
[Sponsors] 
August 24, 2018, 03:49 
A big issue in turbulence modeling

#1 
New Member
Morteza
Join Date: Jan 2018
Posts: 20
Rep Power: 5 
Dear OF users,
I am using pimpleDyMFoam solver for turbulence modeling of fluid flow around a propeller. I am interested in near wall modeling, so on the propeller surface, y+<1 (~0.1). I use kOmegaSST turbulence model with omegaWallFunction, and fixedValue for k and nut on the propeller surface (~1e8). The problem is that since the mesh has very small cells to resolve the boundary layer, the time step becomes very low, order of 1e10. Therefore, it takes more than a month to get a converged solution and desired output. I know that by changing some settings in the fvSolution file, it is possible to increase the Courant number and fix the time step with a larger value, but this increase is not enough to get dt~1e05. I would appreciate if users who have experience in turbulence modeling on dynamic mesh with y+~0.1 can share their experience with dealing the time step, Courant number and divergence issue. Thanks. 

August 24, 2018, 05:38 

#2  
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 317
Rep Power: 12 
Quote:


August 24, 2018, 05:45 

#3  
New Member
Morteza
Join Date: Jan 2018
Posts: 20
Rep Power: 5 
Quote:
2. Moving is done by using AMI patches, one for the statinary part of mesh and the other one for the rotating part, a cylinder around the propeller 3. I have not. What information can I get by doing so? Thanks for your reply. 

August 24, 2018, 08:37 

#4 
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 317
Rep Power: 12 
1. What do you mean by "near wall" model? All scales of turbulence are modelled in RANS, thus such refining near the wall seems to be counterproductive. Wall functions are needed anyway.
2. Good, how regular is the mesh in the interface region? Edge length ratio of the faces on the opposing sides? 3. Grid quality, mass conservation. 

August 24, 2018, 11:08 

#5 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 654
Rep Power: 11 
I recommend another approach.
Simulate the global flow around the propeller with a normal sized mesh, which can be calculated in a few hours. Use the results of this simulation as a boundary condition for the near wall computation. Probably, you may use a quasi 1d simulation for this. I write quasi 1d, because you need a 3d model for the turbulence happenings. But the model may be simply a cuboid. You don't need to solve all points at the propeller this way, only a cross section of different velocity at the boundary, calculated at the first step. It may even be, that you get a theoretical solution for this. Wall functions are nothing different but a theretical solution or at lest model for this region. Most probably you have to make some more complicated models with more difficult geometry at some regions of interest. Or short: Split the problem!
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

August 24, 2018, 13:56 

#6  
New Member
Morteza
Join Date: Jan 2018
Posts: 20
Rep Power: 5 
Quote:
Here is what potentialFoam gives, where the answer to your second question is included: Quote:


August 24, 2018, 14:46 

#7  
New Member
Morteza
Join Date: Jan 2018
Posts: 20
Rep Power: 5 
Quote:


August 24, 2018, 16:26 

#8  
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 317
Rep Power: 12 
Quote:
1. Conservation error is rather high, nevertheless not terribile. The problem may come from initial/Boundary conditions. If your objective is having a URANS solution, try using implicit time stepping along with a high courant (~2). Also, perform many outer iterations if using pimple. It may be good idea to start the solver with a potential field. It may also be important to calculate the mesh peclet, and courant number, based on the potential field and some reference time scale. 2. For k and omega, independent from grid refinement and y+, you need wall functions. Depending on the particular implementation such wall functions may or may not switch from selfsimilar solutions, to empirical functions fitting some prescribed profile (power law, log law). Menter's komega sst proposes a zero gradient for k and omega at the wall, where the value at the first off the wall centroid is calculated according some formulae. One last thing: are the explanations given the product of some study you've done on the komega sst model implemented in OF? I also work on marine propellers, but have seen that accuracy on integral values (kt, kq) is more dependent on the y+ range along the blades and rudder, than the min/max y+ 

August 24, 2018, 16:34 

#9  
New Member
Morteza
Join Date: Jan 2018
Posts: 20
Rep Power: 5 
Quote:
There is not clear explanation provided by openfoam. My boundary/initial values for this simulation are based on experience of other people with the same y+ and solver shared in this forum. The y+ value I have considered is the average on the propeller surface and I believe the average should show a value which covers boundary layer successfully. 

August 25, 2018, 07:52 

#10  
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 317
Rep Power: 12 
Quote:
Considering the mean as a metric for assesing the regime in which the solution of the boundary layer lies seems, to say the best, faulty. The mean may fall in the buffer region, maybe leading to the wrong conclusion that you might need to refine/decimate the nearwall grid. Maybe the distribution you have is very flat, giving the false impression that your solution may fall into the "twighlight" zone and forcing you to, most likely, refine. Commercial meshing packages (gridgen, CUBIT) allow for plotting the distribution of edge sizes on your mesh/regions of interest in an attempt to optimize things 

August 26, 2018, 03:49 

#11 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 654
Rep Power: 11 
> I think it is a very good idea and will solve the problem, but is it possible to use the results of lets say meshA as initial values for meshB, while the two meshes are different?
Of course. You read the results and make some interpolation of boundary values. All in all, you may have to do some manual work (with the pocket calculator). But it is not a complicated task in closer sense.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

Tags 
pimple, timestep, turbulence, yplus 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Checking if Turbulence modeling is on/off  Jack001  OpenFOAM Programming & Development  6  July 17, 2016 15:39 
Only two turbulence options available in CFX Pre  Jack001  CFX  5  March 30, 2016 02:47 
synthetic turbulence fluctuation in LES Modeling  SEB12129  STARCCM+  1  October 9, 2015 12:18 
Boundary conditions for RAS turbulence modeling  HerrSchein  OpenFOAM PreProcessing  0  August 4, 2015 09:25 
CFDWiki Monthly Focus Area: Turbulence Modeling  Jonas Larsson  Main CFD Forum  0  May 6, 2006 19:08 