# StressedFoam

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

 June 16, 2011, 13:31 StressedFoam #1 New Member   Join Date: Jun 2011 Posts: 3 Rep Power: 8 Sponsored Links 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!

 June 16, 2011, 16:14 #2 Senior Member     Philip Cardiff Join Date: Mar 2009 Location: Dublin,Ireland Posts: 638 Rep Power: 23 Hi, Where are you loading your geometry? what are all the boundary conditions? Also what analytical solution are you using? Philip

 June 16, 2011, 16:36 #3 New Member   Join Date: Jun 2011 Posts: 3 Rep Power: 8 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.

 June 18, 2011, 12:55 #4 Senior Member     Philip Cardiff Join Date: Mar 2009 Location: Dublin,Ireland Posts: 638 Rep Power: 23 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

 June 19, 2011, 04:03 #5 New Member   Join Date: Jun 2011 Posts: 3 Rep Power: 8 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.

 November 10, 2011, 18:27 #6 New Member   Concordia_CFD Join Date: Jul 2010 Location: Canada Posts: 24 Rep Power: 9 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

 November 10, 2011, 19:01 #7 Senior Member     Philip Cardiff Join Date: Mar 2009 Location: Dublin,Ireland Posts: 638 Rep Power: 23 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

 November 10, 2011, 22:16 #8 New Member   Concordia_CFD Join Date: Jul 2010 Location: Canada Posts: 24 Rep Power: 9 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

 November 11, 2011, 10:14 #9 Senior Member     Philip Cardiff Join Date: Mar 2009 Location: Dublin,Ireland Posts: 638 Rep Power: 23 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

November 11, 2011, 11:49
#10
New Member

Concordia_CFD
Join Date: Jul 2010
Posts: 24
Rep Power: 9
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
 fsitest.txt (22.8 KB, 11 views)

November 11, 2011, 12:35
#11
Senior Member

Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 638
Rep Power: 23
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

 November 11, 2011, 12:46 #12 New Member   Concordia_CFD Join Date: Jul 2010 Location: Canada Posts: 24 Rep Power: 9 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 13:32.

 November 11, 2011, 13:07 #13 Senior Member     Philip Cardiff Join Date: Mar 2009 Location: Dublin,Ireland Posts: 638 Rep Power: 23 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

 November 11, 2011, 13:26 #14 New Member   Concordia_CFD Join Date: Jul 2010 Location: Canada Posts: 24 Rep Power: 9 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

 November 11, 2011, 13:37 #15 Senior Member     Philip Cardiff Join Date: Mar 2009 Location: Dublin,Ireland Posts: 638 Rep Power: 23 OK great, hopefully it works. Philip

 Tags beam, displacement, stressedfoam

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post fw407 OpenFOAM Running, Solving & CFD 2 July 27, 2008 07:00 quba OpenFOAM Running, Solving & CFD 0 June 22, 2007 15:30 weijing OpenFOAM Running, Solving & CFD 0 August 21, 2006 05:24 weijing OpenFOAM Running, Solving & CFD 0 April 13, 2006 22:59 weijing OpenFOAM Running, Solving & CFD 0 April 13, 2006 22:51