Plasticity
Use the Plasticity subnode to define the properties for modeling elastoplastic materials. This material model is available in the Solid Mechanics, Shell, Layered Shell, Membrane, and Truss interfaces, and can be used together with Linear Elastic Material, Nonlinear Elastic Material, and Hyperelastic Material.
The Nonlinear Structural Materials Module or the Geomechanics Module are required for this material model, and the available options depend on the used products. For details, see https://www.comsol.com/products/specifications/.
See also Elastoplastic Materials in the Structural Mechanics Theory chapter.
Shell Properties

This section is only present when Plasticity is used as a subnode to:
Linear Elastic Material in the Layered Shell interface. See the documentation for the Plasticity node in the Layered Shell chapter.
Linear Elastic Material, Layered in the Shell interface. See the documentation for the Plasticity node in the Shell and Plate chapter.
Hyperelastic Material, Layered in the Shell interface. See the documentation for the Plasticity node in the Shell and Plate chapter.
Linear Elastic Material, Layered in the Membrane interface. See the documentation for the Plasticity node in the Membrane chapter.
Plasticity Model
Use this section to define the plastic properties of the material.
Equivalent Stress
The yield function defines the limit of the elastic regime, Fe, σys) ≤ 0, and sets the onset for plastic deformation. Changing the equivalent stress measure σe allows to specify different yield criteria. See Defining the Yield Criterion for details.
Select the Equivalent stress von Mises, Tresca, Hill orthotropic, or User defined to define the yield criterion.
The default is von Mises criterion with associate plastic potential.
Select Tresca to use Tresca yield criterion. The plastic potential can be an Associated or nonassociated flow rule with the von Mises stress as plastic potential.
Select Hill orthotropic to use Hill’s criterion. From the Specify list select either the Initial tensile and shear yield stresses σys0ij or Hill’s coefficients F, G, H, L, M, and N. The default for either selection uses values From material (if it exists) or User defined. The principal directions of orthotropy are inherited from the coordinate system selection in the parent node. See Expressions for the Coefficients F, G, H, L, M, N for details.
For User defined enter a value or expression for the equivalent stress. Write any expression in terms of the stress tensor components or its invariants in the ϕ(σ) field.
Initial Yield Stress
For all yield criteria, the default Initial yield stress σys0 uses values From material and represents the stress level where plastic deformation starts.
Plastic Potential
Select the Plastic potential Qp related to the flow rule — von Mises, Associated, or User defined (nonassociated). Enter a User defined value in the Qp field as needed.
Equivalent Plastic Strain
Select how the Equivalent plastic strain εpe is computed — von Mises, Associated, or User defined. Enter a User defined value in the hp field as needed. See Isotropic Plasticity for details.
Isotropic Hardening Model
For all yield criteria, select the type of linear or nonlinear isotropic hardening model from the Isotropic hardening model list. See Numerical Solution of the Elastoplastic Conditions for details.
Select Perfectly plastic (ideal plasticity) if the material can undergo plastic deformation without any increase in yield stress.
For Linear the default Isotropic tangent modulus ETiso uses values From material (if it exists) or User defined. The yield level σys is modified as hardening occurs, and it is related to the equivalent plastic strain εpe as
with
For the linear isotropic hardening model, the yield stress increases proportionally to the equivalent plastic strain εpe. The Young’s modulus E is taken from the elastic material properties.
Select Ludwik from the list to model nonlinear isotropic hardening. The yield level σys is modified by the power-law
The Strength coefficient k and the Hardening exponent n use values From material (if it exists) or User defined.
Select Johnson–Cook from the list to model strain rate dependent hardening. The Strength coefficient k, Hardening exponent n, Reference strain rate , and Strain rate strength coefficient C use values From material (if it exists) or User defined.
Select a Thermal softening modelNo thermal softening, Power law, or User defined.
-
For Power law, enter the Reference temperature Tref, the Melting temperature Tm, and the Temperature exponent, m.
-
For User defined, enter the Thermal Softening function f(Th), the Reference temperature Tref, and the Melting temperature Tm. The softening function f(Th) typically depends on the built-in variable for the normalized homologous temperature Th and have the properties f(0) = 0 and f(1) = 1. The variable is named using the scheme <physics>.<elasticTag>.<plasticTag>.Th, for example, solid.lemm1.plsty1.Th.
The yield stress and hardening function for the Johnson–Cook model is given by
In the case of power law softening, .
For Swift nonlinear isotropic hardening, the Reference strain ε0 and the Hardening exponent n use values From material (if it exists) or User defined. The yield level σys is modified by the power-law
Typically, the reference strain equals the onset of plasticity, ε0 = σys0/E.
Select Voce from the list to model nonlinear isotropic hardening. The yield level σys is modified by the exponential law
The Saturation flow stress σsat and the Saturation exponent β use values From material (if it exists) or User defined.
For Hockett–Sherby nonlinear isotropic hardening, the Steady-state flow stress σ, the Saturation coefficient m, and the Saturation exponent n use values From material (if it exists) or User defined. The yield level σys is increased by the exponential law
For Hardening function, the isotropic Hardening function σh(εpe) uses values From material or User defined. The yield level σys is modified as
-
This definition implies that the hardening function σh(εpe) in the Material node must be zero at zero plastic strain. In other words, σys = σys0 when εpe = 0. With this option it is possible to enter any nonlinear isotropic hardening curve. The hardening function can depend on more variables than the equivalent plastic strain, for example the temperature. Select User defined to enter any function of the equivalent plastic strain εpe. The variable is named using the scheme <physics>.epe, for example, solid.epe.
Kinematic Hardening Model
For all yield criteria, select the type of kinematic hardening model from the Kinematic hardening model list. See Kinematic Hardening for details.
Select No kinematic hardening (when either ideal plasticity or an isotropic hardening model is selected as isotropic hardening model) if it is a material that can undergo plastic deformation without a shift in the yield surface.
If Linear is selected as the Kinematic hardening model, the default Kinematic tangent modulus Ek uses values From material. This parameter is used to calculate the back stress σb as plasticity occurs:
with
This is Prager’s linear kinematic hardening model, so the back stress σb is collinear to the plastic strain tensor εp.
If Armstrong–Frederick is selected from the list, the default Kinematic hardening modulus Ck and Kinematic hardening parameter γk use values From material. These parameters are used to calculate the back stress σb from the rate equation
This is Armstrong–Frederick nonlinear kinematic hardening model. Replacing the variable for the back strain instead of the back stress
gives the rate for the back strain
When Chaboche is selected from the Kinematic hardening model list, the default Kinematic hardening modulus C0 uses values From material. Add branches as needed to solve N rate equations for the back stresses:
or equivalently, solve N rate equations for the back strain such as
The total back stress σb is then computed from the sum of the branches
For each Branch row, enter Ci (the hardening modulus of the branch i) in the Hardening modulus (Pa) column and γi (the hardening parameter of the branch i) in the Hardening parameter (1) column.
Use the Add button () and the Delete button () to add or delete a row in the table. Use the Load from file button () and the Save to file button () to load and store data for the branches in a text file with three space-separated columns (from left to right): the branch number, the hardening modulus for that branch, and the hardening parameter for that branch.
To compute the energy dissipation caused by plasticity, enable the Calculate dissipated energy check box in the Energy Dissipation section of the parent material node.
Nonlocal Plasticity Model
Nonlocal plasticity can be used to facilitate for example the modeling of material softening. Typical examples that involve material softening are finite strain plasticity and soil plasticity. In these situations, standard (local) plasticity calculations reveal a mesh fineness and topology dependence, where a mesh refinement fails to produce a physically sound solution. Nonlocal plasticity adds regularization to the equivalent plastic strain, thereby stabilizing the solution.
The default is None. Select Implicit Gradient to add nonlocal regularization to the equivalent plastic strain. Enter a value for the:
Length scale, lint. The length scale should not exceed the maximum element size of the mesh.
Nonlocal coupling modulus, Hnl. This stiffness is the penalization of the difference between the local and nonlocal variables. A larger value enforces the equivalent plastic strain εpe to be closer to the nonlocal equivalent plastic strain εpe,nl.
See also Nonlocal Plasticity in the Structural Mechanics Theory chapter.
Discretization
This section is available with the Implicit gradient nonlocal plasticity model. Select the shape function for the Nonlocal equivalent plastic strain εpe,nl Automatic, Linear, Quadratic Lagrange, Quadratic serendipity, Cubic Lagrange, Cubic serendipity, Quartic Lagrange, Quartic serendipity, or Quintic Lagrange. The available options depend on the order of the displacement field.
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.
Sheet Metal Forming: Application Library path Nonlinear_Structural_Materials_Module/Plasticity/sheet_metal_forming
For an example on large strain and nonlocal plasticity, see Necking of an Elastoplastic Metal Bar: Application Library path Nonlinear_Structural_Materials_Module/Plasticity/bar_necking.
For an example of strain rate dependent plasticity, see Tensile Test with Strain Rate Dependent Plasticity: Application Library path Nonlinear_Structural_Materials_Module/Plasticity/strain_rate_dependent_plasticity
Advanced
Select the Local method to solve the plasticity problem — Automatic or Backward Euler. When Backward Euler is selected, it is possible to specify the maximum number of iterations and the relative tolerance used to solve the local plasticity equations. Enter the following settings:
Maximum number of local iterations. To determine the maximum number of iteration in the Newton loop when solving the local plasticity equations. The default value is 25 iterations.
Relative tolerance. To check the convergence of the local plasticity equations based on the step size in the Newton loop. The final tolerance is computed based on the current solution of the local variable and the entered value. The default value is 1e-6.
For a 2D geometry, enable Include out-of-plane strains to solve for all components of the plastic strain tensor. By default, COMSOL assumes that the out-of-plane components are zero.
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.
See also Numerical Solution of the Elastoplastic Conditions in the Structural Mechanics Theory chapter.
Location in User Interface
Context Menus
Ribbon
Physics tab with Linear Elastic Material, Linear Elastic Material, Layered, Nonlinear Elastic Material, or Hyperelastic Material node selected in the model tree: