General Mechanical

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

SHELL181 and SOLSH190 result difference

TAGGED: ,

• Janne
Subscriber

Hello,

I have modeled a thin plate with 3000 x 3000 x 10 mm dimensions in a static structural analysis using mechanical APDL. I have applied an uniform pressure of 0.001 MPa on the surface. I have made two separate models; 1) one with SHELL181 elements and 2) one with SOLSH190 element. The boundary conditions are:

1) applied to all edges of the shells; ux=uy=uz=0, rotations free

2) applied to four edges of the solid-shell top surface; ux=uy=uz=0.

I except the same results between the models but for some reason I do not get that.

Maximum deflection for SHELL181 model = 53.4639 mm

Maximum deflection for SOLSH190 model = 26.3438 mm

I do not understand why I get the difference as these should be comparable in thin-walled structures. Could someone shed some light please?

I have put the code below for both cases:

SHELL181:

/prep7

longside = 3000

shortside = 3000

! Keypoints, keypoint,number,x,y,z

K,1,0,0,0

K,2,longside,0,0

K,3,longside,shortside,0

K,4,0,shortside,0

! Area

A,1,2,3,4

! MAT properties

mp,ex,1,70e3      ! Young's modulus Material ID 1

mp,prxy,1,0.23     ! Poisson's ratio Material ID 1

! Define Elements

et,1,181 ! 4-Node SHELL181 element, Element ID 1

et,2,154

keyop,2,7,0        ! Use deformed area for application of load

! Element properties for Spacers

sectype,5,shell

secdata,10,1

secoff,mid

! Mesh Pane 1

type,1         ! Element ID

mat,1          ! Material ID

secnum, 5

esize,50 ! Element size

amesh,1

asel,s,loc,z,0

nsla,s,1

esel,all

type,2

esurf

allsel

esel,s,type,,2

nsle

sf,all,pres,1.0e-003

allsel

! Boundary condition

lsel,s,line,,1,4        ! Select

nsll,s,1          ! Select all nodes connected to lines, incl ends

d,all,ux,0       ! Translation x direction is constant (0)

d,all,uy,0       ! Translation y direction is constant (0)

d,all,uz,0       ! Translation z direction is constant (0)

allsel           ! Select all

finish           ! Finish with /prep7

/solu            ! Enters the solution processor

antype,static        ! Analysis type, static structural

nlgeom,off         ! Large Deflection, on/off

solve            ! Starts a Solution

finish

/Post1

set,last

SOLSH190:

/prep7

longside = 3000

shortside = 3000

thickness = 10

! Keypoints, keypoint,number,x,y,z

K,1,0,0,thickness

K,2,longside,0,thickness

K,3,longside,shortside,thickness

K,4,0,shortside,thickness

K,5,0,0,0

K,6,longside,0,0

K,7,longside,shortside,0

K,8,0,shortside,0

! Volumes

V,1,2,3,4,5,6,7,8 !V1

! MAT properties

mp,ex,1,70e3      ! Young's modulus Material ID 1

mp,prxy,1,0.23     ! Poisson's ratio Material ID 1

! Define Elements

et,1,190 ! 8-Node SOLSH190 element, Element ID 1

et,2,154

! Mesh Pane 1

type,1         ! Element ID

mat,1          ! Material ID

esize,50 ! Element size

VEORIENT,1,KP,5,1

vmesh,1

asel,s,loc,z,thickness

nsla,s,1

esel,all

type,2

esurf

allsel

esel,s,type,,2

nsle

sf,all,pres,1.0e-003

allsel

! Boundary condition

lsel,s,line,,1,4        ! Select

nsll,s,1          ! Select all nodes connected to lines, incl ends

d,all,ux,0       ! Translation x direction is constant (0)

d,all,uy,0       ! Translation y direction is constant (0)

d,all,uz,0       ! Translation z direction is constant (0)

allsel           ! Select all

finish           ! Finish with /prep7

/solu            ! Enters the solution processor

antype,static        ! Analysis type, static structural

nlgeom,off         ! Large Deflection, on/off

solve            ! Starts a Solution

finish

/Post1

set,last

• Erik Kostson
Ansys Employee
Hi

These comparisons have been done before - see here for some examples (search the below on the internet):
Comparison of ANSYS elements SHELL181 and SOLSH190

All the best

Erik

• Janne
Subscriber
I know they have done before, and they show good agreement with each other. This is exactly why I do not understand what is wrong with my model.
• Erik Kostson
Ansys Employee
You need to restrain the solsh190 as in the shell181 - so in the midplane of the solid part and not on the top and bottom face/edges (thus you need lines at the midplane of the solid part). If we do that then it is fine and the same. Or if you offset the shell181 to top or bottom (instead of middle).
• Janne
Subscriber
I understand. However, there are no nodes present there. Are there any other possibilities to do this than using 2 elements thickness-wise? Or are you saying that I can add lines at the midplane and restrain those?
• peteroznewman
Subscriber
If you fix rotations of the edge nodes on the shell181 model, it will be more like the fixed displacements of the top and bottom edge nodes of the solsh190 model.
• Janne
Subscriber
Thank you This seems to be true. I suppose this is just the problem with the nature of the solid element, that we cannot achieve the idealized boundary condition that we can with shell element at the midplane.
However, I discovered something interesting. If you I use geometry nonlinearity, and subject top and bot surface of solid elements to only uz=0, and prevent rigid body motion at the middle node of the plate, then I can get nonlinear solution between shell and nonlinear solid-shell to match with identical boundary conditions.
I consider this to be resolved.