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.
Note: When KEYOPT(1) is set to 2 (thermal DOF only), the program 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. Otherwise, the rigid surface temperature equals a uniform temperature specified via the TUNIF or BFUNIF command.
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 of the contact element.
The conductive heat transfer between two contacting surfaces is defined by
where
 = heat flux per unit area |
 = thermal contact conductance coefficient, having
units of heat/(time * temperature) for force-based node-to-surface
contact, or units of heat/(time * temperature * area) for the
traction-based model |
 and  = temperatures of the contact points on the target and
contact surfaces. |
The TCC value is input through a real constant, which can be made a function
of temperature (
), pressure (positive PRESSURE index values indicate
compression, negative PRESSURE index values indicate tension), geometric
penetration (positive GAP index values indicate penetration, negative GAP index
values indicate an open gap), time, and initial contact detection point location
(at the beginning of solution) by using tabular input (that is,
%tabname%). For more information, see Defining Real Constants in Tabular Format.
The user subroutine USERCNPROP is also available for defining TCC. To use this subroutine, you must specify the table name %_CNPROP% as the real constant value. For more information, see Defining Real Constants via a User Subroutine.
TCC has units of heat/(time * area * temperature). If contact occurs, a small value of TCC yields a measured 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).
Note: If CONV is not defined through the SFE command, real
constant TCC will be used instead for modeling convection between two
opening surfaces only if tabular input or a user subroutine is
used. In this case, 
can be made a function of temperature (
), geometric gap, time, and initial contact detection point
location by using the tabular input as described above.
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 option:
| KEYOPT(1) = 2 - Temperature DOF only |
The following solver options must also be set:
When using the fast thermal transient solver, the user subroutines USERFRIC and USERINTER should not be used.
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), or specify a uniform temperature via the TUNIF or BFUNIF command.
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.
If KEYOPT(3) = 2 on the target element, convection is ignored for far-field contact.
Note: If CONV is not defined through the SFE command, real
constant TCC will be used instead only if it is defined by tabular input or a
user
subroutine. TCC can be made a function of temperature 
, geometric gap (positive GAP index values indicate
penetration, negative GAP index values indicate an open gap), time, and initial
contact detection point location by using tabular input (that is,
%tabname%).
To model radiative heat transfer, specify the following:
Emissivity value EMIS, specified through the material property definition.
Stefan-Boltzmann constant SBCT, specified 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.
Radiation view factor RDVF, specified through a real constant (defaults to 1).
Environment (ambient) temperature:
The ambient temperature 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 can be applied either on the contact elements via the SFE command with
KVAL= 2 and CONV specified as a table parameter (this is the same as the bulk temperature in free-surface convection modeling), or via the TUNIF or BFUNIF command.If KEYOPT(3) = 2 is set on the target element, radiation is ignored for far-field contact.
If the environment temperature is not specified, the free-surface radiation loading is not active.
When contact is open, heat transfer through radiation can occur. The equation is defined by
where
 = temperature offset from absolute zero to zero
(defined through the TOFFST command) |
 = surface emissivity (input as material
property) |
 = Stefan-Boltzmann constant (input as real constant).
There is no default for SBCT. If it is not defined, the radiation effect
is excluded. The Stefan-Boltzmann constant should correspond to the
units of the FE model to be solved (for example, 0.1190 x
10-10
BTU/hr-in2-R4;
5.67 x 10-8
W/m2-K4
|
 = radiation view factor, input as a real constant
(defaults to 1). RDVF can be defined as a function of temperature,
geometric gap distance (negative GAP index values indicate an open gap),
time, and initial contact detection point location (at the beginning of
solution) by using tabular input (that is,
%tabname%). The user subroutine
USERCNPROP is also available for defining RDVF (specify the
table name %_CNPROP% as the real constant value). RDVF is only used for
near-field radiation. For far-field radiation, RDVF is set to 1.0 and a
user-assigned value is ignored. Other free-surface conditions recognize
user-specified RDVF. |
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,
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, 
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 would typically perform a coupled transient thermal-structural analysis. If inertia effects are negligible, you can turn off transient effects on structural DOFs by using the command TIMINT,OFF,STRUC. 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
where
 = equivalent frictional stress |
 = sliding rate |
 = fraction of frictional dissipated energy converted
into heat. This value defaults to 1 and can be input as a real constant.
For an input value of true 0, you must enter a very small value (for
example, 1 x 10-8). If you enter 0, the
program interprets this as an input of the default value. |
The amount of frictional dissipation on contact and target surfaces is defined by
and
Where 
is the contact side and 
is the target side, and 
is the weight factor for the distribution of heat between the
contact and target surfaces (input as a real constant). By default,
. For an input of true 0, you must enter a very small value
(for example, 1 x 10-8). If you enter 0, the program
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.The external flux using the SFE command is only applied to either bonded (KEYOPT(12) >= 4) or standard (default, KEYOPT(12) = 0) contact.
The 3D surface-to-surface contact element (CONTA174) can be used to model thermal contact at the surface of thermal shell elements (SHELL131, SHELL132). The degrees of freedom of the thermal shells can be TEMP, TBOT, or TTOP, and the contact can occur at either the top or the bottom surface.
On the contact element, set KEYOPT(1) = 2 (temperature DOF only) and also set an appropriate value for KEYOPT(13). As shown in the table below, KEYOPT(13) enables you to control the temperature degrees of freedom (TEMP, TBOT, TTOP) activated on the contact surface and the target surface when the heat transfer is taking place between thermal shell elements or between thermal shell and thermal solid elements.
To model heat transfer between a thermal shell and a rigid target surface, use KEYOPT(13) = 0, 3, or 5.
| KEYOPT(13) | DOF on Contact Surface | DOF on Target Surface |
|---|---|---|
| 0 | TEMP | TEMP |
| 1 | TBOT | TBOT |
| 2 | TTOP | TTOP |
| 3 | TBOT | TEMP |
| 4 | TEMP | TBOT |
| 5 | TTOP | TEMP |
| 6 | TEMP | TTOP |
| 7 | TBOT | TTOP |
| 8 | TTOP | TBOT |