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

floatingObject in 2D or axi-symmetric

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 15, 2011, 05:59
Default floatingObject in 2D or axi-symmetric
  #1
New Member
 
Jordi Muela
Join Date: Mar 2011
Posts: 27
Rep Power: 7
jordi.muela is on a distinguished road
Hi everyone,

i'm trying to solve the floatingObject case (interDyMFoam solver) in 2D and 2D Axi-symmetric.
I have modified de mesh, the boundary conditions and I have added the necessary constraints at the models.
The problem is that i get divergence in a few time-steps because the object falls down very quickly. I'm 'playing' with the mass at patch pointDisplacement, but the body falls quickly, no matter if the mass is very high or low (differences in magnitude orders).
Where is the problem? The boundary type "sixDoFRigidBodyDisplacement" only works fine in 3D models?
Somebody has already implemented a similar model?
Any response and helpfull will be welcome!

Thank you everyone!
jordi.muela is offline   Reply With Quote

Old   April 9, 2013, 20:48
Default
  #2
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 615
Rep Power: 7
sharonyue is on a distinguished road
Quote:
Originally Posted by jordi.muela View Post
Hi everyone,

i'm trying to solve the floatingObject case (interDyMFoam solver) in 2D and 2D Axi-symmetric.
I have modified de mesh, the boundary conditions and I have added the necessary constraints at the models.
The problem is that i get divergence in a few time-steps because the object falls down very quickly. I'm 'playing' with the mass at patch pointDisplacement, but the body falls quickly, no matter if the mass is very high or low (differences in magnitude orders).
Where is the problem? The boundary type "sixDoFRigidBodyDisplacement" only works fine in 3D models?
Somebody has already implemented a similar model?
Any response and helpfull will be welcome!

Thank you everyone!
Hi,

I am facing the same problem,the box is sinking. How to handle this?
sharonyue is offline   Reply With Quote

Old   May 20, 2013, 06:59
Default
  #3
New Member
 
QuocThien
Join Date: Apr 2013
Posts: 9
Rep Power: 4
neiht is on a distinguished road
hi!
I think that u need restraints the object with low factor to reduce motion and increase the relaxation factor.
Maybe i'm wrong!
neiht is offline   Reply With Quote

Old   May 22, 2013, 10:47
Default
  #4
Senior Member
 
kilroy's Avatar
 
Join Date: Mar 2013
Location: USA
Posts: 120
Rep Power: 4
kilroy is on a distinguished road
I am having the same problem. My object is sinking very fast. I will try to restraint the object with a low factor with increasing the relaxation factor and see what happens.

Thanks for the help,
kilroy is offline   Reply With Quote

Old   May 22, 2013, 19:43
Default
  #5
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 615
Rep Power: 7
sharonyue is on a distinguished road
I tried restrain it in verticalspring. looks like it can deal with the sinking . But this is not DOF. I dont know how to deal with DOF to make it normally.
http://zhan.renren.com/openfoam There is a non-newtonian fluid free surface flow
sharonyue is offline   Reply With Quote

Old   May 23, 2013, 12:14
Default
  #6
Senior Member
 
kilroy's Avatar
 
Join Date: Mar 2013
Location: USA
Posts: 120
Rep Power: 4
kilroy is on a distinguished road
I found the problem. My "rhoInf" variable was "1000" in the "pointDisplacement" file. When I changed it into "1", my object started to float again.
kilroy is offline   Reply With Quote

Old   May 23, 2013, 19:28
Default
  #7
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 615
Rep Power: 7
sharonyue is on a distinguished road
Quote:
Originally Posted by kilroy View Post
I found the problem. My "rhoInf" variable was "1000" in the "pointDisplacement" file. When I changed it into "1", my object started to float again.
Woo!congrats!Is it a 2D case?
sharonyue is offline   Reply With Quote

Old   May 23, 2013, 19:39
Default
  #8
Senior Member
 
kilroy's Avatar
 
Join Date: Mar 2013
Location: USA
Posts: 120
Rep Power: 4
kilroy is on a distinguished road
Yes, it is 2D. But the results I am getting are weird. I don't know if it is because of "rhoInf" or there is another thing wrong somewhere else.
kilroy is offline   Reply With Quote

Old   May 23, 2013, 19:46
Default
  #9
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 615
Rep Power: 7
sharonyue is on a distinguished road
Quote:
Originally Posted by kilroy View Post
Yes, it is 2D. But the results I am getting are weird. I don't know if it is because of "rhoInf" or there is another thing wrong somewhere else.
Umm,I have played that 2D floatingobject some weeks age but failed.I have to use lots of restrains and constrains.If not the object is sinking fast.In a 3D case it looks like normal but its unstable.Anyway its not my major so I give up.But you seems like get something succeed which inspire my interests...Wish you can simulate you case successfully and share you experience and I will check my 2D case again another day.

Reagrds
sharonyue is offline   Reply With Quote

Old   October 31, 2013, 11:15
Default
  #10
New Member
 
Jorge Gadelho
Join Date: Feb 2013
Posts: 9
Rep Power: 4
JGadelho is on a distinguished road
Hello everyone,
I've made the changes has described in the first post to the floatingObject tutorial to transform it to a 2D problem.

Like described, I'm facing the same problem. The object falls very fast. I've tried to change the rhoInf, but with no luck. Any news?

thank you.
JGadelho is offline   Reply With Quote

Old   July 18, 2014, 07:11
Default
  #11
New Member
 
Join Date: Aug 2013
Posts: 3
Rep Power: 3
MarcelK is on a distinguished road
Although this thread is now quite old, I still try to add something to the discussion.
I also modified the floatingObject tutorial and reduced the dimensionality of the problem by one by modifying the mesh and introducing appropriate 6 DoF constraints. To summarize,

  1. I modified the mesh to be only one cell deep. Since I use my own blockMeshDict.m4 to construct two-dimensional meshes, my mesh now ranges from (-0.01, -0.5, -0.5) to (0.01, 0.5, 0.5) and the box ranges from (-0.01, -0.15, -0.06) to (0.01, 0.15, 0.06). The sea level is at 0.0368, thus the water depth is 0.5368.
  2. I added
    Code:
    twoDMotion yes;
    to the dynamicMeshDict.
  3. I changed the pointDisplacement as follows
Code:
        type            sixDoFRigidBodyDisplacement;
        centreOfMass    (0 0 0);
        momentOfInertia (0.005568 0.0007893333333 0.00482133333333);
        mass            0.64;        
        rhoInf          1;  // needed only for solvers solving for kinematic pressure
        report          on;
        value           uniform (0 0 0);
        
        constraints
        {
            maxIterations 500;
            
            fixedLine1
            {
                sixDoFRigidBodyMotionConstraint fixedLine;
                tolerance 1e-6;
                relaxationFactor 0.7;
                fixedLineCoeffs
                {
                    refPoint $centreOfMass;
                    direction (0 0 1);
                }
            }
        
            fixedAxis1
            {
                sixDoFRigidBodyMotionConstraint fixedAxis;
                tolerance 1e-3;
                relaxationFactor 0.7;
                fixedAxisCoeffs
                {
                    axis (1 0 0);
                }
            }
        }
When running the case, I receive exploding velocities of the rigid body and the computation quits with a floating point exception:


Code:
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 982
    Increased the timePrecision from 16 to 17 to distinguish between timeNames at time 0.0648223531977
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2   in "/lib64/libc.so.6"
#3  void Foam::MULES::limiter<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::Field<double>&, Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) at ??:?
#4  void Foam::MULES::limit<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::zeroField const&, Foam::zeroField const&, double, double, int, bool) at ??:?
#5  Foam::MULES::explicitSolve(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, double, double) at ??:?
#6  
 at ??:?
#7  __libc_start_main in "/lib64/libc.so.6"
#8  
 at ??:?
./run.sh: Zeile 16: 45533 Gleitkomma-Ausnahme     interDyMFoam
I would be interested if I missed something in the case setup or if the error is due to numerical difficulties. If the latter should apply, it would be enlightening if anybody could comment on why these difficulties arise.


P.S.: Since I think it is instructive if others can compare to their settings, I uploaded my whole case.
Attached Files
File Type: zip floatingBox2d.zip (14.0 KB, 5 views)
MarcelK is offline   Reply With Quote

Old   March 10, 2015, 08:37
Default
  #12
New Member
 
Ali
Join Date: Oct 2013
Posts: 22
Rep Power: 3
ashim is on a distinguished road
Hi,

I am trying to use waveDyMFoam (Modified according to instruction from waves2foam) to simulate 6DOF for a ship in waves at zero speed. I have run simple cases for 2D and 3D block. both cases are working fine. But when I am trying to use for ship, it is sinking very quickly. From the last time step, I found that free surface is not getting updated , it just goes downward with ship. I couldn't solve the problem for last 2 weeks. I appreciate any kind of help and suggestion.

Ali
ashim is offline   Reply With Quote

Old   March 13, 2015, 08:44
Default
  #13
New Member
 
Join Date: Aug 2013
Posts: 3
Rep Power: 3
MarcelK is on a distinguished road
This looks like a problem with your case setting. A bit more information would be helpful, otherwise it is difficult for us to help you. Did you check your
Code:
U
file and make sure to have
Code:
type movingWallVelocity;
as boundary condition type for the patch associated to your rigid body?
MarcelK is offline   Reply With Quote

Old   March 14, 2015, 07:35
Default
  #14
New Member
 
Ali
Join Date: Oct 2013
Posts: 22
Rep Power: 3
ashim is on a distinguished road
Hi MarcelK,

Thank you very much for your reply. I have checked the U boundary condition for rigid body and it is movigwallVelocity. I have correct the box property and it is not sinking now, But the force is increasing so rapidly after some times and ends with crash. Here is link of case folder. I am running the case in OF 2.3.1. I need to solve this problem within very short time. Any kind of advice is highly appreciated.

Ali

https://www.dropbox.com/sh/i0eg20ywb...fSJd778Ka?dl=0
ashim is offline   Reply With Quote

Reply

Tags
2d model, axi-symmetric, floatingobject, interdymfoam

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
Pressure instabilities with interDyMFoam for the floatingObject case nbadano OpenFOAM Running, Solving & CFD 14 March 8, 2011 09:19
Error in Axi symmetric model. binubtharayil FLUENT 2 August 5, 2009 16:01
doubts about axi symmetric moving reference frame and eers Main CFD Forum 0 July 9, 2009 15:53
BC's for following axi symmetric geometry.. eers Main CFD Forum 0 June 29, 2009 12:16
Axi symmetric flow Emmanuel Resch CD-adapco 4 February 10, 2008 14:29


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