Elastic anisotropy with user defined isotropic creep.

This material model is similar to the previous one, except that

no plasticity is assumed (yield surface coincides with the origin)
the creep model is to be provided by a creep user subroutine

It is activated as soon as a *ELASTIC, TYPE=ORTHO card is followed by a *CREEP, LAW=USER card.

In the present implementation orthotropic elastic behavior is assumed. Consequently, for each temperature 9 constants need to be defined: the elastic constants $C_{1111}$ , $C_{1122}$ , $C_{2222}$ , $C_{1133}$ , $C_{2233}$ , $C_{3333}$ , $C_{1212}$ , $C_{1313}$ and $C_{2323}$ .

The material definition consists of a *MATERIAL card defining the name of the material. The elastic constants are to be defined underneath a *ELASTIC, TYPE=ORTHO card. The creep user subroutine (creep.f) is activated by a *CREEP, LAW=USER card.

The principal axes of the material are assumed to coincide with the global coordinate system. If this is not the case, use an *ORIENTATION card to define a local system.

For this model, there are 7 internal state variables (recall that CalculiX does not make a distinction between plastic strain and creep strain: the field ${\epsilon^p}$ contains the sum of both):

the equivalent plastic strain ${\epsilon}^{peq}$ (1)
the plastic strain tensor ${\epsilon^p}$ (6)

These variables are accessible through the *EL PRINT (.dat file) and *EL FILE (.frd file) keywords in exactly this order (label SDV).

The creep subroutine has to be provided by the user (cf. Section 8.1). Since the material is anisotropic the input to the creep routine is the equivalent deviatoric creep strain, the output is the von Mises stress and the derivative of the equivalent deviatoric creep strain increment w.r.t. the von Mises stress.

This model is for small deformations (small strains and small rotations). However, if NLGEOM is activated on the *STEP card this model is considered to be an Abaqus umat routine linking the corotational Cauchy stress to the corotational mechanical logarithmic strain. In this way, the routine can also be used for large deformations.

Example:

*MATERIAL,NAME=MAT
*ELASTIC,TYPE=ORTHO
500000.,157200.,500000.,157200.,157200.,500000.,126200.,126200.,
126200.
*CREEP,LAW=USER

defines a single crystal with elastic constants 500000., 157200., 500000., 157200., 157200., 500000., 126200., 126200. and 126200.. The creep law has to be provide by the user in the form of a creep.f subroutine.

Example files: beamcr4.