CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Bugs (
-   -   MRFSimpleFoam: wrong boundary conditions on rotating walls (

cves April 15, 2010 11:37

MRFSimpleFoam: wrong boundary conditions on rotating walls
5 Attachment(s)

I am using OpenFoam1.5-dev, svn version 1677, with SIG Turbomachinery add-ons in order to perform the ERCOFTAC centrifugal pump case-study. I have found that the two faceSet made for the setup of MRFSimpleFoam lead to a wrong velocity value on the rotating walls. Indeed the velocity at the wall is set to zero instead of Omega x Radius.

I have followed the instructions and setups given in the openFoam Wiki :

However, I had to decrease the k and epsilon relaxation factor value from 0.7 in the original system/fvSolution file to 0.5 in order to achieved 5000 time steps. I give you the images (U.png and linear.png) of the velocity and the convergence that I get after the 5000 time steps.

I have compared these figures with the ones given by :

which has the same setups except that the svn version is 1240. I saw that the problem comes from the wrong velocity imposed on the rotating blades as you can see the small blue lines around the rotating blades which means a zero velocity value is imposed (U_zoom.png).

I found that the mixerVessel2D has not this problem and the only difference between these two tutorials was the two faceSet for system/faceSetDict_rotorFaces and system/faceSetDict_noBoundaryFaces, which are not done in the mixerVessel2D tutorial. So I remove this two faceSet for the ERCOFTAC centrifugal pump tutorial and run 5000 times steps (see the convergence and velocity profile after 5000 time steps U_noFaceSet.png and linear_noFaceSet.png).

In this case the velocity is correct on the rotating blade but the computation converge into a non-physical result.

If someone has the solution to correct the boundary value on the rotating blades and get a well physical converged solution, please let me know.

Best regards


cves April 20, 2010 03:47

Correction of the ercoftacCentrifugalPump tutorial
5 Attachment(s)

After a few days of research, I have found a way which corrects the ercoftacCentrifugalPump tutorials and can be used as first setup for a MRFSimpleFoam case study for OpenFOAM-1.5-dev svn version greater than 1242. Indeed the faceSet are useless in these versions, OpenFOAM is able to found the faces for MRFSimpleFoam by itself.

This correction leads to a good convergence without any tuning of the relaxation factors. I have attached some pictures of my results. Moreover the converged result is physical and close to the result of:

You just have to replace the makeMesh and constant/MRFZones files of your tutorials by the ones that I have attached to this post. My files are for the stiched mesh but you can also use it for the ggi mesh by adding the ggi boundaries in the nonRotatingPatches of the MRFZones file.

Best regards


waynezw0618 April 20, 2010 07:13

Also in 1.6

cves May 3, 2010 03:38

GGI case
2 Attachment(s)

Here are the modified files to run the GGI case correctly.


All times are GMT -4. The time now is 11:12.