Hardening Parameters in Nonlinear Material Models

Technical Article

Strain hardening is the material ability to reach a higher stiffness by redistributing (stretching) microcrystals in the crystal lattice of the structure. A distinction is made between the material isotropic hardening as scalar quantities or tensorial kinematic hardening.

Figure 01 - Stress-Strain Diagram of Steel (Source: [1])

Theoretical Background

Strain hardening is characterised by internal variables. This is described in more detail in [2]. Using the internal variables, it is possible to consider damage or plasticity of materials, for example. The inner variables describe dissipative effects of the material.

Figure 02 - Strain Hardening in RFEM (von Mises, Tresca, Drucker-Prager, Mohr-Coloumb)

According to [1], Chap. 4.4.2, the state functions of the internal variables, which are usually not observable, are used to describe material defects (displacements, microscopic cracks, etc.), and they can be scalar (for example, isotropic damage) or tensorial (for example, kinematic hardening). To determine the internal variables, there are evolution equations (usually common differential equations) depending on the constitutive (independent and dependent) variables and the internal variables.

Equation 1:
$$\frac{{\mathrm{dβ}}_\mathrm i}{\mathrm{dt}}\;=\;\dot{{\mathrm\beta}_\mathrm i}\left(\mathrm\theta,\mathrm{gradθ},{\mathrm\beta}_1,...{\mathrm\beta}_\mathrm n\right)$$

These must be integrated with regard to the initial conditions.

Therefore, the internal variables are also referred to as a material memory with the initial condition at time t0.

Isotropic hardening is 'widening' of the yield surface without changing the surface position in the stress space. An example of this behaviour is a steel plate, which widens - in theory - due to the bearing stress in all directions. After the plastic deformation, the isotropic material is still isotropic, at least in theory. Generally, isotropic hardening is described by the internal variable α.

Kinematic hardening refers to a translation (displacement) of the yield surface in the stress space. The yield surface does not change its shape. The kinematic hardening compensates the local internal stresses of the material, resulting from local displacement of the material. This is also referred to as the Bauschinger effect in the literature. In this case, the yield strength is reduced as in the case of a multiply-bent wire. The bent wire has to spend less and less force, the more often it is bent. In the case of the kinematic hardening, the material is changed from isotropic to anisotropic. Generally, the kinematic hardening is described by the internal variable β.

  • Free Energy: $\mathrm\psi:\;=\;\mathrm\psi(\mathrm\varepsilon^\mathrm e,\mathrm\alpha,\mathrm\beta)$
  •  Dissipation of Energy: $\mathrm D^\mathrm{in}\;=\;\mathrm\sigma\;\cdot\;\dot{\widetilde{\mathrm\varepsilon}}^\mathrm p\;-\;\frac{\partial\mathrm\psi}{\partial\mathrm\alpha}\;\cdot\;\dot{\mathrm\alpha}\;-\;\frac{\partial\mathrm\psi}{\partial\mathrm\beta}\;\cdot\;\dot{\mathrm\beta}$
  • Thermodynamic Forces Isotropic: $\mathrm\alpha\;=\;-\;\frac{\partial\mathrm\psi}{\partial\mathrm\alpha}$
  • Thermodynamic Forces Kinematic: $\mathrm\tau\;=\;-\;\frac{\partial\mathrm\psi}{\partial\mathrm\beta}$

Equation 2:
$$\mathrm f({\mathrm\sigma}_\mathrm{ij};{\mathrm\varepsilon}_\mathrm p)\;=\;{\mathrm\sigma}_\mathrm e\;-\;\mathrm k({\mathrm\varepsilon}_\mathrm p)\;\mathrm{isotropic}\;\mathrm{yielding}$$

Equation 3:
$$\mathrm f({\mathrm\sigma}_\mathrm{ij};\mathrm\varepsilon_\mathrm{ij}^\mathrm{pl})\;=\;\mathrm F({\mathrm\sigma}_\mathrm{ij}\;-\;{\mathrm\alpha}_\mathrm{ij}(\mathrm\varepsilon_\mathrm{ij}^\mathrm{pl}))\;-\;\mathrm k\;\mathrm{kinematic}\;\mathrm{yielding}$$

Equation 4:
$$\mathrm f(\mathrm\sigma;\mathrm\varepsilon_\mathrm{ij}^\mathrm{pl};{\mathrm\varepsilon}_\mathrm p)\;=\;\mathrm F({\mathrm\sigma}_\mathrm{ij}\;-\;{\mathrm\alpha}_\mathrm{ij}(\mathrm\varepsilon_\mathrm{ij}^\mathrm{pl}))\;-\;\mathrm k({\mathrm\varepsilon}_\mathrm p)\;\leq\;0\;\mathrm{yielding}$$

In Equation 4, σe = F(σij) is the 'effective' stress of the material in the spatial state of stress. On the other hand, K is the limit stress in the uniaxial compression-tension test.

This is based on the assumption that plastic material behaviour in the multiaxial stress state corresponds to the uniaxial state (idealisation).

In the case of the kinematic hardening, the tensor αij describes the centre of the yield surface. The centre is shifted by the respective load step dα ij (see Figure 03).

The program considers the yield surface displacement due to the material displacement occurring analogously. Currently, this hardening type is not taken into account in RFEM.

One possible approach is the displacement according to the Prager rule with c as a material constant:

The effective plastic strain is decomposed into kinematic and isotropic hardening.

Equation 5:
$${\mathrm{dε}}_\mathrm p\;=\;\mathrm{mdε}_\mathrm p^\mathrm{iso}\;+\;\mathrm{dε}_\mathrm p^\mathrm{kin}$$

Equation 6:
$$\mathrm{dε}_\mathrm p^\mathrm{iso}\;=\;{\mathrm{mdε}}_\mathrm p$$

Equation 7:
$$\mathrm{dε}_\mathrm p^\mathrm{kin}\;=\;(1\;-\;\mathrm m)\;{\mathrm{dε}}_\mathrm p$$

m is a factor for checking the ratio of isotropic to kinematic hardening.

Figure 03 - a) isotropic, b) kinematic, c) mixed hardening (Source: [3])

Definition of Strain Hardening in RFEM

As already mentioned in my previous article about the Damage material model, a user-defined strain hardening is required in the program once you select the 'Diagram' option.

For this, the 3rd step is defined in Figure 04, which considers the strain hardening of the material according to von Mises during the plastification.

Equation 8:
$$\mathrm k\;=\;\left(\frac1{{\mathrm f}_\mathrm y}\right)^2\;\cdot\;\frac{\mathrm E}{{\mathrm E}_\mathrm p}$$

Equation 9:
$$\mathrm\sigma\;=\;\left(\mathrm E\;+\;{\mathrm E}_\mathrm p\right)\;\cdot\;\mathrm\varepsilon$$

Figure 04 - Stress-Strain Diagram (Manual)

The example shown in Figure 04 uses a material with the hardening factor of m = Ep = 0.08 kN/cm 2 and the elastic modulus of concrete E = 3,100 kN/cm². The stress in Step 2 and Step 3 of the model is changed as follows.

Equation 10:

Equation 11:
$$\rightarrow\;{\mathrm m}_0\;=\;\frac{{\mathrm\sigma}_1\;-\;{\mathrm\sigma}_0}{{\mathrm\varepsilon}_1\;-\;{\mathrm\varepsilon}_0}\;=\;\frac{2\;-\;0}{0.000645\;-\;0}\;=\;3,100\;\mathrm{kN}/\mathrm{cm}^2$$

Equation 12:
$${\mathrm m}_1\;=\;{\mathrm E}_\mathrm p\;=\;0,08\;=\;\frac{{\mathrm\sigma}_2\;-\;{\mathrm\sigma}_1}{{\mathrm\varepsilon}_2\;-\;{\mathrm\varepsilon}_1}\;=\;\frac{{\mathrm\sigma}_2\;-\;2}{{\mathrm\varepsilon}_2\;-\;0.000645}$$

Equation 13:
$$\rightarrow\;{\mathrm\sigma}_2\;=\;{\mathrm m}_1\;\cdot\;{\mathrm\varepsilon}_2\;+\;{\mathrm\sigma}_1\;=\;0.08\;\cdot\;1\;+\;2\;=\;2.08\;\mathrm{kN}/\mathrm{cm}^2$$

This example shows how you can consider the strain hardening of isotropic plastic material behaviour in the diagram of the Damage material model. For the second strain step, a very large strain step of ε2 = 1 is defined, which is close to ∞.


A user-defined definition of stress-strain diagrams is always required when defining special materials. In the case of such materials, it is also useful to define a strain hardening in order to achieve a better convergence and more realistic consideration of the material behaviour.

By defining intermediate points, it is also possible to consider isotropic hardening by entering the 'Diagram' even for nonlinear materials.


[1]  Nackenhorst, U. (2015). Vorlesungsskript Festkörpermechanik. Hannover: IBNM, Gottfried Wilhelm Leibniz Universität.
[2]  Altenbach, H. (2015). Kontinuumsmechanik - Einführung in die materialunabhängigen und materialabhängigen Gleichungen (3rd edition), Berlin: Springer.
[3]  Pravida, J. M. (1999). Zur nichtlinearen adaptiven Finite-Element-Analyse von Stahlbetonscheiben. Munich: Technical University.


Contact us

Contact to Dlubal

Do you have questions or need advice?
Contact our free e-mail, chat, or forum support or find various suggested solutions and useful tips on our FAQ page.

+49 9673 9203 0


RFEM Main Program
RFEM 5.xx

Main Program

Structural engineering software for finite element analysis (FEA) of planar and spatial structural systems consisting of plates, walls, shells, members (beams), solids and contact elements

Price of First License
3,540.00 USD