[student666]

Hi all,

I'm trying to solve the following case study using OpenFOAM 2.3.1; it is an incompressible, steady state turbulent internal flow inside a bended pipe (simpleFoam). Here's the paper:
http://prod.sandia.gov/techlib/acces...004/043467.pdf
I chose to use this case to better understand turbulence modelling.

I managed to prepare the boundary layers according to what is written on the paper: first layer 0,15mm to the wall and by looking at the pictures, I also added 4/5 layers (1,2 expansion factor).

I chose to use the k-omega turbulence model for the calculation; the reason is because using the RNG-kEpsilon model (or standard kE), OF crashes at the beginning of each calculation.
Can't understand why; I also tried to run the case as laminar in the beginning, and then switching to turbulence, but every time it crashes. (Why?)

Initial conditions as for paper, I only set for the pressure value to 0Pa at outlet, and to 0,1Pa for the internal field.
I get a solution converged in about (monitoring mass-flow difference between inlet & outlet) 1800 iterations.
Anyway when I plot (in para-view) the 45° section on the bend, I'm not able to see any secondary (inertial) eddy as described in the paper (see fig.5).
Even value for p to the wall seems different: I got about 9000Pa (p*rho) instead of 100000Pa (see fig.6)

I can't really understand if my calculation is totally wrong and how should I check for mistakes, or simply it's a post-processing visualization problem.

Can someone help me?

Thanks a lot.

Michele

PS: in the tar file there's the 1800 time folder. If you want to run the case, you should:
1 - import the mesh from unv file
2 – using surfaceToPtach constant/triSurface/inlet.stl & surfaceToPtach constant/triSurface/outlet.stl to generate patches
3 - correct the boundary file
4 - run the case

[RodriguezFatz]

1) Pressure: In the paper they plot the absolute pressure, in OpenFoam you will probably look at relative pressures.
2) Pressure: I don't think you need to multiply pressure with rho as you suggested for the incompressible solvers. It's just "p".
3) If you post the log output of the k-epsilon crash, we can suggest some help.
4) How do the residuals look like in your converged solution?
5) Did you check your flowrate? Does it match the one from the paper?

[RodriguezFatz]

Do you understand the paper? First, they state that the y+ is choosen to capture the strong gradients in the viscous boundary layer. Then they write about wall functions. Does that make sense?

[student666]

Hi and thanks for your kind reply.

1) Pressure: In the paper they plot the absolute pressure, in OpenFoam you will probably look at relative pressures.
2) Pressure: I don't think you need to multiply pressure with rho as you suggested for the incompressible solvers. It's just "p".

1) Ok it should be, so I have to sum the kinetic pressure.
2) Sorry, but I disagree. I'm quite sure that for incompressible solver I have to multiply by rho, as you're supposed to define ni (m2/s) in the transport properties. By the way, it make no sense for me that: water flowing at a mean velocity rate of 5m/s on a pipe of 35,5 mm can generate a static pressure of 9 Pa only, on a 90° bend. I think this is no physically correct.

3) If you post the log output of the k-epsilon crash, we can suggest some help.

Thank you very much, but I deleted the folder with the kEpsilon model as for many crashes and also because it is said that kOmega model better performs calculation for internal flows, even if it is more sensible to initial conditions.
For my calculation, I only divided epsilon by k to estimate omega value, assuming right values given on paper.
Definition of omega at CFD on line, it is said that for some solver, you should to use Epsilon/k/0,09. What should I use then?
http://www.cfd-online.com/Wiki/Speci...ssipation_rate

4) How do the residuals look like in your converged solution?

I attach a picture.

5) Did you check your flowrate? Does it match the one from the paper?

At pag. 13 it is written 2.379kg/s, my solution is 17,72 m3/h. m=2,379*3600/rho(965,35)*2(because half pipe)=17,74m3/h
So I think it matches. futher: if you calculate v*pipeArea*3600=17.84m3/h

Do you understand the paper? First, they state that the y+ is choosen to capture the strong gradients in the viscous boundary layer. Then they write about wall functions. Does that make sense?

Yes, you're right it sounds strange. By what I learned about, RANS models give you a good (averaged) flow behavior. One step forward I should perform is to use a kOmegaSST model, but my calculations give me an y+ value of about 2,86e-6m to get a value of 1. This resolution for the mesh gives me problem with the parabolic inlet profile.
http://www.cfd-online.com/Forums/ope...tml#post566149
In anycase, I can't still understand how to model that inertial effects. Or in other words: should these behaviour only be predicted by using a lowRe turbulence model or not? Or is it only a matter of post-processing I don't know? Or did I understand nothing?

Thank you very much

[student666]

Do you understand the paper? First, they state that the y+ is chosen to capture the strong gradients in the viscous boundary layer. Then they write about wall functions.

If they choose a y+ to capture the strong gradients, then I think it only means to resolve the boundary layer with a low Reynolds turbulent model, or other tools for it (LES?)...
If they write to use wall functions, they plan to not resolve the viscous sub-layer, putting the y+ node in the log-layer.
So these two considerations contradict each other...

Does that make sense?

No!

Keeping the opinion that this paper is right, my question is: why I can't see any inertial effect on the 45° plane? the answers I could give are:
1) there aren't any and my calculation is true;
2) I made some errors;
3) I don't know how to analyze data correctly.

[RodriguezFatz]

Ok, you are absolutely right about pressure normalization.
So they plot the "in-plane velocity" I guess that means the part of the velocity that is parallel to the diagonal plane.
I don't know how to get this in paraFoam, but it's not just the velocity magnitude.

If you still want k-epsilon running you can reproduce the crash and post some log.

[RodriguezFatz]

Here you go:
http://www.cfd-online.com/Forums/ope...-parafoam.html

[JNSN]

I just tried, your mesh is running with kEpsilon turbulence model without any problems. With the post-processing described in Philipps link, you can clearly see the secondary flow in the elbow.
Anyway I have not checked the absolute values (p and U) and compared with the values given in the reference. I also set a uniform (homogenous) inlet velocity as I have not installed the swakForFoam library.

Best regards,
Jan

[student666]

Ok, thanks to all.

About secondary flow, it was only a problem about post-processing.

I re-run the case with the kEpsilon model as well and yes, it worked for me too.
I re-meshed the geometry many times, so maybe this time it fits to kepsilon model better.
I remember there was a floating point exception error; this error use to disappear when the n coefficient for the inlet profile was > 1.
So, at that time, my conclusions were that for very small cells, some ratio about coefficient of the matrix Ax=b, gives to the linear solver a division by very small number like 1/0; but I didn't know how to check this.
It would be of help to know how to map (sometimes) these floating points error; I mean if it is possible to look at the matrix, at the cell or whatever...

I have one more question about the p & U value at the wall in order to check the matching between paper and my calculation, but I'm making this last one on post-proccessing forum.

Bye.