Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations GregLocock on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Element death APDL code 1

Status
Not open for further replies.
YoungTurk

YoungTurk

Mechanical
Jul 16, 2004
333
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.

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
 
Replies continue below

Recommended for you

Sort by date Sort by votes
Hi,

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
 
Upvote 0 Downvote
Thanks for the comment Alex. I don't think I can/should select all the elements before my esel & etable commands because the purpose of the commands is to select elements which have exceeded maximum stress values in order to kill them. I notice that the selection and ekill routine works just fine the first time through the loop; but doesn't seem to work at all after that, so I'm inclined to think my problem has something to do with my restart or antype controls...

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.
 
Upvote 0 Downvote
OK, tried the ALLSEL command before the solve, and still have the same problem; the element selection and ekill routine only runs the first time through. After that its like its not even in the code. Why would that happen?

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. ???
 
Upvote 0 Downvote
Look at the stresses in the 2nd substep. I guess your selection bounds are wrong. Do the selection command by command an see what it hapens, if the elements are selected.

Alex
 
Upvote 0 Downvote
Even if the bounds are wrong (not sure why you say that), something should be happening which is different than running the solution without and elements killed, right? I am getting some elements selected when I manually enter the code into the command line, as well as when I run the loop, but only the first time through in that case (I'm basing this on watching the output window).

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!
 
Upvote 0 Downvote
Here's the whole enchilada, if you wanna give it a try. Insert some legal disclaimer here about not making a million bucks off this hacked together 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.
 
Upvote 0 Downvote
Hi,

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,STRSxy,SxyMax,,,1
ESEL,A,ETAB,STRSyz,SyzMax,,,1
ESEL,A,ETAB,STRSxz,SxzMax,,,1

instead of

Code: 
ESEL,A,ETAB,STRSxy,SxyMax,,1
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: 
SET,1,I,1, 
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: 
ETABLE,STRS,S,Y

Is that what you want?


 
Upvote 0 Downvote
Nice catches! Have adjusted accordingly.

Unfortunately, doesn't seem to get me any different results. Here's what the loop looks like now.

Code: 
*DO,I,1,rsn-1,1
 	/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
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

rcbsimoes
  • Locked
  • Question
ansys apdl, etab, max per row
Replies
1
Views
402
rcbsimoes
rcbsimoes
rcbsimoes
  • Locked
  • Question
Shared Faces in Ansys APDL
Replies
0
Views
273
rcbsimoes
rcbsimoes
H
  • Question
Plasticity behaviour is not being computed in a non-linear analysis in ANSYS Mechanical APDL 2024 r2
Replies
0
Views
1K
hmsilva
H
dixdax
  • Locked
  • Question
Ansys APDL arrays
Replies
0
Views
186
dixdax
dixdax
md_salem
  • Locked
  • Question
how to write a parameter in APDL code inside workbench file ? 1
Replies
15
Views
543
md_salem
md_salem

Part and Inventory Search

Sponsor

Back
Top Bottom