[rock.senthilkumar]

Dear Alberto,
Thanks for your quickest replies.If I am not wrong, OF 1.7.1 tutorials does not have example case for rhoSimpleFoam. Even I searched through Internet to download but failed, then only came to know lot of people are looking for test case. Please correct me if I am wrong.

Originally Posted by alberto

Take a look at the tutorials :-)

[alberto]

Originally Posted by rock.senthilkumar

Dear Alberto,
Thanks for your quickest replies.If I am not wrong, OF 1.7.1 tutorials does not have example case for rhoSimpleFoam. Even I searched through Internet to download but failed, then only came to know lot of people are looking for test case. Please correct me if I am wrong.

You can quickly adapt the cases for rhoPimpleFoam and rhoPorousSimpleFoam to rhoSimpleFoam.

I added the required entries to the attached case, but I did not clean the dictionaries up.

[rock.senthilkumar]

Dear Alberto,
Thank you for your attachments. I will clean up the dictionaries, and let you know how it works for my case. Thank you again.

Originally Posted by alberto

You can quickly adapt the cases for rhoPimpleFoam and rhoPorousSimpleFoam to rhoSimpleFoam.

I added the required entries to the attached case, but I did not clean the dictionaries up.

[ptbs]

Hi aerothermal

I have the same problem with pressure instability with RhoPorousSimpleFoam inducing speed oscillations (up to crash). I made a research with your name on this CFD Online forum and found no trace of a new thread dealing with this problem written by you. Could you be kind enough to tell me (if ever you did it) where this thread is located. In case of no new thread, could you explain me how you stabilized such pressure instabilities.
I reduced the p relaxation factor down to 0.0005! it helps but each time I reduce the outlet pressure, to progressively reach higher speeds (I wish I could reach Mach1 at the outlet, but still am at ~Mach 0.1), I need to reduce further this factor. Is it sufficient to reduce p relaxation factor? Any other tricks you succeeded with?

Many thanks.

Best regards

[aerothermal]

Hi Patty,

Try to use divSchemes div(phi,U) Gauss limitedLinearV 1.0
Usually it helps to stabilize.

I manage to converge my case but the results are not good.
I will posto some results here later.

regards,

aerothermal

[alberto]

Originally Posted by ptbs

Hi aerothermal

I have the same problem with pressure instability with RhoPorousSimpleFoam inducing speed oscillations (up to crash). I made a research with your name on this CFD Online forum and found no trace of a new thread dealing with this problem written by you. Could you be kind enough to tell me (if ever you did it) where this thread is located. In case of no new thread, could you explain me how you stabilized such pressure instabilities.
I reduced the p relaxation factor down to 0.0005! it helps but each time I reduce the outlet pressure, to progressively reach higher speeds (I wish I could reach Mach1 at the outlet, but still am at ~Mach 0.1), I need to reduce further this factor. Is it sufficient to reduce p relaxation factor? Any other tricks you succeeded with?

I believe it is not appropriate to relax so strongly the pressure. If you need to do that, most probably you have a problem in your physical or numerical setup.

Could you post a simple case that reproduces the problem?

Best,
Alberto

[ptbs]

Originally Posted by aerothermal

Try to use divSchemes div(phi,U) Gauss limitedLinearV 1.0
Usually it helps to stabilize.
aerothermal

Hello aerothermal

Thanks for answering. I have tried in my next iterations to use "divSchemes div(phi,U) Gauss limitedLinearV 1.0" instead of "Gauss upwind", as you suggested but using, as initially, a p relaxation factor of 0.2. It has diverged after only 20 iterations. So I kept your suggestion but combine it with a 0.00025 p relaxation factor, waiting for more information from you.

By the way, what is the meaning of the constant 1.0 in "Gauss limitedLinearV 1.0". I tried to watch in the C++ files, but really, it is not clear for an "end user" like me. Is it to be tuned like relaxation factors or just a constant setup for openFoam solvers?

Best regards

[ptbs]

Originally Posted by alberto

Could you post a simple case that reproduces the problem?

Hello Alberto

Well, the case I am studying is quite big and absolutely confidential. So, I will try to make another model, oversimplified but that could recreate this behavior.

However, in case of success, how to post a full case in this forum? Do you need the mesh files or just the dictionaries setting up the rhoPorousSimpleFoam solver? Being new in this forum, I never did it before. Have you a suggestion? A thread to read that describes the best procedure according to your experience? Other similar advices? I read that the attachment to a post in this forum is 98KB max, so may be a zip or tar file could be suitable, but what to place in it?

Be patient, I will try to do it with your recommendations during the next week-end.

Many thanks

[alberto]

Originally Posted by ptbs

Well, the case I am studying is quite big and absolutely confidential. So, I will try to make another model, oversimplified but that could recreate this behavior.

OK.

However, in case of success, how to post a full case in this forum? Do you need the mesh files or just the dictionaries setting up the rhoPorousSimpleFoam solver? Being new in this forum, I never did it before. Have you a suggestion? A thread to read that describes the best procedure according to your experience? Other similar advices? I read that the attachment to a post in this forum is 98KB max, so may be a zip or tar file could be suitable, but what to place in it?

A small complete case reproducing the problem would help. If not that, at least the numerical setup and the boundary conditions you use. If these are fine, your problem might be the mesh

P.S. If you have large files, you can use a service like dropbox (free up to 2GB).

Best,

[ptbs]

Originally Posted by alberto

A small complete case reproducing the problem would help.

Hi Alberto

Here it is. I follow your suggestion and place a complete case very similar in boundary conditions as the one I try to solve, and run it Sunday evening. This case presents all the typical behavior I mentioned previously. Here I have also reduced p relaxation factor down to 0.0025, and even like that it is still unstable. The dropBox links to get the full solved problem is http://dl.dropbox.com/u/21252587/14cfdtest.tar.gz (Sorry for the size of the full simulation ~1.4GB, I think it is better you get all to understand). I used RhoPorousSimpleFoam because I finally want to use the porous element I place in the middle part, but for the moment (to simplify) the Darcy parameters are so low that they do not influence. Moreover, I never see instability from that porous area.

Have a look with paraFoam making a slice at middle XZ plane. The exhaust pipe show very clear instability with time (like waves) that I can really not understand. In my other models these sudden instabilities sometimes happen in the larger inlet pipe during transition regime, although I am very far from my Mach 1 objective at the outlet section ( I wish to decrease progressively the outlet pressure to force the simulation to reach M1 at the outlet pipe).

From what I read, description of problem from other participant to this forum are sometimes similar.

Could you help us?

Many Thanks

[aerothermal]

Dear ptbs,

My low Mach cylinder case in a small tunnel (almost a duct) converged. The waves still does appear but they are not as critical as before.

I used the OF1.6-ext instead of OF1.7.1. It helped a lot in convergence.

See attached the fvSchemes and fvSolution.

Also pay attention in your boundary conditions. Place adequate values for k, epsilon, mut and alphat. Regarding U and p, you should take even more care with the combination of types. Take a look in the tutorial for rhoPorousSimpleFoam. It will help you.

Regards,

aertothermal

fvSchemes.txt

fvSolution.txt

[alberto]

Originally Posted by aerothermal

I used the OF1.6-ext instead of OF1.7.1. It helped a lot in convergence.

It seems you are using a very standard numerics, which would indicate problems in 1.7.1 that are not in 1.6-ext. Do you know what was the difference causing convergence problems?

Best,
Alberto

[aerothermal]

Hi Alberto,

I do not know yet the causes but I am still investigating.

The mesh is tetra based with one region and a prism layer around the cylinder. From wikki site I saw that 1.6-ext has some extra capabilities over 1.7.

FUNDAMENTAL DEVELOPMENTS
Improvements in accuracy and stability on tetrahedral and tet-dominant meshes

http://www.wikki.co.uk/

Regards,

Guilherme da Silva

[alberto]

Yes, but that only applies if you use reconCentral scheme, at least in my understanding.

Anyway, if you find something, please let us know! :-)

[alberto]

Originally Posted by ptbs

Hi Alberto

Here it is. I follow your suggestion and place a complete case very similar in boundary conditions as the one I try to solve, and run it Sunday evening. This case presents all the typical behavior I mentioned previously. Here I have also reduced p relaxation factor down to 0.0025, and even like that it is still unstable. The dropBox links to get the full solved problem is http://dl.dropbox.com/u/21252587/14cfdtest.tar.gz (Sorry for the size of the full simulation ~1.4GB, I think it is better you get all to understand). I used RhoPorousSimpleFoam because I finally want to use the porous element I place in the middle part, but for the moment (to simplify) the Darcy parameters are so low that they do not influence. Moreover, I never see instability from that porous area.

Have a look with paraFoam making a slice at middle XZ plane. The exhaust pipe show very clear instability with time (like waves) that I can really not understand. In my other models these sudden instabilities sometimes happen in the larger inlet pipe during transition regime, although I am very far from my Mach 1 objective at the outlet section ( I wish to decrease progressively the outlet pressure to force the simulation to reach M1 at the outlet pipe).

From what I read, description of problem from other participant to this forum are sometimes similar.

Could you help us?

Many Thanks

The instability seems induced by the outlet condition. Check it.

The under-relaxation factors do not make much sense to me. You relax way too much the pressure, and way too little the density. Better values:

rho - 0.05
p - 0.3

The minimum bound on pressure is too close to the value at the outlet (iterations might trigger bounding too easily).

Also, are pressures set to physical values? 120 Pa?

Additionally, use leastSquares for gradients computation:

    
default         cellLimited leastSquares 1;
grad(p)         leastSquares;

It gives more accurate results on arbitrary grids.

Finally, do you work with a modified version of the solver? Your fvSolution has a nUCorrectors, while the correct syntax in rhoPorousSimpleFoam is nCorrectors.

Best,

[aerothermal]

One thing that helped a lot was to mirror the mesh.
In case of cylinder I mirrored it at mid plane from top to bottom.
So the numerical disturbances did not cause any further symmetry issues.

[alberto]

Hi, in Patty's case the mesh seems OK. I run the for a while, and the solution is smooth. Instabilities originate from the outlet (meaning they probably depend on some physical element not set properly), but that I cannot know for sure since we do not know the details of physical problem.

[aerothermal]

OK. I am downloading it now to take a look.

[ptbs]

Originally Posted by alberto

Hi, in Patty's case the mesh seems OK. I run the for a while, and the solution is smooth. Instabilities originate from the outlet (meaning they probably depend on some physical element not set properly), but that I cannot know for sure since we do not know the details of physical problem.

Many thanks to all of you Alberto and Aerotherm.
I will have a look at your comments and I am very interested hearing even more from you if you make some more tests on this case.

Concerning the physical problem, the case I gave is just an illustrative way to show you the instability I have in my study, as such no real meaning excepted I need very low pressure i.e. very low density. For a more practical case (I can not describe) just imagine that you want to homogenize a pressure and a flux (thanks to the porous part not yet used) before an exit which is at such a low pressure that you reach sonic speed... In this test case, I take air at room temperature.

Concerning the solver, as seen in the submitted case files, I use openFoam.1.7.1 as downloaded from official site released in June 2010. I did it this classical way under a Ubuntu-Linux terminal:
1) echo "deb http://www.openfoam.com/download/ubuntu lucid main" >> /etc/apt/sources.list
2) apt-get update
3) apt-get install openfoam171

Best regards

[alberto]

Originally Posted by ptbs

Concerning the physical problem, the case I gave is just an illustrative way to show you the instability I have in my study, as such no real meaning. For a more practical case (I can not describe) just imagine that you want to homogenize a pressure and a flux (thanks to the porous part not yet used) before an exit which is at such a low pressure that you reach sonic speed... In this test case, I take air at room temperature.

There seem to be no problem with the mesh, so I would simply turn on the porous zone, and consider the actual flow conditions.

You are going to have a sort of wave reflection at the outlet I think. Maybe you want to give a try to waveTransmissive BC's and an unsteady run (rhoPisoFoam, rhoPimpleFoam).

Concerning the solver, as seen in the submitted case files, I use openFoam.1.7.1 as downloaded from official site released in June 2010.

Then your fvSolution has a typo (see my comment).

Best,