UMAT_Lefevre_Sozio_Lopez-Pamies

Description

This Abaqus UMAT subroutine implements a family of internal-variable-based constitutive models for the viscoelastic response of elastomers of any compressibility — including fully incompressible elastomers — undergoing finite deformations, that introduced by Kumar and Lopez-Pamies [1]. The models can be chosen to account for a wide range of non-Gaussian elasticities, as well as for a wide range of nonlinear viscosities.

The present subroutine is implemented for the choice of two-term Lopez-Pamies non-Gaussian elasticities [2] and deformation-enhanced shear-thinning nonlinear viscosity proposed in [1]. It relies on a hybrid formulation [3] to deal with nearly or fully incompressible elastomers.

Usage

The subroutine is to be used as a USER MATERIAL with 15 material CONSTANTS and a TOTAL HYBRID FORMULATION, e.g.,

*USER MATERIAL,CONSTANTS=15,HYBRID FORMULATION=TOTAL

in the input (.inp) file. Due to the hybrid nature of the underlying formulation, hybrid finite elements must be used in the simulation.

Material properties

The 15 material properties of the model are the primary inputs of the subroutine and are listed in order below:

• AMU1: parameter #1 of the equilibrium elasticity
• AALPHA1: exponent #1 of the equilibrium elasticity
• AMU2: parameter #2 of the equilibrium elasticity
• AALPHA2: exponent #2 of the equilibrium elasticity
• AKAPPAE: bulk modulus of the equilibrium elasticity
• AA1: exponent #1 of the non-equilibrium elasticity
• AM2: parameter #2 of the non-equilibrium elasticity
• AA2: exponent #2 of the non-equilibrium elasticity
• AM1: parameter #1 of the non-equilibrium elasticity
• AETA0: parameter #1 of the deviatoric viscosity
• AETAI: parameter #2 of the deviatoric viscosity
• ABETA1: exponent #1 of the deviatoric viscosity
• ABETA2: exponent #2 of the deviatoric viscosity
• AK1: factor #1 of the deviatoric viscosity
• AK2: factor #2 of the deviatoric viscosity

They are entered in the input (.inp) file as follows:

*USER MATERIAL,CONSTANTS=15,HYBRID FORMULATION=TOTAL
AMU1, AALPHA1, AMU2, AALPHA2, AKAPPAE, AM1, AA1, AM2,
AA2, AETA0, AETAI, ABETA1, ABETA2, AK1, AK2

The material parameters AMU1, AMU2 characterizing the equilibrium elasticity are non-negative real numbers (AMU1 ≥ 0, AMU2 ≥ 0) with strictly positive sum (AMU1 + AMU2 > 0).

The two exponents AALPHA1, AALPHA2 are non-zero real numbers (AALPHA1 ≠ 0, AALPHA2 ≠ 0) with MAX{AALPHA1, AALPHA2} > 0 leading to a strongly elliptic strain energy (see eq. (22) in [2]). This is left to the user to check.

The material parameter AKAPPAE characterizing the compressibility of the equilibrium elasticity is a strictly positive real number (AKAPPAE > 0). The material parameters AM1, AM2 characterizing the non-equilibrium elasticity are non-negative real numbers (AM1 ≥ 0, AM2 ≥ 0) with strictly positive sum (AM1 + AM2 > 0).

The two exponents AA1, AA2 are non-zero real numbers (AA1 ≠ 0, AA2 ≠ 0) with MAX{AA1, AA2} > 0 leading to a strongly elliptic strain energy (see eq. (22) in [2]). This is left to the user to check.

The material parameters AETA0, AETAI, ABETA1, ABETA2, AK1, AK2 characterizing the viscous dissipation are all non-negative real numbers (AETA0 ≥ 0, AETAI ≥ 0, ABETA1 ≥ 0, ABETA2 ≥ 0, AK1 ≥ 0, AK2 ≥ 0).

Solution-dependent state variables

• The subroutine uses solution-dependent state variables for the independent components of the symmetric tensorial internal variable ${\mathbf{C}}^{v-1}$. The space for the state variables must be allocated in the input file using the *DEPVAR keyword:

  *DEPVAR
  NSTATV
  

  where NSTATV is the number of state variables required. NSTATV depends on the type of finite elements used:

  • NSTATV = 4 for elements with only 1 non-zero shear component (CPE3H, CPE4H, CPE6H, CPE8H, CAX3H, CAX4H, CAX6H, CAX8H, CPEG3H, CPEG4H, CPEG6H, CPEG8H, ...)
  • NSTATV = 6 for elements with all 3 non-zero shear components (C3D4H, C3D8H, C3D10H, C3D20H, CGAX3H, CGAX4H, CGAX6H, CGAX8H, ...)

  Note that an incorrect value of NSTATV will trigger an error in the subroutine and the error message in the .msg file will indicate the expected value for NSTATV.

• The values of state variables must be initialized according to the initial condition ${\mathbf{C}}^{v-1}={\mathbf{I}}$ using the *INITIAL CONDITIONS keyword as follows:

  • NSTATV = 4:

    *INITIAL CONDITIONS, TYPE=SOLUTION
    ALLELEMENTSET,1.0,1.0,1.0,0.0    
    

  • NSTATV = 6:

    *INITIAL CONDITIONS, TYPE=SOLUTION
    ALLELEMENTSET,1.0,1.0,1.0,0.0,0.0,0.0
    

  where ALLELEMENTSET is an element set of all finite elements associated with the UMAT material.

Energy outputs

• The subroutine uses the variable SSE to output $\psi^E = \Psi^E / J$, the strain energy density per deformed unit volume in the equilibrium branch.

  The corresponding contour plot can be obtained by including the output variable identifier SENER in the element output request keyword *ELEMENT OUTPUT.

  The corresponding total energy (i.e., the volume internal of SSE) can be obtained by including the output variable identifier ALLSE in the history output request keyword *ENERGY OUTPUT.

• The subroutine uses the variable SPD to output $\psi^{NE} = \Psi^{NE} / J$, the strain energy density per deformed unit volume in the non-equilibrium branch. Note that this use of the SPD variable is different from the typical meaning of the SPD variable in UMAT subroutines, which is the plastic dissipation density.

  The corresponding contour plot can be obtained by including the output variable identifier PENER in the element output request keyword *ELEMENT OUTPUT.

  The corresponding total energy (i.e., the volume internal of SPD) can be obtained by including the output variable identifier ALLPD in the history output request keyword *ENERGY OUTPUT.

Contour plots

• Contour plots of the components of the internal variable ${\mathbf{C}}^{v-1}$ can be obtained by including the output variable identifier SDV in the element output request keyword *ELEMENT OUTPUT.

• A UVARM subroutine is also included to create two user output variable, UVARM1 = $I_1$ = $\text{tr}({\mathbf{F}}^T{\mathbf{F}})$ and UVARM2 = $J$ = $\text{det(F)}$. The space for these user output variables must be allocated in the input file using the *USER OUTPUT VARIABLES keyword:

  *USER OUTPUT VARIABLES
  2
  

  The corresponding contour plots can be obtained by including the output variable identifier UVARM in the element output request keyword *ELEMENT OUTPUT.

Additional information

• This subroutine doesn't create predefined field variables.
• Please consult the Abaqus Documentation for additional references regarding the use of the UMAT subroutine for (near-)incompressible material models.

Documented errors

• The line #INCLUDE <SMAASPUSERSUBROUTINES.HDR>, which appears twice in the code (lines 848 and 1235), has generated errors on some versions of Abaqus, but not on others. If the line generates an error, you can comment it out by including the character C as the first character of the line. It is expected that the code will work after this modification.

Examples

The Examples folder contains examples of how to use the present subroutine.

References

The references below can be found in the References folder.

1. Kumar, A., Lopez-Pamies, O., 2016. On the two-potential constitutive modeling of rubber viscoelastic materials. Comptes Rendus Mécanique 344, 102–112.
2. Lopez-Pamies, O., 2010. A new I1-based hyperelastic model for rubber elastic materials. Comptes Rendus Mécanique 338, 3–11.
3. Lefèvre, V., Sozio, F., Lopez-Pamies, O., 2024. Abaqus implementation of a large family of finite viscoelasticity models. Finite Elements in Analysis and Design 232, 104114.