Transient solution not oscillating
 

Hello,

I searched the forum but didn't find something so i do my first post:):

I have a Problem with my transient Solution for which I expect the Forces to oscillate. If I use a converged steady-state solution as initial condition for the transient run, no oscillation apears. If I start on the other hand directly with the transient Run the forces oscillate but with no sufficient convergence. (Convergence of the oscillation of course)

The advection scheme is HighRes and the time discretization is 2nd order. Turbulence is still 1st order and i have smal time steps.

My Question: Is it the right way to start such a transient run with a converged steady-state solution? Or should i start with a transient 1st-order solution?

I appreciate your advice.

Paul

Is this an FSI simulation or is the geometry fixed? What is the geometry?

To get oscillations you need high order numerics and good convergence. Can you attach your CCL file?

If the oscillation is real then any realistic initial condition should end up oscillating.

Sorry, cant post any files now.No FSI but i plan to do it later on.Geometry is a parabolic trough solar collector in 2d near the ground. In addition i have a logarithmic wind profile as initial condition. Reynolds Number is about 4e6. Using SST model but only 1st order numerics for turbulence. I try running with highres then. I think in ansys docu i read that advection and time always need to be 2nd order (or highres) but turbulence can remain at 1st in most cases. I will also try blend-factor=1 for high order numerics then.

Im still not sure about the starting solution. Should i start with an converged steady-state solution with highres schemes or with a transient 1st order solution. Or start directly with transient high order numerics? And does my starting solution only have influence on the time until im converged or can it change the character of the flow?

Thanks for your help and have a nice weekend:)

Paul

The whole idea of turbulence models is they average out the turbulent fluctuations and leave a steady state bulk flow. This may be what is stopping the oscillations.

What oscillates anyway? The air flow around the collector? In this case you will probably need a SAS, DES or LES approach to get something realistic.

Yes, the air flow around the collector should be oscillating and therefore the pressures and forces. Wind tunnel results are conform with that. The strange thing is that at some angles i have the osscilation but at some i don't. Maybe at some critical angles the osscillating is so strong that the RANS approch don't can smooth it?

Im not familiar with LES or DES. Do I need special licences to use them?

Thanks again

Paul

Correct. And this is likely to be grid and time step dependant. This is not a good basis for doing accurate simulations.

If the oscillations are what you want then you should use a model designed for that sort of thing. I think the LES/DES/SAS approaches require an advanced turbulence license. Also they are not topics for beginners, if you are not already proficient in CFD then I would recommend you get some experience with standard CFD models before progressing to them. At the very least read up about them from turbulence textbooks like "Turbulence Modelling for CFD" by Wilcox - then you will have a good idea about the complexity of these models.

Ok. Thank you for your help. I think i will use the time average results then.

SAS SST model
 

Hello again,

I'm currently trying the SAS-SST model for turbulence now. I hope to get a "LES-like behavior" of the oscillating flow with less complexity and effort:). Therefore i still want to use my two-dimensional grid (with only one element in the depth). My question is: Is it acceptable to do a Scale-Adaptive-Simulation with such a 2d grid. The examples i found were all 3d and I know that turbulence is a three-dimensional problem, but maybe it's still possible to get good qualitative results?

Thanks again

Paul

I have performed LES simulations on Aerofoils in the past. I was advised to use a 3D grid with depth 10% of the characteristic length (chord of the aerofoil) and to use delx=dely=delz (cells with equal dimensions in all three dimensions) to take into account of isentropic turbulence.

I do recommend 10-12% in 3rd dimension. Try DES instead with option like 1)simple DES 2)DDES and 3)IDDES

Absolutely not. You will gt rubbish. You need a 3D mesh, or at least a mesh with enough depth in z that it can capture a couple of the largest turbulent structures.

All right. Thanks for the comments. I will try that but I'm not sure if I have enough hardware power to simulate in 3d. Maybe I can use a more coarse grid or just compute over christmas:).

Christmas was invented as a gift to CFD engineers to run those really long simulations you never get enough CPU time to run normally. Just make sure the cleaners don't knock the power cord.

Hi Glenn


I have to model standing wave in a thermoacoustic heat exchanger, but for the beginning to make problem as simple as possible I modeled flow between two parallel plate with the air at the iso condition. At the inlet I used opening with velocity signal of u=0.5 sin (2*pi*f*t) (velocity unti-node)and at the outlet I have wall (velocity node). Frequency of signal is f=13 Hz.

One time I consider the length of the domain to be 27 m which is almost equal to the wavelength . The number of elements in the y and z axis is one. So one can assume it as a 1D acoustic model. I monitored dynamic pressure inside the domain it was oscillating sinusoidaly around the mean value of zero . So it was ok.

Attachment 38852

Then I reduce the length to 6.6 (equal to one quarter wave). And again I used unti node in the inlet (opening with the same velocity signal)and node (wall Bc) at the oulet. But this time at the monitoring point I had kind of pressure drift. pressure was not oscillating around zero. so results show kind of mean pressure in the system. while we don’t expect mean pressure . I don’t know what the reason is for this deviation from zero mean pressure? Is that kind of numerical error? i changed the convergence criteria from 1e-6 to 1e-9. but it was still the same.

Attachment 38853

If it is convergence it will be the imbalances which are better convergence criteria then the residuals. So I would recommend activating the imbalances as a convergence criteria. But if you are converging to 1e-9 then it does not sound like convergence.

I suspect your inlet velocity BC is the cause. I suspect the reflected wave is not interacting with the boundary condition in the manner you expect. This means that initially the inlet pushes air into the domain, but when the reflected wave hits the inlet it is not behaving as expected and this leaves you with a residual positive pressure due to the initial flow. Just a guess, but it sounds plausible.

You might need to be more realistic with your inlet boundary. Either use a wall and moving mesh, or expand the inlet out to a far field condition and apply the inlet boundary at a far field.

Thanks for your advice, i agree with you about the possible cause, when i am monitoring the velocity at the inlet (inlet is an opening boundary with u=0.5 sinwt) it is not sinusoidal neither.


but then if i use the moving wall at the inlet i am not sure from acoustic point of view what kind of reflection we will have in the lnlet. when i am using opening with specified velocity it is velocity unti-node and wall is velocity node so it must create one quarter wave length standing wave in the domain. but using the moving wall in the inlet and fixed wall at the outlet, which Independence will create?

Also in the starting of the solver, i have this message

+--------------------------------------------------------------------+
| Reference Pressure Information |
+--------------------------------------------------------------------+

Domain Group: BODY

This is a transient run with at least one compressible fluid
and no boundary pressure set. The pressure level is set
through the transient term in the continuity equation.
To accelerate convergence, the pressure level will also be
shifted dynamically to satisfy global mass conservation.


could it be the cause for creating non- zero mean pressure in the domain?

If you have a non-closed system with a compressible fluid, you are always better off using a pressure (decide if total or static based on boundary condition guidelines) based boundary condition. Otherwise, you may have an ill-posed problem.

The software is warning you about it, and taking some corrective action. I rather be explicit if possible than leaving it to chance.

Thank you for your reply,
well i am not using a pressure based boundary condition, i am giving the velocity in inflow and wall at outlet boundary. however in the basic setting i am giving the reference pressure which is 1 bar.
i don't know how to get rid of this warning. I guess (not sure) that this may be a reason for having a pressure drift when i am monitoring the pressure in the domain.

what if instead of expand the inlet out to a far field condition, i expand the outlet (wall in this case) to the far field, and instead of wall use the outlet condition with zero relative pressure.
the channel originaly has velocity unti-node in inlet and velocity node at the end. if i use the domain which is two times longer and use the outlet instead of wall, it will be velocity unti-node, velocity unti-node at both ends so i suppose in the middle (which is in reality a wall) i get the velocity node as of in the original case.

That should work fine.