[david]

I tried to simulate the case also with a different geometry where the cyclic patch is between the rotor baffle and stator baffle.



In this case the velocities are ok around the impeller tip. The error seems to occur in the rotating zone along the cyclic patch.

Velocity:


Pressure:


The same problem occured in a simulation of an impeller. The following picture shows the pressure distribution in a cut through an impeller with the blade in the middle and the cyclic patches on the left and the right side.

Is it possible that MRFSimpleFoam has a problem with cyclic patches or did I make something wrong?

Regards
david

[david]

I tried to simulate the case also with a different geometry where the cyclic patch is between the rotor baffle and stator baffle.



In this case the velocities are ok around the impeller tip. The error seems to occur in the rotating zone along the cyclic patch.

Velocity:


Pressure:


The same problem occured in a simulation of an impeller. The following picture shows the pressure distribution in a cut through an impeller with the blade in the middle and the cyclic patches on the left and the right side.



Is it possible that MRFSimpleFoam has a problem with cyclic patches or did I make something wrong?

Regards
david

[david]

I found the solution. If anybody is interested:

The make mesh script removes the boundary faces from the rotating zone. I assume that this operation results in a incorrect computation of the fluxes across the cyclic boundary. The solution is to define separate cyclic patches for the rotating and non-rotating zone. After deleting the boundary faces it is necessary to add the cyclic patch of the rotating zone to the set. This can be done with the topoSetSource patchToFace. The results are identical to the simulation with the full geometry.

Regards
david

[vinz]

Hi David,

It looks like you manage to get something with the cyclic patches and MRFSimpleFoam. I managed to run the tutorial test case without problem.
Now I would like to know how to run my own test case. I have a mesh representing a kind of boat propeler with a tube and 3 blades on it. I can run it with simplefoam staticly. But I'd like t run it with rotation using MRFSimpleFOAM.
Could you indicate me the steps required to do that please?

Regards,

Vincent

[david]

Hi Vincent

The main point is to assign the rotating cells to a cell zone. I think that the following tutorial could be interesting for you:

http://openfoamwiki.net/index.php/MRFSimpleFoam

Take also a look at the mixerVessel2D tutorial. After the excution of makeMesh you can see in blockMeshDict that the cells of the inner blocks are assigned to the cell zone rotor. makeMesh creates a set rotor containing the cells of the zone rotor, takes the faces of these cells and adds them (without the Boundary faces) to faceZones. This is done because MRFSimpleFoam uses an absolute velocity formulation and has to compute the relative flux at the faces in the rotating zone.

In constant/MRFZones you can specify the angular velocity of the rotating cell zone and the corresponding patches:

1
(
rotor
{
patches (patch1 patch2);
origin origin [0 1 0 0 0 0 0] (0 0 0);
axis axis [0 0 0 0 0 0 0] (0 0 1);
omega omega [0 0 -1 0 0 0 0] 35;
}
)

I hope that I was able to help you.

Regards
david

[aganesan]

Hello,
I have just started learning the Turbomachinery capabilities in OpenFOAM (Version 1.4.1) on Linux.
I have good results using simpleFoam and turbFoam for non-turbomachinery applications. But when I open FoamX and try looking for MRFSimpleFoam I just could not find it. When I checked for MRFSimpleFoam directory from the command prompt it is very much present in my tutorials directory. Even though it looks like a basic question, it would really be helpful if somebody can help me in running this mixerVessel2D tutorial.

Anand

[dmoroian]

Hello Anand,
I don't think you can run MRFSimpleFoam out of the box with FoamX, you need some configuration files for it.
The good news is that you can run it directly without FoamX.
Just go to the mixerVessel2D directory and type

./makeMesh

, then go one directory up (cd ../) and type

MRFSimpleFoam ./ mixerVessel2D

.

...as simple as it can be, right?

Dragos

[aganesan]

Hello Dragos,
Thanks a lot for providing me with valuable information.
(i) I was successful with the ./makeMesh command.
(ii) I went one directory up and typed MRFSimpleFoam <singlespace>./<singlespace> mixerVessel2D.I get the following error: bash: MRFSimpleFoam: command not found.
Can I trouble you more for help in this regard?
Thanks in advance.

Anand

[dmoroian]

Ok, that means you have to compile the MRFSimpleFoam. In the same directory with the case mixerVessel2D, there is a subdirectory called MRFSimpleFoam. Go there, and compile the solver:

wmake

.
Then update with rehash or just open a new xterm. No you should be able to run MRFSimpleFoam.

Dragos

[aganesan]

Thanks a lot, Dragos. It works.
So, I guess in order to do turbomachinery calculations, you have to go at the 'source code' level. Is it a fair statement to make? If so, can
you suggest/recommend me with some relevant materials to begin with. I have been able to find some papers through netsearch, but they dont really go into the implementation details.
Thanks again.

Anand

[dmoroian]

Nope, MRFSimpleFoam is a standard solver, that happens to be uncompiled in the 1.4.1 version. No need to look inside, unless you want that.
You can always find good basic information in the documentation that comes along with any commercial software.

Dragos

[grtabor]

Why isn't it in the proper place in the distribution? Its kind of untidy to have it in the tutorial directory rather than in applications.

Gavin

Hi David,
It seems like you did a good job with the solver MRFSimpleFoam. i want to ask you about the cyclic BC in the MRFSimpleFoam.

I'm trying to simulate mixerVessel2D, the tutorial test case.

There was no problem if i started a simulation for a cycle region. the following picture is the velocity distribution.

Unfortunately I get wrong(?) results when I started a simultion for 1/4 cut of the region.

the geometry and cyclic BC are the same as shown by you in May 27, 2008. the following is the velocity result with the cyclic BC.(Don't mind the velocity value at the rotor. when i transfored the OF data to FLUENT, there was a error at the rotor boundary.)


i have read the discussion message posted here, and I added the cyclic face of the rotating zone to the faceZones, as you said.

I checked the face-face pair in the cyclic patches, and I think there was no problem.

my question is that why the velocity contours has a jump at the cyclic boundary. And is it not surprising that the result of 1/4 cut with cyclic BC is different from the cycle one?

Hi David,

if you do not mind, could you email me a copy of the case files for the mixerVessel2D with cyclic BC, including the directories of 0, constant, system?

zhaolj98@yahoo.co.jp

And i want to appreciate everyone who can help me.

[david]

Hi zhaolj

Did you apply the patch for cyclic boundaries:

http://www.cfd-online.com/cgi-bin/Op...c=1&post=20154

If that doesn't fix the problem, then I have really no idea why these jumps occur. Here is my case:

cyclicMixerVessel2D.tar.gz

A readme file with instructions is also included.

Regards
david

Hi David, thank you very much.
yes, i applied the cyclic boundaries. i checked your case files, and i am sure that my case was just done as samely as yours.

i executed your cyclicMixerVessel2D as you said in readme.txt. Unfortunately, the same jumps of velocity occurs at the cyclic boundary.

but there is no jump of pressure.

i checked the cyclic boundary conditions in the latest time directory. here is the U cyclic boundary of the rotating zone in the 500 time directory. And you can see that the cyclic BC is satisfied very well.

periodic1
{
type cyclic;
value nonuniform List<vector>
32
(
(2.22966 2.60265 -2.44821e-19)
(2.08095 3.65685 6.94315e-19)
(2.23047 3.35284 -3.29633e-18)
(2.23759 3.21746 -2.61382e-18)
(2.18124 3.11587 2.69876e-18)
(2.14067 3.09886 -2.87145e-18)
(2.0799 3.11904 1.70075e-18)
(2.01199 3.18502 4.28768e-18)
(1.92898 3.27932 0)
(1.81408 3.37737 0)
(1.60946 3.34545 -2.35826e-18)
(1.28213 3.02688 4.68323e-18)
(0.897623 2.37708 -3.51468e-18)
(0.620053 1.73735 1.12902e-17)
(0.357876 1.34403 -7.31169e-18)
(0.199506 1.06251 6.13411e-18)
(2.60265 -2.22966 -2.44821e-19)
(3.65685 -2.08095 6.94315e-19)
(3.35284 -2.23047 -3.29633e-18)
(3.21746 -2.23759 -2.61382e-18)
(3.11587 -2.18124 2.69876e-18)
(3.09886 -2.14067 -2.87145e-18)
(3.11904 -2.0799 1.70075e-18)
(3.18502 -2.01199 4.28768e-18)
(3.27932 -1.92898 0)
(3.37737 -1.81408 0)
(3.34545 -1.60946 -2.35826e-18)
(3.02688 -1.28213 4.68323e-18)
(2.37708 -0.897623 -3.51468e-18)
(1.73735 -0.620053 1.12902e-17)
(1.34403 -0.357876 -7.31169e-18)
(1.06251 -0.199506 6.13411e-18)
)
;
}

So i think the problem maybe happened in the postprocessing step, not in the solver MRFSimpleFoam.

After the simulation stopped, i executed the following commands:
foamMeshToFluent . cyclicMixerVessel2D
foamDataToFluent . cyclicMixerVessel2D
then the above pictures were made by FLUENT, and the jumps occured.

anyone can tell me where the problem was?

regards
zhaolj

sorry, i made a mistake. there was a pressure jump at the cyclic boudary too.

Hi, David and everyone.

i found the solution. it is a bug in version 1.4.1 which i am working on.

http://www.cfd-online.com/OpenFOAM_D.../126/5850.html

when i replaced "OpenFOAM-1.4.1/src/finiteVolume/fvMatrices/fvMatrix/fvMatrixSolve.C" with the one supplied by Henry Weller, no jump occurs at the cyclic boundary, and the 1/4 piece result matches very well with the one of cycle region.

thank you !