In the vast majority of simulations involving linear elastic materials, we are dealing with an isotropic material that does not have any directional sensitivity. To describe such a material, only two independent material parameters are required. There are many possible ways to select these parameters, but some of them are more popular than others.

Young’s modulus, shear modulus, and Poisson’s ratio are the parameters most commonly found in tables of material data. They are not independent, since the shear modulus, G, can be computed from Young’s modulus, E, and Poisson’s ratio, \nu, as

G = \frac{E}{2(1+\nu)}

Young’s modulus can be directly measured in a uniaxial tensile test, while the shear modulus can be measured in, for example, a pure torsion test.

In the uniaxial test, Poisson’s ratio determines how much the material will shrink (or possibly expand) in the transverse direction. The allowable range is -1 <\nu< 0.5, where positive values indicate that the material shrinks in the thickness direction while being pulled. There are a few materials, called *Auxetics*, which have a negative Poisson’s ratio. A cork in a wine bottle has a Poisson’s ratio close to zero, so that its diameter is insensitive to whether it is pulled or pushed.

For many metals and alloys, \nu \approx1/3, and the shear modulus is then about 40% of Young’s modulus.

Given the possible values of \nu, the possible ratios between the shear modulus and Young’s modulus are

\frac{1}{3} < \frac{G}{E} < \infty

When \nu approaches 0.5, the material becomes incompressible. Such materials pose specific problems in an analysis, as we will discuss.

The bulk modulus, K, measures the change in volume for a given uniform pressure. Expressed in E and \nu, it can be written as:

K = \frac{E}{3(1-2\nu)}

When \nu= 1/3, the value of the bulk modulus equals the value of Young’s modulus, but for an incompressible material (\nu \to0.5), K tends to infinity.

The bulk modulus is usually specified together with the shear modulus. These two quantities are, in a sense, the most physically independent choices of parameters. The volume change is only controlled by the bulk modulus and the distortion is only controlled by the shear modulus.

The Lamé constants \mu and \lambda are mostly seen in more mathematical treatises of elasticity. The full 3D constitutive relation between the stress tensor \boldsymbol \sigma and the strain tensor \boldsymbol \varepsilon can be conveniently written in terms of the Lamé constants:

\boldsymbol \sigma=2\mu \boldsymbol \varepsilon +\lambda \; \mathrm{trace}(\boldsymbol{\varepsilon}) \mathbf I

The constant \mu is simply the shear modulus, while \lambda can be written as

\lambda = \frac{E \nu}{(1+\nu)(1-2\nu)}

A full table of conversions between the various elastic parameters can be found here.

Some materials, like rubber, are almost incompressible. Mathematically, a fully incompressible material differs fundamentally from a compressible material. Since there is no volume change, it is not possible to determine the mean stress from it. The state equation for the mean stress (pressure), *p*, as function of volume change, \Delta V, as

p = f(\Delta V)

will no longer exist, and must instead be replaced by a constraint stating that

\Delta V = 0

Another way of looking at incompressibility is to note that the term (1-2\nu) appears in the denominator of the constitutive equations, so that a division by zero would occur if \nu= 0.5. Is it then a good idea to model an incompressible material approximately by setting \nu= 0.499?

It can be done, but in this case, a standard displacement based finite element formulation may give undesirable results. This is caused by a phenomenon called *locking*. Effects include:

- Overly stiff models.
- Checkerboard stress patterns.
- Errors or warnings from the equation solver because of ill-conditioning.

The remedy is to use a *mixed formulatio*n where the pressure is introduced as an extra degree of freedom. In COMSOL Multiphysics, you enable the mixed formulation by selecting the *Nearly incompressible material* checkbox in the settings for the material model.

*Part of the settings for a linear elastic material with mixed formulation enabled.*

When Poisson’s ratio is larger than about 0.45, or equivalently, the bulk modulus is more than one order of magnitude larger than the shear modulus, it is advisable to use a mixed formulation. An example of the effect is shown in the figure below.

*Stress distribution in a simple plane strain model, \nu = 0.499. The top image shows a standard displacement based formulation, while the bottom image shows a mixed formulation.*

In the solution with only displacement degrees of freedom, the stress pattern shows distortions at the left end where there is a constraint. These distortions are almost completely removed by using a mixed formulation.

In general cases of linear elastic materials, the material properties have a directional sensitivity. The most general case is called anisotropic, which means all six stress components can depend on all six strain components. This requires 21 material parameters. Clearly, it is a demanding task to obtain all of this data. If the stress, \boldsymbol \sigma, and strain, \boldsymbol \varepsilon, are treated as vectors, they are related by the constitutive 6-by-6 symmetric matrix \mathbf D through

\boldsymbol \sigma= \mathbf D \boldsymbol \varepsilon

Fortunately, it is common that nonisotropic materials exhibit certain symmetries. In an orthotropic material, there are three orthogonal directions in which the shear action is decoupled from the axial action. That is, when the material is stretched along one of these principal directions, it will only contract in the two orthogonal directions, but not be sheared. A full description of an orthotropic material requires nine independent material parameters.

The constitutive relation of an orthotropic material is easier when written on compliance form, \boldsymbol \varepsilon= \mathbf C \boldsymbol \sigma:

\mathsf{C} =

\begin{bmatrix}

\tfrac{1}{E_{\rm X}} & -\tfrac{\nu_{\rm YX}}{E_{\rm Y}} & -\tfrac{\nu_{\rm ZX}}{E_{\rm Z}} & 0 & 0 & 0 \\

-\tfrac{\nu_{\rm XY}}{E_{\rm X}} & \tfrac{1}{E_{\rm Y}} & -\tfrac{\nu_{\rm ZY}}{E_{\rm Z}} & 0 & 0 & 0 \\

-\tfrac{\nu_{\rm XZ}}{E_{\rm X}} & -\tfrac{\nu_{\rm YZ}}{E_{\rm Y}} & \tfrac{1}{E_{\rm Z}} & 0 & 0 & 0 \\

0 & 0 & 0 & \tfrac{1}{G_{\rm YZ}} & 0 & 0 \\

0 & 0 & 0 & 0 & \tfrac{1}{G_{\rm ZX}} & 0 \\

0 & 0 & 0 & 0 & 0 & \tfrac{1}{G_{\rm XY}} \\

\end{bmatrix}

\begin{bmatrix}

\tfrac{1}{E_{\rm X}} & -\tfrac{\nu_{\rm YX}}{E_{\rm Y}} & -\tfrac{\nu_{\rm ZX}}{E_{\rm Z}} & 0 & 0 & 0 \\

-\tfrac{\nu_{\rm XY}}{E_{\rm X}} & \tfrac{1}{E_{\rm Y}} & -\tfrac{\nu_{\rm ZY}}{E_{\rm Z}} & 0 & 0 & 0 \\

-\tfrac{\nu_{\rm XZ}}{E_{\rm X}} & -\tfrac{\nu_{\rm YZ}}{E_{\rm Y}} & \tfrac{1}{E_{\rm Z}} & 0 & 0 & 0 \\

0 & 0 & 0 & \tfrac{1}{G_{\rm YZ}} & 0 & 0 \\

0 & 0 & 0 & 0 & \tfrac{1}{G_{\rm ZX}} & 0 \\

0 & 0 & 0 & 0 & 0 & \tfrac{1}{G_{\rm XY}} \\

\end{bmatrix}

Since the compliance matrix must be symmetric, the twelve constants used are reduced to nine through three symmetry relations of the type

\tfrac{\nu_{\rm YX}}{E_Y} = \tfrac{\nu_{\rm YX }}{E_X}

Note that \nu_{\rm YX} \neq \nu_{\rm XY}, so when dealing with orthotropic data, it is important to make sure that the intended Poisson’s ratio values are used. The notation may not be the same in all sources.

Anisotropy and orthotropy commonly occur in inhomogeneous materials. Often, the properties are not measured, but computed using a homogenization process upscaling from microscopic to macroscopic scale. A discussion about such homogenization — in quite another context – can be found in this blog post.

For nonisotropic materials, there are limitations to the possible values of the material parameters similar to those described for isotropic materials. It is difficult to immediately see these limitations, but there are two things to look out for:

- The constitutive matrix \mathbf D must be positive definite.
- For a general anisotropic material, the only option is to check if all of its eigenvalues are positive.
- For an orthotropic material, this is true if all six elastic moduli are positive and \nu_{\rm XY}\nu_{\rm YX}+\nu_{\rm YZ}\nu_{\rm ZY}+\nu_{\rm ZX}\nu_{\rm XZ}+\nu_{\rm YX}\nu_{\rm ZY}\nu_{\rm XZ}<1

- If the material has low compressibility, a mixed formulation must be used.
- It is possible to make an estimate of an effective bulk modulus and the values of the shear moduli.
- In cases of uncertainty, it is better to take the extra cost of the mixed formulation to avoid possible inaccuracies.

When working with geometrically nonlinear problems, the meaning of “linear elasticity” is really a matter of convention. The issue here is that there are several possible representations of stresses and strains. For a discussion about different stress and strain measures, see this previous blog post.

Since the primary stress and strain quantities in COMSOL Multiphysics are Second Piola-Kirchhoff stress and Green-Lagrange strain, the natural interpretation of linear elasticity is that these quantities are linearly related to each other. Such a material is sometimes called a St. Venant material.

Intuitively, one could expect that “linear elasticity” means that there is a linear relation between force and displacement in a simple tensile test. This will not be the case, since both stresses and strains depend on the deformation. To see this, consider a bar with a square cross section.

*The bar subjected to uniform extension.*

The original length of the bar is L_0 and the original cross-section area is A_0=a_0^2, where a_0 is the original edge of the cross section. Assume that the bar is extended at a distance \Delta so that the current length is L=L_0+\Delta=L_0(1+\xi).

Here, 1+\xi is the axial stretch and \xi can be interpreted as the engineering strain. The new length of the edge of the cross section is a=a_0+d=a_0(1+\eta), where \eta is the engineering strain in the transverse directions.

The force can be expressed as the Cauchy stress \sigma_x in the axial direction multiplied by the current cross-section area:

F = \sigma_x A = \sigma_x A_0 (1+\eta)^2

To use the linear elastic relation, the Cauchy stress \boldsymbol \sigma must be expressed as the Second Piola-Kirchoff stress \mathbf S. The transformation rule is

\mathbf \sigma = J^{-1} \mathbf F \mathbf S \mathbf F^T

where \mathbf F is the deformation gradient tensor, and the volume scale is defined as J = det(\mathbf F). Without going into details, for a uniaxial case

\sigma_x = \frac{F_{xX}}{F_{yY}F_{zZ}}S_X= \frac{(1+\xi)}{(1+\eta)^2}S_X

Since for a St. Venant material in uniaxial extension, the axial stress is related to the axial strain as S_X = E \epsilon_X, we obtain

F = S_x A_0 (1+\xi) = E A_0 (1+\xi)\varepsilon_X

Given that the axial term of the Green-Lagrange strain tensor is defined as

\varepsilon_X = \frac{\partial u}{\partial X} + \frac{1}{2}(\frac{\partial u}{\partial X})^2 = \xi+\frac{1}{2}\xi^2

the force versus displacement relation is then

F = E A_0 (1+\xi)(\xi + \frac{1}{2}\xi^2)=E A_0 (\xi+\frac{3}{2}\xi^2+\frac{1}{2}\xi^3)

The linear elastic material furbished with geometric nonlinearity actually implies a cubic relation between force and engineering strain (or force versus displacement, since \Delta =L_0\xi), as shown in the figure below.

*The uniaxial response of a linear elastic material under geometric nonlinearity.
*

As can be seen in the graph, the stiffness of the material approaches zero at the compression side, \xi = \sqrt{{1}/{3}}-1 \approx -0.42. In practice, this means that the simulation will fail at that strain level. It can be argued that there are no real materials that are linear at large strains, so this should not cause problems in practice. However, linear elastic materials are often used far outside the range of reasonable stresses for several reasons, such as:

- Often, you may want to do a quick “order of magnitude” check before introducing more sophisticated material models.
- There are singularities in the model that cause very high strains in a point.
- Read more about singularities here.

- In contact problems, the study is always geometrically nonlinear.
- Often, high compressive strains appear locally in the contact zone at some time during the analysis.

In all of these cases, the solver may fail to find a solution if the compressive strains are large. If you suspect this to be the case, it is a good idea to plot the smallest principal strain. If it is smaller than -0.3 or so, we can expect this kind of breakdown. The critical value in terms of the Green-Lagrange strain is found to be -1/3. When this becomes a problem, you should consider changing to a suitable hyperelastic material model.

Compression may not be the only problem. In the analysis above, Poisson’s ratio did not enter the equations. So what happens with the cross section?

By definition in the uniaxial case, the transverse strain is related to the axial strain by

\varepsilon_Y = -\nu \varepsilon_X

When these strains are Green-Lagrange strains, this is a nonlinear relation stating that

\frac{\partial v}{\partial Y} + \frac{1}{2}(\frac{\partial v}{\partial Y})^2 = -\nu (\frac{\partial u}{\partial X} + \frac{1}{2}(\frac{\partial u}{\partial X})^2)

Thus, there is a strong nonlinearity in the change of the cross section. Solving this quadratic equation gives the following relation between the engineering strains

\eta = \sqrt{1-\nu(\xi^2+2\xi)}-1

The result is shown in the figure below.

*Transverse displacement as a function of the axial displacement for uniaxial tension of a St. Venant material. Five different values of Poisson’s ratio are shown.*

As you can see, the cross section collapses quickly at large extensions for higher values of Poisson’s ratio.

If another choice of stress and strain representation had been made — for example, if the Cauchy stress were proportional to the logarithmic, or “true” strain — it would have resulted in quite a different response. Instead, such a material has a stiffness that decreases with elongation, where the force-displacement response does depend on the value of Poisson’s ratio. Still, both materials can correctly be called “linear elastic”, although the results computed with large strain elasticity can differ widely between two different simulation platforms.

We have illustrated some limits for the use of linear elastic materials. In particular, the possible pitfalls related to incompressibility and to the combination of linear elasticity with large strains have been highlighted.

If you are interested in reading more about material modeling in structural mechanics problems, check out these blog posts:

- Introducing Nonlinear Elastic Materials
- Obtaining Material Data for Structural Mechanics from Measurements
- Part 2: Obtaining Material Data for Structural Mechanics from Measurements
- Fitting Measured Data to Different Hyperelastic Material Models
- Yield Surfaces and Plastic Flow Rules in Geomechanics
- Computing Stiffness of Linear Elastic Structures: Part 1
- Computing Stiffness of Linear Elastic Structures: Part 2

After obtaining our measured data, the question then becomes this: How can we estimate the material parameters required for defining the hyperelastic material models based on the measured data? One of the ways to do this in COMSOL Multiphysics is to fit a parameterized analytic function to the measured data using the Optimization Module.

In the section below, we will define analytical expressions for stress-strain relationships for two common tests — the *uniaxial test* and the *equibiaxial test*. These analytical expressions will then be fitted to the measured data to obtain material parameters.

Characterizing the volumetric deformation of hyperelastic materials to estimate material parameters can be a rather intricate process. Oftentimes, perfect incompressibility is assumed in order to estimate the parameters. This means that after estimating material parameters from curve fitting, you would have to use a reasonable value for bulk modulus of the nearly incompressible hyperelastic material, as this property is not calculated.

Here, we will fit the measured data to several perfectly incompressible hyperelastic material models. We will start by reviewing some of the basic concepts of the nearly incompressible formulation and then characterize the stress measures for the case of perfect incompressibility.

For nearly incompressible hyperelasticity, the total strain energy density is presented as

W_s = W_{iso}+W_{vol}

where W_{iso} is the isochoric strain energy density and W_{vol} is the volumetric strain energy density. The second Piola-Kirchhoff stress tensor is then given by

S = -p_pJC^{-1}+2\frac{\partial W_{iso}}{\partial C}

where p_{p} is the volumetric stress, J is the volume ratio, and C is the right Cauchy-Green tensor.

You can expand the second term from the above equation so that the second Piola-Kirchhoff stress tensor can be equivalently expressed as

S = -p_pJC^{-1}+2\left(J^{-2/3}\left(\frac{\partial W_{iso}}{\partial \bar{I_{1}}}+\bar{I_{1}} \frac{\partial W_{iso}}{\partial \bar{I_{2}}} \right)I-J^{-4/3} \frac{\partial W_{iso}}{\partial \bar{I}_{2}} C -\left(\frac{\bar{I_{1}}}{3}\frac{\partial W_{iso}}{\partial \bar{I}_{1}} + \frac{2 \bar{I}_{2}}{3}\frac{\partial W_{iso}}{\partial \bar{I}_{2}}\right)C^{-1}\right)

where \bar{I}_{1} and \bar{I}_{2} are invariants of the isochoric right Cauchy-Green tensor \bar{C} = J^{-2/3}C.

The first Piola-Kirchhoff stress tensor, P, and the Cauchy stress tensor, \sigma, can be expressed as a function of the second Piola-Kirchhoff stress tensor as

\begin{align}P& = FS\\

\sigma& = J^{-1}FSF^{T}

\end{align}

\sigma& = J^{-1}FSF^{T}

\end{align}

Here, F is the deformation gradient.

Note: You can read more about the description of different stress measures in our previous blog entry “Why All These Stresses and Strains?“

The strain energy density and stresses are often expressed in terms of the stretch ratio \lambda. The *stretch ratio* is a measure of the magnitude of deformation. In a uniaxial tension experiment, the stretch ratio is defined as \lambda = L/L_0, where L is the deformed length of the specimen and L_0 is its original length. In a multiaxial stress state, you can calculate principal stretches \lambda_a\;(a = 1,2,3) in the principal referential directions \hat{\mathbf{N}_a}, which are the same as the directions of the principal stresses. The stress tensor components can be rewritten in the spectral form as

S =\sideset{}{^3_{a=1}}

\sum S_{a} \hat{\mathbf{N}_{a}} \otimes \hat{\mathbf{N}_{a}}

\sum S_{a} \hat{\mathbf{N}_{a}} \otimes \hat{\mathbf{N}_{a}}

where S_{a} represents the principal values of the second Piola-Kirchhoff stress tensor and \hat{\mathbf{N}_{a}} represents the principal referential directions. You can represent the right Cauchy-Green tensor in its spectral form as

C = \sideset{}{^3_{a=1}}

\sum\lambda_a^2 \hat{\mathbf{N}_a}\otimes\hat{\mathbf{N}_a}

\sum\lambda_a^2 \hat{\mathbf{N}_a}\otimes\hat{\mathbf{N}_a}

where \lambda_a indicates the values of the principal stretches. This allows you to express the principal values of the second Piola-Kirchhoff stress tensor as a function of the principal stretches

S_a = \frac{-p_p J}{\lambda_a^2}+2\left(J^{-2/3}\left(\frac{\partial W_{iso}}{\partial \bar{I_{1}}}+\bar{I_{1}} \frac{\partial W_{iso}}{\partial \bar{I_{2}}} \right) -J^{-4/3} \frac{\partial W_{iso}}{\partial \bar{I}_{2}} \lambda_a^2 -\frac{1}{\lambda_a^2}\left(\frac{\bar{I_{1}}}{3}\frac{\partial W_{iso}}{\partial \bar{I}_{1}} + \frac{2 \bar{I}_{2}}{3}\frac{\partial W_{iso}}{\partial \bar{I}_{2}}\right)\right)

Now, let’s consider the uniaxial and biaxial tension tests explained in the initial blog post in our Structural Materials series. For both of these tests, we can derive a general relationship between stress and stretch.

Under the assumption of incompressibility (J=1), the principal stretches for the uniaxial deformation of an isotropic hyperelastic material are given by

\lambda_1 = \lambda, \lambda_2 = \lambda_3 = \lambda^{-1/2}

The deformation gradient is given by

\begin{array}{c} F = \\ \end{array} \left(\begin{array}{ccc} \lambda &0 &0 \\ 0 &\frac{1}{\sqrt{\lambda}} &0 \\ 0 &0 &\frac{1}{\sqrt{\lambda}}\end{array}\right)

For uniaxial extension S_2 = S_3 = 0, the volumetric stress p_{p} can be eliminated to give

S_{1} = 2\left(\frac{1}{\lambda} -\frac{1}{\lambda^4}\right) \left(\lambda \frac{\partial W_{iso}}{\partial \bar{I}_{1_{uni}}}+\frac{\partial W_{iso}}{\partial \bar{I}_{2_{uni}}}\right) ,\; P_1 = \lambda S_1\; \sigma_1 = \lambda^2 S_1,\;\;\;\;

The isochoric invariants \bar{I}_{1_{uni}} and \bar{I}_{2_{uni}} can be expressed in terms of the principal stretch \lambda as

\begin{align*}

\bar{I}_{1_{uni}} = \left(\lambda^2+\frac{2}{\lambda}\right) \\

\bar{I}_{2_{uni}} = \left(2\lambda + \frac{1}{\lambda^2}\right)

\end{align*}

\bar{I}_{1_{uni}} = \left(\lambda^2+\frac{2}{\lambda}\right) \\

\bar{I}_{2_{uni}} = \left(2\lambda + \frac{1}{\lambda^2}\right)

\end{align*}

Under the assumption of incompressibility, the principal stretches for the equibiaxial deformation of an isotropic hyperelastic material are given by

\lambda_1 = \lambda_2 = \lambda, \; \lambda_3 = \lambda^{-2}

For equibiaxial extension S_3 = 0, the volumetric stress p_{p} can be eliminated to give

S_1 = S_2 = 2\left(1-\frac{1}{\lambda^6}\right)\left(\frac{\partial W_{iso}}{\partial \bar{I}_{1_{bi}}}+\lambda^2\frac{\partial W_{iso}}{\partial \bar{I}_{2_{bi}}}\right),\; P_1 = \lambda S_1,\; \sigma_1 = \lambda^2 S_1\;\;\;\;

The invariants \bar{I}_{1_{bi}} and \bar{I}_{2_{bi}} are then given by

\begin{align*}

\bar{I}_{1_{bi}} = \left( 2\lambda^2 + \frac{1}{\lambda^4}\right) \\

\bar{I}_{2_{bi}} = \left(\lambda^4 + \frac{2}{\lambda^2}\right)

\end{align*}

\bar{I}_{1_{bi}} = \left( 2\lambda^2 + \frac{1}{\lambda^4}\right) \\

\bar{I}_{2_{bi}} = \left(\lambda^4 + \frac{2}{\lambda^2}\right)

\end{align*}

Let’s now look at the stress versus stretch relationships for a few of the the most common hyperelastic material models. We will consider the first Piola-Kirchhoff stress for the purpose of curve fitting.

The total strain energy density for a Neo-Hookean material model is given by

W_s = \frac{1}{2}\mu\left(\bar{I}_1-3\right)+\frac{1}{2}\kappa\left(J_{el}-1\right)^2

where J_{el} is the elastic volume ratio and \mu is a material parameter that we need to compute via curve fitting. Under the assumption of perfect incompressibility and using equations (1) and (2), the first Piola-Kirchhoff stress expressions for the cases of uniaxial and equibiaxial deformation are given by

\begin{align*}

P_{1_{uniaxial}} &= \mu\left(\lambda-\lambda^{-2}\right)\\

P_{1_{biaxial}} &= \mu\left(\lambda-\lambda^{-5}\right)

\end{align*}

P_{1_{uniaxial}} &= \mu\left(\lambda-\lambda^{-2}\right)\\

P_{1_{biaxial}} &= \mu\left(\lambda-\lambda^{-5}\right)

\end{align*}

The stress versus stretch relationship for a few of the other hyperelastic material models are listed below. These can be easily derived through the use of equations (1) and (2), which relate stress and the strain energy density.

\begin{align*}

P_{1_{uniaxial}} &= 2\left(1-\lambda^{-3}\right)\left(\lambda C_{10}+C_{01}\right)\\

P_{1_{biaxial}} &= 2\left(\lambda-\lambda^{-5}\right)\left(C_{10}+\lambda^2 C_{01}\right)

\end{align*}

P_{1_{uniaxial}} &= 2\left(1-\lambda^{-3}\right)\left(\lambda C_{10}+C_{01}\right)\\

P_{1_{biaxial}} &= 2\left(\lambda-\lambda^{-5}\right)\left(C_{10}+\lambda^2 C_{01}\right)

\end{align*}

Here, C_{10} and C_{01} are Mooney-Rivlin material parameters.

\begin{align}\begin{split}

P_{1_{uniaxial}}& = 2\left(1-\lambda^{-3}\right)\left(\lambda C_{10} + 2C_{20}\lambda\left(I_{1_{uni}}-3\right)+C_{11}\lambda\left(I_{2_{uni}}-3\right)\\

& \quad +C_{01}+2C_{02}\left(I_{2_{uni}}-3\right)+C_{11}\left(I_{1_{uni}}-3\right)\right)\\

P_{1_{biaxial}}& = 2\left(\lambda-\lambda^{-5}\right)\left(C_{10}+2C_{20}\left(I_{1_{bi}}-3\right)+C_{11}\left(I_{2_{bi}}-3\right)\\

& \quad +\lambda^2C_{01}+2\lambda^2C_{02}\left(I_{2_{bi}}-3\right)+\lambda^2 C_{11}\left(I_{1_{bi}}-3\right)\right)

\end{split}

\end{align}

P_{1_{uniaxial}}& = 2\left(1-\lambda^{-3}\right)\left(\lambda C_{10} + 2C_{20}\lambda\left(I_{1_{uni}}-3\right)+C_{11}\lambda\left(I_{2_{uni}}-3\right)\\

& \quad +C_{01}+2C_{02}\left(I_{2_{uni}}-3\right)+C_{11}\left(I_{1_{uni}}-3\right)\right)\\

P_{1_{biaxial}}& = 2\left(\lambda-\lambda^{-5}\right)\left(C_{10}+2C_{20}\left(I_{1_{bi}}-3\right)+C_{11}\left(I_{2_{bi}}-3\right)\\

& \quad +\lambda^2C_{01}+2\lambda^2C_{02}\left(I_{2_{bi}}-3\right)+\lambda^2 C_{11}\left(I_{1_{bi}}-3\right)\right)

\end{split}

\end{align}

Here, C_{10}, C_{01}, C_{20}, C_{02}, and C_{11} are Mooney-Rivlin material parameters.

\begin{align}

P_{1_{uniaxial}} &= 2\left(\lambda-\lambda^{-2}\right)\mu_0\sum_{p=1}^{5}\frac{p c_p}{N^{p-1}}I_{1_{uni}}^{p-1}\\

P_{1_{biaxial}} &= 2\left(\lambda-\lambda^{-5}\right)\mu_0\sum_{p=1}^{5}\frac{p c_p}{N^{p-1}}I_{1_{bi}}^{p-1}

\end{align}

P_{1_{uniaxial}} &= 2\left(\lambda-\lambda^{-2}\right)\mu_0\sum_{p=1}^{5}\frac{p c_p}{N^{p-1}}I_{1_{uni}}^{p-1}\\

P_{1_{biaxial}} &= 2\left(\lambda-\lambda^{-5}\right)\mu_0\sum_{p=1}^{5}\frac{p c_p}{N^{p-1}}I_{1_{bi}}^{p-1}

\end{align}

Here, \mu_0 and N are Arruda-Boyce material parameters, and c_p are the first five terms of the Taylor expansion of the inverse Langevin function.

\begin{align}

P_{1_{uniaxial}} &= 2\left(\lambda-\lambda^{-2}\right)\sum_{p=1}^{3}p c_p \left(I_{1_{uni}}-3\right)^{p-1}\\

P_{1_{biaxial}} &= 2\left(\lambda-\lambda^{-5}\right)\sum_{p=1}^{3}p c_p \left(I_{1_{bi}}-3\right)^{p-1}

\end{align}

P_{1_{uniaxial}} &= 2\left(\lambda-\lambda^{-2}\right)\sum_{p=1}^{3}p c_p \left(I_{1_{uni}}-3\right)^{p-1}\\

P_{1_{biaxial}} &= 2\left(\lambda-\lambda^{-5}\right)\sum_{p=1}^{3}p c_p \left(I_{1_{bi}}-3\right)^{p-1}

\end{align}

Here, the values of c_p are Yeoh material parameters.

\begin{align}

P_{1_{uniaxial}} &= \sum_{p=1}^{N}\mu_p \left(\lambda^{\alpha_p-1} -\lambda^{-\frac{\alpha_p}{2}-1}\right)\\

P_{1_{biaxial}} &= \sum_{p=1}^{N}\mu_p \left(\lambda^{\alpha_p-1} -\lambda^{-2\alpha_p-1}\right)

\end{align}

P_{1_{uniaxial}} &= \sum_{p=1}^{N}\mu_p \left(\lambda^{\alpha_p-1} -\lambda^{-\frac{\alpha_p}{2}-1}\right)\\

P_{1_{biaxial}} &= \sum_{p=1}^{N}\mu_p \left(\lambda^{\alpha_p-1} -\lambda^{-2\alpha_p-1}\right)

\end{align}

Here, \mu_p and \alpha_p are Ogden material parameters.

Using the *Optimization* interface in COMSOL Multiphysics, we will fit measured stress versus stretch data against the analytical expressions detailed in our discussion above. Note that the measured data we are using here is the *nominal stress*, which can be defined as the force in the current configuration acting on the original area. It is important that the measured data is fit against the appropriate stress measure. Therefore, we will fit the measured data against the analytical expressions for the first Piola-Kirchhoff stress expressions. The plot below shows the measured nominal stress (raw data) for uniaxial and equibiaxial tests for vulcanized rubber.

*Measured stress-strain curves by Treloar.*

Let’s begin by setting up the model to fit the uniaxial Neo-Hookean stress to the uniaxial measured data. The first step is to add an *Optimization* interface to a 0D model. Here, *0D* implies that our analysis is not tied to a particular geometry.

Next, we can define the material parameters that need to be computed as well as the variable for the analytical stress versus stretch relationship. The screenshot below shows the parameters and variable defined for the case of an uniaxial Neo-Hookean material model.

Within the *Optimization* interface, a *Global Least-Squares Objective* branch is added, where we can specify the measured uniaxial stress versus stretch data as an input file. Next, a *Parameter Column* and a *Value Column* are added. Here, we define lambda (stretch) as a measured parameter and specify the uniaxial analytical stress expression to fit against the measured data. We can also specify a weighing factor in the *Column contribution weight* setting. For detailed instructions on setting up the *Global Least-Squares Objective* branch, take a look at the Mooney-Rivlin Curve Fit tutorial, available in our Application Gallery.

We can now solve the above problem and estimate material parameters by fitting our uniaxial tension test data against the uniaxial Neo-Hookean material model. This is, however, rarely a good idea. As explained in Part 1 of this blog series, the seemingly simple test can leave many loose ends. Later on in this blog post, we will explore the consequence of material calibration based on just one data set.

Depending on the operating conditions, you can obtain a better estimate of material parameters through a combination of measured uniaxial tension, compression, biaxial tension, torsion, and volumetric test data. This compiled data can then be fit against analytical stress expressions for each of the applicable cases.

Here, we will use the equibiaxial tension test data alongside the uniaxial tension test data. Just as we have set up the optimization model for the uniaxial test, we will define another global least-squares objective for the equibiaxial test as well as corresponding parameter and value columns. In the second global least-squares objective, we will specify the measured equibiaxial stress versus stretch data file as an input file. In the value column, we will specify the equibiaxial analytical stress expression to fit against the equibiaxial test data.

The settings of the Optimization study step are shown in the screenshot below. The model tree branches have been manually renamed to reflect the material model (Neo-Hookean) and the two tests (uniaxial and equibiaxial). The optimization algorithm is a Levenberg-Marquardt solver, which is used to solve problems of the least-square type. The model is now set to optimize the sum of two global least-square objectives — the uniaxial and equibiaxial test cases.

The plot below depicts the fitted data against the measured data. Equal weights are assigned to both the uniaxial and equibiaxial least-squares fitting. It is clear that the Neo-Hookean material model with only one parameter is not a good fit here, as the test data is nonlinear and has one inflection point.

*Fitted material parameters using the Neo-Hookean model. Equal weights are assigned to both of the test data.*

Fitting the curves while specifying unequal weights for the two tests will result in a slightly different fitted curve. Similar to the Neo-Hookean model, we will set up global least-squares objectives corresponding to Mooney-Rivlin, Arruda-Boyce, Yeoh, and Ogden material models. In our calculation below, we will include cases for both equal and unequal weights.

In the case of unequal weights, we will use a higher but arbitrary weight for the entire equibiaxial data set. It is possible that you may want to assign unequal weights only for a certain stretch range instead of the entire stretch range. If this is the case, we can split the particular test case into parts, using a separate *Global Least-Squares Objective* branch for each stretch range. This will allow us to assign weights in correlation with different stretch ranges.

The plots below show fitted curves for different material models for equal and unequal weights that correspond to the two tests.

*Left: Fitted material parameters using Mooney-Rivlin, Arruda-Boyce, and Yeoh models. In these cases, equal weights are assigned to both test data. Right: Fitted material parameters using Mooney-Rivlin, Arruda-Boyce, and Yeoh models. Here, higher weight is assigned to equibiaxial test data.*

The Ogden material model with three terms fits both test data quite well for the case of equal weights assigned to both tests.

*Fitted material parameters using the Ogden model with three terms.*

If we only fit uniaxial data and use the computed parameters for plotting equibiaxial stress against the actual equibiaxial test data, we obtain the results in the plots below. These plots show the mismatch in the computed equibiaxial stress when compared to the measured equibiaxial stress. In material parameter estimation, it is best to perform curve fitting for a combination of different significant deformation modes rather than considering only one deformation mode.

*Uniaxial and equibiaxial stress computed by fitting model parameters to only uniaxial measured data.*

To find material parameters for hyperelastic material models, fitting the analytic curves may seem like a solid approach. However, the stability of a given hyperelastic material model may also be a concern. The criterion for determining material stability is known as *Drucker stability*. According to the Drucker’s criterion, incremental work associated with an incremental stress should always be greater than zero. If the criterion is violated, the material model will be unstable.

In this blog post, we have demonstrated how you can use the *Optimization* interface in COMSOL Multiphysics to fit a curve to multiple data sets. An alternative method for curve fitting that does not require the *Optimization* interface was also a topic of discussion in an earlier blog post. Just as we have used uniaxial and equibiaxial tension data here for the purpose of estimating material parameters, you can also fit the measured data to shear and volumetric tests to characterize other deformation states.

For detailed step-by-step instructions on how to use the *Optimization* interface for the purpose of curve fitting, take a look at the Mooney-Rivlin Curve Fit tutorial, available in our Application Gallery.

Advanced composites are used extensively throughout the Boeing 787 Dreamliner, as shown in the diagram below. Also known as carbon fiber reinforced plastic (CFRP), the composites are formed from a lightweight polymer binder with dispersed carbon fiber filler to produce materials with high strength-to-weight ratios. Many wing components, for example, are made of CFRP, ensuring that they can support the load imposed during flight while minimizing their overall contribution to the weight of an aircraft.

*Advanced composites are used throughout the body of the Boeing 787. Copyright © Boeing.*

Despite their remarkable strength and light weight, CFRPs are generally not conductive like their aluminum counterparts, thus making them susceptible to lightning strike damage. Therefore, electrically conductive expanded metal foil (EMF) is added to the composite structure layup, shown in the figure below, to dissipate the high current and heat generated by a lightning strike.

*The composite structure layup shown at left consists of an expanded metal foil layer shown at right. This figure is a screenshot from the COMSOL Multiphysics® software model featured in this blog post. Copyright © Boeing.*

The figure also shows the additional coatings on top of the EMF, which are in place to protect it from moisture and environmental species that cause corrosion. Corrosive damage to the EMF could result in lower conductivity, thereby reducing its ability to protect aircraft structures from lightning strike damage. Temperature variations due to the ground-to-air flight cycle can, however, lead to the formation of cracks in the surface protection scheme, reducing its effectiveness.

During takeoff and landing, aircraft structures are subjected to cooling and heating, respectively. Thermal stress manifests as the expansion and compression — or ultimately the displacement — of adjacent layers throughout the depth of the composite structure. Although a single round-trip is not likely to pose a significant risk, over time, each layer of the composite structure contributes to fatigue damage buildup. Repetitive thermal stress results in cumulative strain and higher displacements, which are, in turn, associated with an increased risk of crack formation. The stresses in a material depend on its mechanical properties quantified by measurable attributes such as yield strength, Young’s modulus, and Poisson’s ratio.

By taking the thermal and mechanical properties of materials into account, it is possible to use simulation to design and optimize a surface protection scheme for aircraft composites that minimizes stress, displacement, and the risk of crack formation.

Evaluating the thermal performance of each layer in the surface protection scheme is essential in order to reduce the risks and maintenance costs associated with damage to the protective coating and EMF. Therefore, researchers at Boeing Research & Technology (BR&T), pictured below, are using multiphysics simulation and physical measurements to investigate the effect of the EMF design parameters on stress and displacement throughout the composite structure layup.

*The research team at Boeing Research & Technology from left to right: Patrice Ackerman, Jeffrey Morgan, Robert Greegor, and Quynhgiao Le. Copyright © Boeing.*

In their work, the researchers at BR&T have developed a coefficient of thermal expansion (CTE) model in COMSOL Multiphysics® simulation software. The figure shown above that presents the composite structure layup and EMF is a screenshot acquired from the model geometry used for their simulations in COMSOL Multiphysics.

The CTE model was used to evaluate heating of the aircraft composite structure as experienced upon descent, where the final and initial temperatures used in the simulations represent the ground and altitude temperatures, respectively. The *Thermal Stress* interface, which couples heat transfer and solid mechanics, was used in the model to simulate thermal expansion and solve for the displacement throughout the structure.

The material properties of each layer in the surface protection scheme as well as of the composites are custom-defined in the CTE model. The relative values of the coefficient of thermal expansion, heat capacity, density, thermal conductivity, Young’s modulus, and Poisson’s ratio are presented in the chart below.

*This graph presents the ratio of each material parameter relative to the paint layer. Copyright © Boeing.*

From the graph, trends can be identified that provide early insight into the behavior of the materials, which aids in making design decisions. For example, the paint layer is characterized by higher values of CTE, heat capacity, and Poisson’s ratio, thus indicating that it will undergo compressive stress and tensile strain upon heating and cooling.

Multiphysics simulation takes this predictive design capability one big step forward by quantifying the resulting displacement due to thermal stress throughout the entire composite structure layup simultaneously, taking into account the properties of all materials. The following figure shows an example of BR&T’s simulation results and presents the stress distribution and displacement throughout the composite structure.

*Left: Top-down and cross-sectional views of the von Mises stress and displacement in a one-inch square sample of a composite structure layup. Right: Transparency was used to show regions of higher stress, in red. Lower stress is shown in blue. Copyright © Boeing.*

In the plots at the left above, the displacement pattern caused by the EMF is evident through the paint layer at the top of the composite structure while a magnified cross-sectional view shows the variations in displacement above the mesh and voids of the EMF. The cross section also makes it easy to see the stress distribution through the depth of the composite structure, where there is a trend toward lower stress in the topmost layers. Transparency was used in the plot shown at the right to depict the regions of high stress in the composites and EMF, which is noticeably higher at the intersection of the mesh wires. Stress was plotted through the depth of the composite structure layup along the vertical red line shown in the center of the plot. The figure below shows the relative stress in each layer of the composite structure layup for different metallic compositions of the EMF.

*Relative stress in arbitrary units was plotted through the depth of the composite structure layups containing either aluminum (left) or copper EMF (right). Copyright © Boeing.*

The samples vary by the presence of a fiberglass corrosion isolation layer when aluminum is used as the material for the EMF. The fiberglass acts as a buffer resulting in lower stress in the aluminum EMF, when compared with the copper.

From lightning strike protection to the structural integrity of the composite protection scheme, it all relies on the design of the expanded metal foil layer. The design of the EMF layer can vary by its metallic composition, height, width of the mesh wire, and the mesh aspect ratio. For any EMF design parameter, there is a trade-off between current-carrying capacity, displacement, and weight. By using the CTE model, the researchers at BR&T found that increasing the mesh width and decreasing the aspect ratio are better strategies for increasing the current-carrying capacity of the EMF that minimize its impact on displacement in the composite structure.

The metal chosen for the EMF can also have a significant effect on stress and displacement in the composite structure, which was investigated using simulation and physical testing. Two composite structures, one with aluminum and the other with copper EMF, underwent thermal cycling with prolonged exposure to moisture in an environmental test chamber. In the results, shown below, the protective layers remained intact for the composite structure with copper EMF. However, for the layup with aluminum, cracking occurred in the primer, at the edges, on surfaces, and was particularly substantial in the mesh overlap regions.

*Photo micrographs of the composite structure layup after exposure to moisture and thermal cycling. A crack in the vicinity of the aluminum EMF is contained within the red ellipse. Copyright © Boeing.*

Simulations confirm the experiment results. Shown below, displacements are noticeably higher throughout the composite structure layup when aluminum is used for the EMF layer, where higher displacements are associated with an increased risk for developing cracks. The higher displacement is easiest to observe in the bottom plots, which show displacement ratios for each EMF height.

*Effect of varying the EMF height on displacement in each layer of the surface protection scheme. Copyright © Boeing.*

The larger displacements caused by the aluminum EMF can be attributed in part to its higher CTE when compared with copper, which exemplifies how important the properties of materials are to the thermal stability of the aircraft composite structures.

In the early design stages and along with experimental testing, multiphysics simulation offers a reliable means to evaluate the relative impact of the EMF design parameters on stress and displacement throughout the composite structures. An optimized EMF design is essential to minimizing the risk of crack formation in the composite surface protection scheme, which reduces maintenance costs and allows the EMF to perform its important protective function of mitigating lightning strike damage.

Refer to page 4 of *COMSOL News* 2014 to read the original article, “Boeing Simulates Thermal Expansion in Composites with Expanded Metal Foil for Lightning Strike Protection of Aircraft Structures”.

This article was based on the following publicly available resources from Boeing:

- The Boeing Company. “787 Advanced Composite Design.” 2008-2013.
- J.D. Morgan, R.B. Greegor, P.K. Ackerman, Q.N. Le, “Thermal Simulation and Testing of Expanded Metal Foils Used for Lightning Protection of Composite Aircraft Structures,” SAE Int. J. Aerosp. 6(2):371-377, 2013, doi:10.4271/2013-01-2132.
- R.B. Greegor, J.D. Morgan, Q.N. Le, P.K. Ackerman, “Finite Element Modeling and Testing of Expanded Metal Foils Used for Lightning Protection of Composite Aircraft Structures,” Proceedings of 2013 ICOLSE Conference; Seattle, WA, September 18-20, 2013.

To learn more about adding material property data to your COMSOL Multiphysics® simulations, read the following blog post series on *Obtaining Material Data for Structural Mechanics Simulations from Measurements* by my colleague Henrik Sönnerlind:

General information about aircraft design and structures can be found in chapter 1 of this handbook on aircraft maintenance from the Federal Aviation Administration.

*BOEING, Dreamliner, and 787 Dreamliner are registered trademarks of The Boeing Company Corporation in the U.S. and other countries.*

Let’s begin with a quick review. When solids enter a humid environment, it is likely that some of them will catch water molecules. The absorption and storage of these molecules can cause the solid to swell up, exposing it to increased stresses and strains. This effect is known as *hygroscopic swelling*.

Hygroscopic swelling is a phenomenon that occurs in various sectors of industry, from wood construction and paper to electronics and food processing. Whether an expected behavior or an undesirable effect, it must be modeled accurately in order to quantify its effects.

The Hygroscopic Swelling feature in COMSOL Multiphysics enables you to do exactly that. Available as a subnode for most material models in the structural mechanics interfaces, this feature allows you to analyze the effect of moisture concentrations within the solids, such as resulting deformations and stresses.

*The user interface (UI) of the Hygroscopic Swelling feature. The main inputs are colored and numbered.*

Using the above figure as our guide, we can now take a closer look at how this feature is used.

Hygroscopic swelling creates an inelastic strain that is proportional to the difference between the concentration and the strain-free reference concentration:

\epsilon_\textrm{hs}=\beta_\textrm{h} C_\textrm{diff}

where the coefficient of hygroscopic swelling \beta_\textrm{h} can be given in the material properties or directly in the node (Number 5 in the screenshot above). It does not have to be constant; it can depend on, for example, temperature or the moisture concentration itself.

In small deformation theory, the hygroscopic swelling contribution is additive — that is, the inelastic strain is the sum of the other inelastic strains and the hygroscopic strain. The coefficient of hygroscopic swelling is a second-order tensor, which can be defined as isotropic, diagonal, or symmetric. The expansion can thus be different in different directions. In wood, this effect is very pronounced.

In large deformation theory, available under the Hyperelastic Material model, the hygroscopic contribution is multiplicative — that is, the total deformation gradient tensor F is scaled by the hygroscopic stretch to form the elastic deformation gradient tensor F_\textrm{e} :

\begin{array}{ll}

\epsilon=\frac{1}{2} \left( F_\textrm{e}^\textrm{T}F_\textrm{e}-I \right) & F_\textrm{e}=F J_\textrm{hs}^{-1/3}

\\

J_\textrm{hs}= \left(1+\beta_\textrm{h} C_\textrm{diff} \right)^3

\end{array}

\epsilon=\frac{1}{2} \left( F_\textrm{e}^\textrm{T}F_\textrm{e}-I \right) & F_\textrm{e}=F J_\textrm{hs}^{-1/3}

\\

J_\textrm{hs}= \left(1+\beta_\textrm{h} C_\textrm{diff} \right)^3

\end{array}

In this case, the coefficient of hygroscopic swelling is isotropic, so only uniform volumetric expansion is taken into account.

The hygroscopic swelling has two types of effects. When applied on free structures, it induces deformations. When applied on constrained structures, deformation is impossible, causing the stress inside of the structure to increase. In real structures (often partially constrained), the effect is a mixture of these two behaviors.

*Example of a free solid (left column) and a fully constrained solid (right column) subjected to hygroscopic swelling with a constant moisture concentration. The first row shows roller constraints applied on each solid. Plotted results are the displacement field in the second row and von Mises stress in the third row. The free solid is only constrained by two roller conditions, which enables the solid to expand and completely release the stress. On the contrary, the solid constrained with roller conditions all around it shows no displacement but encounters an increase in stress.*

Depending on the selected moisture concentration type (2), the concentration is defined either as mass concentration ( C_\textrm{mo} and C_\textrm{mo,ref}) or molar concentration ( c_\textrm{mo} and c_\textrm{mo,ref}). As C_\textrm{diff} is the mass concentration difference, the molar mass M_\textrm{m} must also be specified (4) when molar concentration is used as the input. The default value for M_\textrm{m} is the molar mass of water 0.018 \; \textrm{kg}/\textrm{m}^3.

\begin{array} {ll} \epsilon_\textrm{hs}=\beta_\textrm{h} M_\textrm{m} \left(c_\textrm{mo}-c_\textrm{mo,ref} \right) \end{array} for molar concentration

\begin{array} {ll} \epsilon_\textrm{hs}=\beta_\textrm{h}\left(C_\textrm{mo}-C_\textrm{mo,ref} \right) \end{array} for mass concentration

The concentration (1) can either be user-defined or computed by another physics interface. As with any input in COMSOL Multiphysics, user-defined values can be a function of other variables, such as the space coordinates X, Y, and Z.

*On the left: User-defined, space-dependent moisture concentration. On the right: Displacement induced by hygroscopic swelling. The top face, where the concentration is highest, shows the largest displacement.*

The strain-free reference concentration (3) is the moisture concentration at which hygroscopic swelling has no effect. It can often be interpreted as an initial state, or the ex-factory moisture concentration. A moisture concentration higher than the reference concentration represents moistening and causes the solid to expand. A moisture concentration lower than the reference concentration represents drying and causes the solid to shrink.

*Left: Displacement with zero strain reference concentration. Right: Displacement with nonzero strain reference concentration. The applied concentration, which is the same in both cases but lower than the strain reference concentration, implies shrinkage of the solid.*

Often, the moisture concentration within a solid is unknown and has to be computed with a preceding simulation. You can compute the concentration with the *Transport of Diluted Species* interface or the *Transport of Diluted Species in Porous Media* interface. Such an approach is used in our MEMS Pressure Sensor Drift due to Hygroscopic Swelling example, new with COMSOL Multiphysics version 5.1.

One way to feed the computed concentration to the *Solid Mechanics* interface is to specify the desired concentration variable in the combo box of the Hygroscopic Swelling feature. There is, however, an even simpler approach.

In version 5.1, you can use a multiphysics coupling, which is made available when at least a solid mechanics and a transport physics interface are both present in the model tree. With this coupling feature, you simply have to specify which transport interface the concentration derives from and which solid mechanics interface to which you are applying hygroscopic swelling. You will also need to set the reference concentration, the molar mass, and the coefficient of hygroscopic swelling for all of the selected domains. When using the multiphysics coupling, you do not need to add any hygroscopic swelling subnodes to the material models.

*Selecting the participating physics interfaces in the Multiphysics Coupling node for hygroscopic swelling.*

*Left: Moisture concentration computed in the* Transport of Diluted Species interface. *Right: Displacement resulting from hygroscopic swelling.*

In the *Beam*, *Shell*, and *Plate* interfaces, the moisture concentration input is partitioned into an average concentration on the center line or midsurface, and a concentration gradient in the transverse direction(s). The latter causes the structure to bend.

The input for hygroscopic swelling in the *Beam* interface contains concentration gradient in the local *y-* and *z-*directions. In the *Shell* and *Plate* interfaces, it contains a concentration difference between the top face and the bottom face.

*Hygroscopic bending in a 2D* Beam *interface.*

*On the left: Moisture concentration. On the right: Resulting displacement. In the solid, bending is caused by the nonuniform expansion, which is higher on the top face than the bottom face. In the beam, the bending caused by the same effect is captured using the moisture gradient c_{\textrm{g}y}. In both plots, the solid model is placed above the beam model.*

When the “Include moisture as added mass” checkbox is marked (6), the weight of the water that is absorbed or released by the solid will have an effect on the mass-dependent phenomena, such as gravity or rotating frame loads. It will also have an effect on inertial terms in time-dependent or frequency domain studies.

*On the left: Displacement of two bars analyzed with a frequency sweep when one of them is subjected to hygroscopic swelling. On the right: Frequency response of the two bars. The water absorbed during hygroscopic swelling increases the mass and decreases the resonance frequency.*

The total mass, including the water mass uptake, can be calculated in a Mass Properties node under *Definitions*. The mass variable can then be used in postprocessing for comparison with the measured mass of the solid — a convenient way to evaluate the moisture concentration in real life.

*Screenshot of the Mass Properties node.*

Taking hygroscopic swelling into consideration is important in the design of many devices. By analyzing how different materials respond to that effect, you can optimize your design so as to prevent the failure of components and to ensure the device’s intended operation. Here, we have demonstrated how the hygroscopic swelling functionality in COMSOL Multiphysics can be a valuable tool for such an analysis. With the Hygroscopic Swelling feature, you can quantify the effects of hygroscopic swelling in a way that is both accurate and efficient.

- Download the tutorial model: MEMS Pressure Sensor Drift due to Hygroscopic Swelling
- Read more about the new multiphysics coupling feature for hygroscopic swelling on our COMSOL Multiphysics 5.1 release highlights page

In my previous role as a structural analysis consultant, I sometimes came across the problem of how to report ridiculously high stress peaks in a finite element model to a customer. Experienced analysts know when stress peaks are an expected effect of modeling and can be safely ignored. Though, when a requirement that “the stress must nowhere exceed 70% of the yield stress” has been stated, this may still turn out to be an issue. Equally important is the fact that the small red spots in the color plots cannot always be ignored. Thus, we must have appropriate techniques for interpreting the model results.

Sharp reentrant corners will cause a singularity in the derivatives of the dependent variables for all elliptic partial differential equations. In structural mechanics, this means that the strains can become unbounded since the degrees of freedom are the displacements. Unless limited by the material model, the stresses will also be infinite in such a case.

Stresses are investigated in the majority of structural mechanics analyses. This is why singularities present more of an issue in structural mechanics than in most other physics fields. In heat transfer analyses, for instance, you are much more likely to be interested in the temperature than in the local values of the heat flux, the area in which a singularity would become evident.

Let’s have a look at a prototype problem. This problem involves a 2 meters by 1 meter rectangular plate, featuring a square cutout with a side of 0.2 meters, that is subjected to pure tension:

*The plate is constrained along the left edge and has a uniform load along the right edge.*

With two different meshes around the hole, the default plots of the effective stress look completely different. Since the peak stress is twice as high in the model with the finer mesh, most details in the stress field are lost. This can of course be remedied by manually adjusting the range of the plots, but it may hide important details at first glance.

*The same effective stress field in two plots. Both plots are automatically scaled by the mesh-dependent peak stress.*

In fact, the smaller the elements that are used in the corner, the higher the values of stress that will be found. The results will not converge since the “true” solution tends toward an infinite value.

*Stress at the corner as a function of element size (logarithmic horizontal axis).*

If we investigate the stress field close to the hole, we will find that the stress peak is very localized. In the figure below, the stress is plotted along a vertical cut line drawn at a distance of 0.05 meters from the hole. At this distance, the stress is virtually unchanged, even though the peak stress at the corner varies by a factor of two.

*Stress variation along a cut line (represented in red). Five different mesh sizes are used.*

In the real world, there are seldom perfectly sharp corners. Thus, you could argue that by using an accurate geometry representation containing all fillets, it is possible to avoid singularities. While true, this comes with a price tag. If very small geometrical details must be resolved by the mesh, the model grows enormously in size (especially the case in 3D). Even when a perfect CAD geometry is available, it is common practice to *defeature* the geometry to remove small details that are not important within the scope of the analysis. Therefore, in many cases, we actually deliberately introduce sharp corners at the preprocessing stage.

There are, however, some drawbacks to keeping the sharp corner:

- If the material model is nonlinear, there may be numerical problems at the singularity. For example, the strain rate predicted by a creep model is often proportional to a high power of stress. The high stress at the singularity (a value determined only by the mesh) raised to a power of five may result in strain rates so high that the time stepping is forced to be in the order of milliseconds, when you actually want to study an event taking place over months. If you still want to keep the sharp corner, the remedy here is to enclose the singularity in a small elastic domain.
- Adaptive meshing, error estimates, and the like can fail since the singularity will dominate over the rest of the solution. Exclude the corner from any such procedures.
- When running an optimization where stresses are part of the problem formulation, the singularity will lead to solutions that are optimal only in terms of reducing the amplitude of the unphysical peak stress. In the Multistudy Optimization of a Bracket tutorial, the region where the bracket is bolted is excluded from the search for a maximum stress.
- As previously noted, the high stress peaks tend to obscure more interesting features in the solution, both visually and psychologically.

Physically, if the corner is very sharp, the material will be damaged by the high strains. A brittle material may crack; a ductile material may yield. While it may sound alarming, such damage will only cause a local redistribution of the stresses in most cases. As seen from the perspective of the surrounding structure, the effect is no more dramatic than that of somewhat changing the fillet radius. High, very localized stresses will only be a true problem if the loading is cyclic, which creates a risk for fatigue.

In a building, nobody is concerned that the holes for windows and doors are rectangular with sharp corners. But, in an airliner, you will find that the windows are smoothly rounded since the variation between the pressure in the cabin and the pressure outside will provide a cyclic stress history.

*Left: A rectangular window featuring sharp corners. Image by Jose Mario Pires. Licensed under CC BY-SA 4.0 via Wikimedia Commons. Right: A window with smoothly rounded corners. Image by Orin Zebest. Licensed under CC BY-SA 2.0 via Wikimedia Commons.*

This is in fact recognized by many design standards, where high local stresses are allowed as long as the loads are static. The local corner stresses will not in any way affect the load-bearing capacity of the structure. Using this type of approach does rely on a systematic way of classifying the stress fields. Such methods are, for example, described in the *ASME Boiler & Pressure Vessel Code*.

For cyclic loads, on the other hand, it is important to obtain very accurate stress values. The fatigue life depends strongly on the stress amplitude. In this case, an accurate representation of the fillet is necessary, not only geometrically but also in terms of mesh resolution. If the model becomes too large to handle, you can use *submodeling*, an approach that is described in detail in this blog post.

*The detailed submodel on the right is driven by the results from the global analysis.*

Tip: To further explore the submodeling technique, download the Submodeling Analysis of a Shaft tutorial from our Application Gallery.

A force applied to a single point on a solid will locally give infinite stresses. This is the classical *Boussinesq-Cerruti problem* in the theory of elasticity, where the stresses vary as the inverse of the distance from the loaded point.

In the real world, point loads do not exist. The force is always distributed over a certain area. From the finite element analysis perspective, the question is whether or not it is worth the effort to resolve this small region. The answer to that question lies in the *Saint-Venant’s principle*, which states that all statically equivalent load distributions give the same result at a distance that is large enough when compared to the size of the loaded area.

Thus, when detailed results are not important within a distance of, say, three times the size of the loaded area, it actually does not matter how you apply the loads, so long as the resulting force and moment are correct. Just as in the case with the corner singularity, you may still need to avoid the effects of singular stresses. Note that line loads will have the same effect as a point load in causing local infinite stresses.

It is interesting to make mention of the fact that a point load applied on a beam element or perpendicular to a shell will *not* induce a singularity. The bending of the structural elements is governed by equations other than solid mechanics. However, a point load applied in the plane of a shell *will* cause a singularity.

If we think of a constraint in terms of its capability to apply a reaction force, it is evident that the same conclusions can be drawn as those for loads with respect to, for example, constraints applied to a point. But, that is not all. Consider the seemingly symmetric problem below. Here, we have a plate with a constant tensile load on one side and corresponding roller conditions on the other side.

*A square plate with one half of the vertical boundaries constrained and loaded.*

When looking at the stress distribution, it is apparent that the end of the roller condition introduces a singularity that the sudden change in the load does not. A general observation is that the end of a constraint has an effect that is similar to that of a sharp corner.

*Horizontal stress distribution.*

An infinitely stiff environment supporting the structure does not exist in reality. The analyst is again left with a choice: Can I live with the little red spot, or do I need to pay more attention to what is outside of my structure?

If the singularity caused by the boundary condition is not acceptable, you could consider the following approaches:

- Extend the model so that any singularity caused by the boundary condition is moved outside of the area of interest.
- Use a softer boundary condition by applying a Spring Foundation condition, for instance.
- Use infinite elements, which offer a cheap method for extending the computational domain. Learn more with this tutorial.

Situations similar to the one mentioned above are inevitable in many kinds of transitions. An example of such a transition is connecting a rigid domain to a flexible domain.

The art of analyzing welds is so important and complex that it warrants its own blog post. Here, we will only briefly touch on this subject.

Welded structures often consist of thin plates, so it is natural to use shell models in this context. Let’s have a look at the model below. In this example, a stress concentration is evident in the area where the smaller plate is welded to the wide plate.

*Stresses in a simple shell model of two plates welded together.*

The geometry and loads are symmetric with respect to the center of the geometry. The mesh in this model, however, is designed so that it is much finer at one end of the weld. A graph of the stress along the weld line reveals a singularity in the stress field in both plates.

*A stress plot identifying a singularity.*

For many welded structures — ship hulls, cargo cranes, and truck frames — dimensioning against fatigue is important. Refining the modeling process by using a solid model is seldom the answer here. The local geometry and quality of a weld is rarely well defined, unless it has been ground and X-rayed. The local geometry will differ along the weld and between the corresponding welds on two items that nominally should be identical.

When analyzing welds, the most common approach is to average the stress along the weld line or along a parallel line a certain distance away. The cut lines in COMSOL Multiphysics are particularly helpful here. The local coordinate systems also come in handy since stress components parallel and normal to the weld need to be treated differently. These averaged stresses are then compared with handbook values, which are available for a number of weld configurations and weld qualities. To learn more, see *Eurocode 3: Design of steel structures — Part 1-9: Fatigue*.

The worst conceivable geometrical singularity is the one caused by a crack. A crack can be seen as a 180° re-entrant corner, so many aspects of the corner singularity are also applicable here. When a crack is present in a finite element model, it is typically an area of focus within the study.

*The stress field around a crack tip, with the deformation scaled.*

The stress field around the crack tip is known from analytical solutions, at least for linear elasticity and plasticity under some assumptions. Computing the stress field through finite element analysis, however, can be difficult due to the singularity. Fortunately, it is usually not necessary to study the details at the crack tip. When determining the stress intensity factor, for example, you can use either the *J-integral* or *energy release rate* approach. These methods make use of global quantities far from the crack tip, so that the details at the singularity become less important.

Tip: Looking to explore the use of the J-integral approach in further detail? Consult the Single Edge Crack tutorial in our Application Gallery.

Singularities appear in many finite element models for a number of different reasons. As long as you understand how to interpret the results and how to circumvent some of the consequences, the presence of singularities should not be an issue in your modeling. In fact, many industrial-size models require the intentional use of singularities. Keeping down model size and analysis time often necessitates simplification of geometrical details, loadings, and boundary conditions in a way that introduces singularities.

]]>In Part 1 of this blog series, we discussed some of the considerations that you need to make when transforming your measured material data into a constitutive model. Hyperelastic materials were discussed in some detail. Today, we will have a look at how to use nonlinear elastic and elastoplastic materials, and show one way in which you can use your measured data directly in COMSOL Multiphysics.

Some materials already exhibit significant nonlinearity at small strains. Cast iron and some ceramics show this behavior, for example. However, when unloaded from a moderate strain, they follow the same stress-strain path back to the original state, so the response is elastic. This calls for a nonlinear elastic model.

In the previous blog post, we discussed hyperelastic materials, so why not just use one of these models to fit the measured stress-strain curve for, say, a nodular cast iron? The answer is that the hyperelastic material models are tailored for large strains. In elastomers, you may have elongations of several hundred percent of the original length, whereas the elastic range of metals and more brittle materials is usually less than 1%.

The very popular Mooney-Rivlin model will, for example, be essentially linear for small strains, and is therefore not useful in this context. In the Ogden model, the stress is computed as a sum of powers of the stretches. But for small strains, the stretch may have a range from 0.999 to 1.001 or so. In order to predict a significant nonlinearity, the exponent in the power law would have to be extremely high. A stable fitting of data to such an equation is not feasible. At the low strains present in a brittle material, the engineering strain would be a more natural representation of deformation. You can read more about different stress and strain measures in the blog entry “Why All These Stresses and Strains?”

To cope with this situation, COMSOL provides a set of nonlinear elastic models intended for small strains. These material models require the Nonlinear Structural Material Module or the Geomechanics Module and are available in the *Solid Mechanics* and *Membrane* interfaces. Let’s investigate how you can use these materials.

*Selecting a nonlinear elastic material model in COMSOL Multiphysics.*

In total, there are nine nonlinear elastic material models. Some of them have a simple mathematical form determined by a few parameters. One material model is especially useful when dealing with experimental stress-strain data: *Uniaxial data*. This model is explicitly intended for analyses based on measured data. Let’s have a look at the settings for this model:

*The settings for the Uniaxial data nonlinear elastic model.*

The main input is a function relating the uniaxial stress to the uniaxial strain. In this example, the measured data is given in terms of an interpolation function, called `stress_strain_curve`

, but it could also have been an analytical expression. An interpolation function can be entered explicitly as a number of data points or it can be read from a file. Here, the import is made directly from an Excel® file. This requires the LiveLink™ *for* Excel® add-on, but it is also possible to read the data from tabulated text files.

*Imported uniaxial stress-strain curve.*

The uniaxial curve does not, however, provide enough information to completely define a multiaxial constitutive law. One more assumption is needed, which is why you have to provide either a constant Poisson’s ratio or bulk modulus. For many materials, a constant Poisson’s ratio with a value between 0.2 and 0.3 will provide a good approximation. This is all that is needed to complete the material model.

If you study the stress-strain curve above, you will notice that it is different in tension and compression. In a multiaxial stress state, however, a certain point in the material may experience tension in one direction and compression in another. So which branch of the material curve should then be used? The material model is isotropic, so it has the same stiffness in all directions, but it is the volume change that is decisive. If the local volume change is negative, the compression branch is used.

An isotropic nonlinear elastic material is only admissible from the theoretical point of view if:

- The mean stress (“pressure”) or bulk modulus is a function only of the volumetric strain.
- The shear stress or shear modulus is a function only of the shear strains.

If these conditions are violated, you can devise a stress-strain cycle from which it is possible to extract energy, that is, a *perpetuum mobile*.

All of the built-in materials are designed so that these conditions are fulfilled. If you take a look at the settings for the Bilinear elastic material, you will have to input the bulk moduli for this in tension and compression — not the Young’s moduli as you might have anticipated.

Most structural analysts work with Young’s modulus and Poisson’s ratio as the primary parameters for elastic materials. But the requirements above unfortunately mean that if Young’s modulus has a dependence on the strain, then…

- The function describing this dependency can only have some very specific forms.
- Poisson’s ratio must also be a function of strain, which leads to a function that is very difficult to express.

So how was it possible to enter the Uniaxial data above with a constant Poisson’s ratio? The answer is that we created behind-the-scenes allowable functions for the bulk modulus and shear modulus. No reference is made to Young’s modulus, even though that is what you would intuitively derive in the graph.

That said, I have seen quite a number of successful models where an analyst has introduced strain dependencies in the Young’s moduli for isotropic or orthotropic materials in an elastic material model. For practical engineering use, this may work fine. We supply an example of how to define a stress-dependent Young’s modulus in the Modeling Stress-Dependent Elasticity tutorial. The important point for such an approach to be acceptable is that the structure should be subjected to a mainly proportional loading (in the sense that the directions of the principal strains do not rotate).

*Cantilever beam with different values of Young’s modulus in tension and compression. The beam is subjected to a bending moment at the free end. The upper plot shows von Mises stress; the lower plot shows the current value of Young’s modulus.*

When you set out to model nonlinear elasticity by either using the built-in models or by your own expressions, it is important to keep a clear distinction between a *tangent stiffness* and a *secant stiffness*. A nonlinear elastic model is often expressed similarly to the linear model, but with a stress or strain dependence in the elastic constant (which is no longer a constant!). Assume that the shear stress \tau is related to the shear strain \gamma through

\tau = G_S(\gamma) \cdot \gamma

The shear modulus G_S(\gamma) is then a secant shear modulus. When the total strain is multiplied by the secant modulus, the result is the total stress. The tangent shear modulus G_T(\gamma), on the other hand, is the stiffness experienced for a small change in strain, as illustrated by the figure below.

Mathematically, the relation between the two moduli is

G_T(\gamma) = \frac{d \tau}{d \gamma} = G_S(\gamma) + \frac{d G_S(\gamma)}{d \gamma} \gamma

Your measured data will usually have the form

\tau = f(\gamma)

This means that the secant stiffness actually is

G_S(\gamma) = \frac{f(\gamma)}{\gamma}

When converting a stress-strain curve into secant form using this expression, special attention must be given to the possible zero-divide at zero strain.

Also, you may sometimes encounter the statement that a certain material has been fitted to a power law with a certain exponent *n*. This may either mean that

\tau = C \gamma^n

or that

G_s = C \gamma^n

The Power law model in COMSOL Multiphysics uses the former, more common definition, where the strain exponent *n* relates to the slope of the stress-strain curve in a semi-log plot.

A pure tension experiment cannot determine whether a certain measured nonlinearity is caused by plasticity or not. The unloading curve must also be investigated. This is illustrated by the animation below, taken from the previous blog post.

The use of a nonlinear elastic model to simulate plasticity has been explored in a previous blog post.

In addition to using the Uniaxial data model, the Ramberg-Osgood nonlinear elastic material model is specifically intended for use as a simple replacement for a full elastoplastic model. Using a nonlinear elastic material is significantly cheaper in terms of computer resources, but what are the limitations of such an approach?

- Obviously, only a continuous increase in the loading is allowed.
- If there are several external loads acting, for example a pressure load together with thermal expansion, these are usually not proportional to each other. This may cause the local stresses to be non-proportional.
- The three-dimensional response will usually not be the same, even if the uniaxial stress-strain curve is identical for a nonlinear elastic model and a full elastoplastic model. In metal plasticity, like a von Mises flow rule, plastic deformation preserves the volume. This will not be the case in a corresponding nonlinear elastic model.

When deciding upon a suitable material model, you must take into account the accuracy of the whole analysis. In engineering, we are often working with incomplete information, and there will be uncertainties in the loads, in the homogeneity of the materials, and in the actual dimensions of the structure. You will also introduce approximations by the selection of boundary conditions. It is the weakest link in the chain that determines the quality of the results, and that may well not be the exact mathematical foundation of the material model.

In the previous blog post, I stated that “it is not a good idea to just enter a simple stress-strain curve as input.”

So why did I change my mind today? The answer is that when working with the Uniaxial data model, it is the actual measurements that are used. For all hyperelastic models, and most of the other nonlinear elastic models, the measured data must be fitted to a mathematical model with a small number of parameters. It is this fitting that cannot safely be done without human supervision.

]]>We often get requests of the type “I would like to just enter my measured stress-strain curve directly into COMSOL Multiphysics”. In this new blog series, we will take a detailed look at how you can process and interpret material data from tests. We will also explain why it is not a good idea to just enter a simple stress-strain curve as input.

All material models are mathematical approximations of a true physical behavior. Material models can, however, not always be derived from physical principles, like mass conservation or equations of equilibrium. They are by nature phenomenological and based on measurements. The laws of physics will, however, enforce limits on the mathematical structure of material models and the possible values of material properties.

It is well known, even from everyday life, that different materials exhibit completely different behavior. A material can be very brittle, like glass, or very elastic, like rubber. Choosing a material model is not only determined by the material as such, but also by the operating conditions. If you immerse a piece of rubber into liquid nitrogen, it will become as brittle as glass — a popular educational experiment. Also, if you heat up glass, it will start to creep and show viscoelastic behavior.

When analyzing structural mechanics behavior in COMSOL Multiphysics, you can choose between about 50 built-in material models, many of them featuring several options for their settings. You can also set up and define your own material models, or combine several of the material models to, for example, describe a material exhibiting both creep and plasticity at the same time.

Some of the available classes of materials are:

- Linear elastic
- Hyperelastic
- Nonlinear elastic
- Plasticity
- Creep
- Concrete

Without going into details about how you should actually come to the correct decision about an appropriate material model, here are some questions you should ask yourself before you start modeling:

- How large are the stress and strain ranges?
- Will the loading speed be important?
- What is the operating temperature and will it be constant?
- Is there a predefined material model targeted specifically at my material, such as concrete or soil plasticity?
- Is the load constant, monotonously increasing, or cyclic?
- Is the stress state predominantly uniaxial or is it fully three-dimensional?

Based on these considerations, you can then make a choice of a suitable material model. Determining the correct parameters to use in this material model will then be more or less difficult.

On one end of the spectrum, there are common materials (such as steel at room temperature) where many engineers know the material data by heart (E = 210 GPa, *ν* = 0.3, *ρ* = 7850 kg/m^{3}) and where data is easily found in the literature or through a simple web search.

On the other end of the spectrum, finding the high temperature creep data for a cast iron to be used in an exhaust manifold can be a major project in itself. Many tests at different load levels and at different temperatures are required. A complete test program for this may take half a year and have a price tag of several hundred thousand dollars.

*Tensile testing equipment. “Inspekt desk 50kN IMGP8563″ by Smial. Original uploader was Smial at de.wikipedia — Transferred from de.wikipedia; transferred to Commons by User: Smial using CommonsHelper. (Original text: eigenes Foto). Licensed under CC BY-SA 2.0 de via Wikimedia Commons.*

Before starting your simulation with COMSOL Multiphysics, it is not enough to import the geometry of the specimen, select the material model, and apply the loads and other boundary conditions; you should also provide the parameters for the chosen material model in the operating stress-strain and temperature range. These parameters are typically obtained from one or more tests.

The most fundamental test is the *uniaxial tensile test*. This is also what most engineers in daily life refer to when they state that they have a “Stress-Strain curve.” If you look at the list of questions above, it is evident that even this seemingly simple test can leave many loose ends:

- A material may exhibit time dependence even at constant loads, giving creep or viscoelastic effects. Many tests, often at different temperature and stress levels, are needed to give reliable data.
- Material parameters obtained from an ordinary tensile test at low speed may not be representative of the material behavior at high strain rates. A crash analysis might show strain rates as high as 10 s
^{-1}, while conventional uniaxial testing machines can use strain rates as low as 10^{-3}s^{-1}. - Is the material isotropic or would tests in several directions be required?
- If you only have a tension test, what would happen in compression? With a single curve, you cannot really tell.
- A tensile test will supply stress versus strain in the tested direction, but it will not always contain data about the deformations in the transverse direction. Without that data, you have no information at all about the cross-coupling between the directions in the 3D case.
- When curve fitting experimental measurements, perhaps not all data should be given equal weight. It may so be that the response in a certain strain range has a larger impact on your simulation results.

Some materials, like concrete, have little or no capacity to carry loads in tension. Here, the *uniaxial compression test* is the most fundamental test. It has many properties in common with the tensile test.

Other materials, like steel and rubber, can also be tested in compression. It is actually a good idea to do so, as we will demonstrate later in this blog post.

When using only uniaxial testing (whether it is in tension, compression, or both), you can however not achieve the full picture of the properties of a given material. You will need to combine it with some other assumptions like isotropy or incompressibility. For many materials, such assumptions are well justified by experience, though.

We have illustrated how the range of a test will affect your conception of the material behavior in the animation below.

- If you just do the onloading part, it is not possible to discriminate between elastic and plastic behavior.
- By unloading, you can distinguish plastic from elastic behavior, but until the specimen is in a state of significant compression, it is not possible to determine whether an isotropic or a kinematic hardening model would give the best representation.

It is significantly more difficult to design testing equipment that can create a homogenous biaxial stress state. *Biaxial testing* is often used for materials that are available only in thin sheets, like fabrics, for instance. By controlling the ratio between the loads in two perpendicular directions, it is possible to extract much more information than from a uniaxial test.

For soils, which generally need to be confined, *triaxial compression* is a common test. Triaxial compression tests could in principle be applied to a block of any material, but the testing equipment is difficult to design. The low compressibility of most solid materials also makes triaxial testing less attractive, since the measured displacements will be small when the material is compressed in all directions.

The Triaxial Test model shows a finite element model of a triaxial compression test.

The *torsion test*, where a cylindrical test specimen is twisted, is a rather simple test that generates a non-uniaxial stress state. The stress state is, however, not homogenous through the rod. Therefore, some extra processing is needed to translate the moment versus angle results to stress-strain results.

In an upcoming blog post in this series, we will make an in-depth demonstration of how to fit measured data to a number of different hyperelastic material models. In the example here, we will assume that you have been able to fit your data to the tests. The raw data consists of two measurements: one in uniaxial tension and another in equibiaxial tension, as shown below.

The nominal stress (force divided by original area) is plotted against stretch (current length divided by original length).

*Measured stress-strain curves by Treloar.*

Since the data covers a wide range of stretches, the experimental results are clearly nonlinear. The simplest hyperelastic models with one or two parameters will probably not be sufficient to fit the experimental data. The Ogden model with three terms is a popular model for rubber, and it is the model we used here.

A least squares fit will give the results below when assigning equal weights to both data sets. As we can see in the graph, it is possible to fit both experiments very well with a single set of material parameters.

*Fitted material parameters using a three terms Ogden model.*

But what if the biaxial test had not been available? Fitting only the uniaxial data will give a different set of material parameters, which will of course fit that set of experimental data even more closely, but it would deviate from the biaxial results. This is shown below.

*Analytical results for uniaxial and biaxial tension when only the uniaxial data was used to fit the model parameters.*

Clearly, the prediction for a equibiaxial stress state will differ between the two sets of parameters. As we can see, the error in stress in the biaxial curve is more than 20% at some stretch levels.

What about other stress states? Two stress states that can be simulated in a simple finite element model are uniaxial compression and pure torsion. The uniaxial stress-strain curve over a wide range of stretches is shown below. The results on the tensile side are not as sensitive to the data set used for obtaining the material parameters as the compressive side is. This is not surprising as tensile data is used for parameter fitting in both cases, whereas neither of the experiments contain any information about the compressive behavior.

*Uniaxial response ranging from compression to tension. The scale on the *x*-axis is logarithmic.*

Note that operating conditions of rubber parts, such as seals, are often under predominantly compressive states. If the data sets used for parameter fitting contain only tension data, this may be a source of inaccuracy when modeling multiaxial stress states.

Finally, let’s have a look at a simulation where a circular bar is twisted. The same type of discrepancies between the results from two sets of material parameters as above can be seen below.

*Computed torque as function of the twist angle.*

Finally, it should be noted that many hyperelastic models are only conditionally stable. This means that even though the estimated material parameters are perfectly valid for a certain strain range, a unique and continuous stress-strain relation may not even exist for other strain combinations. We often come across such problems in support cases. This is unfortunately rather difficult to detect a *priori*, since it would require a full search of all possible strain combinations.

Measured data must be processed and analyzed before being used as input for simulations. For material models other than the simpler linear elastic model, it is a good idea to make small examples with a unit cube to assess the behavior under different loading states before using the material model in a large-scale simulation.

So the answer to the question: “I would like to just enter my measured stress-strain curve directly into COMSOL Multiphysics” is that such an approach is *not* recommended. That would make the software a black box where the user really must take a number of active decisions in order to obtain meaningful results.

Up next in our Structural Materials series: We will discuss nonlinear elasticity and plasticity.

]]>

With its notable display of historical artwork, the Louvre has become a central landmark in Paris, France. As the Louvre grew in popularity — eventually ranking as one of the world’s most visited museums — it became evident that the building’s original entrance could no longer handle the large number of guests admitted on a daily basis. The need for an entrance with a greater capacity prompted the construction of the Louvre Pyramid within the museum’s courtyard in 1989. This structure now serves as the main entrance to the building, descending visitors into a spacious lobby and then moving them up to the museum level.

*The Louvre Pyramid. (“Courtyard of the Louvre Museum, with the Pyramid” by Alvesgaspar — Own work. Licensed under Creative Commons Attribution Share-Alike 3.0, via Wikimedia Commons).*

In comparison to the Louvre’s classical architecture, the pyramid was based on a more modern design approach — the space frame. A *space frame* is a truss-like structure composed of interlocking struts that form a geometric pattern. Requiring few interior supports, these structures offer a lightweight and elegant solution in structural engineering. Additionally, due to their inherent rigidity, space frames are able to span large areas while maintaining a strong resistance.

The Louvre pyramid is just one example of a building based on a space frame design. Many other structures, such as the Eden Project in England and Globen in Sweden, have also used a space frame as the basis for their construction. With its common application in modern buildings, it is important to study how loads affect the stability of such structures.

In the new COMSOL Multiphysics version 5.0 model, Instability of a Space Arc Frame, we set up and analyze a space frame. In this benchmark model, the frame undergoes concentrated loading at various points, with a small lateral load implemented to break the structure’s symmetry. The description of the space frame and the applied loads are based on the example from “A Mixed Co-rotational 3D Beam Element for Arbitrarily Large Rotations” by Z.X. Li and L. Vu-Quoc.

*A schematic depicting the space frame’s geometry.*

As a constraint, all of the frame’s base points are pinned. Vertical concentrated loads P are applied to the top four corners of the space frame. Meanwhile, lateral loads of 0.001*P are applied to the frame’s two front corners. These lateral loads are designed to perturb the frame’s symmetry to implement a controlled instability. The figure below shows the final state of the deformed frame.

*Deformed space frame.*

Next, we can evaluate the relationship between the compressive load and the horizontal displacement on point A of the frame. Comparing the reference data with the simulation results, the plot below illustrates a strong agreement between the two findings.

*A plot relating load parameter P and displacement v. Here, the simulation results are compared with the reference data.*

Furthermore, this plot highlights an instability occurring at a parameter value of around 8.0, even though a deviation from linearity can be seen much earlier. In practice, an imperfect structure’s critical load is often far lower than that of the ideal structure, as was discussed in this previous blog post.

- Download the model: Instability of a Space Arc Frame

The nonlinear stress-strain behavior in solids was already described 100 years ago by Paul Ludwik in his *Elemente der Technologischen Mechanik*. In that treatise, Ludwik described the nonlinear relation between shear stress \tau and shear strain \gamma observed in torsion tests with what is nowadays called *Ludwik’s Law*:

(1)

\tau = \tau_0 + k\gamma^{1/n}

For n=1, the stress-strain curve is linear; for n=2, the curve is a parabola; and for n=\infty, the curve represents a perfectly plastic material. Ludwik just described the behavior (*Fließkurve*) of what we now call a *pseudoplastic material*.

In version 5.0 of the COMSOL Multiphysics simulation software, beside Ludwik’s power-law, the Nonlinear Structural Materials Module includes different material models within the family of nonlinear elasticity:

- Ramberg-Osgood
- Power Law
- Uniaxial Data
- Bilinear Elastic
- User Defined

In the Geomechanics Module, we have now included material models intended to represent nonlinear deformations in soils:

- Hyperbolic Law
- Hardin-Drnevich
- Duncan-Chang
- Duncan-Selig

The main difference between a nonlinear elastic material and an elastoplastic material (either in metal or soil plasticity) is the reversibility of the deformations. While a nonlinear elastic solid would return to its original shape after a load-unload cycle, an elastoplastic solid would suffer from permanent deformations, and the stress-strain curve would present hysteretic behavior and ratcheting.

Let’s open the Elastoplastic Analysis of a Plate with a Center Hole model, available in the Nonlinear Structural Materials Model Library as *elastoplastic_plate*, and modify it to solve for one load-unload cycle. Let’s also add one of the new material models included in version 5.0, the *Uniaxial data* model, and use the stress_strain_curve already defined in the model.

Here’s a screenshot of what those selections look like:

In our example, the stress_strain_curve represents the bilinear response of the axial stress as a function of axial strain, which can be recovered from Ludwik’s law when n=1.

We can compare the stress distribution after laterally loading the plate to a maximum value. The results are pretty much the same, but the main difference is observed after a full load-unload cycle.

*Top: Elastoplastic material. Bottom: Uniaxial data model.*

Let’s pick the point where we observed the highest stress and plot the *x*-direction stress component versus the corresponding strain. The green curve shows a nonlinear, yet elastic, relation between stress and strain (the stress path goes from a\rightarrow b \rightarrow a \rightarrow c \rightarrow a). The blue curve portraits a hysteresis loop observed in elastoplastic materials with isotropic hardening (the stress path goes from a\rightarrow b \rightarrow d \rightarrow e ).

With the Uniaxial data model, you can also define your own stress-strain curve obtained from experimental data, even if it is not symmetric in both tension and compression.

- P. Ludwik.
*Elemente der Technologischen Mechanik* - “Hypoelasticity“, Chapter 3.3 of
*Applied Mechanics of Solids* - Download the Elastoplastic Analysis of a Plate with a Center Hole model

The piezoelectric modeling interface seeks to:

- Make the modeling workflow more
- Transparent
- Flexible

- Enable you to debug the models more easily

This will allow you to successfully simulate piezoelectric devices as well as easily extend the simulation by coupling it with any other physics.

You may already be familiar with the three different modules that can be used for simulating piezoelectric materials:

Each of these modules gives you a predefined *Piezoelectric Devices* interface that you can use for modeling systems that include both piezoelectric and other structural materials. The Acoustics Module offers two predefined interfaces, namely the *Acoustic-Piezoelectric Interaction, Frequency Domain* interface and the *Acoustic-Piezoelectric Interaction, Transient* interface. These two allow you to model how piezoelectric acoustic transducers interact with the fluid media surrounding them.

*The *Piezoelectric Devices* interface is available in the list of structural mechanics physics interfaces.*

*The *Acoustic-Piezoelectric Interaction, Frequency Domain *and the* Acoustic-Piezoelectric Interaction, Transient* interfaces are available in the list of acoustics physics interfaces.*

These predefined multiphysics interfaces couple the relevant physics governing equations via constitutive laws or boundary conditions. Thus, they offer a good starting point for setting up more complex multiphysics problems involving piezoelectric materials. The new piezoelectric interfaces in COMSOL Multiphysics version 5.0 provide a transparent workflow to visualize the constituent physics interfaces. There is also a separate Multiphysics node that lists how the constituent physics interfaces are connected to each other.

Let’s find out how these multiphysics interfaces are structured.

Upon selecting the *Piezoelectric Devices* multiphysics interface, you see the constituent physics: *Solid Mechanics* and *Electrostatics*. You also see the *Piezoelectric Effect* branch listed under the Multiphysics node, which controls the connection between *Solid Mechanics* and *Electrostatics*.

*Part of the model tree showing the physics interfaces and multiphysics couplings that appear upon selecting the* Piezoelectric Devices *interface.*

By default, all modeling domains are assumed to be made of piezoelectric material. If that is not the case, you can deselect the non-piezo structural domains from the branch *Solid Mechanics > Piezoelectric Material*. These domains then get automatically assigned to the *Solid Mechanics > Linear Elastic Material* branch. This process ensures that all parts of the geometry are marked as either piezoelectric or non-piezo structural materials and that nothing is accidentally left undefined.

If you are working with other material models that are available with the Nonlinear Structural Materials Module, such as hyperelasticity, you can add that as a branch under *Solid Mechanics* and assign the relevant parts of your modeling geometry to this branch. The Solid Mechanics node gives us full flexibility to set up a model that involves not only piezoelectric material but also linear and nonlinear structural materials. The best part is that if these materials are geometrically touching each other, the COMSOL software will automatically take care of displacement compatibility across them.

If some parts of the model are not solid at all, like an air gap, you can deselect them in the Solid Mechanics node.

From the Solid Mechanics node, you will also assign any sort of mechanical loads and constraints to the model.

The Electrostatics node allows you to group together all the information related to electrical inputs to the model. This would include, for example, any electrical boundary conditions such as voltage and charge sources. By default, any geometric domain that has been assigned to the *Solid Mechanics > Piezoelectric Material* branch also gets assigned to the *Electrostatics > Charge Conservation, Piezoelectric* branch. If you have any other dielectric materials in the model that are not piezoelectric, you could assign them to the *Electrostatics > Charge Conservation* branch.

The *Multiphysics > Piezoelectric Effect* branch ensures that the structural and electrostatics equations are solved in a coupled fashion within the domains that are assigned to the *Solid Mechanics > Piezoelectric Material* (and also the *Electrostatics > Charge Conservation, Piezoelectric*) branch.

The multiphysics coupling is implemented using the well-known coupled constitutive law for piezoelectric materials. Note that the *Electrostatics > Charge Conservation, Piezoelectric* branch is mainly used as a placeholder for assigning geometric domains that belong to the piezoelectric material model. This helps the *Multiphysics > Piezoelectric Effect* branch understand whether a domain assigned to the *Electrostatics* interface is piezoelectric or not.

Note: For an example of working with the

Piezoelectric Devicesinterface, check out the tutorial on modeling a Piezoelectric Shear Actuated Beam.

It is also possible to add effects of damping or other material losses in dynamic simulations. You can do so by adding one or more of the following subnodes under the *Solid Mechanics > Piezoelectric Material* branch:

*Damping and losses that can be added to a piezoelectric material.*

Subnode Name | When to Use the Subnode |
---|---|

Mechanical Damping | Allows you to add purely structural damping. Choose between using Loss Factor (in frequency domain) or Rayleigh damping (for both frequency and time domains) models. |

Coupling Loss | Allows you to add electromechanical coupling loss. Choose between using Loss Factor (for frequency domain) or Rayleigh damping (for both frequency and time domains) models. |

Dielectric Loss | Allows you to add dielectric or polarization loss. Choose between using Loss Factor (for frequency domain) and Dispersion (for both frequency and time domains) models. |

Conduction Loss (Time-Harmonic) | Allows you to add electrical energy dissipation due to electrical resistance in a harmonically vibrating piezoelectric material (for frequency domain only). |

Note: For an example of adding damping to piezoelectric models, check out the tutorial on modeling a Thin Film BAW Composite Resonator.

Additional damping also takes place due to the interaction between a piezoelectric device and its surroundings. This can be modeled in greater details using the Acoustic-Piezoelectric Interaction interfaces.

Upon selecting one of the Acoustic-Piezoelectric Interaction interfaces, you see the constituent physics: *Pressure Acoustics*, *Solid Mechanics* and *Electrostatics*. You also see the *Acoustic-Structure Boundary* and *Piezoelectric Effect* branches listed under the Multiphysics node.

*Part of the model tree showing the physics interfaces and multiphysics couplings that appear when selecting the *Acoustic-Piezoelectric Interaction, Frequency Domain* and the* Acoustic-Piezoelectric Interaction, Transient* interfaces.*

By default, all modeling domains are assigned to the *Pressure Acoustics* interface as well as the *Solid Mechanics > Piezoelectric Material* and* Electrostatics > Charge Conservation, Piezoelectric* branches. Note that the *Pressure Acoustics* interface is designed to simulate acoustic waves propagating in fluid media.

Since COMSOL Multiphysics cannot know a *priori* which parts of the modeling geometry belong to the fluid domain and which ones are solids, you are expected to provide that information by deselecting the solid domains from the *Pressure Acoustics, Frequency Domain* (or *Pressure Acoustics, Transient*) branch and deselecting the fluid domains from the *Solid Mechanics* and *Electrostatics* branches.

Once you do that, the boundaries at the interface between the solid and fluid domains are detected and assigned to the *Multiphysics > Acoustic-Structure Boundary* branch. This branch controls the coupling between the *Pressure Acoustics* and *Solid Mechanics* physics interfaces. It does so by considering the acoustic pressure of the fluid to be acting as a mechanical load on the solid surfaces, while the component of the acceleration vector that is normal (perpendicular) to the same surfaces acts as a sound source that produces pressure waves in the fluid.

Note: For an example of Acoustic-Piezoelectric Interaction, check out the tutorial on modeling a Tonpilz Transducer.

The transparency in the workflow as discussed above also paves the way for adding more physics and creating your own multiphysics couplings.

For example, let’s say there is some heat source within your piezoelectric device that produces nonuniform temperature distribution within the device. In order to model this, you can add another physics interface called *Heat Transfer in Solids* in the model tree and prescribe appropriate heat sources and sinks to find out the temperature profile. You could then add a *Thermal Expansion* branch under the Multiphysics node to compute additional strains in different parts of the device as a result of the temperature variation.

The *Multiphysics > Thermal Expansion* branch couples the *Heat Transfer in Solids* and the *Solid Mechanics* interfaces. It might also be possible that the piezoelectric material properties have a temperature dependency. You could represent these properties as functions of temperature and let the *Multiphysics > Temperature Coupling* branch pass on the information related to temperature distribution in the modeling geometry to the *Solid Mechanics* or even the *Electrostatics* branches, thereby producing additional multiphysics couplings.

*Part of the model tree showing the physics interfaces and multiphysics couplings that you can use to combine piezoelectric modeling with thermal expansion and temperature-dependent material properties.*

Similar to adding more physics and multiphysics couplings, it is also possible to disable one or more multiphysics couplings — or even any of the physics interfaces shown in the model tree. This could be immensely helpful for debugging large and complex models.

*The model tree on the left shows a scenario where the Piezoelectric Effect multiphysics coupling is disabled. The model tree on the right shows a scenario where the* Electrostatics* physics interface is disabled.*

For example, you can disable the *Multiphysics > Piezoelectric Effect* branch and solve for the *Solid Mechanics* and *Electrostatics* physics interfaces in an uncoupled sense. You could also solve a model by disabling either the *Solid Mechanics* or the *Electrostatics* interface.

Running such case studies could help in evaluating how the device would respond to certain inputs if there were no piezoelectric material in place. This approach could also be used to evaluate equivalent structural stiffness or equivalent capacitance of the piezoelectric material.

You could also start by adding only one of the constituent physics, say *Solid Mechanics*, and after performing some initial structural analysis, go ahead and add the *Electrostatics* physics interface to the model tree once you are ready to add the effect of a piezoelectric material.

In that case, when you add the *Electrostatics* physics on top of the existing *Solid Mechanics* physics in the model tree, the COMSOL software will automatically add the Multiphysics node. From there, you can manually add the *Piezoelectric Effect* branch. Note that if you take this approach of adding the constituent physics interfaces and multiphysics effect manually, you would also have to manually add the piezoelectric modeling domains to the *Solid Mechanics > Piezoelectric Material*, the *Electrostatics > Charge Conservation, Piezoelectric*, and the *Multiphysics > Piezoelectric Effect* branches.

In a similar fashion, you can continue to add more physics interfaces and multiphysics couplings to your model based on your needs.

To learn more about modeling piezoelectric devices in the COMSOL software environment, you are encouraged to refer to these resources:

- Piezoelectric Features Overview
- Acoustics Module User’s Guide
- MEMS Module User’s Guide
- Structural Mechanics Module User’s Guide

To begin, I would like to highlight several changes in the Linear Elastic Material model of the *Membrane* interface.

First off, the previous version of the interface always assumed geometric nonlinearity. The new version listens to the “Include geometric nonlinearity” setting in the study step settings in the same way as the *Solid Mechanics* interface. The geometric linear version of the membrane can be used when it is acting as cladding on a solid surface. If the membrane is used by itself and not as a cladding, a tensile prestress is, as before, necessary in order to avoid singularity. This is because a membrane without stress or with a compressive stress has no transverse stiffness. To include the prestress effect, you must enable geometric nonlinearity for the study step.

Another update is that linear elastic materials can now also be orthotropic or anisotropic. This affects the settings of the Damping subnode as well, where non-isotropic loss factors are now allowed.

You may also notice that we have added a Hygroscopic Swelling feature as a subnode to the Linear Elastic Material node. (We described the hygroscopic swelling effect in a previous blog post. Check that out to learn more about the effect.)

All of you who use the Nonlinear Structural Materials Module may now use the *Membrane* interface to model thin hyperelastic structures by adding a Hyperelastic Material node. In order to illustrate the Hyperelastic Material model using the *Membrane* interface, we have recreated the Model Library example Inflation of a Spherical Rubber Balloon.

Tip: You can download the new version of the model in the Model Gallery by logging into your COMSOL Access account.

The *Membrane* interface works on the plane stress assumption, and it is assumed that there is no variation across the thickness of the balloon. Also, it requires a prestress to solve the model due to the absence of bending stiffness in the membrane. For this purpose, a separate study has been created before the inflation of the balloon is carried out in further studies. Results from this analysis are used as initial values for the rest of the inflation analyses. Aside from these two changes, the model is similar to the previous Solid Mechanics version.

The advantage of the Membrane version is that it is more computationally efficient. Why is that? Because the *Membrane* interface is on one geometric entity lower than the *Solid Mechanics* interface. The results obtained from the *Membrane* interface are in agreement with the analytical results. The plot below shows the inflation pressure as a function of circumferential stretch for different hyperelastic material models compared to the analytical expression for the Ogden model.

As the internal pressure increases, the balloon starts to inflate and its thickness decreases. Since the pressure is uniform over the surface, the thickness is the same along the cross section for any given inflation pressure. The next plot compares the variation of deformed thickness with applied stretch to the balloon obtained from the *Membrane* interface and the *Solid Mechanics* interface. We see that the thinning of the balloon is accurately captured by the *Membrane* interface.

We have added four new feature nodes to the *Membrane* interface.

They are as follows:

*Prescribed Velocity*— Available at the domain and boundary level*Prescribed Acceleration*— Available at the domain and boundary level*Symmetry*and*Antisymmetry*— Both available at the boundary levels

In addition to the specific improvements I just went over, we have made a few general changes to the structural mechanics interfaces that affect the *Membrane* interface. You will notice that the menus have been restructured for a number of structural mechanics interfaces.

The following interfaces now have restructured menus:

*Solid Mechanics**Shell**Plate**Membrane**Beam**Truss*

You can see a screenshot of the menu structure for the *2D Axisymmetric Membrane* interface below:

As for the Spring Foundation features, we have generalized these so that you can enter the “spring force versus displacement” and the “damping force versus velocity” relations in matrix form, rather than by component.

For 2D Axisymmetric cases, there is a new load type called “Point Load (on Axis)”. With this option, it is now possible to apply loads on a point on a symmetry axis.

For 2D Axisymmetric cases, a Point Load is actually a line load (N/m) since a point represents a ring in axisymmetry. To follow better naming conventions, such a load is now called “Ring Load” in both the *Solid Mechanics* interface and the *Membrane* interface.

Models that were made with COMSOL Multiphysics version 4.4 or earlier still use the old *Membrane* interface and new functionality is not available. To utilize the new functionality for old models, we suggest that you add a new *Membrane* interface and copy all the nodes from the previous interface to the new one.

As always, do not hesitate to contact us if you have any questions.

]]>