[K-al-Eps-o]

I am solving an internal flow inside a succession of elbows with openFoam (v2206).

The solver I am using is simpleFoam with a kOmegaSST model.

My BC are fixedValue uniform velocity profile with zeroGradient pressure at inlet and zeroGradient velocity with fixed pressure at outlet.

Walls are of patch type 'wall' with wallfunctions. To take advantage of the symmetry, only half of the domain is modeled and a boundary of type 'symmetryPlane' (I tried to use 'symmetry' and 'slip' boundary conditions that both led to the same problem) is used.

The velocity profiles I get are very strange and I can't explain where this comes from. For some reason, the velocity is 'damped' at the symmetry plane (which is the plane in the middle of the full domain. Both longitudinal and vertical velocity are exhibiting a M (or W) shape velocity profile along the width (X coordinate) of the domain.

Attached are three pictures.

• The first picture shows the computed domain.
• The second picture shows the velocity magnitude on two slices. One cutting the domain in its length and one cutting the domain in its width, perpendicular to the mean flow and located after the third elbow. On this picture only half of the domain is shown, with the symmetry plane on the right side. The velocity profile on this plane is very strange with a damping of the velocity at the symmetry plane.
• The third picture shows the full domain (using the mirror of the half-domain computed) and velocity profiles along the width of the domain at a certain height and along the height of the domain at the middle of the domain. The bottom left graph shows that the velocity profiles are 'damped' at the symmetry plane, an unexpected behavior.

I can't find what is wrong with my simulation.

[Aeronautics El. K.]

Originally Posted by K-al-Eps-o

I am solving an internal flow inside a succession of elbows with openFoam (v2206).

The solver I am using is simpleFoam with a kOmegaSST model.

My BC are fixedValue uniform velocity profile with zeroGradient pressure at inlet and zeroGradient velocity with fixed pressure at outlet.

Walls are of patch type 'wall' with wallfunctions. To take advantage of the symmetry, only half of the domain is modeled and a boundary of type 'symmetryPlane' (I tried to use 'symmetry' and 'slip' boundary conditions that both led to the same problem) is used.

The velocity profiles I get are very strange and I can't explain where this comes from. For some reason, the velocity is 'damped' at the symmetry plane (which is the plane in the middle of the full domain. Both longitudinal and vertical velocity are exhibiting a M (or W) shape velocity profile along the width (X coordinate) of the domain.

Attached are three pictures.

• The first picture shows the computed domain.
• The second picture shows the velocity magnitude on two slices. One cutting the domain in its length and one cutting the domain in its width, perpendicular to the mean flow and located after the third elbow. On this picture only half of the domain is shown, with the symmetry plane on the right side. The velocity profile on this plane is very strange with a damping of the velocity at the symmetry plane.
• The third picture shows the full domain (using the mirror of the half-domain computed) and velocity profiles along the width of the domain at a certain height and along the height of the domain at the middle of the domain. The bottom left graph shows that the velocity profiles are 'damped' at the symmetry plane, an unexpected behavior.

I can't find what is wrong with my simulation.

You said that you have applied a fixed value uniform velocity at the inlet.
Your inlet is not aligned in the global X-Y-Z, it's at an angle. Have you checked that the velocity you have applied is normal to the boundary and not aligned to the global X-Y-Z?

I'm a bit rusty with Of, does it have a flow rate boundary condition? If so, what happens if you try that instead of the velocity?

[K-al-Eps-o]

Originally Posted by Aeronautics El. K.

You said that you have applied a fixed value uniform velocity at the inlet.
Your inlet is not aligned in the global X-Y-Z, it's at an angle. Have you checked that the velocity you have applied is normal to the boundary and not aligned to the global X-Y-Z?

I'm a bit rusty with Of, does it have a flow rate boundary condition? If so, what happens if you try that instead of the velocity?

Dear Lefteris,

Thanks a lot for your reply.

The pictures are misleading, but the geometry is well aligned with the X-Y-Z axis (I doubled checked). The issue might come from something else.

To continue my investigations, I used three different meshes (cf figure below, from left to right):

1. Mesh1: This mesh (which is the same mesh used to generate results of my first post) models only the left half of the domain. The face with the normal in the positive X direction has "symmetryPlane" as a BC while other wall faces have the "noSlip" BC. This mesh has inflation layers on every external face, except inlet and outlet.
2. Mesh2: This mesh models the full domain and doesn't resort to symmetry plane. It has inflation layers on every external face, except inlet and outlet.
3. Mesh3: Same as the Mesh1, this mesh models only the left half of the domain with a symmetry plane ("symmetryPlane" BC) at the face with normal pointing in the positive X. However, the face with the symmetryPlane BC has no inflation layer.

With Mesh2, I wanted to check what was the correct solution, without using symmetryPlane BC. The solution (see figures below) showed a different (more realistic) solution than with Mesh1.
With the mesh3, I wanted to check if the inflation at the symmetry plane was causing issue. It turned out that the solution with no inflation at the symmetry plane gives a result very close to the one modeling the whole domain. I concluded that the inflation was causing trouble. Is this common knowledge ?

Finally, I am a bit confused by the results. I am expecting the flow to detach from the wall at the elbow, but it seems to stay attached. In addition, I was expecting to observe Dean Vortices, as described in the literature. Do you have any guess about what could be wrong ?

Thanks again for your help.

[slaine]

Can you provide the geometry?

[K-al-Eps-o]

Originally Posted by slaine

Can you provide the geometry?

Sure. Here it is attached.

[slaine]

Was the inlet flow rate 50m/s? That is quite a high flow rate.

As a sanity check I have run it in SimScale using incompressible OpenFoam as the solver.

Mesh (1).jpg
Cutting Plane (1).jpg
result (9).jpg
Particle Trace (1).jpg

[K-al-Eps-o]

Originally Posted by slaine

Was the inlet flow rate 50m/s? That is quite a high flow rate.

As a sanity check I have run it in SimScale using incompressible OpenFoam as the solver.

Attachment 93881
Attachment 93880
Attachment 93882
Attachment 93883

Yes, 50m/s. Fluid is air.

Your result is close but a bit different than mine. Did you simulate water or air ?

[slaine]

Originally Posted by K-al-Eps-o

Yes, 50m/s. Fluid is air.

Your result is close but a bit different than mine. Did you simulate water or air ?

OK. I used water. Are you running compressible or incompressible with air?

[slaine]

Originally Posted by slaine

Can you provide the geometry?

The symmetry plane is definitely not working as intended. What does your mesh look like in a cross section? There should not be boundary layers on the symmetry plane:

Symmetry plane mesh.jpg

In my simulation with a symmetry plane the velocity behaves as expected.

Symmetry plane flow view.jpg

Would it be useful to have the OF setup? You can download that directly from the project here.

Downloading a simulation.jpg
File system.png

[K-al-Eps-o]

Originally Posted by slaine

OK. I used water. Are you running compressible or incompressible with air?

Incompressible. Mach number is small enough to consider the flow incompressible.

[slaine]

Originally Posted by K-al-Eps-o

Incompressible. Mach number is small enough to consider the flow incompressible.

OK, rerunning with air at the shared link.

[K-al-Eps-o]

As I was explaining in this post (but for some reason the picture with the mesh is missing), I tried different meshes (that is why you see three different results.

In fact, the mesh with an inflation layer is the one that created the issue.

Here is a picture of the meshes.

Originally Posted by K-al-Eps-o

Dear Lefteris,

Thanks a lot for your reply.

The pictures are misleading, but the geometry is well aligned with the X-Y-Z axis (I doubled checked). The issue might come from something else.

To continue my investigations, I used three different meshes (cf figure below, from left to right):

1. Mesh1: This mesh (which is the same mesh used to generate results of my first post) models only the left half of the domain. The face with the normal in the positive X direction has "symmetryPlane" as a BC while other wall faces have the "noSlip" BC. This mesh has inflation layers on every external face, except inlet and outlet.
2. Mesh2: This mesh models the full domain and doesn't resort to symmetry plane. It has inflation layers on every external face, except inlet and outlet.
3. Mesh3: Same as the Mesh1, this mesh models only the left half of the domain with a symmetry plane ("symmetryPlane" BC) at the face with normal pointing in the positive X. However, the face with the symmetryPlane BC has no inflation layer.

With Mesh2, I wanted to check what was the correct solution, without using symmetryPlane BC. The solution (see figures below) showed a different (more realistic) solution than with Mesh1.
With the mesh3, I wanted to check if the inflation at the symmetry plane was causing issue. It turned out that the solution with no inflation at the symmetry plane gives a result very close to the one modeling the whole domain. I concluded that the inflation was causing trouble. Is this common knowledge ?

Finally, I am a bit confused by the results. I am expecting the flow to detach from the wall at the elbow, but it seems to stay attached. In addition, I was expecting to observe Dean Vortices, as described in the literature. Do you have any guess about what could be wrong ?

Thanks again for your help.

[K-al-Eps-o]

Originally Posted by slaine

There should not be boundary layers on the symmetry plane

In fact, it seems to be the origin of the issue. Do you have an explaination why ?

[K-al-Eps-o]

Originally Posted by slaine

OK, rerunning with air at the shared link.

Thanks a lot. By the way, the geometry I sent you is already the half domain !

[slaine]

Originally Posted by slaine

OK, rerunning with air at the shared link.

See results with air here:

Cutting plane air.jpg

Particle Trace Air.jpg

Areas of high turbulent kinetic energy.jpg

[slaine]

Originally Posted by K-al-Eps-o

In fact, it seems to be the origin of the issue. Do you have an explaination why ?

This is what I suspected. You want the symmetry plane to represent bulk flow as opposed to a wall with a boundary layer. I am not familiar enough with OF local to know what setting you need to change. However, I suspect that the symmetry plane has not been set correctly. It is acting as a wall as opposed to a symmetry plane. Did you assign a wall boundary condition to the symmetry plane? It should be assigned as only symmetry.

[K-al-Eps-o]

Originally Posted by slaine

This is what I suspected. You want the symmetry plane to represent bulk flow as opposed to a wall with a boundary layer. I am not familiar enough with OF local to know what setting you need to change. However, I suspect that the symmetry plane has not been set correctly. It is acting as a wall as opposed to a symmetry plane. Did you assign a wall boundary condition to the symmetry plane? It should be assigned as only symmetry.

My setup is explained here:

Originally Posted by K-al-Eps-o

Dear Lefteris,

Thanks a lot for your reply.

The pictures are misleading, but the geometry is well aligned with the X-Y-Z axis (I doubled checked). The issue might come from something else.

To continue my investigations, I used three different meshes (cf figure below, from left to right):

1. Mesh1: This mesh (which is the same mesh used to generate results of my first post) models only the left half of the domain. The face with the normal in the positive X direction has "symmetryPlane" as a BC while other wall faces have the "noSlip" BC. This mesh has inflation layers on every external face, except inlet and outlet.
2. Mesh2: This mesh models the full domain and doesn't resort to symmetry plane. It has inflation layers on every external face, except inlet and outlet.
3. Mesh3: Same as the Mesh1, this mesh models only the left half of the domain with a symmetry plane ("symmetryPlane" BC) at the face with normal pointing in the positive X. However, the face with the symmetryPlane BC has no inflation layer.

With Mesh2, I wanted to check what was the correct solution, without using symmetryPlane BC. The solution (see figures below) showed a different (more realistic) solution than with Mesh1.
With the mesh3, I wanted to check if the inflation at the symmetry plane was causing issue. It turned out that the solution with no inflation at the symmetry plane gives a result very close to the one modeling the whole domain. I concluded that the inflation was causing trouble. Is this common knowledge ?

Finally, I am a bit confused by the results. I am expecting the flow to detach from the wall at the elbow, but it seems to stay attached. In addition, I was expecting to observe Dean Vortices, as described in the literature. Do you have any guess about what could be wrong ?

Thanks again for your help.

What is weird is that I applied a symmetryPlane BC on both meshes but the one with the inflation layers acts like a wall.

Anyway, now I know.

Thanks a lot for your help !

[Aeronautics El. K.]

For whatever reason I can now see your responses. I couldn't yesterday. Anyhow.

Originally Posted by K-al-Eps-o

Dear Lefteris,

Thanks a lot for your reply.

The pictures are misleading, but the geometry is well aligned with the X-Y-Z axis (I doubled checked). The issue might come from something else.

Understood.

Originally Posted by K-al-Eps-o

It turned out that the solution with no inflation at the symmetry plane gives a result very close to the one modeling the whole domain. I concluded that the inflation was causing trouble. Is this common knowledge ?

Yes, I'm not sure why you'd have prism cells (or inflation layers or however anyone calls them) on a symmetry plane. It doesn't make much sense.
Some software by default don't allow prism cells on a boundary that is not set as wall, even if you try to define them (the layers) in the mesh controls.
So perhaps in OF, by asking the mesher to build layers, this tricks the code to think that that's a wall and then goes and models a boundary layer...
I don't know, I'm just guessing here.

Originally Posted by K-al-Eps-o

Finally, I am a bit confused by the results. I am expecting the flow to detach from the wall at the elbow, but it seems to stay attached. In addition, I was expecting to observe Dean Vortices, as described in the literature. Do you have any guess about what could be wrong?

Not quite sure. The standard answer would be to check the fluid properties, the boundary conditions at the inlet and outlet, turbulent quantities and of course the mesh. If that doesn't work, you can always question the assumption of steady state flow.

[slaine]

Originally Posted by K-al-Eps-o

My setup is explained here:

Thanks a lot for your help !

You are very welcome. I am glad that I could be of assistance.

[K-al-Eps-o]

Originally Posted by Aeronautics El. K.

If that doesn't work, you can always question the assumption of steady state flow.

I tried to solve the flow with an unsteady solver. It gave me (the same) steady result