Next: Example Model CONTI2 Up: Example Models Previous: Example Model CPE8
Next: Example Model CONTI2
Up: Example Models
Previous: Example Model CPE8
This example illustrates the creation of a sagging cable which is then subjected to a frequency analysis.
PROPERTY FE-PROG ABAQUS
GEOMETRY POINT P1 0
GEOMETRY POINT P2 100
GEOMETRY LINE P1 P2
MESHING TYPE L1 BE2 4
MESHING DIVISION LINE L1 10
PROPERTY MATERIAL ELASTIC STEL 200E9 0.3 7860
PROPERTY PHYSICAL THICKNES CROS 7.8525E-5
PROPERTY ATTACH L1 STEL CROS
PROPERTY BOUNDARY CONSTRAINT P1 123
PROPERTY BOUNDARY CONSTRAINT P2 123
PROPERTY LOAD I-STRESS 1 L1 1.0E6
PROPERTY LOAD STEP-DEF 1 ALL 0 1
PROPERTY LOAD PROC-DEF STAT 1 ALL 0.1 1
PROPERTY LOAD GRAVITY 1 L1 -9.814 2
PROPERTY LOAD STEP-DEF 2 ALL 0 1
PROPERTY LOAD PROC-DEF FREQ 2 ALL 5 20
MESHING GENERATE
UTILITY WRITE ABAQUS c1d2.inp
YES
**********************************************
** ABAQUS 5.2 INPUT DECK *
** CREATED BY FEMGEN/FEMVIEW VERSION 2.305 *
** TRANSLATED BY FEMGEN-ABAQUS VERSION 3.000 *
** FILE CREATED: DATE 13/04/94 TIME 11:51:50 *
**********************************************
**
**********************************************
** BINARY RESULT FILE FORMAT SELECTED *
** MESSAGE LOGGING IS OFF *
** DIALOG SESSION IS OFF *
** ABAQUS/Standard SELECTED *
** EXTERNAL MATERIAL DIRECTORY NOT USED *
** EXTERNAL RESULT OUTPUT FILE NOT USED *
**********************************************
**
*HEADING
FEMGEN MODEL C1D2 TRANSLATED BY PRE-ABAQUS 3.000 TITLE: No model title
**
**********************************************
** MODEL DEFINITION ... *
**********************************************
**
*******************
** MODEL GEOMETRY *
*******************
**
*NODE, NSET=ALLNODE
1, 0.0000000 , 0.0000000 , 0.0000000
2, 10.00000 , 0.0000000 , 0.0000000
3, 20.00000 , 0.0000000 , 0.0000000
4, 30.00000 , 0.0000000 , 0.0000000
5, 40.00000 , 0.0000000 , 0.0000000
6, 50.00000 , 0.0000000 , 0.0000000
7, 60.00000 , 0.0000000 , 0.0000000
8, 70.00000 , 0.0000000 , 0.0000000
9, 80.00000 , 0.0000000 , 0.0000000
10, 90.00000 , 0.0000000 , 0.0000000
11, 100.0000 , 0.0000000 , 0.0000000
*ELEMENT, TYPE=C1D2 , ELSET=L1
1 1 2
2 2 3
3 3 4
4 4 5
5 5 6
6 6 7
7 7 8
8 8 9
9 9 10
10 10 11
**
********************
** SET DEFINITIONS *
********************
**
*ELSET, ELSET=PHY1
L1 ,
*ELSET, ELSET=ALL
PHY1 ,
**
*************************
** PROPERTY DEFINITIONS *
*************************
**
*SOLID SECTION, ELSET=PHY1 ,MATERIAL=STEL
0.7852501E-04,
**
*************************
** MATERIAL DEFINITIONS *
*************************
**
*MATERIAL, NAME=STEL
*DENSITY
7860.000 ,
*ELASTIC, TYPE=ISO
200.0E+09,0.300 ,0.000
*EXPANSION, ZERO= 0.0000000
0.0000000 , 0.0000000
**
**************************
** KINEMATIC CONSTRAINTS *
**************************
**
*NSET, NSET=P1
1
*BOUNDARY
P1 , 1, 3
*NSET, NSET=P2
11
*BOUNDARY
P2 , 1, 3
*INITIAL CONDITIONS, TYPE=STRESS
L1 , 0.100E+07, 0.000 , 0.000 , 0.000 , 0.000 , 0.000
**
**********************************************
** HISTORY DEFINITION ... *
**********************************************
**
**********************************************
** FEMGEN LOADCASE 1 *
**************************
**
*STEP,INC=100,NLGEOM
*STATIC
0.1000000 , 1.000000
*DLOAD, OP=MOD
L1 , GRAV, -9.814000 , 0.0000000 , 1.000000 , 0.0000000
**
***************************
** RESULTS OUTPUT CONTROL *
***************************
**
*NODE FILE
U,RF,CF
*EL FILE, POSITION=AVERAGED AT NODES
S,E
*EL FILE, POSITION=NODES
S,E
*EL FILE, POSITION=INTEGRATION POINTS
S,COORD
E,COORD
ENER,COORD
*END STEP
**
**********************************************
** FEMGEN LOADCASE 2 *
**************************
**
*STEP,INC=100,NLGEOM
*FREQUENCY
5, 20.00000
**
***************************
** RESULTS OUTPUT CONTROL *
***************************
**
*NODE FILE
U
*END STEP
**
**********************************************