CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

MRFSimpleFoam - Selection of rotating region

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Ivanet

Reply
 
LinkBack Thread Tools Display Modes
Old   May 25, 2011, 05:47
Default MRFSimpleFoam - Selection of rotating region
  #1
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Hi folks,
I have the following problem with MRFSimpleFoam: I am trying to simulate a small wind turbine. In my cellSetDict I select the cells where the Coriolis forces are applied. I do that with boxToCell and I call that region rotor:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.5                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      cellSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// Name of set to operate on
name rotor; //rotor;

// One of clear/new/invert/add/delete|subset/list
action new;

// Actions to apply to cellSet. These are all the topoSetSource's ending
// in ..ToCell (see the meshTools library).

topoSetSources
(
    // Cells in cell zone
    boxToCell
    {
    box (-2.5 -2.5 -1)(2.5 2.5 1);
    name rotor;      // name of cellZone

    }

);
Then I run cellSet in my makeMesh Script and convert the set to a zone:
Code:
cellSet
setsToZones -noFlipMap

cp system/faceSetDict_rotorFaces system/faceSetDict
faceSet

cp system/faceSetDict_noBoundaryFaces system/faceSetDict
faceSet

setsToZones -noFlipMap
In MRFZones I define the my geometry (Rotor_CATIASTL) as the rotating patch within the rotor region:
Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      MRFZones;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

1
(
    rotor
    {
        patches (Rotor_CATIASTL);
        // Fixed patches (by default they 'move' with the MRF zone)
    //    nonRotatingPatches (); //(INFLOW,OUTFLOW,TOP);

        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]  -44.4; 
    }
)
So far everything is OK. Now, I run the simulation and in the results I see strange flow effects in the boundary between the rotating and the non-rotating zone. In the pictures attached you can see what I mean. The rotating zone is the box you see in the pictures.

I have also tried to use a cylinder (as well as a sphere) for selecting the rotating cells, but I always get this problem at the "rotating- non-rotating" boundary region.
Do you have a clue why this happen and how it can be solved?
Thanks a lot in advance
Ivan
Attached Images
File Type: jpg Screenshot1.jpg (35.6 KB, 338 views)
File Type: jpg Screenshot2.jpg (41.2 KB, 324 views)
Ivanet is offline   Reply With Quote

Old   May 25, 2011, 06:02
Default
  #2
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
From your images, it looks as though your main issue is that your farfield boundaries are too close to your region of interest. The upstream boundary should be at least 5 blade spans away, the downstream boundary should be at least 10 blade spans away, likewise your side boundaries. This is to prevent the boundary conditions having too strong an influence on the computed flow around the rotor.

Second thing. It is normally standard when modelling rotors with MRF's to have the entire domain as an MRF, with the domain boundaries normally forming a cylinder. I'm assuming you've placed the MRF within a non-rotating domain to simulate varying inflow ala ABL? This normally works best if a mixing plane is present between the rotating and non-rotating zones, but I don't believe that capability exists in OpenFOAM. Someone in the know could possibly elaborate on this further.

Anyway, I'd try both suggestions and see how things go. I'd be interested in seeing your results regardless.
madad2005 is offline   Reply With Quote

Old   May 26, 2011, 09:49
Default
  #3
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Hi madad2005,
Thanks a lot for your quick reply. I have repeated the simulations with a larger domain, just as you propose. Unfortunately the results are still bad.
Actually I also wanted to consider my whole domain is rotating. However, if I do that, then the results are even more strange. That is why I was considering only a small zone as rotating region.
Now the goods news: Today I have managed to get reasonable results. Since I changed a couple of things at once in my simulation, I am still not sure which of my modifications was responsible for the better results. I will check that in the coming days and then I will post it.
Greetings
Ivan
Ivanet is offline   Reply With Quote

Old   May 28, 2011, 02:40
Default problem solved!
  #4
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Hi again, now I know where was the problem. As you can see in my first post, the MRFZones file contained a description of the rotating patches, but no definition of the non-rotating patches. That is wrong. Actually the rotating patches do not need to be defined here, since it will be assumed that all the cells defined within the cellSetDict are rotating cells. It is however important to define which patches do not rotate (inlet, outlet and outer walls).
Cheers
Ivan
Ivanet is offline   Reply With Quote

Old   November 17, 2011, 01:22
Red face Some help for MRFZones in OF
  #5
Member
 
ThanhToan
Join Date: Sep 2010
Posts: 47
Rep Power: 6
trantoan2008 is on a distinguished road
Send a message via Yahoo to trantoan2008 Send a message via Skype™ to trantoan2008
Quote:
Originally Posted by Ivanet View Post
Hi again, now I know where was the problem. As you can see in my first post, the MRFZones file contained a description of the rotating patches, but no definition of the non-rotating patches. That is wrong. Actually the rotating patches do not need to be defined here, since it will be assumed that all the cells defined within the cellSetDict are rotating cells. It is however important to define which patches do not rotate (inlet, outlet and outer walls).
Cheers
Ivan
HI Ivan

Can I ask you some question?
1. In your analysis, is there sliding mesh (OGI) technique that you used?
2. If i want to change rotation axis which will be changed with time dependent, it is possible?

I really appreciate your help. Thank you so much.

Tran
trantoan2008 is offline   Reply With Quote

Old   November 17, 2011, 08:40
Default
  #6
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Hi Tran,
no, in my analysis I did not use any kind of sliding interface.
If you want to use MRFSimpleFoam you only need to define which regions of your domain rotate and which regions do not rotate. Here is explained in detail how to do it:
http://openfoamwiki.net/index.php/Si...vaned_diffuser

MRFSimpleFoam is a steady state solver. If you need a time dependant simulation, you should use a transient solver like e.g. pimpleDyMFoam. In that case you might use a GGI (general grid interface) in order to account for the rotation.
If you want to change the axis of rotation during the simulation I think you need to stop the simulation, modify the axis of rotation in your model and them restart the simulation again.
Greetings
Ivan
Tobias Adam likes this.
Ivanet is offline   Reply With Quote

Old   August 22, 2013, 00:32
Default
  #7
New Member
 
QuocThien
Join Date: Apr 2013
Posts: 9
Rep Power: 4
neiht is on a distinguished road
Can u explain more clearly? I have the same problem and I dont know how to solve
neiht is offline   Reply With Quote

Old   September 7, 2014, 12:08
Default
  #8
New Member
 
Nolwenn
Join Date: Apr 2010
Posts: 23
Rep Power: 7
Nolwenn is on a distinguished road
Hi Ivan,

Did you solve your problem ? I have the same kind of problem, even if I specify inlet, outlet and side patches as fixed ...

Nolwenn
Attached Images
File Type: jpg rotating-nonRotating.jpg (25.8 KB, 42 views)
Nolwenn is offline   Reply With Quote

Old   May 22, 2015, 09:17
Default
  #9
Senior Member
 
M. Montero
Join Date: Mar 2009
Location: Madrid
Posts: 112
Rep Power: 8
be_inspired is on a distinguished road
Similar problem here.

Any information about how to fix the problem?
In OF2.3.x (after fvOptions was included) it is not needed to perform any faceSet operation. Only cellSet is needed I think

After MRFZone, the swirl of the flow is lost and wake rotation is lost?
be_inspired is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Using starToFoam clo OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 33 September 26, 2012 04:04
MRFSimpleFoam: wrong boundary conditions on rotating walls cves OpenFOAM Bugs 3 May 3, 2010 03:38
StarToFoam error Kart OpenFOAM Meshing & Mesh Conversion 1 February 4, 2010 05:38
Rotating region of a centr. pump - Counter R wall Emre CFX 0 September 20, 2007 09:58
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19


All times are GMT -4. The time now is 22:32.