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:
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.
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
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,