Velocity at the wall

[Ionut G]

Hello,

I made a steady state simulation using the k-omega SST turbulence model on an asymmetric diffuser geometry.

I placed monitor points, from y = 0 to the center of the geometry at a given section, and it seems that code saturne is calculating a velocity at the wall too (at y = 0 I have a velocity of 0.008 m/s) even if for the sliding wall I set zero velocity for all the components u,v,w.

Shouldn't be zero velocity at the wall (y = 0)?
Am I doing something wrong?
How can I set zero velocity at y = 0?

I attached the velocity file, listing file and the setup file of the simulation.

I am using Code_Saturne 5.0.9 on Windows 10 64bit

Thank you,
Ionut

[Yvan Fournier]

Hello,

You used a regular wall model for k-omega, which does not enforce a true no-slip condition on the wall, but only a wall friction (so that the mean velocity in the wall-adjacent cell matches that we would have with a more refined mesh and a true no-slip condition, given the expected velocity profile near the wall).
I think you should be able to enforce a true "no-slip" condition by setting "no wall law" in the advanced turbulence model settings, but this assumes you have a fine-enough, "low-Reynolds" mesh, where y+ is near to 1 in the cell adjacent to the mesh (for finer control depending on mesh regions, instead of deactivating the wall law, setting Dirichlet (inlet) value with a velocity matching the sliding wall in low-Reynolds regions an wall laws in other regions could probably work, but I am not sure this is related to your issue, which probably has a simpler explanation:

• Probe values are based on the mean value of the cell containing the probe, and are not interpolated, so it is normal that the velocity does not reach 0.

You could define an interpolation function for probes bt adapting the example in cs_user_postprocess-probes and the cs_interpolate.c sources from the main code repository (where currently only "p0" interpolation is provided), but this is low-level, with no examples yet, and defining an interpolation consistent with the wall modeling would be tricky if you need something more precise, so I would not recommend it, as I doubt it is worth the effort (a mesh sensitivity is probably more usefil if you want to test the model further).

Best regards,

Yvan

[Ionut G]

Hi Yvan, thank you for helping me.

I made another simulation in Code_Saturne using the k-omega SST turbulence model, ensuring that the no wall function it was selected, my mesh y+ is smaller than 1. The mesh generation I made in ICEM CFD.

If I process the results in ParaView the velocity at the wall is different than zero, but If I use Fluent to visualize the results then the velocity at the wall is zero.

Does ParaView can not integrate the variables correctly up to the wall?
Or Code_Saturne does not take into account the no-slip condition on the wall?
Am I doing something wrong?
I attached the listing file and the setup file.

Thank you very much,
Ionut

[Yvan Fournier]

Hello,

Are you visualizing the same results files with ParaView and FLUENT (I assume in EnSight gold or CGNS format) ?
Or different computations on the same mesh ?

In any case, with code_saturne, even with a "no slip" boundary condition, since the solution is cell-centered, what you will see under ParaView is the mean cell value, which should be small if you are wall resolved, but not zero contrary to the wall face value. For scalars, you can activate a visualization of the actual value with a specific boundary-basd field, but for Velocity, we do not have that option yet (I''ll add an entry on the issue tracker to help remind us of this, though I cannot guarantee the priority)

Is the velocity you observe consistent with realistic values at the cell centers along the boundary ?

Regards,

Yvan

[Ionut G]

Hi Yvan,

Are you visualizing the same results files with ParaView and FLUENT (I assume in EnSight gold or CGNS format) ?
Or different computations on the same mesh ?

I managed to run more simulations on different geometries like flat plate and flat channel, but I get the same issue with the velocity near the wall.
The results that I am visualizing are in CGNS format. I open the same results file in both ParaView and FLUENT, the mesh is the same.

Is the velocity you observe consistent with realistic values at the cell centers along the boundary ?

The dimensionless velocity, U+, computed with Code_Saturne follows the experimental data, but there is a shift in the values from Code_Saturne.
The dimensionless velocity, U+, was calculated using the wall shear stress extracted from Code_Saturne.

Do you know why the velocity is shifted upwards at every location, like in the above image?
I understood that near the wall, at the first point from the image above, Code_Saturne will compute a mean value, but after that the values shouldn't be closer to the experiment?


Thank you,

Ionut