[julieng]

Hello,


I want to simulate exchanges between air and solid. I work with komegaSST.

I need to use fine grids to capture heat transfer.

I found on the forum that I need to fixe small values on walls for k and nut 1e-9 for example. Don't find answer for alphat for fine grids, so I keep at wall for alphat



fluid_to_solid
{
type compressible::alphatWallFunction;
value uniform 0;
}


I succeed to calculate a simple duct with an external solid domain with good agreements with analytical solution for power exchange BUT the case is converging only when I fix the volumic mass of the fluid with rhoConst.

If I use "perfectGas" for rho calculation, I have some trouble close to the outlet of the duct. See pictures












What can I try to improve what happens at the outlet?
Find enclosed my 0/ folder to see my BC


My next question is; if I use rhoConst for the fluid I am dealing with an incompressible case, I see that I have to use "alphatJayatillekeWallFunction" for alphat at walls. And no more the BC "compressible::alphatWallFunction", maybe with fine grids I can avoid alphat wall functions. What should I do ?


Best regards


Julien

[Bloerb]

You do not need to use small values at the wall. the standart k and omega wall functions should suffice. There are some authors that recommend a small value, the boundary conditions do something similiar for small values though. And since your archive is empty i can't tell you what to change about your boundary conditions. Since no backflow should occur on this geometry zeroGradient for every variable should work though. It might help to initialize the flow internal field with a constant value in the streamwise direction.

[julieng]

Hello Bloerb,


Thank you for your advise. Excuse me for the empty file, I update attached BC files.
Please have a look to my BC, I have already test the zeroGradient for U at the outlet but it not solves the bad flow profile close to the outlet.
I agree with you, I do not have any backflow in this case.



"It might help to initialize the flow internal field with a constant value in the streamwise direction"
You mean the potential flow solver for initialize the case? I need to have a look at this. But to my understanding, the problem is not initial condition because the case runs a long time before diverging. See the residual:









If I use rhoConst, what about the alphat BC in theory, do I need to consider the model incompressible and use "alphatJayatillekeWallFunction" on the walls?


The case with rhoConst runs fine with my settings, very close to the analytical solution.




See also the checkMesh analysis:


Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 495446
faces: 1521811
internal faces: 1476689
cells: 513300
faces per cell: 5.84161309
boundary patches: 6
point zones: 0
face zones: 0
cell zones: 2

Overall number of cells of each type:
hexahedra: 432000
prisms: 81300
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
ext_solid 9600 9933 ok (non-closed singly connected)
sym_solid 12000 12642 ok (non-closed singly connected)
in_out_solid 1280 1386 ok (non-closed singly connected)
inlet 1071 986 ok (non-closed singly connected)
sym_fluid 20100 20468 ok (non-closed singly connected)
outlet 1071 986 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.15 -0.15 0) (0.15 0 3)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (-6.5439206e-015 2.81517714e-013 3.77727044e-018) OK.
Max cell openness = 1.70063313e-015 OK.
Max aspect ratio = 98.3970962 OK.
Minimum face area = 9.96138356e-007. Maximum face area = 0.000157107685. Face area magnitudes OK.
Min volume = 9.96138356e-009. Max volume = 8.90825374e-007. Total volume = 0.105858512. Cell volumes OK.
Mesh non-orthogonality Max: 30.343881 average: 1.96163007
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.412643704 OK.
Coupled point location match (average 0) OK.

Mesh OK.

End



Best regards


Julien

[Bloerb]

Your mesh is superb, your boundary conditions are fine. So maybe this is an issue with your schemes. What is the content of fvSchemes for fluid and solid? And what about the inlet/ initial values for turbulence? Are those realistic?

[julieng]

Hello Bloerb,


I try this for initialize turbulence parameter values


- Turbulent intensity:2 or 5% http://www.cfd-online.com/Tools/turbulence.php
- Turbulent lenght scale = 0.0038 x Dh (Dh the hydraulic diameter)
- u' = U0 x Turbulent Intensity (U0: velocity away from wall) [m/s]
- k = 3/2 x u'^2 [m2/s2]
- e = 0.09^(3/4) x k^(3/2) / Turbulence lenght scale
- w = e / (0.09 x k)


To resume the case:
fluid = air @ 300 K
v_air inlet = 2.5 m/s in +z direction
gravity (0 0 -9.81)
inside diameter pipe = 0.2 m
lenght pipe = 3 m
solid is the walls of the pipe outside diameter = 0.3 m
heating of the external solid surface with:
h = 40W/(m2.K)
Ta = 500 K
rho_solid=8000 kg/m3
kappa = 20 W/(m.K)
Cp = 450 J/(kg.K)
Initial temp solid = 500 K
Initial temp fluid = 300 K




My fvSolution and fvScheme are attached


I recompute the case with zeroGradient at the outlet for U and p_rgh
the outlet is still the same...


Best regards

[julieng]

Hi, does someone have seen my fvSolution and fvScheme files? Still stuck with my outlet problem.



Bloerb? Still here?


Best regards


Julien

[Bloerb]

The turbulent length scale in OF is 0.07 x Dh. This is however not the main issue. Your nut value is changing a lot over the length of the pipe. It should however be nearly unchanged. You are hence overestimating the turbulence.

To get better results try the following:

• Use wall functions for k and nut.I'd argue this is good enough. There is a much more pressing issue for hitting the empirical and analytical solutions.
• --> Use flowRateInletVelocity with the extrapolateProfile yes; switch activated. Or use fixedMean instead of fixedValue. Currently your velocity profile is not fully developed at the inlet and this makes getting close to the analytical values more difficult.
• You could solve the pipe without temperature and mapped boundaries for k and omega. Afterwards use the computed values to get the actual turbulence values at the inlet instead of fixedValues at the entire patch. This should increase accuracy but is a bit more difficult. And hence more of an expert tip.
• Your epsilon file should read zeroGradient instead of fixedValue. But since you are using kOmegaSST this is not read.
• You might want to consider slightly relaxing rho for your case of non constant rho
• You could lower k and omega relaxation to 0.3
• You could use GAMG for pressure to speed up the solving process.
• The div(((rho*nuEff)*dev2(T(grad(U))))) term should read Gauss linear;

[julieng]

Hello,


I try your suggestions Bloerb. Modify fvSolution file and initial conditions. But I am not able to reach a good flow profile close to the outlet.


So I use a converged < 10-5 case with rho fluid = constant for initialise my case. See the flow profile of the rho const case:



I change for perfectGas instead of rhoConst in thermodynamical properties file. The case now converge < 10-6 but I have still a strange flow profile close to the outlet with a high velocity






The second problem is that the power exchanged between fluid and solid is divided by 5! Far away from the theoretical solution. Other software give me the right flow profile at the outlet also with compressible fluid.



Please could someone try to resolve my case. I join it.


https://www.4shared.com/zip/OgbWLWHE...ible_duct.html


Best regards



Julien