Download mate.notice
Back to the list
Display this manual page in
$$$$ MATE NOTICE BR232186 13/12/09 21:15:20 7841
DATE 13/12/09
Operateur MATE Voir aussi : MODE CARA
-------------- ACIER
IDENTI
PROPAG
TRACTUFI
Description :
___________
The MATE (MATERIAU) operator creates a field of material and/or
geometrical properties. The elements requiring material or
geometrical properties can either be computed all at once
by means of the MATE operator, or separately by means of the
MATE operator for the material properties and the CARA operator
for the geometrical ones before merging the two fields by means
of the ET operator.
The following parts describe the material properties on the one
hand, and the geometrical ones on the other.
****************************
* *
* MATERIAL PROPERTIES *
* *
****************************
There are two possible syntaxes for describing the material
properties depending on whether the material is isotropic, or not.
----------------------------------------------
| 1st syntax : ISOTROPIC materials |
----------------------------------------------
MAT1 = MATE MODL1 NOMCi VALi ... ;
Contents :
__________
MODL1 : model object (MMODEL type)
NOMCi : name of the ith parameter (MOT type) (see below)
VALi : value(s) of the ith parameter (ENTIER, FLOTTANT,
MCHAML, EVOLUTION or LISTMOTS types)
Note 1 : the LISTMOTS type is provided for components
which have to be evaluated by the external users's
subroutine COMPUT, called by the VARI operator.
In this case, the LISTMOTS object gives the list of
the parameters upon the component depends.
Note 2 :if VaLi is a MCHAML object it must be in agreement
with the MODEL, i.e. they must have the same mesh object.
To do so it is possible to start whit a CHPOINT and to
change it in a MCHAML by CHAN operator. Or it is possible
to do like in the cham_vari example
(see exemple : cham_vari.dgibi)
MAT1 : object containing the material properties (MCHAML
type, CARACTERISTIQUES subtype)
Every case
___________
------------------------------------
| Parameter name for any material |
------------------------------------
a) Case of a MECANIQUE formulation
__________________________________
-----------------------------------------------------
| Parameter name for an ELASTIQUE ISOTROPE material |
-----------------------------------------------------
'YOUN' : Young's modulus
'NU ' : Poisson's ratio
'RHO ' : density
'ALPH' : thermal expansion coefficient
'VISQ' : viscosity coefficient
Case of isotropic and elastic joint elements :
- for elastic 2D joint elements, only the
isotropic case is permitted. The NOMCi parameter names to
be input for a 2D joint element are the following :
'KS ' : shear stiffness ( N/m3 )
'KN ' : normal stiffness ( N/m3 )
'RHO ' : density ( kg/m2 )
'ALPN' : thermal expansion coefficient in the normal direction
with respect to the joint ( m/K )
Note : even if the values for KS and KN are identical, they
must be input twice.
- for isotropic and elastic 3D joint elements,
both the shear stiffnesses are identical. The names to be
input are the same as those of the isotropic 2D case.
-----------------------------------------------------
| Parameter name for an ELASTIQUE ARMATURE material |
-----------------------------------------------------
This model concerns the tendons of reinforced concrete (BARR on SEG2)
In the case of passive tendons, the parameters are :
'YOUN' : Young's modulus
'SECT' : section of the tendon
In the case of active tendons (surrounding concrete), the
additionnal parameters to be defined are :
For the loss of prestress by frottement :
'FF ' : ratio of angular frottement (0.18 rd-1)
'PHIF' : ratio of linear frottement (0.002 m-1)
For the loss of prestress at the anchoring point :
'GANC' : sliding at the anchoring point (0.0)
For the loss of tensile stress of the tendon :
'RMU0' : ratio of the loss of tensile stress of the tendon (0.43)
'FPRG' : stress of warranted rupture (1700.e6 Pa)
'RH10' : loss of tensile stress after 1000 hours (2.5 %)
-------------------------------------------------------
| Parameter name for an ELASTIC NON_LINEAIRE material |
-------------------------------------------------------
Elastic model NON_LINEAIRE EQUIPLAS :
-----------------------------------
'TRAC' : key word followed by :
NOMTRAC : tension curve consisting of an EVOLUTIO type
object, with the strains in abscissa, and the
stresses in ordinate. It must contain as first
point, the point (0,0) and as second point, the
yield limit point. It may be drawn by means
of the DESSINE instruction.
NON_LINEAIRE UTILISATEUR model :
------------------------------
The list of the material components is the one defined by the
LISTMOTS object given behind the keyword 'C_MATERIAU' in the
syntax of the MODE operator.
---------------------------------------------------
| Parameter name for an ELASTO-PLASTIQUE material |
---------------------------------------------------
The following parameters will be specified BESIDES those relative
to the elastic behavior. The available plasticity models are the
following :
Plastic model PARFAIT :
-----------------------
'SIGY' : elastic limit
Plastic model with ISOTROPE stress hardening :
---------------------------------------------
'TRAC' : key word followed by :
NOMTRAC : tension curve consisting of an EVOLUTIO type
object, with the strains in abscissa, and the
stresses in ordinate. It must contain as first
point, the point (0,0) and as second point, the
yield limit point. It may be drawn by means
of the DESSINE instruction.
Plastic model with CINEMATIQUE LINEAIRE stress hardening :
----------------------------------------------------------
'SIGY' : elastic limit
'H ' : stress hardening modulus
Plastic model with CHABOCHE type stress hardening :
----------------------------------------------------
The equations for this model are as follows:
--> Notation : S stress tensor
Xi variables of kinematic stress hardening
(i=1 or 2)
EP plastic deformation tensor
p accumulated equivalent plastic deformation
J2 second invariant for deviatoric stresses
--> Criterion : J2 (S-X) = R(p)
--> Stress : dXi = Ci * (2/3 * Ai * PHI(p) * dEP - Xi*dp )
hardenings dR = B * (RM - R ) dp
with : X = X1 for a single centre
X1+X2 for two centres
R(0)=R0
PHI(p)= 1 + (PSI-1)* e**(-OMEG*p)
The data to be input are :
Case of 1 centre without isotropic stress hardening :
'A ','C' : parameters connected with the centre evolution
'PSI ','OMEG' : parameters connected with the reference term
'R0 ' : elastic limit
Case of 1 centre with isotropic stress hardening :
'A ','C : parameters connected with the centre evolution
'PSI ','OMEG' : parameters connected with the reference term
'R0 ' : initial elastic limit
'RM ' : final elastic limit
'B ' : constant connected with the elastic limit
evolution
Case of 2 centres without isotropic stress hardening:
'A1 ','C1 ' : parameters connected with the 1st-centre evolution
'A2 ','C2 ' : parameters connected with the 2nd-centre evolution
'PSI ','OMEG' : parameters connected with the reference term
'R0 ' : elastic limit
Case of 2 centres with isotropic stress hardening:
'A1 ','C1 ' : parameters connected with the 1st-centre evolution
'A2 ','C2 ' : parameters connected with the 2nd-centre evolution
'PSI ','OMEG' : parameters connected with the reference term
'R0 ' : initial elastic limit
'RM ' : final elastic limit
'B ' : constant connected with the elastic limit evolution
Plastic model of DRUCKER-PRAGER PARFAIT type :
---------------------------------------------
'LTR ' : limit in simple tension
'LCS ' : limit in simple compression
In that case, the criterion used is :
ALFA * Tr(S) + Seq = K
with : S stress tensor
Seq Von Mises equivalent stress
ALFA = ( |LCS| - LTR ) / ( |LCS| + LTR )
K = 2. * |LCS| * LTR / ( |LCS| + LTR )
Flow rule is associated.
Plastic model of DRUCKER-PRAGER type:
-------------------------------------
The equations of the model are as follows :
--> Notations : S stress tensor
Seq Von Mises equivalent stress
p cumulated equivalent plastic strain
--> initial criterion : ALFA * Tr(S) + BETA * Seq = K
--> ultimate criterion : ETA * Tr(S) + MU * Seq = KL
--> Hardening : dK = H * dp ( H in algebraic value)
--> Flow potential : GAMM * Tr(S) + DELT * Seq
The parameters to define are:
ALFA, BETA, K, ETA, MU, KL, H, GAMM, DELT
BETON model in plane stresses (2D or thin shells)
-------------------------------------------------
('LTR1') : limit in tension in the 1st direction (YOUN*1.2E-4
by default)
('ETR1') : failure strain in tension in the 1st direction
(by default 3*LTR1/YOUN)
('LTR2') : limit in tension in the 2nd direction (by default
LTR1)
('ETR2') : failure strain in tension in the 2nd direction
(by default 3*LTR2/YOUN)
('BETR') : reduction coefficient for the shear modulus in case of
cracking (between 0. and 1., 0.1 by default)
('VF1X') : two components pertaining to the VF1 vector which
('VF1Y') specify the direction connected with LTR1 (respectively
1. and 0. by default)
('LCS ') : limit in simple compression (YOUN*1.2E-3 by default)
('ECS ') : failure strain in simple compression
(10*LCS/YOUN by default)
('LBIC') : limit in bi-compression
BETON model in plane strains, axisymmetrical and 3D
----------------------------------------------------
In this model, the concrete behavior is non-linear in the field
of tensions, and linear everywhere else.
('LTR1') : limit in tension in the 1st direction (YOUN*1.2E-4
by default)
('ETR1') : failure strain in tension in the 1st direction
(3*LTR1/YOUN by default)
('LTT1') : transitional limit in tension in the 1st direction
(0. by default)
('ETT1') : deformation corresponding to LTT1 (ETR1 by default)
('ERS1') : residual deformation in tension in the 1st direction
(0. by default)
('VF1X') : three components of the VF1 vector specifying the
('VF1Y') direction connected with LTR1
('VF1Z')
('LTR2') : limit in tension in the 2nd direction (by default LTR1)
('ETR2') : failure strain in tension in the 2nd direction
(3*LTR2/YOUN by default)
('LTT2') : transitional limit in tension in the 2nd direction
(0. by default)
('ETT2') : deformation corresponding to LTT2 (ETR2 by default)
('ERS2') : residual deformation in tension in the 2nd direction
(0. by default)
('VF2X') : three components of the VF2 vector specifying the
('VF2Y') direction connected with LTR2
('VF2Z')
('LTR3') : limit in tension in the 3rd direction (LTR1 by default)
('ETR3') : failure strain in tension in the 3rd direction
(3*LTR3/YOUN by default)
('LTT3') : transitional limit in tension in the 3rd direction
(0. by default)
('ETT3') : deformation corresponding to LTT3 (ETR3 by default)
('ERS3') : residual deformation in tension in the 3rd direction
(ERS1 by default )
('VF3X') : three components of the VF3 vector specifying the
('VF3Y') direction connected with LTR3, required solely in 3D
('VF3Z') when necessary.
('BETR') : residual reduction coefficient for the shear modulus
in case of cracking (between 0. and 1., 0.1 by default)
Caution : The VF1, VF2 and VF3 vectors must be orthogonal.
--------
For a computation with a tension limit
different from the two others, it is required that the
vector corresponding to this limit VF1, VF2 or VF3
be defined.
When LTR1, LTR2 and LTR3 are given, both the VF1 and
VF2 vectors are required to define the directions 1, 2
and 3.
Non-zero values corresponding to initial cracks openings
in the directions 1, 2 and 3 can be introduced by means
of the TAB1 table used in the NONLIN procedure thanks to
TAB1.'VARI'.'OUV1', TAB1.'VARI'.'OUV2',
TAB1.'VARI'.'OUV3' may be input.
Ideal plastic model for the TUYAU FISSURE elements :
---------------------------------------------------
'SIGF' : yield stress
'J1C ' : value of J at initiation
'T ' : tearing modulus
Plastic hardening model for the TUYAU FISSURE elements:
------------------------------------------------------
'JDA ' : key word followed by :
NOMJDA : J-Da curve consisting of an EVOLUTIO type object
with the propagation in abscissa and J in ordinate.
'TRAC' : key word followed by :
NOMTRAC : tension curve consisting of an EVOLUTIO type object
with the rotations in abscissa (in radian), and the
moments in ordinate. The TRACTUFI procedure enables
the creation of such a curve in a case without
propagation. The PROPAG procedure enables the
creation of such a curve in a case with propagation.
Damage model for elastoplastic material (Lemaitre-Chaboche)
------------------------------------------------------------
Stress hardening and damage are isotropic. Von Mises'
criterion is coupled with damage
'TRAC' : key word followed by:
NOMTRAC : tension curve consisting of an EVOLUTIO type object
with the strains in abscissa and the stresses in
ordinate. It must contain the origin.
It may be drawn by means of the DESSINE instruction.
'EPSD' : Damage threshold: it is the plastic deformation
from which the material gets damaged.
'DC ' : critical value of the D variable describing
damage. DC features the material rupture
'EPSR' : plastic deformation with material rupture.
UBIQUITOUS model
----------------
It is a plasticity model for the materials bearing one or two
failure directions. According to the direction, the criterion
is of Mohr-Coulomb type with possibly non-associative flow.
This model only works in two dimensions.
'NCRI' : number of failure directions (1 or 2)
'ANG1' : 1st direction angle with Ox (in degrees)
'TRA1' : limit in tension along the 1st direction
'PHI1' : friction angle (in degrees)
'PSI1' : dilatance angle (in degrees)
('ANG2') |
('TRA2') |: same thing for the second direction
('PHI2') |
('PSI2') |
GAUVAIN model
--------------
It is a model of global plasticity for reinforced concrete
beams that are subjected mainly to bending loads.
'TRAC' : key word followed by:
NOMTRAC : tension curve(s) consisting of an EVOLUTIO type
object with strains in abscissa and stresses in
ordinate. Each curve must describe a moment-bending
law, from the negative values (4 points) to the
origin, to the positive values (4 points), a total
of 9 points. The moments are turned into stresses,
and the bendings into strains through the usual
formulas, by considering half the beam height as the
distance from the axis.
If a single curve is provided, it will be used for
the two bending directions.
The curves may be drawn by means of the DESSINE
instruction.
'SCOM' : elastic strain limit in compression
GLOBAL model
-------------
It is a global plasticity model for reinforced concrete beams
which makes it possible to take into account non linear behavior
laws according to the type of loading (axial, bending and
shear).
'COMP' : key word followed by :
NOMCOMP : behavior curve for axial loadings, composed of
an EVOLUTIO type object, with the displacements in
abscissa and axial forces in ordinate
'FLXY' : key word followed by :
NOMFLXY : behavior curve for flexural solicitations in the xOz
plane, composed of an EVOLUTIO type object, with
products (rotation * element length) in abscissa and
flexural moments in ordinate
'FLXZ' : key word followed by :
NOMFLXZ : behavior curve for flexural solicitations in the xOy
plane, composed of an EVOLUTIO type object, with
products (rotation * element length) in abscissa and
flexural moments in ordinate
'CISY' : key word followed by :
NOMCISY : behavior curve for shear solicitations in the xOy
plane, composed of an EVOLUTIO type object, with
displacements in abscissa and shear forces in ordinate
'CISZ' : key word followed by :
NOMCISZ : behavior curve for shear solicitations in the xOz
plane, composed of an EVOLUTIO type object, with
displacements in abscissa and shear forces in ordinate
Notes : - at least one law must be defined for each material
- for any material you can define only one law in bending
(FLXY or FLXZ) and one law in shear (CISY or CISZ);
- for behavior laws in tension-compression and in
bending, the finite element can be POUT or TIMO, for laws
in shear only the TIMO element can be used;
- the EVOLUTIO type objects must describe the laws from
the negative values (2 or 3 points) to the origin, to
the positive values (2 or 3 points), i.e. a total of
5 or 7 points
BA1D model
----------
It is a model for describing the cyclic behavior of reinforced concrete
columns subjected to uniaxial bending
'UELA' : displacement threshold to activate damage (1.0E-3)
'FPLA' : yielding threshold (100)
'HCIN' : kinematic modulus for plasticity (10)
'PFIS' : flow rule parameter for damage (0.3)
'QFRA' : flow rule parameter for damage (0.5)
'APIH' : flow rule parameter for sliding (1.0)
'BPIH' : flow rule parameter for sliding (5)
CAM_CLAY model
--------------
'E0 ' : initial void index
'M ' : friction coefficient
'COHE' : cohesion
'P0 ' : preconsolidation pressure
'KAPA' : elastic slope in an e-log(p) diagram
'LAMD' : plastic slope in an e-log(p) diagram
'G1 ' : shear modulus
HUJEUX model
------------
This model is suitable for sands and some clays. The equations
have the following form :
--> Notations : EE elastic strain tensor
EP plastic strain tensor
S stress tensor
ep trace(EP)
eq second invariant of EP
p trace(S)/3
q second invariant of deviatoric stresses
K1 bulk modulus
G1 shear modulus
--> elasticity : dp = K1*P1*((-p/P1)**N)*trace(dEE)
dq = 3*g1*P1*((-p/P1)**N)*dev(dEE)
--> Criterion : F = q/M*(COHE-p)
+ R * (B*ln((COHE-p)/(COHE+PC)*exp(-1./B)) - 1.)
--> Hardenings : R=R0+eq/(eq+A)
PC= (P0+COHE)*exp(-BETA*ep) - COHE
--> Plastic flow
potential : G = q/M*(COHE-p) + ln(COHE-p)
'M ' : friction coefficient
'COHE' : cohesion
'P0 ' : preconsolidation pressure (> 0.)
'E1 ' : reference elasticity modulus
'P1 ' : pressure associated with supplied value of E1
'BETA' : plastic bulk modulus
'A ' : coefficient in hardening law
'B ' : non zero coefficient
'R0 ' : initial value of R
'N ' : exponent in the non linear elastic law
(between 0. and 1., but different of 1.)
GURSON flow model
-----------------
The yield surface is defined by:
SIGeq - (SIGY+H.epse)*( 1+PORO**2-2*PORO*cosh(-1.5*P/SBAR) ) = 0
'SIGY' : initial flow stress for the non porous material
'H ' : work-hardening parameter
'SBAR' : heterogenous flow stress
'PORO' : initial porosity
JOINT_DILATANT model
--------------------
It is a joint model based on a Mohr-Coulomb criterion and
non associated flow rule.
'PHI ' : friction angle (used in the criterion)
'MU ' : dilatancy angle (used in the flow potential)
'FTRC' : maximum traction resistance
JOINT_SOFT model
----------------
It is a joint model based on a Mohr-Coulomb criterion with softening
in shear and tension and without dilatancy.
'PNOR' : Position of the edge of the cone
'SJTB' : Normal stress (traction) - joint opening relationship.
(EVOLUTION type - Positive value for tension)
'SJCB' : Normal stress (compression) - joint closing relationship.
(EVOLUTION type - Positive value for tension)
'SJSB' : Shear stress - joint sliding relationship for 0 normal stress
(EVOLUTION type)
'BETA' : Parameter controling the shear unloading
'CPLG' : Coupling definition
JOINT_COAT model
----------------
It is an isotropic shear joint model with a plasticity criterion, possible
softening and damage.
'SJSB' : Shear stress - joint sliding relationship (EVOLUTION type)
'BETA' : Parameter controling the shear unloading
ANCRAGE_ELIGEHAUSEN model
--------------------------
It is a joint model with bond slip uniaxial law for shear.
The monotonic behaviour is based on the Eligehausen model.
The joint behaviour remains elastic in tension.
(only in 2D plane stress, plane strain)
'S1T' : Sliding value at the beginning of the plateau
'S2T' : Sliding value at the end of the plateau
'S3T' : Sliding value at the end of softening
'T1T' : Maximum shear stress value
'T3T' : Residual shear stress after the end of softening
'ALFA' : Parameter defining the first part of the monotonic curve
(Suggested value: 0.4)
'PERI' : Perimeter of the steel bar
INTJOI model
---------------
The material parameters to be given as input as the following ones:
* Mechanical part (without corrosion)
'AD' : brittleness (1.0e-5)
'Y0' : initial threshold expressed in terms of energy rate (50)
'ALPA' : coupling coefficient for mode I/II (6)
'GAIN' : kinematic hardening coefficient 1 (2.0e9)
'AAIN' : kinematic hardening coefficient 2 (5.0e-7)
* Corrosion part
'Q1CO' : coefficient related to Gurson's criterion 1 (3.5)
'Q2CO' : coefficient related to Gurson's criterion 2 (0.9)
'Q3CO' : coefficient related to Gurson's criterion 3 (0.1)
'SYCO' : activation stress related to Gurson's criterion (-1.0e6 Pa)
'NCOE' : hardening coefficient 1 (2)
'KCOE' : hardening coefficient 2 (1.0e10)
'TC ' : macroscopic corrosion degree (steel cross section loss)
'GONF' : 0 if no swelling 1 otherwise. If 1, equivalent thermal strain
must be considered to load the steel/concrete interface.
* References
[1] B. Richard, F. RAgueneau, C. Cremona, L. Adelaie, JL Tailhan. (2010). A
three-dimensional steel/concrete model including corrosion effects. Eng
Fracture Mechanics. 77:951-973.
[2] L. Adelaide, B. Richard, F. Ragueneau, C. Cremona. (2010). Thermodynami
admissibility of a set of constitutive equations coupling elasticity,
isotropic damage and internal sliding. Comptes Rendus Mecanique. 338:1
COULOMB model
-------------
It is a dilatant joint model based on a Mohr-Coulomb criterion
and associated flow rule.
'EF ' : second normal stiffness
'ECN ' : strain limit below which the normal stiffness switches
from KN to EF (ECN should be input in absolute value)
'COHE' : cohesion (used in the criterion)
'FRIC' : friction angle (used in the criterion)
('FTRC') : maximum traction resistance (0. by default)
If used JOI1 elements, it's required to give:
'TYPE' : parameter to choose the kind of slip:
- = 1 : displacement
- = 2 : rotation
AMADEI model
------------
It is a non linear incremental joint model accounting for
a strain softening shear behaviour.
'FIMU' : friction angle between asperities
'SGMT' : limit value in pure compression
'I0 ' : initial inclination angle of the asperities
'S0 ' : cohesion
'B0 ' : ratio between residual and pic shear stresses for
low compression
'UP ' : tangential displacement value at pic shear stress
'UR ' : tangential displacement value associated with the
beginning of residual shear behaviour
'KNI ' : initial normal stiffness of the joint
'FI0 ' : residual friction angle of the asperities
'VM ' : normal displacement associated with maximum closure
of the joint, taken positive under compression
ACIER_UNI (steel) model
-----------------------
This is a modified Menegotto-Pinto uni-axial model, which accounts
for the steel buckling
'STSY' : yielding stress
'STSU' : ultimate stress
'EPSH' : hardening strain
'EPSU' : ultimate strain
'ROFA' : RO factor
'BFAC' : ratio between the hardening stiffness in cyclic behavior
and the elastic one
'A1FA' : A1 factor
'A2FA' : A2 factor
'FALD' : ratio between the length of the longitudinal bars
between stirrups and its diameter
'A6FA' : A6 factor
'CFAC' : C factor
'AFAC' : A factor
ACIER_ANCRAGE (anchorage) model
-------------------------------
This is a bond slip uniaxial law for anchorages or lap splices.
This law is based on the steel law PARFAIT_UNI and
the bond slip law ANCRAGE_ELIGEHAUSEN
This model is based on the equilibrium between the tension in the steel
bar
and the bond stress at the concrete-steel interface which are assumed
constant on the anchorage length. This eauilibrium is reached in an
iterative way.
'LANC' : Anchorage length
'SECT' : Section of a steel bar
- Parameters relative to the bond model
'G12' : Shear modulus
'S1T' : Sliding value at the beginning of the plateau
'S2T' : Sliding value at the end of the plateau
'S3T' : Sliding value at the end of softening
'T1T' : Maximum shear stress value
'T3T' : Residual shear stress after the end of softening
'ALFA' : Parameter defining the first part of the monotonic curve
(Suggested value: 0.4)
- Parameters relative to the steel model
'STSY' : yielding stress
'STSU' : ultimate stress
'EPSH' : hardening strain
'EPSU' : ultimate strain
'ROFA' : RO factor
'BFAC' : ratio between the hardening stiffness in cyclic behavior
and the elastic one
'A1FA' : A1 factor
'A2FA' : A2 factor
'FALD' : ratio between the length of the longitudinal bars
between stirrups and its diameter
'A6FA' : A6 factor
'CFAC' : C factor
'AFAC' : A factor
BETON_UNI (concrete) model
--------------------------
This is a Hognestad-like model, accounting for the confinment
'STFC' : maximum compression strength
'EZER' : strain corresponding to 'STFC'
'STFT' : maximum tension strength
'ALF1' : confinment parameter
'OME1' : confinment parameter
'ZETA' : slope of the descending part of the compression curve
'ST85' : stress defining the compression plateau
'TRAF' : factor defining the softening behaviour of the tension
curve
'STPT' : residual stress after complete cracking
Parameters defining the opening and closure of the crack
'FAMX' : F1 (definition of the closure point)
FAMX must be positive to have a physical meaning
If its value is taken negative, a stiff crack closure
is considered and the parameters STPT, FAMX, FACL, FAM1 and
FAM2
are not taken into account by the concrete model
'FACL' : F2 (definition of the point of complete opening)
'FAM1' : F1'(slope associated to F1)
'FAM2' : F2'(slope associated to F2)
FRAGILE_UNI model
------------------
This is a uniaxial damage based model with softening under
both tension and compression. The softening law is hyperbolic with
possible residual strength.
'FC ' : compressive strength
'FC_R' : residual strength under compression
'STRC' : strain controlling the softening behaviour
'FT ' : tensile strength
'FT_R' : residual strength under tension
'STRT' : strain controlling the softening behaviour under tension
BETON_BAEL model
-----------------
This is the concrete uniaxial law used in the french concrete
code BAEL
The model is plastic under compression (parabolic law) and
unilateral with no strength under tension.
'FC ' : compressive strength
MAZARS model
-------------
Same characteristics than the corresponding ENDOMMAGEABLE model
INTIMP model
------------
Corroded steel model accounting for steel/concrete interface
degradation with/without corrosion [1]. The steel model has been
developped by [2,3], the one related to the steel/concrete interface
is presented in [4]. The coupling is realized by the approach
proposed by [5]. The material parameters to be considered as input
are the following ones:
* Steel model:
'SOCT' : steel cross section
'SOGS' : elastic limit (400e6)
'DCS ' : critical damage (0.2)
'TCS ' : corrosion degree (steel cross section loss)
'MS ' : hardening exponent (2.786)
'KS ' : hardening factor (500e6)
* Steel/concrete interface model:
'GCEO' : Coulomb's modulus (15e9)
'AD ' : brittleness (7.5e-5)
'GAMC' : kinematic hardening coefficient 1 (7.0e9)
'ACOE' : kinematic hardening coefficient 2 (5.0e-7)
'LCCO' : anchorage length
'EPSC' : initial threshold (1.0e-4)
'TCI ' : corrosion degree (steel cross section loss)
'CALA' : computation indicator
= 0 if coupled model is used
= 1 if only the interface model is used (for calibration purposes)
= 2 if only the steel model is used
* References:
[1] B. Richard, F. Ragueneau, C. Cremona. (2010). A multifber approach
to describe the ultimate behaviour of corroded reinforced concrete
structures. Euro-C conference, Rohmoos/Schladming, Austria.
[2] A. Ouglova. (2010). Etude du comportement mecanique des structures en
arme ateintes par corrosion. These de L'ENS Cachan.
[3] B. Richard, F. RAgueneau, C. Cremona, L. Adelaie, JL Tailhan. (2010). A
three-dimensional steel/concrete model including corrosion effects. Eng
Fracture Mechanics. 77:951-973.
[4] L. Adelaide, B. Richard, F. Ragueneau, C. Cremona. (2010). Thermodynami
admissibility of a set of constitutive equations coupling elasticity,
isotropic damage and internal sliding. Comptes Rendus Mecanique. 338:1
[5] D. Combescure, F. Wang. (2007). Assessments of existing RC structures u
dynamic loading using non linear modeling. CONSEC 2007, Tours, France.
RICBET_UNI model
----------------
The material parameters to be given as input are the
following ones:
'HYST' : indicator to choose the type of crack closing criterion :
(1) if cracks close when the axial stress is equal to 0
(2) if cracks close when the axial strain is equal to 0
'FT ' : tension strength (2.1e6 MPa)
'ALDI' : brittleness in tension (4.0e-3)
'GAM1' : kinematic hardening modulus 1 (5.0e9)
'A1 ' : kinematic hardening modulus 2 (2.0e-6)
'SIGF' : closing stress (-3.0e6)
'FC ' : compression strength (10.0e6)
'AF ' : plastic modulus 1 (1.0)
'AG ' : plastic modulus 2 (1.0)
'AC ' : plastic isotropic modulus 1 (4.0e10)
'BC ' : plastic isotropic modulus 2 (600.0)
'SIGU' : asymptotic stress in compression (-6.0e6)
* References:
[1] B. Richard, F. Ragueneau (2012). 3D modelling of concrete for
earthquake analysis: damage mechanics and plasticity coupling.
WCCM 2012, Sao Paulo, Brazil.
[2] B. Richard, F. Ragueneau (2012). Continuum damage mechanics based
model for quasibrittle materials subjected to cyclic loadings:
formulation, numerical implementation and applications.
Engineering Fracture Mechanics. In press.
UNILATERAL model
----------------
Same characteristics than the corresponding ENDOMMAGEABLE model
PARFAIT_UNI model
------------------
This is a plastic model with kinematic hardening
which can be used for steel.
'SIGY' : yielding stress
'H ' : stress hardening modulus
PARFAIT_ANCRAGE model
--------------------
This is a uniaxial law for anchorages or lap splices.
This law is based on the steel law ACIER_UNI and
the bond slip law ANCRAGE_ELIGEHAUSEN
This model is based on the equilibrium between the tension in the steel
bar
and the bond stress at the concrete-steel interface which are assumed
constant on the anchorage length. This equilibrium is reached in an
iterative way.
'LANC' : Anchorage length
'SECT' : Section of a steel bar
- Parameters relative to the bond model
'G12' : Shear modulus
'S1T' : Sliding value at the beginning of the plateau
'S2T' : Sliding value at the end of the plateau
'S3T' : Sliding value at the end of softening
'T1T' : Maximum shear stress value
'T3T' : Residual shear stress after the end of softening
'ALFA' : Parameter defining the first part of the monotonic curve
(Suggested value: 0.4)
- Parameters relative to the steel model
'SIGY' : yielding stress
'H ' : stress hardening modulus
STRUT_UNI model
-----------------
This is a "Strut and Tie" non-linear shear model for the fibre
model.
The caracteristics of the concrete diagonal (material +
inclinaition) and the stirrups (material + quantity) must
be precised.
For concrete:
'STFC' : maximum compression strength
'EZER' : strain corresponding to 'STFC'
'STFT' : maximum tension strength
'ALF1' : confinment parameter
'OME1' : confinment parameter
'ZETA' : slope of the descending part of the compression curve
'ST85' : stress defining the compression plateau
'TRAF' : factor defining the softening behaviour of the tension
curve
'STPT' : residual stress after complete cracking
Parameters defining the opening and closure of the crack
'FAMX' : F1 (definition of the closure point)
'FACL' : F2 (definition of the point of complete opening)
'FAM1' : F1'(slope associated to F1)
'THET' : angle between the diagonal strut and the beam local axe
(unit: degrees)
For steel :
'YOUS' : Youn modulus of the steel
'STSY' : yielding stress
'STSU' : ultimate stress
'EPSH' : hardening strain
'EPSU' : ultimate strain
'ROFA' : RO factor
'BFAC' : ratio between the hardening stiffness in cyclic behavior
and the elastic one
'A1FA' : A1 factor
'A2FA' : A2 factor
'ROST' : Volumetric density of the stirrups
'EULT' : Ultimate strain used to compute the damage index
If abs(EULT)>1, the damage index is equal to 0.
If EULT<0, the index is a function of the maximale concrete
strain in compression
If EULT>0, the index is a function of the neutral axis depth
'CISAIL_NL' global model
-------------------------
This is a non-linear shear beam model with softening.
The shear strain-shear force law can be used with both a
Timoshenko element and as material model (for shear) for the
fibre model.
'DELP' : Limit strain of the elastic domain (positive strain)
'DELM' : Limit strain of the elastic domain (negative strain)
'DMAP' : Maximum damage value at the beginning of yielding
(positive strain)
'DMAN' : Maximum damage value at the beginning of yielding
(negative strain)
'BETA' : Pinching parameter (Beta = 0: pinching,
Beta= 1: No pinching)
'ALFA' : Strength degradation parameter under cyclic loading
'TETA' : Residual strength (fraction) after complete degradation
under cyclic loading
'MONP' : Evolution of the shear force (or the shear stress) in
function of the plastic strain (positive strain)
'MONN' : Evolution of the shear force (or the shear stress) in
function of the plastic strain (negative strain)
INFILL_UNI global model
------------------------
This is a non-linear strut model without strength in traction.
Behaviour in compression is based on damage and plasticity.
It is unilateral in traction/compression.
This law can be used with 2 strut elements as global model
of masonry infill panel.
'DELA' : Limit strain of the elastic domain
'DMAX' : Maximum damage value at the beginning of yielding
'BETA' : Pinching parameter (Beta = 0: pinching,
Beta= 1: No pinching)
'GAMM' : Reloading parammeter
'GAMP' : Reloading parameter
'ALFA' : Strength degradation parameter under cyclic loading
'TETA' : Residual strength (fraction) after complete degradation
under cyclic loading
'MONO' : Evolution of the compressive axial force in function of the
plastic strain (compression is positive)
OTTOSEN model with 3D modelisation
----------------------------------
('LTR') : limit stress in tension (default value YOUN*1.2E-4)
('GFTR') : restitued energy ratio
(also known as the fracturing energy)
(default value LTR*3.9E-5 but this value corresponds to
the international units system)
('GS') : modul providing the loose of resistance to shear of a
fracture with its normal opening.
(default value YOUN*1.8E-4, usual value is between 2 and
6 Mpa)
('BTR') : no recouvrable opening ratio (default value 0.2)
('LCS') : limit stress in simple compression
(by default, the behaviour is elastic in compression)
('LCBI') : limit in bi-compression
(default value 1.15*LCS)
('EPCM') : plastic deformation at peak, in simple compression
(default value 4.*LCS/(3.*YOUN))
('EPCU') : ultimate plastic deformation, in simple compression
(default value 5.*EPCM)
The CHAML result of the operator TAILLE applied to the model, must be
added to the CHAML built by MATE operator.
Moreover, in cases of plane strains or axisymetrical option, one can
also define :
('EPSR') : failure strain in the direction normal to the
modelisation plan.
BETON_INSA model
----------------
This concrete model works in plane stresses (2D or thin shells),
plane strains and axisymmetrical situations
('ALFA') : ratio between ultimate simple stresses in tension and
compression (.1 by default)
('LCS ') : limit stress in simple compression
(YOUN*1.E-3 by default)
('EMAX') : failure strain in simple compression
(10*LCS/YOUN by default)
('EPUT') : failure strain in simple tension
(by default 3*ALFA*LCS/YOUN)
('ICOM') : choice of the type behaviour inside the ultimate domain
ICOM = 0 : plastic behaviour with stress hardening
ICOM = 1 : elastic behaviour
(0 by default)
('FTC ') : reduction coefficient for the shear modulus in case of
cracking (between 0. and 1., 0.1 by default)
('GFTR') : tensile fracture energy (if 'EPUT' is not given
the default value for 'GFTR' is 0.15 ).
If GFTR is done its not necessery to give 'EPUT'.
Viscoplastic and rate dependent damage model for concrete in dynamic
BETON_DYNAR_LMT
--------------------------------------------------------------------
- BE CAREFUL the initial porosity influence the real young modulus
Km=YOUNG/(3*(1-2*NU))
Gm=YOUNG/(2*(1+NU))
- Compressibily and shear moduli with the porosity
(Mori-Tanaka)
Kporo=4*XKm*XGm*(1-f)/(4*XGm+3*XKm*f)
Gporo=XGm*(1-f)/(1+f*(6*XKm+12*XGm)/(9*XKm+8*XGm))
- Plasticity criterion FNT:
FNT = 3*J2(SIG) / SGM**2 + 2Q1f cosh(Q2 I1 / 2SGM) - (1+(Q3 f)**2)
- Plastic strain evolution:
EPSP = 1/(1-D)*(FNT/MVP)**NVP * dFNT/dSIG
- Porosity evolution:
Df = K * f/(1-f) * (FNT/MVP)**NVP
- Damage threshold function in tension and compression:
FDi = (EPSE - ED0 - 1/Ai*(Di/(1-Di))**(1/Bi))
- Damage evolution in tension and compression:
Di= (FDi/MDi)**NDi
Input data for the model in complement of the elacticity parameters
'F0' : Initial porosity of the concrete (0.3)
'Q1' : Parameter of the modified Gurson plasticity criterion
(0.5 to 2.)
'Q2' : Parameter of the modified Gurson plasticity criterion
(0.5 to 2.)
'Q3' : Parameter of the modified Gurson plasticity criterion
(0.5 to 2.)
'SGM0': Cement paste without pores resistance (70 Mpa)
'XN' : Exponent of the viscoplasticity threshold (15.)
'NVP' : Parameter of the Perzyna type viscoplasticity (1.5)
'MVP' : Parameter of the Perzyna type viscoplasticity (1.D-2)
'K' : Influence the porosity evolution (15 ^ 60)
'MDT' : Tension damage viscosity parameter (0.5D-4)
'NDT' : Tension damage viscosity parameter (5.)
'MDC' : Compression damage viscosity parameter (0.5D-3)
'NDC' : Compression damage viscosity parameter (20.)
'ED0' : Threshold in deformation for the tension (1.D-04)
'AC' : Parameter for the compression (3000)
'BC' : Parameter for the compression (4.)
'AT' : Parameter for the tension (20000)
'BT' : Parameter for the tension (1.6)
PARFAIT_INSA model
------------------
Perfect Plastic model for the decoupled orthotropic behavior
of thin shells
'SIG1' : elastic limit in the 1st orthotropic direction
'SIG2' : elastic limit in the 2nd orthotropic direction
ECROUIS_INSA model
------------------
Hardening plastic model for the decoupled orthotropic
behavior of thin shells
'TRA1' : key word followed by :
NOMTRA1 : tension curve in the 1st orthotropic direction
consisting of an EVOLUTION type object, with the
strains in abscissa, and the stresses in ordinate.
It must contain as first point, the point (0,0)
and as second point, the yield limit point.
'TRA2' : key word followed by :
NOMTRA2 : tension curve in the 2nd orthotropic direction
consisting of an EVOLUTION type object, with the
strains in abscissa, and the stresses in ordinate.
It must contain as first point, the point (0,0)
and as second point, the yield limit point.
BETOCYCL model
--------------
It is a plasticity model with two yield surfaces,
each one is defined by two mechanisms.
A part of the isotropic hardening of the compressive mechanim of
the external surface is function of the plastic flow due to the
internal surface. Both surfaces are defined by Rankyne-type
criteria with kinematic (internal yield surface) or isotropic
(external yield surface) hardening (or softening).
'HHH1' : Kinematic hardening modulus of the internal surface.
(FLOTTANT type)
'FTPE' : Initial tensile strength of the internal surface.
(FLOTTANT type)
'FCPE' : Initial compressive strength of the internal surface.
(FLOTTANT type)
'FTGR' : Initial tensile strength of the external surface.
(FLOTTANT type)
'FCGR' : Initial compressive strength of the external surface.
(FLOTTANT type)
'WOR0' : Reference cyclic work
(FLOTTANT type)
'TREV' : Law of the isotropic hardening parameter for the
tension mechanism (EVOLUTIO type)
'COEV' : Law of the isotropic hardening parameter for the
compression mechanism (EVOLUTIO type)
'LCAT' : Length associated to the tension law
(FLOTTANT type)
'LCAC' : Length associated to the compression law
(FLOTTANT type)
'EPSO' : Compressive strength degradation parameter (strain)
(FLOTTANT type)
Remarks:
1- The eight first parameters are identified by the IDENTI procedure
from the uniaxial tensile and compressive curves, the mesh and
the 3 other parameters.
2- The utilization of the associated length reduces the dependance
of the global results on the mesh size.
STEINBERG model
---------------
Constitutive equations :
Yielding limit Y :
Y = SIGY.(1+BETA.(P'+EPSI))**N.G/G0
and :
SIGY.(1+BETA.(P'+EPSI))**N < YMAX
with:
P': equivalent plastic strain
P'=sqrt(2/3.EP:EP)
EP: deviatoric plastic strains
G: shear modulus
shear modulus G :
G = G0+GP'.P/(ETA**(1/3))+GT'.(T-300)
G0 = YOUNG0 / ( 2*(1+NU0))
where : YOUNG0 is the initial Young modulus
NU0 is the Poisson's ratio (stay constant)
G0 is the initial shear modulus
TM=TM0*EXP(2.MU0.(1.-1./ETA))/( ETA ** (2./3.) )
and: if T>TM :
G = Y = 0
then, the volumetric strain is fully elastic and
the deviatoric strain is fully plastic
with:
P: hydrostatic pressure:
P=-trace(SIGMA)/3
SIGMA: stress
ETA:compression
ETA=RHO/RHO0
RHO,RHO0:density and initial density of the material
T: temperature expressed in Kelvin in this equation
The shear modulus G is expressed that way:
STRESS=HOOK.STRAIN i.e. D_STRESS=HOOK.D_STRAIN+D_HOOK.STRAIN
'SIGY' : initial yielding limit
'BETA' : hardening coefficient
'N' : hardening coefficient
'EPSI' : initial equivalent plastic strain
'GP' : rate of the evolution of the shear modulus with
the pressure ( no unity): GP'
'GT' : temperature-dependant term correcting the shear
modulus ( homogeanus to the shear modulus)
One enters here the term: GT'.(T-300) thanks to
the use of an EVOLUTION object (the parameter
of this EVOLUTION is the temperature).
'YMAX' : maximal yielding limit at constant shear modulus
'TMO' : melting temperature for ETA=1
'MU' : coefficient MU0 used for the calculation of the
melting temperature
ZERILLI model
-------------
Constitutive equations :
-Yielding limit Y for Face Centered Cubic materials (F.C.C.):
Y = DYG+C2'.sqrt(P').exp(-c3'.T+C4'.T.ln(EPT))+K.L**(-1/2)
-Yielding limit Y for Body Centered Cubic materials (B.C.C.):
Y = DYG+C1'.exp(-C3'.T+C4'.T.ln(EPT))+C5'.(P')**N+K.L**(-.5)
with:
T :temperature
P':equivalent plastic strain
P'=sqrt(2/3.EP:EP)
EP:plastic strains
EPT:equivalent strain rate
EPT=sqrt(2/3.ET:ET)
ET: strain rate
'DYG' : DYG term
'C1' : C1' coefficient
'C2' : C2' coefficient
'C3' : C3'.T term (C3' multiplicated by T) entered as
an EVOLUTION object
( the parameter is the temperature)
'C4' : C4'.T term (C4' multiplicated by T) entered as
an EVOLUTION object
( the parameter is the temperature)
'C5' : C5' coefficient
'N' : N coefficient
'K' : K coefficient
'L' : average grain diameter
'TYPE' : material structure
if the material is FCC: TYPE=0.
if the material is BCC: TYPE=1.
PRESTON model
-------------
Constitutive equations :
-shear modulus G :
G = G0+GP'.P/(ETA**(1/3))+GT'.(T-300)
G0 = YOUNG0 / ( 2*(1+NU0))
where : YOUNG0 is the initial Young modulus
NU0 is the Poisson's ratio (stay constant)
G0 is the initial shear modulus
ETA:compression
ETA=RHO/RHO0
TM=TM0*EXP(2.MU0.(1.-1./ETA))/( ETA ** (2./3.) )
and: if T>TM :
G = Y = 0 ( Y is the yield limit )
then, the volumetric strain is fully elastic and
the deviatoric strain is fully plastic
-Dimensionless terms:
Y' = Y/G
T' = T/TM
EPT'= EPT/X
with:
Y yielding stress
G shear modulus
T temperature
TM melting temperature
X = 1/6.(4/PI)**(.5).OMEGA
OMEGA: Debye's pulsation
OMEGA = (G/RHO)**(.5)
RHO:material's density
EPT: equivalent total strain rate
EPT=sqrt(2/3.ET:ET)
ET: total strain rate
-Dimensionless term for the saturation stress YS:
S1 = S0-(S0-SINF).erf(K'.T'.ln(g/EPT')
S2 = S0.(EPT'/g)**BETA
YS = max(S1,S2)
-Dimensionless term for the yielding limit YL:
L1 = Y0-(Y0-YINF).erf(K'.T'.ln(g/EPT')
L2 = Y1.(EPT'/g)**Y2
YL = max(L1,min(L2,S2))
-Dimensionless term for the yielding stress for
Body Centered Cubic materials (B.C.C.): P=0
Y' = YS-(YS-YL).exp(-TAU.EP/(YS-YL))
-Dimensionless term for the yielding stress for
the other materials: P differs from 0
Coeff1 = (S0-YL).(exp(P.(YS-YL)/(S0-YL))-1)
Coeff2 = 1-exp(-P.(YS-YL)/(S0-YL))
Y' = YS+(S0-YL)/P.ln(1-Coeff2.exp(-P.TAU.EP/Coeff1))
with:
EP: equivalent plastic strain
EP=sqrt(2/3.EPS:EPS)
EPS: palstic strain
The shear modulus G is expressed that way:
STRESS=HOOK.STRAIN i.e. D_STRESS=HOOK.D_STRAIN+D_HOOK.STRAIN
'RHO' : initial density
'TAU' : dimensionless parameter TAU used for
the calculation of the hardening law
'P' : dimensionless parameter P
-if P=0, the microstucture of the material is BCC
-else, the microstructure is NOT BCC
'S0' : dimensionless parameter S0
it gives the saturation stress at T=0°K
'SINF' : dimensionless parameter SINF
it gives the saturation stress at T(°K) infinite
'K' : dimensionless term K'.T used for the
calculation of the yielding limit. It is entered
as an EVOLUTION object (the parameter is
the temperature T)
'G' : dimensionless parameter g used for
the calculation of the saturation stress and
the yielding limit
'Y0' : dimensionless parameter Y0
it gives the yielding limit at T=0°K
'YINF' : dimensionless parameter YINF
it gives the yielding limit at T(°K) infinite
'Y1' : dimensionless Y1used for the calculation
of the yielding limit
'Y2' : dimensionless Y2 used for the calculation
of the yielding limit
'BETA' : dimensionless parameter BETA used for the
calculation of the yielding limit and the
saturation stress
'GP' : rate of the evolution of the shear modulus with
the pressure ( no unity): GP'
'GT' : temperature-dependant term correcting the shear
modulus ( homogeanus to the shear modulus)
One enters here the term: GT'.(T-300) thanks to
the use of an EVOLUTION object (the parameter
of this EVOLUTION is the temperature).
'TMO' : melting temperature for ETA=1
'MU' : coefficient MU0 used for the calculation of the
melting temperature
HINTE model
-----------
This model is done to represent the delamination of laminated
material.
Let us assume two dammaging modes : Y1 shearing mode and Y2
opening between layer.
dissipated energy is :
E = Y1*(d1/dt) + Y2*(d2/dt) d1 et d2 are two
dammage internal varibles
if : d2 < 1 and Y < YR then d1 = d2 = W(Y)
else d1 = d2 = 1
An isotropic dammmage is introduce by :
Y = sup(((Y1)**AL) + ( (GAM1*Y2)**AL))**(1/AL)
the function of delamination is :
w(Y)=((N/(N+1))**N)*( **N)/ ((YC-Y0)**N)
The thermodynamic force reaches at rupture for the ultimate
DR dammage is :
YR = Y0 + ( ((N+1)/N) * (DCRI** (1/N))*(YC-Y0)
Parameters of the model are :
'Y0' : dammaging threshold
'YC' : critical energy of dammage
'GAM1' : coupling parameter betwwenn normal and transverse
energies
'AL' : govern the modelling of mixed mode of rupture
'NN' : set the plus or minus fragility of the joint (the bigger
N is the more brittle the material is)
'DCRI' : allow to simulate a brittle rupture (default DCRI =1)
'KS' : shear stiffness of the joint
'KN' : normal stiffness of the joint
J2 model:
---------
* The model equations are (see [1]):
--> Notation: J2 second invariant of the deviatoric stress tensor
sigy yield stress
epse equivalent plastic strain (internal variable)
F yield function
G flow potential
--> Yield Function:
F = sqrt(3*J2)-sigy(epse)
--> Hardening law:
sigy(epse) = SIG0+KISO*epse +(SIGI-SIG0)*(1-exp(-VELO*epse))
--> Flow Potential:
G = F (associated plasticity)
* The specific model parameters are:
'SIG0' : Initial yield stress
'SIGI' : Limit yield stress
'KISO' : Linear hardening moduli
'VELO' : Velocity parameter
* References:
[1] Simo, J.C. and Hughes, T.J.R. ``Computational Inelasticity'',
Springer-Verlag, New York, 1997
RH_COULOMB model:
-----------------
Rounded Hyperbolic Mohr-Coulomb model (associated and perfect plasticity)
* The model equations are (see [1]):
--> Notations: I1 first invariant of the stress tensor
J2 second invariant of the deviatoric stress tensor
t Lode angle (from -30º to 30º)
F yield function
G flow potential
--> Yield Function:
F = I1/3.D0*sin(PHI)-COHE*cos(PHI)+sqrt(J2*ktet(t)**2+(ar*COHE)**2)
ar = 0.05*cos(PHI)
ktet(t)= aa - bb*sin(3*t) iff abs(t) > 25º
cos(t)-sin(PHI)*sin(t)/sqrt(3) iff abs(t) =< 25º
aa = aa(PHI,25º) see [1]
bb = bb(PHI,25º) see [1]
--> Flow Potential:
G = F (associated plasticity)
* The specific model parameters are:
'COHE' : Cohesion
'PHI ' : Friction angle
* References:
[1] Abbo, A.J. and Sloan, S.W., ``A smooth hyperbolic approximation
to the Mohr-Coulomb yield criterion'', Computers and Structures,
54, 3, 427-441, 1995.
MRS_LADE model:
---------------
* The model equations are (see [1,2]):
--> Notations: I1 first invariant of the stress tensor
J2 second invariant of the deviatoric stress tensor
p = -I1/3
q = sqrt(3*J2)
t Lode angle (from 0º to 60º)
kcon cone internal variable
kcap cap internal variable
dkcon increment of kcon
dkcap increment of kcap
dwp increment of plastic work
Fcon cone yield function
Fcap cap yield function
Gcon cone flow potential
Gcap cap flow potential
--> Cone Yield Function:
Fcon = wwf(t,E)*q*(1+q/QA)**EXPM - etacon(kcon)*p
wwf(t,E) = W-W function
--> Cap Yield Function:
Fcap = ((p-cpm*pcapf(kcap))/(cpr*pcapf(kcap)))**2 +
(wwf(t,E)*q*(1+q/QA)**EXPM/
(etacon(kcon)*cfr*pcapf(kcap)) )**2 - 1
cpm = cpm(PHI,ALP)
cpr = cpr(PHI,ALP)
cfr = cfr(PHI,ALP)
--> Cone hardening/softening law:
etacon(kcon) = aaa*exp(-bbb*kcon)*(K1+kcon)**(1/EXPV) +
K2*ETAB*kcon/(EPSI+kcon)
aaa = aaa(EXPV,K1,K2,EPSI)
bbb = bbb(EXPV,K1,K2,EPSI)
--> Cap hardening law:
pcapf(kcap) = PCAP*(1+kcap**(1/EXPR))
--> Evolution of internal variables:
dkcon = (p/PA))**(-EXPL)/(CCON*PA)* dwp
dkcap = (PCAP/PA)**(-EXPR))/(CCAP*PA)* dwp
--> Cone Flow Potential:
Gcon = wwf(t,E)*q*(1+q/QA)**EXPM - N etacon(kcon)
*( p-2*ALP*pcapf(kcap)*ln(p+ALP*pcapf(kcap)) )
--> Cap Flow Potential :
Gcap = Fcap (associated plasticity)
* The specific model parameters are:
'PC ' : Must be = 0 (just cohesionless materials are implemented)
'PA ' : Scale parameter (usually = 1)
'QA ' : Scale parameter (usually = 1)
'EXPM' : Cone yield function parameter (must be >= 0)
= 0 implies linear p-q relationship in cone region
then etacon(kcon) is identical to the friction angle
'E ' : Shape on the deviatoric plane
From = 1 (circular) to = 0.5 (triangular), usually = 0.7
'K1 ' : Cone hardening/softening law parameter (must be > 0)
'K2 ' : Cone hardening/softening law parameter (must be > 0)
K2*ETAB is the residual value (reached at kcon=infinity)
of etacon(kcon), function related with the friction angle.
'ETAB' : Maximum value of etacon(kcon), function related with the
friction angle, (must be > 0). It is reached at kcon=1
'EXPV' : Cone hardening/softening law parameter (must be > 0)
'EPSI' : Cone hardening/softening law parameter (must be > 0)
'N ' : Degree of non-associativity at the apex (p = 0).
From 0 (incompressibility in all the cone region)
to -1 (associate flow direction at p = 0)
'CCON' : Parameter of cone internal variable evolution (must be > 0)
'EXPL' : Parameter of cone internal variable evolution (must be > 0)
'PCAP' : Initial value of the isotropic yield stress, pcapf(kcap),
(cap intersection with p-axis)
'EXPR' : Parameter of cap internal variable evolution (must be > 0)
'CCAP' : Parameter of cap internal variable evolution (must be > 0)
'PHI ' : Must be = 0, incompressibility is forced at cone-cap
intersection
(parameter related with cap slope at cone-cap intersection)
'ALP ' : Shape of cap function. Intersection of cone-cap is located
at p = ALP * pcapf(kcap) (must be > 0)
Parameters for numerical differentiation (integration of const.
law and computation of consistent tangent moduli, see [3,4]) are fixed
in time-integration operator.
* References:
[1] Sture, S., Runesson, K. and Macari-Pasqualino, E.J.
``Analysis and calibration of a three-invariant plasticity
model for granular materials'', Ing. Archiv, 59, 253-266, 1989.
[2] Perez-Foguet, A. and Huerta, A. ``Plastic flow potential for the
cone region of the MRS-Lade model'', J. Engr. Mech, Vol. 125,
pp. 364-367, 1999.
[3] Perez-Foguet, A., Rodriguez-Ferran, A. and Huerta, A. ``Numerical
differentiation for local and global tangent operators in
computational plasticity'', Comp. Meth. App. Mech. Engrg. Vol. 189,
pp. 277-296, 2000.
[4] Perez-Foguet, A., Rodriguez-Ferran, A. and Huerta, A.
``Numerical differentiation for non-trivial consistent tangent
matrices: an application to the MRS-Lade model'', Int. J. Num. Met.
Engrg., Vol. 48, pp. 159-184, 2000.
VMT_FEFP Model
--------------
* Hyperelastoplastic model, FeFp finite strain plasticity, see [1].
* The plastic equations are descrived in [2]. The plastic model is
called Von Mises - Tresca.
* Hencky's hyperelastic model is used.
* The specific model parameters are:
'SIG0' : Initial yield stress
'SIGI' : Limit yield stress
'KISO' : Linear hardening moduli
'VELO' : Velocity parameter
'MSHA' : Deviatoric section shape (1, Von Mises, to 20, Tresca)
Parameters for local line search (integration of constitutive equation,
see [2]) are fixed in time-integration operator.
* References:
[1] Simo, J.C., ``Numerical analysis of classical plasticity'', in P.G.
Ciarlet and J.J. Lions, editors, Handbook of Numerical Analysis, vol.
IV, Elsevier, Amsterdam, 1998.
[2] Perez-Foguet, A., Armero, F., On the formulation of closest-point
projection algorithms. Part II: Globally convergent schemes, Int. J.
Num. Meth. Engrg., 53:331-374, 2002.
RHMC_FEFP Model
---------------
* Hyperelastoplastic model, FeFp finite strain plasticity (see VMT_FEFP
model)
* The plastic equations are the same as small strain RH_COULOMB model.
* Hencky's hyperelastic model is used.
* The specific model parameters are:
'COHE' : Cohesion
'PHI ' : Friction angle
POWDER_FEFP Model
-----------------
* Hyperelastoplastic model, FeFp finite strain plasticity (see VMT_FEFP
model)
* The plastic equations are descrived in [1]. The plastic model is
elliptic in the invariant stress space and its size and shape depends
on relative density.
* Hencky's hyperelastic model is used.
* The specific model parameters are:
'SIGY' : Yield stress of fully compacted material
'NNN1' : Yield function parameter (density dependence of ellipse)
'NNN2' : Yield function parameter (density dependence of ellipse)
'ETA0' : Initial relative density
* References:
[1] Perez-Foguet, A., Rodriguez-Ferran, A. and Huerta, A. ``Consistent
tangent matrices for density-dependent plasticity models'', Int. J.
Ana. Num. Met. Geomech., Vol. 25, pp. 1045-1075, 2001.
POWDERCAP_FEFP Model
--------------------
* Hyperelastoplastic model (see POWDER_FEFP model)
* The specific model parameters are:
'SIGY' : Yield stress of fully compacted material
'NNN1' : Yield function parameter (density dependence of ellipse)
'NNN2' : Yield function parameter (density dependence of ellipse)
'ETA0' : Initial relative density
'COHE' : Cohesion of fully compacted material
'PHI0' : Initial friction angle
'PHI ' : Fricction angle of fully compacted material
'NNNC' : Yield function parameter (density dependence of cohesion)
ISS_GRANGE model
-----------------
Here is a Soil-Structure Interaction model developped by S.GRANGE
(2008). The original model was developped in Grange's Ph. D.
thesis[1]. A modification of the plasticity and uplift
phenomenons has been done in order to ease the programming.
The model that has been implanted, can only be used with
with orthotropic joint elements JOI1 in 3D. So as to understand the
influence of each parameter, it's recommended to refer to S.Grange's
Ph. D. thesis[1] (recap page 77) and in the articles [2][3].
'DIAM' : diameter of the foundation (if circular)
'LX ' : lenght of the foundation in the x direction
(if linear or rectangular foundation)
'LY ' : lenght of the foundation in the y direction
(if linear or rectangular foundation)
'XA','XB','XC','XD','XE','XF': parameters describing the shape
of the failure criteria
'QMAX' : bearing capacity of the foundation
'A6 ' : growth speed of the loading surface
'ETA3' : viscosity parameter
'XTIM' : time increment for dynamic calculation
'A8 ' : kind of calculation
if = 1 : detachement desactivated
otherwise : detachement activated
'A9 ' : kind of foundation
if = 1 : linear
if = 2 : rectangular
otherwise : circular
The elastic stifnesses of the foundation (Kelz,Kelh,etc...) are
to be precised as the elastic stiffnesses of the othotropic joint
element joi1 (KN,KS1,etc...). Attention must be payed to the axes
permutation (local <-> ISS)!
* References:
[1] Grange, S. (2008). Modelisation simplifiee 3D de l'interaction
sol-structure: application au genie parasismique.
Ph. D. thesis, INP Grenoble.
http://tel.archives-ouvertes.fr/tel-00306842/fr.
[2] S. Grange, P. Kotronis, J. Mazars (2009). A macro-element to
simulate 3D soil-structure interaction considering plasticity
and uplift. International Journal of Solids and Structures 46
3651-3663.
[3] S. Grange, P. Kotronis, J. Mazars (2009). A macro-element to
simulate dynamic Soil-Structure Interaction. Engineering
Structures 31 (2009) 3034-3046.
RUP_THER model
---------------
The RUP_THER model is designed to represent the behaviour of thermal
breaks subject to horizontal shear during earthquakes. It has been
developped by T.T.Huyen Nguyen, during her Ph.D thesis. This model
can be used with orthotropic joint elements JOI1 in 3D. The model
considers the break's steel bars plastification, as well as the
damages of the concrete, which the steel bars are anchored in. A
global hysteresis phenomenon is also considered.
Parameters regarding the steel behaviour:
'KA ' : horizontal shear stiffness of the total steel
section in a thermal break (N/m)
'YA0 ' : elastic strength limit of the steel (N)
'ALPA', 'BETA' : paramaters of the steel cinematic hardening
model
Parameters regarding the concrete behaviour:
'KB ' : horizontal shear stiffness of the concrete
section (N/m)
'YB0 ' : damage threshold of the concrete (N.m)
'C1 ', 'D1 ' : paramaters of the concrete damage model
the expression of the damage is:
d = 1 - 1/(1 + C1*Y**D1)
'ALPB', 'BETB' : paramaters of the concrete cinematic hardening
model
------------------------------------------------
| Parameter name for an ENDOMMAGEABLE material |
------------------------------------------------
MAZARS model
------------
It is an isotropic and scalar damage model for concrete.
(This model may be used unlocally) See the IDENTI procedure
to identify the parameters.
'KTR0' : threshold in deformation for the tension (1.D-04)
'ACOM' : parameter for the compression (1.4)
'BCOM' : parameter for the compression (1900.)
'ATRA' : parameter for the tension (0.8)
'BTRA' : parameter for the tension (17000)
'BETA' : correction for the shear (1.06)
UNILATERAL model
----------------
It is an isotropic and scalar damage model with two damage
variables which manages the crack closures.
'YS1 ' : threshold in energy for the tension (2.5 E-4 MPa)
'YS2 ' : threshold in energy for the compression
(1.5 E-3 MPa)
'A1 ' : parameter for the tension (5000 MPa)
'B1 ' : parameter for the tension (1.5)
'A2 ' : parameter for the compression (10 MPa)
'B2 ' : parameter for the compression (1.5)
'BET1' : manages the inelastic deformations in tension (1MPa)
'BET2' : manages the inelastic deformations in compression
(-40MPa)
'SIGF' : cracks reclosure stress (-3.5MPa)
ROTATING_CRACK model
--------------------
It is a smeared crack type model in which the crack direction
changes for each step. Only the damage induced by traction is
considered.
'EPCR' : strain at beginning of damage in a uniaxial traction
test
'MUP ' : ratio of tangent modulus to Young's modulus, the
uniaxial traction curve being assumed bilinear
SIC_SIC model
-------------
It is an anysotropic scalar damage model specific for SiC/SiC
ceramic matrix composites. This model is available only for 3D
massive elements. Damage is described by means of 3 scalar
variables corresponding to the 3 orthotropy directions of the
composite. Material properties are given using the ORTHOTROPE
keyword. The following parameters are used to define the damage
evolution laws:
G1DC,G1Y0,G1YC,G1P: pour la premiere direction
G2DC,G2Y0,G2YC,G2P: pour la deuxieme direction
G3DC,G3Y0,G3YC,G3P: pour la troisieme direction
AXEP: optional parameter used to specify which one of three
orthotropy directions is the thickness. Must be between 1 and 3
(default = 3).
- Equations of the model:
Notations:
S : stress tensor
E : deformation tensor
C : compliance tensor
Ki : caracteristic tensors of the composite
(obtained from the Hook tensor)
h(-Ei): Heavyside function,
h=0 if -Ei<0
h=1 if -Ei>0
Pi : tensor related to the damage directions
di : damage variables
Stress-Strain relation:
S= C x E - Ceff x E
Ceff= di*Ki-di*h(-Ei)(Pi x Ki x Pi) (sum on i=1,3)
Thermodynamic forces driving the damage process :
Yi= 1/2*E x Ki x E
Yeq= + +
(= positive part of x)
Damage evolution laws:
di=DiDC*(1-EXP-(<(Yeq**1/2-GiY0)/GiYC>**GiP)) (i=1,3)
This model has been developed at the ONERA. For further details on
the model and its identification look at the Brite Euram BE-5462
reports.
The model has been identified on a 2D SiC/SiC composite produced by
SEP. The parameters of the damage evolution laws are the following:
GiDC : 0.6 (i=1,3)
GiY0 : 1.3
GiYC : 4
GiP : 1
VISCOHINTE model
----------------
Laws governing this model are the same as the one governig the
HINTE model. Only variation of dammage is modified.
if d2 <1 and Y**M , w(Y)<1
d1/dt = d2/dt
else : d2 = 1
response of this model is quite the same as for HINTE model for
small dammage
Parameters of the model are :
'Y0' : dammaging threshold
'YC' : critical energy of dammage
'GAM1' : coupling parameter betwwenn normal and transverse
energies
'AL' : govern the modelling of mixed mode of rupture
'NN' : set the plus or minus fragility of the joint (the bigger
N is the more brittle the material is)
'DCRI' : allow to simulate a brittle rupture (default DCRI =1)
'KS' : shear stiffness of the joint
'KN' : normal stiffness of the joint
'MM' : Parameter for delaying effect (default MM = 1)
'KK' : caracteristic time
SICSCAL model
----------------
Scalar damage model developed by ONERA for woven SiCf/SiC.
3 damage variables are considered. Damage variables d1 and d2
correspond
to cracks planes normal to the 2 fibres directions. Damage
variable d3 corresponds to cracks in the ply planes. Details on
constitutive law as well as its validation can be found in
reference SEMT/LM2S/05-034.
Anisotropy directions must be defined such that the fibres
directions correspond to directions 1 and 2.
The constitutive law is:
E = Seff S + Eth + Er + Es
Where E is the strain, S the Stress, Seff, the effective
compliance tensor.
Eth, Er and Es are respectively the thermal, stored and residual
strains.
Seff = S0 + (nui di Hi0) (sum on i=1,3)
S0 : undamaged compliance tensor
Hi0 : fourth-order tensor describing the effect of the damage di
on the compliance
Hi0 is calculated from S0 and from Coefficients HiN, HiHP and HiP
The names of parameters to define are : H1N, H1HP, H1P, H2N, H2HP,
H2P, H3N, H3P.
By default values are:
h1n=1, h1hp =0.7, h1p=0.45
h2n=1, h2hp =0.7, h2p=0.45
h3n=1, h3p=0.7
The deactivation index nui are calculated from parameters DTAL,
TER0, SIF1, SIF2, SIF3, AIF1, AIF2, AIF3. Default values are
SIF1=SIF2=SIF3=3.10-4 and AIF1=AIF2=AIF3=0.
Calculation of residual strains necessitate parameters named ETA1,
ETA2 and ETA3. Default values are ETA1=ETA2=0.1, ETA3=0.
Damage evolutions are calculated using the parameters named DCT1,
DCT2, DCT3, DCN1, DCN2, DCN3, YCT1, YCT2, YCT3, YCN1, YCN2, YCN3,
Y01T, Y02T, Y03T, Y01N, Y02N, Y03N, PT1, PT2, PT3, PN1, PN2, PN3.
Defaults values are DCT1=DCT2=DCT3=DCN1=DCN2=DCN3=4,
YCT1=YCT2=YCT3=YCN1=YCN2= YCN3=1870,83 (Pa**0.5),
Y01T=Y02T=31.6(Pa**0.5), Y03T=Y01N=Y02N=Y03N=173.2(Pa**0.5),
PT1=PT2=1.2, PT3=PN1=PN2=PN3=1.
A coupling parameter maned B must also be defined.
Its default value is B=1.
SICTENS Model :
----------------
Pseudo-tensorial model developed by ONERA for woven SiCf/SiC.
5 damage variables are considered. Damage variables d1 and d2
correspond to cracks planes normal to the 2 fibres directions.
Damage variable d3 corresponds to cracks in the ply plane.
Variables d4 and d5 correspond to cracks planes normal to the +
and - 45° inclination with respect to the fibres directions.
Details on constitutive law well as its validation can be found
in reference SEMT/LM2S/05-034.
Anisotropy directions must be defined such that the fibres
directions correspond to directions 1 and 2.
The constitutive law is:
E = Seff S + Eth + Er + Es
Where E is the strain, S the Stress, Seff, the effective
compliance tensor.
Eth, Er and Es are respectively the thermal, stored and residual
strains.
Seff = S0 + (nui di Hi0) (sum on i=1,5)
S0 : undamaged compliance tensor calculated
Hi0 :fourth-order tensor describing the effect on the compliance
of the damage di.
Hi0 is calculated from S0 and from Coefficients HiN, HiHP and HiP
The names of parameters to define are : H1N, H1HP, H1P, H2N, H2HP,
H2P, H3N, H3P, H4N, H4HP, H4P, H5N, H5HP and H5P.
By default values are:
h1n=1, h1hp =0.7, h1p=0.45
h2n=1, h2hp =0.7, h2p=0.45
h3n=1, h3p=0.7
h4n=1, h4hp =0.7, h4p=1.2
h5n=1, h5hp =0.7, h5p=1.2
The deactivation indexes nui are calculated from parameters DTAL,
TER0, SIF1, SIF2, SIF3, SIF4, SIF5, AIF1, AIF2, AIF3, AIF4, AIF5.
Default values are SIF1=SIF2=SIF3=SIF4=SIF5=3.10-4,
AIF1=AIF2=AIF3=0.5 and AIF4=AIF5=1.
Calculation of residual strains necessitate parameters named ETA1,
ETA2, ETA3, ETA4 and ETA5. Default values are ETA1=ETA2=0.1,
ETA3=0, ETA4=ETA5=0.1.
Damage evolutions are calculated using the parameters named DC1,
DC2, DC3, DC4, DC5, YC1, YC2, YC3, YC4, YC5, Y01, Y02, Y03, Y04,
Y05, PY1, PY2, PY3, PY4, PY5.
Defaults values are:
DC1=DC2=DC3=DC4=DC5=4, YC1=YC2=YC3=1870,83(Pa**0.5),
YC4=YC5=3464.1 (Pa**0.5),Y01=Y02=Y03=173.2 (Pa**0.5),
Y04=Y05=173.2 (Pa**0.5), PY1= PY2=PY3=1., PY4=PY5=1.2.
The coupling parameters B1, B2 and B3 must also be defined.
Their default values are set to 1.
DAMAGE_TC model
----------------
Input data for the model in complement of the elacticity parameters
are the following ones:
'HLEN' : caracteristic length (cf. mesh)
'GVAL' : Fracture energy (300)
'FTUL' : Tension limit strength (3.6e6)
'REDC' : Drop Factor for Peak Tensile Stress (1.7e6)
'FC01' : Elastic Limit Compressive Stress (-25e6)
'RT45' : Equi-biaxial Compressive Ratio (1.18)
'FCU1' : Compressive Peak Stress (-42e6)
'STRU' : Ultimate Limit Strain (-0.015)
'EXTP' : Reference Strain for Plastic Parameter (-0.001)
'STRP' : Reference Stress for Plastic Parameter (-22e6)
'EXT1' : Fitting Point 1 (Strain) (-0.006)
'STR1' : Fitting Point 1 (Stress) (-35e6)
'EXT2' : Fitting Point 2 (Strain) (-0.008)
'STR2' : Fitting Point 2 (Stress) (-22e6)
'NCRI' : indicator 1 : exponential softening in tension
2 : linear softening in tension
DESMORAT model
--------------
Input data for the model in complement of the elacticity parameters
'K0' : threshold in deformation for the tension (5.D-05)
'A' : Damage parameter A (5.D03)
'a' : Damage parameter of about size of the deformations
reached in compression (2.93D-4)
'etaC' : Hydrostatic sensibility in compression parameter (0.)
'etaT' : Hydrostatic sensibility in tension parameter (3.)
'Dc' : Critical value of the damage for the numerical
control of rupture (0.9 to 0.999)
do not forget to declare for input table of PASAPAS :
tab1.'MOVA' = 'D11';
DRUCKER_PRAGER_2 model
----------------------
Input data for the model in complement of the elacticity parameters
'GF' : fracture energy
'LTR' : tension strength
'LCS' : uniaxial compression strength
'LBI' : biaxial compression strength
'SIGY' : elastic limit in uniaxial compression
'EPM' : peak strain in uniaxial compression
'EPU' : ultimate strain in uniaxial compression
'LCAR' : caracteristic length
FATSIN model
--------------
* This non local fatigue model [1,2] is focused for damage of materials loa
under sinusoidal fatigue. Within the material, the mechanical fields
(displacement, strain and stresses) are pseudo-sinusoidal and can be writ
as follow :
x= x_a * sin (2*pi/T * N/T)
where x_a is the amplitude of x, T its period and N the number of cycles.
The model allows the calculation of the damage after N loading cycles.
Based on elasticity (Young modulus E_0 and NU Poisson's ratio) the time
integration is done at the macroscopic scale of the cycles. To do so, the
material is static at its amplitude (positive and negative).
Model equations are (references [1] et [2]) :
--> Notation: Eps_eq : Equivalent strain amplitude
Eps_moy : Non local averaging of Eps_eq
function of the characteristic length
(cf. 'NLOC')
Sig_i : Principale stresses amplitude
: Positive part of x ( =0.5*[x+abs(x)])
E_0 : Young modulus of the virgin material (D=0)
N : Number of cycles
D : Damage
--> Equivalent strain : Eps_eq
___
(\ ( < Sig_i> ) )
Eps_eq = sqrt ( \ ( ----------- )^2 )
( / ( E_0 * (1-D) ) )
(/___ )
--> Damage rate expression :
General formulation
Eps_moy ^ (BETA+1) - KTR0 ^ (BETA+1)
dD/dN = f(D) --------------------------------------------------------
(BETA+1)
Two implemented expressions of f(D) :
1. Classical power law L2R ( Reference [3])
f(D) = C D^ALFA
2. Phenomenological law L3R (Reference [1]) developped for bituminous m
ALFA2 ( D ) ( ( D )
f(D) = -------------- * ( ----- ) ^ (1-ALFA3) * exp ( (-------)^(ALFA3
ALFA1 * ALFA3 ( ALFA2 ) ( ( ALFA2 )
The parameters are :
'KTR0' : threshold connected to material endurance limit
'BETA' : parameter associated to the slope p of the fatigue line
(log(Nf) vs log(Eps_a)) with the relation (BETA=-(p+1)
'LOI ' : 2 for L2R damage growth law
3 for L3R damage growth law
For 'L2R' use
'ALFA' : parameter related to damage curve concavity
'C ' : parameter associated to the fatigue life
For 'L3R' use
'ALFA1' : parameter associated to the fatigue life
'ALFA2' : parameter controlling the damage level for which the damage
rate decreases then increases
'ALFA3' : parameter related to damage curve concavity
Remark: Depending on the choice of the 'LOI' the non used parameter should be
* References:
[1] D. Bodin, (2002), Cyclic damage modeling applied to asphalt mixes fatig
PhD thesis. Ecole Centrale de Nantes. p. 187. (In French)
(http://www.lcpc.fr/fr/recherches/th_soutenues/index1.dml)
[2] D. Bodin, G. Pijaudier-Cabot, C. de La Roche, J.-M Piau and A. Chabot,
A Continuum Damage Approach to Asphalt Concrete Fatigue Modelling, Jour
Engineering Mechanics, ASCE, vol. 130 (6), pp. 700-708.
[3] Paas, R. H. J. W., Scheurs, P. J. G., and Brekelmans, W. A. M. (1993).
continuum approach to brittle and fatigue damage: Theory and numerical
procedures. Int. J. Solids Struct., 30~4!, 579-599.
RICRAG model
-----------------------
This model [1,2] is recommended for monotonic loadings and cyclic ones
with a medium intensity due to the fact that unilateral effect is
partially taken into account. It can be used with the nonlocal
approach. The material parameters to be given as input are the
following ones:
'FT' : tensile strength (3.6e6 )
'ALDI' : brittleness in tension (1.0e-2)
'ALIN' : brittleness in compression (5.0e-4)
'GAM1' : kinematic hardeing modulus 1 (7.0e7 - 7.0e9)
'A1' : kinematic hardeing modulus 2 (7.0e-7)
* References:
[1] B. Richard, F. Ragueneau, C. Cremona, L. Adelaide. (2010). Isotropic
continuum damage mechanics for concrete under cyclic loading: stiffness
recovery, inelastic strains and frictional sliding. Engineering Fractur
Mechanics. 77:1203-1223.
[2] L. Adelaide, B. Richard, F. Ragueneau, C. Cremona. (2010). Thermodynami
admissibility of a set of constitutive equations coupling elasticity,
isotropic damage and internal sliding. Comptes Rendus Mecanique. 338:1
GLRC_DM model
-----------------------
The material parameters to be given as input are the
following ones:
'YOUF' : equivalent Young's modulus for bending part
'NUF ' : equivalent Poisson ratio for bending part
'GAMT' : damage parameter for tension for membrane part
'GAMC' : damage parameter for compression for membrane part
'GAMF' : damage parameter for bending part
'SEUI' : initial threshold to activate damage
'ALF ' : coupling coefficient between membrane and bending parts
They can be identified from physical data by mean of IDENTI procedure [1]
* References:
[1] B. Richard, N. Ile. (2013). Influence of concrete cracking on transfere
movements - phase 2: implementation in Cast3M of a simplified reinforce
concrete model and structural validations (in French). CEA Technical re
RT12-011/A.
RICBET model
-----------------------
The material parameters to be given as input are the
following ones:
'FT ' : tension strength (3.6E6)
'GAM1' : kinematic hardening modulus 1 (5E9)
'A1 ' : kinematic hardening modulus 2 (8E-6)
'ALDI' : brittleness in tension (6.0E-3)
'SREF' : crack closing stress (-3.2E6)
'AF ' : compression threshold surface 1 -
biaxial compression response (0.7)
'AG ' : compression threshold surface 1 -
dilatancy (0.6)
'BF ' : compression threshold surface 2 -
reponse compression biaxiale (0.3)
'BG ' : compression threshold surface 2 -
dilatancy (0.45)
'AC ' : plasticity flow rule in compression 1 (3.2E10)
'BC ' : plasticity flow rule in compression 2 (700)
'SIGU' : asymptotic stress in compression (-4E6)
'FC ' : initial threshold in compression (6E6)
* References:
[1] B. Richard, F. Ragueneau (2012). 3D modelling of concrete for
earthquake analysis: damage mechanics and plasticity coupling.
WCCM 2012, Sao Paulo, Brazil.
[2] B. Richard, F. Ragueneau (2012). Continuum damage mechanics based
model for quasibrittle materials subjected to cyclic loadings:
formulation, numerical implementation and applications.
Engineering Fracture Mechanics. In press.
RICCOQ model
-----------------------
The material parameters to be given as input are the
following ones:
'FT ' : tension strength (3.6E6)
'FC ' : initial threshold in compression (10E6)
'EPUT' : limit tension strain (according to the mesh)
'EPUC' : limit copression strain (according to the mesh)
* References:
[1] B. Richard (2012). SERIES/ENISTAT Project. Preliminary
numerical time history analysis. CEA Technical report
RT-12-013/A.
--------------------------------------------------
| Parameter name for a material in FLUAGE (creep)|
--------------------------------------------------
The following parameters will have to be specified BESIDES those
connected with the elastic behavior. The available creep models
are described below, by the equation modeling a creep test
result at steady stress. They are noted as follows:
ef equivalent creep deformation
s equivalent stress
t time
Only the polynomial model is described by developing
the creep velocity vf with respect to the equivalent stress.
In the calculations, the hypothesis of strain hardening
is put forward.
NORTON creep model:
-------------------
ef = AF1* ( s**AF2 ) * ( t**AF3 )
The parameters to be input are 'AF1 ','AF2 ','AF3 ', as well as
a 'SMAX' stress of reference (equalling Young's modulus times
1.E-3 by default).
BLACKBURN creep model:
----------------------
ef = A * ( 1 - e**(-R*t) ) + B * t
with: A = AF1 * e**(-AF2*s) + AF3 * s**AF4
R = RF1 * e**(-RF2*s) + RF3 * s**RF4
B = BF1 * (sinh(BF2*s)**BF3 + BF4 * e**(-BF5*s)
The parameters to be input are 'AF1' to 'AF4 ', RF1 ' to 'RF4 ',
and 'BF1 ' to 'BF5 ', as well as a 'SMAX' stress of reference
(equalling Young's modulus times 1.E-3 by default).
BLACKBURN_2 creep model:
----------------------
ef = A * ( 1 - e**(-R*t) ) + B * t
with: A = AF1 * e**(-AF2*s) + AF3 * s**AF4
R = RF1 * e**(-RF2*s) + RF3 * s**RF4
B = BF1 * (sinh(BF2*s)**BF3 + BF4 * s**BF5
The parameters to be input are 'AF1' to 'AF4 ', RF1 ' to 'RF4 ',
and 'BF1 ' to 'BF5 ', as well as a 'SMAX' stress of reference
(equalling Young's modulus times 1.E-3 by default).
RCC-MR creep model for steel 316-SS :
--------------------------------------
ef = AF1* ( s**AF2 ) * ( t**AF3 ) if t < TF
and ef = BF1* ( s**BF2 ) if t > TF
with: TF = TF1* ( s**TF2 )
The parameters to seize are 'AF1 ' to 'AF3 ','BF1 ', 'BF2 ',
'TF1 ', 'TF2 ', as well as a 'SMAX' stress of reference
(equalling Young's modulus times 1.E-3 by default).
RCC-MR creep model for steel 304-SS :
-------------------------------------
ef = A1 * ( 1 - e**(-R*t) ) + A2 * ( 1 - e**(-S*t) ) + B * t
with: B = BF1 * (sinh(BF2*s/BF3))**BF3
R = RF1 * (sinh(RF2*s/RF3))**RF3
A1 = AF1 * B / R
S = ( SF1 / RF1 ) * R
A2 = AF2 + AF3*s si s > SF2 , 0. sinon
The parameters to be input are 'AF1' to 'AF3 ','BF1 ' to 'BF3 ',
'RF1 ' to 'RF3 ', 'SF1 ','SF2 ', as well as a 'SMAX' stress of
reference (equalling Young's modulus times 1.E-3 by default).
LEMAITRE creep model :
----------------------
ef = AF1 * ( X**AF2 + Y )
with: dX/dt = ( s / KXF )**( AF3 / AF2 ) * ( AF4**(1/AF2 ) )
dY/dt = ( s / KYF )**AF3 * AF4
The parameters to seize are 'KXF', 'KYF', 'AF1', 'AF2', 'AF3',
'AF4 ', as well as a 'SMAX' stress of reference (equalling
Young's modulus times 1.E-3 by default).
POLYNOMIAL creep model :
------------------------
vf = AF0 + AF1*s**AF2 + AF3*s**AF4 +AF5*s**AF6
The parameters to be input are 'AF0', 'AF1', 'AF2', 'AF3', 'AF4',
'AF5', 'AF6',as well as a 'SMAX' stress of reference (equalling
Young's modulus times 1.E-3 by default).
CERAMIQUE creep model :
------------------------
Above the transition temperature the ceramic creeps
following Norton's Creep Law :
ef = AF1* ( s**AF2 ) * ( t**AF3 )
The three first parameters to be input are therefore
'AF1 ','AF2 ','AF3 ', as well as a ('SMAX') stress of
reference (equalling Young's modulus times
1.E-3 by default).
Below the transition temperature the ceramics behaves
following the Ottosen's model:
('LTR') : limit in tension (default value YOUN*1.2E-4)
('GFTR') : restitued energy ratio
(also known as the fracturing energy)
(default value LTR*3.9E-5 but this value corresponds to
the international units system)
('GS') : modul providing the loose of resistance to shear of a
fracture with its normal opening.
(default value YOUN*1.8E-4, usual value is between 2 and
6 Mpa)
('BTR') : no recouvrable opening ratio (default value 0.2)
The CHAML result of the operator TAILLE applied to the model, must be
added to the CHAML built by MATE operator.
Moreover, in cases of plane strains or axisymetrical option, one can
also define :
('EPSR') : failure strain in the direction normal to the
modelisation plan.
The parameters specific to the 'ceramique' model to be input are:
'TTRA' : The transition Temperature
'ENDG' : The total deformation reached during creep above which
the ceramic looses its rigidity
MAXWELL creep model :
---------------------
The generalized MAXWELL creep model must have at least 4 branches
in addition of the elastic one. It may contain up to 8 branches.
Datas for the four first branches are obligatoty.
For each branch parameters to be defined are the elastic modulus 'EMi'
and the relaxation time 'TRi' (i varying from 1 to 4,5,6,7 or 8).
For the elastic branch, only the modulus 'EM0' must be defined.
The IDENTI procedure help the identification of parameters for concrete
behaviour according EUROCODE 2 or BPEL regulatories or LCPC creep
formula.
MAXOTT creep- plastic concrete model :
--------------------------------------
Parameters for this model are parameters of the MAXWELL model plus
parameters of the OTTOSEN model.
---------------------------------------------------------
| Parameter name for a PLASTIQUE-ENDOMMAGEABLE material |
---------------------------------------------------------
The following parameters will have to be specified BESIDES those
connected with the elastic behavior. The available
damageable plasticity models are the following:
The P/Y fracture model:ductile fracture in triaxial states of stress
--------------------------------------------------------------------
-Elastoplastic behavior:
Isotropic hardening (see: model 'PLASTIQUE' 'ISOTROPE' )
-Fracture equations:
Pseudo porosity:
A=(RHOf-RHO)/RHOf
with :
RHO: material's density
RHOf: material's density when the first fracture
appears ( when the fracture curve is first
reached)
Fracture variable D:
D=f(A) f is a function given by the user
Fracture fonction g(A):
If A<0:
g(A)=1
If A>0:
g(A)=1-D
Model's formulation:
Load (A grows):
SIGMA=SIGMA_PL.g(A)
Unload (A diminushes):
If A>0 :
SIGMA=SIGMA_PL.g(Amax)
If A<0:
SIGMA=SIGMA_PL
with:
SIGMA: final stress
SIGMA_PL: stress obtained from an elastoplastic
calculation
Amax: maximum value of A
'RHO' : initial density of the material
'TRAC' : keyword followed by:
NOMTRAC : tension curve consisting in an EVOLUTION object
'EVOL' : keyword followed by :
NOMEVOL : fracture curve consisting in an EVOLUTION object.
The curve is a function of the parameter P/Y ( where
P = 1/3 * ( SIG_XX + SIG_YY + SIG_ZZ ) and
Y is the effective stress ) by the plastic natural
strain.
When one is located over this curve, fractures appear
and grow, under this curve there's no fracture's grow
or new fracture's appearance.
'COMP' : keyword followed by :
NOMCOMP : curve consisting in an EVOLUTION object.
The curve is a function of the fracture variable by the
pseudo porosity
ROUSSELIER ductile fracture model :
-----------------------------------
- Plastic potential F :
F = J2(SIG/RHO)-R(P)+B(BETA).D.EXP(SM/(RHO.SIG1))
- Damage function B(BETA) :
B(BETA) = SIG1.F0.EXP(BETA)/(1-F0+F0.EXP(BETA))
- Density fraction RHO :
RHO = ( material's density)/( initial material's density)
RHO = 1/(1-F0+F0.EXP(BETA))
- Isotropic plastic hardening
- Damage variable BETA :
d BETA = d P . D.EXP(SM/(RHO.SIG1))
- If f (volume fraction of cavities) > FC: SIG=0.D0
with: SIG = stresses
SM = trace(SIG)/3 : mean stress
P = equivalent plastic strain
R(P) = undamaged tension curve
'TRAC' : keyword followed by:
NOMTRAC : undamaged tension curve consisting in an EVOLUTION object
'SIG1' : parameter SIG1 used in the damage calculation
'D' : parameter D used in the damage calculation
'F' : initial volume fraction of cavities F0
'FC' : critical volume fraction, when this value is over passed
the stresses and the stiffness of the material are put
to 0.
GURSON's ductil fracture model modified by NEEDLEMAN and TVERGAARD
-------------------------------------------------------------------
(GURSON2)
---------
1st case:
---------
- Plastic potential F :
F = J2(SIG)**2-R(Pmat)**2.G_end=0
G_end=1+(Q.F_*)**2-2.Q.F_*.COSH(3.SMT/(2.R(Pmat))
- Fracture function F_*
IF F Notation : S stress tensor
X kinematic stress hardening variables
ai internal variables ( i=2,4 )
EP inelastic strain tensor
p accumulated equivalent inelastic
strain
p1 dp1 = dp but p1=0 at each load reversal
pI value of p1 at load reversal
J2 second invariant of deviatoric tensor
n normal from F criterion
t time
positive part of a
x.y scalar product of x by y
--> Criterion : F = J2 (S-X) = R - KK
--> Stress : dX =M* p1**(M-1) * [ 2/3 *(A*a2 + a1* EP.n)
hardenings - ( C1 -C*a2)* X.n ] *dEP
- ( C0*< pI-P1M0 > + C*a4 )*X*dp
and - G * J2(X)**R * X*dt
yield R = R0*(1-CD) + R0*CD*a2
KK = K *(1+CK*a2)
dEP = 3/2 * < F/KK >**N * n
if p1 > pI : da2 = da4 = NN * p1**(NN-1) * dp
if p1 < pI : da2 = C2*(Q * pI**NN -a2) * dp - G1 * a2**R1 *dt
if p1 < pI : da4 = - BETA*a4*dp/p
For further details, refer to the CEA -N-2612 note.
The parameter values for the steel 316L at 600°C are given for
information only.
The data to be input are the following :
Values for Steel 316
Threshold evolution law : --------------------
'N ' : viscoplasticity threshold
exponent 20
'K ' : initial factor for threshold
normalization 10 MPa
'CK ' : constant in K evolution law 3.87
'R0 ' : initial value for the elastic
limit 80 MPa
'CD ' : constant in R evolution law 0.
Evolution law for the X centre :
'A ' : ALPHA2 coefficient 15000 MPa
'M ' : plastic strain exponent ( <1 ) 0.8
'A1 ' : plastic strain coefficient 200000 MPa
'C ' : ALPHA4 coefficient 40
'C1 ' : reference term coefficient 180
'C0 ' : tuning coefficient for ratchetting 0.
'P1M0' : threshold for tuning
'G ' : restoration term coefficient 1.5E-10 /se
'R ' : restoration term exponent 4
Evolution law for the ALPHA2 and ALPHA4 internal variables:
'NN ' : plastic strain exponent 0.075
'C2 ' : plastic strain coefficient 4
'Q ' : plastic strain coefficient 3.43
'G1 ' : restoration term coefficient 1.5E-6
'R1 ' : ALPHA2 exponent 4.
'BETA' : ALPHA4 coefficient 0.4
CHABOCHE viscoplastic model:
----------------------------
The equations for this model are as follows :
--> Notation : S stress tensor
Xi kinematic stress hardening variables
(i=1 ou 2)
EP inelastic strain tensor
p accumulated equivalent inelastic
strain
q isotropic variable for the memory surface
in deformation
Y kinematic variable for the memory surface
in deformation
I2 tensor second invariant
J2 deviatoric tensor second invariant
n normal from F criterion
nn normal from G threshold
t time
positive part of a
x.y scalar product of x by y
X = X1 for a single centre
X1+X2 for two centres
RR = ALFR * R
K = K0 + ALFK * R
Q(0)=Q0
--> Criterion : F = J2 (S-X) - RR - KK
--> Strain : dXi =2/3 * Ai*Ci*dEP - Ci*Xi*p'*dp
hardening - ( J2(Xi)/BETi )**(Ri-1) * Xi * dt (i=1-2)
if BETi is non zero, else :
dXi =2/3 * Ai*Ci*dEP - Ci*Xi*p'*dp (i=1-2)
with : p' = PHI+(1-PHI)* e** (-B*p)
dp = < F/K >**N * e**(ALF* < F/K >**(N+1))
dR = B*(Q - R)*dp + GAMA*Sign(QR-R)*|QR-R|**M *dt
--> Flow rule : dEP = 3/2 * dp * < S-X > / J2(S-X)
--> Memory of G = I2 (EP-Y) - q < 0
inelastic dQ = 2*MU*(QMAX-Q)* dq
strain dq = ETA * < n.nn > * dp
dY = (3/2 ** 0.5) * (1-ETA) * < n.nn > * nn*dp
QR = Q - QSTA * ( 1 - ((QMAX-Q)/QMAX)**2)
The initial value of Q is Q0 and must be initialized (see after)
For further details, see D. NOUAILHAS's report :
" A viscoplastic modelling applied to stainless steel behavior",
Second Inter. Conf. on Constitutive Laws for Engineering
Materials,
University of Arizona, Tucson,1987
The parameter values for the steel 316L at 600°C are given for
information only.
The data to be input are the following :
Values for Steel 316
Threshold evolution law : --------------------
'N ' : viscoplasticity threshold exponent 24
'KK ' : initial value for elastic limit 10 MPa
'K0 ' : initial factor for the threshold
normalization 116 MPa
'ALFK' : K isotropic evolution coefficient 1.5
'ALFR' : threshold isotropic evolution
coefficient 0.35
'ALF ' : viscosity coefficient 2.E6
Evolution law for the centres X1 and X2 :
'A1 ' : plastic strain coefficient 67.5 MPa
'C1 ' : reference term coefficient 1300
'BET1' : normalization factor for restoration 4807 MPa
'R1 ' : restoration term exponent 4
'A2 ' : plastic strain coefficient 80 MPa
'C2 ' : reference term coefficient 45
'BET2' : normalization factor for restoration 5840 MPa
'R2 ' : restoration term exponent 4
'PHI ' : reference term multiplying coefficient 1.
Evolution law for isotropic stress hardening :
'B ' : isotropic stress hardening coefficient 12
'GAMA' : restoration effect coefficient 2.E-7
'M ' : restoration term exponent 2
Evolution law for the plastic deformation memory :
'QMAX' : Q maximal value 455 MPa
'QSTA' : Q stabilized value 200 MPa
'MU ' : Q evolution law coefficient 19
'ETA ' : factor linking q with the plastic
strain 0.06
+ Initialization of internal variable Q : Q = Q0 = 30 MPa (steel 316)
For this purpose, a field of internal variables must be created,
with a component named 'QQ' , its value being Q0. This field
will be passed in the table argument of PASAPAS.
OHNO viscoplastic model :
-------------------------
The equations for this model are as follows :
--> Notation : S stress tensor
Xi kinematic stress hardening variables
(i=1 ou 2)
EP inelastic strain tensor
p accumulated equivalent inelastic
strain
q isotropic variable for the memory surface
in deformation
Y kinematic variable for the memory surface
in deformation
I2 tensor second invariant
J2 deviatoric tensor second invariant
n normal from F criterion
nn normal from G threshold
t time
positive part of a
x.y scalar product of x by y
X = X1 for a single centre
X1+X2 for two centres
RR = ALFR * R
K = K0 + ALFK * R
Q(0)=Q0
--> Criterion : F = J2 (S-X) - RR - KK
--> Strain hardening :
dXi =2/3 * Ai*Ci*dEP - Ci*Xi*p'*< dEP:Ki >*(J2(Xi)/LIMi)**EXPi
- ( J2(Xi)/BETi )**(Ri-1) * Xi * dt (i=1 or 2)
if BETi is non zero, else :
dXi =2/3 * Ai*Ci*dEP - Ci*Xi*dp' (i=1 or 2)
with : p' = PHI+(1-PHI)* e** (-B*p)
LIMi = Ai/p' (i=1 ou 2)
Ki = Xi/J2(Xi)
dp = < F/K >**N * e**(ALF* < F/K >**(N+1))
dR = B*(Q - R)*dp + GAMA*Sign(QR-R)*|QR-R|**M *dt
--> Flow rule : dEP = 3/2 * dp * < S-X > / J2(S-X)
--> Memory of G = I2 (EP-Y) - q < 0
inelastic dQ = 2*MU*(QMAX-Q)* dq
strain dq = ETA * < n.nn > * dp
dY = (3/2 ** 0.5) * (1-ETA) * < n.nn > * nn*dp
QR = Q - QSTA * ( 1 - ((QMAX-Q)/QMAX)**2)
The initial value of Q is Q0 and must be initialized (see after)
This model is close to the Chaboche's viscoplastic one.
The parameter values for the steel 316L at 600°C are given for
information only.
The data to be input are the following :
Values for Steel 316
Threshold evolution law : --------------------
'N ' : viscoplasticity threshold exponent 24
'KK ' : initial value for elastic limit 10 MPa
'K0 ' : initial factor for the threshold
normalization 116 MPa
'ALFK' : K isotropic evolution coefficient 1.5
'ALFR' : threshold isotropic evolution
coefficient 0.35
'ALF ' : viscosity coefficient 2.E6
Evolution law for the centres X1 and X2 :
'A1 ' : plastic strain coefficient 67.5 MPa
'C1 ' : reference term coefficient 1300
'BET1' : normalization factor for restoration 4807 MPa
'R1 ' : restoration term exponent 4
'A2 ' : plastic strain coefficient 80 MPa
'C2 ' : reference term coefficient 45
'BET2' : normalization factor for restoration 5840 MPa
'R2 ' : restoration term exponent 4
'PHI ' : reference term multiplying coefficient 1.
Evolution law for isotropic stress hardening :
'B ' : isotropic stress hardening coefficient 12
'GAMA' : restoration effect coefficient 2.E-7
'M ' : restoration term exponent 2
Evolution law for the plastic deformation memory :
'QMAX' : Q maximal value 455 MPa
'QSTA' : Q stabilized value 200 MPa
'MU ' : Q evolution law coefficient 19
'ETA ' : factor linking q with the plastic
strain 0.06
+ Initialization of internal variable Q : Q = Q0 = 30 MPa (steel 316)
For this purpose, a field of internal variables must be created,
with a component named 'QQ' , its value being Q0. This field
will be passed in the table argument of PASAPAS.
LEMAITRE viscoplastic model liable to be damaged :
-------------------------------------------------
Notation :
S : stress tensor
dev(S) : stress tensor deviator
tr(S) : stress tensor trace
J0(S) : maximum principal stress
Seq : VON MISES equivalent stress
p : accumulated inelastic strain
D : damage variable
X(S) : creep equivalent stress
The equations for this model are :
dEP = (3/2) * dp * (dev(S) / Seq)
dq = dp * (1 - D)
dq = ( Seq/((1 - D) * KK * (q**(1/M))) ) ** N
dD = (< X(S)/A > ** R) * ((1 - D)**-k) with k function
X(S)= ALP1 * J0(S) + BLP1 * (tr(S)/3) + (1 - ALP1 - BLP1) * Seq
= 0 si y < 0 ; = y si y > 0
The data to be input are the following :
N,M,KK : parameters defining the creep law
A,R : parameters defining the D damage evolution law
ALP1,BLP1 : parameters defining the creep equivalent stress
X(S)
EVOL : key word followed by :
NOMEVOL : curve defining the evolution of the k parameter with
the creep equivalent stress X(S)
This curve is composed of an EVOLUTIO type object
with X(S) in abscissa and k in ordinate
If k is constant, define a constant evolution
SMAX : stress of reference (equalling by default Young's modulus
times 1.E-3)
REMARK FOR MATERIAL VARYING WITH TEMPERATUE T
+++++++++++++++++++++++++++++++++++++++++++++
if the temperatures used to define the evolution of the
N,M,KK,A,R,ALP1,BLP1,EVOL parameters are the same for all them
then
for T = (1 - teta)*T1 + teta*T2
the internal variables rates are :
V(T) = (1 - teta)*V(T1) + teta*V(T2)
V(Ti) being the rate calculated with parameters values
obtained for temperature Ti (i=1,2)
else
V(T) is calculated with parameters values
obtained for temperature T
endif
Perfectly viscoplastic modele:
------------------------------
The viscoplastic deformation rate is given by
devp/dt = ( (s-sigy) / k)**N * (s'/s)
The required parameters are
SIGY : yield stress (no hardening)
K : viscisity parameter
N : exponent of the law
This model works even if SIGY = 0.
Powder viscoplastic models :
----------------------------
Model of ABOUAF for consolidation of powders.
Equations of the model are :
--> Notations :
S stress tensor
s deviator stress tensor
d unit tensor
Seq equivalent stress
I1 first invariant of stress tensor
J2 second invariant of deviatoric stress tensor
rho relative density of porous material
f function of relative density
c function of relative density
evp viscoplastic deformation
t time
T temperature
--> Constitutive equations of Abouaf model :
Seq = (f*I1**2+3/2*c*J2**2)**0.5
devp/dt = rho*A*exp(-Q/RT)*Seq**(n-1)*(f*I1*d+3/2*c*s)
tr(devp/dt) = -(drho/dt)/rho
--> Data to input :
A coefficient of creep law
N power creep law exponent
QSRT activation energy
F0->F5 parameters defining the f function
C0->C5 parameters defining the c fonction
RHOR initial relative density of the material
--> to get any informations, please contact : /DTA/CEREM/SGM
F. Moret 76.88.53.40
C. Dellis 76.88.57.26
P. Le Gallo 76.88.54.64
Two inelastic strain viscoplastic model (DDI) :
-----------------------------------------------
The equations for this model are as follows:
--> Notation : S stress tensor
EP plastic strain tensor
p accumulated equivalent plastic strain
EV creep strain tensor
v accumulated equivalent creep strain
Xpi, Xvi kinematic stress hardening variables (i=1,2)
Rp, Rv isotropic stress hardening variables
J2 deviatoric tensor second invariant
np normal from Fp criterion
nv normal from Fv criterion
positive part of a
Xp = Xp1
Xv = Xv1 for a single centre
Xp = Xp1+Xp2
Xv = Xv1+Xv2 for two centres
--> Criterions : Fp = J2(S-Xp) - Rp
Fv = J2(S-Xv) - Rv
--> Stress : Xp1 = 2/3CP1*ALPHAp1 + 2/3CVP1*ALPHAv1
hardening Xp2 = 2/3CP2*ALPHAp2 + 2/3CVP2*ALPHAv2
Xv1 = 2/3CV1*ALPHAv1 + 2/3CVP1*ALPHAp1
Xv2 = 2/3CV2*ALPHAv2 + 2/3CVP2*ALPHAp2
dALPHApi = dEp - 3/2*(DPi/CPi)*Xpi*dp (i=1,2)
dALPHAvi = dEv - 3/2*(DVi/CVi)*Xvi*dv (i=1,2)
Rp = RP0 + QP*(1-exp(-BP*p))
Rv = RV0 + Qv*(1-exp(-BV*v))
--> Flow rule : dp verifies dFp=0
dEp = 3/2 * dp * < S-Xp > / J2(S-Xp)
dV = (< Fv > / KS) ** n
dEv = 3/2 * dv * < S-Xv > / J2(S-Xv)
Data to be input:
Evolution law for the centres Xpi and Xvi :
'CP1' : ALPHAp1 coefficient
'CP2' : ALPHAp2 coefficient
'CV1' : ALPHAv1 coefficient
'CV2' : ALPHAv2 coefficient
'CVP1' : Visco-plastic coupling coefficient
'CVP2' : Visco-plastic coupling coefficient
Evolution law for the ALPHApi et ALPHAvi internal variables:
'DP1' : ALPHAp1*dp coefficient
'DP2' : ALPHAp2*dp coefficient
'DV1' : ALPHAv1*dv coefficient
'DV2' : ALPHAv2*dv coefficient
Evolution law for isotropic stress hardening:
'BP' : P coefficient
'QP' : plastic strain isotropic hardening coefficient
'RP0' : initial plastic threshold value
'BV' : V coefficient
'QV' : creep strain isotropic hardening coefficient
'RV0' : initial creep threshold value
Evolution law for the creep strain:
'KS' : creep threshold normalization coefficient
'N' : creep law exponent
Athermal Visco elasto plastic Model of KOCKS :
---------------------------------------------------
Constitutive equation :
--> Notations : S isotropic deformation resistance (internal
variable)
SP S variation rate
J2 second invariant for deviatoric stresses
EPP equivalent plastic tensile strain rate
--> Evolution law : EPP = A [SINH(B*J2/S) ** 1./M * EXP(-Q/RT)
--> Variation of internal variable :
SP = H0 (ABS (Ssat - S)/(Ssat - S0))*SIGN(Ssat -S0)*EPP
Saturation of S :
Ssat = SB*(Z/A)**N
Zener Holomon parameter : Z = EPP*EXP(Q/RT)
Data to be input :
'A ' :pre exponential factor
'B ' :normalisation factor for variable S
'M ' :exponent
'Q ' :activation energy
'R ' :gas constant
'H0 ' :athermal initial hardening rate
'AP ' :exponent of hardening law
'SB ' :saturation coefficient
'N ' :exponent for saturation law
'S0 ' :initial value of S parameter
NOUAILLAS_A viscoplastic model:
----------------------------
The difference between this model and the CHABOCHE viscoplastic model
is only on the way to calculated the kinematic stress hardening.
The equations for this model are as follows :
--> Notation : S stress tensor
Ai kinematic stress hardening variables (i=1-2)
Xi kinematic stress hardening (i=1 ou 2)
EP inelastic strain tensor
p accumulated equivalent inelastic
strain
q isotropic variable for the memory surface
in deformation
Y kinematic variable for the memory surface
in deformation
I2 tensor second invariant
J2 deviatoric tensor second invariant
n normal from F criterion
nn normal from G threshold
t time
positive part of a
x.y scalar product of x by y
X = X1 for a single centre
X1+X2 for two centres
RR = ALFR * R
K = K0 + ALFK * R
Q(0)=Q0
--> Criterion : F = J2 (S-X) - RR - KK
--> Strain hardening : Xi = 2/3 * CLi * Ai
dAi = dEP - DNLi * Ai * p' * dp
- 3/2 ( J2(Xi)/GDMi )**(PTMi) * (Xi/J2(Xi)) * dt (i=1-2)
if GDMi is non zero, else :
dAi = dEP - DNLi * Ai * p' * dp (i=1-2)
with : p' = PHI+(1-PHI)* e** (-B*p)
dp = < F/K >**N * e**(ALF* < F/K >**(N+1))
dR = B*(Q - R)*dp + GAMA*Sign(QR-R)*|QR-R|**M *dt
--> Flow rule : dEP = 3/2 * dp * < S-X > / J2(S-X)
--> Memory of G = I2 (EP-Y) - q < 0
inelastic dQ = 2*MU*(QMAX-Q)* dq
strain dq = ETA * < n.nn > * dp
dY = (3/2 ** 0.5) * (1-ETA) * < n.nn > * nn*dp
QR = Q - QSTA * ( 1 - ((QMAX-Q)/QMAX)**2)
The initial value of Q is Q0 and must be initialized (see after)
For further details, see D. NOUAILHAS's report :
" A viscoplastic modelling applied to stainless steel behavior",
Second Inter. Conf. on Constitutive Laws for Engineering
Materials,
Threshold evolution law :
'N ' : viscoplasticity threshold exponent
'KK ' : initial value for elastic limit
'K0 ' : initial factor for the threshold
normalization
'ALFK' : K isotropic evolution coefficient
'ALFR' : threshold isotropic evolution
coefficient
'ALF ' : viscosity coefficient
Evolution law for the centres X1 and X2 :
'CL1 ' : plastic strain coefficient
'DNL1' : reference term coefficient
'GDM1' : normalization factor for restoration
'PTM1' : restoration term exponent
'CL2 ' : plastic strain coefficient
'DNL2' : reference term coefficient
'GDM2' : normalization factor for restoration
'PTM2' : restoration term exponent
'PHI ' : reference term multiplying coefficient
Evolution law for isotropic stress hardening :
'B ' : isotropic stress hardening coefficient
'GAMA' : restoration effect coefficient
'M ' : restoration term exponent
Evolution law for the plastic deformation memory :
'QMAX' : Q maximal value
'QSTA' : Q stabilized value
'MU ' : Q evolution law coefficient
'ETA ' : factor linking q with the plastic
strain
+ Initialization of internal variable Q : Q = Q0 = 30 MPa (steel 316)
For this purpose, a field of internal variables must be created,
NOUAILLAS_B viscoplastic model:
----------------------------
The difference between this model and the NOUAILLAS_A viscoplastic
model is only mainly on the evolution of the isotropic hardening.
The equations for this model are as follows :
--> Notation : S stress tensor
Ai kinematic stress hardening variables (i=1-2)
Xi kinematic stress hardening (i=1 ou 2)
EP inelastic strain tensor
p accumulated equivalent inelastic
strain
I2 tensor second invariant
J2 deviatoric tensor second invariant
t time
positive part of a
X = X1 for a single centre
X1+X2 for two centres
--> Criterion : F = J2 (S-X) - RR
--> Strain hardening : X1 = 2/3 * CL1 * A1
dA1 = dEP - DNL1 * A1 * p' * dp
- 3/2 ( J2(X1)/GDM1 )**(PTM1) * (X1/J2(X1)) * dt
if GDM1 is non zero, else :
dA1 = dEP - DNL1 * A1 * p' * dp
X2 = 2/3 * CL2 * A2
dA2 = dEP - DNL2 * A2 * p' * dp
with : p' = PHI+(1-PHI)* e** (-B*p)
dp = < F/K >**N * e**(ALF* < F/K >**(N+1))
dR = B*(Q - R)*dp + GAMA*Sign(QR-R)*|QR-R|**M *dt
--> Flow rule : dEP = 3/2 * dp * < S-X > / J2(S-X)
The initial value of Q is Q0 and must be initialized (see after)
For further details, see D. NOUAILHAS's report :
" A viscoplastic modelling applied to stainless steel behavior",
Second Inter. Conf. on Constitutive Laws for Engineering
Materials,
Threshold evolution law :
'N ' : viscoplasticity threshold exponent
'KK ' : initial value for elastic limit
'K0 ' : initial factor for the threshold
normalization
'ALF ' : viscosity coefficient
Evolution law for the centres X1 and X2 :
'CL1 ' : plastic strain coefficient
'DNL1' : reference term coefficient
'GDM1' : normalization factor for restoration
'PTM1' : restoration term exponent
'CL2 ' : plastic strain coefficient
'DNL2' : reference term coefficient
'PHI ' : reference term multiplying coefficient
'B ' : kinematic stress hardening coefficient
Evolution law for isotropic stress hardening :
'RMAX' : R maximal value
'BR ' : R coefficient
VISK2 viscoplastic model :
-----------------------------
Beneath the threshold the stress-strain equation is equivalent to
elasticity. Beyond, a plastic kinematic hardening effect is added
to a viscoelastic Maxwell type effect, with an extension to
nonlinear law. (DMT 98/013)
Please give the following data :
'SIGY' : elastoplastic threshold
'H ' : kinematic hardening
'ETA ' : viscoelastic coefficient
'HVIS' : viscoelastic modulus
'N ' : viscoelastic exponent
General Strain model MISTRAL considered as a viscoplastic behaviour
-------------------------------------------------------------------
This model applies for an orthotropic material and consider the
following strains:
- thermal strain,
- elastic strain,
- 0 or 1 instantaneous plastic strain,
- 0 to 3 viscoplastic strains,
- irradiation growth.
De ce fait, pour tout materiau traite par MISTRAL :
- la dilatation thermique existant par ailleurs dans CASTEM
doit etre mise àzero : 'ALP1' 0. 'ALP2' 0. 'ALP3' 0. ,
- les coefficients d'elasticite doivent etre definis de la
façon generale existant dans CASTEM pour un materiau orthotrope :
'YG1 ' E1 'YG2 ' E2 'YG3 ' E3
'NU12' NU12 'NU23' NU23 'NU13' NU13
'G12 ' MU12 ['G13 ' MU13 'G23 ' MU23]
mais les objets E1, E2, E3, NU12, NU23, NU13, MU12, [MU23, MU13]
sont necessairement des evolutions donnant les coefficients
d'elasticite en fonction de la temperature absolue (en K).
Le modele MISTRAL fonctionne pour des elements massifs et pour
les types de calcul suivants : tridimensionnel, axisymetrie,
deformations planes, contraintes planes et deformations planes
generalisees.
Les donnees àintroduire sont les suivantes :
'DILT' : PDILT, liste de reels contenant les parametres des
fonctions traduisant l'evolution des coefficients de
dilatation thermique en fonction de la temperature.
'NDIM' : NDIME, liste de 4 entiers en format reel contenant :
- le nombre de deformations plastiques instantanees ÃÂ
seuil (0 ou 1),
- le nombre de deformations viscoplastiques (0 à3),
- le numero maximal de niveau de contraintes internes
pour toute deformation plastique precedente (0 à2 dans
version actuelle), le niveau 0 correspondant aux
contraintes internes (directement) mesurables,
- 1 ou 0 selon qu'il existe ou non des couplages par
les contraintes internes entre deformations plastiques
de natures differentes.
'COHI' : PCOHI, liste de reels contenant les parametres des
fonctions traduisant l'evolution des coefficients
d'anisotropie plastique (de Hill) en fonction de la
temperature et de la fluence de neutrons rapides *.
'ACOU' : PECOU, liste de reels contenant les parametres relatifs
àla loi d'ecoulement **.
'ECRI' : PECRI, liste de reels contenant les parametres relatifs
àla loi d'ecrouissage isotrope *.
'ECRC' : PECRC, liste de reels contenant les parametres relatifs
àla loi d'ecrouissage cinematique *.
'DURI' : PDURI, liste de reels contenant les parametres relatifs
àla variable de durcissement d'irradiation *.
* : pour toutes les deformations plastiques
** : pour toutes les deformations viscoplastiques
'CROI' : PCROI, liste de reels contenant les parametres de la loi
de croissance sous irradiation.
'INCR' : PINCR, liste de reels contenant les increments maximaux
autorisees pour la determination automatique du pas de
temps lors de l'integration des equations d'evolution
des variables materiau par MISTRAL.
Avec certains types de calcul de CASTEM, toutes les bases de
l'espace à3 dimensions ne sont pas accessibles pour la base
principale d'orthotropie, par exemple : la base (radiale,
circonferentielle, axiale) n'est pas accessible en mode
axisymetrique (la direction circonferentielle est toujours en
3eme position). Or les lois des gaines des combustibles sont
habituellement exprimees dans cette base.
C'est pourquoi on doit fournir les deux nombres suivants pour
definir la base principale d'orthotropie pour MISTRAL (toujours dans
l'espace à3 dimensions) par rapport àla base principale
d'orthotropie pour CASTEM (il s'agit d'une simple permutation des
axes avec eventuel changement de sens pour conserver l'orientation
de l'espace) :
'SIP1' : SENSIP1, numero d'ordre de la 1ere direction de la base
MISTRAL dans la base CASTEM, affecte du signe - s'il y a
changement de sens.
'SIP2' : SENSIP2, numero d'ordre de la 2eme direction de la base
MISTRAL dans la base CASTEM, affecte du signe - s'il y a
changement de sens.
Avant l'appel àl'operateur 'MATE', les donnees peuvent etre lues
sur un fichier, et en plus mises en forme adaptee àCASTEM pour les
coefficients d'elasticite, par la procedure @mistpar de la façon
suivante :
fichier = 'nom du fichier de donnees' ;
PDILT E1 E2 E3 NU12 NU23 NU13 MU12 MU23 MU13
NDIME PCOHI PECOU PECRI PECRC PDURI PCROI PINCR
= @mistpar fichier SENSIP1 SENSIP2 ;
Les nombres SENSIP1 et SENSIP2, affecte à'SIP1' et 'SIP2' dans
l'operateur 'MATE', sont arguments de cette procedure pour transformer
les coefficients d'elasticite de la base d'orthotropie MISTRAL
àcelle de CASTEM.
GATT_MONERIE model :
--------------------
The GATT_MONERIE model describes viscoplasticity behaviour of
standard UO2 fuel or with additional chromium. It is available when
using solid elements and for the following types of calculation :
three-dimensional, axisymmetrical, plane strains, plane stresses and
generalized plane strains.
In this model :
the Young's modulus E is expressed as follows :
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
E = Em(T) * Ef(f)
where: Em(T) is a function of the temperature (possibly a constant)
T expressed in Kelvin
Ef(f) is a function of the porosity f of the material
(possibly a constant)
f is an internal variable of the model representing porosity
the shear modulus G is expressed as follows :
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
G = Gm(T) * Gf(f)
where: Gm(T) is a function of the temperature (possibly a constant)
T expressed in Kelvin
Gf(f) is a function of the porosity f of the material
(possibly a constant)
f is an internal variable of the model representing porosity
the POISSON coefficient NU is deduced from :
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
NU = (E/2G) - 1
the thermal expansion coefficient ALPHA is expressed as follows :
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
ALPHA = ALPHAm(T) * ALPHAf(f)
where: ALPHAm(T) is a function of the temperature (possibly a
constant) T expressed in Kelvin
ALPHAf(f) is a function of the porosity f of the material
(possibly a constant)
f is an internal variable of the model representing porosity
As part of this model, the data - concerning the elastic behaviour
of the model - to be input are as follows :
'YOUN' : Young's modulus
'NU ' : Poisson's ratio
'ALPH' : thermal expansion coefficient
'RHO ' : initial density
ALPH is COMPULSORY
RHO is COMPULSORY (see below)
The visco-plastic strain Evp consists of a primary and secondary
creep which has its origin in thermal effects, and a creep due to
irradiation.
Creep due to thermal effects :
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
The primary creep rate vEvp0 is expressed as follows :
vEvp0 = 1.5 * KPRIM * ( Sigeq**(AP-1)) / Evpq**BP ) * Sigprim
Two mechanisms (diffusion and dislocation) are involved in
secondary creep.
For each of theses two mechanisms, the thermodynamic potential PSIi
is defined as
(i=1 : first mechanism / i=2 : second mechanism) :
PSIi = (AKi /(Ni+1)) *
( Ai(f)*((1.5*Sigm)**2) + Bi(f)*(Sigeq**2) ) ** ((Ni+1)/2) )
where: Sigma is the stress tensor,
Sigm = (trace Sigma)/3,
II is the identity tensor,
Sigprim = Sigma - Sigm*II,
Sigeq is the Von Mises equivalent stress :
Sigeq = (1.5 * Sigprim : Sigprim)**0.5
Evpq = ( (2/3) * (Evp :: Evp) ) ** 0.5
Evp :: Evp is the tensorial product of
visco-plastic strain Evp
KPRIM = KP * exp(- QP/R*T)
Ai(f) and Bi(f) are functions of the porosity f :
Ai(f) = (Ni*(f**(-1/Ni) - 1))**(-2*Ni/(Ni+1))
Bi(f) = (1 +(2f/3)) / ( (1-f)**(2*Ni/(Ni+1)) )
(Ni a constant of the model)
AK1 = WC1 * K1 * (DG**M1) * exp(- Q1/R*T)
WC1 = 1 + 0.5*CR1*[1+th((CR-CR2)/CR3)]
AK2 = WC2 * K2 * (DG**M2) * exp(- Q2/R*T)
WC2 = 2 * [1-cos(DG/DG0)]
(KP, AP, BP, Ki, Ni and Mi constants of the model,
QP primary creep activation energy,
Qi mechanism i activation energy,
CR1, CR2, CR3 constants for the diffusion mechanism,
CR chromium concentration,
DG grain size,
DG0 constant for the dislocation mechanism,
R universal gas constant,
T temperature expressed in Kelvin)
For each mechanism, the creep rate vEvpi is expressed as follows :
vEvpi =
(1/3 * dPSIi/dSigm * II) + (1.5 * dPSIi/dSigeq * Sigprim/Sigeq)
that is :
vEvpi = 0.5 * AKi *
( ( Ai(f)*((1.5*Sigm)**2) + Bi(f)*(Sigeq**2) ) ** ((Ni-1)/2) ) *
( Ai(f)*1.5*Sigm*II + 3*Bi(f)*Sigprim)
The thermodynamic potential PSI is the result of coupling between
the two mechanisms using the static coupling function Theta0 or
the dynamic coupling function Theta :
PSI = (1-Theta0)*PSI1 + Theta0*PSI2 or
PSI = (1-Theta )*PSI1 + Theta *PSI2
Definition of the static coupling function Theta0 :
---------------------------------------------------
Theta0(T,GSigeq) = 0.5*BETA * (1 + th((T-(OMEG*(GSigeq**(-Q))))/H))
(th : hyperbolic tangent,
OMEG, Q and H constants of the model,
BETA : parameter which allows to introduce the coupling)
and dTheta0/dSigma = 0.5*BETA*Q*(OMEG/H)*(GSigeq**(-Q-2)) *
[1-(th((T-(OMEG*(GSigeq**(-Q))))/H)**2] *
[(9A1/(4B1+A1))*Sigm*II + 1.5*(B1/(B1+A1/4))*Sigprim]
where GSigeq =
( (B1/(B1+A1/4)) * (Sigeq**2) + (9A1/(4B1+A1)) * (Sigm**2) ) ** 0.5
Definition of the dynamic coupling function Theta :
---------------------------------------------------
vTheta(T,Sigeq) = signe(Theta0-Theta)*((Theta0-Theta)**2)/Theta0/to
(Theta0 : static coupling function defined above,
to caracteristic time, depending only on grain size for UO2 fuel
and equal to
to = DYN1 * (1 + th((DYN2-T)/DYN3)) + 1 for AFA3GLAA fuel,
DYN1, DYN2 and DYN3 constants of the model)
The creep rate vEvp12 due to the two mechanisms and the static
coupling, is expressed as follows :
vEvp12 = (1-Theta0)*vEvp1 + Theta0*vEvp2 + dTheta0/dSigma*(PSI2-PSI1)
The creep rate vEvp12 due to the two mechanisms and the dynamic
coupling, is expressed as follows :
vEvp12 = (1-Theta)*vEvp1 + Theta*vEvp2
The thermal creep rate (primary and secondary) is expressed by :
vEvp = vEvp0 + vEvp12
This creep rate vEvp is moreover multiplied by an acceleration
factor, the expression of which is : 1 + K*PHI
with: PHI the fission flux,
K a constant of the model
Creep due to irradiation :
^^^^^^^^^^^^^^^^^^^^^^^^^^
The creep rate vEvpir is expressed as follows :
vEvpir = A * PHI * (Sigma**(N3-1))*exp(-Q3/R*T)
where: Sigma is the stress tensor,
Sigm = (trace Sigma)/3,
II is the identity tensor,
Sigprim = Sigma - Sigm*II,
A and N3 are constants of the model,
PHI is the fission flux,
Q3 is the system activation energy,
R is the universal gas constant,
T is the temperature expressed in Kelvin
As part of this model, the data - concerning the visco-plastic
behaviour of the model - to be input are as follows :
'R ' : universal gas constant
For the two mechanisms related to the creep due to thermal effects :
'DG ' : grain size
for primary creep :
'KP ' : a constant of the model
'AP ' : a constant of the model
'BP ' : a constant of the model
'QP ' : primary creep activation energy
for the first mechanism (secondary creep) :
'K1 ' : a constant of the model
'M1 ' : a constant of the model
'Q1 ' : first mechanism activation energy
'N1 ' : a constant of the model
'CR ' : chromium concentration
'CR1 ' : a constant of the model
'CR2 ' : a constant of the model
'CR3 ' : a constant of the model
for the second mechanism (secondary creep) :
'K2 ' : a constant of the model
'M2 ' : a constant of the model
'Q2 ' : second mechanism activation energy
'N2 ' : a constant of the model
'DG0 ' : a constant of the model
for the coupling between the two mechanisms :
'OMEG' : a constant of the model
'Q ' : a constant of the model
'H ' : a constant of the model
'BETA' : 1. or 0. if coupling is taken into consideration or not
for the acceleration applied to the creep due to thermal effects :
'K ' : a constant of the model
for the creep due to irradiation :
'A ' : a constant of the model
'Q3 ' : system activation energy
'N3 ' : a constant of the model
The strain rate related to solid swelling is expressed as follows :
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
vEgs = (1/3) * KGON * (d Bu / dt) * II
The strain rate related to densification is expressed as follows :
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
vEd = (1/3) *
d/dt [-1*(1+KGON*Bu)*A*Ln(Bu/BUMI)/(1 - POR0 + A*Ln(Bu/BUMI))]
* II
where II is the identity tensor
A coefficient is obtained from an iterative method, which
requires the following data :
'ADEN' : specific data of the material
'KGON' : swelling coefficient
'BUMI' : burn-up threshold under which the density is constant
Bu is the burn-up : internal variable of the model
The Bu computation from the time evolution of PHI (fission flux)
requires the following data :
'RHO ' : initial density
'EFIS' : mean energy per fission
'POR0' : initial porosity
Optional data :
'TYPE' : 0. (default value) if UO2 fuel, 1. if AFA3GLAA fuel
'COMP' : 0. (default value) if compressible fuel, 1. if not
'DYN ' : 0. (default value) if static coupling,
1. if dynamic coupling
for UO2 fuel :
'DYN1' : constant of the dynamic coupling function (to)
for AFA3GLAA fuel :
'DYN1' : constant of the dynamic coupling function
'DYN2' : constant of the dynamic coupling function
'DYN3' : constant of the dynamic coupling function
Before using the 'MATE' operator, the data can be read in a file,
and written in an appropriate format for CAST3M, thanks to the
@GATTPAR procedure, the syntax of which is :
file = 'name of the data file' ;
tata = '@GATTPAR' file ;
(see the @GATTPAR procedure notice for further information)
UO2 model :
-----------
The UO2 model describes viscoplasticity behaviour of standard UO2
fuel or with addiational chromium and takes into account fracture
under tensile loading. This model results from the coupling between
the fracture model proposed by OTTOSEN and the viscoplasticity
GATT_MONERIE model. It is available :
- when using solid elements and for the following types of
calculation : three-dimensional, axisymmetrical, plane strains,
plane stresses and generalized plane strains
- when using thin shell elements with or without transverse shear
in three-dimensional calculations
For the description of the data to be input for using this model,
please refer to the chapter related to the GATT_MONERIE model
concerning viscoplasticity caracteristics.
The fracture caracteristics to be input are as follows :
('LTR') : limit stress in tension (default value YOUN*1.2E-4)
('LTR1') : limit stress in tension for the first fracture direction
(default value LTR)
('LTR2') : limit stress in tension for the second fracture direction
(default value LTR)
('LTR3') : limit stress in tension for the third fracture direction
(default value LTR) - not available under plane stresses
condition nor for calculations using shell elements
('GFTR') : restitued energy ratio (i.e. the fracturing energy)
(default value LTR*3.9E-5)
('GFT1') : fracturing energy for the first fracture direction
(default value GFTR)
('GFT2') : fracturing energy for the second fracture direction
(default value GFTR)
('GFT3') : fracturing energy for the third fracture direction
(default value GFTR) - not available under plane stresses
condition nor for calculations using shell elements
('GS') : modulus providing the loss of shear resistance of a
fracture with its normal opening
(default value YOUN*1.8E-4)
('GS1') : for the first fracture direction
modulus providing the loss of shear resistance of a
fracture with its normal opening (default value GS)
('GS2') : for the second fracture direction
modulus providing the loss of shear resistance of a
fracture with its normal opening (default value GS)
('GS3') : for the third fracture direction
modulus providing the loss of shear resistance of a
fracture with its normal opening (default value GS) -
not available under plane stresses condition nor for
calculations using shell elements
('EPSR') : failure strain in the direction normal to the
mesh plane in case of axisymmetrical, plane strains
or generalized plane strains calculations
(default value 3.*LTR/YOUN)
('EPSB') : strain determining the slope change in case of a bilinear
relation between stress and fracture opening strain in
the direction normal to the mesh plane for
axisymmetrical, plane strains or generalized plane
strains calculations (default value 0.)
('WRUP') : opening displacement inducing rupture (default value 0.)
('WRU1') : opening displacement inducing rupture for the first
fracture direction (default value WRUP or 2*GFT1/LTR1 if
WRUP=0.)
('WRU2') : opening displacement inducing rupture for the second
fracture direction (default value WRUP or 2*GFT2/LTR2 if
WRUP=0.)
('WRU3') : opening displacement inducing rupture for the third
fracture direction (default value WRUP or 2*GFT3/LTR3 if
WRUP=0.) - not available for calculations using shell
elements or undertaken with plane stresses,
plane strains, generalized plane strains or
axisymmetrical conditions
('BILI') : opening determining the slope change in case of a
bilinear relation between stress and fracture opening
(default value 0.)
('BIL1') : for the first fracture direction
opening determining the slope change in case of a
bilinear relation between stress and fracture opening
(default value BILI)
('BIL2') : for the second fracture direction
opening determining the slope change in case of a
bilinear relation between stress and fracture opening
(default value BILI)
('BIL3') : for the third fracture direction
opening determining the slope change in case of a
bilinear relation between stress and fracture opening
(default value BILI) - not available for calculations
using shell elements or undertaken with plane stresses,
plane strains, generalized plane strains or
axisymmetrical conditions
('BTR') : non recoverable opening ratio (default value 0.2)
('SIMP') : allows to simplify or not the resolution
0. exact resolution
1. simplified resolution - fracturing energy is supposed
to be equal to zeo
(default value 0.)
Remark : the default values are given in the international unit
-------- system
The CHAML result of the operator TAILLE applied to the model, must be
added to the CHAML built by MATE operator.
VISCODD model :
-----------------------
The constitutive equations read as :
--> stating : S stress tensor
SEQ damage equivalent stress
EP anelastic strain tensor
p equivalent anelastic strain
M anisotropic damage tensor built on DC
t time
positive part of a
r isotropic hardening parameter
R isotropic hardening threshold
DD isotropic smooth damage
YD energy rate for smooth damage
DC creep anisotropic damage
YC energy rate for creep damage
H(.) Heaviside function
--> Compute SEQ : SEQ = SQRT((S:M:S)/((1-DD)*(1-DC))
--> Criteria : F = SEQ - R - SIGY
--> Hardening : dR = b*(Ri - R)*dr
--> Viscosity law : dr = **n dt
--> Yield law : dEP = dr * M:S / (SEQ*(1-DD)*(1-DC))
--> Smooth damage : dDD = (YD/sd)**rd*dr * H(p-pd)
--> Creep damage : dDC = (YC/sc)**rc * dt * H(p-pc)
The parameters of the constitutive equations follow as :
'N ' : exponent for the viscoplastic equation
'K ' : viscosity modulus
'B ' : hardening coefficient
'RI ' : limit value for hardening
'SIGY' : elasticity threshold
'SD ' : smooth damage coefficient
'RD ' : smooth damage exponent
'PD ' : smooth damage threshold
'SC ' : creep damage coefficient
'RC ' : creep damage exponent
'PC ' : creep damage threshold
The short test visco2d.dgibi treats a 16MND5 steel short cylinder
following this model. For further detail splease refer to
B. Vereecke thesis :
"Probabilistic analysis of the evolution of a set of pressure
vessel steels in case of extreme loading".
"Analyse probabiliste du comportement d'une famille d'aciers pour
cuve de REP en cas d'accident grave ",
These de doctorat, Universite Paris 6, LMT-Cachan
SYCO1 model
-----------
This modele is compatible with 2D plane stress, 2D plane strain
and 3D formulations and with massive and XFEM elements.
The viscoplastic constitutive law of Symonds & Cowper "standard"
is given by:
sig_dyn(T,epse,rate_epse) = sig_stat(T,epse)*(1+(rate_epse/D)**(1/p))
where sig_dyn is the dynamic Von Mises equivalent stress,
sig_stat is the static Von Mises equivalent stress,
epse if the cumulated equivalent plastic strain,
rate_epse is the rate of the cumulated equivalent plastic strain,
D and p are the constants caracterising the material's viscosity.
Parameters of the material:
'PSYC' p
'DSYC' D
SYCO2 model
-----------------
This modele is compatible with 2D plane stress, 2D plane strain
and 3D formulations and with massive and XFEM elements.
The modified viscoplastic constitutive law of Symonds & Cowper
is given by:
sig_dyn(T,epse,rate_epse) = sig_stat(T, epse)*(1+ H(T,epse)*(rate_epse**(1/p)
where sig_dyn is the dynamic Von Mises equivalent stress,
sig_stat is the static Von Mises equivalent stress,
epse if the cumulated equivalent plastic strain,
rate_epse is the rate of the cumulated equivalent plastic strain,
and H(T, epse) = A + B * EXP(-epse/C).
A, B, C et p are the constants caracterising the material's viscosity.
Parameters of the material:
'PSYC' P
'ASYC' A
'BSYC' B
'CSYC' C
-----------------------------------------------
| Parameter name for a VISCO_EXTERNE material |
-----------------------------------------------
The parameters of all the laws of the 'VISCO_EXTERNE' group are the
same as these of the 'ELASTIQUE' 'ISOTROPE' behavior.
-----------------------------------------------------------
| Parameter name for an ELASTIQUE MODAL material |
-----------------------------------------------------------
'FREQ' : frequency ('FLOTTANT' type)
'MASS' : generalised mass ('FLOTTANT' type)
'DEFO' : eigenmode ('CHPOINT' type)
Optional parameter
'AMOR' : generalised damping ('FLOTTANT' type)
'CGRA' : center of rotation ('POINT' type)
-----------------------------------------------------------
| Parameter name for an ELASTIQUE STATIQUE material |
-----------------------------------------------------------
'RIDE' : result of product stiffness * displacement ('CHPOINT' type)
'MADE' : result of product mass * displacement ('CHPOINT' type)
'DEFO' : displacement field ('CHPOINT' type)
Optional parameter
'AMOR' : generalised damping ('FLOTTANT' type)
b) Cas d'une formulation LIQUIDE
________________________________
---------------------------------------
| Noms des parametres pour un LIQUIDE |
---------------------------------------
b) Case of a LIQUIDE formulation
________________________________
--------------------------------
| Parameter name for a LIQUIDE |
--------------------------------
'RHO ' : density
'RORF' : reference density
'CSON' : sound speed
'CREF' : reference speed
'LCAR' : length scale
'G ' : gravity acceleration
------------------------------------------------------------
| Parameter name for a fluid-structure homogeneized medium |
------------------------------------------------------------
'B11 ' : acoustic permeability with respect to the axis X
'B22 ' : acoustic permeability with respect to the axis Y
'B12 ' : mixed acoustic permeability
'ROF ' : fluid density
'CSON' : sound speed in the fluid
'YOUN' : pipe stiffness
'ROS ' : pipe density
'RORF' : fluid reference density
'CREF' : reference speed in the fluid
'LCAR' : typical length scale of the fluid domain
'E111' : |
'E112' : |
'E121' : | second order cellular coefficients
'E122' : |
'E221' : |
'E222' : |
------------------------------------------------------
| Parameter name for a fluid-pipe transition element |
------------------------------------------------------
'RHO ' : density
'RORF' : reference density
'LCAR' : typical length scale
c) Case of THERMIQUE and DARCY formulations
_______________________________________________________
-------------------------------------------
| Parameter name in THERMIQUE formulation |
-------------------------------------------
'K' : isotropic conductivity
'RHO' : specific mass
'C' : specific heat
'H' : exchange coefficient
- for phase changing
'TPHA' : temperature of transformation phase
'QLAT' : latent heat per unit of mass
- For CONVECTION
'H' :exchange coefficient
- For RAYONNEMENT (radiation)
'EMIS' : coefficient of emissivity for solid elements
'EINF' : emissivity for the lower layer
'ESUP' : emissivity for the upper layer
'E_IN' : emisivity of the infinite field if needed
'CABS' ; absorbing cvoefficient of the cavity if needed
'TABS' : temperature of the cavity if needed
The shell layers are designated with respect to the element
outside normal : the top layer is directed towards the
outside normal opposite the median plane. If the
elements are not oriented coherently, it is required that
they be reoriented using the ORIENT operator.
- For ADVECTION
In addition RHO and C
'VITE' : speed inside the tube.
---------------------------------------
| Parameter name in DARCY formulation |
---------------------------------------
'K' : isotropic permeability
d) Case of a CONTACT formulation
___________________________________
COULOMB friction model :
------------------------
'MU' : friction coefficient
('COHE'): cohesion coefficient
('ADHE'): adherence coefficient
FROCABLE Friction of tendons
----------------------------
FF : See BPEL99 french code
PHIF : See BPEL99 french code
e) Case of a POREUX formulation
_____________________________
-----------------------------------------------------
| Parameter name for an ELASTIQUE ISOTROPE material |
-----------------------------------------------------
'YOUN' : Young's modulus
'NU ' : Poisson's ratio
'RHO ' : density
'ALPH' : thermal expansion coefficient
'MOB ' : Biot's modulus
'COB ' : Biot's coefficient
'PERM' : intrinsic permeability
'VISC' : fluid dynamic viscosity
'ALPM' : coefficient of the pressure-temperature coupling
Case of porous joints
'KS ' : shear stiffness
'KN ' : normal stiffness
'COB ' : Biot's coefficient
'MOB ' : Biot's modulus
'PERT' : intrinsic tangential permeability
'PERH' : intrinsic normal permeability of the upper face
'PERB' : intrinsic normal permeability of the lower face
'VISC' : fluid dynamic viscosity
g) Case of a MAGNETODYNAMIQUE formulation
_________________________________________
Shells (CORFOU modelisation)
------
'ETA' : resistivity (in ohm.m)
'PERM' : relative permeability
mu = mur.mu0 with mu0 = 4.pi.e-7 henry/m
h) Case of a MELANGE formulation
_____________________________________
CEREM modelling (phase transformation of 16MND5 steel)
---------------
'AC1' : initial temperature of transformation
'AR1' : final temperature of transformation
'MS0' : initial martensitic transformation temperature
'BETA':
'AC' :
'AA' :
'ZS' :
'TPLM':
'CARB':
'ACAR': transformation temperature when cooling
'DG0' : grain size
'AGRA':
'TIHT': initial temperature before cooling
'TFHT': final temperature
'DTHT': temperature step
'NHTR': final phases proportions de phases for several
cooling processes (NUAGE type)
'NLEB': data for Leblond modelling when heating (NUAGE type)
'ZA' : austenite proportion
'ZF' : ferrite proportion
'ZB' : bainite proportion
'ZM' : martensite proportion
'MS' ; martensitic transformation temperature
PARALLELE modelling
-------------------
The phase parameters are named after the four first letters of
the phases names enclosed in the modelling.
ZTMAX modelling (transition between 2 phases )
---------------
'PHA1', 'PHA2' : proportions phase 1 / phase 2
'VIPH' : maximum value of the variable
'VDEH' : minimum value of the variable
'AC1', 'AC2': beginning and end of the transition 1->2
when the variable increases
'AC3', 'AC4': beginning and end of the transition 2->1
when the variable decreases
'VPAR' : name of the variable (default : 'T')
i) Case of a FISSURE formulation
________________________________
Notations : f : friction coefficient
e : crack opening at the inlet
RE : Reynolds number
REC : critical Reynolds number
-------------------------------------------------------
| Parameters for the POISEU_BLASIUS friction law |
-------------------------------------------------------
It is the default law forthe FISSURE formulation.
Laminar regim : f=96/RE
Smooth turbulent regim : f=0.316*RE^(-0.25) (Blasius)
The critical Reynolds number REC is 2042 (intersection between the
2 fonctions)
'RUGO': rugosity (m)
RUGO/2e must be less than 1e-4
--------------------------------------------------------
| Parameters for the POISEU_COLEBROOK friction law |
--------------------------------------------------------
f = max(96/RE;Colebrook)
Colebrook implicit formula :
1/sqrt(f) = -2 log(RUGO/2e/3.7+2.51/RE/sqrt(f)) (log of the base 10)
The critical Reynolds number varies with rugosity
'RUGO': rugosity (m)
RUGO/2e must be greater than or equal to 1e-4
-------------------------------------------------------
| Parameters for the FROTTEMENT1 friction law |
-------------------------------------------------------
Laminar regim : f=k/RE
Turbulent regim : f=(a+bRE^c)^d
'REC': critical Reynolds number given by the user
'FK': k
'FA': a
'FB': b
'FC': c
'FD': d
-------------------------------------------------------
| Parameters for the FROTTEMENT2 friction law |
-------------------------------------------------------
Laminar regim : f=k/RE
Turbulent regim : f=a(b+clogRE)^d
'REC': critical Reynolds number given by the user
'FK': k
'FA': a
'FB': b
'FC': c
'FD': d
-------------------------------------------------------
| Parameters for the FROTTEMENT3 friction law |
-------------------------------------------------------
FROT3 : k*Colebrook over the whole range of Reynolds
'RUGO': rugosity (m)
RUGO/2e must be greater than or equal to 1e-4
'FK': k
-------------------------------------------------------
| Parameters for the FROTTEMENT4 friction law |
-------------------------------------------------------
FROT4 : k*(max(96/RE;Colebrook))
'RUGO': rugosity (m)
RUGO/2e must be greater than or equal to 1e-4
'FK': k
j) Case of a LIAISON (linkage) formulation
--------------------------------------------------
Please see also DYNE notice
'SORT' : optional component (type TABLE)
The object MMODEL type of the LIAISON indices the TABLE
-------------------------------------------------------
| Parameters for the POINT_PLAN FLUIDE law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'INER' : 'COEFFICIENT_INERTIE' (inertia parameter)
'CONV' : 'COEFFICIENT_CONVECTION' (convection parameter)
'VISC' : 'COEFFICIENT_VISCOSITE' (viscosity parameter)
'PELO' : 'COEFFICIENT_P_D_C_ELOIGNEMENT'
( remoteness pressure loss coefficient)
'FRAP' : 'COEFFICIENT_P_D_C_RAPPROCHEMENT'
(proximity pressure loss coefficient)
'JFLU' : 'JEU_FLUIDE' (fluid gap)
-------------------------------------------------------
| Parameters for the POINT_PLAN FROTTEMENT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'JEU' : (gap)
'GLIS' : 'COEFFICIENT_GLISSEMENT' (sliding parameter)
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE' (tangential parameter)
'ATAN' : 'AMORTISSEMENT_TANGENTIEL' (tangential damping)
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
'LOIC' : 'LOI_DE_COMPORTEMENT' (displacement vs force curve)
(type EVOLUTION)
-------------------------------------------------------
| Parameters for the POINT_PLAN law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'JEU' : (gap)
composantes optionnelles
'LOIC' : 'LOI_DE_COMPORTEMENT' (displacement vs force curve)
(type EVOLUTION)
'PERM' : 'LIAISON_PERMANENTE'(integers 0 or 1, ENTIER type)
'SPLA' : 'SEUIL_PLASTIQUE' (yield limit )
'AMOR' : 'AMORTISSEMENT' (damping)
-------------------------------------------------------
| Parameters for the POINT_POINT FROTTEMENT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'JEU' : (gap)
'POIB' : 'POINT_B'
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE'
'ATAN' : 'AMORTISSEMENT_TANGENTIEL'
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
'LOIC' : 'LOI_DE_COMPORTEMENT' (displacement vs force curve)
(type EVOLUTION)
'MODE' :
-------------------------------------------------------
| Parameters for the POINT_POINT DEPLACEMENT_PLASTIQUE law|
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'ECRO' : 'ECROUISSAGE' (hardening)
'JEU' :
'POIB' : 'POINT_B'
'PERM' : 'LIAISON_PERMANENTE' (integers 0 or 1, ENTIER type)
'LOIC' : 'LOI_DE_COMPORTEMENT' (displacement vs force curve)
(type EVOLUTION)
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
-------------------------------------------------------
| Parameters for the POINT_POINT ROTATION_PLASTIQUE law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'ECRO' : 'ECROUISSAGE' (hardening integers 0 : isotropic,
or 1 : kinematic , ENTIER type)
'JEU' : (gap)
'POIB' : 'POINT_B'
'PERM' : 'LIAISON_PERMANENTE' (integers 0 or 1, ENTIER type)
'LOIC' : 'LOI_DE_COMPORTEMENT' (displacement vs force curve)
(type EVOLUTION)
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
'ELAS' : (integers 0 or 1, ENTIER type)
-------------------------------------------------------
| Parameters for the POINT_POINT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'JEU' : (gap)
'POIB' : 'POINT_B'
'PERM' : 'LIAISON_PERMANENTE' (integers 0 or 1, ENTIER type)
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
'LOIC' : 'LOI_DE_COMPORTEMENT' (displacement vs force curve)
(type EVOLUTION)
-------------------------------------------------------
| Parameters for the POINT_CERCLE MOBILE law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'PCER' : 'CERCLE' (circle center)
'RAYO' : 'RAYON' (circle radius)
'GLIS' : 'COEFFICIENT_GLISSEMENT' (sliding parameter)
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE' (tangential stifness)
'ATAN' : 'AMORTISSEMENT_TANGENTIEL' (tangential damping)
composantes optionnelles
'CINT' : 'CONTACT_INTERIEUR'
'AMOR' : 'AMORTISSEMENT' (damping)
-------------------------------------------------------
| Parameters for the POINT_CERCLE FROTTEMENT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'EXCE' : 'EXCENTRATION' (offset vector from the structure
to the center of the circle)
'RAYO' : 'RAYON' (circle radius)
'GLIS' : 'COEFFICIENT_GLISSEMENT' (sliding parameter)
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE' (tangential stifness)
'ATAN' : 'AMORTISSEMENT_TANGENTIEL' (tangential damping)
composantes optionnelles
'CINT' : 'CONTACT_INTERIEUR'
'AMOR' : 'AMORTISSEMENT' (damping)
-------------------------------------------------------
| Parameters for the loi POINT_CERCLE law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'EXCE' : 'EXCENTRATION' (offset vector from the structure
to the center of the circle)
'RAYO' : 'RAYON' (circle radius)
composante optionnelle
'AMOR' : 'AMORTISSEMENT' (damping)
-------------------------------------------------------
| Parameters for the CERCLE_PLAN FROTTEMENT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'JEU' : (gap)
'RAYS' : 'RAYON_SUPPORT' (circle radius)
'GLIS' : 'COEFFICIENT_GLISSEMENT' (sliding parameter)
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE' (tangential stifness)
'ATAN' : 'AMORTISSEMENT_TANGENTIEL' (tangential damping)
composante optionnelle
'AMOR' : 'AMORTISSEMENT' (damping)
-------------------------------------------------------
| Parameters for the CERCLE_CERCLE FROTTEMENT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'EXCE' : 'EXCENTRATION' (offset vector from the structure
to the center of the circle)
'RAYS' : 'RAYON_SUPPORT' (main structure circle radius)
'GLIS' : 'COEFFICIENT_GLISSEMENT' (sliding parameter)
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE' (tangential stifness)
'ATAN' : 'AMORTISSEMENT_TANGENTIEL' (tangential damping)
'RAYB' : 'RAYON_BUTEE'
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
'CINT' : 'CONTACT_INTERIEUR'
-------------------------------------------------------
| Parameters for the PROFIL_PROFIL INTERNE law |
| PROFIL_PROFIL EXTERNE |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'RAID' : 'RAIDEUR' (stiffness)
'PFIX' : 'PROFIL_FIXE' (target structure geometry) (type MAILLAGE)
'PMOB' : 'PROFIL_MOBILE' (main structure geometry) (type MAILLAGE)
'ERAI' : 'EXPOSANT_RAIDEUR' (stiffness exponent)
-------------------------------------------------------
| Parameters for the LIGNE_LIGNE FROTTEMENT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'LIMA' : 'LIGNE_MAITRE' (main structure geometry) (type MAILLAGE)
'LIES' : 'LIGNE_ESCLAVE' (target structure geometry) (type MAILLAGE)
'RAID' : 'RAIDEURS' (stifness)
'GLIS' : 'COEFFICIENT_GLISSEMENT' (sliding parameter)
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE' (tangential stifness)
'ATAN' : 'AMORTISSEMENT_TANGENTIEL' (tangential damping)
'JEU' : (gap)
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
'RECH' : 'RECHERCHE' (integers 0 : local or
1 : global, ENTIER type)
'SYME' : 'SYMETRIE' (integers 0 or 1, ENTIER type)
-------------------------------------------------------
| Parameters for the LIGNE_CERCLE FROTTEMENT law |
-------------------------------------------------------
'NORM' : 'NORMALE' (normal vector) (type POINT)
'LIMA' : 'LIGNE_MAITRE' (main structure geometry) (type MAILLAGE)
'LIES' : 'LIGNE_ESCLAVE' (target structure geometry) (type MAILLAGE)
'RAID' : 'RAIDEURS' (stifness)
'GLIS' : 'COEFFICIENT_GLISSEMENT' (sliding parameter)
'ADHE' : 'COEFFICIENT_ADHERENCE' (adherence parameter)
'RTAN' : 'RAIDEUR_TANGENTIELLE' (tangential stifness)
'ATAN' : 'AMORTISSEMENT_TANGENTIEL' (tangential damping)
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
'RECH' : 'RECHERCHE' (integers 0 : local or
1 : global, ENTIER type)
'RAYO' : 'RAYON' (circle radius)
'ACTN' : 'ACTNOR' (integers 0 or 1, ENTIER type)
'INVE' : 'INVERSION' (integers 0 or 1, ENTIER type)
-------------------------------------------------------
| Parameters for the PALIER_FLUIDE RHODE_LI law |
-------------------------------------------------------
'LONG' : 'LONGUEUR_PALIER' (bearing length)
'RAYO' : 'RAYON_ARBRE' (shaft radius)
'VISC' : 'VISCOSITE_FLUIDE' (fluid viscosity)
'RHOF' : 'RHO_FLUIDE' (fluid density)
'PADM' : 'PRESSION_ADMISSION' (admission pressure)
'VROT' : 'VITESSE_ARBRE' (shaft whirl speed)
'EPSI' : 'CRITERE_ARRET' (convergence criteria)
'PHII' :
'AFFI' :
'TLOB' : 'GEOMETRIE_PALIER' (table of lobe geometry)
composantes optionnelles
'AMOR' : 'AMORTISSEMENT' (damping)
-------------------------------------------------------
| Parameters for the COUPLAGE DEPLACEMENT law |
-------------------------------------------------------
'ORIG' : 'ORIGINE'(point associated to the mode inducing the force)
'COEF : 'COEFFICIENT'
-------------------------------------------------------
| Parameters for the COUPLAGE VITESSE law |
-------------------------------------------------------
'ORIG' : 'ORIGINE'(point associated to the mode inducing the force)
'COEF : 'COEFFICIENT'
-------------------------------------------------------
| Parameters for the POLYNOMIALE law |
-------------------------------------------------------
'COEF' : 'COEFFICIENT'
'PCO1' ... 'PCO9' : points associated to the modes
inducing the force) (maximum 9)
'TCO1' ... 'TCO9' : tables contributions (maximum 9)
Law not available with DYNE
-------------------------------------------------------
| Parameters for the NEWMARK MODAL law |
-------------------------------------------------------
'JEU' :
'EXCE' :
if jeu < 0 u - exce > jeu
if jeu > 0 u - exce < jeu
'FROT' : friction coefficient
'MOFR' : model (MMODEL type) on which is cast the friction
k) Case of a DIFFUSION formulation
__________________________________
-------------------------------------------------------
| Parameters for the FICK law |
-------------------------------------------------------
'KD' : diffusion coefficient
'CDIF' : term analogous to (rho*Cp) in thermal problems
--------------------------------------------------------------
| 2nd syntax : ORTHOTROPES, ANISOTROPES ,UNIDIRECTIONNELS and
--------------------------------------------------------------
--------------------
SECTION materials |
--------------------
| 'DIRECTION' P1 (P2) | | ('PARALLELE') |
MAT1 = MATE MODL1 | | | 'PERPENDICULAIRE' | ...
| 'RADIAL' P1 (P2) | | 'INCLINE' FLOT1 (P3) |
... NOMCi VALi ... ;
Contents :
_________
MODL1 : model object (MMODEL type)
NOMCi : name of the ith parameter (MOT type)
VALi : values(s) of the ith parameter (ENTIER, FLOTTANT,
MCHAML, EVOLUTION or LISTMOTS types)
Note : the LISTMOTS type is provided for components
which have to be evaluated by the external users's
subroutine COMPUT, called by the VARI operator.
In this case, the LISTMOTS object gives the list of
the parameters upon the component depends.
MAT1 : object containing the material properties (MCHAML type,
CARACTERISTIQUES subtype)
The orthotropic and anisotropic properties are provided by bases
which depend on shell and solid elements such as the following :
------------------------------------------
| Bases of orthotropy for shell elements |
------------------------------------------
The bases of orthotropy are defined by the datum relative to the
first direction of orthotropy. First of all, a vector VEC1 is
defined :
'DIRECTION' : the P1 direction is projected (POINT type) onto a
plane tangent to the shell; the result is a VEC1
vector.
'RADIAL' : corresponds to "DIRECTION (PT - P1)", PT being a
current point of the shell (direction that can vary
according to the point of the element).
then, the first direction of orthotropy is specified :
'PARALLELE' : VEC1 is therefore the first direction of
orthotropy
'PERPENDICULAIRE': the first direction of orthotropy is therefore
perpendicular to VEC1
'INCLINE' : the first direction of orthotropy makes a FLOT1
angle (FLOTTANT type) with respect to the
direction VEC.
P3 (POINT type) provides the direction of the
normal which is outside the shell. This vector
is compulsory in 3D.
For instance, for a cylindrical shell, we shall write
'DIRECTION' P1, P1 being directed according to the cylinder axis,
then 'PARALLELE' if the first direction of orthotropy is parallel
to the axis 'PERPENDICULAIRE' if it is perpendicular to the axis,
or 'INCLINE' FLOT1 if it coils up along the cylinder.
Note 1 :
----------
The P2 direction is not used for shell elements.
Note 2 :
----------
For the orthotropic elastic 3D joint elements, the bases of
orthotropy are the same as those of the shell elements. Only
the 'RADIAL' option is forbidden.
------------------------------------------
| Bases of anisotropy for solid elements |
------------------------------------------
First of all, a trihedron is constructed from the two vectors VEC1
and VEC2 provided by the user. The first axis corresponds to VEC1.
The third axis is perpendicular to the vectors VEC1 and VEC2.
The second axis completes the trihedron. The vectors VEC1 and VEC2
are given by:
'DIRECTION' : the direction P1 (point type) corresponds to VEC1
and the direction P2 (point type) corresponds to
VEC2.
'RADIAL' : in 2D, VEC1 connects the current point to P1;
in 3D, VEC1 follows the axis P1 P2 and VEC2
follows the perpendicular to VEC1 that started
at the current point
The anisotropic basis corresponds to the trihedron defined above,
it may rotate about the axis 3 :
'PARALLELE' : VEC1 is therefore the first direction of
orthotropy (no rotation about the axis 3)
'PERPENDICULAIRE': the first direction of orthotropy is therefore
perpendicular to VEC1 (rotation of +90 about
the axis 3)
'INCLINE' : the first direction of orthotropy makes a FLOT1
angle (FLOTTANT type) with the VEC1 direction
(rotation of any angle about the axis 3)
Note 2 :
-----------
Defining a single vector (VEC1) in a two-dimensional case is
sufficient. The second axis corresponds to a vector which makes
an angle of + 90 degrees with the VEC1 vector.
Note 3 :
-----------
The 'RADIAL' instruction, as well as the direction P3 are not
used for solid elements.
-----------------------------------------
| Direction of unidirectional materials |
-----------------------------------------
The above syntax for the bases of orthotropy (or anisotropy)
for shell and solid elements also applies to
unidirectional materials. In this case, the first axis of
orthotropy corresponds to the direction of the unidirectional
materials.
Every case
___________
------------------------------------
| Parameter name for any material |
------------------------------------
a) Case of a MECANIQUE formulation
__________________________________
-------------------------------------------------------
| Parameter name for an ELASTIQUE ORTHOTROPE material |
-------------------------------------------------------
Thin shells (COQ2, COQ3, DKT)
-------------------------------
'YG1 ', 'YG2 ' : Young's moduli
'NU12' : Poisson's ratio
'G12 ' : shear modulus
'ALP1', 'ALP2' : thermal expansion coefficients
'RHO ' : density
Shells with tranverse shear (DST, COQ4, COQ6, COQ8)
----------------------------------------------
'YG1 ', 'YG2 ' : Young's moduli
'NU12' : Poisson's ratio
'G12 ' 'G23 ', 'G13 ' : shear moduli
'ALP1', 'ALP2' : thermal expansion coefficients
'RHO ' : density
3D joints elements (JOI4)
-------------------------
'KS1 ', 'KS2 ' : shear stiffnesses according to the
directions 1 and 2 of the joint plane
( N/m3 )
'KN ' : normal stiffness from the joint plane
( N/m3 )
'RHO ' : joint density ( kg/m2 )
'ALPN' : thermal expansion coefficient
according to the joint normal ( m/K )
Uniaxial joint elements in 3D (JOI1)
------------------------------------
Units are indicated for information in international system.
'KS1 ', 'KS2 ' : shear stiffnesses in the two
directions of the normal plane
to the joint axis ( N/m )
'KN ' : normal stiffness ( N/m )
'QS1 ', 'QS2 ' : flexural rotational stiffness in the
two directions of the normal plane
to the joint axis ( N.m )
'QN ' : torsional stiffness ( N.m )
'ALPN' : thermal expansion coefficient in the normal
direction to the joint ( m/K )
'ALP1' : thermal expansion coefficient in the first
transverse direction to the joint ( m/K )
'ALP2' : thermal expansion coefficient in the second
transverse direction to the joint ( m/K )
'ALQN' : thermal expansion coefficient in rotation
along the normal direction to the joint ( 1/K )
'ALQ1' : thermal expansion coefficient in rotation along
the first transverse direction to the joint ( 1/K )
'ALQ2' : thermal expansion coefficient in rotation along
the second transverse direction to the joint ( 1/K )
'MASS' : mass of the whole block represented by the joint
element ( kg )
'JX ' : moment of inertia around the axis X ( kg/m² )
'JY ' : moment of inertia around the axis Y ( kg/m² )
'JZ ' : moment of inertia around the axis Z ( kg/m² )
Uniaxial joint elements in 2D (JOI1)
------------------------------------
Units are indicated for information in international system.
'KS ' : shear stiffness ( N/m )
'KN ' : normal stiffness ( N/m )
'QS ' : flexural rotational stiffness ( N.m )
'ALPN' : thermal expansion coefficient in the normal
direction to the joint ( m/K )
'ALPS' : thermal expansion coefficient in the
transverse direction to the joint ( m/K )
'ALQS' : thermal expansion coefficient in rotation
( 1/K )
'MASS' : mass of the whole block represented by the joint
element ( kg )
'JZ ' : moment of inertia around the axis Z ( kg/m² )
Three-dimensional solid elements
----------------------------------
'YG1 ', 'YG2 ', 'YG3 ' : Young's moduli
'NU12', 'NU23', 'NU13' : Poisson's ratio
'G12 ', 'G23 ', 'G13 ' : shear moduli
'ALP1', 'ALP2', 'ALP3' : thermal expansion coefficient
'RHO ' : density
Two-dimensional solid elements
--------------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
------------------------------------------------------------------
| plane stress | axisymmetrical | Fourier's series |
| | plane strain | |
|--------------------|--------------------|----------------------|
|'YG1','YG2' |'YG1', 'YG2', 'YG3' | 'YG1', 'YG2', 'YG3' |
|'NU12','G12 ' |'NU12','NU23','NU13'| 'NU12','NU23','NU13' |
|'YG3', 'NU23','NU13'|'G12 ' | 'G12 ','G23 ','G13 ' |
|'ALP1','ALP2' |'ALP1','ALP2','ALP3'| 'ALP1','ALP2','ALP3' |
|'RHO' |'RHO ' | 'RHO' |
------------------------------------------------------------------
Remarks
-------
- In case of NON_LINEAIRE UTILISATEUR model affected to three or
two-dimensional solid elements, the elastic orthotropic properties
must be given in the same order as defined above, the definition of
the orthotropic bases (key words 'DIRECTION'...or 'RADIAL'...)
occuring just after the definition of the shear moduli.
As a consequence, in case of thermal expansion, the definition of
the orthotropic bases appears then just before the definition of
the thermal expansion coefficients.
- In case of NON_LINEAIRE UTILISATEUR model affected to 1D finite
elements, Young's moduli and Poisson's ratios must be given in the
same order as defined for the three-dimensional solid elements.
-------------------------------------------------------
| Parameter name for an ELASTIQUE ANISOTROPE material |
-------------------------------------------------------
Three-dimensional solid elements
-----------------------------------
The parameter names for a three-dimensional case correspond to
the 21 terms which are independent of Hooke's matrix for an
anisotropic material :
| sig1 | |D11 sym. | | eps1 |
| sig2 | |D21 D22 | | eps2 |
| sig3 | = |D31 D32 D33 | x | eps3 |
| tau12| |D41 D42 D43 D44 | | gama12|
| tau13| |D51 D52 D53 D54 D55 | | gama13|
| tau23| |D61 D62 D63 D64 D65 D66 | | gama23|
When necessary, these parameters are required to be added :
'ALP1','ALP2','ALP3' : thermal expansion coefficients
'AL12','AL23','AL13'
'RHO' : density
Two-dimensional solid elements
--------------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
------------------------------------------------------------------
| plane stress | axisymmetrical | Fourier's series |
| | plane strain | |
------------------------------------------------------------------
|'D11','D21','D22' |'D11','D21','D22' | 'D11','D21','D22' |
|'D31','D32','D33' |'D31','D32','D33' | 'D31','D32','D33' |
|'D41','D42','D43' |'D41','D42','D43' | 'D41','D42','D43' |
|'D44' |'D44' | 'D44','D55','D65' |
| | | 'D66' |
|'ALP1','ALP2' |'ALP1','ALP2','ALP3'| 'ALP1','ALP2','ALP3' |
|'AL12','RHO ' |'AL12','RHO ' | 'AL12','RHO ' |
------------------------------------------------------------------
Note : In the case of the plane stress, the coefficients D11,
D21, ... must be the same as the coefficients in the
case of the plane strain. The modifications because of
the hypothesis of plane stress are made by the operator.
For the 2D or 3D joint elements, the anisotropic option is not
defined.
Uniaxial joint elements in 3D (JOI1)
------------------------------------
Units are indicated for information in international system.
The parameter names for a three-dimensional case correspond to
the 21 terms which are independent of Hooke's matrix for an
anisotropic material :
| EFFX | |D11 sym. | | EXX |
| EFFY | |D21 D22 | | GXY |
| EFFZ | = |D31 D32 D33 | x | GXZ |
| MOMX | |D41 D42 D43 D44 | | CXX |
| MOMY | |D51 D52 D53 D54 D55 | | CXY |
| MOMZ | |D61 D62 D63 D64 D65 D66 | | CXZ |
When necessary, these parameters are required to be added :
'ALP1','ALP2','ALP3' : thermal expansion coefficients
'ALQ1','ALQ2','ALQ3' in translation and in rotation
'MASS ' : mass of the whole block represented by the joint
element ( kg )
'JX ' : moment of inertia around the axis X ( kg/m² )
'JY ' : moment of inertia around the axis Y ( kg/m² )
'JZ ' : moment of inertia around the axis Z ( kg/m² )
Uniaxial joint elements in 2D (JOI1)
------------------------------------
Units are indicated for information in international system.
The parameter names for a two-dimensional case correspond to
the 6 terms which are independent of Hooke's matrix for an
orthotropic material :
| EFFX | | D11 sym.| | EXX |
| EFFY | = | D21 D22 | x | GXY |
| MOMZ | | D31 D32 D33 | | CXZ |
When necessary, these parameters are required to be added :
'ALP1','ALP2','ALQ3' : thermal expansion coefficients
'MASS ' : mass of the whole block represented by the joint
element ( kg )
'JZ ' : moment of inertia around the axis Z ( kg/m² )
------------------------------------------------------------
| Parameter name for an ELASTIQUE UNIDIRECTIONNEL material |
------------------------------------------------------------
'YOUN' : Young's modulus
'RHO ' : density
'ALPH' : thermal expansion coefficient
----------------------------------------------------
| Parameter name for an ELASTIQUE SECTION material |
----------------------------------------------------
'MODS' : object of type MMODEL defining the section model
'MATS' : object of type MCHAML associated with the section model,
defining the material and geometrical characteristics
of the section
('MAHO') : Hooke's matrix of the equivalent beam (type LISTREEL)
b) Case of a THERMIQUE formulation
___________________________________
----------------------------------------------------------
| Parameter name for a THERMIQUE ORTHOTROPE formulation |
----------------------------------------------------------
Shells (COQ2, COQ3, COQ4, COQ6, COQ8)
--------------------------------------
'K1','K2','K3' : thermal conductivities
'RHO' : density
'C ' : specific heat
'H ' : exchange coefficient
Three-dimensional solid elements
----------------------------------
'K1','K2','K3' : thermal conductivities
'RHO' : density
'C ' : specific heat
'H ' : exchange coefficient
Two-dimensional solid elements
--------------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
-------------------------------------------
|two-dimensional and | Fourier's series |
| axisymmetrical | |
-------------------------------------------
| 'K1','K2' | 'K1','K2','K3' |
| 'RHO','H','C' | 'RHO','H','C' |
-------------------------------------------
---------------------------------------------------------
| Parameter name for a THERMIQUE ANISOTROPE formulation |
---------------------------------------------------------
Three-dimensional solid elements
----------------------------------
'K11','K21','K22' : terms independent of the
'K31','K32','K33' anisotropic conductivities matrix
'RHO' : density
'H' : exchange coefficient
'C' : specific heat
Two-dimensional solid elements
---------------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
-------------------------------------------
|two-dimensional and | Fourier's series |
| axisymmetrical | |
-------------------------------------------
|'K11','K21','K22' | 'K11','K21','K22' |
| | 'K33' |
| 'RHO','H','C' | 'RHO','H','C' |
-------------------------------------------
Note :
________
The geometrical properties must be input simultaneously with the
material properties, when carrying out a thermal analysis of
shells or a mechanical analysis of thick orthotropic shells.
c) Case of a DARCY formulation
_______________________________
------------------------------------------------------
| Parameter name for a DARCY ORTHOTROPE formulation |
------------------------------------------------------
Three-dimensional hybrid elements
---------------------------------
'K1','K2','K3' : hydraulic permeabilities
Two-dimensional solid elements
--------------------------------
'K1','K2' : hydraulic permeabilities
-----------------------------------------------------
| Parameter name for a DARCY ANISOTROPE formulation |
-----------------------------------------------------
Three-dimensional hybrid elements
---------------------------------
'K11','K21','K22' : terms independent of the
'K31','K32','K33' anisotropic permeabilities matrix
Two-dimensional hybrid elements
-------------------------------
'K11','K21','K22' : terms independent of the
anisotropic permeabilities matrix
d) Case of a POREUX formulation
_______________________________
-------------------------------------------------------
| Parameter name for an ELASTIQUE ORTHOTROPE material |
-------------------------------------------------------
Three-dimensional solids
---------------------------
'YG1 ', 'YG2 ', 'YG3 ' : Young's moduli
'NU12', 'NU23', 'NU13' : Poisson's ratios
'G12 ', 'G23 ', 'G13 ' : shear moduli
'ALP1', 'ALP2', 'ALP3' : thermal expansion coefficients
'RHO ' : density
'COB1', 'COB2', 'COB3' : Biot's coefficients
'MOB ' : Biot's moduli
'PER1', 'PER2', 'PER3' : intrinsic permeabilities
'VISC' : fluid dynamic viscosity
'ALPM' : coefficient of the pressure-temperature
coupling
Two-dimensional solids
------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
------------------------------------------------------------------
| plane stress |axisymmetrical plane| Fourier's series |
| | strain | |
|--------------------|--------------------|----------------------|
|'YG1', 'YG2', 'YG3' |'YG1', 'YG2', 'YG3' | 'YG1', 'YG2', 'YG3' |
|'NU12','NU23','NU13'|'NU12','NU23','NU13'| 'NU12','NU23','NU13' |
|'G12 ' |'G12 ' | 'G12 ','G23 ','G13 ' |
|'ALP1','ALP2' |'ALP1','ALP2','ALP3'| 'ALP1','ALP2','ALP3' |
|'RHO' |'RHO ' | 'RHO' |
|'COB1','COB2','COB3'|'COB1','COB2','COB3'| 'COB1','COB2','COB3' |
|'MOB ' |'MOB ' | 'MOB ' |
|'PER1','PER2' |'PER1','PER2' | 'PER1','PER2','PER3' |
|'VISC' |'VISC' | 'VISC' |
|'ALPM' |'ALPM' | 'ALPM' |
------------------------------------------------------------------
---------------------------------------------------------
| Parameter name for an ELASTIQUE ANISOTROPE material |
---------------------------------------------------------
Three-dimensional solids
---------------------------
The parameter names for a three-dimensional case correspond to
the 21 terms which are independent of Hooke's matrix for an
anisotropic material and to the 6 terms which are independent of
Biot's matrix :
| sig1 | |D11 sym. | | eps1 | |COB1 |
| sig2 | |D21 D22 | | eps2 | |COB2 |
| sig3 | = |D31 D32 D33 | x | eps3 | - |COB3 | x p
| tau12| |D41 D42 D43 D44 | | gama12| |CO12 |
| tau13| |D51 D52 D53 D54 D55 | | gama13| |CO13 |
| tau23| |D61 D62 D63 D64 D65 D66 | | gama23| |CO23 |
and to Biot's modulus : 'MOB '
When necessary, these parameters are required to be added :
'ALP1','ALP2','ALP3' : thermal expansion coefficients
'AL12','AL23','AL13'
'RHO' : density
'PER1','PER2','PER3' | : matrix of intrisic permeabilities
'PE12','PE13','PE23' |
'VISC' : fluid visvosity
'ALPM' : coefficient of the pressure-temperature
coupling
Two-dimensional solids
-------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
-----------------------------------------------------------------
| plane stress |axisymmetrical plane| Fourier's series |
| | strain | |
|--------------------|--------------------|----------------------|
|'D11','D21','D22' |'D11','D21','D22' | 'D11','D21','D22' |
|'D31','D32','D33' |'D31','D32','D33' | 'D31','D32','D33' |
|'D41','D42','D43' |'D41','D42','D43' | 'D41','D42','D43' |
|'D44' |'D44' | 'D44','D55','D65' |
| | | 'D66' |
|'ALP1','ALP2' |'ALP1','ALP2','ALP3'| 'ALP1','ALP2','ALP3' |
|'AL12','RHO ' |'AL12','RHO ' | 'AL12','RHO ' |
|'COB1','COB2','COB3'|'COB1','COB2','COB3'| 'COB1','COB2','COB3' |
|'CO12','MOB ' |'CO12','MOB ' | 'CO12','MOB ' |
|'PER1','PER2','PE12'|'PER1','PER2','PE12'| 'PER1','PER2','PER3' |
|'VISC' |'VISC' | 'PE12','VISC' |
|'ALPM' |'ALPM' | 'ALPM' |
------------------------------------------------------------------
-------------------------------------------------------------
| Parameter name for an ELASTIQUE UNIDIRECTIONNEL material |
-------------------------------------------------------------
'YOUN' : Young's modulus
'RHO ' : density
'ALPH' : thermal expansion coefficient
'MOB ' : Biot's modulus
'COB ' : Biot's coefficient
'PERM' : intrisic permeability
'VISC' : fluid dynamic viscosity
'ALPM' : coefficient of the pressure-temperature
coupling
e) Case of a MAGNETODYNAMIQUE formulation
_________________________________________
Shells (CORFOU modelisation)
------
'ETA1' : resistivity along the first direction of orthotropy
(in ohm.m)
'ETA2' : resistivity along the second direction of orthotropy
(in ohm.m)
'PERM' : relative permeability
mu = mur.mu0 with mu0 = 4.pi.e-7 henry/m
f) Case of a DIFFUSION formulation
___________________________________
----------------------------------------------------------
| Parameter name for a DIFFUSION ORTHOTROPE formulation |
----------------------------------------------------------
Three-dimensional solid elements
----------------------------------
'KD1','KD2','KD3' : diffusion coefficients
'RHO' : mass density
'CDIF' : term analogous to (rho*Cp)
in thermal problems
Two-dimensional solid elements
--------------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
-------------------------------------------
|two-dimensional and | Fourier's series |
| axisymmetrical | |
-------------------------------------------
| 'KD1','KD2' | 'KD1','KD2','KD3' |
| 'CDIF','RHO' | 'CDIF','RHO' |
-------------------------------------------
---------------------------------------------------------
| Parameter name for a DIFFUSION ANISOTROPE formulation |
---------------------------------------------------------
Three-dimensional solid elements
----------------------------------
'KD11','KD21','KD22' : independent terms of the
'KD31','KD32','KD33' : anisotropic diffusion matrix
'RHO' : mass density
'CDIF' : term analogous to (rho*Cp)
in thermal problems
Two-dimensional solid elements
---------------------------------
The parameter names for the different two-dimensional cases are
summed up in the following table :
-------------------------------------------
| two-dimensional and | Fourier's series |
| axisymmetrical | |
-------------------------------------------
| 'KD11','KD21','DK22' | 'KD11','KD21', |
| | 'KD22','KD33' |
| 'CDIF','RHO' | 'CDIF','RHO' |
-------------------------------------------
-----------------------------------------------------------------
*****************************
* *
* GEOMETRICAL PROPRIETES *
* *
*****************************
-----------------------------------------------------------------
-----------------------------------------
| Feature name for the solid elements |
-----------------------------------------
('DIM3') : thickness in the case of plane stresses
-------------------------------------------------------
| Feature names for the COQ2, COQ3, COQ4, DKT, DST elements |
-------------------------------------------------------
'EPAI' : shell thickness
('ALFA') : coefficient used for the plasticity criterion
(2/3 by default)
('EXCE') : offset of the mid-plane with respect to the reference
plane regarded as positive in the direction of the
normal (not available for COQ3)
('DIM3') : thickness in the other direction (case of COQ2, plane
stresses)
--------------------------------------------
| Feature name for the COQ6, COQ8 elements |
--------------------------------------------
'EPAI' : shell thickness
('EXCE') : offset with respect to the mid-plane regarded as
positive in the direction of the normal
--------------------------------------
| Feature name for the ROT3 elements |
--------------------------------------
'EPAI' : shell thickness (with 'MATE')
--------------------------------------------
| Feature name for the COQ6, COQ8 elements |
--------------------------------------------
----------------------------------------------
| Feature names for the QUAS or TRIS elements |
----------------------------------------------
The section is described in the xOy plane. The Ox axis of the section
system is the local axis Oy of the TIMO element.
'ALPY' : coefficient multiplying the shear stress sxy
(Ox et Oy are local axis of the TIMO element).
'ALPZ' : coefficient multiplying the shear stress sxy
(Ox et Oz are local axis of the TIMO element).
In the case of a homogeneous section these coefficients may be
calculated using Timoshenko theory.
-----------------------------------------------
| Feature name for generalized joint elements |
-----------------------------------------------
('EPAI') : thickness of the joint
------------------------------------
| Feature name for a BARRE element |
------------------------------------
'SECT' : cross section
-----------------------------------
| Feature name for a CERCE element|
-----------------------------------
'SECT' : cross section
------------------------------------------------------------
| Feature name for a POUTRE or TIMO element (BEAM or TIMO) |
------------------------------------------------------------
The beam features are defined in the element local axes (Ox stands
for the beam axis oriented from the first point towards the second,
Oy is defined by the user when necessary, Oz completes the basis).
Axis Oy and Oz must be principal axis because the crossing moments
of inertia are not given (except for the TIMO element in the case of
a SECTION model).
'SECT' : cross section
'INRY' : moment of inertia with respect to the local axis Oy
(3D only)
'INRZ' : moment of inertia with respect to the local axis Oz
'TORS' : twisting moment of inertia
(3D only)
('SECY') : reduced section used to compute shear force
according to the local axis Oy
('SECZ') : reduced section used to compute shear force
according to the local axis Oz (3D only)
('VECT') : key word for defining the local axis Oy. It must be
followed by a vector pertaining to the xOy plane
(POINT type object) (3D only)
('DX ') | : 3 distances for computing stresses from the moments
('DY ') | for the plasticity criterion
('DZ ') | (see VMIS).
'SECT' : cross section
The default value of the SECY and SECZ for the TIMO element
is SECT, and for the POUTRE element we do not considerate the shear
deformation potential energy (this is equivalent with giving infinite
values for the reduced sections.
-----------------------------------
| Feature name for a TUYAU element|
-----------------------------------
This element is used in the modeling of parts of straight pipe or
elbow which differ only in their radius of curvature. The pipe
features are defined in the element local base, in the same way
as the POUTRE element.
'EPAI' : thickness
'RAYO' : pipe external radius
('RACO') : if elbow, radius of curvature
('VECT') : key word for defining the local axis Oy. It must be
followed by a POINT type object modeling an xOy vector.
This is especially required when dealing with an elbow.
Caution : for elbows, the local vector Oz, deduced
--------
from Ox and Oy, is situated in the elbow plane, and
is oriented, according to convention, towards the
elbow extrados.
('PRES') : internal pressure
('CFFX') : coefficient to compute the membrane stress from
the EFFX force, for the plasticity criterion
(1. by default), (see VMIS).
('CFMX') : coefficient to compute the torsion stress from
the MOMX moment, for the plasticity criterion
(3.**0.5 by default), (see VMIS).
('CFMY') : coefficient to compute the flexion stress from
the MOMY moment, for the plasticity criterion
((pi/4)*gamma by default), (see VMIS).
('CFMZ') : coefficient to compute the flexion stress from
the MOMZ moment, for the plasticity criterion
((pi/4)*gamma by default), (see VMIS).
('CFPR') : coefficient to compute the circumferential stress
induced by the pressure. This coefficient is not
used for the plasticity criterion but is used for
the equivalent stress calculation.
(0. by default), (see VMIS).
Remark : for CFMY and CFMZ, gamma is equal to 1. for
-------
straight parts and to maxi ( 1., (8/9)/lambda**2/3 )
for elbows, with lambda = epai*raco/rmoy**2 where
rmoy is the pipe mean radius.
----------------------------------------
| Feature name for a LINESPRING element|
----------------------------------------
'EPAI' : shell thickness
'FISS' : notch depth
'VX ' |
'VY ' | : components of the normal vector with respect to the
shell plane (its direction refers to the side of the
'VZ ' | shell where the notch opens)
Note :
_______
Angles must not be smaller than 175 degrees or greater than
185 degrees between the elements in their plane (defined by
the normal vector).
-------------------------------------------
| Feature name for a TUYAU FISSURE element|
-------------------------------------------
This element enables the modeling of parts of straight pipe or
cracked elbow which differ only in their radius of curvature.
The pipe features are defined in the element local axes in the
same way as for the POUTRE element.
'EPAI' : thickness
'RAYO' : pipe external radius
'ANGL' : crack whole opening in degrees
'VX ' |
'VY ' | : components of the vector defining the cracked pipe axis
'VZ ' |
'VXF ' |
'VYF ' | : components of the vector defining the crack orientation
'VZF ' |
Note :
______
The validity domain for this element is corresponding to a ratio
RAYO/EPAI between 5.5 and 20.5.
--------------------------------------
| Feature name for a RACCORD element |
--------------------------------------
For elements of fluid-structure coupling different from LITU,
it is necessary that the fluid position be known with respect to
the coupling element. For this, the geometrical object
modeling the fluid will be supplied after the key word 'LIQU'.
-----------------------------------
| Feature name for a LSE2 element |
-----------------------------------
'RAYO' : pipe internal radius
('RACO') : if elbow, radius of curvature
------------------------------------
| Feature name for a LITU element |
------------------------------------
'RAYO' : pipe internal radius
('RACO') : if elbow, radius of curvature
('VECT') : key word for defining the local axis Oy. It must be
'VZ ' | followed by a POINT type object modeling a vector
xOy. This is especially required when dealing with an
elbow.
Caution : for elbows, the local vector Oz deduced from
-------
Ox and Oy, is situated in the elbow plane, and is
oriented, according to convention, towards the elbow
extrados.
------------------------------------------
| Feature name for a HOMOGENEISE element |
------------------------------------------
'SCEL' : measurement of an enlarged elementary cell
'SFLU' : measurement of the fluid domain in the enlarged cell
'EPS ' : medium tubular step
'NOF1' : ratio between the norm of the tube modal deformed
shape and the norm of the pressure according to the
axis of the tubes
'NOF2' : ratio between the scalar product of the tube modal
deformed shape and the pressure modal deformed shape
according to the axis of the tubes
Note :
________
Note that when studying a slab, both 'NOF1' and 'NOF2'
coefficients equal one.
---------------------------------------------------
| Feature name for section elements TRIS and QUAS |
---------------------------------------------------
'ALPY' : cross-sectional warping in the local direction Oy
'ALPZ' : cross-sectional warping in the local direction Oz
$$$$