[balrog_f]

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 (3-5 coeff. loops) and bounded CDS.
The optimal time step seems to be around 3e-06s, 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

[ghorrocks]

Have you done a convergence tolerance sensitivity study? Try a tighter convergence tolerance and see if that helps. Also are you running double precision?

[balrog_f]

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 1e-05 (to fullfill the key data, mentioned in my first post).

I will try a residual target of 1e-06.

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 well-wrought, retrospectively.

[ghorrocks]

In this case the best thing to do is simply run it with 1e-6 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.

[balrog_f]

Thank you very much for your answer Glenn. Does it make sense to change the residual target from 1e-05 to 1e-06 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 .res-file 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 1e-06 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 1.1e-05. 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?

[ghorrocks]

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.

[balrog_f]

Thank you for your help Glenn. I tried the simulation with a residual target of 1E-06 but the solver isn't able to achieve this regarding the continuity equation, no matter how small the timestep is (min. 1E-15). The best it gets is 4.3E-06.
Is there another way to solve the problem mentioned in my first post? What should be my next step if there isn't one?

[ghorrocks]

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.

[balrog_f]

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?

[balrog_f]

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 1E-06). 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 1E-06 -> timestepsize 1E-07s). 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?

[ghorrocks]

this problem can be solved with numerical damping.

That is a bad idea in a LES simulation. LES simulations require a numerical approach which has very low damping/dissipation so it can model the structures inherent in LES. If you add damping you will damp the structures and your LES model will suffer.

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.

[balrog_f]

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?

[ghorrocks]

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.

[balrog_f]

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

[balrog_f]

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?

[ghorrocks]

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.

[balrog_f]

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 1e-06(currently running at 1e-06) again at the point where diffusion starts(somewhere around timestep 50000 i guess)?Trying a better mesh?

[balrog_f]

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 CFX-Solver updates the pressure change to drive the mass flow rate toward the specified value. The update is based on an internally-estimated 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?

[ghorrocks]

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.

[balrog_f]

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 u-velocity (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 u-velocity 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 1e-05. 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 (~1.2e-06s) to achieve convergence in 3-5 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?