Defining the viscous component of a two-layer viscoplasticity model

The two-layer viscoplasticity model in Abaqus/Standard is useful for modeling materials in which significant time-dependent behavior as well as plasticity is observed. For metals this typically occurs at elevated temperatures. This model consists of three parts: elastic, plastic, and viscous. You can define the viscous behavior of the material by selecting a creep law and entering viscosity parameters. See Two-layer viscoplasticity, for more information.

  1. From the menu bar in the Edit Material dialog box, select MechanicalPlasticityViscous.

    (For information on displaying the Edit Material dialog box, see Creating or editing a material.)

  2. Click the arrow to the right of the Law field, and select the creep law of your choice:

    • Select Strain to choose a strain-hardening power law.

    • Select Time to choose a time-hardening power law.

    • Select User to define the creep law with user subroutine CREEP.

    See Creep behavior, for more information.

  3. Toggle on Use temperature-dependent data to define data that depend on temperature.

    A column labeled Temp appears in the Data table.

  4. Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.

  5. If you selected the Strain-Hardening or Time-Hardening creep law, enter the following data in the Data table:

    A

    Power law multiplier, A. (Units of F-nL2⁢nT-1-m.)

    n

    Equivalent deviatoric stress order, n.

    m

    Total time or equivalent creep strain order, m.

    f

    The fraction, f, that defines the ratio of the elastic modulus of the elastic-viscous network to the total (instantaneous) modulus.

    Temp

    Temperature.

    Field n

    Predefined field variables.

    You may need to expand the dialog box to see all the columns in the Data table. For detailed information on how to enter data, see Entering tabular data.

  6. If you are defining the creep law with user subroutine CREEP, enter the following in the Data table:

    f

    The fraction, f, that defines the ratio of the elastic modulus of the elastic-viscous network to the total (instantaneous) modulus.

    Temp

    Temperature.

    Field n

    Predefined field variables.

    For detailed information on how to enter data, see Entering tabular data.

  7. If desired, select Potential from the Suboptions menu to define anisotropic viscosity. See Defining anisotropic yield and creep” for details.

  8. Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see Browsing and modifying material behaviors, for more information).