Learning Forum

[nhossain]

Dear Support Engineers:

Is it permissible to use Shell Element (Shell 181) with Beam Element (Beam 188)? I am trying to explain the problem at my best capacities. Please see the image below.

Laminate_Bending_Trial_1.txt

[peteroznewman]

ANSYS Staff are not permitted to open attachments.
You can send a collection of replies to put sections of your code to show that. It won't all fit in a single post. Here is the first part down to !! Model Geometry
!
finish
/clear
/prep7


!! Element type and material's property
et,1,181 !! Shell element 181, 4-node structural shell
!! Used for Composite Shell


keyopt,1,1,0 !! Bending and Membrane Stiffness
keyopt,1,3,2 !! Full Integration
keyopt,1,8,1 !! Store data for Top and Bottom for all layers
!! Multi-layer elements
keyopt,1,9,0 !! No user sub-routine


!! Material Properties, Graphite Epoxy
mptemp,1,0 !! Temperature for material properties
!! 1 -- staring location
!! 0 -- T1 = 0


mpdata,ex,1,,126e3 !! Material properties data
!! ex -- Ex
!! 1 -- Mat. ID
!! ,, -- Starting location of the data
!! Default -- last location + 1
!! Ex = 126 GPa = 126e3 MPa, for Graphite Epoxy


mpdata,ey,1,,11e3 !! Material properties data
mpdata,ez,1,,126e3 !! Material properties data


mpdata,prxy,1,,0.28 !! Material properties data
mpdata,pryz,1,,0.024 !! Material properties data
mpdata,prxz,1,,0.28 !! Material properties data


mpdata,gxy,1,,6.6e3 !! Material properties data, Gxy = 6.6 MPa
mpdata,gyz,1,,4.57e3 !! Material properties data
mpdata,gxz,1,,6.6e3 !! Material properties data

[peteroznewman]

!! Model geometry
rectng,0,1000,0,1000 !! 1 m x 1 m block
!! 1000 mm x 1000 mm block


!! Shell layer stacking
sectype,1,shell !! Section type
!! 1 -- Section ID
!! Shell -- Section Type


!! Laminate type
!! [0/60/-60]s


secdata,2,1,0,3 !! Section data
!! 2 -- Thickness, 2 mm = 2e-3 m
!! 1 -- Material ID
!! 0 -- Angle or orientation
!! 3 -- # of integration points
secdata,2,1,60,3
secdata,2,1,-60,3
secdata,2,1,-60,3
secdata,2,1,60,3
secdata,2,1,0,3


secoffset,mid !! Shell nodes will be offset to midplane of the section


!! Make mesh
esize,,50


type,1
mat,1
asel,all
amesh,all


!! Now, use Beam Element
et,2,188 ! 2D Beam element 188
sectype,2,beam,csolid! Section type
! 1 - section id, user defined
! beam -- type of section
! csolid -- subtype
secdata,5 ! Section data
! 5 -- radius, mm
!


!! Material, steel
mp,ex,2,200e9 !! ex -- 200e9 MPa = 1e6 x 200e3 MPa
mp,prxy,2,0.3 !! prxy -- item name


!! Make FE model
esize,,50


!! Recall ID
type,2
mat,2
Lmesh,2




nummrg,all

[peteroznewman]

!! Boundary Condition
!! See lines and area
/pnum,line,1
lplot
/pnum,area,1
aplot


!! Apply Symm BC
dl,1,1,symm !! dl -- dof at lines
!! 1 -- line # 1
!! 1 -- area # 1, area connected with line # 1
!! symm -- Symmetric


dl,4,1,symm


!! Apply Simple Supported BC
dl,2,1,uz,0 !! uz = 0
dl,3,1,uz,0 !! uz = 0




!! Select a desired node at Beam
nsel,s,loc,x,1000
nsel,r,loc,y,500
nlist


f,all,fx,1000 !! This could be a force or moment load




allsel
eplot
finish


/solution
solve
finish


/post1
set,last
layer,1
shell,top
plnsol,u,sum


!!
set,last
nsel,s,loc,x,1000
prrsol


!! Select the desired layer
set,last
layer,1
shell,top
plnsol,s,x


layer,2
shell,top
plnsol,s,x


layer,3
shell,top
plnsol,s,x

[ErKo]

thanks for posting the input.

The error message is super clear I believe (shell section nr 1 does not go on beams). So a command is missing which tells apdl to use section nr 2. for the beams (now it is using sec 1 which is a shell section, hence the error msg) so add:

secnum,2

to
mat,2
type,2
....
so before meshing the beams.