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

2D VAWT simulation - rpm ramp function?

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

Like Tree2Likes
  • 2 Post By linnemann

Reply
 
LinkBack Thread Tools Display Modes
Old   July 12, 2013, 07:33
Default 2D VAWT simulation - rpm ramp function?
  #1
Member
 
Anand Lobo
Join Date: Jun 2013
Posts: 56
Rep Power: 4
Boloar is on a distinguished road
Hi all,

I successfully made a 2D VAWT simulation at a constant specified RPM and wind speed.
I'd like to try a slight modification to it, namely: start the RPM at 0 and ramp it up to a given RPM, with wind speed remaining constant, so I can see the airflow interaction. How would I go about doing this?

For info: I used the AMI implementation from the pimpleDyMFoam/propeller tutorial. Based on my rudimentary programming skills, I hope I'd only need to insert some sort of ramp function into dynamicMeshDict? Or would I need to mess with the source code?

Your input is appreciated!
Boloar is offline   Reply With Quote

Old   July 25, 2013, 04:03
Default Is it possible at all?
  #2
Member
 
Anand Lobo
Join Date: Jun 2013
Posts: 56
Rep Power: 4
Boloar is on a distinguished road
No replies at all makes me think this is an impossible request, but I'd like confirmation of the fact in that case.
Boloar is offline   Reply With Quote

Old   July 25, 2013, 14:31
Default
  #3
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Hi

It is not possible using the built-in methods.

you can look at the openfoam code for solidBodyMotionFunctions

https://github.com/OpenFOAM/OpenFOAM...otionFunctions

You can take the axisRotationMotion and make a new library that could take a table as input. Similar to as how you can use a table for the BC's

https://github.com/OpenFOAM/OpenFOAM...ataEntry/Table

I know this might not be what you were looking for but that is my best bet.

I must say I do not know if it is possible to change the RPM while the case is running. That should be easy to test with your case. You might also run into problems if running in parallel.

There is also the oscillatingRotatingMotion code you could take a look at, that is definitely time varying.

https://github.com/OpenFOAM/OpenFOAM...RotatingMotion
SailorLiu and Boloar like this.
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   July 27, 2013, 03:28
Default
  #4
Member
 
Anand Lobo
Join Date: Jun 2013
Posts: 56
Rep Power: 4
Boloar is on a distinguished road
Quote:
Originally Posted by linnemann View Post
Hi

It is not possible using the built-in methods.

you can look at the openfoam code for solidBodyMotionFunctions

https://github.com/OpenFOAM/OpenFOAM...otionFunctions

You can take the axisRotationMotion and make a new library that could take a table as input. Similar to as how you can use a table for the BC's

https://github.com/OpenFOAM/OpenFOAM...ataEntry/Table

I know this might not be what you were looking for but that is my best bet.

I must say I do not know if it is possible to change the RPM while the case is running. That should be easy to test with your case. You might also run into problems if running in parallel.

There is also the oscillatingRotatingMotion code you could take a look at, that is definitely time varying.

https://github.com/OpenFOAM/OpenFOAM...RotatingMotion
Thank you linneman, much appreciated. I'll check these out now.

This might be a good thing to put on the to-do list for future OF builds, assuming it isn't already - time-varying parameters would be useful to no end.
Boloar is offline   Reply With Quote

Old   July 30, 2013, 07:46
Default
  #5
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Hi I think you are going to like this as Henry has added some of the stuff you would like.

He has added the possibility to change the omega on run-time.

More here

https://github.com/OpenFOAM/OpenFOAM...e559f51eeb8084

EDIT: See next post for table input
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.

Last edited by linnemann; August 2, 2013 at 13:39.
linnemann is offline   Reply With Quote

Old   August 2, 2013, 13:34
Default
  #6
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Ehm I think Henry has come to your rescue :-)

I can see that from the new tutorial for interPhaseChangeDyMFoam that he uses the table as input for omega. So just upgrade to the latest git and you are good to go.

https://github.com/OpenFOAM/OpenFOAM...ynamicMeshDict

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh   solidBodyMotionFvMesh;

motionSolverLibs ( "libfvMotionSolvers.so" );

solidBodyMotionFvMeshCoeffs
{
    cellZone        innerCylinderSmall;

    solidBodyMotionFunction  rotatingMotion;
    rotatingMotionCoeffs
    {
        origin      (0 0 0);
        axis        (0 1 0);
        omega       table
        (
            (0    0)
            (0.01 419)
            (100  419)
        );
    }
}


// ************************************************************************* //
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   August 3, 2013, 03:40
Default
  #7
Member
 
Anand Lobo
Join Date: Jun 2013
Posts: 56
Rep Power: 4
Boloar is on a distinguished road
Quote:
Originally Posted by linnemann View Post
Ehm I think Henry has come to your rescue :-)

I can see that from the new tutorial for interPhaseChangeDyMFoam that he uses the table as input for omega. So just upgrade to the latest git and you are good to go.

https://github.com/OpenFOAM/OpenFOAM...ynamicMeshDict
Holy moly, that is awesome. It'd have to be a big table if I want fine-grain control over the RPM, but this is perfect for starters. My thanks to Henry, and thanks to you Linneman for keeping me apprised on this.
Boloar is offline   Reply With Quote

Old   August 3, 2013, 04:37
Default
  #8
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Hi

The table makes linear interpolation between the entries so it does not have to be that big.

Glad to help
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   August 3, 2013, 04:42
Default
  #9
Member
 
Anand Lobo
Join Date: Jun 2013
Posts: 56
Rep Power: 4
Boloar is on a distinguished road
That's good, I didn't think about interpolation.
Now all I need is a computer that's somewhat less than 5 years old, to do the simulations faster, hahah

Thanks again!
Boloar 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
2D vawt simulation meshing and fluent error daysley FLUENT 5 April 15, 2014 19:51
swak4Foam installation problem Claudio87 OpenFOAM 9 May 8, 2013 10:20
Compile problem ivanyao OpenFOAM Running, Solving & CFD 1 October 12, 2012 09:31
Error with Wmake skabilan OpenFOAM Installation 3 July 28, 2009 00:35
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51


All times are GMT -4. The time now is 07:10.