGaussSeidel preconditioner
+ Relaxation factor h and T: 0.05

The boundary conditions for T are:

+ Inlet: fixedValue 315
+ Cooling tubes (wall): 272
+ All other walls: zerosGradient

For alphat:

+ Inlet: calculated
+ outlet: zerosGradient
+ all walls: compressible::alphatjayatillkeWallFunction

The oils are treated according to thermophysicalProperties:

+ heRhoThermo
+ pureMixture
+ hConst, rhoConst

It seems that it is the enthalpy equations that generate instabilities. Is this kind of problem known or could you mention a solution or a test to perform.

Thanks for your help

Best regards

GaspA

[Alczem]

Hey


I always have a hard time with buoyantSimpleFoam too!


What I would try:

• Set calculated for the outlet for alphat too
• Maybe try compressible::alphatWallFunction instead, I had more success with this one when using the kOmegaSST model.
• For the temperature, inletOutlet is a good choice for the outlet instead of zeroGradient
• Make sure your p_rgh conditions are ok
• 80 for non-orthogonality is quite high, maybe you can work on your mesh?
• Last but not least, you can try to run your simulation in pseudotransient with buoyantPimpleFoam and localEuler as a ddtScheme, it is usually more stable, but slower to achieve a "converged" state

Good luck!

[piu58]

Some time ago, I calculated something with buoyantSimpleFoam too: A very simple geometry, a flat plate. I had to deal with concentrations instead of heat, which arose additional problems.

I got the simulation running with free convection. I got non-physical results however, if I added external flow. Do you have external flow?

I experimented for a long time, but did not find a solution(!) for my problem. After a while, at the end of the plat the simulation generated unphysical high velocity, which went through the ceiling.