

May 16, 2022 at 8:47 amJanneSubscriber
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 solidshell 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 thinwalled 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 ! 4Node 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
! Load
esel,s,type,,2
nsle
sf,all,pres,1.0e003
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 ! 8Node 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
! Load
esel,s,type,,2
nsle
sf,all,pres,1.0e003
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

May 16, 2022 at 9:00 amErik KostsonAnsys EmployeeHi
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

May 16, 2022 at 9:03 amJanneSubscriberI 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.

May 16, 2022 at 10:12 amErik KostsonAnsys EmployeeYou 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).

May 16, 2022 at 10:14 amJanneSubscriberI understand. However, there are no nodes present there. Are there any other possibilities to do this than using 2 elements thicknesswise? Or are you saying that I can add lines at the midplane and restrain those?

May 16, 2022 at 10:35 ampeteroznewmanSubscriberIf 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.

May 16, 2022 at 10:40 amJanneSubscriberThank 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 solidshell to match with identical boundary conditions.
I consider this to be resolved.

 The topic ‘SHELL181 and SOLSH190 result difference’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 How to do the frequency response of the nonlinear vibration of a flexible PCB?
 Importing Line and Solid Bodies from SpaceClaim to Mechanical
 how to open SendCommand in Ansys
 problems facing during solution
 Still facing the same issue
 Failed to move file from solver directory to scratch directory: file.rst
 Adaptive Sizing
 Stiffness factor
 Import DAT file
 Import pressure data (coordinates and value) to ansys workbench through excel

8808

4658

3153

1688

1478
© 2023 Copyright ANSYS, Inc. All rights reserved.