adding porous media in rotatine zone

Adding feature of "Relative velocity Resistance formulation" which exists in Ansys-fluent for better prediction of source term when rotating region and porous zone are located in one zone. in Ansys-Fluent, the results, when you choose this option or not selecting it, are quite different. it seems that Openfoam can only calculate porous source term based on absolute velocity. when it is calculated Darcy-Forchimmier source term based on absolute velocity, it seems that porous zone is fixed in position and not rotating(see attachment files)

added feature request label

Thanks for your request - are you able to sponsor the developments/contribute code?

Hi I am working to develop this feature in simpleFoam and rhoPimpleFoam solvers. I have done a part of it (I am not a professional programmer) but it needs to improve because the velocity contour outer rotating region is drastically dropped . I can send you my solvers and test cases that I compared them with Ansys-fluent in same b.c and geometry. is it good and do you need more information? Regards Roshanak

Hi @Rabiee, I think it would be nice if you can share solvers, test cases, and guidelines to reproduce the issue/solution. Thank you.

Dear @Rabiee , we have been testing a potential fix. Could you please share your test case, if possible?

Hi, sure, I tried to add this feature (relative resistance formulation) in porousSimpleFoam solver, The solver and a case sample is attached porousSimpleFoamDynamic.rar if in the new version of OF you developed this feature, please inform me

0.rar

constant.rarsystem.rar

Hi @roshanak878 , thank you.

• Would you consider to test the following branch on your local cases? https://develop.openfoam.com/Development/openfoam/-/tree/feature-porous-mrf
  • A boolean keyword MRFRelativeVelocity (by default=true) has been added into constant/porosityProperties.
• I couldn't replicate the velocity/pressure OpenFOAM information with the latest develop (not feature-porous-mrf`) (i.e. the first image in the first entry of yours). Could you please tell me whether the attached case is verbatim the same with the case you used to obtain the reported results? If so, could you please share the OpenFOAM environment details (maybe a version difference causes a problem)?
  • I will test feature-porous-mrf on your test case once I can replicate the OpenFOAM image of yours by using the test case.

Please let me know if anything needs to be elaborated.

Hi @kuti I developed my solver in version 4.1 I uploaded a related solver, with a case working with this software. In the case that I uploaded, there are two cylinders rotating without inlet and outlet. Now, I uploaded the case two cylinders that are rotating and pressure and velocity plots comparable with mineCylinder.rarAnsys results.

Hi @Rabiee

In your solver, I couldn't understand the rationale for one of the terms: in UEqn.H, the term U=Urelative-U;.

Could you please explain it, if possible?

Many thanks.

Hi @kuti This is the way that porous media resistance term needs to be defined. If you look at Ansys-fluent tutorial, it said that for the rotating region, it is necessary to use relative resistance formulation for adding porous media source term. The source term includes =muU/C1+0.5rhoC2UU--> velocity of this term must be relative velocity (rw), not absolute velocity. So, I defined a new variable called Urelative and use it to define relative velocity that must be adopted for porous media source term. Anyway, that is the way I did it and work properly (you can look at OF generated result versus Ansys-Fluent-Figure attached) If it is not clear yet, please let me know Regards Roshanak

mentioned in merge request !472 (closed)

assigned to @andy

changed milestone to %v2112

added bug label

added Doing label

changed milestone to %v2206