CFD Online Discussion Forums - New implemented EASM (NASA EASMko2003)

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - New implemented EASM (NASA EASMko2003) (https://www.cfd-online.com/Forums/openfoam/106701-new-implemented-easm-nasa-easmko2003.html)

New implemented EASM (NASA EASMko2003)

Hello everyone

I have implemented an incompressible version of the explicit algebraic Reynolds Stress model EASMko2003 which has been developed by C. Rumsey and T. Gatski at NASA.
Validation is currently in progress. The results are not very good yet. Especially the convergence is not good in some cases. In the attachments you find some examples of validation results for the turbulent flat plate (exp. by Wieghardt, reference http://www.grc.nasa.gov/WWW/wind/val...rb/fpturb.html) and the backward-facing step (which you find here http://openfoamwiki.net/index.php/Ma...bulentBackstep)

You can try the model yourself and play around with it. I'd be happy if you shared some of your experiences here. Please check the code before you use it - it may still have errors that I oversaw. Quite well-tested components are the solving algorithm for the cube root; rather uncertain parts are divDevReff(), devReff() and the equation for Rturb_.

Current problems are

great sensitivity to boundary conditions
sharp gradients in the flow field which may occur due to sharp gradients in the parameter C_mu_star which appears in the expression for the eddy viscosity. This parameter is found by solving a cubic equation which may degenerate and exposes some problematic behavior under certain circumstances.

Have fun,
Johannes

Dear Foamers,

I recently completed the work on the model. There was a wrong sign in a rather critical position (in divDevReff()) and the wall boundary conditions for the turbulent backstep were somewhat tricky to choose. Bottom line: there are new validation results that look much better than the old ones, especially for the backstep case. Those weird sharp edges in the velocity profile have disappeared. Below you find the current results and the new code. However, please perform a proper validation yourself before using the model.

Johannes

1) There might be a sign error in cmustar; 2) Convergence seems to be slower than the SST model.

Dear Daniel,

thanks for testing the model. Could you please elaborate on your first point as to where the wrong sign might be? I have indeed checked the sign for C_mu_star many times, however it is possible that there is still something wrong. In the NASA sources, there is a pitfall. I found two sources with different signs, however the different signs canceled out by changing the sign of the RST at the same time.

I also observed that the convergence is normally slower than the SST model. However I came across a case where it beat standard kOmega on a coarse mesh and even led to better results. The test case was a backward-facing step.

Regards
Johannes

Hi Johannes,

Quote:

In the NASA sources, there is a pitfall

Really? Did you mean here,

Code:

            CmuStar_[index] =

                (

                    (gamma1Star_ * a1_)

                  / (

                        Foam::sqr(gamma1Star_)

                      - 2.0 * WSqr_[index] * tauSqr_[index] * Foam::sqr(a2_)

                    )

                ).value();

Where you put

Code:

            CmuStar_[index] =

                (

                    (gamma1Star_ * a1_)

                  / (

                        Foam::sqr(gamma1Star_)

                      + 2.0 * WSqr_[index] * tauSqr_[index] * Foam::sqr(a2_)

                    )

                ).value();

I just did a channel flow simulation, so far so good. As soon as I came to another verification case, it blows up quickly. I am still looking into it.

And also, have you ever yourself tested the channel case, I found that different from the SST model, it seems either your code or the EASM model gives an early defect layer in High Re. Can you verify this? Thanks a lot.

http://flic.kr/p/dZzZxD

Hi Daniel,

sorry that I let you wait so long but I've been quite busy recently.

No I have not tested the channel case. I only ran the turbulent flat plate and the backward-facing step. The original plan was to do a 3D validation of a pipe bend as well but we didn't have enough time to do so.

Concerning your question about the wrong sign I must admit that I cannot readily justify why I put it this way. I remember spending a lot of time with these few lines of code, comparing them against other solution methods. I also changed signs back and forth between different part of the code (like minus here, cancels with the minus there). Since the sign appears in a product of squares, this is probably not the source of difference here.
Therefore it might well be that you discovered a real error. With which sign did you run the channel validation case? Did you notice any differences?

The line of code you recited is to solve the cubic equation at the point when it it comes close to degenerating into a linear equation. Therefore the most important requirement is that the solution be continuous along that point. The resulting value of C_mu_star should be somewhere close to 0.18 if I recall it correctly. If the continuity is violated it might be a source of divergence.

Thanks for testing
Johannes