Skip to content

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>
                <bcsAndLoads>
                   <temperature name="L_top" value="30"/>
                   <temperature name="L_bottom" value="20"/>
                </bcsAndLoads>
                ....               
            </heatConduction>
        </pdeList>
    </sequenceStep>

    <sequenceStep index="2">
        <analysis>
            <static/>
        </analysis>
        <pdeList>
            <mechanic subType="planeStress">
                <regionList>
                    <region name="S_beam"/>
                </regionList>
                <bcsAndLoads>
                    <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>
                </bcsAndLoads>
                ....
            </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>    
     ...
 </bcsAndLoads>                

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>