CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > Phoenics

how to use k-omega low reynolds number in phoenics?

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Search this Thread Display Modes
Old   May 2, 2015, 06:46
Default how to use k-omega low reynolds number in phoenics?
New Member
Neeraj Mehra
Join Date: May 2015
Posts: 1
Rep Power: 0
wilcox is on a distinguished road
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 . Please Help. Even if any can tell me how get k-omega low re library file or tutorial it will be a great help.
wilcox is offline   Reply With Quote

Old   February 4, 2020, 13:10
New Member
Join Date: Oct 2019
Posts: 11
Rep Power: 6
CHAM Support is on a distinguished road

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).

CHAM Support is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Foam::error::PrintStack almir OpenFOAM Running, Solving & CFD 91 December 21, 2022 05:50
simpleFoam parallel AndrewMortimer OpenFOAM Running, Solving & CFD 12 August 7, 2015 19:45
AMI interDyMFoam for mixer danny123 OpenFOAM Running, Solving & CFD 4 June 19, 2013 05:49
Question about momentum thickness Reynolds number Anna Tian Main CFD Forum 2 March 4, 2013 11:45
Low Reynolds number airfoil. Pablo Cornejo FLUENT 14 October 19, 2005 10:41

All times are GMT -4. The time now is 08:39.