Hello everyone. Would you tell me the difference of k-w model between in CFX11 and in CFX4.2? I am doing a benchmark simulation with k-w model in CFX11, but the results are different from the results simulated in CFX4.2 by other researchers. It shows that the flow seperates earlier in my results. Thanks a lot!

Hi,

The numerics of CFX11 are fundamentally different to CFX4.2. It does not surprise me they are different. Check both solutions are properly grid independant and converged before comparing.

Glenn Horrocks

I did not find any difference between cfx 5.6 and cfx11. Take a look on your bc and ic, besides the mesh!

Thanks for you all reply! I am sure there is no problem in boundary condition since it is a quite simple simulation case( please see the wireframe of the model here: http://imageshack.dk//viewimage.php?...e/20i84866.jpg ) The air is supplied from the inlet located at the left upper part and exhausted from the right bottom part. I set inlet with velocity, k and w; outlet with zero pressure. It is two dimensional simulation. The simulation results I got is quite different from other researchers got before. Because it is a benchmark model, I hope I can also get the similar results. In fact, I have got similar results with k-e model, SST model,but not with k-w model and BSL model. So I am wondering if there is some change of k-w model in CFX11 which is the same with low-Reyonld k-w model provided by Wilcox or Menter?

To Glenn Horrocks: I checked the monitor line and the output file ,it converged completely with residual 10E-6 and P-mass imbalance below 0.001.

Thank you very much!

Best Regards, Li

Hi, Glenn is for sure right about the numerics. But I would be very surprised, if using exactly the same model with different program versions, no matter how old one of them is, one would get worse results. Imagine that one has a well calibrated model, checked against experimental values and, from one software release to another, the results are changed. It would be inacceptable from the software provider. If it were actually the fact, I wouldn't blame the software provider. It would rather indicate that the simulation setup had a hidden mistake, which was not revealed, because of less sophisticated, not so accurate numerics. In your case, maybe you should certify that your model is in all aspects exactly identical to the one in the paper you're reading. Another less probable possibility is that sometimes authors don't reveal all details of their numeric setup or perform slight adjustments in the published results. If available, you could compare your results to experimental data.

I agree with Magnoli that different numerics should not produce different results for the same model setup. Check your boundary condition and model setup, especially, turbulence model. By the way, how is the result reported in that paper compared test data?

Hi Magnoli, thank you very much for your post. I totally agree with you that there might be a hidden mistake, but the problem is that I don't what it is. So simple boundary conditions, so simple geometry model, and the simulation results that I got are in good agreement with experiment data in k-e model.

Maybe there will be someone to say that k-w model has higher requirement for the mesh. I checked the mesh file and result file in CFX-post. The mesh file meet the criteria of parameters in mesh macro and Y plus is around 2.5. If you have any hints for it, please feel freely to tell me. Thank you very much!

Hi longbow, thanks for your post! The simulation results are in good agreement with the experiments with k-e and k-w model, but not with SST model. However, what I got is that the simulation results with k-e model are in good agreement with experiments data, but not with k-w model and SST model. By the way, would you tell me what you mean to check the model setup, especailly the turbulence model? Thanks!

Hi, there is something in this paper that sounds strange. k-e and k-w simulations agree with experiments and SST does not? SST is a blending of k-w and k-e. When both deliver good results, why should SST not? Is there any discussion about it in the paper? Is your mesh identical to the one used in the paper? Are the y+ values the same? Have the authors of the paper used the standard model coefficients? By the way, what are the flow features measured in the experiment? Some people recommend to use y+ around 1 for integration up to the wall, but if you're already with y+ below 3, I wouldn't expect any big difference. Certify that you also have a sufficient number of cells inside the boundary layer.

Hi magnoli, thanks agagin for your interest in this topic. Yeah, I am also confused. There is no discussion about why SST cannot get good agreement with experiments. And I also doubt that the model coefficients are not the same, that is why I asked if there is any difference of k-w model between cfx4.2 and cfx11. But he mentioned that he used low-Reynold k-w model in cfx4.2.

The references I referred are written by 'Jens Christian Bennetsen', 'Numerical Simulation of Turbulent Airflow in Livestock Buildings' PhD thesis, DTU and 'Lars Koellgaard Voigt', 'Comparison of turbulence models for numerical calculation of airflow in an annex 20 room', DTU.Jens didn't simulate it with SST model in cfx4.2 version, but Lars simulate it with k-w model(Wilcox), k-w BSL(Menter) and k-w SST(Menter) with a programmed flow solver.

I am sure the grid is not the same becuase they used structural grid while I used unstructural grid generated in Ansys workbench11. Thanks again.

Best Regards,Li

Hi, If the grid is not the same, you should certify that your grid is not causing the discrepancies. Maybe you can make a grid dependency check, varying the density, number of cells in the boundary layer and proximity of the first grid point to the wall. Something was not clear to me, has one of the authors used a in-house developed code? If that is the case, it is very likely that it was calibrated for his specific problem and the results will probably not match. Have you also checked the inlet turbulent content and the inlet velocity profile?

Hi Magnoli, thanks again! I will take your suggestions to try grid independent simulation. As to the inlet, I used the inlet boundary condition applied by the references as same as the benchmark test recorded(velocity, k and e). If you would like to have a look at the benchmark test, you probably can open this website: http://www.cfd-benchmarks.com/, two-dimensional benchmark test.

Yeah, there is one reference in which he used a code developed personally in the department. I will also try to have a look at the coefficient of k-w model in cfx11 to see if they are the same as those in k-w model(Wilcox). I do appreciate your post.

Best Regards,Li