|
[Sponsors] |
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 4, 2013, 14:06 |
|
#101 | |
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 21 |
Quote:
were you able to run the FSI case in parallel without any problem? (completely I mean, end of simulation time) I have a problem you can see in this post : click @ Dr. Cardiff can FSI solver handle multiple FSI interfaces that are separate? |
||
September 4, 2013, 14:44 |
|
#102 | |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,096
Rep Power: 34 |
Quote:
the solver currently setup to use only one FSI interface; however, it should be straight-forward to extend it to an arbitrary number if you don't mind a bit of coding. Alternatively, you could merge your patch to make sure you have only one FSI interface (it doesn't matter is the FSI interface is discontinuous). Philip |
||
September 9, 2013, 07:03 |
|
#103 |
New Member
Join Date: Mar 2013
Posts: 17
Rep Power: 13 |
Hi,
I've modified the settings of the test case to run the FSI2 case. However, after some simulation time the solver stops, and when I look into the mesh there is a large overlap at the tip of the flap.I have attached a couple of screenshots in order to visualize the problem. https://dl.dropboxusercontent.com/u/...pshot3.png.zip Any idea what is happening here? Is the interpolation between the solid and fluid mesh which is not correct? Or the problems lies somewhere else? Hints anyone? Thanks alot! Best regards, David |
|
September 11, 2013, 03:15 |
|
#104 |
New Member
Vincent
Join Date: Aug 2013
Location: Singapore
Posts: 7
Rep Power: 13 |
Hi Philip,
I am trying to plot the displacement of the plate (at the plate back center point) in paraView by create selection and "plot selection over time", however, the following error appear: ERROR: In /home/vin-82/OpenFOAM/OpenFOAM-1.6-ext/ThirdParty/rpmBuild/BUILD/ParaView-3.12.0/VTK/Charts/vtkContext2D.cxx, line 177 vtkContext2D (0x9ce0930): Attempted to paint a line with <2 points. and there is no data appear on the plot. May i know how to solve this problem? Thanks |
|
September 11, 2013, 11:19 |
|
#105 | |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,096
Rep Power: 34 |
Quote:
I have noticed problems using the ParaView filter "Plot selection over time" when there are a large number of time-steps. So I would suggest you try a test case with about 10 time-steps and see if that works, then try large numbers of time-steps. Best regards, Philip |
||
September 15, 2013, 18:14 |
|
#106 |
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 21 |
@ Dr. Cardiff
I want to use dynamicRefineFvMesh as a dynamicFvMesh in dynamicMeshDict on FSI solver. I have changed what I think is necessary for dynamicRefineFvMesh. But I am still getting this error: Code:
Time = 1e-06, iteration: 3 Current fsi under-relaxation factor (Aitken): 0.999595 Maximal accumulated displacement of interface points: 0.0251937 --> FOAM FATAL ERROR: Problem with mesh motion solver selection From function pimpleFsiElasticNonLinULSolidFoam in file moveFluidMesh.H at line 140. FOAM aborting Aborted (core dumped) regards |
|
September 16, 2013, 06:12 |
|
#107 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,096
Rep Power: 34 |
@Bruno
Nice work! @Daniel Sorry, I am not familiar with dynamicRefineFvMesh. Philip |
|
September 16, 2013, 15:02 |
|
#108 | |
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 21 |
Quote:
sorry for lots of questions Does FSI solver support topological changes in the fluid region? I want to use dynamicTopoFvMesh for my test case, I have problems with PatchToPatchInterpolation. this problem occurs after mesh refinement. regards |
||
September 16, 2013, 22:14 |
|
#109 |
New Member
Vincent
Join Date: Aug 2013
Location: Singapore
Posts: 7
Rep Power: 13 |
Hi Philip,
Good morning! I have found a file "gpDeflection" in the tutorial, is this file for plotting the deflection of the plate? Thanks. Regards, Vincent |
|
September 24, 2013, 00:18 |
|
#110 |
New Member
Join Date: Jan 2010
Posts: 11
Rep Power: 16 |
I've been following this post for some time and having been playing around with trying to merge the CHT solver with the FSI solver. The problem I keep coming back to is how the different solvers handle the solid and fluid. In the FSI solver, there are separate directories for the different regions with separate meshes whereas the CHT solver seems to lump everything together into one mesh with different regions. Am I wrong in thinking that there will need to be some major reworking of how the CHT handles the fluid and solid since it does not match the FSI solver? Any pointers would certainly be appreciated and I will happily share results if there ever are any! Also, if I need to clarify anything, please let me know.
|
|
September 24, 2013, 19:44 |
|
#111 |
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 21 |
Hi Dr. Cardiff
I am working on simulation of flexible pipe with FSI solver. I have changed the fluid solver to use pimple algorithm. I have a question about FSI outer corrector: In my simulation, in each time step I get only 3 outer iteration for every time step. The solver also produces FSI under relaxation factor higher than 1 (e.g. 1.00078) furthermore, FSI residual suddenly drop in iteration 3, it acts like: iteration #1: fsi residual = 1 iteration #2: fsi residual = 0.997888 iteration #3: fsi residual = 5.4322e-5 Any suggestion would be appreciated, tell me if you need more information about case setup. regards |
|
September 26, 2013, 22:41 |
Problem with analytical solution of hotCylinder : elasticThermalSolidFoam
|
#112 | |
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AUS
Posts: 137
Rep Power: 15 |
Hi Cardif,
I'm having problem with the analytical solution of the hot Cylinder case that is provided with the elasticThermalSolidFoam. When I run the case it gives error like this: Create time Create mesh for time = 0 Writing analytical solution for a plain strain cylinder with concentric hole, where inner radius = 0.5 outer radius = 0.7 inner temperature = 100 outer temperature = 0 inner pressure = 0 outer pressure = 0 E = 200e9 u = 0.3 alpha = 1e-5 Writing analytical termpature field Writing analytical sigmaR field Writing analytical sigmaTheta field Writing analytical sigmaZ field #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 in "/home/adminuser/OpenFOAM/adminuser-2.1.0/platforms/linux64GccDPOpt/bin/analyticalHotCylinder" #4 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #5 in "/home/adminuser/OpenFOAM/adminuser-2.1.0/platforms/linux64GccDPOpt/bin/analyticalHotCylinder" Basically it creates the problem when calculating the sigmaZ. Will you please suggest me how to get rid of this?? Quote:
Last edited by ahmmedshakil; September 27, 2013 at 02:23. |
||
September 27, 2013, 02:26 |
Problem with analytical solution of hotCylinder : elasticThermalSolidFoam
|
#113 | |
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AUS
Posts: 137
Rep Power: 15 |
I solved the problem. It was coming from the atan(y/x) function. I am using OpenFoam 2.1.0 and for two argument passing through arc tan function -->the correct function is: atan2(y,x).
Quote:
|
||
September 29, 2013, 12:29 |
|
#114 |
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 21 |
Hello Dr. Cardiff
I have tested my case with fixedRelaxationFactor method with value of 0.2 and the solution will converge and FSI residual reduces smoothly and after 43 outer iterations it will reach to FSI convergence tolerance. Is there anything special that I am missing with Aitken method? I have found this old topic with the same problem that I have: http://www.cfd-online.com/Forums/ope...ation-fsi.html regards |
|
September 30, 2013, 14:25 |
|
#115 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,096
Rep Power: 34 |
@Daniel
As regards topological changes, changes may be required but I do not have any experience with this. As regards "Aitken" vs. "Fixed" relaxation, there is quite a bit of literature on this for FSI if you search google. For instance, the implemented Aitken procedure is presented here by Z. Tukovic. @Vincent The "gpDeflection" file is a gnuplot script; but it was used when the solver specifically wrote out the beam tip displacement to a file. It was removed to make the code more generic, it would have to be coded in to the solver. @ahmmedshakil Thanks for the fix! Philip |
|
September 30, 2013, 14:50 |
|
#116 | |
Senior Member
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 21 |
Quote:
Nice to have you back thanks for the answer. well I have read 4 papers so far on coupling algorithm, Fixedrelaxation, Aitken and IQN-ILS. But I can not understand why fsi under relaxation factor goes higher than 1. This is the case I am working on it for now: (you can see the geometry in attachment) as for the fluid region: fluid/0/motionU: Code:
dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { FSI { type fixedValue; value uniform (0 0 0); } OUTLET { type zeroGradient; } INLET { type zeroGradient; } } Code:
dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { FSI { type zeroGradient; } OUTLET { type fixedValue; value uniform 0; } INLET { type fixedValue; value uniform 50; } } Code:
dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { FSI { type fixedValue; value uniform (0 0 0); } OUTLET { type zeroGradient; } INLET { type pressureInletVelocity; value uniform (0 0 0); } } Code:
dimensions [0 1 0 0 0 0 0]; internalField uniform (0 0 0); boundaryField { FSI { type solidTraction; nonLinear updatedLagrangian; traction uniform ( 0 0 0 ); pressure uniform 0; value uniform (0 0 0); } O_WALL { type solidTraction; nonLinear updatedLagrangian; traction uniform ( 0 0 0 ); pressure uniform 0; value uniform (0 0 0); } INLET { type zeroGradent; } OUTLET { type zeroGradent; } } Code:
solidPatch FSI; solidZone FSIZone; fluidPatch FSI; fluidZone FSIZone; //movingRegion region0; fsiRelaxationFactor 0.01; interfaceDeformationLimit 0.01; outerCorrTolerance 1e-4; couplingScheme Aitken; fsi yes; Code:
dynamicFvMesh dynamicMotionSolverFvMesh; twoDMotion no; //solver velocityLaplacian; solver laplaceFaceDecomposition; diffusivity quadratic inverseDistance 1(FSI); frozenDiffusion yes; distancePatches ( FSI ); Is there anything obviously wrong with my setup? Actually I dont know what kind of boundary condition should I use for patch which is shown by arrow in the attachment. sorry for long question! regards |
||
October 1, 2013, 06:11 |
Appropriate boundary condition for displacement U
|
#117 |
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AUS
Posts: 137
Rep Power: 15 |
Hi,
I'm solving similar problem as arc welding in thin plate. I'm using elasticThermalSolidFoam solver. In my cases, I have to impose the boundary condition for U as follows (given in diagram also), (a) At X=0 and X= L ------------> sigmaxx = 0, sigmaxy =0, (b) At Y=0 -------------> du/dy =0, v=0, (c) At Y =H ---------------> sigmayx =0, sigmayy=0. As I am new to solid mechanics solver in OpenFoam, I'm wondering which boundary condition should I use.... either it (1) fixedDisplacement boundary with value (0 0 0) OR (2) fixedDisplacementZeroShare with value (0 0 0) OR anything else Anyone have idea which boundary condition I can use?? | Y sigmayx=0, sigmayy=0 |---------------------------------------------------------| | | sigmaxx=0 | | sigmaxx=0 sigmaxy=0 | | sigmaxy=0 | | | | |---------------------------------------------------------|-------------->X du/dy =0, v=0 The problem is similar to the case 4.4 mentioned by the paper: "I. Demirdžić, D. Martinović Finite volume method for thermo-elasto-plastic stress analysis, Computer Methods in Applied Mechanics and Engineering, vol 109, 331-349". |
|
October 1, 2013, 06:28 |
|
#118 | |
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AUS
Posts: 137
Rep Power: 15 |
Sorry, the image will be as attached (above the diagram a bit disfigured)..
Quote:
|
||
October 3, 2013, 13:16 |
|
#119 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,096
Rep Power: 34 |
Hi ahmmedshakil,
For your boundary conditions, the left, top and right are traction boundaries so use solidTraction with zero pressure and traction. For the bottom boundary, it is effectively a symmetryPlane (zero normal displacement, zero normal gradient of shear displacements). directionMixed can be also be used but is only necessary when the normal displacement is non-zero. Philip |
|
October 3, 2013, 13:27 |
|
#120 | |||
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,096
Rep Power: 34 |
Hi Daniel,
Quote:
As regards application of the Aitken's method to under-relaxation in FSI procedure, sometimes people may limit it but I am not sure of the reasoning (maybe they feel uncomfortable with relaxation factor >1 and/or <0) Quote:
As far as I know, it is a boundary condition for the fluid velocity field for a wall that is moving. This should not be used as a solid boundary condition. Quote:
As regards what boundary condition to use for the patch shown, this depends on what physical condition you want to enforce. Typically you don't use zeroGradient as a solid boundary as it does not really correspond to a physical condition (it's kind of like zero strain). Philip |
||||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
GPU Linear Solvers for OpenFOAM | gocarts | OpenFOAM Announcements from Other Sources | 37 | August 17, 2022 15:22 |
[Virtualization] OpenFOAM oriented tutorial on using VMware Player - support thread | wyldckat | OpenFOAM Installation | 2 | July 11, 2012 17:01 |
New OpenFOAM Forum Structure | jola | OpenFOAM | 2 | October 19, 2011 07:55 |
Cross-compiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingw-w64 | wyldckat | OpenFOAM Announcements from Other Sources | 3 | September 8, 2010 07:25 |
OpenFOAM Debian packaging current status problems and TODOs | oseen | OpenFOAM Installation | 9 | August 26, 2007 14:50 |