In the stress and strain arrays and in the matrices DDSDDE, DDSDDT, and DRPLDE, direct components are stored first, followed by shear components. There are NDI direct and NSHR engineering shear components. The order of the components is defined in “Conventions,” Section 1.2.2 of the Abaqus Analysis User's Guide. Since the number of active stress and strain components varies between element types, the routine must be coded to provide for all element types with which it will be used.

If a local orientation (“Orientations,” Section 2.2.5 of the Abaqus Analysis User's Guide) is used at the same point as user subroutine UMAT, the stress and strain components will be in the local orientation; and, in the case of finite-strain analysis, the basis system in which stress and strain components are stored rotates with the material.

You should ensure that the integration scheme coded in this routine is stable—no direct provision is made to include a stability limit in the time stepping scheme based on the calculations in UMAT.

DDSDDE and—for coupled temperature-displacement and coupled thermal-electrical-structural analyses—DDSDDT, DRPLDE, and DRPLDT must be defined accurately if rapid convergence of the overall Newton scheme is to be achieved. In most cases the accuracy of this definition is the most important factor governing the convergence rate. Since nonsymmetric equation solution is as much as four times as expensive as the corresponding symmetric system, if the constitutive Jacobian (DDSDDE) is only slightly nonsymmetric (for example, a frictional material with a small friction angle), it may be less expensive computationally to use a symmetric approximation and accept a slower convergence rate.

An incorrect definition of the material Jacobian affects only the convergence rate; the results (if obtained) are unaffected.

The constitutive Jacobian (DDSDDE) must provide both the stiffness (storage modulus) and damping (loss modulus) for modeling frequency domain viscoelastic behavior.

There are several special considerations that need to be noted.

Open-section beam elements

When user subroutine UMAT is used to describe the material response of beams with open sections (for example, an I-section), the torsional stiffness is obtained as

where J is the torsional constant, A is the section area, k is a shear factor, and is the user-specified transverse shear stiffness (see “Transverse shear stiffness definition” in “Choosing a beam element,” Section 29.3.3 of the Abaqus Analysis User's Guide).

If the material model allows large volume changes and geometric nonlinearity is considered, the exact definition of the consistent Jacobian should be used to ensure rapid convergence. These conditions are most commonly encountered when considering either large elastic strains or pressure-dependent plasticity. In the former case, total-form constitutive equations relating the Cauchy stress to the deformation gradient are commonly used; in the latter case, rate-form constitutive laws are generally used.

For total-form constitutive laws, the exact consistent Jacobian is defined through the variation in Kirchhoff stress:

For rate-form constitutive laws, the exact consistent Jacobian is given by

For user-defined almost incompressible or incompressible elastic materials, a few different options are available depending on whether hybrid or nonhybrid elements are used. For all cases the first option should be to use user subroutine UHYPER instead of user subroutine UMAT when it is possible to do so. In user subroutine UMAT incompressible materials can be modeled via a penalty method; that is, you ensure that a finite bulk modulus is used. The bulk modulus should be large enough to model incompressibility sufficiently but small enough to avoid loss of precision. As a general guideline, the bulk modulus should be about – times the shear modulus. The tangent bulk modulus can be calculated from

If a hybrid element is used with user subroutine UMAT, Abaqus/Standard, by default, replaces the pressure stress calculated from your definition of STRESS with that derived from the Lagrange multiplier and modifies the Jacobian appropriately (“Hybrid incompressible solid element formulation,” Section 3.2.3 of the Abaqus Theory Guide). This approach is suitable for material models that use an incremental formulation (for example, metal plasticity) but is not consistent with a total formulation that is commonly used for hyperelastic materials. In the latter situation, the default formulation may lead to convergence problems. Such convergence problems may be observed, for example, when an almost incompressible nonlinear elastic user material is subjected to large deformations. Abaqus/Standard provides an alternate total formulation when user materials are used with hybrid elements (see “User-defined mechanical material behavior,” Section 26.7.1 of the Abaqus Analysis User's Guide). This formulation is consistent with the native almost incompressible formulation used by Abaqus for hyperelastic materials (“Hyperelastic material behavior,” Section 4.6.1 of the Abaqus Theory Guide) and works better than the default formulation for such cases.

The total hybrid formulation assumes that the response of the material can be written as the sum of its deviatoric and volumetric parts and that these parts are decoupled from each other. In particular, the volumetric response is assumed to be defined in terms of a strain energy potential, , which is a function of an alternate variable, in place of the actual volume change . The alternate variable is made available inside user subroutine UMAT by extending the STRESS array beyond NTENS, with the NTENS+1 entry providing read access to . You must define the hydrostatic part of the stress tensor as . The formulation also requires the additional derivatives and . You must define these additional derivatives inside user subroutine UMAT as the NTENS+1 and the NTENS+2 entry, respectively, of the STRESS array. In addition, the bulk modulus of the material (contributes toward the material Jacobian matrix, DDSDDE) must be defined as

Abaqus/Standard also provides a fully incompressible user material formulation for use with hybrid elements to define a fully incompressible user material response. This formulation is consistent with the native formulation used by Abaqus for incompressible hyperelastic materials and assumes that the deviatoric stress can be derived from a strain energy potential function. You need define only the deviatoric stress and Jacobian to define a fully incompressible material response through user subroutine UMAT.

For incompressible pressure-sensitive materials the element choice is particularly important when using user subroutine UMAT. In particular, first-order wedge elements should be avoided. For these elements the technique is not used to alter the deformation gradient that is passed into user subroutine UMAT, which increases the risk of volumetric locking.

Abaqus/Standard passes zero strain increments into user subroutine UMAT to start the first increment of all the steps and all increments of steps for which you have suppressed extrapolation (see “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide). In this case you can define only the Jacobian (DDSDDE).

Several utility routines may help in coding user subroutine UMAT. Their functions include determining stress invariants for a stress tensor and calculating principal values and directions for stress or strain tensors. These utility routines are discussed in detail in “Obtaining stress invariants, principal stress/strain values and directions, and rotating tensors in an Abaqus/Standard analysis,” Section 2.1.11.