## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Stress or Strain data not available for nodes of REINF264

• mer153
Subscriber

Hi,

I want to select nodes on a reinforcement line body (REINF264) using the line of code below:

nsel,R,S,EQV,0

This doesn't select any nodes. However, if I change the criterion to displacement (nsel,R,U,X,0), then it can select the required nodes based on the defined criterion on the line body.

Why using the stress or strain criterion, I cannot select any nodes? My conjecture is that the stress or strain values are not either available or defined for these nodes. Is this correct?

• Bill Bulat
Ansys Employee

Yes, it looks like REINF264 calculates only component stress results:

• mer153
Subscriber

Dear Bill,

Thank you for your help. This makes a lot of sense.

NSEL command for the stress only accepts the following components:

X, Y, Z, XY, YZ, XZ  ---> Component stress.

1, 2, 3 ---> Principal stress

Eqv ---> Equivalent stress

Would you please tell me how we can get the principal stress values (Sx in your figure) if our line elements are oriented in different directions (not necessarily in the X direction).

Thank  you

• mer153
Subscriber

If I remove the component term “X” and update the code as (nsel,R,S,,4000), then the code works. What I want to do after selecting these nodes is to find elements that all their nodes are part of the selected list of nodes and kill these elements. However, now I have two other problems. Please let me know if you suggest creating a new post for these questions.

My first question is why there is no correspondence between the calculated stress values and the defined criterion for selecting the nodes. I defined the stress threshold of 4000 (I am not sure if the units are Pa) for the selection of the nodes of REINF elements and performed the simulation. I expected to see that when the max principal stress of the REINF elements exceeds 4000 Pa, the solver selects these elements to apply further operations on them using the next lines of code. However, I can see that they are selected even if the stress values of the REINF elements are much lower than this threshold.

I want to perform the EKILL command on the elements that have the selected node in the previous step. So, I added the following lines to my code (esln,S,1, ekill, all). Although the ESLN command options “,1” is stating that only elements that all their nodes are selected by the NSEL command should be selected, I see that some neighboring solid264 elements are also selected, and EKILL command is performed on them as well. This is happening while before using the (nsel,R,S,,4000) I selected only REINF264 elements by (esel,s,type,,3). Type 3 elements in the ELIST are REINF264 elements.

I can share an example case with you through ANSYS Customer portal if you deem it helpful.

• Bill Bulat
Ansys Employee

The APDL test case input at the bottom of this post illustrates a way, by selecting discreet REINF264 element table stress results (rather than nodes), to identify fibers whose SX stresses have exceeded some allowable stress. SX is always the axial component of REINF264 stress (regardless of the orientation of the REINF264 relative to the global X axis).

Copy the APDL below into a text file and read that text file into an interactive MAPDL session with the /INPUT command.

An alternative to using EKILL might be to define a material damage law for your REINF264:

I can see from the table below that material damage laws are supported by REFINF264:

Yet another (probably easier) option might be to define bilinear isotropic or kinematic hardening laws for your REINF264 (I see these options in the table above too).

fini
/cle

/vie,1,1,1,1
/vup,1,z
/esha,1
/pnu,type,1
/num,1

/sys,del file*.png

/title,FIBER REINFORCED CANTILEVER BEAM

C*******************************************
C*** PARAMETERS
C*******************************************
l=0.100 ! LENGTH
t=0.005 ! THICKNESS
w=0.010 ! WIDTH

a_f=(t/10)**2 ! FIBER CROSS SECTION AREA

E_m=2e11/1e3 ! MATRIX ELASTIC MODULUS
nu_m=0.3 ! MATRIX POISSON'S

E_f=2e11/1e1 ! FIBER ELASTIC MODULUS
nu_f=0.2 ! FIBER POISSON'S

esz=t/5 ! MATRIX MESH SIZE
dvz=5 ! MESH DIVISIONS IN Z (THICKNESS) DIRECTION

u_tip=0.01 ! ENFORCED DISPLACEMENT OF BEAM TIP

s_failure=0.15e9 ! FIBER FAILURE STRESS

C*******************************************
C*** MODEL
C*******************************************
/prep7
n,1,,w/2,t/2 ! REMOTE POINT NODES
n,2,l,w/2,t/2

bloc,,l,,w,,t ! BEAM GEOMETRY

et,1,185 ! MATRIX ATTRIBUTES
mp,ex,1,E_m
mp,nuxy,1,nu_m

lsel,s,leng,,t ! MESH
lesi,all,,,dvz
alls
vmes,all

C*******************************************
C*** REMOTE PTS AT BEAM ENDS
C*******************************************
et,2,174
keyo,2,4,1 ! FORCE DISTRIBUTED
keyo,2,2,2 ! MPC
keyo,2,12,5 ! BONDED

et,3,170
keyo,3,2,1 ! USER-SPECIFIED PILOT NODE CONSTRAINT
keyo,3,5,3 ! SHELL-SOLID

r,2

real,2
type,2
nsel,s,loc,x
nsel,u,node,,1
esurf

type,3
tsha,pilo
alls
e,1

d,1,all

et,4,174
keyo,4,4,1 ! FORCE DISTRIBUTED
keyo,4,2,2 ! MPC
keyo,4,12,5 ! BONDED

et,5,170
keyo,5,2,1 ! USER-SPECIFIED PILOT NODE CONSTRAINT
keyo,5,5,3 ! SHELL-SOLID

r,4

real,4
type,4
nsel,s,loc,x,l
nsel,u,node,,2
esurf

type,5
tsha,pilo
alls
e,2

d,2,ux
d,2,uy
d,2,uz,-u_tip
d,2,rotx
d,2,roty
d,2,rotz

C*******************************************
C*** REINFORCING
C*******************************************
et,6,264
mp,ex,6,E_f
mp,nuxy,6,nu_f
sect,6,reinf,disc
secd,6,a_f,edgo,1,0.5,0.5,0.5,0.5
mat,6
secn,6
esel,s,type,,1
ereinf

esel,s,ename,,264
eplo

C*******************************************
C*** SOLVE
C*******************************************
/solu
nsub,5,5,5
outr,all,all
nlge,on
alls
solv
fini

C*******************************************
C*** POST PROCESS REINF264
C*******************************************
/post1
set,last

esel,s,ename,,264
plns,s,x,2
/sho,png \$plns,s,x,2 \$/sho,close \$/wait,2

etab,sx,s,x
esel,u,etab,sx,-s_failure,s_failure
plns,s,x,2
/sho,png \$plns,s,x,2 \$/sho,close \$/wait,2

Best,

Bill