Table of contents


Break down into modules

The FinEtools package consists of many modules which fall into several categories. The top-level module, FinEtools, includes all other modules and exports functions to constitute the public interface. The user is free to generate their own public interface, however. More details are provided in the section Make up your own public interface.

  • Top-level: FinEtools is the top-level module. For interactive use it is enough to do using FinEtools, however in some cases functions from modules need to be brought into the scope individually (most importantly, the algorithm modules). This is the ONLY module that EXPORTS functions, none of the other modules exports a single function. The entire public (i. e. exported) interface of the FinEtools package is specified in the file FinEtools.jl (i. e. in the FinEtools module). The user is free to specify his or her own set of exported functions from the FinEtools package to create an ad hoc public interface.

  • Utilities: Refer to the modules FTypesModule (definition of basic numerical types), PhysicalUnitModule (for use with numbers specified using physical units), AssemblyModule (assembly of elementwise matrices and vectors), CSysModule (coordinate system module), MatrixUtilityModule (utilities for operations on elementwise matrices), BoxModule (support for working with bounding boxes), ForceIntensityModule (force-intensity module), RotationUtilModule (support for spatial rotations).

  • Mesh entities: FENodeSetModule, FESetModule (node set and finite element set types).

  • Mesh Generation: MeshLineModule, MeshQuadrilateralModule, MeshTriangleModule, MeshTetrahedronModule, MeshHexahedronModule, VoxelBoxModule.

  • Mesh manipulation: MeshSelectionModule (searching of nodes and elements), MeshModificationModule (mesh boundary, merging of meshes and nodes, smoothing, partitioning), MeshUtilModule (utilities), FENodeToFEMapModule (search structure from nodes to elements).

  • Mesh import/export: MeshImportModule, MeshExportModule.

  • Fields: FieldModule, GeneralFieldModule, ElementalFieldModule, NodalFieldModule (modules for representing quantities on the mesh).

  • Integration: Support for integration over solids, surfaces, curves, and points: IntegRuleModule, IntegDomainModule. The package defines some common bilinear and linear forms to aid in constructing weighted residual methods.

  • General algorithms: AlgoBaseModule (algorithms), FEMMBaseModule (FEM machine for general tasks).

Arithmetic types

The FinEtools package tries to make typing arguments easier. The arithmetic types used throughout are FInt for integer data, FFlt for floating-point data, and Complex{FFlt} for applications that work with complex linear algebra quantities.

The module FTypesModule defines these types, and also defines abbreviations for vectors and matrices with entries of these types.

Some algorithms expect input in the form of a data dictionary, FDataDict, and also produce output in this form.

Physical units

The PhysicalUnitModule provides a simple function, phun, which can help with providing input numbers with the correct conversion between physical units. For instance, it is possible to specify the input data as

E = 200*phun("GPa");# Young's modulus
nu = 0.3;# Poisson ratio
rho = 8000*phun("KG*M^-3");# mass density
L = 10.0*phun("M"); # side of the square plate
t = 0.05*phun("M"); # thickness of the square plate

A few common sets of units are included, :US, :IMPERIAL, :CGS, :SIMM (millimeter-based SI units), and :SI (meter-based SI units). The resulting values assigned to the variables are floating-point numbers, for instance

julia> E = 200*phun("GPa")

Numbers output by the simulation can also be converted to appropriate units for printing as

julia> E/phun("MPa")

It is also possible to use a macro to define physical units:

E = 200*u"GPa";# Young's modulus
nu = 0.3;# Poisson ratio
rho = 8000*u"KG*M^-3";# mass density
L = 10.0*u"M"; # side of the square plate
t = 0.05*u"M"; # thickness of the square plate
t / u"mm"

Mesh entities

The mesh consists of one set of finite element nodes and one or more sets of finite elements.

One of the organizing principles of the finite element collection is that finite elements can appear as representations of the interior of the domain, but in a different model as parts of the boundary. Thus for instance 4-node quadrilaterals are finite elements that represent cross-sections of axially symmetric models or surfaces of membranes, but they are also the boundaries of hexahedral models.

A mesh is generated by one of the functions specialized to a particular finite element type. Thus there are mesh generation functions for lines, triangles, quadrilaterals, tetrahedra, and hexahedra.

Mesh generation

As an example, the following code generates a hexahedral mesh of simple rectangular block.

fens, fes  = H8block(h, l, 2.0 * pi, nh, nl, nc)

The finite element node set and the finite element set are returned. More complicated meshes can be constructed from such mesh parts. There are functions for merging nodes and even multiple meshes together.

The code snippet below constructs the mesh of an L-shaped domain from the meshes of three rectangles.

W = 100. # width of the leg
L = 200. # length of the leg
nL = 15 # number of elements along the length of the leg
nW = 10 # number of elements along the width
tolerance = W / nW / 1.0e5 # tolerance for merging nodes
Meshes = Array{Tuple{FENodeSet,FESet},1}()
push!(Meshes, Q4quadrilateral([0.0 0.0; W W], nW, nW))
push!(Meshes, Q4quadrilateral([-L 0.0; 0.0 W], nL, nW))
push!(Meshes, Q4quadrilateral([0.0 -L; W 0.0], nW, nL))
fens, outputfes = mergenmeshes(Meshes, tolerance);
fes = cat(outputfes[1], cat(outputfes[2], outputfes[3]))

As an example of the merging of nodes to create the final mesh, consider the creation of a closed hollow tube.

fens, fes  = H8block(h, l, 2.0 * pi, nh, nl, nc) # generate a block
# Shape into a cylinder
R = zeros(3, 3)
for i = 1:count(fens)
    x, y, z =[i,:];
    rotmat3!(R, [0, z, 0])
    Q = [cos(psi * pi / 180) sin(psi * pi / 180) 0;
        -sin(psi * pi / 180) cos(psi * pi / 180) 0;
        0 0 1][i,:] = reshape([x + Rmed - h / 2, y - l / 2, 0], 1, 3) * Q * R;
# Merge the nodes where the tube  closes up
candidates = selectnode(fens, box = boundingbox([Rmed - h -Inf 0.0; Rmed + h +Inf 0.0]), inflate = tolerance)
fens, fes = mergenodes(fens, fes,  tolerance, candidates);

The final mesh used for a simulation consists of a single node set and one or more finite element sets. The finite elements may be divided into separate sets to accommodate different material properties, different orientations of the material coordinate systems, or different formulations of the discrete model. The assignment of the finite elements to sets may be based on geometrical proximity, topological connections, or some other characteristic. See the "mesh selection" discussion for details.

Structured mesh generation

The simplest possible meshes can be generated in the form of one-dimensional, two-dimensional, and three-dimensional blocks. The spacing of the nodes can be either uniform (for instance Q8block), or the spacing can be given with an arbitrary distribution (for instance Q4blockx). Meshes of tetrahedra can be generated in various orientations of the "diagonals".

More complex meshes can be generated for certain element types: for instance an annulus (Q4annulus), quarter of a plate with a hole (Q4elliphole), quarter of a sphere (H8spheren), layered plate (H8layeredplatex).

Hexahedral meshes can also be created by extrusion of quadrilateral meshes (H8extrudeQ4).


Simple meshes such as blocks can be deformed into geometrically complex shapes, for instance by tapering or other relocation of the nodes. For instance, we can generate a block and then bend it into one quarter of an annulus as

fens,fes = Q4block(rex-rin,pi/2,5,20);
for i=1:count(fens)[i,1];[i,2];[i,:]=[r*cos(a) r*sin(a)];


Multiple mesh regions can be generated and then merged together into a single mesh. Refer to the MeshModificationModule. Meshes can be also mirrored.

Boundary extraction

Mesh composed of any element type can be passed to the function meshboundary, and the boundary of the mesh is extracted. As an example, the code

fens,fes = Q4block(rex-rin,pi/2,5,20);
bdryfes = meshboundary(fes);

generates a mesh of quadrilaterals in the set fes, and bdryfes = meshboundary(fes) finds the boundary elements of the type L2 (line elements with two nodes) and stores them in the finite element set bdryfes.

Conversion between element types

For any element shape (line, triangle, quadrilateral, hexahedron, tetrahedron) there is the linear version and the quadratic version. Conversion routines are provided so that, for example, mesh can be generated as eight-node hexahedra and then converted to twenty-node hexahedra as

fens, fes = H8toH20(fens, fes)

Other conversion routines can convert triangles to quadrilaterals, tetrahedra to hexahedra, and so on.


Meshes composed of some element types can be uniformly refined. For instance, quadrilateral meshes can be refined by bisection with Q4refine.

Selection of mesh entities

There are many instances of problem definitions where it is important to partition meshes into subsets. As an example, consider a tube consisting of inner ABS core and outer fiber-reinforced laminate layer. The mesh may consist of hexahedra. This mesh would then need to be partitioned into two subsets, because the materials and the material orientation data are different between the two regions.

As another example, consider a simple beam of rectangular cross-section, clamped at one end, and loaded with shear tractions at the free end. The entire boundary of the beam needs to be separated into three subsets: the first subset, for the traction-free boundary, is ignored. The second subset, for the clamped cross-section, is extracted and its nodes are used to formulate the essential boundary condition. The third subset is extracted and used to define an FEM machine to compute the load vector due to the shear traction.

There are several ways in which mesh entities (nodes and finite elements) can be selected. The simplest uses element labels: some mesh-generation routines label the generated elements. For example,

fens,fes = H8layeredplatex(xs, ys, ts, nts)

generates a plate-like mesh where the layers are labeled. It is therefore possible to select the bottom-most layer as

rls = selectelem(fens, fes, label = 1)

where rls is a list of integer indexes into the set fes, so that we can extract a subset corresponding to this layer as

botskin = subset(fes, rls)

Geometrical techniques for selecting finite elements or nodes can be based on

  • the location within or overlap with boxes;
  • distance from a given point;
  • distance from a given plane;
  • connectedness (selection by flooding).

Additionally, surface-like finite elements (quadrilaterals and triangles embedded in three dimensions), or lines embedded in two dimensions, can be selected based upon the orientation of their normal (facing criterion).

As an example, consider a straight duct with anechoic termination. A triangle mesh is generated as

fens,fes  =  T3block(Lx,Ly,n,2);

and its boundary is extracted as

bfes  =  meshboundary(fes)

The finite elements from the piece of the boundary on the left parallel to the Y axis can be extracted as

L0 = selectelem(fens,bfes,facing = true, direction = [-1.0 0.0])

where the numbers of the finite elements whose normals point in the general direction of the vector [-1.0 0.0] are returned in the integer array L0.


The structure to maintain the numbering and values of the degrees of freedom in the mesh is the field. Consider for instance the temperature field: we write

\[T(x) = \sum_i N_i(x) T_i\]

The understanding is that $T_i$ are the degrees of freedom, and the basis functions $N_i(x)$ are defined implicitly by the finite element mesh. (More about basis functions below.) Each element has its own set of functions, which when multiplied by the degree of freedom values describe the temperature over each individual finite element. The basis functions are implicitly associated with the nodes of the finite elements. The degrees of freedom are also (explicitly) associated with the nodes. The field may also be generalized a bit by extending the above sum simply to entities of the mesh, not only the nodes, but perhaps also the elements.

The role of the field is then to maintain the correspondence between the entities and the numbers and values of the degrees of freedom.

Abstract Field

The assumption is that a field has one set of degrees of freedom per node or per element. For simplicity we will refer to the nodes and elements as entities. It assumes that concrete subtypes of the abstract field have the following data, one row per entity:

  • values::FMat{T}: Array of the values of the degrees of freedom, one row for each entity. All the arrays below have the same dimensions as this one.
  • dofnums::FIntMat: Array of the numbers of the free degrees of freedom. First the free degrees of freedom are numbered, then the fixed (prescribed) degrees of freedom.
  • is_fixed::Matrix{Bool}: Array of Boolean flags, true for fixed (prescribed) degrees of freedom, false otherwise.
  • fixed_values::FMat{T}: Array of the same size and type as values. Its entries are only relevant for the fixed (prescribed) degrees of freedom.
  • nalldofs::FInt: the total number of all degrees of freedom.
  • nfreedofs::FInt: the total number of free degrees of freedom.

The methods defined for the abstract field include:

  • Return the number of degrees of freedom and the number of entities.

  • Gather and scatter the system vector.

  • Gather elementwise vectors or matrices of values, the degree of freedom numbers, or the fixed values of the degrees of freedom.

  • Set or clear essential boundary conditions.

  • Copy a field. Clear the entries of the field.

Nodal Field

In this case the abstract field is subtyped to a concrete field where the entities are nodes.

Elemental Field

In this case the abstract field is subtyped to a concrete field where the entities are the elements.

General Field

In this case the abstract field is subtyped to a concrete field where the entities are use-case specific.

Numbering of the degrees of freedom

The simplest method is at the moment implemented: number all free degrees of freedom, row-by-row and column-by-column, starting from 1 up to nfreedofs(f), for the field f. Then number the prescribed degrees of freedom are numbered, up to nalldofs(f).

There is also a method to supply the numbering of the nodes, perhaps resulting from the Reverse Cuthill-McKee permutation. This may be useful when using LU or LDLT factorization as the fill-in may be minimized.

Finite element

The finite element set is one of the basic entities in FinEtools. It is a homogeneous collection of finite elements defined by the connectivity (collection of node numbers, listing the nodes connected by the element in a specific order). The finite element set provides specialized methods to compute the values of basis functions and the values of the gradients of the basis functions with respect to the parametric coordinates.

Element types

The finite element sets are instances of concrete types. Each particular shape and order of element has its own type. There are types for linear and quadratic quadrilaterals, for instance, FESetQ4 and FESetQ8. Each element set provides access to the number of nodes connected by the element (nodesperelem), the connectivity as the two dimensional array conn, and the integer label vector label.

The concrete finite element set types are subtypes of the abstract type for elements of different manifold dimension (3, 2, 1, and 0), for instance for the quadrilaterals that would be AbstractFESet2Manifold. These types are in turn subtypes of the abstract finite element set type AbstractFESet.

The concrete finite element set type provides specialized methods to compute the values of the basis functions, bfun, and methods to compute the gradients of the basis functions with respect to the parametric coordinates, bfundpar. FinEtools at the moment supports only the so-called nodal basis functions: each basis function is associated with a node. And that is true both globally (in the sense that each basis function is globally supported), and locally over each finite element, and all such functions are 1 at its own node, and zero at all the other nodes.

Finite element set functions

  • Methods defined for the abstract type:

    • nodesperelem: Get the number of nodes connected by the finite element.
    • count: Get the number of individual connectivities in the FE set.
    • setlabel!: Set the label of the entire finite elements set.
    • connasarray: Retrieve connectivity as an integer array.
    • fromarray!: Set connectivity from an integer array.
    • subset: Extract a subset of the finite elements from the given finite element set.
    • cat: Concatenate the connectivities of two FE sets.
    • updateconn!: Update the connectivity after the IDs of nodes changed.
    • map2parametric: Map a spatial location to parametric coordinates.
  • Methods dispatched based on the manifold type:

    • manifdim: Return the manifold dimension.
    • Jacobian: Evaluate the Jacobian.
    • gradN!: Compute the gradient of the basis functions with the respect to the "reduced" spatial coordinates.
  • Methods dispatched on the concrete type:

    • boundaryconn: Get boundary connectivity.
    • boundaryfe: Return the constructor of the type of the boundary finite element.
    • bfun: Compute the values of the basis functions at a given parametric coordinate.
    • bfundpar: Compute the values of the basis function gradients at a given parametric coordinate.
    • inparametric: Are given parametric coordinates inside the element parametric domain?
    • centroidparametric: Return the parametric coordinates of the centroid of the element.


There are two kinds of integrals in the weighted-residual finite element method: integrals over the interior of the domain, and integrals over the boundary of the domain.

Consequently, in a typical simulation one would need two meshes: one for the interior of the domain, and one for the boundary. Obviously, the mesh for the boundary will be derived from the mesh constructed for the interior.

Often only a part of the entire boundary is used: on some parts of the boundary the boundary condition is implied as homogeneous (i. e. zero). For instance, a traction-free boundary. Therefore the necessary integrals are typically evaluated over a subset of the entire boundary.

Manifold dimension

Finite elements have a certain manifold dimension. Tetrahedra and hexahedra are three-manifolds, triangles and quadrilaterals are two-manifolds, triangles and quadrilaterals are two-manifolds, lines are one-manifolds, and points are zero-manifolds.

Elements are equipped with an "other" dimension attribute which boosts the manifold dimension to produce the required dimension for the integration. For instance, a line element can be equipped with an "other" dimension to represent a cross-section so that a volume integral can be evaluated over a line element. Or, a line element can be given an "other" dimension as a thickness to result in a physical dimension needed to evaluate a surface integral.

The "other" dimension has the following meaning for finite elements of different manifold dimensions:

Manifold dimensionVolume integralSurface integral

Integration over the interior

The integrals are always volume integrals. This means that for elements which are of lower manifold dimension than three the "other" dimension needs to compensate.

For three-manifold finite elements (tetrahedra and hexahedra) the "other" dimension is always 1.0. This really means there is no "other" dimension to a volume-like element.

For finite elements of manifold dimension less than tthree, the "other" dimension varies according to the model (axially symmetric versus simple plane 2D) as shown in the table below.

Manifold dimensionAxially symmetricPlane 2D
2$2\pi r$Thickness
1$2\pi r\times$ ThicknessCross-section
0$2\pi r\times$ Cross-sectionVolume

The integral is approximated with numerical quadrature as

\[\int_{\Omega} f dV \approx \sum_q f(\xi_q) J(\xi_q) W_q\]

Here $f$ is the integrand, $f(\xi_q)$ is the value of the integrand at the quadrature point, $J(\xi_q)$ is the value of the Jacobian at the quadrature point. Importantly, the Jacobian incorporates the "other" dimension, and therefore it is the volume Jacobian. (For the interior integrals the Jacobian is computed by the Jacobianvolume method.)

Integration over the boundary

The integrals are always surface integrals. This means that for elements which are of lower manifold dimension than two the "other" dimension needs to compensate.

For two-manifold finite elements (triangles and quadrilaterals) the "other" dimension is always 1.0. This really means there is no "other" dimension to a surface-like element.

For finite elements of manifold dimension less than two, the "other" dimension varies according to the model (axially symmetric versus simple plane 2D) as shown in the table below.

Manifold dimensionAxially symmetricPlane 2D
1$2\pi r$Thickness
0$2\pi r\times$ ThicknessCross-section

The integral is approximated with numerical quadrature as

\[\int_{\partial \Omega} f dS \approx \sum_q f(\xi_q) J(\xi_q) W_q \]

Here $f$ is the integrand, $f(\xi_q)$ is the value of the integrand at the quadrature point, $J(\xi_q)$ is the value of the Jacobian at the quadrature point. Importantly, the Jacobian incorporates the "other" dimension, and therefore it is the surface Jacobian. (For the boundary integrals the Jacobian is computed by the Jacobiansurface method.)

Example: axially symmetric model, line element L2

The surface Jacobian in this case is equal to the curve Jacobian times 2*pi*r.

Integration Domain

As explained above, integrating over the interior or the boundary may mean different things based on the features of the solution domain: axially symmetric?, plane strain or plane stress?, and so forth.

The module IntegDomainModule supports the processing of the geometry necessary for the evaluation of the various integrals. The module data structure groups together a finite element set with an appropriate integration rule, information about the model (axially symmetric or not), and a callback to evaluate the "other" dimension.

Other dimension

The discussion of the surface and volume integrals introduces the notion of the "other" dimension. In order to evaluate Jacobians of various space dimensions the Geometry Data module takes into account whether or not the model is axially symmetric, and evaluates the "other" dimension based upon this information.

A finite element set is equipped with a way of calculating the "other" dimension. For instance, the line element with two nodes, L2, can be given the "other" dimension as a "thickness" so that surface integrals can be evaluated over the line element. However, if this line element is used in an axially symmetric model, the same "other" dimension of "thickness" will result in the integral along the length of this line element being a volume integral.

Thus, the way in which the "other" dimension gets used by the integration domain methods depends on the model. As an example, consider the method

function Jacobianvolume(self::IntegDomain{T}, J::FFltMat, loc::FFltMat, conn::CC, N::FFltMat)::FFlt where {T<:AbstractFESet2Manifold, CC<:AbstractArray{FInt}}
    Jac = Jacobiansurface(self, J, loc, conn, N)::FFlt
    if self.axisymmetric
        return Jac*2*pi*loc[1];
        return Jac*self.otherdimension(loc, conn,  N)

which evaluates the volume Jacobian for an element of manifold dimension 2 (surface). Note that first the surface Jacobian is calculated, which is then boosted to a volume Jacobian in two different ways, depending on whether the model is axially symmetric or not. For the axially symmetric case the "other" dimension is implied,

The callback function computes the "other" dimension from two kinds of information: (a) the physical location of the quadrature point, and (b) the interpolation data for the element (connectivity and the values of the basis functions at the quadrature point).

  • The approach ad (a) is suitable when the "other" dimension is given as a function of the physical coordinates. The simplest case is obviously a uniform distribution of the "other" dimension. When no callback is explicitly provided, the "other" dimension callback is automatically generated as the trivial
function otherdimensionunity(loc::FFltMat, conn::CC, N::FFltMat)::FFlt where {CC<:AbstractArray{FInt}}
    return 1.0

which simply returns 1.0 as the default value.

  • The approach ad (b) is appropriate when the "other" dimension is given by values given at the nodes of the mesh. Than the connectivity and the array of the values of the basis functions can be used to interpolate the "other" dimension to the quadrature point.

Evaluation of integration data

Importantly, the Integration Domain (IntegDomain) method integrationdata evaluates quantities needed for numerical integration: locations and weights of quadrature points, and the values of basis functions and of the basis function gradients with respect to the parametric coordinates at the quadrature points.

FEM machines

The construction of the matrices and vectors of the discrete form of the weighted residual equation is performed in FEM machines. (FEM = Finite Element Method.)

As an example consider the weighted-residual form of the heat balance equation

\[\int_{V} \vartheta c_V\frac{\partial T}{\partial t} \; \mathrm{d} V +\int_{V}(\mathrm{grad}\vartheta)\; \kappa (\mathrm{grad}T )^T\; \mathrm{d} V -\int_{V} \vartheta Q \; \mathrm{d} V +\int_{S_2} \vartheta\;\overline{q}_{n}\; \mathrm{d} S+ \int_{S_3} \vartheta\;h (T-T_a) \; \mathrm{d} S = 0\]

where $\vartheta(x) =0$ for $x \in{S_1}$ .

The test function is taken to be one finite element basis function at a time, $\vartheta = N_{j}$, and the trial function is

\[T = \sum_{i= 1} ^{N} N_{i} T_i .\]

Here by $N_{j}$ we mean the basis function constructed on the mesh and associated with the node where the degree of freedom $j$ is situated.

Now the test function and the trial function is substituted into the weighted residual equation.

Example: internal heat generation rate term

For instance, for the term

\[\int_{V} \vartheta Q \; \mathrm{d} V\]

we obtain

\[\int_{V} N_{j} Q \; \mathrm{d} V\]

This integral evaluates to a number, the heat load applied to the degree of freedom $j$. When these numbers are evaluated for all the free degrees of freedom, they constitute the entries of the global heat load vector.

Evaluating integrals of this form is so common that there is a module FEMMBaseModule with the method distribloads that computes and assembles the global vector. For instance to evaluate this heat load vector on the mesh composed of three-node triangles, for a uniform heat generation rate Q, we can write

fi = ForceIntensity(FFlt[Q]);
F1 = distribloads(FEMMBase(IntegDomain(fes, TriRule(1))), geom, tempr, fi, 3);

IntegDomain(fes, TriRule(1)) constructs integration domain for the finite elements fes using a triangular integration rule with a single point. FEMMBase is the base FEM machine, and all it needs at this point is the integration domain. The method distribloads is defined for the base FEM machine, the geometry field geom, the numbering of the degrees of freedom is taken from the field tempr, the internal heat generation rate is defined as the force intensity fi, and the integrals are volume integrals (3).

Example: conductivity term

The conductivity term from the weighted residual equation

\[\int_{V}(\mathrm{grad}\vartheta)\; \kappa (\mathrm{grad}T )^T\; \mathrm{d} V\]

is rewritten with the test and trial functions as

\[\sum_{i=1}^N \int_{V}(\mathrm{grad}N_{j})\; \kappa (\mathrm{grad}N_{i} )^T\; \mathrm{d} V \; T_i\]

The sum over the degree of freedom number $i$ should be split: some of the coefficients $T_i$ are for free degrees of freedom ($1 \le i \le N_{\mathrm{f}}$, with $N_{\mathrm{f}}$ being the total number of free degrees of freedom), while some are fixed (prescribed) for nodes which are located on the essential boundary condition surface $S_1$ ($N_{\mathrm{f}} < i \le N$).

Thus the term splits into two pieces,

\[\sum_{i=1}^{N_{\mathrm{f}}} \int_{V}(\mathrm{grad}N_{j})\; \kappa (\mathrm{grad}N_{i} )^T\; \mathrm{d} V \; T_i\]

where the individual integrals are entries of the conductivity matrix, and

\[\sum_{i=N_{\mathrm{f}}+1}^N \int_{V}(\mathrm{grad}N_{j})\; \kappa (\mathrm{grad}N_{i} )^T\; \mathrm{d} V \; T_i\]

which will represent heat loads due to nonzero prescribed boundary condition.

The FEM machine for the heat conduction problem can be created as

material = MatHeatDiff(thermal_conductivity)
femm = FEMMHeatDiff(IntegDomain(fes, TriRule(1)), material)

where we first create a material to provide access to the thermal conductivity matrix $\kappa$, and then we create the FEM machine from the integration domain for a mesh consisting of three node triangles, using one-point integration rule, and the material. This FEM machine can then be passed to a method, for instance the calculate the global conductivity matrix K

K = conductivity(femm, geom, Temp)

where the geometry comes from the geometry field geom, and the temperature field Temp provides the numbering of the degrees of freedom. Note that the global conductivity matrix is square, and of size $N_{\mathrm{f}}\timesN_{\mathrm{f}}$. In other words, it is only for the degrees of freedom that are free (actual unknowns).

The heat load term due to the nonzero essential boundary conditions is evaluated with the method nzebcloadsconductivity

F2 = nzebcloadsconductivity(femm, geom, Temp);

where the geometry comes from the geometry field geom, and the temperature field Temp provides the numbering of the degrees of freedom and the values of the prescribed (fixed) degrees of freedom. The result is a contribution to the global heat load vector.

Base FEM machine

The following operations are provided by the base FEM machine:

  • Integrate a function expressed in terms of a field. This is typically used to evaluate RMS discretization errors.

  • Integrate a function of the position. Perhaps the evaluation of the moments of inertia, or the calculation of the volume.

  • Transfer field between meshes of different resolutions.

  • Calculate the distributed-load system vector.

  • Construct a field from integration-point quantities. This is typically used in the postprocessing phase, for instance to construct continuous distribution of stresses in the structure.

Material and Material Orientation

The material response is described in material-point-attached coordinate system. These coordinate systems are Cartesian, and the material coordinate system is typically chosen to make the response particularly simple. So for orthotropic or transversely isotropic materials the axes would be aligned with the axes of orthotropy.

The type CSys (module CSysModule) is the updater of the material coordinate system matrix. The object is equipped with a callback to store the current orientation matrix. For instance: the coordinate system for an orthotropic material wound around a cylinder could be described in the coordinate system CSys(3, 3, updatecs!), where the callback updatecs! is defined as

function updatecs!(csmatout::FFltMat, XYZ::FFltMat, tangents::FFltMat, fe_label::FInt)
    csmatout[:, 2] = [0.0 0.0 1.0]
    csmatout[:, 3] = XYZ
    csmatout[3, 3] = 0.0
    csmatout[:, 3] = csmatout[:, 3]/norm(csmatout[:, 3])
    csmatout[:, 1] = cross(csmatout[:, 2], csmatout[:, 3])


Solution procedures and other common operations on FEM models are expressed in algorithms. Anything that algorithms can do, the user of FinEtools can do manually, but to use an algorithm is convenient.

Algorithms typically (not always) accept a single argument, modeldata, a dictionary of data, keyed by Strings. Algorithms also return modeldata, typically including additional key/value pairs that represent the data computed by the algorithm.

Base algorithms

These are not specific to the particular physics at hand. Examples of algorithms are Richardson extrapolation, calculation of the norm of the field, or calculation of the norm of the difference of two fields. These algorithms are the exceptions, they do not return modeldata but rather return directly computed values.

Model data

Model data is a dictionary, with string keys, and arbitrary values. The documentation string for each method of an algorithm lists the required input. For instance, for the method linearstatics of the AlgoDeforLinearModule, the modeldata dictionary needs to provide key-value pairs for the finite element node set, and the regions, the boundary conditions, and so on.

The modeldata may be also supplemented with additional key-value pairs inside an algorithm and returned for further processing by other algorithms.

Queries of quadrature-point data

A number of quantities exist at integration (quadrature) points. For instance for heat conduction this data may refer to the temperature gradients and heat flux vectors. In stress analysis, such data would typically be stress invariants or stress components.

How this data is calculated at the quadrature point obviously varies depending on the element type. Not only on the element order, but the element formulation may invoke rules other than those of simple gradient-taking: take as an example mean-strain elements, which define strains by using averaging rules over the entire element, so not looking at a single integration point only.

For this purpose, FinEtools has ways of defining implementations of the function inspectintegpoints to take into account the particular features of the various finite element formulations. Each FEMM typically defines its own specialized method.


One way in which quadrature-point data is postprocessed into graphical means is by constructing node-based fields. For instance, extrapolating quadrature-point data to the nodes is commonly done in finite element programs. This procedure is typically referred to as "averaging at the nodes". The name implies that not only the quadrature-point data is extrapolated to the nodes of the element, but since each element incident on a node may have predicted (extrapolated) a different value of a quantity (for example stress), these different values need to be somehow reconciled, and averaging, perhaps weighted averaging, is the usual procedure.

Compute continuous stress fields

Individual FEMMs may have different ways of extrapolating to the nodes. These are implemented in various methods of the function fieldfromintegpoints. The resulting field represents quadrature-point data as a nodal field, where the degrees of freedom are extrapolated values to the nodes.

Compute elementwise stress fields

Most finite element postprocessing softwares find it difficult to present results which are discontinuous at inter-element boundaries. Usually the only way in which data based on individual elements with no continuity across element boundaries is presented is by taking an average over the entire element and represent the values as uniform across each element. Various methods of the function elemfieldfromintegpoints produce elemental fields of this nature.



At the moment importing is mostly limited to the mesh data (properties, boundary conditions, analysis of data, etc. are typically not imported). The following formats of finite element input files can be handled:

  • NASTRAN (.nas files).
  • Abaqus (.inp files).


  • VTK (.vtk so-called legacy files). Export of geometry and fields (nodal and elemental) is supported.
  • Abaqus (.inp files). Mesh data and selected property, boundary condition, and procedure commands can be handled.
  • NASTRAN (.nas files). Very basic mesh and select other attributes are handled.
  • STL file export of surface data.
  • H2Lib triangular-surface export (.tri files).
  • CSV file export of numerical data is supported.

Tutorials and Examples


The FinEtools tutorials are written up in the repositories for the applications, heat diffusion, linear and nonlinear deformation and so on.

The tutorials are in the form of Julia files with markdown. These are converted to markdown files using the Literate workflow.


The examples of the use of the FinEtools package are separated in their own separate repositories, for instance FinEtoolsHeatDiff, FinEtoolsAcoustics, and so on. For a complete information refer to the list of the repositories.

The examples are in the form of Julia files with multiple functions, where each function defines one or more related examples. Take for instance the example file Fahy_examples.jl. This incantation will run all the examples from the example file:

include("Fahy_examples.jl"); Fahy_examples.allrun()

This will run just a single example from this file:

include("Fahy_examples.jl"); Fahy_examples.fahy_H8_example()

The example file Fahy_examples.jl consists of a module (whose name matches the name of the file), and the module defines multiple functions, one for each example, and one to run all examples, allrun.


Check out the numerous tests in the test folder. There are hundreds of tests which exercise the various functions of the library. These examples may help you understand how to extract the desired outcome.

Make up your own public interface

Here we assume that the FinEtools package is installed. We also assume the user works in his or her own folder, which for simplicity we assume is a package folder in the same tree as the package folder for FinEtools.

The user may have his or her additions to the FinEtools library, for instance a new material implementation, or a new FEMM (finite element model machine). Additionally, the user writes some code to solve particular problems.

In order to facilitate interactive work at the command line(REPL), it is convenient to have one or two modules so that using them allows for the user's code to resolve function names from the FinEtools package and from the user's own code.

Here are two ways in which this can be accomplished.

  1. The user exports his or her own additions from the module add2FinEtools (the name of this module is not obligatory, it can be anything). In addition, the public interface to the FinEtools package needs to be brought in separately.

    using FinEtools using add2FinEtools

  2. The user may change entirely the public interface to the FinEtools package by selectively including parts of the FinEtools.jl file and the code to export his or her own functionality in a single module, let us say myFinEtools (this name is arbitrary), so that when the user invokes

    using myFinEtools

    all the functionality that the USER considers to be public is made available by exports.

Method 1 has the advantage that the interface definition of the FinEtools package itself does not change, which means that package code does not need to be touched. It also has a disadvantage that the interface to FinEtools does not change which means that if there is a conflict with one of the exported functions from FinEtools, it needs to be resolved by fiddling with other packages.

Method 2 has the advantage that when there is a conflict between one of the exported FinEtools functions and some other function, be it from another package or the user's own, the conflict can be resolved by changing the public interface to FinEtools by the USER (as opposed to by the DEVELOPER). Also, in this method the USER has the power to define the public interface to the FinEtools package, and if the user decides that nothing should be exported for implicit resolution of functions, that is easily accomplished.

These two methods have been described by examples in the FinEtoolsUseCase package. Refer to the Readme file and to the method descriptions in the method 1 and 2 folders.