# Linear Steady-State Heat Transfer Analysis

Heat transfer analysis solves for unknown temperatures and fluxes under thermal loading.

Temperature represents the amount of thermal energy available, and fluxes represent the flow of thermal energy.

Conduction deals with thermal energy exchange by molecular motion. Free convection deals with thermal energy exchange between solids and surrounding fluids. Thermal loading is defined as energy flows into and out of the system.

In linear steady-state analysis, material properties such as conductivity and convection coefficient are linear. Temperature and fluxes at the final thermal equilibrium state are of interest. The basic finite element equation is:

- ${K}_{C}$
- Conductivity matrix
- $H$
- Boundary convection matrix due to free convection
- $T$
- An unknown nodal temperature
- $f$
- Thermal loading vector

Thermal load vector can be expressed as:

- ${f}_{B}$
- Power due to heat flux at boundary specified by QBDY1 card
- ${f}_{H}$
- Boundary convection vector due to convection specified by CONV or CONVG entries
- ${f}_{Q}$
- Power vector due to internal heat generation specified by QVOL card.

The matrix on the left hand side of Equation 1 is singular unless temperature boundary conditions are specified. The equilibrium equation is solved simultaneously for the unknown temperatures, using a Gauss elimination method that exploits the sparseness and symmetry for computational efficiency. Once the unknown temperatures at the nodal points of the elements are calculated, temperature gradient $\nabla T$ can be calculated according to element shape functions. Element fluxes can be calculated by using:

Heat Transfer | Structural | |
---|---|---|

Unknown | Temperature | Displacement |

Temperature gradient | Strain | |

Flux | Stress | |

${K}_{C}$ | Conductivity matrix | Stiffness matrix |

$H$ | Boundary convection matrix | Elastic foundation stiffness matrix |

$f$ | Thermal loading vector | Load vector |

${Q}_{Vol}$ | Element volumetric | Gravity load |

The thermal loads and boundary conditions are defined in the Bulk Data section of the input deck. They need to be referenced in the Subcase Information Entry section using an SPC or MPC and LOAD statement in a SUBCASE.

Forced Convection is available for Linear Steady-State Heat Transfer via Darcy Flow Analysis and 1D Forced Convection Analysis via CAFLUID.

## Input Data for Thermal Structural Analysis

Both GRID and SPOINT can be used to specify a thermal point.

Fixed temperatures are specified with SPC, SPC1,
and SPCD data with the component ID blank or zero.
MPC data can be used to specify the relationship between
temperatures of different points using component ID blank or zero. If you want to use
component ID 1, then `SPSYNTAX`=mixed must be
specified in the input deck. Rigid elements are ignored in heat transfer analysis.

Elements that generate heat are listed in QVOL data. The heat generated by an element is equal to the element volume * QVOL * HGEN, where HGEN is a scale factor (default=1.0) listed on the material (MAT4 or MAT5) data.

Heat flux load QBDY1 and convective heat transfer CONV are applied to the structure through surfaces identified by the CHBDYE card. The CHBDYE elements associate heat exchange surfaces with conduction elements. A 1D element can have heat flux applied at each end and along its length. A 2D element can have heat flux on its surface and along any edge. A 3D element can have head flux applied on any face.

Fixed values of heat flux are specified using the QBDY1 card. This data lists the CHBDYE element ID and the heat flux value (Q0). The power exchanged through a CHBDYE element is equal to Q0 multiplied by the effective area of the CHBDYE element. For a 1D element, the area at the end is the cross-sectional area of the element. For flux into the side of a 1D element, the effective area is the length times the circumference of the element which is calculated from the cross-sectional area, assuming that the cross-section is circular. For 2D elements, the effective area for the surface of the element is its area and the effective area of a side is equal to the length of the side multiplied by the thickness of the element. For 3D elements, the effective area is just the area of the face.

Free convection heat flux is specified for CHBDYE elements using the CONV data which lists the CHBDYE element ID, the ambient temperature (TAMB), and the ID of the PCONV data which lists the MAT4 material ID. The MAT4 data contains the convection coefficient H. The heat flux per unit area from convection is H*(T-TAMB), where $T$ is the grid temperature. Automatic free convection definition can be activated via CONVG Bulk/Subcase pair.

- Shell elements are considered to be membranes in Heat Transfer Analysis. Composite properties are homogenized (1 degree of freedom per grid). The temperature distribution through the thickness of shell elements is not calculated. Only nodal temperature is determined.
- Flux for composite plate or shell elements are calculated with homogenized conductivity of the entire element.

## Thermal Analysis Results

Output for Linear Steady-State Heat Transfer Analysis typically consists of grid temperature (THERMAL entry), temperature gradient and heat flux (FLUX entry) in the elements.

Power at SPC grids (SPCFORCE entry) are also calculated, which is a measure of power flowing in and out of the system. Heat flow results are available through the RESULTANT and SECTION entries.

## Coupled Thermal Structural Analysis and Optimization

Each heat transfer SUBCASE defines a temperature set, which can be referred by a structural SUBCASE by TEMP(LOAD) to perform thermal-structural analysis.

The temperature set identification is the same as heat transfer SUBCASE identification by default. It can be changed by using TSTRU card. If the temperature set identification is the same as a Bulk Data temperature set identification, the temperatures from heat transfer analysis override Bulk Data temperatures.

Coupled Thermal Structural Analysis is done in the following fashion. Heat transfer analysis is performed first to determine the temperature field of the structure. The temperature field is used as part of the loading for structural analysis and/or update temperature dependent structural material properties. A single finite element mesh is usually used for both thermal and structural analysis. The finite element governing equation for static structural analysis is:

Where, $K$ is the global stiffness matrix, $u$ is the unknown displacement vector, ${f}_{T}$ is the temperature loading, and $f$ is the structural loading such as forces, pressures, and so forth. Displacement vector $u$ is solved by the linear equation solver.

In coupled thermal structural optimization, ${f}_{T}$ sensitivities due to design changes are calculated. Besides the usual responses such as displacement, stress, mass, and so on. Temperature can also be a response in optimization.

The coupling in thermal structural analysis is sequential, that is, the thermal analysis affects the subsequent structural analysis. On the other hand, in coupled thermal structural optimization, the coupling works both ways, that is the thermal influence on structural and the structural influence on thermal. In other words, the optimizer modifies the structural design to satisfy constraints, which in turn affects the thermal analysis.

Temperature responses are supported in Sizing, Shape, Topography, and Topology Optimization, but the CHBDYE element cannot be used in the Design Domain of Topology Optimization.