CFD Online Discussion Forums

CFD Online Discussion Forums (
-   Phoenics (
-   -   how to use k-omega low reynolds number in phoenics? (

wilcox May 2, 2015 06:46

how to use k-omega low reynolds number in phoenics?
Hello everyone,
I am new to this forum. I need help with Phoenics software. I was using k-omega model in Phoenics and got very good results for jet-flow through circular orifice at Reynolds number 10^5 and comparison with journals was also perfect. But when I started using 10^4 Reynolds the result started having little discripancies with journal data. Moreover, when I tried to use k-omega low Reynolds model for 3600 reynolds it doesn't work at all. No matter how good the mesh is the solver shows NaN for all the values without any error message and keeps on running :confused:. Please Help. Even if any can tell me how get k-omega low re library file or tutorial it will be a great help.

CHAM Support February 4, 2020 13:10


Presumably the case considered is flow through an orifice plate in a circular plate. It’s not made clear what quantities are being used for assessing the performance of the high-Reynolds-number model, but the computed pressure drop through the orifice is known to be sensitive to the mesh density in the region of the vena contracta. Lowering the flow Reynolds number may result in a deterioration of agreement with the measured data; and in any event, for both Reynolds numbers, the sensitivity of the model results to mesh size and distribution should be assessed systematically. When doing this, care should be taken to ensure good numerical resolution in those regions where flow properties vary rapidly, such as for example, in the vicinity of the vena contracta. Care should also be taken that the wall functions are not invalidated in the approach flow by allowing the near-wall mesh node to be located too close to the wall by allowing y+ to be much less than 30 when not using scalable wall functions.

Reverting to a low-Reynolds-number closure increases the complexity of the CFD model, because now wall functions are dispensed with, and the flow field needs to be meshed into the laminar sublayer and down to the wall. Consequently, the mesh will need a high concentration of grid cells near the wall, with the wall-adjacent node positioned at y+=1.0 or less, and at least five cells need to be located in the laminar sublayer. The use of such high mesh densities and the more complex turbulence modelling can lead to convergence issues, if not handled carefully; and I suspect that this why the simulation has diverged. The use of the double-precision CFD solver is recommended when using low-Reynolds two-equation models, and usually the relaxation needs to be heavier than when using the equivalent high-Reynolds-number closure.

The various alternative forms of the low-Re k-w turbulence model can be found under: main menu, models, turbulence models, low-re kw variants - see also

As may be evident from the above discussion, things to check are the Y+ values (YPLS) near the wall in the solution file (this can be activated under the main menu, output, derived variables, Yplus). If these are not within the correct range the wall function will be invalid and the turbulence model will not give you correct results. This could happen if the near-wall grid is too coarse or too fine, depending on your setup. You can find more information in this tutorial here:

Good library cases on this subject are N110 (pipe with orifice plate) and T213 (pipe expansion).


All times are GMT -4. The time now is 15:28.