Dear Elmer Users
I am quite new in FEM and CSM calcualtion. At the moment I am trying to get the CSM1 case results proposed by the Turek and Hron Paper: http://citeseerx.ist.psu.edu/viewdoc/do ... 1&type=pdf.
The problem is quite simple: a beam is fixed on one side. The body gets a volume force. My values are not converging to the reference data. I calculate the case on an equidistant hexahedral mesh. Here are my results so far:
CSM1 Test CASE Turek Hron
Grid 70 x 4 x 4
displacement in x: 5.6069263e13 m
displacement in y: 0.07580281 m
Grid 140 x 8 x 8
displacement in x: 3.7717619e14 m
displacement in y: 0.078753294 m
Grid 280 x 16 x 16
displacement in x: 2.6036727e14, m
displacement in y: 0.079596393 m
Turek Hron Ref Data
displacement in x: −0.007187 m
displacement in y: 0.06610 m
I am happy for any hints and ideas that you have. I don't know why I get this deviation, especially for the displacement for the x diretion. Thank you a lot!
If you need any additional informations to my case please ask me.

My Case File:
Header
CHECK KEYWORDS Warn
Mesh DB "."
Include Path ""
Results Directory ""
End
Simulation
Max Output Level = 5
Coordinate System = Cartesian
Coordinate Mapping(3) = 1 2 3
Simulation Type = Steady state
Steady State Max Iterations = 1
Output Intervals = 1
Timestepping Method = BDF
BDF Order = 1
Solver Input File = case.sif
Post File = case.vtu
End
Constants
Gravity(4) = 0 1 0 0
Stefan Boltzmann = 5.67e08
Permittivity of Vacuum = 8.8542e12
Boltzmann Constant = 1.3807e23
Unit Charge = 1.602e19
End
Body 1
Target Bodies(1) = 1
Name = "Body 1"
Equation = 1
Material = 1
Body Force = 1
End
Material 1
Name = "Rubber"
Density = 1000.0
Poisson ratio = 0.4
Youngs modulus = 1.4e6
End
Equation 1
Name = "Equation 1"
Calculate Stresses = True
Active Solvers(1) = 1
End
Solver 1
Equation = Nonlinear elasticity
Procedure = "StressSolve" "StressSolver"
Variable = dofs 3 Displacement
Exec Solver = Always
Stabilize = True
Bubbles = False
Lumped Mass Matrix = False
Optimize Bandwidth = True
Steady State Convergence Tolerance = 1.0e5
Nonlinear System Convergence Tolerance = 1.0e7
Nonlinear System Max Iterations = 1
Nonlinear System Newton After Iterations = 3
Nonlinear System Newton After Tolerance = 1.0e3
Nonlinear System Relaxation Factor = 1
Linear System Solver = Iterative
Linear System Iterative Method = GCR
Linear System Max Iterations = 500
Linear System Convergence Tolerance = 1.0e8
Linear System Preconditioning = ILU1
Linear System ILUT Tolerance = 1.0e3
Linear System Abort Not Converged = False
Linear System Residual Output = 1
Linear System Precondition Recompute = 1
End
Solver 2
Exec Solver = after timestep
Equation = "result output"
Procedure = "ResultOutputSolve" "ResultOutputSolver"
Output File Name = "beam"
Output Format = String "vtu"
Binary Output = False
Save Geometry Ids = True
Ascii Output = True
End
Boundary Condition 1
Target Boundaries(1) = 5
Name = BoundaryCondition 1
Displacement 1 = 0
Displacement 2 = 0
Displacement 3 = 0
End
Body Force 1
Name = "Gravity"
Stress Bodyforce 2 = $ 2.0*1000
End

Turek Hron CSM Benchmark Case

 Site Admin
 Posts: 3309
 Joined: 22 Aug 2009, 11:57
 Antispam: Yes
 Location: Espoo, Finland
 Contact:
Re: Turek Hron CSM Benchmark Case
Hi FSI
You seem to solving in 3D? The original case is in 2D if I'm mistaken. Does it assumes plane stress or plane strain? Oftentimes it is a good idea to use quadratic elements for elasticity since they give better precision for the same computational cost.
This is a very nice case. However, I believe that these very competent experts made the case such that it would prove their monolithic approach would be needed. Are you really solving such cases where the coupling is so strongly? We have successfully used Elmer to model blood flow simulations which are also known to be tricky. There we have a nice remedy in the artificial compressibility that mimics the elastic response of the artery. Even that strategy faces here some challenges as the elasticity problem has more inertial effects and the pressurevolume response cannot easily be used to improve the convergence.
Peter
You seem to solving in 3D? The original case is in 2D if I'm mistaken. Does it assumes plane stress or plane strain? Oftentimes it is a good idea to use quadratic elements for elasticity since they give better precision for the same computational cost.
This is a very nice case. However, I believe that these very competent experts made the case such that it would prove their monolithic approach would be needed. Are you really solving such cases where the coupling is so strongly? We have successfully used Elmer to model blood flow simulations which are also known to be tricky. There we have a nice remedy in the artificial compressibility that mimics the elastic response of the artery. Even that strategy faces here some challenges as the elasticity problem has more inertial effects and the pressurevolume response cannot easily be used to improve the convergence.
Peter

 Posts: 3
 Joined: 20 Jun 2018, 17:48
 Antispam: Yes
Re: Turek Hron CSM Benchmark Case
Dear Peter,
thank you a lot for your quick response! What do you mean by plane stress or plane strain. As far as I understand displacement is calculated before the stress solver is taken into account. At the moment I am not care about coupling approaches I have different schmemes in mind, but this is another topic. My focus is to benchmark the CSM solver and before I don't get the same vaules as in the paper for the CSM case, I can't expect correct values in my FSI.
I followed your hint and run the case again in 2D with a quad mesh.
The results are now for a grid of 580 x 32
displacement in x: 7.6934897e15 m
displacement in y: 0.067089553 m
Now I have two questions:
Why I get a deviation from the 3d to the 2d case in the y displacement (How affect the 3rd degree of freedom for the displacement calculation the result?). The y displacement seems now correct in comparison to the ref data.
Why I don't get a displacement in x direction? It seems to converging against zero both 2d and 3d.
Thank you for your support!
Best Marc
thank you a lot for your quick response! What do you mean by plane stress or plane strain. As far as I understand displacement is calculated before the stress solver is taken into account. At the moment I am not care about coupling approaches I have different schmemes in mind, but this is another topic. My focus is to benchmark the CSM solver and before I don't get the same vaules as in the paper for the CSM case, I can't expect correct values in my FSI.
I followed your hint and run the case again in 2D with a quad mesh.
The results are now for a grid of 580 x 32
displacement in x: 7.6934897e15 m
displacement in y: 0.067089553 m
Now I have two questions:
Why I get a deviation from the 3d to the 2d case in the y displacement (How affect the 3rd degree of freedom for the displacement calculation the result?). The y displacement seems now correct in comparison to the ref data.
Why I don't get a displacement in x direction? It seems to converging against zero both 2d and 3d.
Thank you for your support!
Best Marc

 Site Admin
 Posts: 3309
 Joined: 22 Aug 2009, 11:57
 Antispam: Yes
 Location: Espoo, Finland
 Contact:
Re: Turek Hron CSM Benchmark Case
Hi Marc,
You might rather use the geometric nonlinear module: ElasticSolve.
By the way, the default solver settings for elasticity solver are often quite slow. If you compute something larger you may want to touch them also.
Peter
You might rather use the geometric nonlinear module: ElasticSolve.
By the way, the default solver settings for elasticity solver are often quite slow. If you compute something larger you may want to touch them also.
Peter

 Posts: 3
 Joined: 20 Jun 2018, 17:48
 Antispam: Yes
Re: Turek Hron CSM Benchmark Case
Hi Peter,
thank you again for your hint. Now I get quite nice values for the displacement (error < 1% to the reference values). Is their any literature or an extended Solver Manual, where I can get all of this informations?
Best Marc
thank you again for your hint. Now I get quite nice values for the displacement (error < 1% to the reference values). Is their any literature or an extended Solver Manual, where I can get all of this informations?
Best Marc

 Site Admin
 Posts: 3309
 Joined: 22 Aug 2009, 11:57
 Antispam: Yes
 Location: Espoo, Finland
 Contact:
Re: Turek Hron CSM Benchmark Case
Hi Marc
The Elmer Models Manual has usually the information on each physical module. Unfortunately some more rarely used features may be undocumented. StressSolver and ElasticSolver are pretty well covered. The extended manual over this would be the code itself...
Peter
The Elmer Models Manual has usually the information on each physical module. Unfortunately some more rarely used features may be undocumented. StressSolver and ElasticSolver are pretty well covered. The extended manual over this would be the code itself...
Peter