[andras]

Hi Foamers,
I conducted a comparison between OpenFOAM, Fluent and an experiment. The test case is a turbulent, isothermal free-jet (air/air) which was measured using LDA. The on-axis measurements were compared to steady state simulation results of OpenFOAM and Fluent. Further comparisons of other turbulence models and off-axis points will follow.

The computational domain (purely hex-cells):


Plot of velocity magnitude on the axis of the free-jet:

[grtabor]

Very interesting. At first glance it isn't possible to say which code is performing better - is it possible to generate some kind of correlation coefficient between the experimental data and each computation?

What numerics are being used in OpenFOAM and Fluent respectively?

Gavin

[mprinkey]

A grid refinement study may also be in order.

[jmb_jr]

Hi

I wrote an article for a conference here in Brazil that compared all the turbulence models available in Fluent (2D axissymetric steady-state) with experiment results. It was interesting that all the models didn't predicted correctly the self-similarity and a significant discrepancy in all the Reynolds stresses was observed. I think it'd be interesting to show us the comparison of all the Reynolds stresses in the self-similarity condition.

Julio

[andras]

Hi all,
what I can give you for now is a poster presentation (in german language) containing comparisons of turbulence models in Fluent and experimental data which was done by colleagues of mine. Have a look at figure 3 (Abbildung 3) in the top right corner ("Messung" means measurement). Figure 4 shows comparisons of core lengths in multiples of duct diameters.

http://www.cfd.at/download/gvc_freistrahl.pdf

Our simple 2-beam LDA can not measure turbulence intensities reproduceably. That is why we stuck to velocity profiles in the comparisons of experiments and CFD codes.


andras

[JBeilke]

Have you run some transient tests for verification? I would never trust a steady state calculation for this type of flow configuration.

[andras]

Here is a snapshot (at 3.95s) from a transient simulation I have done recently to confirm the result of the steady state simulation presented above. The time step size was 0.001s.

This result is in good agreement with the steady state simulation.

[lourens]

Hi all,

In comparing fluent and FOAM in a very simple, steady calculation, I found a strange difference. My situation is:

2D
inlet with a uniform velocity (5 m/s),
uniform k (1) and
uniform epsilon (0.01).
symmetry boundary on the top.
smooth wall with wall functions on the bottom.
simple k-epsilon model

domain lenght 1000m
domain height 200m

I am not concerned on the wall functions, but on the decay of the turbulence over the length of the domain: in fluent both k and epsilon decay much faster compared with OpenFOAM.

Anyone any idea?

Regards,

Lourens.

[lr103476]

Are you using the same solver settings (discretisation schemes, convergence criteria, time step and turbulence modelling) in both Fluent and OpenFOAM?

Regards, Frank

[lourens]

I am using a steady calculation, changing the time step in OpenFOAM does not make a difference, changing Fluent from linear to second order for all variables does not make any difference, both are using k-epsilon with the same coefficients. Have not yet tried to change discretisation schemes in FOAM. Any idea what discretisation schemes in FOAM should be used for the best comparison?
Length over which turbulence decays differs roughly a factor of 3.

Regards, Lourens.

[lr103476]

Well, the central scheme which is the standard in OpenFOAM is comparable with the second order discretisation in Fluent, but Fluent applies some extra diffusion for stability. At least, that's my experience. You could also try upwind in both solvers, just for comparison.

Frank

[hjasak]

Run checkMesh and see if the size of both domains is the same. Maybe you did not scale the domain properly after mesh conversion.

Hrv

[lourens]

Checked the domain size and both have the same size (domains are equal in paraview too). Did no scaling of the domain after mesh conversion.
I'll have a look if an other discretisation in FOAM makes any difference.

Lourens

[lourens]

Changing schemes in OpenFOAM or Fluent does not make the difference. The reason might be the extra diffusion mentioned by Frank. If I have time I will write down the equations and see if I can get an "decaying turbulence" curve by hand.

In the near future I will have the opportunity to do a comparison between a windtunnel experiment and a CFD calculation. The CFD package used will be Fluent, but I will try to compare the results with an OpenFOAM calculation too. One of the problems in the comparison is that I can't get the nutStandardRoughWallFunction, which seems to be programmes in OF1.4, working, see also
http://www.cfd-online.com/OpenFOAM_D...tml?1189679691

Anyone any idea?

Regards,

Lourens.

[sek]

I've once compared OpenFOAM and FLUENT for turbulent flow over an axisymmetric body at a range of incidence angles. In terms of the forces and moments, the OpenFOAM results using high-order discretizations closely matched the FLUENT results based on similar discretization schemes. The results were presented at this year's workshop, which I believe is posted somehwere.

[paka]

Here it is: http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/WorkshopZagrebJun2007/presentations/s lides/slidesKimZagreb2007.pdf

[oell]

Hi,
I was asked to do some researches about OpenFOAM. So I did some Tutorials pand set up some own cases. My Professor is very satisfacted with the results and would like to see a comparison between OpenFOAM and Fluent or CFX. Therfor I googled a lot and could find a lot of interessting Stuff, but the problem is, that I couldn't find any time comparisons. Has somebody some facts about that? At least for the above mentioned freestream or the in the paper mentioned BOR body?

Regards,

Olli

[yannocean]

Hello, in this post sek describe a benchmark between UNCLE, FLUENT and OPENFOAM. the benchmark is floa past a BOR (Body Of Revolution). I would make the test case with OpenFoam myself for training. So where can I faind some details of the body, the shape?
Regards
Yann

[NewtonKF]

Hi Andras, can you share the LDA data from your experiment??? And, can you tell more about your BCs??? I'm working on a LES code and I'm looking for some data to validate my code...

thanks in advance...

Newton.

[tushar]

Dear Andras;
i am also interested in varifiying the openfoam computation with experimetnal results for the round jet case. can you post here the boundary condtions which you have used for jet. Thanking you.
regards