×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Getting reaction forces on ANSYS (APDL) LS-DYNA - Explicit Dynamics Analysis

Getting reaction forces on ANSYS (APDL) LS-DYNA - Explicit Dynamics Analysis

Getting reaction forces on ANSYS (APDL) LS-DYNA - Explicit Dynamics Analysis

(OP)
Good day to all,
I'm trying to simulate honeycomb crushing in ANSYS Mechanical APDL with LS-DYNA.
The solution runs fine and I can animate the result without problem.
However, I can't get either structural forces from /POST1 and, most importantly, can't get reaction forces from /POST26.
I'm using a SHELL163 element and I tried using the manual to extract information without success.
Here's the code I'm using up to the solve command:

CODE -->

NOM_ARC	=	'Honeycomb'
/FILNAM,NOM_ARC				 

/DELETE,NOM_ARC,BCS			
/DELETE,NOM_ARC,esav
/DELETE,NOM_ARC,full
/DELETE,NOM_ARC,mntr
/DELETE,NOM_ARC,rst
/DELETE,NOM_ARC,stat
/DELETE,file,page

KEYW,PR_STRUC,1


L	= 	3.175E-3		
H	= 	0.015			
T	=	5.08E-5			
ANG	=	30			
PI	=	ACOS(-1)	
ANR	=	ANG*PI/180		

K	= 	10   


E	=	67E9			
P	=	0.33			
RHO 	=	2700			

FRIS	=	0.3			
FRID	=	0.2			
ELE_TIP	=	'SHELL163'
		

ELE_OPT1=	0		
ELE_OPT2=	0		
ELE_OPT3=	0		
ELE_OPT4=	0		

MSH_KEY	=	1			
ELE_SIZ =	3E-4			

TIEMPO = 	1.2e-3			

/PREP7


ET,1,ELE_TIP				
KEYOP,1,1,ELE_OPT1
KEYOP,1,2,ELE_OPT2
KEYOP,1,3,ELE_OPT3
KEYOP,1,4,ELE_OPT4

*SET,_RC_SET,1, 
R,1 
RMODIF,1,1,5/6,3,T,T,T,T,  		

MP,DENS,1,RHO		

MP,EX,1,E		

MP,NUXY,1,P		
TB,EOS,1,,,1,1

TBDATA,1,350.25e6
TBDATA,2,275e6
TBDATA,3,.36
TBDATA,4,.022
TBDATA,5,1.0
TBDATA,6,1400
TBDATA,7,30
TBDATA,8,10
TBDATA,9,4500
TBDATA,10,0
TBDATA,11,-.8
TBDATA,12,2.1
TBDATA,13,-.5
TBDATA,14,.0002
TBDATA,15,.61
TBDATA,16,140e9

EDMP,RIGI,2,0,0		

MP,DENS,2,RHO*10000		

MP,EX,2,E		

MP,NUXY,2,P	

K,1,0,0,0
K,2,-L*cos(ANR)+L/2*tan(ANR),0,0
K,3,L/2*tan(ANR),L/2,0
K,4,L/2*tan(ANR),-L/2,0
K,5,0,0,H
K,6,-L*cos(ANR)+L/2*tan(ANR),0,H
K,7,L/2*tan(ANR),L/2,H
K,8,L/2*tan(ANR),-L/2,H

K,9,-0.005,-0.005,H+0.001
K,10,0.005,-0.005,H+0.001
K,11,0.005,0.005,H+0.001
K,12,-0.005,0.005,H+0.001

L,1,2   !L1
L,1,3   !L2
L,1,4   !L3
L,1,5   !L4
L,5,6   !L5
L,5,7   !L6
L,5,8   !L7
L,2,6   !L8
L,3,7   !L9
L,4,8   !L10

L,9,10  !L11
L,10,11 !L12
L,11,12 !L13
L,12,9  !L14


AL,1,8,5,4	!A1
AL,2,9,6,4	!A2
AL,3,10,7,4	!A3

AL,11,12,13,14	!A4

MAT,1	
TYPE,1	
MSHKEY,MSH_KEY
ESIZE,ELE_SIZ
AMESH,1	
AMESH,2	
AMESH,3	

MAT,2
TYPE,1	
MSHKEY,MSH_KEY
ESIZE,ELE_SIZ
AMESH,4

ESEL,S,MAT,,1  
NSLE,S  
CM,HONEYCOMB,NODE   
ALLSEL,ALL 

ESEL,S,MAT,,2  
NSLE,S  
CM,PLACA,NODE   
ALLSEL,ALL


EDCGEN,ANTS,HONEYCOMB,PLACA,FRIS,FRID,0,0,0, , , , ,0,10000000 	

EDCGEN,ASSC, , ,FRIS,FRID,0,0,0, , , , ,0,10000000,0,0	 

FINISH	
		
/SOLU

LSEL,S,LOC,Z,0
NSLL,S,1
D,ALL,ALL,0,
ALLSEL,ALL

EDINT,3,4


LSEL,S, , ,       8 
NSLL,S,1
CM,BORDE8,NODE
ALLSEL,ALL

EDBOUND,ADD,SLIDE,BORDE8,-L*cos(ANR)+L/2*tan(ANR),0,0,

LSEL,S, , ,       9 
NSLL,S,1
CM,BORDE9,NODE				
ALLSEL,ALL

EDBOUND,ADD,SLIDE,BORDE9,L/2*tan(ANR),L/2,0,

LSEL,S, , ,       10 
NSLL,S,1
CM,BORDE10,NODE
ALLSEL,ALL

EDBOUND,ADD,SLIDE,BORDE10,L/2*tan(ANR),-L/2,0,

EDVEL,VELO,PLACA,0,0,-K,0,0,0, , , , , ,   

TIME,TIEMPO,

SOLVE 

Sorry for the fact some parameters are in Spanish.
I'm specifically trying to get the reaction forces in the base of the Y over the analysis time with the Time-History Postprocessor, but when I try to add one of the nods for analysis the data appears to be invalid.
Also, even if I try to get the structural forces using the general postprocessor, it says that info is not available.

Can you please help me and tell me how I can get that info?
Many Thanks.

RE: Getting reaction forces on ANSYS (APDL) LS-DYNA - Explicit Dynamics Analysis

Did you figure this out?

RE: Getting reaction forces on ANSYS (APDL) LS-DYNA - Explicit Dynamics Analysis


issure the below command before solving,


/SOLU

EDRST,50
EDHTIME,500
EDOPT,ADD,,BOTH ! Write results files for both ANSYS and LS-DYNA postprocessors
EDENERGY,1,1,1,1
EDOUT,GLSTAT ! global statistics data
EDOUT,MATSUM ! material energy summary (on Part ID basis)
EDOUT,SPCFORC ! single point constraint (reaction) forces
EDOUT,RCFORC ! resultant interface forces
EDOUT,SLEOUT ! sliding interface energies data
EDOUT,RBDOUT ! rigid body data (UX, VX, AX, etc.)
EDDBL,DOUBLE ! Selects a numerical precision type (Single is default)

!!!Then.......
FINISH
/POST26
FILE,'PRIMARY_model','HIS','.'
KEYW,LSDYNA_H,1
/UI,COLL,1
NUMVAR,200
SOLU,191,NCMIT
STORE,MERGE
EDREAD,2,GLSTAT
STORE,MERGE
XVAR,1
PLVAR,3,4,7,8,11,17,

EDREAD,2,RCFORC,2, , ,
XVAR,1
PLVAR,4,

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources