- 积分
- 14
- 注册时间
- 2003-3-25
- 仿真币
-
- 最后登录
- 1970-1-1
|
原文出自http://www.engin.brown.edu/courses/En175/Abaqustut/template.inp
**
** This is a template for an ABAQUS input file.
** The main steps of an elastic stress analysis are listed,
** together with a list of useful keywords for each part of
** the computation. You can check the ABAQUS manual for
** detailed information about each keyword.
**
**
**
**************************************************************
** **
** GENERAL INSTRUCTIONS TO ABAQUS **
** **
**************************************************************
**
**
** *HEADING allows you to assign a title to the job
** *PREPRINT controls printing to the .dat file
** *RESTART used to control printint to .res file
** *FILE FORMAT used to control printing to .fil file
**
**************************************************************
** **
** MESH GENERATION **
** **
**************************************************************
**
** *NODE Define node numbers and coordinates
** *NGEN Generate a line of nodes
** *NCOPY Copy a set of nodes
** *NFILL Fill a block with nodes
** *NSET Define a named node set
** *NMAP Map a set of nodes from one coord system to another
**
** *ELEMENT Define connectivity and type for an element
** *ELGEN Generate connectivity for a regularly numbered block
** *ELSET Define a named set of elements
** *ELCOPY Copy a set of elements
** LIST OF SOME ELEMENT TYPES
** CPE3 3 noded plane strain triangle
** CPE4 4 noded plane strain quadrilateral
** CPE6 6 noded plane strain triangle
** CPE8 8 noded plane strain quadrilateral
** CPS3 3 noded plane stress triangle
** CPS4 4 noded plane stress quadrilateral
** CPS6 6 noded plane stress triangle
** CPS8 8 noded plane stress quadrilateral
** C3D4 4 noded tetrahedron
** C3D6 6 noded triangular prism
** C3D8 8 noded brick
** C3D10 10 noded tetrahedron
** C3D15 15 noded triangular prism
** C3D20 20 noded brick
**
** For problems involving large plastic strains or nearly incompressible
** materials, add suffix R or H to element type (eg CPE4R, C3D4H)
** to use reduced integration (R) or hybrid element (H)
**
**
** *SYMMETRIC MODEL GENERATION turns a 2D mesh into a 3D mesh with axial symmetry, by rotating
** the 2D mesh about an axis of revolution. Can
** also be used to extend a 3D mesh by reflection
** about a plane.
**
** *SOLID SECTION Assign material properties to elements
**
**
**
**
** *SURFACE DEFINITION Define a surface on a set of elements for contact problems
** *RIGID SURFACE Define the shape of a rigid surface for contact problems
**
**
**
**************************************************************
** **
** MATERIAL PROPERTY DEFINITION **
** **
**************************************************************
**
** *MATERIAL Begin material property definition
**
** *ELASTIC Define elastic properties
** *EXPANSION Specify thermal expansion coefficient
** *PLASTIC Define strain hardening characteristics
** *DENSITY Define mass density
** *CREEP Define creep properties of a material
** *RATE DEPENDENT Define a rate dependent viscoplastic material
** *HYPERELASTIC Define properties for large strain elasticity, eg rubber.
** *NO TENSION Define material which cannot support tension (Use with *ELASTIC)
** *CONCRETE, *TENSION STIFFENING Define properties for concrete
** *CLAY PLASTICITY Define properties of a soil (`Cam-clay')
**
**
**************************************************************
** **
** TIME INDEPENDENT BOUNDARY CONDITIONS **
** **
**************************************************************
**
** *NSET Define a named set of nodes
** *BOUNDARY Fix nodes
** *MPC Constrain relative motion of nodes
**
**************************************************************
** **
** DEFINE INITIAL CONDITIONS **
** (Dynamic or time dependent problems only) **
** **
**************************************************************
**
** *INITIAL CONDITIONS Define initial values of DOFs, velocities, etc.
**
**
**************************************************************
** **
** INFORMATION DEFINING TIME VARYING LOADS **
** **
**************************************************************
**
** *NSET Define a named set of nodes
** *ELSET Define a named set of elements
** *AMPLITUDE Define time variation of load
**
** *STEP Begin a load step
** *STEP, NLGEOM Activate large deformation analysis
**
** *STATIC Set up a quasi--static analysis with time independent materials
** *VISCO Set up a quasi--static analysis with time dependent material
** *DYNAMIC Set up time variation for a dynamic problem
**
** *DLOAD Define distributed loads or body forces acting on elements
** *BOUNDARY Define time varying nodal displacements
** *CLOAD Apply concentrated forces to nodes
**
** *EL FILE Print element integration point data to the .fil file
** *NODE FILE Print nodal variables to the .fil file
**
** Partial list of element variables
** S All stress components
** SP All principal stresses
** SINV All stress invariants (including MISES, TRESC, PRES, INV3)
** E All strain components
** EP All principal strains
** NE All nominal strain components
** NEP All principal nominal strains
** DG All components of the deformation gradient
** EE All elastic strain components
** EEP All principal elastic strains
** THE All thermal strain components
** THEP All principal thermal strains
** PE All plastic strain components
** (including equivalent plastic strain)
** PEP All principal plastic strains
** CE All creep strain components
** (including equivalent creep strain)
** CEP All principal creep strains
** ENER All energy densities
**
** Partial list of nodal variables
** U All degrees of freedom (displacements)
** V All velocity components
** COORD All nodal coordinates
** CF All components of nodal forces/moments
** RF All reaction forces at nodes
**
** *END STEP Terminate step definition (required) |
评分
-
1
查看全部评分
-
|