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

MRFSource no more available in OpenFOAM 4?

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

Like Tree1Likes
  • 1 Post By akidess

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 31, 2016, 00:11
Default MRFSource no more available in OpenFOAM 4?
  #1
Member
 
Al
Join Date: Jul 2013
Location: Japan
Posts: 47
Blog Entries: 3
Rep Power: 13
donQi is on a distinguished road
Hello,

in the past, when launching simpleFoam simulations with MRF, I used to write in the fvOptions file :

Code:
MRF1
{
    type            MRFSource; 
    active          true;
    selectionMode   cellZone;
    cellZone        cylinder_inner;

    MRFSourceCoeffs
    {
        origin      (0 0 0);
        axis        (-1 0 0);
        omega     90;
    }
}
in OpenFOAM 2.4 the source file was here:
src/fvOptions/sources/derived/MRFSource/MRFSource.C

but in OpenFOAM 4 is no more there. I would like to know what do you currently use to set an MRF source in OpenFOAM 4?
donQi is offline   Reply With Quote

Old   August 31, 2016, 03:37
Default
  #2
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 29
akidess will become famous soon enough
Have a look at the tutorials. The relevant file is constant/MRFProperties.
donQi likes this.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
akidess is offline   Reply With Quote

Old   August 31, 2016, 04:39
Default
  #3
Member
 
Al
Join Date: Jul 2013
Location: Japan
Posts: 47
Blog Entries: 3
Rep Power: 13
donQi is on a distinguished road
Thank you very much Anton.

for future readers, I copy here an example from the tutorial:
incompressible/simpleFoam/mixerVessel2D/constant/MRFProperties

Origin, axis and omega of the MRF zone are now set in the constant/MRFProperties file:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  plus                                  |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      MRFProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

MRF1
{
    cellZone    rotor;
    active      yes;

    // Fixed patches (by default they 'move' with the MRF zone)
    nonRotatingPatches ();

    origin    (0 0 0);
    axis      (0 0 1);
    omega     104.72;
}

// ************************************************************************* //
donQi is offline   Reply With Quote

Old   July 26, 2017, 12:23
Default
  #4
Member
 
Jason G.
Join Date: Sep 2009
Location: St. Louis, IL
Posts: 89
Rep Power: 16
JasonG is on a distinguished road
I recently upgrade from OF 2.4, and now I am also having issues running a past model on OF 3.0. I am attempted to model a fluid region that has an impeller to increase the static pressure.

The model has two zones: c0 = impeller domain, c1 = everything else. The previous fvOptions file looked like:

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


#include        "../0/initialConditions"

MRF1
{
    type            MRFSource;
    active          true;
    selectionMode   cellZone;
    cellZone        c0;

    MRFSourceCoeffs
    {
        // Fixed patches (by default they 'move' with the MRF zone)
        active          true;
	nonRotatingPatches ( inlet_1 outlet_1 boundary diffuser );   //patches need to be ones not rotating in actual frame
	origin (0 0 0);
        axis   (0 0 1);
     //  omega  constant 638.7905062;
	
        omega table
        (
        (0 0)
        (100 0)
	(200 $omega)
	(10000 $omega)
        );


		
    }
}


// ************************************************************************* //

Per the above, I attempted to run the following:

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


#include        "../0/initialConditions"

MRF1
{

//    selectionMode   cellZone;
    cellZone        c0;
    active          yes;

    // Fixed patches (by default they 'move' with the MRF zone)

     nonRotatingPatches ( inlet_1 outlet_1 boundary diffuser );   //patches need to be ones not rotating in actual frame
    origin (0 0 0);
    axis   (0 0 1);
    //  omega  constant 638.7905062;
    omega table
    (
    (0 0)
    (100 0)
    (200 $omega)
    (10000 $omega)
    );


		

}


// ************************************************************************* //

When I examine my two different log files, I notice the following:
OF 3.0:
Code:
Creating MRF zone list from MRFProperties
    creating MRF zone: MRF1
No finite volume options present
OF 2.4:

Code:
Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type MRFSource
    Source: MRF1
    - applying source for all time
    - selecting cells using cellZone c0
    - selected 690499 cell(s) with volume 1.49875838



The model begins looking normal, but then suddenly crashes during the Omega ramping. I reviewed results just after the ramping, and the rotational velocity appears to correctly apply to only the impeller fluid domain. Just as the solution crashed, it appeared it was applying velocities to the entire domain. Any help is greatly appreciated!


EDIT: Honing in on my results just as the solution crashes, I am able to see that a few elements where the pressure field goes unbounded (outside of the MRF zone). I assume this is likely an issue with internal solver controls slightly changing b/t the two OF versions, as I am utilizing the same mesh file for both runs.
JasonG is offline   Reply With Quote

Old   February 20, 2019, 21:31
Default
  #5
New Member
 
Chenguang Zhang
Join Date: Jul 2012
Location: Baton Rouge Louisiana
Posts: 15
Rep Power: 13
Taozi is on a distinguished road
I am puzzled as to why the openfoam developers keep shoveling things around. To me this change adds no new functionality, only creates annoying compatibility issues that cost researchers precious time to fix.
Taozi is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Frequently Asked Questions about Installing OpenFOAM wyldckat OpenFOAM Installation 3 November 14, 2023 12:58
OpenFOAM Foundation releases OpenFOAMŪ 3.0.0 CFDFoundation OpenFOAM Announcements from OpenFOAM Foundation 1 November 7, 2015 16:16
OpenFOAM Foundation Releases OpenFOAM v2.3.0 opencfd OpenFOAM Announcements from OpenFOAM Foundation 3 December 23, 2014 04:43
Suggestion for a new sub-forum at OpenFOAM's Forum wyldckat Site Help, Feedback & Discussions 20 October 28, 2014 10:04
64bitrhel5 OF installation instructions mirko OpenFOAM Installation 2 August 12, 2008 19:07


All times are GMT -4. The time now is 00:47.