
[Sponsors] 
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 29, 2017, 17:54 

#361 
New Member
Tom Dylan
Join Date: May 2015
Posts: 20
Rep Power: 11 
Thank you very much for this hint, Philip!
Now the solver is compiled without any errors. And that was the reason for confusion: lduMatrix::solverPerformance > lduSolverPerformance Is there any documentation out there of the syntax changes during the evolution of o30ext  o40ext? Next time I might check the errors myself. The modifications I am trying to implement is to consider the dependence of the fluid (gas & water mixture) stiffness K' (equivalent to the fluid compressibility 1/K') from the actual pore pressure. This of course enhances the nonlinearity since the pore pressure equation is affected by the volumetric strain increment *and* the change of the fluid stiffness K' in response to pore pressure changes. First tests indicate numerous iterations and nonconvergence after a couple of time steps. However, a "lagged scheme" in which K' from the previous time step is considered (instead of simultaneous evaluation of K' within the iteration loop) yields reasonable results. These of course depend on the time step size selection... Strongly non linear systems (e. g. unsaturated flow in porous media) sometimes are addressed through Picarditeration approaches. I wonder if a Picard scheme might improve the convergence of the current problem. Anyway, I succeeded installing o40x in opensuse leap 42.2. thanks again for your support! Tom 

June 30, 2017, 05:35 

#362  
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 
Hi Tom,
I am glad the code is now compiling for you. Quote:
Quote:
Underrelaxation of the K field will probably help, or more underrelaxation of the p and U fields (equations and fields). Philip 

July 10, 2017, 05:27 
fsiFoam in extend4.0 / running in parallel

#363 
New Member
Georg Göbel
Join Date: Sep 2016
Location: Karlsruhe
Posts: 8
Rep Power: 10 
Hello fsiFoamers,
is anyone running fsiFoam on ext4.0 in parallel? In the ext3.1 version there was this decomposeParFsitool, which was easy to use and worked fine, but on ext4.0 there is nothing like that. The Allrun skript suggest the use of standard decomposePar, but all my parallel jobs break while calling the first solid solver. It could depend on our machine here so it would be nice, if some of you could give me some short information about your experiences in running the ext4.0 version of fsiFoam in parallel. Thanks a lot in advance Georg BTW: the robinbc approach in the ext4.0 version is much more stable, even for high fluid density! Thanks to everyone who took part in developing, i highly appreciate your work. 

July 10, 2017, 09:24 

#364 
New Member
Iago Lessa de Oliveira
Join Date: May 2015
Posts: 23
Rep Power: 11 
Hello Georg,
I've been using fsiFoam for a couple months now and also used version 3.2 before. While for version 3.2 I was only able to decompose my cases with decomposeParFsi, in version 4.0 decomposePar worked great. There are only two issues I found so far: 1) I was not able to visualize the partitions on ParaView and 2) If I decompose from the latest timestep which is different from zero, the decomposition does not create the directory "processor*/constant" (instead, the utility name it "processor*/0") However, since you say your solid solver is not called properly in run time, did you link the fluid and solid directories? I think this already happened to me, and I remember that I missed the links between fluid and solid. Is there any error message ? Iago iago 

July 11, 2017, 11:24 

#365 
New Member
Georg Göbel
Join Date: Sep 2016
Location: Karlsruhe
Posts: 8
Rep Power: 10 
Hello Iago,
thanks for your reply. Now i know that the problem is somewhere on our machine or local extend installation. I was succesfully viszualizing the partitions with foamToVTK. It works both in 3.1 and 4.0. Georg 

July 12, 2017, 06:57 
implementing spatial heterogeneity of the saturated hydraulic conductivity

#366  
New Member
Tom Dylan
Join Date: May 2015
Posts: 20
Rep Power: 11 
Hi Philip,
Quote:
I played a little bit around trying to implement the pressure dependence of the Kfluidfield (stiffness of the water gas mixture within the pores) and I came to stable results with the fixed point approach (relaxing only p and U): Code:
fvm::ddt(p) == fvm::laplacian(coeff_Dp, p)  fvc::div(fvc::ddt(coeff_Dp2,U)) ); solverPerfP = pEqn.solve(); p.relax(); dp = p  p.oldTime(); dp.correctBoundaryConditions(); Kfluid = 1.0/(Sr/K_ + (1.0Sr)/(p0+psi*gamma+dp)); coeff_Dp = (kSat/gamma*Kfluid/n); coeff_Dp2 = Kfluid/n; Probably relaxing Kfluid (how ?), as you suggest, might enhance convergence. Now I tried to implement heterogeneity of the saturated hydraulic conductivity, which in natural settings is always an issue, by introducing the field kSat. in open water environments it is not uncommon to find conductivity contrasts spanning 4 orders of magnitude: sand 1^04 m/s, silt 1^8 m/s. The coeff_Dp field varies correspondingly over orders of magnitude. First I decided to adapt the laplacian scheme to harmonic, which makes more sense than a linear one from an geohydraulic point of view: Code:
laplacian(Dp,p) Gauss harmonic corrected; From the (very illustrative) convergence analysis in "On finite volume method implementation of poroelasticplasticity soil model" by Tang, Heledal & Cardiff it is clear, that a very large Kfluid (due to almost compressed gas in 20 m below phreatic surface) becomes stiffer than the bulk modulus of the soil and therefore mesh and time step sizes are determined by the bulk modulus, the water unit weight and the hydraulic conductivity! It turned out that a mesh size of approx. 0.2 m is necessary. I reduced the model to 2D (app. 120 m x 20 m) but could not reach convergence yet. I could imagine that my problem is not the first one to exhibit strongly varying laplacian terms. So I would appreciate any hints on strategies to overcome these kind of difficulties. Tom 

July 18, 2017, 14:52 

#367  
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 
Hi Tom,
Quote:
Quote:
Code:
... Kfluid.storePrevIter(); Kfluid = 1.0/(Sr/K_ + (1.0Sr)/(p0+psi*gamma+dp)); Kfluid.relax(); ... Quote:
Philip 

July 31, 2017, 13:36 

#368 
New Member
Iago Lessa de Oliveira
Join Date: May 2015
Posts: 23
Rep Power: 11 
Hello,
In the new version of the FSI toolkit, a great number of new boundary conditions (BC) was implemented for the fluid part. One of them is called outflowPressure, which I suppose is intended for outlets of the flow domain with a specified pressure on it. However, I am trying to understand what exactly this BC performs. I looked in its .C and .H files, but so far I only understood that the BC accounts for a correction/modification of the pressure involving a relation with the face normal velocity gradient through a variable called pp: pp = nu.value()*(n & pU.snGrad()) where pU = patch().lookupPatchField<volVectorField, vector>("U") I could not guess more (my C++ is very limited, unfortunately) and, so far, I did not find any information about this specific implementation of this boundary condition in the forums or even comparing with the implemented BC's in other versions of foamextend. Does anyone knows what exactly this BC implements? Thanks in advance for any help Iago 

November 21, 2017, 06:17 
elasticThermalSolidFoam

#369  
New Member

Hello,
Quote:
What I'm actually trying to do is model steadystate elastic strain in semiconductor structures.[1] There's a "builtin" strain which comes from a "misfit" between two crystals with different atomic spacings. I had been using solidDisplacementFoam for this, and it basically worked, although I was faking the misfit strain with a thermal strain (setting the thermal conductivity to zero). Basically, elasticThermalSolidFoam does not give the expected result (the solidDisplacementFoam result is correct) which is why I'm curious about the status of that !incremental bug, or the outcome of this thread. Ideally I'd like to be able to properly specific a misfit strain somehow, i.e. that two different (orthotropic) materials are obliged to maintain the same lattice spacing at the interface despite having different natural lattice spacings, but for now the fake thermal strain thing would be ok. Thanks! 1. http://aip.scitation.org/doi/abs/10.1063/1.4765009 

December 6, 2017, 03:19 

#370  
Member
Thaw Tar
Join Date: Apr 2013
Location: Yangon, Myanmar
Posts: 35
Rep Power: 13 
Quote:
Hi, could anybody please explain me about this question, too. I also have this very confusion. I cannot figure out how the computed fluid force (traction force) is used in the solid solver. Thaw Tar 

December 7, 2017, 05:45 

#371 
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 
Hi Thaw Tar,
The fluid force/traction is applied to the solid as a traction boundary condition in the "setInterfaceForce.H" header file (just before "solveSolid.H" in the "icoFsiElasticNonLinULSolidFoam.C" file). Philip 

December 7, 2017, 22:50 

#372  
Member
Thaw Tar
Join Date: Apr 2013
Location: Yangon, Myanmar
Posts: 35
Rep Power: 13 
Quote:
Now I understood how the fluid force was used as a boundary condition for the solid solver. And also for the advice to increase the solid solver iteration count and to control the convergence with residuals. It worked very well!!! Thaw Tar 

December 8, 2017, 03:07 

#373 
Member
Thaw Tar
Join Date: Apr 2013
Location: Yangon, Myanmar
Posts: 35
Rep Power: 13 
Dear Dr. Cardiff and others,
I am sorry for disturbing again. But I have one problem with the fsiFoam solver. I ran the simulation for some time steps and wrote out the data. But when I restart the simulation from the last time step, it showed this following error: Create extended GGI zonetozone interpolator Checking fluidtosolid face interpolator Fluidtosolid face interpolation error: 0.0126103 Checking solidtofluid point interpolator (GGI) Extended GGI, master point distance, max: 1e+15, avg: 2.30143e+14, min: 0.002 Extended GGI, master point orientation (<0), max: 1, min: 1, nIncorrectPoints: 638/982 > FOAM FATAL ERROR: Master point addressing is not correct From function ExtendedGGIInterpolation::masterToSlavePointInterp olate(const Field<Type> pf) in file ./numerics/ggi/ExtendedGGIInterpolation/ExtendedGGIInterpolation.C at line 703. FOAM aborting Aborted (core dumped) If anyone has the solution and could explain to me how to fix it, I would be very grateful. Thaw Tar 

December 14, 2017, 15:10 

#374 
New Member
Ricardo Ferreira
Join Date: May 2015
Posts: 16
Rep Power: 11 
Dear Formers, I trying simulate a 3D valve compressors. Initially, we created a 2D simple model with a cantilever beam, which will be a valve, as showed by mesh picture attached. At a certain time of simulation, the FSI interface doesn't match with solid mesh anymore (Uncoupled_meshes.png). In addition, the simulation does not diverge and the solution proceeds with those uncoupling meshes. Can someone help me? I know that if I try to restart the simulation from the last time step the error "Master point addressing is not correct" occurs.
Thanks. 

January 11, 2018, 08:21 
How to get the contact area and normal contact stress?

#375 
New Member
Jingwei Wang
Join Date: Dec 2017
Posts: 2
Rep Power: 0 
Hello Everybody,
Nice to be here! I am a phD student in Germany facing with a task of simulating and calculating dry sliding wear in a total hip replacement in a long term. As is all known, FEM method in Abaqus is a common and relative simple approach to perform this task. So far, I have not found any paper which used FVM method to simulate dry sliding wear. But with solidmechanics solver in combination with dynamical mesh technology in foam extend can the same goal be theoretically achieved. My plan is finally to publish a paper with both fem and fvm approach, and show that fvm can be a good alternative approach. Now, I am at the beginning stage and already tried NonLinUL solvers to build some simple contact models. The results are pretty good compared with abaqus. The problem I am confonted with is that i am not albe to get the contact area and normal contact stress from the soildmechanics solver in foamextend , but I really need these two for simulating wear. Can I get some help or cooperation from here? Since these two results are very common and important for contact problems and can usually be directly obtained from some fem softwares, I am looking forward to seeing these two can also be included in foamextend 5.0. Best regards, Jingwei 

January 12, 2018, 09:06 

#376 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 
Hi,
I guess Phil can help you more based on the fact that he developed it but since I am using an own solid stress solver, it should be not a big deal to get the contact area. In the contact class there should be some information about the cells / faces which are in contact and thus, you should easily be able to calculate the area. The normal contact stress should be similar. However, I do not know how the normal contact stress is given in terms of mathematical expressions. Again, Philip should be the one who could give more fundamental insight. I just wanted to let you know that it is possible.
__________________
Keep foaming, Tobias Holzmann Last edited by Tobi; January 25, 2018 at 09:26. 

January 12, 2018, 09:59 

#377  
New Member
Jingwei Wang
Join Date: Dec 2017
Posts: 2
Rep Power: 0 
Quote:
Thanks for your answer. Actually my German name is also Tobias. I agree with you that the key point is to get the information about which cell/surfaces are really in contact. The rest things are pretty easy. By the way, If you are interested in the mathematical expression of normal conact stress from FEM method which is vertexbased, you can send me a PM, I can send you a link or a paper. Jingwei 

January 25, 2018, 09:22 

#378  
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 
Quote:
Further to Tobias's response: The topic of my PhD was on modelling a hip joint in OpenFOAM, so some of the following articles may be useful: Quote:
Further to Tobias's response: The topic of my PhD was on modelling a hip joint in OpenFOAM, so some of the following articles may be useful:
As regards calculating the normal contact stress (), it is not written by default but you can write a utility to do this (send me a PM with your email and I will send you a utility that will work). For the contact area, it is possible to do it in a similar way. Philip 

January 31, 2018, 04:51 
VIV of a finite length vertical cylinder by fsiFoam

#379 
Member
Thaw Tar
Join Date: Apr 2013
Location: Yangon, Myanmar
Posts: 35
Rep Power: 13 
Dear all,
I tried to simulate the fluid structure interaction of a finite length vertical cylinder with a fixed bottom using fsiFoam and succeeded. It could simulate the occurrence of VIV and lockin. https://www.youtube.com/watch?v=NnFrh9ygWos Special thanks to Dr. Cardiff for developing the solid solver and his advice to tighten the solid solver by increasing the iteration count. I will test on more cases of reduced velocities. Thaw Tar 

January 31, 2018, 07:40 

#380  
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,091
Rep Power: 34 
Quote:
If the solid and fluid interface do not match then this typically means that the FSI loop did not converge to a tight enough tolerance (or did not converge at all) in each timestep. I would suggest looking at the FSI residual and check if it is converging in each timestep; if it is not then try a larger maximum number of FSI correctors or a different FSI coupling method or smaller timesteps; if it is converging, then try a tighter FSI tolerance. Separately, the segregated solid solver is typically not very efficient for slender geometries (like your thin beam): it much prefers "blocky" geometry. I understand you probably can't change your geometry, but if you PM me your email address then I can send you a workinprogress coupled solid solver that may be more efficient/robust in this case. Best, Philip Also, nice simulation Thaw Tar. 

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 
Crosscompiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingww64  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 