[raunakjung]

Hello everyone. Please help me in the following:

I am carrying out LES simulations in LES.

Simulations are initialized by using steady state solutions. I am using Hexahedral mesh. Mesh size is on the turbulent length scale, Courant number is 0.5-1. The Central scheme is used for advection scheme and second order backward Euler is used for the transient scheme.

Velocity inlet condition and static pressure outlet were used. Simulations are adiabatic and in the incompressible region.


I am getting unrealistic values when comparing simulation results with experimental results.

What could be done for the following situation?

1. Should I use different advection scheme?
2. Should I initialize my simulation in a different way ? What is the role of velocity fluctuation?

Thank You

[ghorrocks]

There are so many things which could be wrong.... FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Please show an image of what you are modelling, your mesh, your output file (or at least an section of it), the results you are getting and the result you expect to get.

[raunakjung]

Originally Posted by ghorrocks

There are so many things which could be wrong.... FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Please show an image of what you are modelling, your mesh, your output file (or at least an section of it), the results you are getting and the result you expect to get.

I am carrying out simulation of a fluidic oscillator . I am using hexahedral mesh. Meshing quality by 3*3*3 determinant is 0.95-1.00 = 100% and equivalence skewness is min 0.334

[raunakjung]

Originally Posted by ghorrocks

There are so many things which could be wrong.... FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Please show an image of what you are modelling, your mesh, your output file (or at least an section of it), the results you are getting and the result you expect to get.

Also when comparing the results with RANS simulations which is close to experimental results the LES results are very unrealistic.

[ghorrocks]

Have you checked your turbulence dissipation spectrum? Checked the sub grid model is around the correct levels of dissipation? Have you checked your mesh size is properly matched with the LES length scale?

Also I see oscillations in the LES simulation. There is something wrong there.

the LES results are very unrealistic

Are you comparing time averaged LES results or instantaneous LES results? You need to do time averaging to see the mean flow field.

[raunakjung]

Originally Posted by ghorrocks

Have you checked your turbulence dissipation spectrum? Checked the sub grid model is around the correct levels of dissipation? Have you checked your mesh size is properly matched with the LES length scale?

Also I see oscillations in the LES simulation. There is something wrong there.



Are you comparing time averaged LES results or instantaneous LES results? You need to do time averaging to see the mean flow field.

I used previous RANS simulations to calculate the integral length scale.after finding the turbulent length scale I put atleast 5 cells across it to resolve 80% of TKE.

This is a fluidic oscillator. It produces oscillating jet inside the chamber due to coanda effect.

I haven't checked the levels of dissipation .I must admit my research is inadequate. These are not time average LES results. How is time average of mean flow field carried out ?

[ghorrocks]

Your estimate of the mesh element size may be over resolving it. You would have to check by looking at the turbulence spectrums.

You have to check the turbulence spectrums to do LES. The whole point of LES is to get the turbulence dissipation right, so calculate your turbulence spectrums and check they are OK.

Are you saying the result you showed is a time averaged result? It suggests you have not run it long enough, it is not periodic or your simulations is miles off.

In a periodic flow you have another option for averaging: ensemble averaging. Then you run several periods and average across the same point in the cycle for each modelled cycle. It is a really nice way of averaging for periodic flows as it side-steps the problem of the averaging time length scale affecting the turbulence time scale.

Another alternative is spatial averaging.

[icornejo]

Hi, I obtained good results in LES simulations using bounded central difference for momentum and second order implicit for time. Even with a CFL about 10. I assume that you checked the grid independency, time step independency and time span (time required to stabilize the time-averaged values). I see that your geometry is a bit complex, all that close angles produce a lot of shear, because the flow tries to follow the wall in impossible angles, that in reality are not perfect corners. Maybe your wall y+ is to high and the LES is not solving the walls appropiately, check it. Also take a look in your sub-grid turbulence viscosity ratio (probanly you are using smagorinsky or similar). It must be low (for example below 1) . If dont, means that your LES is not solving an important portion of the flow.

Regards.

Sent from my SM-T810 using CFD Online Forum mobile app

[raunakjung]

Originally Posted by icornejo

Hi, I obtained good results in LES simulations using bounded central difference for momentum and second order implicit for time. Even with a CFL about 10. I assume that you checked the grid independency, time step independency and time span (time required to stabilize the time-averaged values). I see that your geometry is a bit complex, all that close angles produce a lot of shear, because the flow tries to follow the wall in impossible angles, that in reality are not perfect corners. Maybe your wall y+ is to high and the LES is not solving the walls appropiately, check it. Also take a look in your sub-grid turbulence viscosity ratio (probanly you are using smagorinsky or similar). It must be low (for example below 1) . If dont, means that your LES is not solving an important portion of the flow.

Regards.

Sent from my SM-T810 using CFD Online Forum mobile app

Thank you for your answer. My mesh has 5 cells across the integral length scale which i found using RANS simulations. The LES settings guide said it can resolve 80 % of turbulent kinetic energy. I have used automatic wall functions for the following case. The results were taken after 0.2 seconds with time step of 0.00001 sec. My courant number is 0.5 -1. I initialized my simulation using previous RANS simulations . Is the geometry too complex for it ? Can you say how you initialized your LES simulation ?

[icornejo]

I used different ways to initialize the problem. Honestly, the only difference using a RANS based initial guess is that you sabe running time and avoid some divergence problems. LES predictions, once stabilized, doesnt depend too much on the starting point. You dont have "evident problems" in your mesh or settings. It is still a possibility that your geometry has to many close angles. As you know, LES has problems solving the walls, even more walls with hard angles. Maybe you should look for a simpler known problem to solve and gain confidence about your procedure. Regards.

Sent from my SM-T810 using CFD Online Forum mobile app

[raunakjung]

Originally Posted by icornejo

Hi, I obtained good results in LES simulations using bounded central difference for momentum and second order implicit for time. Even with a CFL about 10. I assume that you checked the grid independency, time step independency and time span (time required to stabilize the time-averaged values). I see that your geometry is a bit complex, all that close angles produce a lot of shear, because the flow tries to follow the wall in impossible angles, that in reality are not perfect corners. Maybe your wall y+ is to high and the LES is not solving the walls appropiately, check it. Also take a look in your sub-grid turbulence viscosity ratio (probanly you are using smagorinsky or similar). It must be low (for example below 1) . If dont, means that your LES is not solving an important portion of the flow.

Regards.

Sent from my SM-T810 using CFD Online Forum mobile app

Thank you for your answer. What is the expected difference when using Central difference scheme and bounded central difference scheme ? Is bounded central difference scheme computationally expensive than central difference scheme ?

Thank you

[icornejo]

CDS is ideal for LES, because produce significantly less numerical diffusion. The problem of the traditional CDS is that can produce unbounded values and non physical oscillations in the flow. It is specially stronger in LES, because of the diffusivity of the turbulence at the sub grid scale. Bounded CDS is a mixing between CDS and UDS that ensures bounded solutions always (which is a very relevant stuff). Some softwares, as Fluent, automatically set to bounded CD the momentum scheme when you set LES to model de flow. Yes, the bounded version is more expensive.

Sent from my SM-T810 using CFD Online Forum mobile app

[raunakjung]

Originally Posted by icornejo

Hi, I obtained good results in LES simulations using bounded central difference for momentum and second order implicit for time. Even with a CFL about 10. I assume that you checked the grid independency, time step independency and time span (time required to stabilize the time-averaged values). I see that your geometry is a bit complex, all that close angles produce a lot of shear, because the flow tries to follow the wall in impossible angles, that in reality are not perfect corners. Maybe your wall y+ is to high and the LES is not solving the walls appropiately, check it. Also take a look in your sub-grid turbulence viscosity ratio (probanly you are using smagorinsky or similar). It must be low (for example below 1) . If dont, means that your LES is not solving an important portion of the flow.

Regards.

Sent from my SM-T810 using CFD Online Forum mobile app

Thank you for your help.I carried out my simulation again my refining mesh and using CDS scheme. When the mean quantities are compared the results are now realistic. Can you provide material to check turbulence viscosity ratio ?