Abaqus/CAE User's Manual  


12.9.4 Defining other mechanical models

You can create the following additional material models:

Defining deformation plasticity

Abaqus/Standard provides a deformation theory Ramberg-Osgood plasticity model for use in developing fully plastic solutions for fracture mechanics applications in ductile metals. The model is most commonly applied in static loading with small-displacement analysis for which the fully plastic solution must be developed in a part of the model.

See “Deformation plasticity,” Section 19.2.13 of the Abaqus Analysis User's Manual, for more information.

To define a deformation plasticity model:

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

    (For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)

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

    A column labeled Temp appears in the Data table.

  3. Enter the following data in the Data table:

    Young's Modulus

    Young's modulus, E, defined as the slope of the stress-strain curve at zero stress.

    Poisson's Ratio

    Poisson's ratio, .

    Yield Stress

    Yield stress, .

    Exponent

    Hardening exponent, n, for the plastic (nonlinear term).

    Yield Offset

    Yield offset, .

    Temp

    Temperature.

    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,” Section 3.2.7.

  4. 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,” Section 12.7.2, for more information).

Defining damping

You can define damping for mode-based analyses and for direct-integration dynamic analysis in Abaqus/Standard and for explicit dynamic analysis in Abaqus/Explicit. See “Dynamic analysis procedures: overview,” Section 6.3.1 of the Abaqus Analysis User's Manual, and “Material damping,” Section 22.1.1 of the Abaqus Analysis User's Manual, for more information.

To define damping:

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

    (For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)

  2. In the Alpha field, enter a value for the factor to create Rayleigh mass proportional damping. The default is 0. (Units of T–1.)

  3. In the Beta field, enter a value for the factor to create Rayleigh stiffness proportional damping. The default is 0. (Units of T.)

  4. In the Composite field, enter a value for the fraction of critical damping to be used with this material in calculating composite damping factors for the modes. The default is 0. (This value applies only to Abaqus/Standard analyses.)

  5. In the Structural field, enter a value for the factor to create imaginary stiffness proportional damping. The default is 0.

  6. 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,” Section 12.7.2, for more information).

Defining thermal expansion

You can define thermal expansion either by entering thermal expansion coefficients in the Edit Material dialog box or, if the thermal strains are complicated functions of field and state variables, with user subroutine UEXPAN. See “Thermal expansion,” Section 22.1.2 of the Abaqus Analysis User's Manual, for more information.

To define thermal expansion:

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

    (For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)

  2. Click the arrow to the right of the Type field, and specify the directional dependence of the thermal expansion.

  3. Toggle on Use user subroutine UEXPAN if you want to define the increments of thermal strain in user subroutine UEXPAN.

  4. If you toggled on Use user subroutine UEXPAN, 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,” Section 12.7.2 for more information).

    If you choose to specify thermal expansion coefficients directly in the Edit Material dialog box, perform the remaining steps in this procedure.

  5. If the thermal expansion is temperature- or field-variable-dependent, enter a value for the Reference temperature, .

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

    A column labeled Temp appears in the Data table.

  7. 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.

  8. Enter the applicable data in the Data table:

    Expansion Coeff alpha

    Isotropic thermal expansion coefficient, . (Units of –1.)

    alpha11, alpha22, and alpha33

    Three values to define orthotropic thermal expansion, , , and . (Units of –1.)

    alpha11, alpha22, alpha33, alpha12, alpha13, and alpha23

    Six values to define anisotropic thermal expansion, , , , , , and . (Units of –1.)

    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,” Section 3.2.7.

  9. 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,” Section 12.7.2, for more information).

Defining brittle cracking

You can use the brittle cracking model in Abaqus/Explicit for applications in which the concrete behavior is dominated by tensile cracking and compressive failure is unimportant. See “Cracking model for concrete,” Section 19.6.2 of the Abaqus Analysis User's Manual, for more information.

Defining a brittle cracking model

The brittle cracking model in Abaqus/Explicit is most accurate in applications where the brittle behavior dominates and it is adequate to assume that the material is linear elastic in compression. You can use this model for plain concrete and for other materials such as ceramics or brittle rocks, but it is primarily intended for the analysis of reinforced concrete structures. See “Cracking model for concrete,” Section 19.6.2 of the Abaqus Analysis User's Manual, for more information.

To define a brittle cracking model:

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

    (For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)

  2. Click the arrow to the right of the Type field, and select a method for defining the postcracking behavior:

    • Select Strain to specify the postcracking behavior by entering the postfailure stress-strain relationship directly.

    • Select Displacement to define the postcracking behavior by entering the postfailure stress/displacement relationship directly.

    • Select GFI to define the postcracking behavior by entering the failure stress and the Mode I fracture energy.

  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 Strain or Displacement from the list of Type options, enter the following data in the Data table:

    Direct stress after cracking

    Remaining direct stress after cracking, . (Units of .)

    Direct cracking strain

    Direct cracking strain, . (Enter this value if you selected Strain from the list of Type options.)

    Direct cracking displacement

    Direct cracking displacement, . (Units of L.) (Enter this value if you selected Displacement from the list of Type options.)

    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,” Section 3.2.7.

  6. If you selected GFI from the list of Type options, enter the following data in the Data table:

    Failure stress

    Failure stress, . (Units of .)

    Mode I fracture energy

    Mode I fracture energy, . (Units of .)

    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,” Section 3.2.7.

  7. Select Brittle Shear from the Suboptions menu to define the postcracking shear behavior of the material. See “Defining brittle shear” for details.

  8. If desired, select Brittle Failure from the Suboptions menu to specify the brittle failure criterion. See “Defining brittle failure” for details.

  9. 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,” Section 12.7.2, for more information).

Defining brittle shear

An important feature of the cracking model is that, while crack initiation is based on Mode I fracture only, postcracked behavior includes Mode II as well as Mode I.

Mode II shear behavior is based on the common observation that the shear behavior depends on the amount of crack opening. More specifically, the cracked shear modulus is reduced as the crack opens. Therefore, Abaqus/Explicit offers a shear retention model in which the postcracked shear stiffness is defined as a function of the opening strain across the crack.

You must provide postcracking shear data to complete a brittle cracking model definition. See “Shear retention model” in “Cracking model for concrete,” Section 19.6.2 of the Abaqus Analysis User's Manual, for more information.

To define brittle shear:

  1. Create a material model as described in “Defining a brittle cracking model.”

  2. From the Suboptions menu in the Edit Material dialog box, select Brittle Shear.

    A Suboption Editor appears.

  3. Click the arrow to the right of the Type field, and select a method for specifying postcracking shear behavior:

    • Select Retention Factor to specify the postcracking shear behavior by entering the shear retention factor-crack opening strain relationship directly.

    • Select Power Law to specify the postcracking shear behavior by entering the mateiral parameters for the power law shear retention model.

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

    A column labeled Temp appears in the Data table.

  5. 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.

  6. If you selected Retention Factor from the list of Type options, enter the following data in the Data table:

    Shear retention factor

    Shear retention factor, .

    Crack opening strain

    Crack opening strain, .

    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,” Section 3.2.7.

  7. If you selected Power Law from the list of Type options, enter the following data in the Data table:

    e and p

    Material parameters and p.

    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,” Section 3.2.7.

  8. Click OK to return to the Edit Material dialog box.

Defining brittle failure

When one, two, or all three local direct cracking strain or displacement components at a material point reach the value defined as the failure strain or displacement, the material point fails and all the stress components are set to zero. If all of the material points in an element fail, the element is removed from the mesh. See “Brittle failure criterion” in “Cracking model for concrete,” Section 19.6.2 of the Abaqus Analysis User's Manual, for more information.

To define brittle failure:

  1. Create a material model as described in “Defining a brittle cracking model.”

  2. From the Suboptions menu in the Edit Material dialog box, select Brittle Failure.

    A Suboption Editor appears.

  3. Select an option from the list of Failure criteria:

    • Select Unidirectional to indicate that an element will be removed when any local direct cracking strain (or displacement) component reaches the failure value.

    • Select Bidirectional to indicate that an element will be removed when any two direct cracking strain (or displacement) components reach the failure value.

    • Select Tridirectional to indicate that an element will be removed when all three possible direct cracking strain (or displacement) components reach the failure value.

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

    A column labeled Temp appears in the Data table.

  5. 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.

  6. Enter the following data in the Data table:

    Direct cracking failure strain or displacement

    The value you enter depends on the method you chose in the Edit Material dialog box for specifying postcracking behavior (as described in “Defining a brittle cracking model”).

    If you selected Strain, enter the direct cracking failure strain, .

    If you selected Displacement or GFI, enter the direct cracking failure displacement, . (Units of L.)

    Temp

    Temperature.

    Field n

    Predefined field variables.

  7. Click OK to return to the Edit Material dialog box.