Max principal Srain does not match Principal stress 1

[Yoman228]

I have a model that uses material of steel with yield around 400Mpa. It is base on Ramberg Osgood material behaviour where the total stain is 0.5% at yield

I get the following results.

Mises = 370Mpa
Max Principal stress = 430Mpa
Max. Principal strain = 0.25%

The question is if my Max Principal stress is above yield shouldn’t the Max. Principal strain is more then 0.5%?

 

[xerf]

Each increment the FEM solution is obtained in terms of displacements. The displacements are called primary dependent variable.

Based on the solution of the displacement field the secondary dependent variable are obtained, namely:

- First, the strains are computed from the kinematic solution at each integration point, i.e. using gradient formulas of displacement field.

- Second, using the the computed strains and the constitutive relations (in your case Ramberg-Osgood law) the program computes the components of the stress tensor at each integration point. Using the components of strain tensor first an equivalent strain measure is computed. This is typically defined as e=(2/3*E_ij*E_ij)^0.5. Using the equivalent strain and the stress-strain information provided by user as the constitutive relation, the program establishes the value of the Mises stress.Finally, using the Mises value, the value of the strain components and flow rule, the program computes the components of the stress tensor.

Generally, all the above computations are performed with respect to global coordinates, or with respect to material orientation (if the user assigned material directions), which do not coincide with the principal directions.

There are can be many details involved and topic is quite vast and I think additional details can be found in the Theory Manual - > Materials.

Another point is that Ramberg Osgood is not a real plasticity model but rather it describes plasticity in a manner similar to non-linear elasticity.

 

[Yoman228]

how should I name that strain in report then?
Eqv strain in Principal direction?
currently I am reporting it as maximum Principal strain which is very misleading as client compare them to maximum principal stress.

 

[xerf]

The maximum principal strain is diferent than an equivalent strain.

The equivalent strain si a scalar magnitude of the strain tensor and based on all the componentes of the strain tensor. It is not characterized by a direction.

The maximum principal strain represents the maximum eigenvalue of the strain tensor or to put it in a different way it represents the maximum component value of the strain tensor with respect to its principal directions, i.e. the direction which are charaterized by zero shear components.

It is ok to look at the principal components , but the point is that the constitutive relation you use (Ramberg Osgood) does not use the principal values of strain and stress tensor and therefore you can have individual components of the stress and strain with larger values than Mises Stress and Equivalent Strain at "yielding".

Also, if you use banded contour plots, be aware that they can be misleading regarding the max./min. values shown by the spectrum color. This is caused by the plotting algorithm which is based on the values extrapolated at nodes.

 

[Yoman228]

Thx for the reply, I am still a little unclear of the following.

“can have individual components of the stress and strain with larger values than Mises Stress and Equivalent Strain at "yielding"

I understood that the Principal stress is higher then the Mises stress by studying the Von Mises yield surface diagram.

But however, I can not find the right word to explan to the client that the maximum principal strain that is given in ABAQUS (maximum eigenvalue of the strain tensor) is a lot lower then the strain which gives the maximum principal stress (as they compare the results in tensile test which is 2D).

I will be very thankful if I can get some help on this. Should I quote some formulation? Which one should I use?

 

[xerf]

Typically, the material behavior (i.e. constitutive relation) is obtained based on simple uniaxial tests.

This uniaxial curve stress=f(strain) is provided by the user in FEM program. This uniaxial curve involves one

However, in FEA the state of stress and strain are multiaxial. In order to use the uniaxial experimental stress-strain curve, the FE program converts the multiaxial strain tensor (6 scalar components) in equivalent strain (1 scalar value). This strain is called equivalent because it "converts" a multiaxial state of strain to an equivalent uniaxial (1 scalar component) state of strain. Similarly MISES stress is an equivalent stress (1 scalar component) which "converts" a multiaxial state of stress to an equivalent uniaxial state of stress.

Using the equivalent strain and the uniaxial curve (obtained experimentally in uniaxial tests) the program obtains the equivalent MISES stress. This is further use to compute the individual components of the multiaxial stress tensor.

Therefore the yielding condition is estimated by "converting" a 3D (or 2D) states of stress and strains to "equivalent" 1D (uniaxial) states which can be used in conjunction with uniaxial experimental data.

This equivalence is of course not perfect and depends on the plasticity theory used etc.

The computation of multiaxial state of stress based on multiaxial state of strain (in the most used computational plasticity theories) is not obtained through a direct relation between a strain component and the corresponding stress components, or as in generalized Hooke's law for linear elasticity. (The computational platicity theories are are not always trivial.)

That is if the yielding occurs: then
stress_ij is not imediately computed in terms of strain_ij. Instead more sofisticated algorithms, usually making use of equivalent stress and strain measures are used.

Computational plasticity/inelatisticity is a huge topic by itself. See for example:
- Computational Inelasticity by J. C. Simo , Thomas J. Hughes
- Inelastic Analysis of Solids and Structures by Milos Kojic, Klaus-Jürgen Bathe
- Introduction to Computational Plasticity by Fionn Dunne, Nik Petrinic

The last book is written in context of ABAQUS, so it is a very good point to start (if interested) in studying the computational plasticity.

ABAQUS theory manual, the chapter on Materials contains relevant information to each specific theory and material model implemented in ABAQUS, showing how the multiaxial states of strain and stress are computed.