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

Patch end points mesh motion and movingWallVelocity

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

Like Tree5Likes
  • 2 Post By pbo
  • 1 Post By pbo
  • 1 Post By WiWo
  • 1 Post By TengWU

Reply
 
LinkBack Thread Tools Display Modes
Old   March 21, 2008, 12:21
Default Hi, Happy Easter to everyon
  #1
pbo
Member
 
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 8
pbo is on a distinguished road
Hi,

Happy Easter to everyone!

If you're not busy egg hunting, I have a couple of questions for you:

1) what happens to the end points shared by 2 contiguous patches, when one patch moves and the other one next to it does not?
Is the displacement of the shared points a blend of the moving patch and the still patch?

2) Does the movingWallVelocity BC for U have a destabilizing effect on the computation?

In my case, playing around with icoFsiFoam, the computation blows in a few time steps when using movingWallVelocity, but it does not when using a fixedValue of (0 0 0) (which is a physically-wrong BC for a deforming patch though).

Isn't one better off by writing the displacement velocities of the deforming patch in a non uniform list after the fixedValue BC, instead of using movingWallVelocity?

3) Will Zeljko's updated Lagrangian finite volume method solver be released in a near future in OpenFOAM-dev? (the current icoFsiFoam relies on a small strain deformation solver -- stressedFoam -- so any large deformation in the solution is to be interpreted with caution)

Cheers,

Patrick
immortality and neiht like this.
pbo is offline   Reply With Quote

Old   March 21, 2008, 13:38
Default Hello Patrick, 1) You have
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,762
Rep Power: 21
hjasak will become famous soon enough
Hello Patrick,

1) You have a problem with consistency of a boundary condition in mesh motion: a "lower" (eg. slip), will be over-ridden by the "higher" (eg. fixed value).

2) No need: moving wall velocity is an absolutely consistent version of a fixed value velocity. It is done because the code can calculate the wall-normal motion flux better than anything else.

Have a look at the flux field for the boundary - do you have a non-zero flux for it?

3) Yes, we are writing some papers about it. This is the main reason I am reluctant to release the tutorial, 'cause the new code from Zeljko is so much better. This will definitely come out in SVN at some stage, but the Eccomas, Commodia and journal papers are not out yet.

This is what I propose to do: I will give you a tutorial for icoFsiFoam as it stands without checking it in. Please find flappingConsoleSmall_HJ_21Mar2008.tgz in

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/run/

It runs for me... but not too many questions please.

Enjoy,

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

Old   March 22, 2008, 02:56
Default Hrv, thanks for the swift r
  #3
pbo
Member
 
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 8
pbo is on a distinguished road
Hrv,

thanks for the swift reply.
The flappingConsole case runs fine for me as well :-)

I understand now why my computations were diverging:
The case I was trying to run with icoFsiFoam (aeroelastic deformations of a gliding dragonfly wing section) was actually well set-up, but because of the low stiffness and density I specified in the mechanicalProperties file (well, can't do otherwise with membrane wings), the weak coupling algorithm became unstable. So, the movingWallVelocity BC had nothing to do with the unstability (which was delayed by switching to fixedValue BC). I should have not doubted it!

At some point, I am going to redo those "insectaneous" FSI simulations with a strong coupling algorithm.

Cheers,

Patrick
chathanm likes this.
pbo is offline   Reply With Quote

Old   September 1, 2008, 08:50
Default I am working on a moving mesh
  #4
New Member
 
Anant Grewal
Join Date: Mar 2009
Posts: 6
Rep Power: 8
agrewal is on a distinguished road
I am working on a moving mesh problem for transonic flow using sonicFoamAutoMotion. I would like to run a inviscid case. In that case how to I ensure that my movingWallVelocity BC permits slip?
Thanks
Anant
agrewal is offline   Reply With Quote

Old   March 29, 2010, 13:35
Default
  #5
Member
 
Wolfgang W.
Join Date: Nov 2009
Location: Switzerland
Posts: 57
Rep Power: 7
WiWo is on a distinguished road
Hello everyone,

I hope this is the right place to post an issue I have concerning the movingWallvelocity boundary condition. Sorry to bring up a question about this BC again - Prof. Jasak writes that it's consistent and I believe that.

So here's what bothers me. My project is concerned with blood flow inside compliant vessels. I'm using a modified version of icoFsiFoam - basically added an outer iteration loop to be able to tackle strongly coupled systems. The solver seems to perform well when I increase the density of the fluid.

But at a certain point there seems to be a problem with fluid leaking out of my vessel (see image 1 - I didn't visualize the solid part which covers the fluid top & bottom), when I use the movingWallVelocity BC. It's strange and I checked the data sets - phi is zero at the the fluid-solid interface as should be ... still something must be wrong.

I ran the same case again using fixedValue BC at the fluid-solid interface (see image 2), which yields a much nicer flow pattern - here of course phi is not zero at the boundary.
I use a fixedValue velocity inlet and a totalPressure BC for the outlet in both cases.

Does anybody have an idea what is going wrong here? Is this problem possibly connected to the outer iterations I introduced - like, do I have to compensate or adapt anything with respect to the movingWallvelocity BC?

I would be glad if somebody could help or comment on that issue.

Cheers,
Wolfgang
Attached Images
File Type: jpg comparison_movingWallVelocity.jpg (66.7 KB, 119 views)
File Type: jpg comparison_fixedValue.jpg (86.5 KB, 96 views)
immortality likes this.
WiWo is offline   Reply With Quote

Old   December 29, 2010, 10:24
Default
  #6
New Member
 
khaled
Join Date: Nov 2010
Posts: 11
Rep Power: 6
PeterII is on a distinguished road
Hi Wolfgang
I'm interested by simulating blood flow in compliant vessel and I wish that you help me to do some simulation with icofsifoam.

best regards
khaled
PeterII is offline   Reply With Quote

Old   January 25, 2012, 10:57
Default
  #7
New Member
 
Martin
Join Date: Dec 2011
Posts: 2
Rep Power: 0
chathanm is on a distinguished road
hey
it is great to hear that you worked in FSI for a membrane wing.
actually i am a new stater in OpenFOAM. if you dont mind, could you explain how to do FSI in openfoam in short
regards
chathanm is offline   Reply With Quote

Old   March 6, 2013, 12:55
Default
  #8
New Member
 
Teng Wu
Join Date: Feb 2012
Posts: 9
Rep Power: 5
TengWU is on a distinguished road
Quote:
Originally Posted by WiWo View Post
Hello everyone,

I hope this is the right place to post an issue I have concerning the movingWallvelocity boundary condition. Sorry to bring up a question about this BC again - Prof. Jasak writes that it's consistent and I believe that.

So here's what bothers me. My project is concerned with blood flow inside compliant vessels. I'm using a modified version of icoFsiFoam - basically added an outer iteration loop to be able to tackle strongly coupled systems. The solver seems to perform well when I increase the density of the fluid.

But at a certain point there seems to be a problem with fluid leaking out of my vessel (see image 1 - I didn't visualize the solid part which covers the fluid top & bottom), when I use the movingWallVelocity BC. It's strange and I checked the data sets - phi is zero at the the fluid-solid interface as should be ... still something must be wrong.

I ran the same case again using fixedValue BC at the fluid-solid interface (see image 2), which yields a much nicer flow pattern - here of course phi is not zero at the boundary.
I use a fixedValue velocity inlet and a totalPressure BC for the outlet in both cases.

Does anybody have an idea what is going wrong here? Is this problem possibly connected to the outer iterations I introduced - like, do I have to compensate or adapt anything with respect to the movingWallvelocity BC?

I would be glad if somebody could help or comment on that issue.

Cheers,
Wolfgang
Hey Wolfgang,

I have the same confusion as you proposed for the movingWallVelocity boundary condition. I'm wondering have you figured it out?

Thanks,
immortality likes this.
TengWU is offline   Reply With Quote

Old   March 6, 2013, 15:17
Default
  #9
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17
immortality is on a distinguished road
I have two question.
1)does movingWallVelocity have anything more for impermeability of wall so that phi be zero.
if we use zeroGradient for T and p and wall velocity for U does it do the same work that movingWallVelocity does?
2)how to find phi value on a patch?
immortality is offline   Reply With Quote

Old   March 6, 2013, 15:23
Default
  #10
New Member
 
Teng Wu
Join Date: Feb 2012
Posts: 9
Rep Power: 5
TengWU is on a distinguished road
Quote:
Originally Posted by immortality View Post
I have two question.
1)does movingWallVelocity have anything more for impermeability of wall so that phi be zero.
if we use zeroGradient for T and p and wall velocity for U does it do the same work that movingWallVelocity does?
2)how to find phi value on a patch?
Hi ehsan,

you can find the phi value in the time dic;
do you think the fixedValue boundary condition will give the wall velocity for U, which means this boundary condition define a relative velocity for wall?
TengWU is offline   Reply With Quote

Old   March 6, 2013, 16:49
Default
  #11
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17
immortality is on a distinguished road
hi dear Teng
thanks.but then how is it possible to see values of phi on a patch?it doesn't appear in paraView.
I want to know if we set values as I told ((zeroGradient for p and T) and also fixedValue for wall is it different to movingWallVelocity? where's the impermeability for wall in movingWallVelocity BC?
immortality is offline   Reply With Quote

Old   March 6, 2013, 17:08
Default
  #12
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Teng,

The difference is that the movingWallVelocity gives you the absolute velocity of the wall, however, when e.g. solving for the turbulence, you are merely interested in the velocity (face fluxes) relative to the mesh motion. This is why the dynamic solvers have these fvc::makeRelative and fvc::makeAbsolute scattered throughout the code (movingWallVelocity on a static grid gives you zero velocity on the boundary).

This also means that if your boundary is moving, then the velocity at this boundary is non-zero - the physical flux of fluid on the other hand is 0.

You can make a quick test to convince yourself: Make a box of fluid with a boundary that allows for the water to flow in and out, e.g. the top boundary. Then start moving the lower boundary and specify either

Code:
type fixedValue;
value uniform (0 0 0);
or

Code:
type movingWallVelocity;
value uniform (0 0 0);
It is only in the case of movingWallVelocity that you will see any velocities in the domain.

Kind regards,

Niels
ngj is offline   Reply With Quote

Old   March 6, 2013, 17:53
Default
  #13
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17
immortality is on a distinguished road
I'm still looking forward to know about questions I propounded.
immortality is offline   Reply With Quote

Old   March 6, 2013, 17:59
Default
  #14
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17
immortality is on a distinguished road
dear Niels I can't figure out what you have said.especially your last sentence in your example.do you mean that movingWallVelocity allow fluid to move through it?
also I have questions propounded at above post.
thanks.
immortality 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
MovingWallVelocity Boundary Condition ralph OpenFOAM Running, Solving & CFD 7 June 18, 2013 07:15
HELP NEEDED HOW TO MAP VALUES FROM PATCH OF ONE MESH TO PATCH OF ANOTHER MESH mkraposhin OpenFOAM Running, Solving & CFD 3 September 4, 2011 09:42
How to obtain the index of all the points that belong to a particular patch mathieu OpenFOAM Running, Solving & CFD 2 October 15, 2008 09:16
Visualizing Patch Motion jaswi OpenFOAM Paraview & paraFoam 5 June 26, 2007 18:36
Saving patch motion as an IOobject jaswi OpenFOAM Running, Solving & CFD 1 June 26, 2007 13:07


All times are GMT -4. The time now is 06:20.