
[Sponsors] 
Simulation FPEs  turbulence for transient and steadystate? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
February 21, 2017, 05:57 
Simulation FPEs  turbulence for transient and steadystate?

#1 
New Member
Dave
Join Date: Aug 2016
Posts: 23
Rep Power: 10 
Hi all!
I'm currently running a simulation to model the water flow in a swimming pool. There are two inlets with velocity at ~2.5 m/s, a "skim" outlet (top of the domain) and a "sump" outlet (bottom). Figure 1 illustrates the domain. The aim has been to use this model to learn a range of OpenFOAM (v.4) techniques such as steadystate, transient, turbulent and eventually free surface modelling. Figure 1  Domain I have calculated the flow to be turbulent and I have attempted to simulate with both a ke and kOmegaSST model. The model runs fine in simpleFoam, albeit with a residuals output higher than i'd like (Figure 2). residuals_simpleFoam&kwSST.png Figure 2  residuals for SimpleFOAM (steadystate) & kwSST model (Click to enlarge) From what I saw here, due to the magnitude and relative unsteadiness of the residuals I'm assuming transient modelling is more appropriate for this simulation. I have tried to simulate turbulence in transient using pisoFoam, however this quickly spits out floating point errors. I calculated my turbulence parameters from here, here and here. I initially used a kOmegaSST model based on this article , however since I was having issues I changed to a ke model inline with the cavity tutorial in the OpenFOAM user guide. Considering the list of articles here, from watching the logs I get the impression my epsilon value is destabilising (rapidly diverges to a high negative value) and hence is the reason for the crashes. This seems to be backed up by the fact that my simulation runs fine in transient if I turn the turbulence off in the transportProperties dictionary. Doing this gives me residual values that, to my knowledge, are much more acceptable (Figure 3). As such, I'm assuming my problem lies within the definition of turbulence somewhere and have switched back to a kwSST model as this article suggests it to be better for nozzle flows, which I'm assuming is what my inlets represent. residuals_pisoFoam&laminar.png Figure 3  residuals for pisoFoam (transient) but with turbulence off (laminar flow) (Click to enlarge) I've attached my case if anyone is interested in taking a look at my simulation setup. https://drive.google.com/open?id=0B3...WxTMU1aNDktR0E I think the problem arises from my state of knowledge, however having scoured the internet for a few weeks now I can't seem to find a explanation that sticks, particularly;
Can anyone shed any light on these points/my simulation & understanding in general? Your help would be greatly appreciated! Apologies if my post is a little lengthy  trying to provide all the details! Best regards, Dave 

February 23, 2017, 11:23 

#2 
Senior Member

Hi Dave,
I have had a quick look at your case and the most important thing I can see is the erroneous definition of your patches (see attached pictures). Overall I think the quality of the mesh is very good, but the mesh may be too much refined. For your settings I have seen some errors: First of all, your timestep still gets you slightly above a Courant number of 1 (from the log file), so I guess it would be best to lower it a bit more. Second of all, I would suggest the following modifications to the fvSchemes file: Code:
gradSchemes { default Gauss linear; grad(k) cellLimited Gauss linear 1.0; grad(omega) cellLimited Gauss linear 1.0; grad(epsilon) cellLimited Gauss linear 1.0; } Code:
divSchemes { default none; div(phi,U) Gauss limitedLinearV 1; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,omega) Gauss upwind; div(phi,R) Gauss limitedLinear 1; div(R) Gauss linear; div(phi,nuTilda) Gauss limitedLinear 1; div((nuEff*dev2(T(grad(U))))) Gauss linear; } Code:
nCorrectors 2; nNonOrthogonalCorrectors 1; Code:
"(UkepsilonomegaRnuTilda)" { solver smoothSolver; smoother GaussSeidel; tolerance 1e05; relTol 0; minIter 1; } Regards, Tom 

February 28, 2017, 04:09 

#3 
New Member
Dave
Join Date: Aug 2016
Posts: 23
Rep Power: 10 
Hi Tom,
Thanks for your comprehensive reply! Apologies in the lateness of mine I haven't been very well. Yesterday evening I made the adjustments to my fvSchemes and Solution as suggested and the simulation ran! Perhaps you could explain a little about how you knew to do this? I still find fvSchemes and Solutions are my poorest areas of knowledge with regards to CFD/OpenFOAM and i'm struggling to adjust them too far away from the tutorial cases for my specific runs. With regards to the mesh, my approach was to model the geometry in solidworks with inlets & outlet openings, then "cap" them with individual thin plates to represent my patches. I could then apply boundary conditions to these patches. I think that is why the images are showing a strange overlap? I'm not convinced this is the right way to approach modelling custom geometries as the reason the mesh count is so high is that the features (inlet/outlet patches) are lost without very high resolution in these areas. Could you suggest a better way of approaching this? I'm also a little confused as to how to approach calculating the minimum cell length for use with the Courant number. Currently i've been assuming an aspect ratio of ~1 and taking the cube root of the minimum cell volume as shown in the checkMesh results. i'm not sure this is correct though, as my time step is calculated for Co=0.5 yet my simulation runs at Co = 1.2 like you say. Is there a more efficient approach to this? Currently i'm getting a time step so miniscule that on my machine it would take approximately 18 years to complete! On the transient simulation my Courant number settles to ~0.2 so I guess increasing the time step again could aid this. Many thanks for your help! Best regards, Dave 

February 28, 2017, 11:59 

#4 
Senior Member

Hi Dave,
No problem. Part of the changes come from experience, but some of it is also from knowledge about the finite volume discretisation method and some particular issues with the numerical solution of the NavierStokes equations. A lot of information can be found in "Computational Methods for Fluid Dynamics" by Peric and Ferziger. For the meshing I would assume it may be better to separate the inlets/outlets from the main geometry as diferent STLs and have openings in the main geometry, however I do not use snappy that often, so I am not sure. The high resolution for the patches is indeed necessary, but it is not in the bulk of your domain. So you could use a coarse base mesh and refine up to higher levels near these patches, and perhaps use some refinement boxes near these jets. For the Courant number your approach is reasonable, but there may be some trial and error involved to get the optimal timestep. Good luck, Tom 

March 3, 2017, 06:59 

#5 
New Member
Dave
Join Date: Aug 2016
Posts: 23
Rep Power: 10 
Hi Tom,
Thanks for the reference  I've downloaded the book and i'll be sure to work my way through it. Apologies for the confusion  but the method of meshing you describe is what I did in this case. I'm not sure if it's just a visualisation error rather than anything erroneous about the mesh? I'm going to look at reducing the mesh density and hopefully maintain an acceptable order of magnitude for the residuals, however this seems difficult to achieve at present Thanks for clarifying that about the Courant number, I've never been sure if this method was a reasonable approach. I've modified a couple of other transient simulations using your modified fvSchemes and Solutions and they also run  I can't thank you enough for your help! Best regards, Dave 

March 5, 2017, 15:06 

#6 
Senior Member

Hi Dave,
The errors also pop up in the result of checkMesh, where there are a couple of patches reported with a very low number of faces: Code:
Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology body 1808760 1864011 ok (nonclosed singly connected) inlet1 54 213 ok (nonclosed singly connected) inlet2 35 138 ok (nonclosed singly connected) skim 4 16 ok (nonclosed singly connected) sump 53 219 ok (nonclosed singly connected) Good luck, Tom Last edited by tomf; March 6, 2017 at 03:10. Reason: Input checkmesh part about number of faces 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Setting the height of the stream in the free channel  kevinmccartin  CFX  12  October 13, 2022 21:43 
The difference between steady state and transient  JuPa  CFX  36  December 9, 2019 22:50 
mass flow in is not equal to mass flow out  saii  CFX  12  March 19, 2018 05:21 
Constant velocity of the material  Sas  CFX  15  July 13, 2010 08:56 
Monitor point values in a steady state simulation  Kushagra  CFX  2  July 13, 2008 20:03 