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

Suggestions for a fan

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 7, 2006, 05:20
Default Hi! I'd like to simulate a fa
  #1
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 214
Rep Power: 9
fra76 is on a distinguished road
Hi!
I'd like to simulate a fan rotating within a bigger mesh with OpenFOAM.
The question is: which is the best way to do this? I mean, sliding meshes, or defining a rotating part of the grid, or setting a prevalence and a swirl as boundary condition...
Francesco
fra76 is offline   Reply With Quote

Old   April 7, 2006, 06:19
Default Depends whether the outer stat
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Depends whether the outer static part influences the solution around the fan. In mixer vessels for example, the outside part will have baffles etc. and for an accurate simulation you need a sliding interface. On the other hand, if your case is something like a ceiling fan in a room, just mesh it statically and spin the whole thing.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   April 7, 2006, 06:32
Default Hi Hrvoje, What do you mee
  #3
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Hi Hrvoje,

What do you meen by "spin the whole thing"?

Eric
lillberg is offline   Reply With Quote

Old   April 7, 2006, 06:35
Default I mean add the centrifugal and
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
I mean add the centrifugal and Coriolis force into the momentum/pressure coupling and specify the conditions in the rotating frame of reference.

Does that sound OK?

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   April 7, 2006, 06:43
Default Oh, of course... For a whil
  #5
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Oh, of course...

For a while I thought you had implemented even more ingenious ways to transform the mesh :-)

/E
lillberg is offline   Reply With Quote

Old   April 11, 2006, 09:53
Default Hi again! I've decided to try
  #6
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 214
Rep Power: 9
fra76 is on a distinguished road
Hi again!
I've decided to try perhaps the hardest way, but I'd like to simulate the fan with a sliding interface.
Is there a tutorial which explains how to use this feature?
Thanks a lot
Francesco
fra76 is offline   Reply With Quote

Old   April 14, 2006, 02:12
Default Hello, You probably already
  #7
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello,

You probably already found this one, but anyway. You could have a look at the mixer2D case inside icoTopoFoam.

I am currently trying to simulate a fan with sliding meshes as well in 3D that is, but I keep having problems with the convergence. I tried several b.c.'s but it did not help. After a while the solution blows up, courant no's go to infinity. I also tried to increase my domain but, this did help either. I thought it might be a problem with my mesh, so I made another testcase, but also for this case the courant no blows up. The mesh I'm using is not of perfect quality, by far not. Could this be the reason for the solution to blow up? Is it possible to get the solution to convergence even on a not so good mesh?
Background info for this simulation is that I would like to simulate a helicopter. So I wanted to start by simulating a rotating fan :-)

kind Regards
Guido
guido_adriaensen is offline   Reply With Quote

Old   April 19, 2006, 05:49
Default Hello, If you'are intereste
  #8
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello,

If you'are interested I now have made a mixer3D case, based upon the mixer2D case. It is not exactly the 2D case extracted in the third dimension, it only has a fan. I have done simulations for 10RPM, but also for 3000RPM.




I would now like to expand the simulation to turbFoam, I would like to create something like turbTopoFoam. Could anybody instruct me where to start looking, what do I need to modify?

kind regards
Guido
guido_adriaensen is offline   Reply With Quote

Old   April 19, 2006, 14:09
Default Hi guido, I've already buil
  #9
New Member
 
Andrea Palazzi
Join Date: Mar 2009
Posts: 15
Rep Power: 8
giampippetto is on a distinguished road
Hi guido,

I've already built a turbTopoFoam application somehow (i'm not very expert in CFD), but in my tests it always diverges, so for the moment I've put it aside. Moreover the dynamic mesh thing seems to have changed from 1.2 to 1.3, I aven't had time yet to look into 1.3 so I'm not sure that my code is still valid. However if you're interested I can send you my source code, let me know.

Bye
Andrea
giampippetto is offline   Reply With Quote

Old   April 20, 2006, 01:54
Default Hello Andrea, I would be ve
  #10
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello Andrea,

I would be very interested in your application. As I understand it has been written for OF1.2, I'm currently still working with that version as well, so that should not cause any problem.

I haven't made the switch to OF1.3 yet, so I cannot yet comment on the changes regarding dynamic meshes. Maybe some of the experts around here? Is it recommended to make the switch to OF1.3, if so why?

thank you
Guido
guido_adriaensen is offline   Reply With Quote

Old   April 20, 2006, 06:35
Default Guido: If you want to increase
  #11
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Guido: If you want to increase the speed of your calculations by 10% without increasing the clock-rate of your computer, then I would recommend OF. For other reasons to upgrade: see the README-file.

(and so far I've seen no bad effects of upgrading)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   May 3, 2006, 09:22
Default Hello, I have added mixerFv
  #12
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello,

I have added mixerFvMesh to rhoTurbFoam and created a kind of rhoTurbTopoFoam. The application runs, but I would like to know whether I should make adjustments to the equations that are being solved, or is this automagically oke?
If have run the mixer2D tutorial and it works, at least the propellor rotates and the solution does not diverge.
I don't know if it is relevant, but I'm using OF1.2
Is it really this simple? If so, great job guys! If not where to start? Any hints?

kind regards
Guido
guido_adriaensen is offline   Reply With Quote

Old   May 3, 2006, 09:38
Default Yup, it is that simple. If you
  #13
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Yup, it is that simple. If you're getting the solution and using the pressure-velocity bits like in icoTopoFoam, the turbulence will just slot into place.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 3, 2006, 09:59
Default Hi Hrv. That is what I have
  #14
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hi Hrv.

That is what I have been doing!
You have done a great job, my compliments. OF keeps on amazing me :-)

kind regards.
Guido
guido_adriaensen is offline   Reply With Quote

Old   May 29, 2006, 08:51
Default Hi, I'm still working on th
  #15
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 214
Rep Power: 9
fra76 is on a distinguished road
Hi,

I'm still working on the fan, without sliding interfaces.
I'd like to build a turbulent, steady state solver for a still volume containing a rotating zone.
I don't know if I'm on the right way, but I've deduced this equations, in order to modify simpleFoam:


volVectorField Fcent = (Omega ^ (Omega ^ mesh.C()));
volVectorField Vtang = (Omega ^ mesh.C());

[...]

tmp<fvvectormatrix> UEqn
(
fvm::div(phi, U)
+ turbulence->divR(U)
+ (2*Omega ^ U)
+ Fcent
+ fvm::div(phi, Vtang)
+ turbulence->divR(Vtang)
+ (2*Omega ^ Vtang )
);

UEqn().relax();

solve(UEqn() == -fvc::grad(p));

[...]


where Omega is a (constant) vector field read from an input file. The corresponding section in createField.H is:


Info << "Reading field Omega\n" << endl;
volVectorField Omega
(
IOobject
(
"Omega",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);


Well, the error I get, after adding the entries corresponding to "(Omega^C)" in the divSchemes and laplacianSchemes sections in the fvSchemes file, is:


Starting time loop

Time = 0.01



--> FOAM FATAL ERROR : gradientInternalCoeffs cannot be called for a calculatedFvPatchField.
You are probably trying to solve for a field with a calculated boundary conditions.

From function calculatedFvPatchField<type>::gradientInternalCoef fs() const
in file fields/fvPatchFields/basicFvPatchFields/calculated/calculatedFvPatchField.C at line 172.

FOAM exiting


I read in the message board that this is an error related to some misdeclaration of a boundary, but I've checked all my input files...

What can be wrong?

Francesco
fra76 is offline   Reply With Quote

Old   July 4, 2006, 05:51
Default Hi Guido, How can I get you
  #16
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
Hi Guido,

How can I get your mixer3D case?

I'm trying to understand how to set up a sliding grid interface in OF1.3. Did you port your code and case to OF1.3?

Can you show which lines you changed in icoTopoFoam to make it into turbTopoFoam?

Hċkan.
hani is offline   Reply With Quote

Old   January 18, 2008, 05:31
Default Hi Hrv, you wrote: "I
  #17
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi Hrv,

you wrote:

"I mean add the centrifugal and Coriolis force into the momentum/pressure coupling and specify the conditions in the rotating frame of reference."

Which conditions should I specify? Can you better explain what is the rotating frame of reference?

I'm quite new to this kind of problems, so please be patient with me

Thank you in advance

Francesco
francesco_b is offline   Reply With Quote

Old   January 18, 2008, 10:57
Default Hi Francesco for the start
  #18
Senior Member
 
Join Date: Mar 2009
Posts: 248
Rep Power: 9
jaswi is on a distinguished road
Hi Francesco

for the start please go through the material on this link.

http://venus.imp.mx/hilario/SuperComputo/Fluent.Inc/manuals/fluent5/ug/html/node 552.htm

Once you know what rotating frame of reference means and how the momentum equations are modified for this purpose , you will be able to ask specific questions and believe me people do help on this forum.

Just be more specific.

Hope that helps

Start FOAMing NOW :-)

Best Regards
Jaswinder
jaswi is offline   Reply With Quote

Old   January 23, 2008, 12:58
Default Hi Jaswinder, Thank you for
  #19
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi Jaswinder,

Thank you for the material, very interesting

My case is like the one in fig. 16.3.2; the problem is that I don't know how to impose the boundary condition on the interface between the two reference frames, I looked in the mixerVessel2D tutorial but I could not find the answer. I think I'm missing something, any hints?

Thanks in advance

Francesco
francesco_b is offline   Reply With Quote

Old   January 29, 2008, 07:41
Default Hi Francesco Sorry for the
  #20
Senior Member
 
Join Date: Mar 2009
Posts: 248
Rep Power: 9
jaswi is on a distinguished road
Hi Francesco

Sorry for the late reply.

If there are no problems in revealing the geometry to others then mail me the case setup . I will take a look at it and try to resolve the issue.

As far as i have understood the mixer setup in openfoam, there is no need to define a boundary condition on the interface. The way you define your zones is important.

Regarding the mixerVessel2D case, which one are you using as it has been set up using two approaches in the Prof. Jasak's dev version.

- MRF using the static mesh approach
- icoDynFOAM using the dynamic mesh appraoch (look for mixerVessel2D case under the icoDynFOAM tutorials)

Best Regards
Jaswinder
jaswi 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
CFD options/ suggestions? MK Main CFD Forum 9 July 31, 2008 15:24
Going to buy RAM, suggestions? HSeldon FLUENT 3 May 21, 2007 08:01
Need some suggestions Dazhu Main CFD Forum 0 October 3, 2006 10:11
Suggestions for convergence David CFX 4 November 12, 2002 02:50
Any suggestions? Montresor FLUENT 3 June 29, 2001 07:21


All times are GMT -4. The time now is 07:28.