Ansys > Building A Model > Loads and Boundary Conditions
XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">   
Loads and Boundary Conditions
The Loads and Boundary Conditions form appears when the Loads⁄BCs toggle, located on the Patran main form, is chosen. The selections on this form will determine which Loads and Boundary form will appear, and ultimately, which ANSYS loads and boundary conditions will be created.
The following page gives an introduction to the Loads and Boundary Conditions form, followed by details of the loads and boundary conditions supported by the Patran ANSYS Application Preference.
Loads & Boundary Conditions Form
The Loads and Boundary Conditions form is used to create ANSYS loads and boundary conditions. For more information, see Loads and Boundary Conditions Form (p. 21) in the Patran Reference Manual.
The following table outlines the options when the Analysis Type is set to Structural.
 
Object
Type
Nodal
Nodal
Element Uniform
Nodal
Element Uniform*
Nodal
Contact
Element Uniform (ANSYS 5 Only)
 
Note:  
*Inertial Loads are shown as Element Uniform Type but actually apply to the entire model.
The following table outlines the options when the Analysis Code is set to Thermal.
 
Object
Type
Temp (Thermal)
Nodal
Convection
Element Uniform
Element Uniform (ANSYS 5 Only)
Nodal
Nodal
Static
This subordinate form appears when the Input Data button is selected when Static is the selected Load Case Type. The information contained on this form will vary according to the selected Object. However, defined below is information that remains standard to this form.
Object Tables
On the static input data form, there are areas where the load data values are defined. The data fields presented depend on the selected Object and Type. In some cases, the data fields also depend on the selected Target Element Type. These Object Tables list and define the various input data which pertain to a specific selected object.
Displacement
 
Object
Type
Type
Displacement
Nodal
Structural
Creates the ANSYS D command. All nonblank entries will generate prescribed displacements with the D command.
 
Input Data
Description
Translations (T1,T2,T3)
Defines the prescribed translational displacement vector. Components of the vector are entered in model length units. The vector is not transformed. The analysis coordinate frames of the nodes in the application region are changed to the analysis coordinate frame specified on this form.
Rotations (R1,R2,R3)
Defines the prescribed rotational displacement vector. Components of the vector are entered in radians. The vector is not transformed. The analysis coordinate frames of the nodes in the application region are changed to the analysis coordinate frame specified on this form.
Force
 
Object
Type
Type
Force
Nodal
Structural
Creates the ANSYS F command.
 
Input Data
Description
Force (F1,F2,F3)
Defines the applied translational force vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the F command(s).
Moment (M1,M2,M3)
Defines the applied rotational force vector with respect to the specified analysis coordinate frame. This vector is transformed from the specified analysis coordinate frame to the analysis coordinate frames of the nodes in the application region before it is written to the F commands(s).
Pressure
 
Object
Type
Type
Dimension
Pressure
Element Uniform
Structural
2D
Creates the ANSYS EP command for ANSYS Revision 4.4A. Creates the SFE command with the Lab data field set to PRES for ANSYS Revision 5.
 
Input Data
Description
Top Surf Pressure
Defines the top surface pressure on shell and/or plate elements which is directed inward when positive.
Bot Surf Pressure
Defines the bottom surface pressure on shell and/or plate elements which is directed inward when positive.
Edge Pressure
Defines the edge pressure on 2D solid elements which is directed inward when positive. The IFACE data field of the EP command, or the LKEY data field of the SFE command, varies based on the element edges chosen in the application region. Top and/or bottom surface pressures cannot be used in the same application region as edge pressure.
 
Object
Type
Type
Dimension
Pressure
Element Uniform
Structural
3D
Creates the ANSYS EP command for ANSYS Revision 4.4A. Creates the SFE command with the Lab data field set to PRES for ANSYS Revision 5.
 
Input Data
Description
Pressure
Defines the face pressure on solid elements which is directed inward when positive. The IFACE data field of the EP command, or the LKEY data field of the SFE command, varies based on the element faces chosen in the application region.
Temperature
 
Object
Type
Type
Temperature
Nodal
Structural
Creates the ANSYS T command for ANSYS Revision 4.4A. Creates the BF command with the Lab field set to Temp for ANSYS Revision 5.
 
Input Data
Description
Temperature
Defines the nodal temperature values for a structural analysis.
Inertial Loads
Object
Type
Type
Dimension
Inertial
Element Uniform
Structural
N/A
Creates the ANSYS ACEL, OMEGA, and DOMEGA commands. Inertial Loads are defined using a custom form, as shown below, to define the input data. Since ANSYS Inertial Loads apply to the entire model, no application region selection is permitted.
Voltage
 
Object
Type
Type
Voltage
Nodal
Structural
Creates the ANSYS NT command with Lab set to VOLT for ANSYS Revision 4.4A. Creates the D command with the Lab field set to VOLT for ANSYS Revision 5.
 
Input Data
Description
Voltage
Defines the nodal voltage values for a structural analysis.
Contact (Deform-Deform)
 
Object
Type
Type
Contact
Element Uniform
Structural
Defines contact between two deformable structural bodies. For 2D and 3D models, contact bodies are modeled by CONTAC48 and CONTAC49 elements, respectively. The entries on the Application Region and Input Data forms are used to define Components, and appropriate ANSYS GCGEN, material (MP), and real constant (R) commands are created. Contact LBCs are used only for nonlinear static analyses.
Contact Select Application Region (ANSYS 5)
Temperature (Thermal)
 
Object
Type
Type
Temp (Thermal)
Nodal
Thermal
Creates the ANSYS NT, TEMP command.
 
Input Data
Description
Temperature
Defines the prescribed temperature value.
Convection
 
Object
Type
Type
Dimension
Convection
Element Uniform
Thermal
2D
Creates the ANSYS EC command for ANSYS Revision 4.4A. Creates the SFE command with the Lab data field set to PRES for ANSYS Revision 5.
 
Input Data
Description
Top Surf Convection
Defines the top surface film coefficient on shell elements.
Bot Surf Convection
Defines the bottom surface film coefficient on shell elements.
Edge Convection
Defines the edge film coefficient on 2D solid elements. The entry in the IFACE data field of the EC command, or the LKEY data field of the SFE command, varies based on the element edges chosen in the application region. Top and/or bottom surface convections cannot be used in the same application region as edge convection.
Ambient Temp
Defines the sink temperature for the shell or 2D solid elements. This produces an entry in the TBULK data field of the EC command, or in the VAL1 data field of the SFE command.
 
Object
Type
Type
Dimension
Convection
Element Uniform
Thermal
3D
Creates the ANSYS EC command for ANSYS Revision 4.4A. Creates the SFE command with the Lab data field set to PRES for ANSYS Revision 5.
 
Input Data
Description
Convection
Defines the film coefficient on faces of solid elements. The entry in the IFACE data field of the EC command, or the LKEY data field of the SFE command, varies based on the element faces chosen in the application region.
Ambient Temp
Defines the sink temperature for the solid elements. This produces an entry in the T BULK data field of the EC command, or in the VAL1 data field of the SFE command.
Heat Flux
 
Object
Type
Type
Dimension
Heat Flux
Element Uniform
Thermal
2D
Creates the ANSYS SFE command. This is only supported by ANSYS Revision 5.   
Input Data
Description
Top Surf Heat Flux
Defines the top surface heat flux on shell elements. The Lab data field of the SFE command is set to HFLUX.
Bot Surf Heat Flux
Defines the bottom surface heat flux on shell elements. The Lab data field of the SFE command is set to HFLUX.
Edge Heat Flux
Defines the edge heat flux on 2D solid elements. The entry in the LKEY data field of the SFE command varies based on the element edges chosen in the application region. Top and/or bottom surface heat fluxes cannot be used in the same application region as an edge heat flux.
 
Object
Type
Type
Dimension
Heat Flux
Element Uniform
Thermal
3D
Creates the ANSYS SFE command. This is only supported by ANSYS Revision 5.0.
 
Input Data
Description
Heat Flux
Defines the heat flux on faces of solid elements. The entry in the LKEY data field of the SFE command varies based on the element faces chosen in the application region.
Heat Source
 
Object
Type
Type
Heat Source
Nodal
Thermal
Creates the ANSYS HFLOW command.
 
Input Data
Description
Heat Source
Defines the applied nodal heat source.
Voltage Thermal
Object
Type
Type
Voltage
Nodal
Thermal
Creates the ANSYS NT command with Lab set to VOLT for ANSYS Revision 4.4A. Creates the D command with the Lab field set to VOLT for ANSYS Revision 5.
 
Input Data
Description
Voltage
Defines the nodal voltage values for a thermal-electric analysis.