# Mechanic PDE

## Governing Equations

The governing equation can easily be derived from the conservation equation for the momentum density ($\rho \dot{\mathbf{u}}$). Assuming that the force density $\mathbf{f}$ can be represented as $\mathbf{f} = \nabla \cdot \mathbf{\sigma} + \mathbf{g}$, we obtain \begin{equation} \frac{\partial^2 \rho \mathbf{u}}{\partial t^2} - \nabla \cdot \mathbf{\sigma} = \mathbf{g}, \end{equation} where $\rho$ denotes the density, $\mathbf{u}$ the displacement, $\mathbf{\sigma}$ the stress tensor (rank 2) and $\mathbf{g}$ the force density. It has to be noted that $\mathbf{f}$ is a body force density which is exerted from the outside. We assume linear, elastic material behaviour which may be anisotropic and express it via Hooks Law which is given by \begin{equation} \mathbf{\sigma} = \mathbf{C} : \mathbf{s}, \end{equation} where $\mathbf{C}$ denotes the stiffness tensor (rank 4) and $\mathbf{s}$ the strain tensor (rank 2). Furthermore, we assume small strains in order to use the linearized strain displacement relationship given as \begin{equation} \mathbf{s} = \frac{1}{2} ( \mathbf{u} + \mathbf{u}^{\textrm{T}}). \end{equation} Multiplying (1) with a the test function $\mathbf{u}^\prime$ and inserting (2) and (3) finally leads to the weak form of the PDE given by \begin{equation} \int_{\Omega} \mathbf{u}^\prime \cdot \rho \frac{\partial^2 \mathbf{u}}{\partial t^2} \mathrm{d}\Omega + \frac{1}{2} \int_{\Omega} (\nabla \mathbf{u}^\prime) : \mathbf{C} : \left( \nabla \mathbf{u} + (\nabla \mathbf{u})^{\textrm{T}} \right) \mathrm{d}\Omega - \int_{\Gamma} (\mathbf{u}^\prime \cdot \mathbf{\sigma}) \cdot \mathbf{n} \mathrm{d}\Gamma = \int_{\Omega} \mathbf{u}^\prime \cdot \mathbf{g} \, \mathrm{d}\Omega. \end{equation}

## Boundary conditions

The boundary conditions can be given as

\begin{equation} \mathbf{u}(t) = \mathbf{u}_{\textrm e}(t) \qquad \textrm{on } \Gamma_{\textrm e}, \end{equation}
\begin{equation} \mathbf{\sigma}(t)\cdot\mathbf{n} = \mathbf{\sigma}_{\textrm n}(t) \qquad \textrm{on } \Gamma_{\textrm n}, \end{equation}

with $\mathbf{u}_{\textrm e}$ as the Dirichlet (essential) BC-value, $\Gamma_{\textrm e}$ the essential boundary, $\mathbf{n}$ the normal vector on the Neumann (natural) boundary $\Gamma_{\textrm n}$ and $\mathbf{\sigma}_{\textrm n}$ the traction at the boundary. Please note that all surfaces that are not manually defined will automatically be free of traction. The boundary conditions can be defined in the xml-file within the <bcsAndLoads> tag.

        <bcsAndLoads>
<fix name="">
<comp dof=""/>
</fix>
<displacement name="">
<comp dof="" value=""/>
</displacement>
<pressure name="" value=""/>
<normalStiffness name="" volumeRegion="" value=""/>
<thermalStrain name="" value=""/>

• fix: Fixes the nodes of the given geometry where only the direction (e.g. "x", "y", "z") specified by the tag <comp dof =""> is locked. This allows to fix the geometry in one or more directions (homogeneous Dirichlet value $\mathbf{u} = \mathbf{0}$).
• displacement: Similar to <fix>, but instead of setting the value of the displacement to zero a certain value can be specified (inhomogeneous Dirichlet value $\mathbf{u} = \mathbf{u}_{\textrm e}$).
• pressure: Prescribes a value for a uniform pressure applied to a surface (inhomogeneous Neumann value $\mathbf{\sigma}\cdot\mathbf{n} = \mathbf{\sigma}_{\textrm n}$).
• normalStiffness: Prescribes a stiffness acting in normal direction to a surface.
• thermalStrain: Used to prescribe a thermal strain on a volume.

## Sources

Besides providing values for the boundary conditions the RHS can be used. For the mechanic PDE we can provide the given sources via the xml within the <bcsAndLoads> tag.

        <bcsAndLoads>
<force name="">
<comp dof="" value=""/>
</force>
<forceDensity name="">
<comp dof="" value=""/>
</forceDensity>

• force: Used to prescribe a force on a volume, where the direction is specified by the tag <comp dof =""> (e.g. "x", "y", "z").
• forceDensity: Similar to <force> but with a force-density instead of an absolute force.

## Material

In the general case the material used for the simulaiton is anisotropic which can be defined in the material-xml as

  <material name="material2">
<mechanical>
<density>
<linear>
<real> 1.0e+3 </real>
</linear>
</density>
<elasticity>
<linear>
<tensor dim1="6" dim2="6">
<real>
1.34615E+03 5.76923E+02 5.76923E+02 0.00000E+00 0.00000E+00 0.00000E+00
5.76923E+02 1.34615E+03 5.76923E+02 0.00000E+00 0.00000E+00 0.00000E+00
5.76923E+02 5.76923E+02 1.34615E+03 0.00000E+00 0.00000E+00 0.00000E+00
0.00000E+00 0.00000E+00 0.00000E+00 3.84615E+02 0.00000E+00 0.00000E+00
0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 3.84615E+02 0.00000E+00
0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 3.84615E+02
</real>
</tensor>
</linear>
</elasticity>
</mechanical>
</material>


For this example, all 21 individual components of the elasticity tensor can be defined. For a simpler case, e.g. an isotropic material, the definition of the elasticity reduces to

<elasticity>
<linear>
<isotropic>
<elasticityModulus>
<real> 3e7 </real>
</elasticityModulus>
<poissonNumber>
<real> 0.2 </real>
</poissonNumber>
</isotropic>
</linear>
</elasticity>


where the stiffness tensor is defined via

\begin{equation} \mathbf{C} = \begin{bmatrix} 2 \mu + \lambda & \lambda & \lambda & 0 & 0 & 0\\ \lambda & 2 \mu + \lambda & \lambda & 0 & 0 & 0\\ \lambda & \lambda & 2 \mu + \lambda & 0 & 0 & 0\\ 0 & 0 & 0 & \mu & 0 & 0\\ 0 & 0 & 0 & 0 & \mu & 0\\ 0 & 0 & 0 & 0 & 0 & \mu \end{bmatrix}. \end{equation}

Here, the Voigt notation as well as the definition for $\mu$ and $\lambda$ given by

\begin{equation} \mu = \frac{E}{2(1+\nu)} \end{equation}
\begin{equation} \lambda = \frac{E \nu}{(1+\nu)(1-2\nu)} \end{equation}

has been used. In these equations, $E$ enotes the elasticity modulus and $\nu$ the poisson ration.

## Analysis Types

Since in general we are dealing with a time-dependent PDE, we can distinguish three analysis types:

• Transient: $\frac{\partial }{\partial t}\neq 0$
    <analysis>
<transient>
<numSteps>10</numSteps>
<deltaT>0.1</deltaT>
</transient>
</analysis>

• Harmonic: $\partial / \partial t (\cdot) = j \omega (\cdot)$
<analysis>
<harmonic>
<numFreq>10</numFreq>
<startFreq>10</startFreq>
<stopFreq>3000</stopFreq>
<sampling>linear</sampling>
</harmonic>
</analysis>

• Eigenfrequency: $\partial / \partial t (\cdot) = j \omega (\cdot)$ and $RHS = 0$
    <analysis>
<eigenFrequency>
<numModes>5</numModes>
<freqShift>0</freqShift>
<writeModes>yes</writeModes>
</eigenFrequency>
</analysis>


## Postprocessing Results

#### Node Results

• Mechanic Displacement: Displacement vector for each node. (primary solution)
<nodeResult type="mechDisplacement">

• Mechanic Velocity: Velocity vector for each node. \begin{equation} \mathbf{v} = \frac{\partial \mathbf{u}}{\partial t} \end{equation}
<nodeResult type="mechVelocity">

• Mechanic Acceleration: Acceleration vector for each node. \begin{equation} \mathbf{a} = \frac{\partial^2 \mathbf{u}}{\partial t^2} \end{equation}
<nodeResult type="mechAcceleration">

• Mechanic RHS load: Right hand side source term in the FE formulation as nodal loads
<nodeResult type="mechAcceleration">


#### Element Results

• Mechanic Strain \begin{equation} \mathbf{s} = \frac{1}{2} ( \mathbf{u} + \mathbf{u}^{\textrm{T}}). \end{equation}
<elemResult type="mechStrain">

• Mechanic Stress \begin{equation} \mathbf{\sigma} = \mathbf{C} : \mathbf{s}, \end{equation}
<elemResult type="mechStress">

• Mechanic Kinetic Energy Density \begin{equation} e_\mathrm{kin} = \frac{1}{2} \rho \mathbf{v}^{\textrm{T}} \cdot \mathbf{v} \end{equation}
<elemResult type="mechKinEnergyDensity">

• Von Mises stress: Equivalent stress according to von Mises. \begin{equation} \sigma_\mathrm{v} = \sqrt{\frac{1}{2} \left( (\sigma_{11}-\sigma_{22})^2 + (\sigma_{22}-\sigma_{33})^2 + (\sigma_{33}-\sigma_{11})^2 \right) + 3 (\sigma_{12}^2 + \sigma_{23}^2 + \sigma_{31}^2)} \end{equation}
<elemResult type="vonMisesStress">


#### Region Results

• Mechanic Kinetic Energy \begin{equation} E_\mathrm{kin} = \int_{{\Omega}} e_\mathrm{kin} \, dV \end{equation}
<regionResult type="mechKinEnergy">

• Mechanic Deformation Energy \begin{equation} E_\mathrm{def} = \frac{1}{2} <u,Ku> \end{equation}
<regionResult type="mechKinEnergy">