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

This section is only present when Creep is used as a subnode to:
Linear Elastic Material in the Layered Shell interface. See the documentation for the Creep node in the Layered Shell chapter.
Linear Elastic Material, Layered in the Shell interface. See the documentation for the Creep node in the Shell and Plate chapter.
Linear Elastic Material, Layered in the Membrane interface. See the documentation for the Creep node in the Membrane chapter.
Creep Model
Select the FormulationSmall strains or Large strains to apply either an additive or multiplicative decomposition between elastic and inelastic strains.
Select a Material modelNorton, Garofalo (hyperbolic sine), Nabarro–Herring, Coble, Weertman, or User defined.
Norton
For Norton, enter the following settings:
Reference stress σref. The default is 1 MPa.
Garofalo (Hyperbolic Sine)
For Garofalo (hyperbolic sine), enter the following settings:
Reference stress σref. The default is 1 MPa.
Nabarro–Herring
For Nabarro–Herring, enter the following settings:
Coble
For Coble enter the following settings:
Weertman
For Weertman, enter the following settings:
Reference stress σref. The default is 1 MPa.
User Defined
For User defined, enter an expression for the creep rate f as a function of the equivalent stress σe. The default expression is <item>.sequ/1[Pa*s], where <item> is the name of the creep node.
For Norton, Garofalo (hyperbolic sine), Nabarro–Herring, Coble, Weertman, or User defined, select an Equivalent stress von Mises (the default), Hill orthotropic, pressure, or User defined.
Isotropic Hardening Model
Select the isotropic hardening function hNone, Strain hardening, Time hardening, or User defined.
Strain hardening
For Strain hardening, enter the following settings:
Hardening exponent m. The default is 0.
Equivalent creep strain shift εshift. The default is 1e-5.
Reference time tref. The default is 1 h.
Time hardening
For Time hardening, enter the following settings:
Hardening exponent m. The default is 0.
Time shift tshift. The default is 0 s.
Reference time tref. The default is 1 h.
User defined
For User defined, enter an expression for the hardening function h as a function of equivalent creep strain εce, time t or any other variable in the model.
Thermal Effects
Select a thermal creep function — None, Arrhenius, or User defined.
Arrhenius
For Arrhenius, enter the following setting:
Reference temperature Tref. The default value, Inf, corresponds to omitting the term with Tref in the Arrhenius expression.
Creep activation energy Q. The default is 0 J/mol.
User defined
For User defined, enter an expression for the thermal creep function g as a function of temperature T or any other variable in the model.
Time Stepping
Select a MethodAutomatic, Backward Euler, Forward Euler, or Domain ODEs.
The Backward Euler method is not available with the Layered Shell interface nor with the Linear Elastic Material, Layered material model in the Shell and Membrane interfaces.
Automatic
The Automatic method corresponds to the backward Euler method except for the Layered Shell interface or when Linear Elastic Material, Layered is used. Domain ODEs are solved in these cases.
Backward Euler
For the Backward Euler method, you can make the following settings:
Maximum number of local iterations. This defines the maximum number of iterations of the Newton loop when solving the local creep equations.
Absolute tolerance. This defines the absolute tolerance for convergence of the local creep equations. Convergence is judged based on the step size, that is, the size of the Newton correction, of each equation.
Relative tolerance. This defines the relative tolerance for convergence of the local creep equations. Convergence is judged based on the step size, that is, the size of the Newton correction, of each equation.
Residual tolerance. This defines the tolerance for convergence of the local creep equations based on the residual of each equation.
Setting either the Absolute tolerance and Relative tolerance, or the Residual tolerance to zero ignores the corresponding convergence check. An error is returned if all are set to zero. If both a step size and residual convergence check is requested, it is sufficient that one of the conditions is satisfied for convergence.
Forward Euler
For the Forward Euler method, enter the Maximum creep strain increment.
It is recommend to reset the solver settings to its default values when selecting the forward Euler method, since the method is only conditionally stable. This will add a Maximum step constraint to the Time-Dependent Solver based on an estimate of the stability limit used to update the creep equations. The value entered in the Maximum creep strain increment field is taken in to account, which can be used to improve the accuracy of the method. If the solver sequence cannot be reset, the stability limit can be entered manually in the Time-Dependent Solver settings by using the variable <item>.tmax, where <item> is the name of the creep node.
Domain ODEs
No settings are needed for the Domain ODEs method. However, this method adds degrees-of-freedom that are solved as part of the general solver sequence. The scaling of these fields can affect the convergence of the overall solution.
Advanced
For a 2D geometry, enable Include out-of-plane strains to solve for all components of the creep 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.
To compute the energy dissipation caused by creep, enable the Calculate dissipated energy check box in the Energy Dissipation section of the parent material node (Linear Elastic Material, Nonlinear Elastic Material, or Hyperelastic Material).
Location in User Interface
Context Menus
Ribbon
Physics tab with Linear Elastic Material, Linear Elastic Material, Layered, Hyperelastic Material, or Nonlinear Elastic Material node selected in the model tree: