Heat sink

Here we perfom the computation of the temperature field and the occuring mechanical deformation of a CPU heat sink.

Thermal boundary conditions are given as follows:

• $\Gamma_s$: set heat flux to $216666.67\, W/m^2$
• $\Gamma_i$: set to thermal isolation
• $\Gamma_r$: radiation with $h=70$W/m and $T_{\rm r}=20^\circ$C

and for the computation of the mechanical deformation we apply full support on $\Gamma_s$, meaning to set the displacement $\mathbf{u}$ to zero on this surface.

The geometry is already provided by a STL-file, which can be directly imported in trelis via the command import. All files for this example can be downloaded here.

Meshing

To obtain a highly qualitative mesh, we use the SubMap algorithm in trelis.

With the commands block and nodeset we define our computational volume and the surfaces at which we describe the boundary conditions. The complete journal file heatsink.jou includes the reading of the STL-file, the meshing and exporting as an ANSYS-cdb file. After the cdb-file is written to disc, you can convert it to the standard cfs-file with the convert_mesh.xml and executing

cfs -p convert_mesh.xml -g heatsink

---

XML Simulation Setup

The ready-to-use xml file is provided here as well as the material xml file.

Here, we will just discuss the main parts of the XML description file.

• Input: we use a scaling of $10^{-3}$ to get the coordinates in meter.

    <input>
        <hdf5 fileName="heatsink.cfs" scaleFac="1e-3"/>
    </input>
  

• Domain: we just need to perform the simulation for the aluminium block

    <domain geometryType="3d">
        <regionList>
            <region name="V_alu" material="alu"/>
        </regionList>
    </domain>
  

• The first sequece is a static analysis to obtain the temperture field

    <sequenceStep index="1">
        <analysis>
            <static/>
        </analysis>
        <pdeList>
            <heatConduction>
                <regionList>
                    <region name="V_alu" polyId="lagrange"/>
                </regionList>
                <bcsAndLoads>
                    <heatFlux name="S_source" value="216666.67"/>                    
                    <heatTransport name="S_radiation" volumeRegion="V_alu" bulkTemperature="20" heatTransferCoefficient="75"/>
                </bcsAndLoads>
                .....
              </heatConduction>
          </pdeList>
      </sequenceStep>
  

• The second sequence step performs the computation of the mechanical deformation

      <sequenceStep index="2">
      <analysis>
          <static/>
      </analysis>
  
          <pdeList>
              <mechanic subType="3d">
                 <regionList>
                     <region name="V_alu" polyId="lagrange"/>
                 </regionList>
                 <bcsAndLoads>
                    <thermalStrain name="V_alu">
                        <sequenceStep index="1">
                            <quantity name="heatTemperature" pdeName="heatConduction"/>
                            <timeFreqMapping>
                                <constant/>
                            </timeFreqMapping>
                        </sequenceStep>
                    </thermalStrain>
                    <fix name="S_source">
                        <comp dof="x"/>
                        <comp dof="y"/>
                        <comp dof="z"/>
                     </fix>
                 </bcsAndLoads>
  
                 <storeResults>
                  ....
               </mechanic>
          </pdeList>    
      </sequenceStep>
  

Perform the openCFS simulation by executing

cfs heatMechSink

---

Result

You can now investigate the results in paraview

• Temperature distribution

• Mechanial displacement on deformed structure