MFront version 3.0 provides two interfaces for the Abaqus/Standard and Abaqus/Explicit finite element solvers. Those interfaces are fairly features complete:

It shall be pointed out that the Abaqus/Standard and Abaqus/Explicit solvers have a long history. In particular, the design choices made for the UMAT and VUMAT interfaces were meant to allow the users to easily write finite-strain behaviours in rate-form. However, their choices differ in many points. As a consequence, those interfaces are not compatible “out of the box”: i.e. one cannot restart a simulation with Abaqus/Explicit after a computation with Abaqus/Standard without precautions.

MFront strives to provides behaviours that can be used “just-like” other UMAT and VUMAT subroutines, but there are some cases (namely finite strain orthotropic behaviours) where we were obliged to make some unusual choices that are described in this document for various reasons:


There are also cases of misuses of the generated libraries that can not be prevented by MFront. The most important ones are the following:

Current status

These interfaces have been extensively tested through MTest. Tests on Abaqus/Standard and Abaqus/Explicit shows that MFront behaviours are efficient (to the extent allowed by the UMAT and VUMAT interfaces respectively) and reliable.

How the use MFront behaviours in Abaqus/Standard and Abaqus/Explicit

When compiling mechanical behaviours with the Abaqus/Standard and/or Abaqus/Explicit interfaces, MFront generates:

The user must launch Abaqus/Standard or Abaqus/Explicit with one of the previous generic files as an external user file. Those files handles the loading of MFront shared libraries using the material name: the name of the material shall thus define the function to be called and the library in which this function is implemented.

The function name includes the modelling hypothesis, see below. An identifier can optionnaly be added to reuse the same behaviour for several material (with different material properties for instance). The identifier is discarded in the umat.cpp, vumat-sp.cpp and and vumat-dp.cpp files.

Thus, the material name in Abaqus/Standard and Abaqus/Explicit is expected to have the following form: LIBRARY_FUNCTION_HYPOTHESIS_IDENTIFIER.

The first part is the name of library, without prefix (lib) or suffix (.dll or .so depending on the system). This convention implies that the library name does not contain an underscore character.

For example, on UNIX systems, if one want to call the ELASTICITY_3D behaviour in library, the name of the material in the Abaqus/Standard input file has to be: ABAQUSBEHAVIOUR_ELASTICITY_3D.

This leads to the following declaration of the material:


It is important to note that the name of the behaviour is automatically converted to upper-case by Abaqus/Standard or Abaqus/Explicit. The name of the libraries generated by MFront are thus upper-cased. The user shall thus be aware that he/she must not rename MFront generated libraries using lower-case letters.


Note on libraries locations

As explained above, MFront libraries will be loaded at the runtime time. This means that the libraries must be found by the dynamic loader of the operating system.

Under Linux

Under Linux, the search path for dynamic libraries are specified using the LD_LIBRARY_PATH variable environment. This variable defines a colon-separated set of directories where libraries should be searched for first, before the standard set of directories.

Depending on the configuration of the system, the current directory can be considered by default.

Under Windows

Under Windows, the dynamic libraries are searched:

Compilation of the generic umat.cpp or vumat-*.cpp files

Depending on the compiler and compiler version, appropriate flags shall be added for the compilation of the generic umat.cpp or vumat-*.cpp files which are written against the C++11 standard.

The procedure depends on the version of Abaqus used. In every case, one shall modify a file called abaqus_v6.env which is delivered with Abaqus. The modified version of this file must be in the current working directory.

Versions later than Abaqus 2017

In the abaqus_v6.env, one can load a specific environment file using the importEnv function:

# Import site specific parameters such as licensing and doc parameters

This file, called custom_v6.env, is used to modify the compile_cpp entry which contains the command line used to compile C++ files. The content of this file can be copied from one of the system specific environment file delivered with Abaqus. For example, under LinuX, one can use the lnx86_64.env as a basis to build the custom_v6.env.

Here is an example of a modified custom_v6.env (we changed several paths that must be updated to match your installation):

# Installation of Abaqus CAE 2017
# Mon Jul 17 15:06:17 2017
compile_cpp = ['g++', '-O2', '-std=c++11','-c', '-fPIC', '-w', '-Wno-deprecated', '-DTYPENAME=typename',
               '-D_LINUX_SOURCE', '-DABQ_LINUX', '-DABQ_LNX86_64', '-DSMA_GNUC',
               '-DFOR_TRAIL', '-DHAS_BOOL', '-DASSERT_ENABLED',
               '-D_BSD_TYPES', '-D_BSD_SOURCE', '-D_GNU_SOURCE',
               '-DABQ_MPI_SUPPORT', '-DBIT64', '-D_LARGEFILE64_SOURCE', '-D_FILE_OFFSET_BITS=64', '%P',
               # '-O0', # <-- Optimization level
               # '-g',  # <-- Debug symbols

The last line define a set of paths where shared libraries will be searched for, which is useful if one does not want to install TFEL and MFront on in system wide path (such as /usr/) or modify the LD_LIBRARY_PATH environment variable. One can also specify a shared directory (on a NFS file system for example) to access material behaviours shared among a team of colleagues.

Versions prior to Abaqus v2017

The appropriate flags can be defined in the abaqus_v6.env file that can be overridden by the user.

For the gcc compiler, one have to add the --std=c++11 flag. The modifications to be made to the abaqus_v6.env are the following:

cppCmd  = "g++"     # <-- C++ compiler
compile_cpp = [cppCmd,
               '-c', '-fPIC', '-w', '-Wno-deprecated', '-DTYPENAME=typename',
               '-D_LINUX_SOURCE', '-DABQ_LINUX', '-DABQ_LNX86_64', '-DSMA_GNUC',
               '-DFOR_TRAIL', '-DHAS_BOOL', '-DASSERT_ENABLED',
               '-D_BSD_TYPES', '-D_BSD_SOURCE', '-D_GNU_SOURCE',
               '-DABQ_MPI_SUPPORT', '-DBIT64', '-D_LARGEFILE64_SOURCE',
               '-D_FILE_OFFSET_BITS=64', '-O2', '-std=c++11',

Generated input files

Here is an extract of the generated input file for a MFront behaviour named Plasticity for the plane strain modelling hypothesis for the Abaqus/Standard solver:

** Example for the 'PlaneStrain' modelling hypothesis
1, ElasticStrain_11
2, ElasticStrain_22
3, ElasticStrain_33
4, ElasticStrain_12
5, EquivalentPlasticStrain
** The material properties are given as if we used parameters to explicitly
** display their names. Users shall replace those declaration by
** theirs values and/or declare those parameters in the appropriate *parameters
** section of the input file
*User Material, constants=4
<YoungModulus>, <PoissonRatio>, <H>, <s0>

Main features

Supported behaviours

Isotropic and orthotropic behaviours are both supported.

For orthotropic behaviours, there are two orthotropy management policy (see the AbaqusOrthotropyManagementPolicy keyword):

For Abaqus/Standard, small and finite strain behaviours are supported. For orthotropic finite strain behaviours, one must use the MFront orthotropy management policy. The reason of this choices is given below.

For Abaqus/Explicit, only finite strain are supported. Small strain behaviours can be used using one of the finite strain strategies available.

Modelling hypotheses

The following modelling hypotheses are supported:

The generalised plane strain hypothesis is currently not supported.

The Abaqus/Standard interface

The Abaqus/Standard solver provides the UMAT interface. In this case, the behaviour shall compute:

For finite strain analyses, small strain behaviours can be written in rate form. The behaviour in integrated in the Jauman framework. This is different from Abaqus/Explicit which uses a corotational basis based on the Green-Nagdi rate.

Finite strain behaviours and orthotropy management policy

Orthotropic finite strain behaviours are only supported using the MFront orthotropy management policy. In this case, all quantities are expressed in the global configuration. Rotation in the initial material frame is handled by MFront.

Finite strain strategies

Engineers are used to write behaviours based on an additive split of strains, as usual in small strain behaviours. Different strategies exist to:

Through the @AbaqusFiniteStrainStrategy, the user can select on of various finite strain strategies supported by MFront, which are described in this paragraph.


The usage of the @AbaqusFiniteStrainStrategy keyword is mostly deprecated since MFront 3.1: see the @StrainMeasure keyword.

The Native finite strain strategy

Among them is the Native finite strain strategy which relies on build-in Abaqus/Standard facilities to integrate the behaviours written in rate form. The Native finite strain strategy will use the Jauman rate.

Those strategies have some theoretical drawbacks (hypoelasticity, etc…) and are not portable from one code to another.

Two other finite strain strategies are available in MFront for the Abaqus/Standard interface (see the @AbaqusFiniteStrainStrategy keyword):

Those two strategies use lagrangian tensors, which automatically ensures the objectivity of the behaviour.

Each of these two strategies define an energetic conjugate pair of strain or stress tensors:

The first strategy is suited for reusing behaviours that were identified under the small strain assumptions in a finite rotation context. The usage of this behaviour is still limited to the small strain assumptions.

The second strategy is particularly suited for metals, as incompressible flows are characterized by a deviatoric logarithmic strain tensor, which is the exact transposition of the property used in small strain behaviours to handle plastic incompressibility. This means that all valid consistutive equations for small strain behaviours can be automatically reused in finite strain analysis. This does not mean that a behaviour identified under the small strain assumptions can be directly used in a finite strain analysis: the identification would not be consistent.

Those two finite strain strategies are fairly portable and are available (natively or via MFront) in Cast3M, Code_Aster, Europlexus and Zebulon, etc…

Consistent tangent operator for finite strain behaviours

The “Abaqus User Subroutines Reference Guide” indicates that the tangent moduli required by Abaqus/Standard \(\underline{\underline{\mathbf{C}}}^{MJ}\) is closely related to \(\underline{\underline{\mathbf{C}}}^{\tau\,J}\), the moduli associated to the Jauman rate of the Kirchhoff stress :

\[ J\,\underline{\underline{\mathbf{C}}}^{MJ}=\underline{\underline{\mathbf{C}}}^{\tau\,J} \]

where \(J\) is the determinant of the deformation gradient \({\underset{\tilde{}}{\mathbf{F}}}\).

By definition, \(\underline{\underline{\mathbf{C}}}^{\tau\,J}\) satisfies: \[ \overset{\circ}{\underline{\tau}}^{J}=\underline{\underline{\mathbf{C}}}^{\tau\,J}\,\colon\underline{D} \] where \(\underline{D}\) is the rate of deformation.

The Abaqus/Explicit interface

Using Abaqus/Explicit, computations can be performed using single (the default) or double precision. The user thus must choose the appropriate generic file for calling MFront behaviours:

For double precision computation, the user must pass the double=both command line arguments to Abaqus/Explicit so that both the packaging steps and the resolution are performed in double precision (by default, if only the double command line argument is passed to Abaqus/Explicit, the packaging step is performed in single precision and the resolution is performed in double precision).

It is important to carefully respect those instructions: otherwise, Abaqus/Explicit will crash due to a memory corruption (segmentation error).

Here is an example of Abaqus invocation:

Abaqus user=vumat-dp.cpp double=both job=...

Finite strain strategies

As for Abaqus/Standard, user may choose one of the finite strain strategies available through MFront.

The Native finite strain strategy

The Native finite strain strategy relies on build-in Abaqus/Explicit facilities to integrate the behaviours written in rate form, i.e. it will integrate the behaviour using a corotationnal approach based on the polar decomposition of the deformation gradient.

The other finite strain strategies described for Abaqus/Standard are also available for the Abaqus/Explicit interface:


MFront behaviours can optionally compute the stored and dissipated energies through the @InternalEnergy and @DissipatedEnergy keywords.

In Abaqus/Standard, the stored energy is returned in the SSE output and the dissipated energy is returned in the SPD output.

In Abaqus/Explicit, the stored energy is returned in the enerInternNew variable and the the dissipated energy is returned in the enerInelasNew output.



“Relation between tangent operators”

Most information reported here are extracted from the book of Belytschko ([5]).

Relations between tangent operator

Relation with the moduli associated to the Truesdell rate of the Cauchy Stress \(\underline{\underline{\mathbf{C}}}^{\sigma\,T}\)

The moduli associated to the Truesdell rate of the Cauchy Stress \(\underline{\underline{\mathbf{C}}}^{\sigma\,T}\) is related to \(\underline{\underline{\mathbf{C}}}^{\tau\,J}\) by the following relationship:

\[ \underline{\underline{\mathbf{C}}}^{\tau\,J}=J\,\left(\underline{\underline{\mathbf{C}}}^{\sigma\,T}+\underline{\underline{\mathbf{C}}}^{\prime}\right)\quad\text{with}\quad\underline{\underline{\mathbf{C}}}^{\prime}\colon\underline{D}=\underline{\sigma}\,.\,\underline{D}+\underline{D}\,.\,\underline{\sigma} \]


\[ \underline{\underline{\mathbf{C}}}^{MJ}=\underline{\underline{\mathbf{C}}}^{\sigma\,T}+\underline{\underline{\mathbf{C}}}^{\prime} \]

Relation with the spatial moduli \(\underline{\underline{\mathbf{C}}}^{s}\)

The spatial moduli \(\underline{\underline{\mathbf{C}}}^{s}\) is associated to the Lie derivative of the Kirchhoff stress \(\mathcal{L}\underline{\tau}\) , which is also called the convected rate or the Oldroyd rate:

\[ \mathcal{L}\underline{\tau}=\underline{\underline{\mathbf{C}}}^{s}\,\colon\,\underline{D} \]

The spatial moduli is related to the moduli associated to Truesdell rate of the Cauchy stress \(\underline{\underline{\mathbf{C}}}^{\sigma\,T}\):

\[ \underline{\underline{\mathbf{C}}}^{\sigma\,T}=J^{-1}\,\underline{\underline{\mathbf{C}}}^{s} \]

Thus, we have: \[ \underline{\underline{\mathbf{C}}}^{MJ}= J^{-1}\underline{\underline{\mathbf{C}}}^{s}+\underline{\underline{\mathbf{C}}}^{\prime} = J^{-1}\left(\underline{\underline{\mathbf{C}}}^{s}+\underline{\underline{\mathbf{C}}}^{\prime\prime}\right)\quad\text{with}\quad\underline{\underline{\mathbf{C}}}^{\prime\prime}\colon\underline{D}=\underline{\tau}\,.\,\underline{D}+\underline{D}\,.\,\underline{\tau} \]

Relation with \(\underline{\underline{\mathbf{C}}}^{\mathrm{SE}}\)

The \(\underline{\underline{\mathbf{C}}}^{\mathrm{SE}}\) relates the rate of the second Piola-Kirchhoff stress \(\underline{S}\) and the Green-Lagrange strain rate \(\underline{\varepsilon}^{\mathrm{GL}}\):

\[ \underline{\dot{S}}=\underline{\underline{\mathbf{C}}}^{\mathrm{SE}}\,\colon\,\underline{\dot{\varepsilon}}^{\mathrm{GL}} \]

As the Lie derivative of the Kirchhoff stress \(\mathcal{L}\underline{\tau}\) is the push-forward of the second Piola-Kirchhoff stress rate \(\underline{\dot{S}}\) and the rate of deformation \(\underline{D}\) is push-forward of the Green-Lagrange strain rate \(\underline{\dot{\varepsilon}}^{\mathrm{GL}}\), \(\underline{\underline{\mathbf{C}}}^{s}\) is the push-forward of \(\underline{\underline{\mathbf{C}}}^{\mathrm{SE}}\):

\[ C^{c}_{ijkl}=F_{im}F_{jn}F_{kp}F_{lq}C^{\mathrm{SE}}_{mnpq} \]

For all variation of the deformation gradient \(\delta\,{\underset{\tilde{}}{\mathbf{F}}}\), the Jauman rate of the Kirchhoff stress satisfies: \[ \underline{\underline{\mathbf{C}}}^{\tau\,J}\,\colon\delta\underline{D}=\delta\underline{\tau}-\delta{\underset{\tilde{}}{\mathbf{W}}}.\underline{\tau}+\underline{\tau}.\delta{\underset{\tilde{}}{\mathbf{W}}} \]


Thus, the derivative of the Kirchhoff stress with respect to the deformation gradient yields: \[ \displaystyle\frac{\displaystyle \partial \underline{\tau}}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}}=\underline{\underline{\mathbf{C}}}^{\tau\,J}\,.\,\displaystyle\frac{\displaystyle \partial \underline{D}}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}}+\left(\partial^{\star}_{r}\left(\tau\right)-\partial^{\star}_{l}\left(\tau\right)\right)\,.\,\displaystyle\frac{\displaystyle \partial {\underset{\tilde{}}{\mathbf{W}}}}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}} \]

with \(\delta\,\underline{D}=\displaystyle\frac{\displaystyle \partial \underline{D}}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}}\,\colon\,\delta\,{\underset{\tilde{}}{\mathbf{F}}}\) and \(\delta\,{\underset{\tilde{}}{\mathbf{W}}}=\displaystyle\frac{\displaystyle \partial {\underset{\tilde{}}{\mathbf{W}}}}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}}\,\colon\,\delta\,{\underset{\tilde{}}{\mathbf{F}}}\)

\[ \displaystyle\frac{\displaystyle \partial \underline{\sigma}}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}}=\displaystyle\frac{\displaystyle 1}{\displaystyle J}\left(\displaystyle\frac{\displaystyle \partial \underline{\tau}}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}}-\underline{\sigma}\,\otimes\,\displaystyle\frac{\displaystyle \partial J}{\displaystyle \partial {\underset{\tilde{}}{\mathbf{F}}}}\right) \]

Numerical approximation of \(\underline{\underline{\mathbf{C}}}^{MJ}\)

Following [6], an numerical approximation of \(\underline{\underline{\mathbf{C}}}^{MJ}\) is given by: \[ \underline{\underline{\mathbf{C}}}^{MJ}_{ijkl}\approx\displaystyle\frac{\displaystyle 1}{\displaystyle J\,\varepsilon}\left(\underline{\tau}_{ij}\left({\underset{\tilde{}}{\mathbf{F}}}+{\underset{\tilde{}}{\mathbf{\delta F}}}^{kl}\right)-\underline{\tau}_{ij}\left({\underset{\tilde{}}{\mathbf{F}}}\right)\right) \]

where the perturbation \({\underset{\tilde{}}{\mathbf{\delta F}}}^{kl}\) is given by:

\[ {\underset{\tilde{}}{\mathbf{\delta F}}}^{kl}=\displaystyle\frac{\displaystyle \varepsilon}{\displaystyle 2}\left(\vec{e}_{k}\otimes\vec{e}_{l}+\vec{e}_{l}\otimes\vec{e}_{k}\right)\,.\,{\underset{\tilde{}}{\mathbf{F}}} \]

Such perturbation leads to the following rate of deformation: \[ \delta\,\underline{D}=\left({\underset{\tilde{}}{\mathbf{\delta F}}}^{kl}\right)\,{\underset{\tilde{}}{\mathbf{F}}}^{-1}=\displaystyle\frac{\displaystyle \varepsilon}{\displaystyle 2}\left(\vec{e}_{k}\otimes\vec{e}_{l}+\vec{e}_{l}\otimes\vec{e}_{k}\right) \]

The spin rate \(\delta\,\underline{W}\) associated with \({\underset{\tilde{}}{\mathbf{\delta F}}}^{kl}\) is null.

Relation with the moduli associated to the Truesdell rate of the Cauchy Stress \(\underline{\underline{\mathbf{C}}}^{\sigma\,T}\)

The moduli associated with Truesdell rate of the Cauchy Stress can be related to the moduli associated to the Green-Nagdi stress rate.

\[ \underline{\underline{\mathbf{C}}}^{\sigma\,G}=\underline{\underline{\mathbf{C}}}^{\sigma\,T}+\underline{\underline{\mathbf{C}}}^{\prime}-\underline{\sigma}\otimes\underline{I}+\underline{\underline{\mathbf{C}}}^{\mathrm{spin}} \]

where \(\underline{\underline{\mathbf{C}}}^{\mathrm{spin}}\) is given in [7]. The computation of the \(\underline{\underline{\mathbf{C}}}^{\mathrm{spin}}\) moduli is awkward and is not currently supported by MFront.

Relation with other moduli

The previous relation can be used to relate to other moduli. See the section describing the isotropic case for details.


Doghri, Issam. Mechanics of deformable solids: Linear, nonlinear, analytical, and computational aspects. Berlin; New York : Springer, 2000. ISBN 3540669604 9783540669609 3642086292 9783642086298.
EDF. R5.03.22 révision : 11536: Loi de comportement en grandes rotations et petites déformations. Référence du Code Aster. EDF-R&D/AMA, 2013. Available from:
EDF. R5.03.22 révision : 11536: Loi de comportement en grandes rotations et petites déformations. Référence du Code Aster. EDF-R&D/AMA, 2013. Available from:
Miehe, C., Apel, N. and Lambrecht, M. Anisotropic additive plasticity in the logarithmic strain space: Modular kinematic formulation and implementation based on incremental minimization principles for standard materials. Computer Methods in Applied Mechanics and Engineering. November 2002. Vol. 191, no. 47–48, p. 5383–5425. DOI 10.1016/S0045-7825(02)00438-3. Available from:
Belytschko, Ted. Nonlinear Finite Elements for Continua and Structures. Chichester ; New York : Wiley-Blackwell, 2000. ISBN 9780471987741.
Sun, Wei, Chaikof, Elliot L and Levenston, Marc E. Numerical approximation of tangent moduli for finite element implementations of nonlinear hyperelastic material models. Journal of biomechanical engineering. December 2008. Vol. 130, no. 6, p. 061003–061003. DOI 10.1115/1.2979872. Available from:
Simo, Juan C and Hughes, Thomas J. R. Computational inelasticity. New York : Springer, 1998. ISBN 0387975209 9780387975207.