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

FSI porous media thin shell

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

Like Tree1Likes
  • 1 Post By hjasak

Reply
 
LinkBack Thread Tools Display Modes
Old   May 21, 2008, 16:14
Default HI all, I've had a quick br
  #1
New Member
 
Novak Elliott
Join Date: Mar 2009
Posts: 6
Rep Power: 8
novak is on a distinguished road
HI all,

I've had a quick browse through the FSI posts and Porous media posts and I have the following question:

Can OpenFOAM do both together, in a 3-domain problem?

e.g., a fluid-saturated poroelastic cylinder, sheathed by a thin flexible permeable membrane, surrounded by an annulus of fluid contained within an outer rigid cylinder.

The inner cylinder would be governed by the Biot equations of poroelasticity, the outer fluid would obviously be the standard Navier-Stokes equations, the intervening membrane could be modelled with thin-shell theory with the transmembrane flow handled by Darcy's law at the boundary condition.

I know both icoStructFoam and icoFsaFoam are possibilities for the FSI but as a composite problem does this sound feasible?

cheers,
Novak.
novak is offline   Reply With Quote

Old   May 22, 2008, 03:35
Default Hi Novak, This is a bit bor
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Hi Novak,

This is a bit borderline. Fluids are no problem, including porous media. Having a porous membrane in the flow is also OK and the automatic mesh motion will take care of deformation of the fluid mesh.

However, doing stress analysis on a thin shell is a problem. FVM will not do it to the level I'd be happy with (maybe Finite Area would be better, let's see what Zeljko says), and the FEM solver does not do discretisation for shells. If you delegate thin shell stress analysis to another tool, the rest can be done in OpenFOAM. As an example, several people last year did a flow around sails on the last Workshop.

Enjoy,

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

Old   May 27, 2008, 17:15
Default Hi Hrv, Thanks for your rep
  #3
New Member
 
Novak Elliott
Join Date: Mar 2009
Posts: 6
Rep Power: 8
novak is on a distinguished road
Hi Hrv,

Thanks for your reply. I found the following thesis report on FSI with OpenFOAM:
http://powerlab.fsb.hr/ped/kturbo/Op...RIVOLA_FSI.pdf
(linked from the OpenFOAM page http://foamcfd.org/resources/theses.html)

The relative merits of the two solvers were compared:
1. IcoFsiFoam:
+ integrated automesh motion capacity to minimise mesh degenration
- only allows for a domain with 2 regions
- difficult to use(?)
2. IcoStructFoam
+ easy to use do to better architecture(?)
- only handles small structural deformations
- only allows for a domain with 2 regions
Generally:
* OpenFOAM structural equations only handle homogeneous structures
* OpenFOAM's ability to handle large displacements for thin-shell structures is limited by small cell sizes and small timestep sizes hence long computation times
=> a 3rd party structural solver (IMPACT) was coupled to OpenFOAM to achieve the required FSI solution of a 3-domain problem with a thin polymer membrane.

Can you comment on any of these points?

cheers,
Novak.
novak is offline   Reply With Quote

Old   May 28, 2008, 19:00
Default Hello, To your points: i
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Hello,

To your points:

icoFsiFoam vs. icoStructFoam. I wrote the early versions of icoFsiFoam, which has since become Zeljko's problem. It will currently take non-linear materials in large deformation, zonal materials, crack propagation, contact stresses and self contact. This is currently a "paper factory" and with my new block solver it will become massively more powerful. I cannot comment on icoStructFoam, but I'm sure Bernhard will oblige.

A limit to 1 fluid and 1 solid is pure lazyness: you can have as many solids as you like (under one zone if solving same equations (even with different material properties), or simply generalise the FSI interface into a PtrList and run as many as you like. BTW, this is what I did for contact stresses a few years back

large displacement for think shells: do I REALLY have to? I've got the solver machinery, this needs to go into a FEM solver (alive and well in the dev branch). but the matrices are very difficult to solve and you need special solvers. I think I've got enough, but adding it to OpenFOAM is a pretty major project (= money). Why not just use another code if you can live with explicit coupling + Zeljko's adaptive relaxation tricks?

Regarding the coupling to another solver, have a look at the sail simulation in OpenFOAM at the Second OpenFOAM Workshop last year. I think the slides are also available:

http://www.openfoamworkshop.org/2007/index.php?title=Coupled_Simulations_and_Flu id-Structure_Interaction

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/WorkshopZagrebJun2007/presentations/a bstracts/abstractRussoZagreb2007.pdf

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/WorkshopZagrebJun2007/presentations/s lides/slidesKaracZagreb2007.pdf

Hope this is enough for a first shot,

Hrv
hua1015 likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 29, 2008, 04:48
Default Hi! @icoStructFoam: This th
  #5
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi!

@icoStructFoam: This thing is better not commented on. I wrote it as a feasiblitiy study and decided to publish it AS AN EXAMPLE. I personally don't work currently on FSI (that was some stuff I managed to pass on). The basic code was written around v1.2 (or 1.1? I can't remember) and since then only adapted to compile on new versions. Some of the stuff I wouldn't write the way I wrote it back then.
Yes. It only handles small deformations.
Yes. Materials can only be homogenous. But that can be easily changed by changing the constants to fields.

The latest version of iceStructFoam is in the extend-svn. If somebody fells like cleaning it up or working it into a generally usable solver: drop me a mail and we will work something out

Bernhard
__________________
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   January 6, 2009, 16:59
Default Hello! We develloped a nice F
  #6
New Member
 
Hansjoerg Seybold
Join Date: Mar 2009
Posts: 16
Rep Power: 8
hansjoerg is on a distinguished road
Hello!
We develloped a nice FEM code for thin shells
and large deformations based on a new technique for C1-continuous FEM
on arbitrary curved manifolds.

Where would you suggest to start to couple the code to a OpenFOAM fluid solver.

How can the remeshing be done efficiently/accurately
in FOAM

The surface mesh could be provided by the FEM mesh
(2D but curved space described by subdivision surfaces)

Thanks a lot
Hansjoerg
hansjoerg 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
Free media&porous media.Big changes in properties. Isi Main CFD Forum 1 July 14, 2008 07:18
shell conduction @ thin walls Jiri Beran FLUENT 0 May 18, 2008 14:08
Modeling thin perforated plates as porous media Mike FLUENT 0 August 21, 2007 04:16
About Porous wall for thin surface. windhair1 CFX 2 October 14, 2003 05:44
Plastic Flow, thin shell type Dave Pinella Main CFD Forum 0 December 4, 2001 10:27


All times are GMT -4. The time now is 13:15.