Next: Infinite Elements Up: Model Definition Previous: Degenerate Elements

Spring Elements

Spring elements may be defined in two ways; each spring can be defined individually by assigning a spring element variant to a FEMGEN point or line, or the command 'PROPERTY BOUNDARY ELASTIC' can be used to define a number of SPRING1 elements (placing a spring between a node and ground in a particular direction). The latter method is achieved via the following command:

PROPERTY BOUNDARY ELASTIC [const_name] part_name/ALL spring_const dir

**Table 2.6:** SPRING1 element definition.
Argument	Meaning
const_name	FEMGEN constraint name (optional).
part_name	Any geometry containing nodes.
Spring_const	Spring stiffness.
dir	Degree of Freedom Indicator (1,2,3).

Notes:

1.: The interface will simply apply the same spring value to all nodes attached to the specified geometry.
2.: Note that it is not possible to generate spring elements between two parts of a structure via the 'PROPERTY BOUNDARY ELASTIC' command. In such cases, a number of FEMGEN lines should be used to connect the two parts.

Example FEMGEN Command:

PROPERTY BOUNDARY ELASTIC CO1 L4 200 1

Corresponding ABAQUS Input File:

               
*ELEMENT, TYPE=SPRING1, ELSET=SPL4  
   17 ,    21
   18 ,    16
   19 ,    11
   20 ,     6
   21 ,     1
*SPRING, ELSET=SPL4  
    1
  200.0000    ,

Next: Infinite Elements Up: Model Definition Previous: Degenerate Elements

Femsys Limited
9/9/1999