Modeling of shearwall using ShellMITC4 element

[snehalhk]

I am modeling a simple shearwall using ShellMITC4 element. The programme is working fine. But when i model the same wall using SAP2000 the result does not match. Can you please guide me where i am doing mistake while programming in OpenSEES. I am attaching the input file of openSEES. Thanks in advance.

#\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\

# Units = kN , m , sec

wipe
model BasicBuilder -ndm 3 -ndf 6
file mkdir Shearwall

# Nodes for shearwall:

node 1 0.0 0.0 0.0
node 2 3.0 0.0 0.0
node 3 3.0 0.0 3.0
node 4 0.0 0.0 3.0
node 5 3.0 0.0 6.0
node 6 0.0 0.0 6.0
node 7 3.0 0.0 9.0
node 8 0.0 0.0 9.0
node 9 3.0 0.0 12.0
node 10 0.0 0.0 12.0
node 11 3.0 0.0 15.0
node 12 0.0 0.0 15.0



fix 1 1 1 1 1 1 1
fix 2 1 1 1 1 1 1


#Shear wall section
section ElasticMembranePlateSection 1 25000000 0.2 0.15 0


# shear wall elements
element shellMITC4 1 1 2 3 4 1
element shellMITC4 2 4 3 5 6 1
element shellMITC4 3 6 5 7 8 1
element shellMITC4 4 8 7 9 10 1
element shellMITC4 5 10 9 11 12 1



# define LATERAL load -------------------------------------------------------------
# Lateral load pattern
pattern Plain 1 Linear {
load 11 5 0.0 0.0 0.0 0.0 0.0
load 12 5 0.0 0.0 0.0 0.0 0.0
}

# Define RECORDERS -------------------------------------------------------------
recorder Node -file Shearwall/DFree.out -time -node 11 12 -dof 1 2 3 4 5 6 disp; # displacements of free nodes
recorder Node -file Shearwall/DBase.out -time -node 1 2 -dof 1 2 3 4 5 6 disp; # displacements of support nodes
recorder Node -file Shearwall/RBase.out -time -node 1 2 -dof 1 2 3 4 5 6 reaction; # support reaction
recorder Node -file Shearwall/FNode.out -time -node 1 2 3 4 5 6 7 8 9 10 11 12 -dof 1 2 3 4 5 6 reaction
recorder Element -file Shearwall/stress1.out -time -ele 1 2 3 4 5 stresses


constraints Plain
numberer RCM
system BandGeneral
test NormDispIncr 1.0e-9 20
algorithm Newton
integrator LoadControl 1
analysis Static
analyze 1

puts "Done!"

Thanks and regard
Snehal Kaushik
Ph.D Scholar
IIT Guwahati, India

[fmk]

if the script is working, then either your model or the sap model is incorrect or the discretization of the mesh is not fine enough to capture differences in the mechanics of the models. it is basically plane stress problem you have so why use shell elements in the first place? also it's an elastic model, you might as well use a Linear solution algorithm as well (you will not notice it here, but when you get to a large model the coe will run a lot faster).

here is an example that is used to verify the shell element (also quad and brick elements) for the case of an elastic planar wall that is used in the ETABS verification manual.
http://opensees.berkeley.edu/WebSVN/fil ... arWall.tcl

when i run it i get:

PlanarShearWall.tcl: Verification of Linear Elastic Planar Shear Wall

- using Quad elements
# Stories Wall Height Wall Length ETABS SAP2000 OpenSees Difference
6 720 120 2.3926 2.4287 2.4293 0.0006
6 720 360 0.0985 0.1031 0.1032 0.0001
6 720 720 0.0172 0.0186 0.0187 0.0001
3 360 120 0.3068 0.3205 0.3212 0.0007
3 360 360 0.0169 0.0187 0.0187 0.0000
3 360 720 0.0046 0.0052 0.0052 0.0000
1 120 120 0.0144 0.0185 0.0187 0.0002
1 120 360 0.0024 0.0029 0.0029 0.0000
1 120 720 0.0011 0.0013 0.0013 0.0000

- using Shell elements
#Stories Wall Height Wall Length ETABS SAP2000 OpenSees Difference
Using ShellMITC4 - Developed by: Leopoldo Tesser, Diego A. Talledo, Veronique Le Corvec
6 720 120 2.3926 2.4287 2.4279 0.0008
6 720 360 0.0985 0.1031 0.1032 0.0001
6 720 720 0.0172 0.0186 0.0187 0.0001
3 360 120 0.3068 0.3205 0.3210 0.0005
3 360 360 0.0169 0.0187 0.0187 0.0000
3 360 720 0.0046 0.0052 0.0052 0.0000
1 120 120 0.0144 0.0185 0.0187 0.0002
1 120 360 0.0024 0.0029 0.0029 0.0000
1 120 720 0.0011 0.0013 0.0013 0.0000

- using Brick elements
#Stories Wall Height Wall Length ETABS SAP2000 OpenSees Difference
6 720 120 2.3926 2.4287 2.4270 0.0017
6 720 360 0.0985 0.1031 0.1031 0.0000
6 720 720 0.0172 0.0186 0.0187 0.0001
3 360 120 0.3068 0.3205 0.3207 0.0002
3 360 360 0.0169 0.0187 0.0187 0.0000
3 360 720 0.0046 0.0052 0.0052 0.0000
1 120 120 0.0144 0.0185 0.0187 0.0002
1 120 360 0.0024 0.0029 0.0029 0.0000
1 120 720 0.0011 0.0013 0.0013 0.0000

PASSED Verification Test PlanarShearWall.tcl

[snehalhk]

Thanks a lot for your valuable comments. I tried the same wall making it finer mesh using Shell element. Now the deflection and base reactions are matching with the SAP2000 results but the stresses are still not matching. Can you please explain how the stresses are recorded in openSEES. If any research paper is there explaining the stress behaviour will be helpful for me.

Thanks and regards,
Snehal

[snehalhk]

I suppose that the stresses we are getting in shell element is calculated at integration points. Kindly confirm.
If we need to calculate at nodal points, we have to do it manually or there is any other simple method.

Thanks and regards,
Snehal

[fmk]

the stresses are recorded at the gauss points. manual calculation is required if you want them at the nodes.

[ospinag]

Did somebody worked how to interpolate shell stresses from gauss points to nodal points? I've tried a simple 2D interpolation using matlab, but when comparing the stresses of two elements with common nodes, it can be seen that the error is very high using this interpolation. I guess I'll have to use the Gauss legendre interpolation to work this out, but I've not been able to find the proper expression. Is it as simple as inverting displacement interpolation problem x = N(e,s)*xi ? Thanks!