[nskelly]

Hi all,

I am running a RANS (k-omega SST) simulation as a precursor for LES simulation over a backward facing step. When running the RANS simulation I obtain a block profile (using a mapped patch BC).

However, when I change to LES, the block profile becomes parabolic at the step (which is not what I need for my experiment).

I am running using pisoFoam solver with Smagorinsky SGS model. I believe the mesh is fine enough for LES so I am not sure what the problem is. Re = 2000 ( 0.63 m/s) based on outlet height.


Any help/advice would be appreciated.

[mAlletto]

If your profile becomes parabolic that means that you have a laminar flow.

If the Re number in the experiment is the same as in your LES simulation, this is a hint that your numerical dissipation is too high (did you ensure you simulated 2nd Order).

But this is only a guess since your problem description is not very detailed.

[mAlletto]

A just a comment: Re = 2000 is very close to the Reynolds number very the transition from laminar to turbulent flow happens.


By the way how do you define the Re number? based on the channel half width or the width?

[nskelly]

Thanks for responding.

I have attached my fvSchemes, they are all second order (I believe).

You are right that Re =2000 is in the transitional regime. However, simulating Re = 5000, parabolic profile is still evident.

My Reynolds number is based on the inlet height (h) --> Re = 2h*U/v.

[nskelly]

Forgot to attache fvSchemes

[mAlletto]

I do not see any attachments. By the way, very do you get your parabolic profile?

Can you attach some slides of paraview to get a better picture what's happening?

[nskelly]

Velocity profiles for RANS and LES are attached.

[mAlletto]

I guess you show the profile right befor the step. Isn't it?

What kind of boundary conditions did you apply?

So the profile gets laminar. What is the resolution in terms of y+ close to the wall?

Do you know this boundary condition: https://www.openfoam.com/documentati...ty-dfsem.html?

[nskelly]

Sorry this is right at the step - attached are just before the step.

So I have been using mapped patch boundary condition which I hope maps a plane downstream of the step. But I have also been running a simulation with a turbulentInlet BC prescribing some turbulent fluctuations

y+ < 0.5 from what I calculated. Could it possibly be my BC for turbulent viscosity (nut)? I am using zeroGradient on all faces (inlet, outlet, walls).

I have not heard of the DFSEM BC but looks like it might help.

[mAlletto]

Can you also post the 0/U file. In order to unterstand from whitch patch you map the inflow velocity

[nskelly]

I have attached my U file and blockMeshDict

[mAlletto]

Having a quick look at the blockMeshDict i saw that you used only 10 cells in spanwise direction. This are too few for a wall bounded LES. check for the resolution requirement for wall bounded LES of Piomelli. As fare as I remember in spanwise direction you need
a resolution of Delta z+ of 30 to 50 to resolve the streamwise vortices responsible for the mixing between the viscous sublayer and the inertial layer.


Furthermore the offset is also too low. For such a low Re number you need at least 5 channel heights of offset in order that the two point correlation drop to zero. You need to ensure that the flow field on the position of the plane you map from and your inlet plane are uncorrelated.





Best


Michael

[nskelly]

Sorry for the late reply.

Thank you for all the advice.

I will increase the both the number of cells and the refinement in the z direction to resolve the three dimensional vortices.

I was always unsure of the offset of the mapping plane, I will increase to your suggestions.

I will keep you updated.

Thanks again.