studying a valve case
 

Hi all,

I'm studing a simple case which is a box with circular inlet (velocity 5,3 m/s) and an outlet (pressure =0) with walls and a valve (which is also wall). I simulate with air and using simpleFoam. Attached the pictures of the geometry and in the next post i will attach the problem pictures.

My problem is that using internal field, I have elements with high pressure at the interface between the inlet and the wall. Taking in consideration that I use feature edge: P { margin-bottom: 0.21cm; }
surfaceFeatureExtract -includedAngle 150 -writeObj constant/triSurface/surfacemesh.stl surfacemesh.



Can anybody help me to solve this issue?

it may return to your mesh, first check your mesh with checkMesh

Dear Nima Sam,

I already check the mesh, & I think there is no problem.

well, did you consider uniform velocity at inlet and fixedValue for walls ?
if yes, you may want to try a profile for inlet velocity to make it much smooth near wall :)
However you should provide more details until we can help you :)

Dear Nima Sam,

yes I consider uniform velocity with fixedValue at inlet (0 0 5.3) and a fixed value wich is also uniform of (0 0 0) at walls

attached are the U, P, boundary files.

taking in consideration that:
stlSurface_mur --> wall
stlSurface_clapet --> valve
stlSurface_entree ---> inlet
stlSurface_sortie --->outlet

best regards,
Mina

well, its some how reasonable :), you assign a uniform fixed value velocity for inlet and also :) you assigned a no slip condition on wall :),consider just cells in edges, on those cells should be imposed both above conditions :), or in other words when fluid enters geometry with a uniform velocity, it should be compatible with no slip conditions on wall, so it should become zero :) so in one or two inlet cells you observed a high-pressure :) as i said in previous post you can assign a non-uniform velocity at inlet, for example parabolic one, then you would not see those high pressure

I see, thanks a lot NimaSam for your help i will try now to search about non uniform velocity at inlet.

Regards,
Mina

But when i tried another geometry for inlet for example a rectangular surface instead of circular one.. I didn't realize these strange elements with high pressure !!!

Greetings to all!

@Mina: I got your PM some time ago, but only today did I manage to look into this.
I only have a few comments to make:

• The "blockMeshDict" file seems to be in metres, so I guess that you use transformPoints to change from millimetres to metres?
• The images seem to have been taken while the "p" field was shown in vertex mode. In other words, instead of showing the values in the centre of the cells, it's showing the interpolated values on the vertexes of the mesh. Attached are two images that show the differences between the two modes.
  • The reason why this is important is because the representation you've shown us does not reflect properly where the crazy results are exactly.
  • In addition, you have not indicated what residual values you have for the respective runs, since it's very possible that the first case with the circular inlet didn't converge.
• Another thing that might help is to use the filters "Slice" and "Extract Cells By Region", which can help you inspect which exact cells have the strange values.

Best regards,
Bruno


edit: Looks like the untrained readers are not able to understand which is which, in the attached images. It's simple:

• The picture on the left is the one with the cells/faces representation, as you can see from the large data squares in the main 3D display.
• The picture on the right is the one with the point/vertex/interpolated representation, which is looks so smooth, pretty and not very accurate ;)

for more clarification,
whats differences between point and vertex?by poit it means its a cell center point and vertices are its corners points,right?

Hi Ehsan,

For reference, the official guide says this: http://www.paraview.org/Wiki/ParaVie...s.2C_arrays.29

I can't believe I'm going to have to explain this :( ... OK, in ParaView there are three basic geometrical types of representation:

• Points
• Lines
• Surfaces

If this wasn't enough, there are at least two basic types of data content:

• Data that is registered in points, aka "Point Data". Among these are the following usual usage scenarios:
  • The data is associated to the vertexes of cells and faces as real data.
  • The data is associated to the vertexes of cells and faces as interpolated data. One example of this type of data is to use the filter "Cell Data" to "Point Data".
• Data that is registered in surfaces, aka "Cell Data". Among these are the following usual usage scenarios:
  • The data is associated to the centre of each cell or face as real data (this is how OpenFOAM usually stores the real data).
  • The data is associated to the centre of each cell or face as interpolated data or perhaps as an average of the data. Example of interpolation for this case is the filter "Cell Data" to "Point Data".

In addition, ParaView uses the following convention:

• Data on surfaces are either the real values from the centres i.e. "Cell Data" or are showing the interpolated values from the "Point Data".
• Data on points are usually only the data from themselves, assuming that they have the geometrical characteristic associated to it.
  • Note: Glyphs themselves (e.g. used as vector representation or for seeing where the points are) only work on "Point Data".
• Data on Lines... are probably what ParaView thinks it's best to show, depending on "Cell Data" or "Point Data".

Is it clear enough now? :confused:


Best regards,
Bruno

very good description dear Bruno.there is one cfd-online and one Bruno Santos!
I don't know what I could do if you were not here. ;)
another non related question! how do you write lists in your posts?

Ask here: http://www.cfd-online.com/Forums/sit...k-discussions/

Dear Bruno,
First of all, my STL file was in "mm" so after blockMesh and snappyhexMesh, I use transfomPoints to change from millimetres to metres. Is there any problems related to this?

Here are some pictures using cells/faces representation

I used these residuals values residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon|omega)" 1e-3;
}
and I put the endTime in controlDIct file to 3000 but in fact the solution didn't converge and it stops while attending the 3000 and it didn't converge before. I think i can't make the endTime more than 3000 because it took a lot of time to calculate.


and in the next post i will attach other pictures using slice fliter

Regards,
Mina

These are other pictures, you can see these strange cells with high pressure .

Hi Mina,

OK, there are several issues that seem to be possibly be occurring here:

1. The cells near the corners of the cylinders are clearly a headache. Having one layer of cells with very low pressure and the ones next to it with high pressure values, seems to indicate that you have got vortexes in the zone of those cells. Here are a few solutions:
   • Remove completely the sharp edge where you're having problems, by applying a fillet in the CAD stage or something. This is if only you can modify the geometry.
   • Increase or reduce the mesh resolution near the edges of that cylinder, so that it can either better solve the vortexes or completely ignore them.
2. It all depends if you have the turbulence model turned on or off. Because if you are solving in laminar mode, you will need very low inlet and outlet fluid speeds.
3. If you are using a turbulence model, then you should check the y+ "yPlus" field on the walls. You can run:
   
   Code:

   ---

   yPlusRAS

   ---

   to calculate the y+.
   Depending on the values you get for y+, you need to adjust your mesh accordingly. More on this topic: http://www.cfd-online.com/Wiki/Dimen...e_%28y_plus%29

Best regards,
Bruno

Dear Bruno,

Thank you so much for your reply.
I created a very simple case which is a simple cylinder with inlet (velocity =5.3), walls , outlet (P=0).
I used the solver simpleFoam with turbulent.
I tried to vary the mesh with different values, increasing and reducing also i tried to apply a filled but the same problem is still there.
I'm so surprise, I attached some pictures which explain this issue.

Hi Mina.

Could you post here the test case?
This is strange behavior indeed :)
I am guessing that it is caused due an inconsistent boundary conditions or due the numerical pressure singularity phenomena (e.g."L" problem or squeeze flow issue).

Btw. It is usual to use pressure driven flow. In the test case that can be interpreted as PRESSURE driven flow in cylindrical pipe there exists an analytical solution. You can find it as Poiseuille fluid flow. It could help you to set the model properly.

Best regards

Martin

Dear Martin,

here is the test case