Ansys > Building A Model > Finite Elements
XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">   
Finite Elements
Finite Elements in Patran is used to define the basic finite element construction. The Finite Elements form appears when Finite Elements, located on the Patran main form, is chosen. Use this application to create ANSYS nodes and elements.
Nodes
Nodes in Patran will generate the ANSYS N command. Create Nodes either directly by using the Node object, or indirectly by using the Mesh object. An ANSYS NROTAT command is generated for each node associated to a non-global analysis coordinate frame.
Elements
Finite Elements in Patran assign element topology, such as Quad⁄4 which is used for standard finite elements. The type of elements created are not determined until the element properties are assigned. Either create elements directly, by using the Element object, or indirectly by using the Mesh object. The element connectivity is entered using the ANSYS EN command.
Multi-Point Constraints
Multi-point Constraints (MPCs) can be created from the Finite Elements form. MPCs are special element types which define a rigorous behavior between several specified nodes. The forms for creating MPCs are found by selecting MPC as the Object on the Finite Elements form. The full functionality of the MPC forms are defined in Create MPC Form (for all MPC Types Except Cyclic Symmetry and Sliding Surface) (p. 129) in the Reference Manual - Part III.
MPC Types
To create an MPC, first select the type of MPC to be created from the option menu. The MPC types that appear in this option menu are dependent on the current settings of the Analysis Code and Analysis Type preferences. The following table describes the MPC types which are supported for Patran ANSYS.
 
MPC Type
Analysis Type
Description
Structural
Thermal
Creates an ANSYS CE explicit MPC between a dependent degree-of-freedom and one or more independent degrees-of-freedom. The dependent term consists of a node ID and a degree-of-freedom, while an independent term consists of a coefficient, a node ID, and a degree-of-freedom. An unlimited number of independent terms can be specified, while only one dependent term can be specified. The constant term is obtained from the Create MPC form.
Rigid (Fixed)
Structural
Creates the ANSYS CERIG command which constrains all degrees-of-freedom at one or more dependent nodes to the corresponding degrees-of-freedom at one independent node. An unlimited number of dependent terms can be specified, while only one independent term can be specified. Each term consists of a single node. There is no constant term for this MPC type.
Rigid (Pinned)
Structural
Creates the ANSYS CERIG command which constrains only the translational components. An unlimited number of dependent terms can be specified, while only one independent term can be specified. Each term consists of a single node. There is no constant term for this MPC type.
CP
Structural
Thermal
Creates an ANSYS CP command between the selected degree-of-freedom of the independent node and the same degree-of-freedom of one or more dependent nodes. An unlimited number of dependent terms may be specified. Only one independent node and degree-of-freedom may be specified. There is no constant term for this MPC type.
Degrees-of-Freedom
When a list of degrees-of-freedom is expected for an MPC term, a listbox containing the valid degrees-of-freedom is displayed on the form. A degree-of-freedom is valid if:
1. It is valid for the current Analysis Code Preference.
2. It is valid for the current Analysis Type Preference.
3. It is valid for the selected MPC type.
In most cases, all degrees-of-freedom which are valid for the current Analysis Code and Analysis Type preferences are valid for the MPC type.
The following degrees-of-freedom are supported by the Patran ANSYS MPCs for the various analysis types:
 
Degree-of-freedom
Analysis Type
UX
Structural
UY
Structural
UZ
Structural
RX
Structural
RY
Structural
RZ
Structural
Temperature
Thermal
 
Note:  
Make sure that the degree-of-freedom selected for an MPC actually exists. For example, a node that is attached only to solid structural elements will not have any rotational degrees-of-freedom. However, Patran will allow you to select rotational degrees-of-freedom at this node when defining an MPC.
Explicit MPCs
This form appears when Define Terms is selected from the Finite Elements form when Explicit is the selected type. Use this form to create the ANSYS CE command.
 
Note:  
The equation used to define Explicit MPCs in Patran (3‑1) in the Reference Manual - Part III is different than the equation used by ANSYS. The equation used by ANSYS is:  C0 = C1U1 + C2U2 +C3U3 + ... + CnUn.   This will cause the independent terms to have the opposite sign in the ANSYS PREP7 input file than the values input in the Patran Define Terms form. The dependent term from the Patran form will be placed in the first term (C1U1) of the equation, with C1 set to one, to comply with the ANSYS convention.
Rigid (Fixed)
This form appears when the Define Terms button is selected on the Finite Elements form when Rigid (Fixed) is the selected Type. Use this form to create the ANSYS CERIG command.
Rigid (Pinned)
This form appears when the Define Terms button is selected on the Finite Elements form when Rigid (Pinned) is the selected Type. Use this form to create the ANSYS CERIG command.
CP
This form appears when the Define Terms button is selected on the Finite Elements form when CP is the selected Type. Use this form to create the ANSYS CP command.
DOF Lists
Degree-of-freedom (DOF) lists can be created from the Finite Elements form. DOF Lists are a collection of node IDs and degrees-of-freedom. The form for creating DOF Lists is found by selecting DOF Lists as the Object on the Finite Elements form. The full functionality of the DOF List forms is defined in Creating DOF List (p. 136) in the Reference Manual - Part III.
Define Terms
This form appears when the Define Terms button is selected on the Finite Elements form when
DOF List is the selected Type. Use this form to create the ANSYS M command for each node,
DOF combination selected.