wrong displacement values using "ElasticSolver"?

[kevinarden]

"With this definition we say that the Young's modulus is constant, regardless of stress and strains. Is this correct?
Are you saying that the ElasticSolver decides by its own that beyond a certain strain the material is no longer linear?
Moreover, beyond the yield strength, in typical materials the Young's modulus decreases, whereas according to the ElasticSolver solution the Young's modulus increases at higher strain!"

ElasticSolver is geomterically non-linear solver, it does not have material non-linear built in. In geometric non-linear the young's modulus is constant, there is no yielding but at high displacements the structure stiffens in tension as you try to pull it farther and farther, in compression it may stiffen or buckle, in bending it typically gets stiffer. These geometric non-linears are not related to material or yielding. For example I ran
0.1x0.01x1.0 square shape fixed at 1 end pull on the other. E=5.E6, F= 5.E5, the linear displacement is 0.01, but using the geometric non-linear solver the displacement is 0.088, a high Poisson ratio will reduce it to 0.081. However if I change E to 5.E11 then both the linear and geometric non-linear solvers produce 1.E6.

Your problem, as defined, is geometrically non-linear, it will stiffen the more you stretch it if you use the geometric non-linear solver.

[kevinarden]

I ran the 0.1x0.01x1.0 in calculix, another open source fea tool. Using non-linear geometry option. It also calculated 0.088 same as ElastcSolver

calculix.png

(58.27 KiB) Not downloaded yet

[tomatoma]

It all starts to make more sense thanks to your last explanations!
Does it have something to do with the stiffness matrix being updated by the (non-linear) ElasticSolver as the bodies are deformed and not being updated by the (linear) StressSolver regardless of the large deformation?

[kevinarden]

That is correct.

[tomatoma]

I just would like to summarize this case and make some considerations on the strain_zz result:

L0: 0.05
E: 5e6
Poisson ratio: 0
Specific Force along z-axis: 5e5 (on surface with dimensions 0.3 x 0.05)

Results obtained with (StressSolver, ElasticSolver):

DeltaL (displacement): 5e-3, 4.4e-3
stress_zz: 5e5, 5e5
strain_zz: 0.1, 0.0919
other stresses and strains: negligible, negligible

In this simple uniaxial tension experiment, which is the theory (the formulas) behind it?
Are there any analytical relationships to derive (and verify) the results obtained with ElasticSolver?
I read the theory section in the Linear Elasticity and Finite Elasticity chapters of the ElmerModelsManual, but the subject is well beyond my abilities!
I thought that in this simple uniaxial case one could derive some simpler equations to verify the results given by the ElasticSolver.
For example, I couldn't even understand the relationship between the displacement and the strain_zz for the results obtained with the ElasticSolver, let alone derive them from the initial data!