*HEADING
 PIPE WHIP SIMULATION
**
**  This example simulates a pipe-on-pipe impact resulting from 
**  the rupture of a high-pressure line in a power plant. It is 
**  assumed that a sudden release of fluid could cause one segment 
**  of the pipe to rotate about its support and strike a 
**  neighboring pipe.
**
**  Generate a 138 x 45 mesh for the impacting pipe.
**
*SYSTEM
 0., 0., 3.3125, 0., 1., 3.3125
 0., 0., 4.3125
*NODE, SYSTEM=C
  1, 3.0965, -90., -25.
 46, 3.0965,  90., -25.
*NODE, SYSTEM=R
 100000, 0., 0., -25.
*NGEN, NSET=SECTA, LINE=C
 1, 46, 1, 100000, 0., 0., -25., 0., 0., 1.
*NCOPY, SHIFT, CHANGE NUMBER=1242, OLD SET=SECTA, NEW SET=SECTB
 15., 0., 0.
  0., 0., 0., 0., 0., 1., 0.
*NFILL, NSET=END1P1
 SECTA, SECTB, 27, 46
*NCOPY, SHIFT, CHANGE NUMBER=5106, OLD SET=SECTA, NEW SET=SECTC
 35., 0., 0.
  0., 0., 0., 0., 0., 1., 0.
*NFILL, NSET=MIDP1
 SECTB, SECTC, 84, 46
*NCOPY, SHIFT, CHANGE NUMBER=6348, OLD SET=SECTA, NEW SET=SECTD
  50., 0., 0.
   0., 0., 0., 0., 0., 1., 0.
*NFILL, NSET=END2P1
 SECTC, SECTD, 27, 46
*NSET, NSET=PIPE1
 END1P1, MIDP1, END2P1
*ELEMENT, TYPE=S4R
 1, 1, 2, 48, 47
*ELGEN, ELSET=PIPE1
 1, 45, 1, 1, 138, 46, 45
*SHELL SECTION, ELSET=PIPE1, MATERIAL=STEEL, SECTION INTEGRATION=GAUSS
 0.432, 
*NSET, NSET=SECTE, GENERATE
  1, 6349, 46
 46, 6394, 46
*BOUNDARY
 SECTE, YSYMM
 REFPT, 1, 1, 0.
 REFPT, 3, 3, 0.
*NSET,NSET=PLANE,GENERATE
 6349, 6394, 1
*NODE,NSET=REFPT, SYSTEM=C
 200001, 0., 0., 25.
*ELSET, ELSET=MIDP1, GENERATE
 1216, 4995, 1
**
**  Generate a 48 x 72 mesh for the impacted pipe.
**
*SYSTEM
 0., 0., -3.3125, -1., 0., -3.3125
 0., 0.,  0.
*NODE, SYSTEM=C
 10001, 3.0965,   0., 0.
 10072, 3.0965,   355.0000    , 0.
*NODE, SYSTEM=R
 100001, 0., 0., 0.
*NGEN, NSET=SECTF, LINE=C
 10001, 10072, 1, 100001, 0., 0., 0., 0., 0., 1.
*NCOPY, SHIFT, CHANGE NUMBER=1512, OLD SET=SECTF, NEW SET=SECTG
 0.,  7., 0.
 0.,  0., 0., 0., 0., 1., 0.
*NFILL, NSET=MIDP2
 SECTF, SECTG, 21, 72
*NCOPY, SHIFT, CHANGE NUMBER=3456, OLD SET=SECTF, NEW SET=SECTH
 0., 25., 0.
 0.,  0., 0., 0., 0., 1., 0.
*NFILL, NSET=ENDP2
 SECTG, SECTH, 27, 72
*NSET, NSET=PIPE2
 MIDP2, ENDP2
*ELEMENT, TYPE=S4R
       10001,       10001,       10002,       10074,       10073
*ELGEN, ELSET=OPENLOOP
       10001, 71, 1, 1, 48, 72, 72
*ELEMENT, TYPE=S4R
       10072,       10072,       10001,       10073,       10144
*ELGEN, ELSET=CLOSURE
       10072,          48,          72,          72
*ELSET, ELSET=PIPE2
 OPENLOOP, CLOSURE
*SHELL SECTION, ELSET=PIPE2, MATERIAL=STEEL, SECTION INTEGRATION=GAUSS
 0.432, 
*BOUNDARY
 SECTF, YSYMM
 SECTH, ENCASTRE
*ELSET, ELSET=MIDP2, GENERATE
       10001, 11512, 1
*ELSET, ELSET=ETOP
185, 
*ELSET, ELSET=EBOT
602, 
*ELSET, ELSET=ELOUT
ETOP,EBOT
*NSET, NSET=NOUT
200,602
**
**  Material description.
**
*MATERIAL, NAME=STEEL
*ELASTIC
 30.E6, 0.3
*PLASTIC
 45.E3, 
*DENSITY
 7.324E-4, 
**
**  The impacting pipe is allowed to rotate about a fixed pivot 
**  with an initial angular velocity of 75 radian/sec.
**
*INITIAL CONDITIONS, TYPE=ROTATING VELOCITY
 PIPE1, 75., 0., 0., 0.
 25., 3.0965, 3.3125, 25., -3.0965, 3.3125   
**
**  The simulation will run for 0.015 second
**
*RESTART, WRITE, NUMBER INTERVAL=3, TIMEMARKS=NO
*ELGEN, ELSET=PIPE11
 1, 45, 1, 1, 137, 46, 45
*RIGID BODY,REF NODE=200001,TIE NSET=PLANE
*ELEMENT, TYPE=MASS, ELSET=MASS
200000, 200001
*ELEMENT, TYPE=ROTARYI, ELSET=ROTARY
200001, 200001
*MASS, ELSET=MASS
1.E-6,
*ROTARY INERTIA, ELSET=ROTARY
1.E-7,1.E-7,1.E-7
*STEP
*DYNAMIC, EXPLICIT
 , 0.015
*CONTACT 
*CONTACT INCLUSIONS, ALL ELEMENT BASED
*OUTPUT,FIELD,VAR=PRESELECT,NUMBER INTERVAL=5
**
** Output requests for qa testing
**
*NSET,NSET=QA_TEST
NOUT,
*ELSET,ELSET=QA_TEST
ELOUT,
*OUTPUT,FIELD,NUMBER INTERVAL=1
*NODE OUTPUT, NSET=QA_TEST
 U,
*ELEMENT OUTPUT, ELSET=QA_TEST
 PEEQ,
*OUTPUT,HISTORY,VAR=PRESELECT,TIME INTERVAL=0.00375
*FILE OUTPUT, NUMBER INTERVAL=1
*EL FILE, ELSET=ELOUT
 PEEQ,
*NODE FILE, NSET=NOUT
 U,
*ENERGY FILE
*END STEP