HOMTOOLS

Heterogeneous Materials

Homtools — 2015-03-17T10:33:33Z

Homtools can be used to estimate the average mechanical response of a heterogeneous material by the way of Finite Element Analysis on a Representative Volume Element (RVE). It allows to compute the relationship between the average stress and the average strain, according to three different methods of localization: kinematic uniform boundary conditions (KUBC), periodic boundary conditions (PBC) and static uniform boundary conditions (SUBC). For all these methods, the average loading can be either the average stress or the average strain (or an independent combination of average strains and stresses components). The constitutive materials of the RVE can be either linear or non-linear and the analysis can be in small or finite-strain. The presence of interaction properties (such as contact and friction) is naturally taken into account.

Localisation boundary conditions

The following figures illustrate a simple 2D test case of a stiff elastic cylindrical filler in a soft elastic matrix, treated with the three available methods in Homtools: KUBC (Kinematic Uniform Boundary Conditions), PBC (Periodic Boundary Conditions), SUBC (Static Uniform Boundary Conditions).

These methods require specific boundary conditions.

KUBC (click for a description)

This method consists in applying on the boundary the displacement field that would occur if the strain were uniform inside the RVE.

In small strains, the boundary conditions are :

\cdot \vec{OM} " title="\quad \vec{u} = < \bf{\varepsilon(\vec{u})}> \cdot \vec{OM} " />

in which :

is the displacement field,
is the strain field,
is the position vector of the point on the boundary.
" title="< \bullet >" /> is the averaging operator over the RVE: = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " title=" < \bullet > = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " />
is the inner product.

In finite strains, the boundary conditions are :

-\bf{Id}\right) \cdot \vec{OM} " title="\quad \vec{u} = \left(< \bf{f}>-\bf{Id}\right) \cdot \vec{OM} " />

in which :

is the deformation gradient,
is the identity tensor.
is the position vector of the point on the boundary in the reference configuration.
" title="< \bullet >" /> is the averaging operator over the RVE in the reference configuration: = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " title=" < \bullet > = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " />
is the inner product.

There is no restriction concerning the use of this method, except that no rigid part must intersect the boundary (holes are permitted).

SUBC (click for a description)

This method consists in applying on the boundary the stress vector field that would occur if the stress were uniform inside the RVE.

In small strains, the boundary conditions are :

\cdot \vec{n} " title="\quad \bf{\sigma} \bf{\cdot} \vec{n}} = <\bf{\sigma}> \cdot \vec{n} " />

in which :

is the cauchy stress tensor,
is the outwarding normal. " title=" < \bullet >" /> is the averaging operator over the RVE: = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " title="< \bullet > = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " />
is the inner product.

In finite strains, the boundary conditions are :

\cdot \vec{n} " title="\quad \bf{\pi} \bf{\cdot} \vec{n}} = <\bf{\pi}> \cdot \vec{n} " />

in which :

is the Piolla Kirchoff II stress tensor,
is the outwarding normal in the reference configuration. " title="< \bullet >" /> is the averaging operator over the RVE in the reference configuration: = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " title=" < \bullet > = \frac{1}{\mbox{Vol}(V)} \displaystyle \int_V \; \bullet \; \mbox{d}V " />
is the inner product.

There is no restriction concerning the use of this method, except that no holes must intersect the boundary (rigid parts are permitted but a specific treatment is required).

PBC (click for a description)

The method is theoretically relevant for periodic media, which can be defined by a periodicity cell and the associated periodicity vector of translation. The periodic homogenisation process consists in assuming that the strains and stresses are periodic at the level of the periodicity cell (which is defined as the RVE). The periodicity of stresses and strains leads to specific periodic boundary conditions for the localisation problem on the RVE.

In small strains, the boundary conditions are :

\cdot \vec{OM} " title="\vect{u} - < \bf{\varepsilon(\vec{u})}> \cdot \vec{OM} " /> periodic and antiperiodic.

A quantity is said to be "periodic" (resp. "antiperiodic") when it takes the same value (resp. opposite value) at two opposite points on the boundary (one of them being the image of the other by translation of a periodicity vector).

In finite strains, the boundary conditions are :

-\bf{Id}\right) \cdot \vec{OM} " title="\vect{u} - \left(< \bf{f}>-\bf{Id}\right) \cdot \vec{OM} " /> periodic and antiperiodic. A quantity is in this case said to be "periodic" (resp. "antiperiodic") when it takes the same value (resp. opposite value) at two opposite points on the boundary (one of them being the image of the other by translation of a periodicity vector in the initial configuration).

There is no restriction concerning the use of this method (periodic holes and rigid parts intersecting the boundary are permitted but a specific treatment is required for the rigid parts).

The difficulty of applying these methods resides in the creation of the corresponding non classical boundary conditions, that can be written as linear constraints between the displacements at each point on the boundary of the RVE and the average strains.

In Homtools, we use Reference Points to prescribe the average loading and these constraints.

Reference Points to apply the average loading and the specific boundary conditions

The average strains are introduced as degrees of freedom of Reference Points and Homtools automatically generates the linear constraints (*equation) between these additionnal degrees of freedom and the displacements on the boundary of the RVE. Thanks to duality properties, the reaction forces at the Reference Points are the average stresses multiplied by the volume of the RVE. With this method, prescribing average strains or stresses becomes as easy as prescribing displacements or concentrated forces at a node. Furthermore, obtaining the relationship between the average strain and the average stress does not require any specific post-treatment.

For fiinte strain problems, the degrees of freedom of the Reference Points are the components of the average deformation gradient tensor and the reaction forces are the components of the avrage Piola-Kirchoff II stress tensor.

How to use Homtools

The main steps are :
mesh the RVE
in the "Interaction" module, create the Reference Points (2 for 2D problems in plane stress or strain or 3D problems in small strains, 3 for 3D problems in finite strains)
in the "Interaction" module, choose "Homtools" in the drop off menu "Plug-in" and answer the questions.

in the "Load" module, prescribe the average strains components or/and the stresses components by prescribing the degrees of freedom (dsplacements) or the nodal forces at the reference points.
after solving the problem, in the "Vizualisation" module, you can obtain the effective response of the RVE by the postreatment of the displacements and yhe nodal forces at the Reference Points.

Check the following video to see the steps required to define a complete homogenization problem (in french).

Remarks

for the method SUBC, no hole should intersect the boundary of the RVE (inconsistency of the method in this case). Furthermore, the displacement field is not unique for this method (rigid translations and rotations are not fixed)
the method PBC is theoretically only relevant for periodic materials. The linear constraints couple the displacements at nodes on opposite faces of the boundary. The mesh of opposite faces must be identical: at each node of a face must correspond a node on the opposite face defined by translation of a periodicity vector. In Homtools, you must define the couple of faces together with a periodicity vectors : the mesh of the second set must result from the translation of the mesh of the first set according to the periodicity vector. You must repeat the operation as many times as necessary for all the couple of faces. Fot this method, the displacement field is not unique: the rigid translation is not fixed by the periodicity conditions and you can make the solution unique by fixing the dispalcements at a node in the RVE.

Homtools Support

Homtools — 2015-03-02T09:04:05Z

Homtools is a research product which is provided as is. Therefore documention and help are very succinct. Nevertheless, we will try to regroup frequently asked questions on this page. If you need specifc support or if you want a specific development to be done in homtools do not hesitate to contact us. - Support

About Homtools

Homtools — 2015-02-16T21:25:59Z

Homtools is developed and maintened since 2010 at the Laboratory of Mechanic and Acoustic (CNRS UPR7051). Initially this set of tools was designed to simplify the full field homogenization process of nonlinear composite materials. Since 2010, Homtools is slowly growing...

The devel team is actually composed by its creators:

Stéphane Lejeunes is a CNRS Research Engineer. He works on the modeling and the simulation of Rubber materials and structures. He is also a numerician and software developer for nonlinear and multiphysics problems.
Stéphane Bourgeois is an Associate Professor at Ecole Centrale Marseille. He works on the modeling of rod and tapespring structures and on the numerical homogeneisation of structures and materials

If you want to participate to this project or to share your experiences with Homtools do not hesitate to contact us!

Download

Homtools — 2015-02-06T15:32:22Z

Homtools is a opensource project that is avaible with the terms of CecillC licence. Homtools is a research software that is provided as is. No responsibility can be imputed to the authors in any usage of this software. If you use Homtools for producing research results, we should be grateful if you add this reference to your paper/communication:

“Une Toolbox Abaqus pour le calcul de propriétés effectives de milieux hétérogènes Lejeunes Stéphane, Bourgeois Stéphane 2011, 10th National Conference on Computational methods for Structures, Giens, France ”

Installing Homtools is very simple:

Unpack the archive (zip file) in a directory
Modify or create the abaqus_v6.env file in your home directory with the following line: plugin_central_dir = "/path/to/homtools/dir"

Homtools 0.9 ( 238 kb)

Tutorial ( 1.2 Mb)

Post-computations

Homtools — 2015-01-26T13:54:10Z

Post-computation are often needed to determine specific macro quantities. Homtools furnish scripts that operate on ODB files.

Compute spatial average of a nodal field

Computing average quantity for fields which are in the output database of an Abaqus Job (ODB) can be done with a simple command line. Homtools furnish a script that compute an average value of a nodal field for a given set of elements. The nodal field is simply interpolated at Gauss Points and integrated over elements.

Users just have to edit the file Field_Average.py and to modify the following lines with appropriate values:

odbname='Job.odb'
fieldname='U'
elsetname=' ALL ELEMENTS'
stepname='Step-1'
framenumber=-1

RVE generation

Homtools — 2015-01-26T13:17:48Z

Homtools provides scripts to randomly generate simple micro-structures. In the current version 2D voronoi cells and 2D spherical inclusions are available.

Randomly generate RVE

You want to study the influence of micro-structural parameters on the macroscopic response of your RVE? Homtools provides two examples of random generation of simple geometry of RVE (voronoi cells and spherical inclusions). Starting from these examples you can developed your own RVE generator. Feel free to share our experiences with us: we will add your development to the sources.

RVE generation is avaible in the part module of Abaqus CAE: Plug-ins->Homtools

Here is the GUI interface for 2D random spherical inclusions

Heterogeneous Structures

Homtools — 2015-01-26T13:15:53Z

Homtools can be used to estimate the average mechanical response of heterogeneous periodic beams or plates by the way of Finite Element Analysis on the 3D periodicity cell. It allows to compute the relationship between the average generalized stresses (normal stress, bending moments, twisting moment...) and the average generalized strains (normal strain, bending curvatures...). It can be used for example to estimate the effective inertia of the equivalent homogeneous beam in the linear elasticity framework. Nevertheless, the constitutive materials of the periodicity cell can be non-linear and the presence of interaction properties is naturally taken into account. Homtools can thus help to build a non-linear effective beam or plate model and identify its parameters.

Heterogeneous Periodic Beams

This functionnality is relevant for heterogeneous beams that are periodic in the direction of their axis. In that case, a periodicity cell can be defined, together with a periodicity vector which is parallel to the beam axis. The kinematics of the effective beam model is the one of Navier-Euler-Bernoulli (no transverse shearing). Four effective generalized strains are considered : the normal strain, the two bending strains and the twisting strain. The associated effective generalized stresses are the normal stress, the bending moments and the twisting moment. Homtools allows to prescribe an average loading in terms of these effective strains or stresses (or any independent combination of them) on the 3D periodicity cell. It requires non-classical boundary conditions that can be written as linear constraints between the displacements at each point on the boundary of the periodicity cell and the average strains.

click here for details

This method consists in applying periodicity conditions on the two opposite cross-sections of the periodicity cell . A local orthonormal coordinates system must be defined, such that the axis is the beam reference axis. The normal strain characterize the effective elongation along . The bending strains and are the effective curvature around the axis and and is the twisting strain around. The effective stresses (normal stress , bending moment and , and twisting moment ) are defined as:

" title=" N=< \sigma_{zz}> " />
" title=" M_1=< y \, \sigma_{zz}> " />
" title=" M_2=< -x \, \sigma_{zz}> " />
" title=" M_t=< x \, \sigma_{yz}-y \, \sigma_{xz}> " />

in which = \frac{1}{l} \displaystyle \int_V \; \bullet \; \mbox{d}V " title=" < \bullet > = \frac{1}{l} \displaystyle \int_V \; \bullet \; \mbox{d}V " /> with the length of the periodicity cell (norm of the periodicity vector).

The periodic homogenisation process consists in assuming that the strain field is the sum of a pure Euler-Bernoulli-Navier strain field and of a periodic fluctuation strain field that takes into account the heterogenities. It leads to the following boundary conditions:

periodic and antiperiodic,

in which:

is the displacement that leads to a pure Euler-Bernoulli-Navier strain field ( are the coordinates of a current point) :

a quantity is said to be "periodic" (resp. "antiperiodic") when it takes the same value (resp. opposite value) at two opposite points on the boundary (one of them being the image of the other by translation of a periodicity vector).

Homtools uses Reference Points to prescribe the average loading and these constraints.

Heterogeneous Periodic Plates

Under construction

Macro nodes and Reference axis or plane

As in the case of material homogeneisation, reference nodes needs to be added to the model. The degree of freedom of these nodes are associated to the generalized strains. Linear relation (*equation) will automatically be generated by Homtools between the reference nodes and all the mesh nodes that are selected by the users as boundary nodes. However, users also need to define an axis (for beam) or a plane (for plates) which will be used as the neutral axis or plane to define the effective generalzed strains and stresses.

Here is a sample of the GUI for beam:

What is homtools?

Homtools — 2015-01-26T12:59:02Z

What is Homtools?

Homtools is a set of python scripts for Abaqus that greatly simplify the determination of homogenized characteristics of heterogeneous materials and structures.

Homtools has been developed to simplify and to automatize the tasks which are required to perform an homogeneization problem on a Representative Volume Element of material or structure. Several full field approaches are available. The toolbox integrates some GUIs that permit to easily define the appropriate specific boundary conditions and the average loadings in the CAE.

What kind of problems can be solved with Homtools?