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

StressedFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 16, 2011, 13:31
Default StressedFoam
  #1
New Member
 
Join Date: Jun 2011
Posts: 3
Rep Power: 5
CFD_buw is on a distinguished road
Dear members,
I have problems with stressedFoam. I generated a cube with a fixed beam inside. For the mesh generation I just used blockMesh. Then I implemented a pressure which acts on the beam. With the help of sampleDict I am able to read out the displacements in x, y and z direction. The problem is, that my analytical solution results in a different value.
The pressure is 650000 N/m^2 , the length of the beam is 0.2, the cross section is 0.008 m * 0.008 m and the youngs modulus E = 2 * 10 ^11 N/m^2.
My analytical solution for the maximal displacement is 3.174 * 10^-4 m but OpenFoam results in 1.215*10^-5 m.
Has somebody experience with this problem and can somebody give me a good hint?

Warm regards and thank You!
CFD_buw is offline   Reply With Quote

Old   June 16, 2011, 16:14
Default
  #2
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 538
Rep Power: 17
bigphil will become famous soon enough
Hi,


Where are you loading your geometry? what are all the boundary conditions?

Also what analytical solution are you using?


Philip
bigphil is offline   Reply With Quote

Old   June 16, 2011, 16:36
Default
  #3
New Member
 
Join Date: Jun 2011
Posts: 3
Rep Power: 5
CFD_buw is on a distinguished road
Hello bigphil,

thank You for Your fast replay.
The analytical solution is calculated with the normal bending beam which is fixed on both ends. After calculating the defelxion curve I can determine the maximum displacement in the middle of the beam.

The boundary conditions are:
The surrounding walls of the cube have a zeroGradient.
The pressure field is constant with a value of 650000 N/m^2.

I am loading the geometry in paraview and I am able to see the right behaviour. The magnitude of the displacement U is a maximum in the middle of the beam. But unfortunately the value is really small. The dimension are already checked...

Warm regards.
CFD_buw is offline   Reply With Quote

Old   June 18, 2011, 12:55
Default
  #4
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 538
Rep Power: 17
bigphil will become famous soon enough
Hi,

Are you sure you want to use the zeroGradient BC, it doesn't really have a physical interpretation for a displacement solver (well maybe it's equivalent to a zero strain condition), if you want a traction/stress-free BC at the solids walls then you should use the tractionDisplacement BC and set the traction and pressure to zero.

Philip
bigphil is offline   Reply With Quote

Old   June 19, 2011, 04:03
Default
  #5
New Member
 
Join Date: Jun 2011
Posts: 3
Rep Power: 5
CFD_buw is on a distinguished road
Hey Phillip,

I will try to change it on Tuesday and will post You my experiences. Generally, if I think about the boundaries, then You should be right with Your idea. Lets see ...

Warm regards.
CFD_buw is offline   Reply With Quote

Old   November 10, 2011, 17:27
Default
  #6
New Member
 
Concordia_CFD
Join Date: Jul 2010
Location: Canada
Posts: 24
Rep Power: 6
marzbali is on a distinguished road
Hello,

Does wall boundary exist in stressedFoam? I mean when a face is fixed and cannot move then what boundary condition should be used? The zero traction apparently is used for free end of the beam not the fixed end, right?
I apologize for my poor knowledge in solid mechanics, since I only worked with fluid solvers

Regards,
Marzbali
marzbali is offline   Reply With Quote

Old   November 10, 2011, 18:01
Default
  #7
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 538
Rep Power: 17
bigphil will become famous soon enough
Hi Marzbali,

You can fix a solid boundary using fixedValue in your displacement boundary conditions (0/U or 0/D):
Code:
patchOfInterest 
{
type fixedValue;
value uniform (0 0 0);
}
Philip
bigphil is offline   Reply With Quote

Old   November 10, 2011, 21:16
Default
  #8
New Member
 
Concordia_CFD
Join Date: Jul 2010
Location: Canada
Posts: 24
Rep Power: 6
marzbali is on a distinguished road
Hi Philip,

Thanks for your quick reply. yeah, that makes sense. The reason that I'm asking is because I'm simulating the deformation of a disk subject to a pressure force with a 2D axisymmetric model in stressedFoam. For the top and bottom surfaces tracionDisplacement is used and the periphery of the disk doesn't move so fixedValue should be used. I have divergence problem now because motionU reaches 1e35 after 1 iteration! Have you had a similar case before?

Regards,
Marzbali
marzbali is offline   Reply With Quote

Old   November 11, 2011, 09:14
Default
  #9
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 538
Rep Power: 17
bigphil will become famous soon enough
Marzbali,

motionU... does that mean you are using icoFsiFoam the extend version of OpenFOAM?

As far as I can see motionU is the motion of the fluid mesh, so maybe the motion of the fluid mesh is too extreme, I'm not sure without knowing more about the case and solver.

Philip
bigphil is offline   Reply With Quote

Old   November 11, 2011, 10:49
Default
  #10
New Member
 
Concordia_CFD
Join Date: Jul 2010
Location: Canada
Posts: 24
Rep Power: 6
marzbali is on a distinguished road
Hi Philip,

Yes, actually I'm using interFsiFoam solver in OF-1.5-dev. I'm modeling impact of a water droplet on SS disk. So the geometry is axisymmetric and simply two domains with the same size and cells on top of each other. I have attached the output if you'd like to have a look. If you want I can upload the case here so you can try it, please let me know.

Cheers,
Marzbali
Attached Files
File Type: txt fsitest.txt (22.8 KB, 8 views)
marzbali is offline   Reply With Quote

Old   November 11, 2011, 11:35
Default
  #11
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 538
Rep Power: 17
bigphil will become famous soon enough
Marzbali,

OK looking at your stress residuals:
Quote:
PCG: Solving for Ux, Initial residual = 0.401083, Final residual = 0.00399601, No Iterations 43
PCG: Solving for Uy, Initial residual = 0.406038, Final residual = 0.00313817, No Iterations 34
PCG: Solving for Uz, Initial residual = 0.429895, Final residual = 0.00335018, No Iterations 34
They have not converged at all, they are still about 0.4, they should be 1e-6.

What kind of mesh are you using for your solid? Maybe it would be good if you upload your case.

Philip
bigphil is offline   Reply With Quote

Old   November 11, 2011, 11:46
Default
  #12
New Member
 
Concordia_CFD
Join Date: Jul 2010
Location: Canada
Posts: 24
Rep Power: 6
marzbali is on a distinguished road
Hello,

The mesh is structured wedge type and uniformly distributed. Its size is 25 microns. You can see the case in the attachment.

Thanks.
Marzbali

Last edited by marzbali; November 11, 2011 at 12:32.
marzbali is offline   Reply With Quote

Old   November 11, 2011, 12:07
Default
  #13
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 538
Rep Power: 17
bigphil will become famous soon enough
Marzbali,

"checkMesh" fails on your solid mesh.
How did you create the axisymmetric mesh? There should not be an axis patch (patches are only for faces, you can only apply boundary conditions to faces in the cell centred finite volume method).
So I think there is some special way to make an axialMesh maybe something like this utility, but I haven't tried it.

Philip
bigphil is offline   Reply With Quote

Old   November 11, 2011, 12:26
Default
  #14
New Member
 
Concordia_CFD
Join Date: Jul 2010
Location: Canada
Posts: 24
Rep Power: 6
marzbali is on a distinguished road
Philip,

You brought up a very good point. I forgot to check the solid mesh and you're right it fails. I defined both front and back wedges in one patch and apparently in this case they have to be separated. I divided them to 2 patches and it's running now. Let's see if it converges or not!!
Regarding the axis patch, I saw in nozzleFlow2D tutorial that axis is defined with only two vertices but basically it is a face with zero area. It would work when it is set to empty.

Thanks a million for your help and best regards.
Marzbali
marzbali is offline   Reply With Quote

Old   November 11, 2011, 12:37
Default
  #15
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 538
Rep Power: 17
bigphil will become famous soon enough
OK great,
hopefully it works.

Philip
bigphil is offline   Reply With Quote

Reply

Tags
beam, displacement, stressedfoam

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
A dynamic case for stressedFoam fw407 OpenFOAM Running, Solving & CFD 2 July 27, 2008 07:00
StressedFoam boundary conditions description quba OpenFOAM Running, Solving & CFD 0 June 22, 2007 15:30
Some problem about stressedFOAM with tetra meshes weijing OpenFOAM Running, Solving & CFD 0 August 21, 2006 05:24
Compare stressedFoam and stressFemFoam in tutorial case plateHole weijing OpenFOAM Running, Solving & CFD 0 April 13, 2006 22:59
Compare stressedFoam and stressFemFoam in tutorial case plateHole weijing OpenFOAM Running, Solving & CFD 0 April 13, 2006 22:51


All times are GMT -4. The time now is 23:45.