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

Simulate flow field of moving body by dynamic meshes

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 9, 2006, 23:09
Default This problem is shown as follo
  #1
Member
 
Luckyluke
Join Date: Mar 2009
Posts: 51
Rep Power: 7
luckyluke is on a distinguished road
This problem is shown as follows:

,
or similar 3D case.

I wonder if the present OpenFOAM1.2 have the solver for such problem. If the FOAM1.2 has not got this feature, how should I do? From whcih exsisted solver should I carete a new one? Give me some ideas, please.

Thanks all. This is not my project, but I am interested in this simulation. The Fluent6 did have this feature.
luckyluke is offline   Reply With Quote

Old   January 9, 2006, 23:23
Default It is should be noted that the
  #2
Member
 
Luckyluke
Join Date: Mar 2009
Posts: 51
Rep Power: 7
luckyluke is on a distinguished road
It is should be noted that the mesh topology will change along the motion.
luckyluke is offline   Reply With Quote

Old   January 10, 2006, 04:08
Default Fluent is only capable of solv
  #3
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 8
lr103476 is on a distinguished road
Fluent is only capable of solving these dynamic mesh problems with first order methods marching in time.

By the way, the mesh you showed is far too coarse and the solution by far not very accurate. The movement of the cells from on timestep to the next restrict the choice of this timestep. So higher order time integration techniques are very welcome for this type of problems.

I am investigating if OpenFOAM can do the job for 2d flapping wings, and later for 3d wings. It is also very dependent on the Reynolds number. I am studying flapping wings at Re=110. Then, the behavior of the second order discretized convective flux at these changing meshes may play an important role.

Goodluck
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   January 10, 2006, 04:13
Default Hi Frank, Just for my info
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,731
Rep Power: 20
hjasak will become famous soon enough
Hi Frank,

Just for my info - did you get it to run correctly? Do you have topological changes as well or just mesh motion?

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

Old   January 10, 2006, 04:26
Default Hi, I am still working on a
  #5
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 8
lr103476 is on a distinguished road
Hi,

I am still working on a proper set-up of space and time discretization techniques using static cylinders at Re=150. Just for validation. The plan is to extend to moving cylinders using only mesh motion at first. Later also topological changes may be implemented. And, if possible, also some body forces, which depends on the complexity of the wing motion in 3d.

When I succeed in simulating flapping wings/cylinders I will post the results.

Could you maybe comment on this? Maybe you've got some tips on the solver settings at Re=150?

Thanks, Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   January 10, 2006, 04:37
Default Heya, For the test above, y
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,731
Rep Power: 20
hjasak will become famous soon enough
Heya,

For the test above, you don't need much: take icoFoamAutoMotion and the automatic mesh motion solver will do the job nicely. The second-order discretisation on moving meshes has been tested in detail by my colleague and a former student dr. Tukovic (and he IS thorough) - you will find the details in his PhD Thesis (unfortunately not yet translated to English in full, but I'm sure he can answer questions).

In order to use the automatic mesh motion solver all you need to do is to prescribe the motion of the boundary; the rest is done for you automatically. :-)

For topological changes, I would really need to see the mesh - it very much depends on what the domain, mesh and motion looks like. If you'd like to force the one above to very large deformations, I would have some layer addition/removal in a circle/cylinder around the wing. You would probably want to use a combination of automatic mesh motion and topo changes (ask Tomasso about what we did for in-cylinder flows).

Finally, setting up the solver on Re=150 should not be too tricky. Decent (second order in space and time) spatial discretisation will be fine. You may wish to have a go at my bounded second order spatial scheme if you're worried about numerics. Check that PISO is converging... No further thoughts, really.

Please keep me posted,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is online now   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
P U T field solving in solid and liquid two meshes In parallel kar OpenFOAM Running, Solving & CFD 2 February 20, 2008 05:18
Moving mesh turbulent incompressible flow of complex meshes philippose OpenFOAM Running, Solving & CFD 5 March 13, 2007 04:35
simulate CO2 from human body DW FLUENT 0 June 3, 2005 12:41
Dynamic Meshes F Bos FLUENT 1 July 6, 2004 05:59
SIMULATE A THOTTLE BODY Pierre Rutten FLUENT 0 March 7, 2002 09:29


All times are GMT -4. The time now is 03:28.