User-defined mechanical material laws. next up previous contents
Next: ABAQUS umat routines Up: User subroutines. Previous: Gap conductance (gapcon.f)   Contents


User-defined mechanical material laws.

This is an extremely important and powerful interface, allowing the user to define his/her own mechanical material behavior. The subroutine ``umat.f'' is a driver subroutine, calling user-defined routines similar to ``umat_user.f'', depending on the kind of material present in the model. To create a new material law, a ``umat_user.f'' routine must be written and an appropriate call must be inserted in routine ``umat.f''. In ``umat.f'' the name of the user material is to be defined. This is a character string the NAME parameter following the keyword card *MATERIAL has to start with. For instance, if you define a new material with the name FUNNY_MATERIAL, then in order to use this material, the material name has to start with this string. This is the main difference in usage between predefined and user-defined materials in CalculiX: if you use predefined materials you are completely free to choose a name for your material, if you use a user-defined material, its name has to start with a predefined string. Since a material name can be up to 80 characters long, there is generally enough freedom to define several versions of this material, e.g. FUNNY_MATERIAL1, FUNNY_MATERIAL2 etc.

The header and input/output variables of the umat_user routine are as follows:

      subroutine umat_user(amat,iel,iint,kode,elconloc,emec,emec0,
     &        beta,xokl,voj,xkl,vj,ithermal,t1l,dtime,time,ttime,
     &        icmd,ielas,mint_,nstate_,xstateini,xstate,stre,stiff,
     &        iorien,pgauss,orab,pnewdt)
!
!     calculates stiffness and stresses for a user defined material
!     law
!
!     icmd=3: calcutates stress at mechanical strain
!     else: calculates stress at mechanical strain and the stiffness
!           matrix
!
!     INPUT:
!
!     amat               material name
!     iel                element number
!     iint               integration point number
!
!     kode               material type (-100-#of constants entered
!                        under *USER MATERIAL): can be used for materials
!                        with varying number of constants
!
!     elconloc(21)       user defined constants defined by the keyword
!                        card *USER MATERIAL (max. 21, actual # =
!                        -kode-100), interpolated for the
!                        actual temperature t1l
!
!     emec(6)            Lagrange mechanical strain tensor (component order:
!                        11,22,33,12,13,23) at the end of the increment
!                        (thermal strains are subtracted)
!     emec0(6)           Lagrange mechanical strain tensor at the start of the
!                        increment (thermal strains are subtracted)
!     beta(6)            residual stress tensor (the stress entered under
!                        the keyword *INITIAL CONDITIONS,TYPE=STRESS)
!
!     xokl(3,3)          deformation gradient at the start of the increment
!     voj                Jacobian at the start of the increment
!     xkl(3,3)           deformation gradient at the end of the increment
!     vj                 Jacobian at the end of the increment
!
!     ithermal           0: no thermal effects are taken into account
!                        1: thermal effects are taken into account (triggered
!                        by the keyword *INITIAL CONDITIONS,TYPE=TEMPERATURE)
!     t1l                temperature at the end of the increment
!     dtime              time length of the increment
!     time               step time at the end of the current increment
!     ttime              total time at the start of the current increment
!
!     icmd               not equal to 3: calculate stress and stiffness
!                        3: calculate only stress
!     ielas              0: no elastic iteration: irreversible effects
!                        are allowed
!                        1: elastic iteration, i.e. no irreversible
!                           deformation allowed
!
!     mint_              max. # of integration points per element in the
!                        model
!     nstate_            max. # of state variables in the model
!
!     xstateini(nstate_,mint_,# of elements)
!                        state variables at the start of the increment
!     xstate(nstate_,mint_,# of elements)
!                        state variables at the end of the increment
!
!     stre(6)            Piola-Kirchhoff stress of the second kind
!                        at the start of the increment
!
!     iorien             number of the local coordinate axis system
!                        in the integration point at stake (takes the value
!                        0 if no local system applies)
!     pgauss(3)          global coordinates of the integration point
!     orab(7,*)          description of all local coordinate systems.
!                        If a local coordinate system applies the global 
!                        tensors can be obtained by premultiplying the local
!                        tensors with skl(3,3). skl is  determined by calling
!                        the subroutine transformatrix: 
!                        call transformatrix(orab(1,iorien),pgauss,skl)
!
!
!     OUTPUT:
!
!     xstate(nstate_,mint_,# of elements)
!                        updated state variables at the end of the increment
!     stre(6)            Piola-Kirchhoff stress of the second kind at the
!                        end of the increment
!     stiff(21):         consistent tangent stiffness matrix in the material
!                        frame of reference at the end of the increment. In
!                        other words: the derivative of the PK2 stress with
!                        respect to the Lagrangian strain tensor. The matrix
!                        is supposed to be symmetric, only the upper half is
!                        to be given in the same order as for a fully
!                        anisotropic elastic material (*ELASTIC,TYPE=ANISO).
!                        Notice that the matrix is an integral part of the 
!                        fourth order material tensor, i.e. the Voigt notation
!                        is not used.
!     pnewdt             to be specified by the user if the material
!                        routine is unable to return the stiffness matrix
!                        and/or the stress due to divergence within the
!                        routine. pnewdt is the factor by which the time
!                        increment is to be multiplied in the next
!                        trial and should exceed zero but be less than 1.
!                        Default is -1 indicating that the user routine
!                        has converged.

The parameter ielas indicates whether irreversible effects should be taken into account. Forced displacements can lead to huge strains in the first iteration. Therefore, convergence in quasistatic calculations is often enhanced if the first iteration is completely linear, i.e. material and geometric nonlinearities are turned off. The parameter ielas is the appropriate flag.

Two extra routines are at the user's disposal for conversion purposes. ``str2mat.f'' can be used to convert Lagrangian strain into Eulerian strain, Cauchy stress into PK2 stress, or Kirchhoff stress into PK2 stress. The header and a short description are as follows:

      subroutine str2mat(str,ckl,vj,cauchy)
!
!     converts the stress in spatial coordinates into material coordinates 
!     or the strain in material coordinates into spatial coordinates. 
!
!     INPUT:
!
!     str(6):     Cauchy stress, Kirchhoff stress or Lagrange strain
!                 component order: 11,22,33,12,13,23
!     ckl(3,3):   the inverse deformation gradient
!     vj:         Jakobian determinant
!     cauchy:     logical variable
!                 if true: str contains the Cauchy stress
!                 if false: str contains the Kirchhoff stress or
!                           Lagrange strain
!
!     OUTPUT:
!
!     str(6):     Piola-Kirchhoff stress of the second kind (PK2) or
!                 Euler strain
!

The second routine, ``stiff2mat.f'' converts the tangent stiffness matrix from spatial coordinates into material coordinates.

      subroutine stiff2mat(elas,ckl,vj,cauchy)
!
!     converts an element stiffness matrix in spatial coordinates into
!     an element stiffness matrix in material coordinates. 
!
!     INPUT:
!
!     elas(21):   stiffness constants in the spatial description, i.e.
!                 the derivative of the Cauchy stress or the Kirchhoff
!                 stress with respect to the Eulerian strain
!     ckl(3,3):   inverse deformation gradient
!     vj:         Jacobian determinant
!     cauchy:     logical variable
!                 if true: elas is written in terms of Cauchy stress
!                 if false: elas is written in terms of Kirchhoff stress
!
!     OUTPUT:
!
!     elas(21):   stiffness constants in the material description,i.e.
!                 the derivative of the second Piola-Kirchhoff stress (PK2)
!                 with respect to the Lagrangian strain
!



Subsections
next up previous contents
Next: ABAQUS umat routines Up: User subroutines. Previous: Gap conductance (gapcon.f)   Contents
guido dhondt 2012-10-06