Damage2p

From OpenSeesWiki
Revision as of 04:01, 26 September 2012 by Fmk (talk | contribs) (Created page with '{{CommandManualMenu}} This command is used to construct a three-dimensional material object that has a Drucker-Prager plasticity model coupled with a two-parameter damage model....')
(diff) ← Older revision | Latest revision (diff) | Newer revision → (diff)
Jump to navigation Jump to search



This command is used to construct a three-dimensional material object that has a Drucker-Prager plasticity model coupled with a two-parameter damage model.

nDMaterial Damage2p $matTag $fcc <-fct $fct> <-E $E> <-ni $ni> <-Gt $Gt> <-Gc $Gc> <-rho_bar $rho_bar> <-H $H> <-theta $theta> <-tangent $tangent>
$matTag integer tag identifying material
$fcc concrete compressive strength
$fct optional concrete tensile strength
$E optional Young modulus
$ni optional Poisson coefficient
$Gt optional tension fracture energy density
$Gc optional compression fracture energy density
$rho_bar ptional parameter of plastic volume change
$H optional linear hardening parameter for plasticity
$theta optional ratio between isotropic and kinematic hardening
$tangent optional integer to choose the computational stiffness matrix


The material formulations for the Damage2p object are "ThreeDimensional" and "PlaneStrain"

This code has been Developed by: Leopoldo Tesser - Dept. DICEA - Univeristy of Padua - Italy, contact leopoldo.tesser AT dicea.unipd.it

NOTES

1. Admissible values: The input parameters vary as follows:

$fcc negative real value (positive input is changed in sign automatically)
$fct positive real value (for concrete like materials is less than $fcc)
$Gt positive real value (integral of the stress-strain envelope in tension)
$Gc positive real value (integral of the stress-strain envelope after the peak in compression)
$rhoBar positive real value 0=rhoBar<sqrt(2/3)
$H positive real value (usually less than $E)
$theta positive real value 0=$theta=1 (with: 0 hardening kinematic only and 1 hardening isotropic only
$tangent 0: computational tangent; 1: damaged secant stiffness (hint: in case of strong nonlinearities use it with Krylov-Newton algorithm)


  1. Default values: The Damage2p object hve the following defualt parameters:
$fct = 0.1*abs(fcc)
$E = 4750*sqrt(abs(fcc)) if abs(fcc)<2000 because fcc is assumed in MPa (see ACI 318) = 57000*sqrt(abs(fcc)) if abs(fcc)>2000 because fcc is assumed in psi (see ACI 318)
$ni' = 0.15 (from comparison with tests by Kupfer Hilsdorf Rusch 1969)
'$Gt = 1840*fct*fct/E (from comparison with tests by Gopalaratnam and Shah 1985)
$Gc = 6250*fcc*fcc/E (from comparison with tests by Karsan and Jirsa 1969)
$rhoBar = 0.2 (from comparison with tests by Kupfer Hilsdorf Rusch 1969)
$H = 0.25*E (from comparison with tests by Karsan and Jirsa 1969 and Gopalaratnam and Shah 1985)
'$theta = 0.5 (from comparison with tests by Karsan and Jirsa 1969 and Gopalaratnam and Shah 1985) _ $tangent = 0

Example

This example provides the input file and corresponding results for a confined triaxial compression (CTC) test using a single 8-node brick element and the Drucker-Prager constitutive model. A schematic representation of this test is shown below, (a) depicts the application of hydrostatic pressure, and (b) depicts the application of the deviator stress. Also shown is the stress path resulting from this test plotted on the meridian plane. As shown, the element is loaded until failure, at which point the model can no longer converge, as this is a stress-controlled analysis. 

#########################################################
#							#
# File is generated for the purposes of testing the	#
#	Drucker-Prager model --> conventional triaxial 	#
#				 compression test	#
#							#
#   Created:  03.16.2009 CRM				#
#   Updated:  12.02.2011 CRM				#
#							#
# ---> Basic units used are kN and meters		#
#							#
#########################################################

#-------------------------------------------------------
# create the modelBuilder and build the model
#-------------------------------------------------------
wipe

model BasicBuilder -ndm 3 -ndf 3

#--create the nodes
node 1	1.0	0.0	0.0
node 2	1.0	1.0	0.0
node 3 	0.0	1.0	0.0	
node 4	0.0	0.0	0.0
node 5	1.0	0.0	1.0
node 6 	1.0	1.0	1.0
node 7 	0.0	1.0	1.0
node 8 	0.0	0.0	1.0

#--triaxial test boundary conditions
fix 1 	0 1 1
fix 2 	0 0 1
fix 3	1 0 1
fix 4 	1 1 1
fix 5	0 1 0
fix 6 	0 0 0
fix 7	1 0 0
fix 8 	1 1 0

#--define material parameters for the model
#---bulk modulus
	set k       27777.78
#---shear modulus
	set G       9259.26
#---yield stress
	set sigY    5.0
#---failure surface and associativity
	set rho     0.398
	set rhoBar  0.398
#---isotropic hardening
	set Kinf    0.0
	set Ko 	    0.0
	set delta1  0.0
#---kinematic hardening
	set H 	    0.0
	set theta   1.0
#---tension softening
	set delta2  0.0
#---mass density
        set mDen    1.7

#--material models
#	   type	         tag  k   G   sigY   rho   rhoBar   Kinf   Ko   delta1   delta2   H   theta   density 
nDMaterial DruckerPrager 2    $k  $G  $sigY  $rho  $rhoBar  $Kinf  $Ko  $delta1  $delta2  $H  $theta  $mDen

#--create the element
#	type	 tag  nodes		matID  bforce1  bforce2  bforce3
element stdBrick 1    1 2 3 4 5 6 7 8   2      0.0      0.0      0.0

puts "model Built..."

#-------------------------------------------------------
# create the recorders
#-------------------------------------------------------
set step 0.1

# record nodal displacements
recorder Node -file displacements1.out -time -dT $step -nodeRange 1 8 -dof 1 2 3 disp

# record the element stress, strain, and state at one of the Gauss points
recorder Element -ele 1 -time -file stress1.out  -dT $step  material 2 stress
recorder Element -ele 1 -time -file strain1.out  -dT $step  material 2 strain
recorder Element -ele 1 -time -file state1.out   -dT $step  material 2 state

puts "recorders set..."

#-------------------------------------------------------
# create the loading
#-------------------------------------------------------

#--pressure magnitude
set p 10.0
set pNode [expr -$p/4] 

#--loading object for hydrostatic pressure
pattern Plain 1 {Series -time {0 10 100} -values {0 1 1} -factor 1} { 
	load 1  $pNode 	0.0	0.0
	load 2  $pNode	$pNode	0.0
	load 3  0.0	$pNode  0.0
	load 5  $pNode  0.0	0.0
	load 6  $pNode	$pNode	0.0
	load 7 	0.0	$pNode	0.0
}

#--loading object deviator stress
pattern Plain 2 {Series -time {0 10 100} -values {0 1 5} -factor 1} { 
	load 5  0.0	0.0	$pNode
	load 6  0.0	0.0	$pNode
	load 7  0.0	0.0	$pNode
	load 8  0.0	0.0	$pNode
}

#-------------------------------------------------------
# create the analysis
#-------------------------------------------------------

integrator LoadControl 0.1
numberer RCM
system SparseGeneral
constraints Transformation
test NormDispIncr 1e-5 10 1
algorithm Newton
analysis Static

puts "starting the hydrostatic analysis..."
set startT [clock seconds]
analyze 1000

set endT [clock seconds]
puts "triaxial shear application finished..."
puts "loading analysis execution time: [expr $endT-$startT] seconds."

wipe

References

Tesser L.,"Efficient 3-D plastic damage model for cyclic inelastic analysis of concrete structures", Report of the University of Padua, Italy, 2012. (soon available at paduareserach.cab.unipd.it)

Petek K.A., "Development and application of mixed beam-solid models for analysis of soil-pile interaction problems", Ph.D. dissertation, Univerisity of Washington, USA, 2006

Retrieved from "https://opensees.ist.berkeley.edu/wiki/index.php?title=Damage2p&oldid=10104"