[philippose]

Hello,
I have been doing a couple of simulations using simpleFoam with the k-epsilon turbulence model for flow through a hydraulic valve.

Basically, I have the spool open to various (fixed) positions, and I run a steady state simulation at each position. The mesh for the fully open case has around 350,000 cells, and for a case of 1/3 open, I have roughly 300,000 cells.

The medium is oil (nu = 4.6e-5), and I am currently running the simulation with an inlet pressure of 6bar, and outlet of 0bar (delta P = 6bar).

For the fully open case, the simulation gave me a mass flow value within about 1.5l/min of the values I got from experiment, but for the 1/3 open case, I am getting over 6 l/min more from the simulation compared to experiment.

During the simulation (for the 1/3 open case), I noted that even around 2000 iterations, the epsilon values are being "bounded", though the velocity and pressure fields seem to have converged (initial residual around 3e-6).

I was wondering, is this because the Reynolds number around the highest velocity points (around 33m/s), are too high? Is this a case which should be solved using Large Eddy Models? Or should I try another turbulence model? When I do a manual calculation of Re, I get something like 728, but for this particular system, I dont know when the flow goes into the turbulent region.

Any suggestions? Or should I try to burn my laptop with a finer mesh?

I am basically a total newcomer to the field of CFD, and am not yet conversant with the way one chooses between different solvers.

When would one use an LES system, and when would one use a Turbulence model? As far as I read, the LES is another form of turbulence modeling right?

Have a nice day!

Regards,
Philippose

[hjasak]

What you need to do is to adjust your convection and diffusion discretisation (it's probably diffusion that's giving you trouble) to get rid of the unboundedness.

Hrv

[msrinath80]

"When would one use an LES system, and when would one use a Turbulence model? As far as I read, the LES is another form of turbulence modeling right?"

Preface:

LES (a.k.a. Large Eddy Simulation) actually resolves all the large scale eddies in the flow, in that it does NOT "model" them using simplified (mostly empirical) expressions. Of course all eddy scales smaller than the grid size are not resolved, but "modeled" using sub-grid scale models. So for very fine grids, LES is always superior to any turbulence "model" when it comes to resolving the large-scale features of the flow. Of course DNS (a.k.a. Direct Numerical Simulation) is the highest on the ladder of turbulence simulation as it resolves ALL length scales in the flow.

Turbulence models (e.g. k-epsilon, k-omega etc.), in general are just "models" as the name rightly claims. They are usually based on empirically obtained data and typically have very limited scope of applicability. For some very specific cases (and that too almost always single-phase flows), they perform reasonably well. In most practical cases they are inadequate, and for reasonable CFD predictions, one usually resorts to techniques like LES, even if it is computationally more expensive.

So to answer your question, LES is not just another form of turbulence modeling. Yes it does model the small scales; nevertheless, it is still far more accurate than standard turbulence models for a wide variety of flows.

[philippose]

Hello,
Thank you very much for the really quick replies... Thanks a lot Srinath, for that explanation on the differences between LES and Turbulence models. Its something I didnt really find in such simple terms on the Internet.

Hrv, I have been looking up about Convective and Diffusion discretisation, and found an article in the "CFD-Online" Wiki regarding these schemes.

Did you mean the div(phi, epsilon) or the Laplacian discretisation scheme laplacian(DepsilonEff, epsilon) ?

For the div scheme I am using Gauss Upwind Discretisation, and for the laplacian I am using the Gauss Linear Corrected scheme. However, both these schemes dont seem to have any adjustable parameters (assuming this was what you wanted me to adjust). These were the schemes I found in the "PitzDaily" example in the simpleFoam tutorial set.

My relaxation parameters are 0.3 for U, p, k and epsilon.

Could you provide me with a little more guidance in this matter?

I ran the same simulation with a finer mesh.... has done 895 iterations so far... since afternoon... but the boundedness problem still seems to persist.

Thank you!

Philippose

[hjasak]

First, do a checkMesh and tell me how badly non-orthogonal your mesh is. The scheme you should adjust is laplacian(DepsilonEff, epsilon) (and probably k as well). You can start with

Gauss linear limited 0.5;

and then increase the factor towards 1, depending on how bad the mesh is. The other thing that may hevlp you (it should not, but it may), is to tighten the tolerance on the pressure solution to get better fluxes. Also, please check your outlet boundaries for flow intrainment - this may cause you trouble as well.

Enjoy,

Hrv

[philippose]

Hello again Hrv,
Thanks once again for coming to the rescue :-) A Good evening to you!

I did a checkMesh, and here is a summary of the relevant results from the mesh:

----- begin -------

Number of points: 66903
edges: 411334
faces: 664835
internal faces: 616841
cells: 320419
boundary patches: 7
point zones: 0
face zones: 0
cell zones: 0

Number of non-orthogonality errors: 0.
Number of severely non-orthogonal faces: 130.
Mesh non-orthogonality Max: 89.4 average: 15.5699
Non-orthogonality check OK.

--> FOAM Warning : From function primitiveMesh::checkFaceSkewness(const bool report, labelHashSet* setPtr) const
in file meshes/primitiveMesh/primitiveMeshCheck.C at line 838 Large face skewness detected. Max skewness = 3324.49 percent.
This may impair the quality of the result.
83 highly skew faces detected.
Writing 83 skew faces to set skewFaces

------ end ------

The severe skewness warnings are warnings that I got also with the initial mesh (fully open case), though the results were accurate to around 1.5 l/min (after 2500 iterations).

All my meshes are created by importing STL files from Pro-E into Netgen, and writing the mesh in Netgen neutral format, with subsequent conversion using netgenToFoam.

I have one outlet patch, and I did not see any hint of flow intrainment at this patch... the flow direction throughout the patch is consistent.

Today I created a new mesh with a longer path from the flow critical regions to the final outlet patch.... Maybe this distance was too small and hindering the convergence of flow. Need to check it out.

Could you tell me how one chooses the best discretisation scheme for a given scenario? In the article in "CFD-Online" regarding diffusion discretisation, I found an approach which switched between the upwind and the centre-differencing approaches, with a factor which determined how smooth the transition is, at regions with high non-orthogonality.

Is there a general source of information for the various dicretisation schemes, and the advantages and disadvantages of each?

I shall try the adjustments you have suggested with the original mesh before putting in the new mesh.

Thank you for all the assistance, and have a nice day!

Philippose

[hjasak]

Mesh non-orthogonality Max: 89.4 degrees

Need I say more? You need a better mesh :-) As for the bounded laplacian schemes, this is nothing to do with upwinding, I simply limit the non-orthogonal correction in a consistent manner.

The "best" reference I can give you to OpenFOAM discretisation is my Thesis (1996, sigh) but it doesn't have the new stuff, including bounded discretisation of Laplace terms. I am hoping to include this into my CFD lecture notes and we may speak about it in some future OpenFOAM Workshops.

Enjoy,

Hrv

[philippose]

Hi Hrv,
Yet again :-) Thanks for the guidance... shall look into means of reducing the mesh non-orthogonality... I guess I need to do a lot more reading up on the various terms used in CFD :-) Didnt see any direct means of correcting non-orthogonality in NetGen.

I got hold of your thesis a few minutes back... are your CFD Lecture notes available on the Internet too ?

I downloaded the CFD lecture notes from the Aerospace institute of my University (RWTH-Aachen, Germany). www.aia.rwth-aachen.de (in case you are interested).

Anyway, so that will keep me quiet for sometime :-) I guess you wont be hearing from me for a...hmm... few days atleast :-)!

Enjoy your day!

Philippose

[ep4]

Hi,

after some tries, i still keep bounding errors for k and epsilon. I'm considering a heated flat plate. I use buoyantFoam and the k-epsilon turbulence model. I have tried fine and coarse mesh, respectively with y+ values smaller and bigger than 1.

In the system/fvSchemes file, for the laplacian term, i have tried to use Gauss linear corrected, limited 0.5 and uncorrected. In each case, i have bounding errors and the simulation stops after many time steps.

When trying to use the "bounded" scheme, it answers me that it doesn't know this scheme... I don't know why it can not found it.

I don't understand why i keep such errors while using the uncorrected scheme which is bounded.

Does anyone could help me?

Thank you

Eric