non-null velocity at walls despite noSlip condition
 

Hi all!

It's all in the title.

- OF version: v1606+
- solver: simpleFoam
- general problem description: "quick and dirty" laminar flow simulation with stream wise flow periodicity and symmetry BCs on the model boundaries which are not cyclic or walls.

The mesh and other numerical settings might not be optimal, but the simulation runs smoothly and with 20 layers of elements across the domain (10 in the model, x2 due to symmetry BC), I would expect the zero velocity condition at the walls to be enforced without a problem.

I attach here the complete setup, minus the Gmsh-generated mesh file (too big). Also, a screen capture of the velocity at the walls, which will give you a good idea of what the missing mesh looks like.

Basically, the velocity field at the wall in the xy-plane is almost identical to the one on the symmetry plane 10 prism layers away...

Any clue?

Update
 

I've switched the initial condition at the walls from noSlip to fixedValue, and this enforced zero velocity successfully.

Apparently the noSlip condition is new, and is supposed to be equivalent to fixedValue with a value of (0 0 0):
https://github.com/OpenFOAM/OpenFOAM...98d0b13f22b515

Maybe a bug?

Hi, although late, are you able to confirm this? I've been using the noSlip condition for U at my wing wall I'm still getting nonzero values for the surface velocities.

edit: i'm guessing there's something to do with how the data is viewed from paraview as well? I'm unsure about this. Hoping someone could enlighten!

I'm also experiencing non-zero velocities at my noSlip boundaries (when viewed in paraview). Might this be due to the mapping from cells to faces? The velocity in the cell center of the boundary cells is not equal to zero, I guess, and mapping or interpolating this value to the face may lead to non-zero wall velocities. Is there a way to access the face values?

Has anyone found any detailed information on this? I'm also getting non zero velocity at walls with noSlip BC's.

noSlip not zero on wall
 

I can confirm the problem with the noSlip boundary condition on walls. I ran the tutorial airfoil2D and attached the velocity profiles at the wall. y-axis is U_magnitude and x-axis runs from underneath the profile to above. I tested the boundary conditions:


1. type fixedValue;
value uniform (0 0 0);


2. type movingWallVelocity;
value uniform (0 0 0);


3. type noSlip;


the first two are identical, as expected and the third does not reach zero at the wall.


Greetings,
Kraneberger


Attachment 85962

Attachment 85963

Attachment 85964

Hi,


How did you take data and plot ?


With tutorials/simpleFoam/airFoil2D case, velocities at the wall is zero with noSlip condition as shown here,

Attachment 85969


The picture above is obtained only with patch/walls (without internalMesh) using ParaView.

Hi snak,


I obtained the plots via "Plot over Line". What version of OpenFoam did you run the tutorial with. I used v1912.



In the attached picture you can see that I get the same results when only importing walls in paraview.


Attachment 85989


Greetings,
Kraneberger

Hi Kraneberger,

I used OpenFOAM v2106. With v1912, I got the same result as shown here:
Attachment 86000

I used paraFoam command. paraFoam will stat paraview with the OpenFOAM libraries and reader modules.

When I use a native openfoam reader (*.foam), wall velocity is NOT zero as you say.

It will be better to use openfoam utility such as sample to extract data. PlotOverLine interpolates data and not exactly show your result in some case.

Thankyou for taking the time, snak.


I tried it the way you suggested and I can find the zero velocities now. I was confused, because I did the same thing three times in a row. For movingWallVelocity and fixedValue I got identical results and with noSlip the graph changed. The mistake must be on my end and is a post-processing error, not an OpenFoam calculation error ;-)


Greetings,
Kraneberger

Hi Kraneberger,

I found the open issue at VTK site.
https://gitlab.kitware.com/vtk/vtk/-/issues/18085

Using ParaView without a OpenFOAM Plugin (or not using paraFoam) causes this misleading visualization. Using fixedValue instead of noSlip may be convenient for you if you want visualize your results without reconstruction etc.


Added:
The problem with noSlip b.c. wll be fixed after the release of ParaView 5.9.1. There is no problem with the recent nightly built like ParaView-5.9.1-1583-g94277a4...

https://www.paraview.org/download/?version=nightly

I see. Thanks for finding the bug report. I will use a more up to date paraview version from now on :-)