ABAQUS umat routines

There are two interfaces to include ABAQUS umat routines: umat_abaqus is meant to include linear materials, umat_abaqusnl for nonlinear materials. For nonlinear materials the logarithmic strain and infinitesimal rotation are calculated, which slows down the calculation. Consequently, the nonlinear routine should only be used if necessary.

The linear routine is triggered by putting ABAQUS in front of the material name. The total length of the material name should not exceed 80 characters, consequently, 74 characters are left for the proper material name. For instance, if the material name in the ABAQUS routine is supposed to be ``WOOD'', you must specify ``ABAQUSWOOD'' in the CalculiX input file. The part ``ABAQUS'' is removed from the name before entering the umat routine.

The nonlinear routine is triggered by putting ABAQUSNL in front of the material name.

Notice that the following fields are not supported so far: sse, spd, scd, rpl, ddsddt, drplde, drpldt, predef, dpred, drot, pnewdt, celent, layer, kspt. If you need these fields, contact ``dhondt@t-online.de''. Furthermore, the following fields have a different meaning:

• in the linear version:
  • stran:
    • in CalculiX: Lagrangian strain tensor
    • in ABAQUS: logarithmic strain tensor
  • dstran:
    • in CalculiX: Lagrangian strain increment tensor
    • in ABAQUS: logarithmic strain increment tensor
  • temp:
    • in CalculiX: temperature at the end of the increment
    • in ABAQUS: temperature at the start of the increment
  • dtemp:
    • in CalculiX: zero
    • in ABAQUS: temperature increment
• in the nonlinear version:
  • temp:
    • in CalculiX: temperature at the end of the increment
    • in ABAQUS: temperature at the start of the increment
  • dtemp:
    • in CalculiX: zero
    • in ABAQUS: temperature increment