# HeatMechPDE

## Heat conduction - mechanics coupling

This coupling is modelled as a pure forward coupling from a heat conduction simulation, e.g. performed in sequence step 1, to a computational mechanics using the temperature distribution and consider the thermal stress as a right hand side load.

### Coupling conditions

The thermal stain $\mathbf{s}_\mathrm{th}$ is model as

\begin{equation} \mathbf{s}_\mathrm{th} = \mathbf{\alpha}_\mathrm{th} \Delta T = \mathbf{\alpha}_\mathrm{th} \big( T - T_\mathrm{ref} \big) \end{equation}

with a given reference temperatur $T_\mathrm{ref}$ and the thermal expansion tensor of rank 2

\begin{equation} \mathbf{s}_\mathrm{th} = \left( \begin{array}{lll} \alpha_{11} & \alpha_{12} & \alpha_{13} \\ & \alpha_{22} & \alpha_{23} \\ \text{sym} & & \alpha_{33} \end{array} \right) \end{equation}

In doing so, the mechanical PDE for the displacement $\mathbf{u}$ changes to

\begin{equation} \rho \frac{\partial^2 \mathbf{u}}{\partial t^2} - \mathbf{\mathcal{B}}^T \mathbf{C} \mathbf{\mathcal{B}} \mathbf{u} = \mathbf{g} + \mathbf{\mathcal{B}}^T \mathbf{C} \mathbf{\alpha}_\mathrm{th} \end{equation}

### Analysis Types

Depending on the temporal setting, the coupled PDEs can be solved for the following analysis types:

• Static case ($\partial / \partial t = 0$)
<analysis>
<static>
</static>
</analysis>

• Transient case ($\partial / \partial t (\cdot) \neq 0$)
<analysis>
<transient>
<numSteps>100</numSteps>
<deltaT>1e-3</deltaT>
</transient>
</analysis>


### Single PDEs

As described, a typical application is the computation of a temperature distribution in sequence step 1 and then in step 2 the deformed mechanical structure, e.g

    <sequenceStep index="1">
<analysis>
<static/>
</analysis>
<pdeList>
<heatConduction>
<regionList>
<region name="S_beam"/>
</regionList>
<temperature name="L_top" value="30"/>
<temperature name="L_bottom" value="20"/>
....
</heatConduction>
</pdeList>
</sequenceStep>

<sequenceStep index="2">
<analysis>
<static/>
</analysis>
<pdeList>
<mechanic subType="planeStress">
<regionList>
<region name="S_beam"/>
</regionList>
<fix name="L_fix">
<comp dof="x"/>
<comp dof="y"/>
</fix>
<thermalStrain name="S_beam">
<sequenceStep index="1">
<quantity name="heatTemperature" pdeName="heatConduction"/>
<timeFreqMapping>
<constant step="1"/>
</timeFreqMapping>
</sequenceStep>
</thermalStrain>
....
</mechanic>
</pdeList>
</sequenceStep>


### Defining the coupling

• Coupling terms: Within the mechanical PDE we assume to have on the computational domain a temperature distribution, e.g. from a previous sequence step (see above), or which is provided by the input file and then is defined by
 <bcsAndLoads>
...
<thermalStrain name="Vol_bpsg_B1">
<grid>
<defaultGrid quantity="heatTemperature" dependtype="GENERAL" sequenceStep="2">
<globalFactor>1</globalFactor>
</defaultGrid>
</grid>
</thermalStrain>
...


### Material and postprocessing results

The thermal expansion tensor of rank 2 is defined within the material file, e.g. for an isotropic material as follows

<material name="alu">
<mechanical>
<density>2700.0</density>
...

<thermalExpanison>
<isotropic>
<real>22e-6</real>
</isotropic>
<refTemperature>
<real>25</real>
</refTemperature>
</thermalExpanison>
...
</mechanical>


Additional posprocessing results available for the mechaical PFE are defined in <storeResults>

          <storeResults>
...
<elemResult type="mechThermalStress">
<allRegions/>
</elemResult>
<elemResult type="mechThermalStrain">
<allRegions/>
</elemResult>
...
</storeResults>