Solving for Solid Temperature

In solid-only simulations, the Finite Element Solid Energy model calculates the temperature distribution in the solid or solid shell region based on the thermal settings that you specify at the boundaries. In Conjugate Heat Transfer (CHT) simulations, this model also accounts for the thermal data coming from the fluid at the fluid-structure interface. The simulation can be combined with the Solid Stress model. In this case the thermal loads from the temperature distribution are incorporated when solving for the solid displacement.

When setting up a solid temperature simulation there are 4 different scenarios that can be modelled:
  • Temperature only - requires a solid region and Finite Element Solid Energy model only.
  • Temperature and Stress - requires only a solid region with both the Finite Element Solid Energy and Solid Stress model.
  • Pure CHT - requires both solid and fluid regions with interface as well as the Finite Element Solid Energy model.
  • CHT and FSI - requires both solid and fluid regions with interface and both the Finite Element Solid Energy and Solid Stress models.

The Finite Element Solid Energy and Solid Stress models use the same mesh. See Mesh Requirements and Guidelines.

The following instructions outline the basic workflow for modeling heat conduction in solid materials and shell parts. For more information on modeling heat transfer between a fluid and a solid, see Conjugate Heat Transfer.
  1. Define the required regions, interfaces, and continua.
    In Conjugate Heat Transfer (CHT) simulations, define the fluid and solid regions and create a contact-mode interface between the fluid and the solid. Set the interface Type to Mapped Contact Interface.
  2. Follow the instructions in Applying Thermal Loads, choosing the Finite Element Solid Energy model.
Define the material properties that are required to model heat conduction and convection:
  1. Expand the relevant [Physics Continuum] > Models > Solid > [Solid Material] > Material Properties node.
  2. Specify the solid Density and Specific Heat using a constant input.
  3. Specify the Thermal Conductivity of the solid material:
    • For isotropic solids, define the thermal conductivity as a scalar using either a constant value, scalar expression, or field function.
    • For anisotropic solids, define the thermal conductivity as a tensor.
    For more information on the available methods, see Material Properties.
  4. Select the [Physics Continuum] > Initial Conditions > Static Temperature node and initialize the solid temperature to the appropriate value.
    In CHT simulations, setting accurate initial conditions can have a large impact on convergence.
Define the thermal behavior at the solid boundaries. For boundaries that are not part of a fluid-solid interface:
  1. Select the [Solid Region] > Boundaries > [Wall Boundary] > Physics Conditions > Thermal Specification node.
    • For thermally isolated boundaries, which prevent energy transfer, set Method to Adiabatic.
    • For non-adiabatic boundaries, which allow for energy transfer, choose the Method based on the quantity that you want to specify. The Finite Element Solid Energy allows for specification of temperature, heat flux, and convective flux.
    For more information, see Finite Element Solid Energy Model Reference.
At the interface between a fluid and a solid, the fluid boundary receives the solid temperature, whereas the solid boundary receives the convective flux from the fluid boundary. Simcenter STAR-CCM+ automatically sets the thermal specification of the boundaries at the two sides of the interface to match the fields that are mapped to the two boundaries. See Interface Inputs.

For both the fluid and the solid interface boundaries:

  1. Select the [Region] > Boundaries > [Interface Boundary] > Physics Conditions > Time Averaging Option node and set this option to specify whether the field computed at the boundary is time-averaged before it is mapped to the other side of the interface.
    For more information, see Time Averaging Option
When you create a mapped contact interface between a fluid region and a solid region for which the solid stress model is active, Simcenter STAR-CCM+ automatically activates the fluid structure coupling solver. If you wish to run the simulation as a CHT simulation without fluid structure coupling then you must decouple the fluid load from the solid region.
  1. To run a CHT simulation without fluid structure coupling, select [Solid Region] > Boundaries > [Interface Boundary] > Physics Conditions > FSI Coupling Specification node and set Option to Uncoupled.
To account for energy contributions coming from phenomena that are not modeled in the simulation, you can apply a user-defined energy source on the solid region:
  1. Select the [Solid Region] > Physics Conditions > Energy Source Option and set Method as required.
    For more information on the available options, see Region Inputs.
For solid-solid interfaces, select the method that Simcenter STAR-CCM+ uses for constraining the surfaces:
  1. Select the [Solid/Solid Interface] > Physics Conditions > Constraint Mapping node and set Method to either Node to Surface or Surface to Surface.
    In general, the Surface to Surface method is more accurate, but it requires higher computational effort. For more information, see Interface Settings.
  2. Select the Solvers > Finite Element Solid Energy node and, if required, adjust the solver properties (see Finite Element Solid Energy Solver).
    By default, Simcenter STAR-CCM+ solves for the solid temperature using a direct solver which, for large cases, can have large memory and time requirements. To compute the solution of the linear system using an iterative approach, set Solver Method to Iterative. For more information on the available settings, see FE Sparse Direct Solver Reference and FE Iterative Solver Reference.
In unsteady simulations, high temperature gradients at boundaries can lead to local oscillations in the temperature solution. In this case, you can either refine the mesh or increase the time-step. From 1D heat conduction, it is possible to estimate the minimum time-step required for unsteady thermal analyses as:
图 1. EQUATION_DISPLAY
Δt>ρcp6κh
(342)

where ρ is the density, cp is the specific heat, κ is the thermal conductivity, and h is the element length.

  1. Set a time-step that is higher than the value given by Eqn. (342).
Simcenter STAR-CCM+ also provides lumping techniques for the heat capacity matrix that you can apply in regions with linear (first-order) mesh elements. Lumping is recommended in regions where the relationship between the thermal diffusivity α , the average mesh element size Δ x , and the simulation time-step Δ t follows Eqn. (348). To activate lumping:
  1. Select the [Solid Region] > Physics Conditions > Lumped Heat Capacity Matrix Option and set Method to Lump 1st-order elements.
    For more information, see Region Inputs.
  2. Complete the simulation setup by following the instructions provided in the following sections.