CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Community Contributions > OpenFOAM CC Toolkits for Fluid-Structure Interaction

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

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

Like Tree134Likes

Closed Thread
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 23, 2022, 08:30
Default
  #661
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5
MFWilliams is on a distinguished road
Yes, of course the dimensions show what pressure it is. That was silly.


Ohh I see. Is there functionality in cfMesh or snappyHexMesh to be able to specify the surface level mesh on the fluid interface to triangular whilst keeping the main internal fluid domain hexahedral? Or would it involve changing the whole fluid domain mesh to tetrahedral and then extruding the solid domain to create the triangular prism elements?


Merlin

Last edited by MFWilliams; February 23, 2022 at 11:01.
MFWilliams is offline  

Old   February 23, 2022, 13:06
Default
  #662
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,092
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by MFWilliams View Post
Yes, of course the dimensions show what pressure it is. That was silly.
No problem

Quote:
Originally Posted by MFWilliams View Post
Ohh I see. Is there functionality in cfMesh or snappyHexMesh to be able to specify the surface level mesh on the fluid interface to triangular whilst keeping the main internal fluid domain hexahedral? Or would it involve changing the whole fluid domain mesh to tetrahedral and then extruding the solid domain to create the triangular prism elements?
For snappyHexMesh, no.

For cfMesh, you can use tetMesh or pMesh instead of cartesianMesh, but as you noted, this will change the internal fluid mesh too. It is possible to create a utility to split all surface faces into triangles but I don't think this exists and some non-trivial coding would be involved. So your options would be to use a set mesh for the fluid and then extrude the solid as triangular prisms. Or use this same triangular prism solid mesh with the original Cartesian fluid domain (non-conformal interface).
bigphil is offline  

Old   February 24, 2022, 07:15
Default
  #663
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5
MFWilliams is on a distinguished road
Brilliant thank you very much for clarifying that.


Merlin
MFWilliams is offline  

Old   February 25, 2022, 07:14
Default
  #664
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5
MFWilliams is on a distinguished road
For my FSI simulation, I am getting the warning "Max iterations reached within momentum loop". Is there a way to increase the number of iterations it can complete or do you know why this might be happening?


Thanks
Merlin
MFWilliams is offline  

Old   February 25, 2022, 07:45
Default
  #665
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,092
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by MFWilliams View Post
For my FSI simulation, I am getting the warning "Max iterations reached within momentum loop". Is there a way to increase the number of iterations it can complete or do you know why this might be happening?


Thanks
Merlin
Set nCorrectors in constant/solid/solidProperties (or constant/solidProperties in a solid only case) to be a larger number, e.g. 1000, or 5000 or 10000.
bigphil is offline  

Old   February 25, 2022, 09:56
Default
  #666
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5
MFWilliams is on a distinguished road
Quote:
Originally Posted by bigphil View Post
Set nCorrectors in constant/solid/solidProperties (or constant/solidProperties in a solid only case) to be a larger number, e.g. 1000, or 5000 or 10000.

Thank you very much.
MFWilliams is offline  

Old   February 27, 2022, 11:15
Default
  #667
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5
MFWilliams is on a distinguished road
If anyone is interested, I have greatly improved the oscillations in my FSI simulation by changing the BC for the pressure of the fluid on the fluid solid interface patch from a zeroGradient to extrapolatedPressure BC.

I am also having trouble with setting the coupling time to start later in the simulation and I was wondering if anyone had any ideas about it.

I have a working FSI sim and I have tried changing the coupling start time to 0.01 seconds. But when I run it, it now breaks before it even gets to the coupling and the fluid velocities are much higher than they are when I have coupling from the start. I also have a working CFD sim which is exactly the same as the fluid for my FSI simulation and that has no problems.

The log file of the broken FSI sim is here


Does anyone know why specifying the coupling start time might cause problems?

Thank you in advance for your help.
MFWilliams is offline  

Old   March 1, 2022, 09:49
Default
  #668
New Member
 
ilhado's Avatar
 
Iago Lessa de Oliveira
Join Date: May 2015
Posts: 23
Rep Power: 11
ilhado is on a distinguished road
Quote:
That meshing workflow is what I am currently using but is it possible to specify the element types using extrudeMesh? As I wanted to try create the solid domain using tetrahedral elements because of what Iago said that it can help pressure oscillations.
As Philip pointed out, yes I meant to use triangular prisms and not tetrahedral cells. Sorry the confusion. What I do is to create the fluid and solid meshes separately. For the fluid I use cfMesh. But for the solid I extrude a better-quality STL of the wall surface, since you normally get these aneurysms geometries as STL from the original images. The extrusion can be made with OpenFOAM's extrudeMesh, but I use VMTK in general to manipulate these surfaces and perform the extrusion.

This procedures leads to non-conformal meshes at the FSI interface, so you have to be carefull with using a sufficiently refined mesh, otherwise it may not even pass the GGI test at the beginning of the FSI simulation that checks the FSI interpolation errors.
bigphil likes this.
ilhado is offline  

Old   March 1, 2022, 10:33
Default
  #669
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5
MFWilliams is on a distinguished road
Quote:
Originally Posted by ilhado View Post
As Philip pointed out, yes I meant to use triangular prisms and not tetrahedral cells. Sorry the confusion. What I do is to create the fluid and solid meshes separately. For the fluid I use cfMesh. But for the solid I extrude a better-quality STL of the wall surface, since you normally get these aneurysms geometries as STL from the original images. The extrusion can be made with OpenFOAM's extrudeMesh, but I use VMTK in general to manipulate these surfaces and perform the extrusion.

This procedures leads to non-conformal meshes at the FSI interface, so you have to be carefull with using a sufficiently refined mesh, otherwise it may not even pass the GGI test at the beginning of the FSI simulation that checks the FSI interpolation errors.

That was my bad misinterpreting what you saying about triangular prisms for meaning tetrahedral elements.


Ok have you found there to be any sort of minimal functional ratio between the number of nodes on the fluid interface to nodes on the solid interface?


Thank you for the help
Merlin
MFWilliams is offline  

Old   March 1, 2022, 11:02
Default
  #670
New Member
 
ilhado's Avatar
 
Iago Lessa de Oliveira
Join Date: May 2015
Posts: 23
Rep Power: 11
ilhado is on a distinguished road
Quote:
Ok have you found there to be any sort of minimal functional ratio between the number of nodes on the fluid interface to nodes on the solid interface?
No, the number of cells in each mesh was solely a result of mesh independence studies. In any case, I am no real expert on GGI, so I am not sure whether a relation like this exists and may influence the simulation.

Iago
MFWilliams likes this.
ilhado is offline  

Old   May 7, 2022, 15:53
Default Problems with multi-domain multi-material simulation (elasticSolidFoam)
  #671
Member
 
Richardpluff
Join Date: May 2014
Posts: 95
Rep Power: 12
CRI_CFD is on a distinguished road
Dear foamers,


Hope I am on the right place to get some tips about my simulation. I have been dealing with it for a long time and can't find the way to make it work. I am not a newcomer to OpenFOAM but never used it for solid mechanics problems and I would like to start doing it.



I have a block and some teeth. I created my stls and divided them into load, support, lower_teeth and block. The idea would be to impose a load (solidTraction for example) once the geometry is clamped by the support (I would say fixedDisplacement equal to 0).


Two different domains will be present (one for the block=bone, another one for the Lower_teeth=teeth), together with 2 different materials (bone and teeth).


I used snappy for meshing. After enclosing my geometry in a block using blockMesh and meshing with snappy, I got 3 domains meshed. I needed to remove the one corresponding to the background, so I used setSet, subSetMesh and splitMeshRegions). Seems that it works (checkMesh is OK). New contacts (interfaces) between regions have been created.


I define my material properties regions using materials file and cellstoRegion (renamed to have 0 and 1 indexes only). I remove everything related to the background mesh (like ffminx, ffmaxx...in boundary file, cellRegions...). I checked in Paraview and materials assignement has been carried out succesfully.



I share here the case in One Drive (it is heavy, just in case you want to give a try to it):


https://1drv.ms/u/s!AjenQBoiljuzgoQs...rRL4Q?e=fe5Pjf



BCs are supposed to be a load on the load boundary and clamped support. I would like to know stress and deformations produced due to this load.


When I run elasticSolidFOam, the simulations explodes after a few iterations (static analysis), with too high values of stress and strain. I tried many things (remesh, play with Bcs and numerical schemes, material properties or use only one material...) but nothing seems to work.


Any hints on my set up? Mesh? BCs? Contacts?



Also another remark is that I am unable to see the different mesh regions created in the former step (they can be imported in Paraview, but they do not contain U, V, sigma, epsilon...fields...). Why not? Only the whole internal mesh is populated with such values.



@bigphil or any other guru here...could you please give me a hand on this?



I apologise in advance if this is not the best place to open my thread...


Thanks to all solid mechanics foam extend community!
CRI_CFD is offline  

Old   May 12, 2022, 16:28
Default solids4foam error building on fe35 aarch64
  #672
Senior Member
 
Sultan Islam
Join Date: Dec 2015
Location: Canada
Posts: 141
Rep Power: 10
EternalSeekerX is on a distinguished road
Hello,

So im buiding solids4foam on fe35 for aarch64 using foam extend 4.1. I get an error when replacing solutions.c

Code:
 fe-aarch64OS  localhost  ../solids4foam-release  cp filesToReplaceInOF/solution.C /home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/foam/matrices/solution/

 fe-aarch64OS  localhost  ../solids4foam-release  wmake libso /home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/foam

Making dependency list for source file matrices/solution/solution.C
SOURCE=matrices/solution/solution.C ;  g++ -std=c++11 -DlinuxARM8 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -floop-optimize -falign-loops -falign-labels -falign-functions -falign-jumps -fprefetch-loop-arrays -march=native -mtune=native  -DNoRepository -ftemplate-depth=100 -DOMPI_SKIP_MPICXX -I/usr/local/OpenMPI-4.0.3/gcc-7/openmpi/include -fexceptions     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/ThirdParty/zlib-1.2.3 -IlnInclude -I. -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/foam/lnInclude -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linuxARM8GccDPInt32Opt/solution.o
SOURCE=global/global.Cver ; sed -e 's/VERSION_STRING/4.1/' -e 's/BUILD_STRING/4.1-70b064d0f326/' $SOURCE > Make/linuxARM8GccDPInt32Opt/global.C; g++ -std=c++11 -DlinuxARM8 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -floop-optimize -falign-loops -falign-labels -falign-functions -falign-jumps -fprefetch-loop-arrays -march=native -mtune=native  -DNoRepository -ftemplate-depth=100 -DOMPI_SKIP_MPICXX -I/usr/local/OpenMPI-4.0.3/gcc-7/openmpi/include -fexceptions     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/ThirdParty/zlib-1.2.3 -IlnInclude -I. -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/foam/lnInclude -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/OSspecific/POSIX/lnInclude   -fPIC -c Make/linuxARM8GccDPInt32Opt/global.C -o Make/linuxARM8GccDPInt32Opt/global.o
matrices/solution/solution.C:426:6: error: prototype for 'void Foam::solution::setSolverPerformance(const Foam::word&, const lduSolverPerformance&) const' does not match any in class 'Foam::solution'
 void Foam::solution::setSolverPerformance
      ^~~~
In file included from matrices/solution/solution.C:26:0:
matrices/solution/solution.H:174:18: error: candidates are: template<class Type> void Foam::solution::setSolverPerformance(const Foam::BlockSolverPerformance<Type>&) const
             void setSolverPerformance
                  ^~~~~~~~~~~~~~~~~~~~
matrices/solution/solution.H:166:18: error:                 template<class Type> void Foam::solution::setSolverPerformance(const Foam::word&, const Foam::BlockSolverPerformance<Type>&) const
             void setSolverPerformance
                  ^~~~~~~~~~~~~~~~~~~~
matrices/solution/solution.C:462:6: error: prototype for 'void Foam::solution::setSolverPerformance(const lduSolverPerformance&) const' does not match any in class 'Foam::solution'
 void Foam::solution::setSolverPerformance
      ^~~~
In file included from matrices/solution/solution.C:26:0:
matrices/solution/solution.H:174:18: error: candidates are: template<class Type> void Foam::solution::setSolverPerformance(const Foam::BlockSolverPerformance<Type>&) const
             void setSolverPerformance
                  ^~~~~~~~~~~~~~~~~~~~
matrices/solution/solution.H:166:18: error:                 template<class Type> void Foam::solution::setSolverPerformance(const Foam::word&, const Foam::BlockSolverPerformance<Type>&) const
             void setSolverPerformance
                  ^~~~~~~~~~~~~~~~~~~~
make: *** [matrices/solution/solution.dep:322: Make/linuxARM8GccDPInt32Opt/solution.o] Error 1
make: *** Waiting for unfinished jobs....
I'm using gcc-7.5 and OpenMPI 4.0.3. Weirdly enough if I replace the original solution.c back, foam extend compiles correctly. Should I be replacing certain. C files In a certain order for it to recognize certain libraries?

Edit 2: it seems that whatever changes the replaced solution.c does, is not valid for FE41, I don't know why the allcheck is even running them when its building from FE4.1

Edit 3: After install bg, solids4foam check script detected foam version correctly, howver now in the compilation, I have this errror:

Code:
    -L/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/lib/linuxARM8GccDPInt32Opt     -lincompressibleTurbulenceModel -lincompressibleRASModels         -lincompressibleLESModels -llduSolvers -linterfaceProperties         -lfiniteArea -loversetMesh -loversetDynamicFvMesh     -lblockCoupledSolids4FoamTools     -lsolids4FoamModels     -lfiniteVolume     -lincompressibleTransportModels     -ldynamicFvMesh     -ldynamicMesh     -lmeshTools     -ltopoChangerFvMesh      -lfoam -ldl   -lm -o /home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/mergeSubMeshesNew
/usr/bin/ld: /home/fe-aarch64OS/foam/fe-aarch64OS-4.1/lib/linuxARM8GccDPInt32Opt/libsolids4FoamModels.so: undefined reference to `__aarch64_ldadd4_acq_rel'
collect2: error: ld returned 1 exit status
make[1]: *** [/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/wmake/Makefile:160: /home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/mergeSubMeshesNew] Error 1
make: *** [/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/wmake/MakefileApps:39: mergeSubMeshesNew] Error 2

Last edited by EternalSeekerX; May 13, 2022 at 13:04.
EternalSeekerX is offline  

Old   May 13, 2022, 09:32
Default
  #673
Neb
Member
 
Join Date: Mar 2020
Posts: 66
Rep Power: 6
Neb is on a distinguished road
Hi ,
have you solved your problem?
Neb is offline  

Old   May 13, 2022, 12:15
Default
  #674
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,092
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by EternalSeekerX View Post
Edit 2: it seems that whatever changes the replaced solution.c does, is not valid for FE41, I don't know why the allcheck is even running them when its building from FE4.1
No file replacements are required for FE41. The Allwmake script should automatically skip these replacements.

Quote:
Originally Posted by EternalSeekerX View Post
Edit 3: After install bg, solids4foam check script detected foam version correctly, howver now in the compilation, I have this errror:
Code:
undefined reference to `__aarch64_ldadd4_acq_rel'
Can you give the full error? i.e. the log file from "Allwmake &> log.Allwmake"
bigphil is offline  

Old   May 17, 2022, 00:51
Question Issue solved?
  #675
Senior Member
 
Sultan Islam
Join Date: Dec 2015
Location: Canada
Posts: 141
Rep Power: 10
EternalSeekerX is on a distinguished road
Quote:
Originally Posted by Neb View Post
Hi ,
have you solved your problem?
Quote:
Originally Posted by bigphil View Post
No file replacements are required for FE41. The Allwmake script should automatically skip these replacements.



Can you give the full error? i.e. the log file from "Allwmake &> log.Allwmake"
So something odd is happening, I basically deleted fe41 and rebuild from scratch.

Here is both fef41 log and solids4foam attached!

I find it odd that it works now, i think. Only issue I see is the missing S4F for abaqus thingy
Attached Files
File Type: zip FE41+Solids4Foam logs.zip (132.9 KB, 0 views)

Last edited by EternalSeekerX; May 17, 2022 at 05:58.
EternalSeekerX is offline  

Old   May 18, 2022, 08:27
Default
  #676
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,092
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by EternalSeekerX View Post
So something odd is happening, I basically deleted fe41 and rebuild from scratch.

Here is both fef41 log and solids4foam attached!

I find it odd that it works now, i think. Only issue I see is the missing S4F for abaqus thingy
OK, glad it works. No need to worry about the abaqus UMATs unless you actually plan to use them.
bigphil is offline  

Old   May 18, 2022, 22:57
Thumbs up abaqus UMAT compiled fine
  #677
Senior Member
 
Sultan Islam
Join Date: Dec 2015
Location: Canada
Posts: 141
Rep Power: 10
EternalSeekerX is on a distinguished road
Quote:
Originally Posted by bigphil View Post
OK, glad it works. No need to worry about the abaqus UMATs unless you actually plan to use them.
I see, well I did it just to see if it compiles, it worked nice

Code:
fe-aarch64OS  localhost  ../Solids4Foam  ./Allwmake -j4

filesToReplaceInOF/Allcheck

No checks for versions of foam-extend greater than 4.0
eigen3 found.
Updating Make/files link
Using Make/files.foamextend
'/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/lib/linuxARM8GccDPInt32Opt/libblockCoupledSolids4FoamTools.so' is up to date.
Updating Make/files link
Using Make/files.foamextend
'/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/lib/linuxARM8GccDPInt32Opt/libsolids4FoamModels.so' is up to date.
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file abaqusUmatLinearElastic/abaqusUmatLinearElastic.C
SOURCE=abaqusUmatLinearElastic/abaqusUmatLinearElastic.C ;  g++ -std=c++11 -DlinuxARM8 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -floop-optimize -falign-loops -falign-labels -falign-functions -falign-jumps -fprefetch-loop-arrays -march=native -mtune=native  -DNoRepository -ftemplate-depth=100 -std=c++11     -Wno-old-style-cast -Wno-deprecated-declarations     -DFOAMEXTEND=41     -I../solids4FoamModels/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/finiteVolume/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/meshTools/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/finiteArea/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/lagrangian/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/dynamicMesh/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/dynamicMesh/dynamicMesh/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/dynamicMesh/dynamicFvMesh/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/dynamicMesh/topoChangerFvMesh/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/sampling/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/surfMesh/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/postProcessing/foamCalcFunctions/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/errorEstimation/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/ThirdParty/packages/metis-5.1.0/platforms/linuxARM8GccDPInt32Opt/include     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/decompositionMethods/decompositionMethods/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/decompositionMethods/metisDecomp/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/decompositionMethods/scotchDecomp/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/mesh/extrudeModel/lnInclude     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/applications/utilities/mesh/generation/extrudeMesh     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/applications/utilities/mesh/generation/extrudeMesh/extrudedMesh     -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/applications/utilities/preProcessing/mapFields -IlnInclude -I. -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/foam/lnInclude -I/home/fe-aarch64OS/.root/opt/OpenFOAM/foam/foam-extend-4.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linuxARM8GccDPInt32Opt/abaqusUmatLinearElastic.o
'/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/lib/linuxARM8GccDPInt32Opt/libabaqusUmatLinearElastic.so' is up to date.
Compiling abaqusUmatLinearElastic.f and placing object in /home/fe-aarch64OS/foam/fe-aarch64OS-4.1/lib/linuxARM8GccDPInt32Opt
Updating Make/files link
Using Make/files.foamextend
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/solids4Foam' is up to date.

Copying solids4FoamScripts.sh to /home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt

make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/abaqusMeshToFoam' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/addPatch' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/addTinyPatch' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/flattenPatch' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/decomposeParNew' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/projectPatchToSphere' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/mergeSubMeshesNew' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/set2dMeshThickness' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/setInitialTemperature' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/splitPatch' is up to date.
'/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/lib/linuxARM8GccDPInt32Opt/libsimpleMeshSmoothers.so' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/surfaceTractions' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/volPointInterpolate' is up to date.
make[1]: '/home/fe-aarch64OS/foam/fe-aarch64OS-4.1/applications/bin/linuxARM8GccDPInt32Opt/simpleSmoothMesh' is up to date.

solids4foam compilation complete; check for errors above


 fe-aarch64OS  localhost  ../Solids4Foam
bigphil likes this.
EternalSeekerX is offline  

Old   May 19, 2022, 15:31
Talking Flexible Dam Break worked on aarch64 container
  #678
Senior Member
 
Sultan Islam
Join Date: Dec 2015
Location: Canada
Posts: 141
Rep Power: 10
EternalSeekerX is on a distinguished road
So, I tested the flexible dam break tutorial on my fedora 35 aarch64 container and it worked haha.

Here is a gif:

https://giphy.com/gifs/AMRmCkVzNaP0XxdKcD
bigphil likes this.
EternalSeekerX is offline  

Old   August 5, 2022, 10:33
Default Impact test simulation using solids4Foam
  #679
Member
 
Ashish Magar
Join Date: Jul 2016
Location: Mumbai, India
Posts: 81
Rep Power: 10
ashishmagar600 is on a distinguished road
Hello Philip,



I am doing a simplistic impact test simulation, where an object will be falling due to gravity on a fixed object. I took help from this post Bouncing ball to get started.



However, the 'res' residuals are always 1 and only 'relRes' are converged. After a few time steps the simulation crashes with diverging relative residuals. Also I would like to mention, as per your suggestion I have only DD relaxation but cant see any rigid body motion.



Is there any thing I am missing or doing wrong?
ashishmagar600 is offline  

Old   August 5, 2022, 11:02
Default
  #680
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,092
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by ashishmagar600 View Post
Hello Philip,



I am doing a simplistic impact test simulation, where an object will be falling due to gravity on a fixed object. I took help from this post Bouncing ball to get started.



However, the 'res' residuals are always 1 and only 'relRes' are converged. After a few time steps the simulation crashes with diverging relative residuals. Also I would like to mention, as per your suggestion I have only DD relaxation but cant see any rigid body motion.



Is there any thing I am missing or doing wrong?
Did you also try the ./tutorials/solids/elastoplasticity/impactBar tutorial case? It might be helpful.
bigphil is offline  

Closed Thread

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 14:33.