
[Sponsors] 
April 7, 2017, 04:38 
LES periodic boundary conditions

#1 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Hi,
as this is my first post/thread on the forum i hope i did everything like it is recommended in the guidelines. So please tell me if I did something wrong I'm doing a LES (wale model) to simulate the flow over a dimpled surface. For this, I use translational boundary conditions (pressure change). The simulation is initialized with a RANS solution and I'm using adaptive time stepping (35 coeff. loops) and bounded CDS. The optimal time step seems to be around 3e06s, which leads to a max. CFL number of 0.5. The simulation converges very well but for some reason, the pressure monitored at the fictional "outlet" starts to diverge after around 35000 timesteps and the oscillation starts to increase more and more. I have no idea why. What could be the reason for this behaviour? key data:  ~ 11 million nodes (structured hex)  y+ < 1,3 (mostly <1)  max. aspect ratio = 10.5  one flow through time with RANS initial velocity =~ 0.02s  Re =~ 12000  RANS velocity field is perturbated with the in CFX integrated velocity perturbation for LES (expert parameter : fluctuation for LES)  second order backward euler is used as transienst scheme 

April 7, 2017, 08:04 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
Have you done a convergence tolerance sensitivity study? Try a tighter convergence tolerance and see if that helps. Also are you running double precision?


April 7, 2017, 10:15 

#3 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Thanks for your quick answer Glenn. Yes, the simulation is running on double precision. I didn't do a convergence tolerance sensitivity study, yet. What is the best/fastest way this can be done, regarding a LES?
My actual Residual Target is 1e05 (to fullfill the key data, mentioned in my first post). I will try a residual target of 1e06. I tried this already because it is a geometrically sensitive problem, but with adaptive timestepping regarding CFL=1 and this doesn't work out quite well. Convergence couldn't be achieved anymore after a frew thousand timesteps. So i thought it will be the same for the adaptive timestepping regarding number of coeff. loops. This wasn't wellwrought, retrospectively. 

April 8, 2017, 08:43 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
In this case the best thing to do is simply run it with 1e6 residual target and see if makes a difference to the divergence at 35000 timesteps. Note that with a tighter convergence tolerance it will automatically make the time steps smaller, so you will have to run more iterations to get to the same physical time.


April 8, 2017, 09:55 

#5 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Thank you very much for your answer Glenn. Does it make sense to change the residual target from 1e05 to 1e06 just right before (regarding total simulation time) the divergence can be observed, just to save time or has it to be set right on from the beginning of the simulation? This can be done because i simulate about 10k of timesteps > look at the solution, if it is okay i will use the .resfile as an initial file for the next 10k of timesteps. With this approach i try to make sure not to "waste" time.
Another question which comes up to my mind regarding the smaller timesptes for a residual target of 1e06 is, sometimes when the solver choosed the timestep to big the timestep doesn't converge at all no matter how many iterations are made, it is stucked at a specific residual value let's say at 1.1e05. I know that in CFX every timestep has to converge but how can I avoid the mentioned behaviour? Has it really such a bad effect on the solution? 

April 9, 2017, 08:07 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
Yes, you can use the normal time steps to get close to the point in question and then change to a tighter convergence criteria.
And yes, adaptive time stepping sometimes does this. You can minimise it by careful adjustment of the adaptive time stepping parameters, such as slowing down the increasing time step size or putting a maximum time step size on. 

April 13, 2017, 10:45 

#7 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Thank you for your help Glenn. I tried the simulation with a residual target of 1E06 but the solver isn't able to achieve this regarding the continuity equation, no matter how small the timestep is (min. 1E15). The best it gets is 4.3E06.
Is there another way to solve the problem mentioned in my first post? What should be my next step if there isn't one? 

April 13, 2017, 20:03 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
The problem is either physical (ie something happens at the time it crashes, such as a shock wave reaches a boundary) or numerical (ie inadequate convergence or numerical errors).
If it is physical then you will need to look at the results to figure that out. If it is numerical then there are standard things to do: * Double precision numerics * Improve mesh quality * Smaller time step * tighter convergence * Better initial condition "Improve mesh quality" is a critical one which is often overlooked. EVERYTHING becomes easier when the mesh quality improves. 

April 21, 2017, 06:25 

#9 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Thank you very much for your answer, Glenn. So I checked it and it must be a numerical error. I read some theory about numerical errors and this problem can be solved with numerical damping. Is there a possibility to do this in ANSYS CFX because this is a very complex topic and it would take a lot of time, I think, to find the correct damping function which doesn't distort the solution on the one hand, but damps out the numerical errors on the other hand?


April 24, 2017, 08:42 

#10 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Maybe a picture of the monitored pressure averaged over the "outlet" and "inlet" helps you to understand my problem. I tried to provide better initial conditions with an URANS solution (with this I achieved the tighter convergence criteria of 1E06). But it shows almost the same behaviour as the initialization with RANS, except that the oscillations are not totally diverging (run with double precision, residual target 1E06 > timestepsize 1E07s). Is it worth letting it run for some more time?
monitored pressure.png Another thing you already mentioned is the mesh. I am using a structured hex mesh trying to achieve the best quality i get. So the min orthogonal quality is 0.82 and the max 0.99 (average 0.97). Isn't this already a quiet good mesh quality? BUT the thing I forgot to mention is that my growth rate is 1.06. Could this be a problem? Last edited by balrog_f; April 24, 2017 at 11:58. 

April 24, 2017, 19:25 

#11  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
Quote:
What boundary conditions are you using for this model? Have you read the section in the CFX documentation on selecting boundary conditions? I suspect you have selected numerically unstable boundary conditions. Mesh quality  even if the mesh is pretty good, things will be easier if it is even better. I would recommend making a mesh with significantly better (or worse) mesh quality and see what difference it results in. Then you can see how sensitive you are to mesh quality. 

April 25, 2017, 04:25 

#12 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Thank you very much for your reply Glenn. I am using translational periodic boundary condition in streamwise direction with pressure change as interface model. But I dont know the pressure drop from the beginning on, just the velocity. Thats why the pressure change is given over an expression which reads out the pressure drop and consistently corrects it during the run based on the given velocity.
So maybe massflow rate as an interface model would be a better idea? 

April 25, 2017, 20:52 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
The approach you describe has no underrelaxation or other numerical stabilisation methods. It is unlikely to converge nicely.
So use the built in mass flow rate option as that has the numerical stability stuff already in there. 

April 28, 2017, 05:11 

#14 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Thank you so much for your help Glenn. I tried it and it looks good at the moment. I will give you a feedback as soon as I have final results


April 28, 2017, 05:32 

#15 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
I have one more question. Is it necessary to initialize my LES with a RANS/URANS solution which are also computed with the massflow boundary conditions or can I use the already existing solutions with the pressure change boundary condition (converged pretty good) as initialization file, just to save time? Does this affect the solution?


April 28, 2017, 08:56 

#16 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
The closer your initial condition is to the result you are looking for, the quicker and easier it will converge. If the difference between the pressure driven flow and the mass flow rate driven flow is small then it will make little difference.


May 12, 2017, 06:30 

#17 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Hi Guys,
my LES was running for a while now with the MassFlowRate interface model and it looks very good. Massflowrate is set over an expressions which looks like this: MassFlow=Ubulk*rho*area()@PerLength Side 1 rho = 1.185 [kg m^3] But now the same behaviour occurs as mentioned in my first post in this thread (compare screens below). I don't know why, this really makes no sense for me. I can't magine what is happening? If anybody has an idea why the simualtion behaves like that and how i can solve this problem, i would be very thankful because I don't know how i can fix it. Even an explanation what is happening would be very helpful. Mabye solve it with a "handwritten" damping function, but this would damp out some structures i want to obtain, right? Should i try it with a convergence criteria of 1e06(currently running at 1e06) again at the point where diffusion starts(somewhere around timestep 50000 i guess)?Trying a better mesh? 

May 12, 2017, 06:46 

#18 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Another point could be the pressure update multiplier at the additional interface model tab. I found this in the CFX documentation about it:
"13.1.2.1.1.2.1. Pressure Update Multiplier Enter a numerical quantity or CEL expression that specifies the pressure update multiplier. When imposing a mass flow rate at a domain interface, the CFXSolver updates the pressure change to drive the mass flow rate toward the specified value. The update is based on an internallyestimated coefficient, which may not be optimal. The Pressure Update Multiplier provides user control to tune convergence behavior. The default value is 0.25. If convergence is slow (as may occur for low Reynolds number flows), consider increasing the value. If convergence is unstable, consider decreasing the value. Note that values above 1 are permissible." So the obtained behaviour looks unstable, right? So maybe decreasing the value would help? But I don't know how sensitive it is. Anybody has an idea or experience with it? 

May 12, 2017, 08:15 

#19 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 
Your simulation seems to run fine up to 50k time steps. I see the mass flow rate is still increasing. Is it heading towards a pseudo steady state? Are you sure you need timesteps this fine? Is your convergence tolerance too tight?
I am guessing here, but I suspect when the flow rate reached some threshold it looses numerical stability and diverged. I would have a look at the flow and see if you can identify something which could trigger instability. It may or may not be physical. I would not add global damping. This is a bad idea in LES. Any damping function will need to be specifically targetted to the region of instability, so it does not damp out the turbulence structures. 

May 12, 2017, 08:46 

#20 
Member
Join Date: Apr 2017
Posts: 53
Rep Power: 9 
Hi Glenn, thank you for your answer. Why should the mass flow rate increase? Where can you see that? The mass flow rate is or should be my constant value. The local uvelocity (not areaaveraged) is heading upon a pseudo steady state, i guess. This is a good thing I think because I can only start evaluating my LES when all values of interest (especially the velocity components) have reached a pseudo steady state . So the behaviour of the uvelocity until timestep 50k is exactly what i want/need for my LES, right? I need to reach a pseudo steady state. My convergence tolerance is 1e05. Do you think this is to tight? I am not sure whether I need timesteps this fine but the solver homed in on this fine timestep (~1.2e06s) to achieve convergence in 35 iterations in every timestep. What for example can trigger instability? For What and where should I look at the flow? So would you say damping in general is a bad idea for LES?


Tags 
les, les simulation result, les wale, periodic boundary 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Radiation in semitransparent media with surfacetosurface model?  mpeppels  CFX  11  August 22, 2019 08:30 
Translational Periodic Boundary Conditions  HeatTransferFan  CFX  19  December 12, 2016 12:15 
Basic NozzleExpander Design  karmavatar  CFX  20  March 20, 2016 09:44 
Radiation interface  hinca  CFX  15  January 26, 2014 18:11 
An error has occurred in cfx5solve:  volo87  CFX  5  June 14, 2013 18:44 