You can use surface-to-surface contact elements and the node-to-surface contact element, in combination with thermal-structural coupled field solid elements or thermal elements, to model heat transfer that occurs in the contact surface. To activate both the structural and thermal DOFs, set KEYOPT(1) = 1. To activate the thermal DOF only, set KEYOPT(1) = 2.
The following thermal contact features are supported.
Thermal contact conduction between two contacting surfaces.
Heat convection from a “free surface” to the environment or between two open surfaces separated by small gap (“near field” convection).
Heat radiation from a “free surface” to the environment or between two open surfaces separated by a small gap (“near field” radiation).
Heat generation due to frictional dissipation.
Heat flux input.
When KEYOPT(1) is set to 2 (thermal DOF only), ANSYS ignores heat generation due to friction.
Each contact pair can cover one or more thermal contact features. Which feature is active depends on the contact status:
If you wish to model free surface convection, free surface radiation, or a surface with a supplied heat flux value, you can define a “free” thermal surface. A free thermal surface can be a contact surface with no associated target (that is, the contact pair lacks target elements). You can also set KEYOPT(3) = 1 of the target element type definition to define a free thermal surface. When this KEYOPT is set, both free surface radiation and convection are considered as long as open contact is detected. In this case, there is no convective and radiative heat transfer between the contact and target surfaces.
For interface heat conduction, near field convection, or near field radiation, a temperature for both the contact and target surfaces is required. For a general target surface, the temperature varies along the surface (see figure below). In this case, the temperature at the intersection between the target surface and the normal from the contact detection point represents the target temperature. For a rigid target, the temperature on the pilot node represents the entire rigid target surface temperature, if the pilot node exists.
To take into account the conductive heat transfer between contact and target surfaces, you need to specify the thermal contact conductance coefficient which is real constant TCC.
The conductive heat transfer between two contacting surfaces is defined by
q = TCC X (Tt -Tc)
The TCC value is input through a real constant, which can be made a function of temperature [(Tc + Tt)/2], pressure, time, and location by using the %TABLE% option. TCC has units of heat/(time x area x temp). If contact occurs, a small value of TCC yields a measure amount of imperfect contact and a temperature discontinuity across the interface. For large values of TCC, the resulting temperature discontinuity tends to vanish and perfect thermal contact is approached. When not in contact, however, it is assumed that no heat is transferred across the interface. To model contact conduction between two surfaces where a small gap exists, use KEYOPT(12) = 4 or 5 to define either the “bonded contact” or “no-separation contact” options (see Selecting Surface Interaction Models).
You can take advantage of the fast thermal transient solver option (THOPT,QUASI) in the contact analysis. (See Nonlinear Options in the Thermal Analysis Guide for more information on this solver option.) To do so, you must use the following contact element key options:
|KEYOPT(1) = 2 - Temperature DOF only|
|KEYOPT(12) = 5 or 6 - Bonded always or bonded initial|
The following solver options must also be set:
The following two cases are supported:
Thermal conductivity at contact. The only real constant used is TCC, which can be a function of time and temperature.
Perfect thermal contact which supports dissimilar meshes on both sides of the contacting interface (TCC = infinity). This case requires the internal MPC approach (KEYOPT(2) = 2) and contact nodal detections (KEYOPT(4) = 1 or 2) or CONTA175.
To model convective heat transfer, you must specify the heat convection coefficient CONV using the SFE command (with KVAL = 1 and CONV as a table parameter). CONV can be a constant value (only uniform is allowed) or a function of temperature, time, or location as specified through tabular input. For free surface convection (see Thermal Contact Behavior vs. Contact Status for a definition of “free-surface contact”), you must also specify bulk temperature through the SFE command (with KVAL = 2 and CONV as a table parameter). You can access this command through the following GUI paths:
|Main Menu> Preprocessor> Loads> Define Loads> Apply> Thermal> Convection> On Elements> Uniform|
|Main Menu> Solution> Define Loads> Apply> Thermal> Convection> On Elements> Uniform|
The SFE surface load must be applied to the contact elements only. If either the convection coefficient or bulk temperature is not specified, the convection loading will not be active.
To model radiative heat transfer, specify the following:
Emissivity value EMIS, specified through the material property definition.
Stefan-Boltzmann constant SBCT through a real constant.
Offset temperature TOFFST. If you define your data in terms of degrees Fahrenheit or degrees Celsius, you must specify a temperature offset using the TOFFST command. You can access this command through the following GUI paths:
|Main Menu> Preprocessor> Loads> Analysis Type> Analysis Options|
|Main Menu> Preprocessor> Material Props|
Radiation view factor RDVF, specified through a real constant (defaults to 1).
Environment (ambient) temperature. It is only used for modeling radiation between a portion of the contact surface to the environment when the contact status is “free-surface contact” (see Thermal Contact Behavior vs. Contact Status). The temperature is only applied on the contact elements and is input on the SFE command with KVAL = 2 and CONV as a table parameter (this is the same as the bulk temperature in free surface convection modeling). If the environment temperature is not specified through the SFE command, the free surface radiation loading will not be active.
When contact is open, heat transfer through radiation can occur. The equation is defined by
q = RDVF x EMIS x SBCT [(Te + TOFFST)4 - (Tc + TOFFST)4]
For “near-field” radiation, when an intersection from a contact detection point to the target surface (in the direction of normal to the contact point) is detected, and the gap distance is smaller than the pinball radius, Te is the target temperature at the intersection. The radiation modeling here assumes that the radiative heat transfer occurs in the direction of the normal between two surfaces with a small gap. By defining RDVF as a function of gap, you can account for geometry effects. Use the Radiosity Solver method for more generalized radiation problems (see the Thermal Analysis Guide for more information).
For “free-surface contact” radiation, Te becomes the “ambient” temperature defined by “bulk temperature” input on the SFE command (with KVAL = 2 and CONV as the table). For a definition of free-surface contact, see Thermal Contact Behavior vs. Contact Status.
In order to model heat generation due to frictional dissipated energy, you should perform a coupled transient thermal-structural analysis. If you wish you can turn off transient effects on structural DOFs by using TIMINT,STRUC,OFF. However, you must include transient effects on the thermal DOF. Two real constants are required:
FHTG is the frictional dissipated energy converted into heat.
FWGT is the weight factor for the distribution of heat between contact and target surfaces.
In the coupled thermal-structural contact modeling, the rate of frictional dissipation is given by
q = FHTG x τ x V
The amount of frictional dissipation on contact and target surfaces is defined by
qc = FWGT x FHTG x τ x V
qT = (1 - FWGT) x FHTG x τ x V
Where qc is the contact side and qT is the target side, and FWGT is the weight factor for the distribution of heat between the contact and target surfaces (input as a real constant). By default, FWGT = 0.5. For an input of true 0, you must enter a very small value (for example, 1E-8). If you enter 0, ANSYS interprets this as an input of the default value.
You can apply heat flux on the contact elements through the SFE command. Only uniform flux can be applied. Heat flux cannot be applied on target elements. However, for near field contact, the external flux is applied on contact and will contribute to target elements.
For a free thermal surface, if KEYOPT(3) of the target element is set to 1, the external flux is only applied on the contact side. On a given contact element either CONV or HFLUX (but not both) may be specified. However, you can define two different contact pairs: one models convection and the other models heat flux.