Element death APDL code
Element death APDL code
(OP)
I'm trying to get element death to work in a loop to simulate a realistic failure. Problem is, the ESEL and EKILL only seem to happen on the first loop iteration; after that the peripheral commands set to read the results set and solve continue to execute, but the ESEL and EKILL commands don't appear to execute whatsoever. I did read chapter 12 on element birth and death (repeatedly) but as usual, I seem to be missing something (or the documentation does). Here's the code. Be kind, I'm no advanced programmer.
/SOLU
!*
ANTYPE,0
ANTYPE,0
NLGEOM,1
NSUBST,rsn,0,0
OUTRES,ERASE
OUTRES,ALL,ALL
AUTOTS,0
LNSRCH,1
NEQIT,100
PSTRES,1
RESCONTRL,DEFINE,ALL,ALL,rsn
TIME,pressure
/STATUS,SOLU
SOLVE
FINISH
/REPLOT
*DO,I,1,rsn-1,1
/POST1
PLNSOL, U,Y, 0,1.0
/WAIT,30
/POST1
SET,1,I,1,
ETABLE,STRS,S,X
ESEL,S,ETAB,STRS,SxMax
ESEL,A,ETAB,STRS,-100000,SxMin
ETABLE,STRS,S,Y
ESEL,A,ETAB,STRS,SyMax
ESEL,A,ETAB,STRS,-100000,SyMin
ETABLE,STRS,S,Z
ESEL,A,ETAB,STRS,SzMax
ESEL,A,ETAB,STRS,-100000,SzMin
ETABLE,STRS,S,XY
ESEL,A,ETAB,STRS,SxyMax,,1
ETABLE,STRS,S,YZ
ESEL,A,ETAB,STRS,SyzMax,,1
ETABLE,STRS,S,XZ
ESEL,A,ETAB,STRS,SxzMax,,1
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,INVE
ANTYPE,,REST,1,I,0
RESCONTRL,DEFINE,ALL,ALL,I
SOLVE
*ENDDO
CODE
/SOLU
!*
ANTYPE,0
ANTYPE,0
NLGEOM,1
NSUBST,rsn,0,0
OUTRES,ERASE
OUTRES,ALL,ALL
AUTOTS,0
LNSRCH,1
NEQIT,100
PSTRES,1
RESCONTRL,DEFINE,ALL,ALL,rsn
TIME,pressure
/STATUS,SOLU
SOLVE
FINISH
/REPLOT
*DO,I,1,rsn-1,1
/POST1
PLNSOL, U,Y, 0,1.0
/WAIT,30
/POST1
SET,1,I,1,
ETABLE,STRS,S,X
ESEL,S,ETAB,STRS,SxMax
ESEL,A,ETAB,STRS,-100000,SxMin
ETABLE,STRS,S,Y
ESEL,A,ETAB,STRS,SyMax
ESEL,A,ETAB,STRS,-100000,SyMin
ETABLE,STRS,S,Z
ESEL,A,ETAB,STRS,SzMax
ESEL,A,ETAB,STRS,-100000,SzMin
ETABLE,STRS,S,XY
ESEL,A,ETAB,STRS,SxyMax,,1
ETABLE,STRS,S,YZ
ESEL,A,ETAB,STRS,SyzMax,,1
ETABLE,STRS,S,XZ
ESEL,A,ETAB,STRS,SxzMax,,1
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,INVE
ANTYPE,,REST,1,I,0
RESCONTRL,DEFINE,ALL,ALL,I
SOLVE
*ENDDO





RE: Element death APDL code
Although I don't really understand what you are doing with all this esel,,etab, I guess you should select all elements before you define your element table:
CODE
/POST1
PLNSOL, U,Y, 0,1.0
/WAIT,30
SET,1,I,1,
esel,s,all
ETABLE,STRS,S,X
...
If this don't work, perhaps you should explain how you defined SxMin, SyMin,...
In the end I would also select everything before solving:
[code]
...
RESCONTRL,DEFINE,ALL,ALL,I
alls
SOLVE
...
[code]
If you do that, you don't have to select all elements anymore before the etab comand.
Regards
Alex
RE: Element death APDL code
I will however try selecting all of the elements rather than my invert selection. The more I think about it the more that sounds like the right approach.
The SxMin,... values are defined with simple SxMin=1000 type commands up in the program header. I did it that way so others could easily modify the model without being code monkeys.
RE: Element death APDL code
Just to clarify, if I only run the loop once, making two SOLVE commands for the entire program, then the elements "die" as planned and the model reacts appropriately. With more than two its asif I haven't changed anything from the initial solution. ???
RE: Element death APDL code
Alex
RE: Element death APDL code
If you could post an Ekill and restart routine even just selecting a particular element or volume for the kill, I think I'd get it from there in terms of adjusting my selection. And thanks again for the HELP!
RE: Element death APDL code
CODE
!* Definition of variables ************************************************
!*
tft=0.125 !top flange thickness
bft=0.125 !bottom flange thickness
fw=1.5 !flange width
ch=1.25 !core height
ra=50 !rib angle
rt=0.075 !rib thickness
ir=0.0625 !inside radius of the core
esf=.5 !element size factor
lat=.5 !load applicator thickness
pressure=100 !pressure applided to applicator - psi (must be an integer multiple of pinc)
pinc=50 !Pressure increment in results sets and solution
rsn=pressure/pinc !number of results sets (and restart sets) to record
SxMax=4140 !Max Stresses
SyMax=160
SzMax=4140
SxMin=-4020
SyMin=-10000
SzMin=-4020
SxyMax=430 !Shear max stress values are absolute values
SyzMax=430
SxzMax=2850
ed=1 !extrusion depth
!*
!*
tl=.4 !multiplication factor for length of the target length beneath the core radius tl*(ir+rt)
!*
!******************************************************
/Title, True Failure
/NOPR
/PMETH,ON,0
KEYW,PR_SET,1
KEYW,PR_STRUC,1
KEYW,PR_THERM,0
KEYW,PR_FLUID,0
KEYW,PR_MULTI,0
/GO
!*
/COM,
/COM,Preferences for GUI filtering have been set to display:
/COM, Structural with p-Method elements
/PREP7
!*
/COM, INPUT LINE INFORMATION FOR THE CORRUGATED SECTION
*AFUN,DEG ! Units for angular functions are degrees
K , 1 , 0.000 , bft , 0 ,
K , 2 , 0.000 , bft+rt , 0 ,
K , 3 , (fw-TAN(ra/2)*(ir+rt)-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra))/2+TAN(ra/2)*(ir) , bft+rt , 0 ,
K , 4 , fw-(fw-TAN(ra/2)*(ir+rt)-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra))/2-TAN(ra/2)*(ir+rt) , ch+bft , 0 ,
K , 5 , fw , ch+bft , 0 ,
K , 6 , fw , ch-rt+bft , 0 ,
K , 7 , fw-(fw-TAN(ra/2)*(ir+rt)-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra))/2-(TAN(ra/2)*(ir)) , ch-rt+bft , 0 ,
K , 8 , fw-(fw-TAN(ra/2)*(ir+rt)-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra))/2-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra) , bft , 0 ,
K , 9 , (fw-(fw-TAN(ra/2)*(ir+rt)-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra))/2-TAN(ra/2)*(ir+rt))-tl*(ir+rt) ,ch+bft , 0 ,
K , 10 , 0.000 , ch+bft , 0 ,
K , 11 , 0.000 , bft+ch+tft , 0 ,
K , 12 , fw , bft+ch+tft , 0 ,
K , 13 , fw-(fw-TAN(ra/2)*(ir+rt)-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra))/2-TAN(ra/2)*(ir)-(ch-rt)/TAN(ra)+tl*(ir+rt) , bft , 0 ,
K , 14 , fw , bft , 0 ,
K , 15 , fw , 0 , 0 ,
K , 16 , 0 , 0 , 0 ,
K , 17 , 0.000 , bft+ch+tft+lat , 0 ,
K , 18 , fw , bft+ch+tft+lat , 0 ,
!
/COM, LINES ARE CONNECTED BETWEEN KEYPOINTS LISTED BELOW
L, 1, 2
L, 2, 3
L, 3, 4
L, 4, 5
L, 5, 6
L, 6, 7
L, 7, 8
L, 8, 1
/COM, LINE FILLET FOR ALL THE CORNERS
LFILLT,2,3,ir, ,
LFILLT,6,7,ir, ,
LFILLT,3,4,ir+rt, ,
LFILLT,7,8,ir+rt, ,
!*
/COM, INPUT LINES FOR FACES AND LOAD APPLICATOR
L, 24, 9
L, 9, 10
L, 10, 11
L, 11, 12
L, 12, 5
L, 5, 24
L, 26, 13
L, 13, 14
L, 14, 15
L, 15, 16
L, 16, 1
L, 11, 17
L, 17, 18
L, 18, 12
L, 19, 26
L, 20, 25
L, 22, 23
L, 24, 21
!*
/COM, Define Element Types
ET,1,SOLID185
!KEYOPT,1,6,4
!*
ET,2,CONTA173
!*
/COM, Input Material Properties, #1 Orthotropic, #2 Isotropic
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,1,,7E+005
MPDATA,EY,1,,7E+005
MPDATA,EZ,1,,70000
MPDATA,PRXY,1,,0.2
MPDATA,PRYZ,1,,0.2
MPDATA,PRXZ,1,,0.45
MPDATA,GXY,1,,78000
MPDATA,GYZ,1,,78000
MPDATA,GXZ,1,,295000
!*
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,2,,29000000
MPDATA,PRXY,2,,0.26
/COM, Select areas
FLST,2,4,4
FITEM,2,16
FITEM,2,23
FITEM,2,24
FITEM,2,25
AL,P51X
FLST,2,6,4
FITEM,2,14
FITEM,2,15
FITEM,2,16
FITEM,2,17
FITEM,2,4
FITEM,2,13
AL,P51X
FLST,2,4,4
FITEM,2,6
FITEM,2,29
FITEM,2,4
FITEM,2,5
AL,P51X
FLST,2,4,4
FITEM,2,10
FITEM,2,28
FITEM,2,11
FITEM,2,29
AL,P51X
FLST,2,4,4
FITEM,2,7
FITEM,2,27
FITEM,2,3
FITEM,2,28
AL,P51X
FLST,2,4,4
FITEM,2,12
FITEM,2,26
FITEM,2,9
FITEM,2,27
AL,P51X
FLST,2,4,4
FITEM,2,8
FITEM,2,1
FITEM,2,2
FITEM,2,26
AL,P51X
FLST,2,6,4
FITEM,2,19
FITEM,2,20
FITEM,2,21
FITEM,2,22
FITEM,2,8
FITEM,2,18
AL,P51X
/COM, Extrude all areas to extrusion depth ed
FLST,2,8,5,ORDE,2
FITEM,2,1
FITEM,2,-8
VEXT,P51X, , ,0,0,-ed,,,,
/COM, Set Element Edge Sizes
!Rib
FLST,2,5,5,ORDE,5
FITEM,2,20
FITEM,2,24
FITEM,2,28
FITEM,2,32
FITEM,2,36
AESIZE,P51X,rt/5,
!flanges
FLST,5,12,4,ORDE,6
FITEM,5,30
FITEM,5,38
FITEM,5,-42
FITEM,5,67
FITEM,5,72
FITEM,5,-76
CM,_Y,LINE
LSEL, , , ,P51X
CM,_Y1,LINE
CMSEL,,_Y
!*
LESIZE,_Y1,tft/2, , , , , , ,1
!Through the depth
FLST,5,12,4,ORDE,12
FITEM,5,45
FITEM,5,-46
FITEM,5,50
FITEM,5,-51
FITEM,5,55
FITEM,5,-56
FITEM,5,60
FITEM,5,-61
FITEM,5,65
FITEM,5,-66
FITEM,5,70
FITEM,5,-71
CM,_Y,LINE
LSEL, , , ,P51X
CM,_Y1,LINE
CMSEL,,_Y
!*
LESIZE,_Y1, , ,ed*10, , , , ,1
/COM, Assign material properities
FLST,5,7,6,ORDE,2
FITEM,5,2
FITEM,5,-8
CM,_Y,VOLU
VSEL, , , ,P51X
CM,_Y1,VOLU
CMSEL,S,_Y
!*
CMSEL,S,_Y1
VATT, 1, , 1, 0
CMSEL,S,_Y
CMDELE,_Y
CMDELE,_Y1
CM,_Y,VOLU
VSEL, , , , 1
CM,_Y1,VOLU
CMSEL,S,_Y
!*
CMSEL,S,_Y1
VATT, 2, , 1, 0
CMSEL,S,_Y
CMDELE,_Y
CMDELE,_Y1
/COM, Create Coordinate systems to align material properties
Local,11,0,0,0,0,25,0,0
!Lower Corner
Local,12,0,0,0,0,50,0,0
!Flat rib section
Local,13,0,0,0,0,25,0,0
!Upper Corner
/COM, Call the coordinate system and material properties for volume 6
TYPE, 1
MAT, 1
REAL,
ESYS, 11
SECNUM,
/COM, Mesh Volume 6 the lower corner
CM,_Y,VOLU
VSEL, , , , 6
CM,_Y1,VOLU
CHKMSH,'VOLU'
CMSEL,S,_Y
!*
VSWEEP,_Y1
!*
CMDELE,_Y
CMDELE,_Y1
CMDELE,_Y2
/COM, Call the coordinate system and material properties for volume 5
TYPE, 1
MAT, 1
REAL,
ESYS, 12
SECNUM,
/COM, Mesh Volume 5 the flat rib section
CM,_Y,VOLU
VSEL, , , , 5
CM,_Y1,VOLU
CHKMSH,'VOLU'
CMSEL,S,_Y
!*
VSWEEP,_Y1
!*
CMDELE,_Y
CMDELE,_Y1
CMDELE,_Y2
/COM, Call the coordinate system and material properties for volume 4
TYPE, 1
MAT, 1
REAL,
ESYS, 13
SECNUM,
/COM, Mesh Volume 4 the upper corner
CM,_Y,VOLU
VSEL, , , , 4
CM,_Y1,VOLU
CHKMSH,'VOLU'
CMSEL,S,_Y
!*
VSWEEP,_Y1
!*
CMDELE,_Y
CMDELE,_Y1
CMDELE,_Y2
!*
/COM, Call the coordinate system and material properties for the flat sections and sweep them
TYPE, 1
MAT, 1
REAL,
ESYS, 0
SECNUM,
FLST,5,4,6,ORDE,4
FITEM,5,2
FITEM,5,-3
FITEM,5,7
FITEM,5,-8
CM,_Y,VOLU
VSEL, , , ,P51X
CM,_Y1,VOLU
CHKMSH,'VOLU'
CMSEL,S,_Y
!*
VSWEEP,_Y1
!*
CMDELE,_Y
CMDELE,_Y1
CMDELE,_Y2
!*
/COM, Call the coordinate system and material properties for the load applicator and sweep it
TYPE, 1
MAT, 2
REAL,
ESYS, 0
SECNUM,
CM,_Y,VOLU
VSEL, , , , 1
CM,_Y1,VOLU
CHKMSH,'VOLU'
CMSEL,S,_Y
!*
VSWEEP,_Y1
!*
CMDELE,_Y
CMDELE,_Y1
CMDELE,_Y2
!*
/COM, Apply symmetry conditions
FLST,2,24,5,ORDE,17
FITEM,2,1
FITEM,2,-9
FITEM,2,11
FITEM,2,13
FITEM,2,-14
FITEM,2,16
FITEM,2,-17
FITEM,2,20
FITEM,2,23
FITEM,2,-24
FITEM,2,28
FITEM,2,32
FITEM,2,36
FITEM,2,38
FITEM,2,40
FITEM,2,42
FITEM,2,44
DA,P51X,SYMM
/COM, Apply zero bottom displacement
FLST,2,1,5,ORDE,1
FITEM,2,43
!*
/GO
DA,P51X,UY,0
FLST,2,1,3,ORDE,1
FITEM,2,16
!*
/GO
DK,P51X, ,0, ,0,UX,UY,UZ, , , ,
/COM, Apply Load to top
/PREP7
FLST,2,1,5,ORDE,1
FITEM,2,12
/GO
!*
SFA,P51X,1,PRES,pressure
/COM, CONTACT PAIR CREATION - START
CM,_NODECM,NODE
CM,_ELEMCM,ELEM
CM,_KPCM,KP
CM,_LINECM,LINE
CM,_AREACM,AREA
CM,_VOLUCM,VOLU
/GSAV,cwz,gsav,,temp
MP,MU,1,
MAT,1
MP,EMIS,1,7.88860905221e-031
R,3
REAL,3
ET,3,170
ET,4,174
R,3,,,1.0,0.1,0,
RMORE,,,1.0E20,0.0,1.0,
RMORE,0.0,0,1.0,,1.0,0.5
RMORE,0,1.0,1.0,0.0,,1.0
KEYOPT,4,4,0
KEYOPT,4,5,0
KEYOPT,4,7,0
KEYOPT,4,8,0
KEYOPT,4,9,0
KEYOPT,4,10,1
KEYOPT,4,11,0
KEYOPT,4,12,0
KEYOPT,4,2,0
KEYOPT,3,5,0
! Generate the target surface
ASEL,S,,,19
CM,_TARGET,AREA
TYPE,3
NSLA,S,1
ESLN,S,0
ESURF
CMSEL,S,_ELEMCM
! Generate the contact surface
ASEL,S,,,27
CM,_CONTACT,AREA
TYPE,4
NSLA,S,1
ESLN,S,0
ESURF
ALLSEL
ESEL,ALL
ESEL,S,TYPE,,3
ESEL,A,TYPE,,4
ESEL,R,REAL,,3
/PSYMB,ESYS,1
/PNUM,TYPE,1
/NUM,1
EPLOT
ESEL,ALL
ESEL,S,TYPE,,3
ESEL,A,TYPE,,4
ESEL,R,REAL,,3
CMSEL,A,_NODECM
CMDEL,_NODECM
CMSEL,A,_ELEMCM
CMDEL,_ELEMCM
CMSEL,S,_KPCM
CMDEL,_KPCM
CMSEL,S,_LINECM
CMDEL,_LINECM
CMSEL,S,_AREACM
CMDEL,_AREACM
CMSEL,S,_VOLUCM
CMDEL,_VOLUCM
/GRES,cwz,gsav
CMDEL,_TARGET
CMDEL,_CONTACT
/COM, CONTACT PAIR CREATION - END
!*
/COM, CONTACT PAIR CREATION - START
CM,_NODECM,NODE
CM,_ELEMCM,ELEM
CM,_KPCM,KP
CM,_LINECM,LINE
CM,_AREACM,AREA
CM,_VOLUCM,VOLU
/GSAV,cwz,gsav,,temp
MP,MU,1,0
MAT,1
R,4
REAL,4
ET,5,170
ET,6,174
KEYOPT,6,9,0
KEYOPT,6,10,1
R,4,
RMORE,
RMORE,,0
RMORE,0
! Generate the target surface
ASEL,S,,,45
CM,_TARGET,AREA
TYPE,5
NSLA,S,1
ESLN,S,0
ESURF
CMSEL,S,_ELEMCM
! Generate the contact surface
ASEL,S,,,33
CM,_CONTACT,AREA
TYPE,6
NSLA,S,1
ESLN,S,0
ESURF
ALLSEL
ESEL,ALL
ESEL,S,TYPE,,5
ESEL,A,TYPE,,6
ESEL,R,REAL,,4
/PSYMB,ESYS,1
/PNUM,TYPE,1
/NUM,1
EPLOT
ESEL,ALL
ESEL,S,TYPE,,5
ESEL,A,TYPE,,6
ESEL,R,REAL,,4
CMSEL,A,_NODECM
CMDEL,_NODECM
CMSEL,A,_ELEMCM
CMDEL,_ELEMCM
CMSEL,S,_KPCM
CMDEL,_KPCM
CMSEL,S,_LINECM
CMDEL,_LINECM
CMSEL,S,_AREACM
CMDEL,_AREACM
CMSEL,S,_VOLUCM
CMDEL,_VOLUCM
/GRES,cwz,gsav
CMDEL,_TARGET
CMDEL,_CONTACT
/COM, CONTACT PAIR CREATION - END
FINISH
/SOLU
!*
ANTYPE,0
ANTYPE,0
NLGEOM,1
NSUBST,rsn,0,0
OUTRES,ERASE
OUTRES,ALL,ALL
AUTOTS,0
LNSRCH,1
NEQIT,100
PSTRES,1
RESCONTRL,DEFINE,ALL,ALL,rsn
TIME,pressure
/STATUS,SOLU
SOLVE
FINISH
/REPLOT
*DO,I,1,rsn-1,1
/POST1
PLNSOL, U,Y, 0,1.0
/WAIT,30
/POST1
SET,1,I,1,
ETABLE,STRS,S,X
ESEL,S,ETAB,STRS,SxMax
ESEL,A,ETAB,STRS,-100000,SxMin
ETABLE,STRS,S,Y
ESEL,A,ETAB,STRS,SyMax
ESEL,A,ETAB,STRS,-100000,SyMin
ETABLE,STRS,S,Z
ESEL,A,ETAB,STRS,SzMax
ESEL,A,ETAB,STRS,-100000,SzMin
ETABLE,STRS,S,XY
ESEL,A,ETAB,STRS,SxyMax,,1
ETABLE,STRS,S,YZ
ESEL,A,ETAB,STRS,SyzMax,,1
ETABLE,STRS,S,XZ
ESEL,A,ETAB,STRS,SxzMax,,1
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,ALL
ANTYPE,,REST,1,I,0
RESCONTRL,DEFINE,ALL,ALL,rsn-I
SOLVE
*ENDDO
FINISH
Sorry for length, but I'm not sure of how to post a file.
RE: Element death APDL code
I begin to understand what your code do. But I think there a small error in it. It has to be:
CODE
ESEL,A,ETAB,STRSyz,SyzMax,,,1
ESEL,A,ETAB,STRSxz,SxzMax,,,1
instead of
CODE
ESEL,A,ETAB,STRSyz,SyzMax,,1
ESEL,A,ETAB,STRSxz,SxzMax,,1
Is That correct ?
Second: I hope you are aware that etable works just for the selected elements. In the first do loop after
CODE
ETABLE,STRS,S,X
ESEL,S,ETAB,STRS,SxMax
ESEL,A,ETAB,STRS,-100000,SxMin
there are no elements selected. After that you define a new EMPTY table with:
CODE
Is that what you want?
RE: Element death APDL code
Unfortunately, doesn't seem to get me any different results. Here's what the loop looks like now.
CODE
/POST1
PLNSOL, U,Y, 0,1.0
/WAIT,30
SET,1,I,1,
ETABLE,STRS,S,X
ESEL,S,ETAB,STRS,SxMax
ESEL,A,ETAB,STRS,-100000,SxMin
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,ALL
/POST1
ETABLE,STRS,S,Y
ESEL,S,ETAB,STRS,SyMax
ESEL,A,ETAB,STRS,-100000,SyMin
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,ALL
/POST1
ETABLE,STRS,S,Z
ESEL,S,ETAB,STRS,SzMax
ESEL,A,ETAB,STRS,-100000,SzMin
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,ALL
/POST1
ETABLE,STRS,S,XY
ESEL,S,ETAB,STRS,SxyMax,,,1
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,ALL
/POST1
ETABLE,STRS,S,YZ
ESEL,S,ETAB,STRS,SyzMax,,,1
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,ALL
/POST1
ETABLE,STRS,S,XZ
ESEL,S,ETAB,STRS,SxzMax,,,1
ESEL,R,MAT,,1
/SOLU
EKILL,ALL
ESEL,ALL
ANTYPE,,REST,1,I,0
RESCONTRL,DEFINE,ALL,ALL,rsn
SOLVE
*ENDDO