Marciniak-Kuczynski (M-K) damage

The M-K damage initiation criterion is used to predict sheet metal forming limits for arbitrary loading paths. The model introduces thickness imperfections, in the form of grooves, in the sheet material to simulate defects. Damage occurs when the ratio of deformation in the grooves relative to deformation in the original sheet thickness exceeds a critical value. By default, Abaqus evaluates four grooves at equally spaced angles of 0°, 45°, 90°, and 135° with respect to the local 1-direction of the material at each time increment and uses the worst result to determine damage initiation. The M-K criterion can be used in conjunction with the Mises and Johnson-Cook plasticity models, including kinematic hardening.

Context:

For more information, see Damage initiation for ductile metals.

  1. From the menu bar in the Edit Material dialog box, select MechanicalDamage for Ductile MetalsM-K Damage.

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

  2. To define material damage data that depend on temperature, toggle on Use temperature-dependent data.

    A column labeled Temp appears in the Data table.

  3. To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.

    Field variable columns appear in the Data table.

  4. If desired, modify the critical deformation severity factors Fe⁢q, Fn⁢n, and Fn⁢t.

    The severity factors each have a default value of 10 and are related to the ratios of equivalent plastic, normal, and tangential strain in the groove area compared to the nominal thickness area. Abaqus/Explicit will ignore severity factors that are set to 0. If all of these parameters are set equal to zero, the M-K criterion is based solely on nonconvergence of the equilibrium and compatibility equations.

  5. Select the Frequency—the number of increments between calculating the M-K criterion.

    Using the default frequency, 1, can be expensive since Abaqus evaluates each groove at every increment.

  6. Select the Number of imperfections—the number of angular groove positions to evaluate.

    The groove positions are equally spaced, starting at 0° and ending at 180⁢(n-1)n with respect to the local 1-direction of the material.

  7. Enter damage parameters in the Data table:

    Groove Size

    The ratio of the thickness at the groove to the nominal material thickness.

    Angle

    The starting angle (in degrees) with respect to the 1-direction of the local material orientation.

    Temp

    Temperature, θ.

    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.

  8. Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.

    For more information, see Damage evolution.”

  9. Click OK to exit the material editor.