channel395DFSEM different results
 

Hi,

I'm running the tutorial case channel395DFSEM but what I get is different from the solution reported in: https://www.openfoam.com/documentati...nnel-flow.html

In particular the velocity profile is more or less the same while the Reynolds stress tensor is way much different and also the friction coefficient has nothing to do with the one reported in the Guide.

I'm using OpenFOAM+ 20.06.
Is this a common problem or am I doing something wrong?

Thank you

Hi Chiara,

I'm having the same problem, have you had any progress?

Thanks

Markella

Hi Agavi!

Yes, try to set 3 cells per eddy in U:

inlet
{
type turbulentDFSEMInlet;
delta 2;
nCellPerEddy 3;
mapMethod nearestCell;
value $internalField;
}

Chiara

Hi,

It is a common problem arising from various issues due to the original paper (e.g. the normalisation factor C1 is not dimensionless, or the average length scale term contains a typo - the operator min in Eq. 14 of the paper is actually a max operator etc.). These ambiguities seemed to force the implementation of the method - "interpretative".

Honestly, despite my reviews, I haven't seen any other academic work which could be able to reproduce the results illustrated in the original paper. Yet I have seen various works explicitly stating that the results of the paper could not be reproduced by either using OpenFOAM or CodeSaturne. (No offence to the authors of the work; I am more than happy to be proven incorrect in my obserfvations.)

Therefore, the heuristic solution has been using the nCellPerEddy object, which does not exist in the original paper. The nCellPerEddy is set between 3 to 5.

The issues related to the turbulentDFSEMInlet boundary condition hopefully will be resolved.

Hope these help for now.

It looks like it worked ! thank you both :) :)

Hi,

I'm trying to solve a similar problem, just changing de dimensions of the domain from meters to centimeters.

For that, I set:

1.-scale 0.01 in blockMeshDict,

2.-adjust the timestep in control dict.

3.-scale x0.01 the file points @ constant/boundaryData/inlet/

4.-modify delta to 0.02 at 0/U -> turbulentDFSEMInlet

However the result is a perfectly laminar flow.

Thank you in advance for your help!!

HeleShawMan