Solver Reference Manual
Solver Reference Manual
LUSAS Version 14.5 : Issue 1
LUSAS
Forge House, 66 High Street, Kingston upon Thames,
Surrey, KT1 1HN, United Kingdom
Tel: +44 (0)20 8541 1999
Fax +44 (0)20 8549 9399
Email: [email protected] http://www.lusas.com
Distributors Worldwide
Copyright ©19822010 LUSAS
All Rights Reserved.
Table of Contents
Table of Contents
LUSAS Data Chapters ............................................................................. 1
Chapter 2 Syntax and Data Preparation .................................................... 7
Reading and Writing LUSAS Data Syntax .............................................. 7
Chapter 3 LUSAS Data Input..................................................................... 13
System Parameters ............................................................................... 13
Geometric Properties ............................................................................ 43
Composite Geometry ............................................................................. 46
Geometric Assignments ........................................................................ 47
Linear Material Properties ..................................................................... 48
Joint Material Properties ....................................................................... 58
Material Properties Mass ....................................................................... 72
Nonlinear Material Properties ............................................................... 73
Field Material Properties ..................................................................... 133
Material Assignments .......................................................................... 139
Composite Assignments ..................................................................... 142
Activate/Deactivate Elements ............................................................. 143
Damping Properties ............................................................................. 152
Freedom Template ............................................................................... 189
Transformed Freedoms ....................................................................... 193
Constraint Equations ........................................................................... 194
Support Conditions ............................................................................. 196
General Point/Patch Loads.................................................................. 223
i
Table of Contents
Retained Freedoms ............................................................................. 239
Load Combinations ............................................................................. 246
Enveloping Results ............................................................................. 247
Modal Damping Control ...................................................................... 308
Harmonic Response Control ............................................................... 313
Appendix A LUSAS User Options .......................................................... 323
LUSAS User Options ........................................................................... 323
LUSAS User Options by Category ...................................................... 329
Appendix B Nonlinear Hardening Material Convention ........................ 335
Nonlinear Hardening Material Convention ......................................... 335
Appendix C Material Model Interface ..................................................... 339
Solver User Interface Routines ........................................................... 339
Programming Rules............................................................................. 341
User Defined Constitutive Models ...................................................... 343
User Defined Resultant Models .......................................................... 354
User Defined Joint Models .................................................................. 363
User Defined Creep Models ................................................................ 371
User Defined Damage Models ............................................................. 375
User Defined Friction Models.............................................................. 378
UserDefined Rate of Internal Heat Generation .................................. 381
ii
Notation
A Cross sectional area
Ap Plastic area
As, Asy, Asz Effective shear area
A1 ... An Nodal cross sectional areas
x
,
y
,
z
,
xy a r
Mass Rayleigh damping constant
Coefficient of thermal expansion
s
Softening parameter
,
xz
,
x
,
y
yz
,
z
Orthotropic thermal expansion coefficients
Angular accelerations (radians/sec
2
)
b
r r
Stiffness Rayleigh damping parameter
Shear retention factor/parameter
Principal stresses direction (radians)
C Specific heat capacity
C i
(i)th hardening stiffness
C0 NeoHookean rubber model constant
C1, C2 MooneyRivlin rubber model constants
c Cohesion
co Initial cohesion
D ij
Rigidity coefficients
du, dq Relative displacement, rotation
E Modulus of elasticity (Young‟s modulus)
Ep Elastoplastic modulus
E x
, E y
, E z
Orthotropic modulus of elasticity
e p
Strain at peak compressive strength
e y
, e z
Eccentricity
x
,
y
,
z
Direct strains (local or global)
s
Maximum shear strain
e
Von Mises equivalent strain
c
Creep strains
p Equivalent plastic strain
F x
, F y
, F z
Forces (local or global)
F yld
Yield force
F Deformation gradient
xy f c f t
’ Compressive strength of concrete
’ Tensile strength of concrete
x
,
y
,
z
Flexural strain resultants
,
xz
,
yz
Torsional strain resultants
G Shear modulus
Gf Fracture energy
G xy
, G xz
, G yz
Orthotropic shear modulus values
x
,
y
,
z
Membrane strain resultants
iii
Notation
Notation
x
,
y
,
z
Field gradients (local or global)
H Enthalpy
H
I1
Isotropic hardening parameter
H
K1
Kinematic hardening parameter
h c
Convective heat transfer coefficient
x
,
y h r
,
z
1
,
2
a
,
b
Radiative heat transfer coefficient
Rotations (local or global)
Loof node rotations (local)
Nodal rotations for thick shells
Angle defining principal directions of l1, l2
I y
, I z
1st moments of inertia
I yy
, I zz
2nd moments of inertia
I yz
Product moment of inertia
J Volume ratio (determinant of F)
K Spring stiffness
K c
Contact stiffness
K l
Liftoff stiffness
K o
Original gap conductance
K t
Torsional constant
k Thermal conductivity
k x
, k y
, k z
Orthotropic thermal conductivity values
k r
Bulk modulus
Hardening stiffness
1
,
L i
Limit of (i)th hardening stiffness
2
,
3
Principal stretches
M Mass
m x
, m y
, m z
Mass in element local directions
M x
, M y
, M z
Concentrated moments (local or global)
M x
, M y
, M z
, M q
Flexural moments (local or global)
M xy
, M xz
, M yz
Torsional moments (local or global)
M
1
ri
, M
Coulomb friction coefficient
,
ri
2
Concentrated loof moments (local or global)
Ogden rubber model constants
N x
, N y
, N z
, N q
Membrane resultants (local or global)
N x
, N y
, N xy
Stress resultants
Nmax, Nmin Principal stress resultants
N s
Maximum shear stress resultant
xy
,
xz
N e
Von Mises equivalent stress resultant
Poisson‟s ratio
,
yz
Orthotropic Poisson‟s ratio
P x
, P y
, P z
Concentrated loads (global)
Mass density
Q Field loading for nodes
q a
Field face loading intensity
q v
Field volume loading intensity
iv
Notation q x
, q y
, q z
Field fluxes (local or global)
q s
Stress potential parameters
Sp Plastic shear area
y
Yield stress
y
,
yo
Initial uniaxial yield stress
z
Direct stresses (local or global)
x
,
max,
min Principal stresses
xy
,
xz
,
yz
Shear stresses (local or global)
s Maximum shear stress
e
Von Mises equivalent stress
T Temperature
T, To Final, initial temperatures
t1 ... tn Nodal thicknesses
U, V, W Displacements (global)
Field variable
e External environmental temperature
Frictional angle
o Initial frictional angle
Body force potential
Vx, Vy, Vz Nodal initial velocities (global)
V1
1
, V1
2
... V3
3
Left stretch tensor components
W x
, W y
, W z
Uniformly distributed load intensities
X, Y, Z Nodal coordinates (global)
Xcbf, Ycbf, Zcbf Constant body forces (global)
Xo, Yo, Zo Offsets of finite element model coordinate system from point about which global angular acceleration and velocities are applied
y
1
, z
1
... y
4
, z
4
Cross sectional coordinates (local)
Zyp, Zzp Torsional plastic modulus values
Zyyp, Zzzp Flexural plastic modulus values
Frequency of vibration
x
,
y
,
z
Angular velocities (global) (radians/sec)
v
Notation
vi
Introduction
Chapter 1
Introduction
Introduction
This manual contains details of the data sections available for input in a LUSAS datafile. The data sections required at any one time will depend upon the type of analysis to be carried out. Some of the sections are of specialised application, others are general to all problems. For example, the ELEMENT TOPOLOGY and NODE
COORDINATES sections are required to define the problem in all analyses, however, the thermal conductivity of a material is only applicable to a heat transfer analysis. The specialised sections are referenced in the Modeller User Manual where a brief description is available of the problem type to which the command applies.
LUSAS Data Chapters
A full list of LUSAS data chapters, in the order in which they must be specified, is shown below.
Data section
SYSTEM
PROBLEM
UNITS
OPTION
GROUP
ELEMENT TOPOLOGY
SOLUTION ORDER
SOLVER FRONTAL
SOLVER CONJUGATE GRADIENT
Description
System parameters
Problem definition
Unit definition
User options
Grouped data
Element topology
Equation solution order
Solve using Frontal method
Solve using iterative Conjugate
Gradient method
NODE COORDINATES Node coordinates
LOCAL CARTESIAN COORDINATES Local Cartesian coordinates
LOCAL CYLINDRICAL
COORDINATES
Local cylindrical coordinates
LOCAL SPHERICAL COORDINATES Local spherical coordinates
1
Chapter 1 Introduction
Data section
GLOBAL CARTESIAN
COORDINATES
SPACING
SPACING ARC RATIOS
QUADRILATERAL SPACING
COPY NODES
RENUMBER NODES
DELETE NODES
GEOMETRIC PROPERTIES
COMPOSITE GEOMETRY
Description
Global Cartesian coordinates
Spacing of nodes on a line
Spacing of nodes on an arc
Spacing of nodes in a quadrilateral
Copying nodes
Renumbering nodes
Deleting nodes
Geometric properties
Laminated/composite shell/solid thicknesses
Geometric property assignments
Isotropic model
Orthotropic plane stress model
GEOMETRIC ASSIGNMENTS
MATERIAL PROPERTIES
MATERIAL PROPERTIES
ORTHOTROPIC
MATERIAL PROPERTIES
ORTHOTROPIC PLANE STRAIN
MATERIAL PROPERTIES
ORTHOTROPIC THICK
MATERIAL PROPERTIES
ORTHOTROPIC AXISYMMETRIC
MATERIAL PROPERTIES
ORTHOTROPIC SOLID
MATERIAL PROPERTIES
ANISOTROPIC
Orthotropic plane strain model
Orthotropic thick model
Orthotropic axisymmetric model
Orthotropic solid model
Anisotropic model
MATERIAL PROPERTIES
ANISOTROPIC SOLID
RIGIDITIES
MATRIX PROPERTIES STIFFNESS
MATRIX PROPERTIES MASS
MATRIX PROPERTIES DAMPING
JOINT PROPERTIES
JOINT PROPERTIES GENERAL
Anisotropic model for solid elements
Linear rigidity model
Stiffness matrix property definition
Mass matrix property definition
Damping matrix property definition
Standard linear joint model
General linear joint model
JOINT PROPERTIES NONLINEAR 31 Standard elastoplastic joint model
JOINT PROPERTIES NONLINEAR 32 General elastoplastic joint model
JOINT PROPERTIES NONLINEAR 33 Nonlinear smooth contact model
JOINT PROPERTIES NONLINEAR 34 Nonlinear frictional contact model
JOINT PROPERTIES NONLINEAR 35 Nonlinear viscous damper model
MATERIAL PROPERTIES MASS Mass for nonstructural mass elements
PLASTIC DEFINITION Nonlinear plasticity material data
Optimised implicit Von Mises model MATERIAL PROPERTIES
NONLINEAR 75
MATERIAL PROPERTIES
NONLINEAR 64
DruckerPrager yield surface model
2
LUSAS Data Chapters
Data section
MATERIAL PROPERTIES
NONLINEAR 61
MATERIAL PROPERTIES
NONLINEAR 65
MATERIAL PROPERTIES
Description
Tresca yield surface model
NonAssociated MohrCoulomb yield surface model
Nonlinear multicrack concrete model
NONLINEAR 94
MATERIAL PROPERTIES
NONLINEAR 29
MATERIAL PROPERTIES
NONLINEAR USER
MATERIAL PROPERTIES
NONLINEAR RESULTANT USER
VISCOUS DEFINITION
Stress resultant elastoplastic model
User defined nonlinear material model
User defined nonlinear resultant material model
Viscous material data
CREEP PROPERTIES
CREEP PROPERTIES USER
Creep material properties
User defined creep material properties
VISCOELASTIC PROPERTIES Viscoelastic properties
VISCOELASTIC PROPERTIES USER User defined viscoelastic properties
DAMAGE PROPERTIES
DAMAGE PROPERTIES USER
DAMAGE PROPERTIES HASHIN
TWO PHASE MATERIAL
MATERIAL PROPERTIES RUBBER
MATERIAL PROPERTIES
NONLINEAR 81
MATERIAL PROPERTIES
NONLINEAR 86
MATERIAL PROPERTIES
NONLINEAR 89
MATERIAL PROPERTIES
NONLINEAR 27
MATERIAL PROPERTIES
NONLINEAR 26
MATERIAL PROPERTIES
Damage properties
User defined damage model
Hashin damage model for composites
Two phase material parameters
Rubber material properties
Volumetric crushing model
CEBFIP creep model
Generic polymer material model
2D elastoplastic interface model
3D elastoplastic interface model
Delamination interface properties
NONLINEAR 25
SHRINKAGE PROPERTIES
CEB_FIP_90
SHRINKAGE PROPERTIES
GENERAL
SHRINKAGE PROPERTIES USER
MATERIAL PROPERTIES FIELD
ISOTROPIC
MATERIAL PROPERTIES FIELD
ORTHOTROPIC
Concrete shrinkage properties
General shrinkage properties
User defined shrinkage model
Isotropic field model
Orthotropic field model
3
Chapter 1 Introduction
Data section
MATERIAL PROPERTIES FIELD
ORTHOTROPIC SOLID
MATERIAL PROPERTIES FIELD
LINK 18
MATERIAL PROPERTIES FIELD
Description
Orthotropic solid field model
Linear convection/radiation model
Nonlinear convection/radiation model
LINK 19
COMPOSITE MATERIAL
PROPERTIES
MATERIAL ASSIGNMENTS
COMPOSITE ASSIGNMENTS
ELEMENT AGES
Laminated/composite shell/solid materials
Material property assignments
Composite property assignments
Age of elements when using CEBFIP concrete model
Deactivate elements DEACTIVATE ELEMENTS
ACTIVATE ELEMENTS
DAMPING PROPERTIES
Activate elements
Frequency dependent Rayleigh parameters for viscous and/or structural damping
SLIDELINE PROPERTIES
SLIDELINE PROPERTIES USER
Slideline property definition
User defined slideline properties
SLIDELINE_SURFACE DEFINITION Slideline surface definition
SLIDELINE ASSIGNMENTS Slideline property assignments
THERMAL GAP PROPERTIES Linear thermal gap properties
LINEAR
THERMAL GAP PROPERTIES
GENERAL
General thermal gap properties
THERMAL CONTACT PROPERTIES Thermal contact properties
THERMAL RADIATION Thermal radiation properties
PROPERTIES
THERMAL ENVIRONMENT Thermal environment properties
PROPERTIES
THERMAL RADIATION SYMMETRY Thermal radiation symmetry planes
THERMAL_SURFACE SYMMETRY
ASSIGNMENT
Thermal radiation symmetry surface
THERMAL_SURFACE DEFINITION Thermal surface definition
THERMAL_SURFACE PROPERTY Thermal surface property assignment
ASSIGNMENT
THERMAL ASSIGNMENT Thermal gap and radiation surface
VIEW_FACTOR OUTPUT
ENVIRONMENTAL NODE
DEFINITION
ENVIRONMENTAL NODE
ASSIGNMENTS assignment
View factor output control
Environmental node definition
Environmental node assignment
4
LUSAS Data Chapters
Data section
NODAL FREEDOMS
FREEDOM TEMPLATE
CARTESIAN SETS
TRANSFORMED FREEDOMS
CONSTRAINT EQUATIONS
SUPPORT NODES
COUPLE
COUPLE READ
COUPLE WRITE
LOAD CASE
PDSP
CL
ELDS
DLDL, DLDG
DLEL, DLEG
PLDL, PLDG
UDL
FLD
CBF
BFP
BFPE
VELOCITY
ACCELERATION
SSI
SSIE
SSIG
SSR
SSRE
SSRG
TEMP
TMPE
ENVT
TEMPERATURE LOAD CASE
TDET
RIHG
TEMPERATURE LOAD
ASSIGNMENTS
TDET
RIHG
CURVE DEFINITION
CURVE ASSIGNMENT
5
Description
Number of freedoms at a node for thick shells
Optional definition of list of freedoms
Local Cartesian sets
Transformed freedoms
Constraint equations
Support conditions
Coupled analyses initialisation
Coupled analysis data read
Coupled analysis data write
Load case definition
Prescribed variables
Concentrated loads
Element loads
Distributed loads
Distributed element loads
Element point loads
Uniformly distributed loads
Face loads
Constant body forces
Body force potentials
Element body force potentials
Velocities
Acceleration
Initial stresses and strains at nodes
Initial stresses and strains for elements
Initial stresses and strains at Gauss points
Residual stresses at nodes
Residual stresses for elements
Residual stresses at Gauss points
Temperature loads at nodes
Temperature loads for elements
Environmental temperatures
Temperature load case
Temperature dependent environmental temperatures
Rate of internal heat generation
Temperature load assignments
TDET assignments
RIHG assignments
General curve definitions
General curve assignment
Chapter 1 Introduction
Data section
RETAINED FREEDOMS
ELEMENT OUTPUT
NODE OUTPUT
LOAD COMBINATION
ENVELOPE START
Description
Retained freedoms
Element output control
Nodal output control
Load combinations
Enveloping results start
ENVELOPE FINISH
SUPERELEMENT ASSIGN
SUPERELEMENT DEFAULT
SUPERELEMENT DEFINE
SUPERELEMENT USE
Enveloping results finish
Open a new superelement database
Change the default superelement database
Defines a superelement
Uses the superelement in the residual structure
Recovers superelement results SUPERELEMENT RECOVER
SUPERELEMENT DISTRIBUTE
SUPERELEMENT MODAL_DATA
NONLINEAR CONTROL
DYNAMIC CONTROL
TRANSIENT CONTROL
VISCOUS CONTROL
EIGENVALUE CONTROL
GUYAN CONTROL
SPECTRAL CONTROL
Distributes mass and stiffness from the residual structure to the superelement
Utilises user modal data in the residual structure
Nonlinear analysis control
Dynamic analysis control
Transient field analysis control
Creep analysis control
Eigenvalue analysis control
Guyan reduced eigenvalue analysis
Spectral response analysis control
HARMONIC_RESPONSE CONTROL Harmonic Response analysis control
FOURIER CONTROL Fourier analysis control
MODAL_DAMPING CONTROL Control for distributed viscous and/or structural damping
PLOT FILE
RESTART WRITE
RESTART READ
END
Plot file generation
Write to a restart file
Read from a restart file
Problem termination.
6
Reading and Writing LUSAS Data Syntax
Chapter 2 Syntax and Data
Preparation
Reading and Writing LUSAS Data Syntax
Although the commands and numerical values required for each stage of the data input may vary for different analyses, there is a common form, or syntax, for every data line.
This chapter defines the syntax rules to which every line of data input must conform.
LUSAS data syntax consists of command words and parameters. Command words instruct LUSAS of the data chapter or section being specified. Parameters provide details of the command section and are in the form of alphanumeric values. All data input for LUSAS is in a free format field, so reducing the time spent specifying data and reducing the possibility of errors. Certain command words or parameters are optional, and some data should be entered several times for different values.
Occasionally, alternative command words or parameters can achieve the same objective.
How To Read Syntax Lines In This Manual
In this manual LUSAS data syntax lines are identified by a keyboard icon in the margin, and each separate line begins with a bullet as shown below. Enter the text as you read it on the page whilst following these rules:
Curved brackets { } show alternative data input separated by a vertical line. You must choose one of the alternatives (mutually exclusive and compulsory). The brackets are not part of the syntax. Do not include them in your data input.
{COMMAND 1  COMMAND 2}
Square brackets [ ] show optional data input. You may use one of the data input options, or none at all. The brackets are not part of the syntax. Do not include them in your data input.
[option]
7
Chapter 2 Syntax and Data Preparation
or
[option 1  option 2]
Triangular brackets < >i=1,n show data input that you should repeat along the same line according to the subscript. The chevrons and subscript are not part of the syntax. Do not include them in your data input.
An arrow is used to indicate that lines should be repeated for tabulated data entry. For example, the following syntax line means enter n values across and m down.
< Vi(1) >i=1,n
. . . .
< Vi(m) >i=1,n
Throughout this manual, the form of LUSAS input data is indicated by syntax lines as described above, and the parameters and command words used are defined beneath each group of syntax lines. The data input is divided into data chapters and data sections. Commonly a data chapter will contain several data sections. For example, the data chapter:
NONLINEAR CONTROL
can contain the data sections:
INCREMENTATION
STEP REDUCTION
ITERATION
BRACKETING
BRANCHING
CONVERGENCE
OUTPUT
INCREMENTAL COUPLE READ
INCREMENTAL COUPLE WRITE
TERMINATION
Data chapters must generally be specified in order. Within each data chapter, data sections may generally be specified freely. In either case, those chapters or sections which are not mandatory may be omitted. A full list of LUSAS data sections, and their usual order, is given in the Introduction.
Data Delimitation
The position of data items on a line is not important providing each word or parameter is sufficiently delimited. The delimiters used in LUSAS are blank spaces and commas.
8
Reading and Writing LUSAS Data Syntax
Command Words
Command words instruct LUSAS of the data section currently being specified.
Commonly a data section (or command line) will require the specification of more than one command word. The LUSAS command interpreter only decodes the first 4 letters of each word, hence long commands may be abbreviated.
Titles
For most data chapters in LUSAS it is possible to add a title which will be printed out as a heading in the output file. Whenever a syntax line indicates that a title may be written, it may consist of any characters required. For example:
NODE COORDINATES [TITLE title]
title descriptive text
Numerical Values
When a syntax line indicates that a numerical value is required, for convenience, it can be written in a number of ways as indicated in the syntax line below. There should be no spaces within a numerical value. Where an integer parameter is specifically indicated, integer input should be used. However, in general, integer and real numbers may be mixed freely. Small or large numerical values may be written in exponential
(E) format.
[+  ]< DIGIT >[.< DIGIT >][E[+  ]< DIGIT >]
Simple Arithmetic Expressions
When a syntax line indicates that a numerical value is required it can be written as a simple arithmetic expression as indicated by the following:
VALUE < [*VALUE] [/VALUE] [**VALUE] >
The arithmetic expressions allowed in LUSAS are as follows, (note + and  are not allowed)
Multiplication
*
Division
/
Exponentiation **
Some examples of the use of arithmetic expressions are shown below:
Expression
8*2
8/2/2
8/2
Means
16
2
4
Expression
8**2
25E1/2
8*2/4
9
Means
64
1.25
4
Chapter 2 Syntax and Data Preparation
25E1*2 5 8/4**2 0.5
One of the uses of arithmetic expression input is that you can record in the data lines the component values which make up a numerical value. For example, the moment of inertia of a rectangular section is I=b*d*d*d/12 and you may wish to record the breadth b=4.3 and depth d=8.51, say, in the data as:
4.3*8.51**3/12
The arithmetic expression facility may also be employed for the conversion of units.
Comments
Comment lines may be placed anywhere in the data. A comment line must start with the letter C and must be followed by a space or comma. For example:
C This is a comment
Alternatively, individual lines of data may be annotated using a colon (:). All information specified to the righthand side of the colon will be treated as a comment.
For example:
1 13 1 71E9 0.34
Line Continuation
: This is a comment
When the data input is too long for a line, it may be continued onto the next line by the use of the continuation indicator, which is a space followed by three full stops (...).
Data lines may be continued in this way onto as many lines as is required. However, a title may continue onto one extra line only.
Implied Sequence Generation
The implied sequence facility may be used as a simple method for the automatic generation of data, and is incorporated into many of the LUSAS data sections. The general form of the implied sequence generator is:
N N last
N diff
where:
Nis the first number in the sequence
N last
is the last number in the sequence
N diff
is the difference between consecutive sequence numbers
Each specified number must be an integer. LUSAS will check that a valid sequence is formed and will write an error message if this is not the case. Sequences comprising of one number only, for example 5, may be specified as (5 5 0) or (5 0 0).
10
Reading and Writing LUSAS Data Syntax
The implied sequence generator is commonly used for the specification of sequences of nodes or elements, and its use can substantially reduce the amount of data specified.
For example, the instruction to assign material number 3 to elements 10, 20 and 30 may be written simply as:
MATERIAL ASSIGNMENTS
10 30 10 3
Incremental Line Generation
Throughout all stages of LUSAS input there are commands which can be used to generate data lines.
FIRST < V i
> i=1,n
[R]
INC <
1
i
> i=1,n
[R
1
]
. . . . . . .
INC <
1
i
> i=1,n
[R m
]
where:
Vithe numerical values on the data line to be generated. In certain circumstances these may consist of words which are simply duplicated.
Nthe number of numerical values on the data line
Rthe total number of repetitions of the first data line (inclusive) with unit increments added to each successive line. If this item is excluded a value of R=1 is assumed.
1
ithe increments added to all data generated in the lower (m1) levels. These increments may take any numerical values.
Rmthe total number of repetitions of all data lines generated in the lower (m1) levels.
The following simple examples illustrate the use of the general data generation. The data lines:
1 10 1 5.1
11 20 1 5.2
21 30 1 5.3
31 40 1 5.4
may be automatically generated using the data commands:
FIRST 1 10 1 5.1
INC 10 10 0 0.1 4
When constructing element meshes by hand (as opposed to automatic mesh generation) it is often useful to number the nodes and elements such that the incremental line generator may be used. For example, when using 8 noded quadrilateral elements, the
11
Chapter 2 Syntax and Data Preparation
node numbering may be specified so as to include fictitious central nodes. In this way a general element topology sequence is maintained.
TABLE Input
In certain circumstances, for example the specification of temperature dependent material properties, LUSAS requires a tabular form of input data. In such cases the
TABLE data command may be used.
TABLE N [TITLE title]
< V
(1)i
> i=1,n
. . . .
< V( m)i
> i=1,n
where:
Nis the table identification number.
V
(k)i
are the values for the kth row of the table.
mis the number of rows in the table.
Notes
Data specified in tabulated form will be linearly interpolated at values between those values indicated.
Nonlinear variations may be input by increasing the number of tabulated data lines, and therefore approximating the nonlinear distribution by a number of straight lines.
The end of tabulated input is indicated by a new command word.
12
System Parameters
Chapter 3 LUSAS
Data Input
System Parameters
The data section SYSTEM may be used to modify certain values which define particular machine and program parameters.
SYSTEM vbname = n
END
vbname permitted system variable name (see below)
n
Notes
the new value to be assigned to vbname
1. The SYSTEM header must be the first command in the input data.
2. SYSTEM input must always be terminated by the END command.
The following system variables may be modified (the default settings are shown in brackets):
BULKLF
Linear viscosity coefficient for explicit dynamics elements (0.06)
BULKQF
Quadratic viscosity coefficient for explicit dynamics elements (1.5)
CRKTOL
Tolerance on ratio for cracking (0.01)
CTOL
Creep strain convergence tolerance (1.0E8)
DECAY
Maximum diagonal decay allowed before problem termination (1.0E20)
DECAYL
Limit of diagonal decay before warning messages are output (1.0E4)
EIGSCL
Scaling factor used to compute the stresses from eigenvectors (1.0E20)
HGVISC
Hourglass viscosity coefficient for explicit dynamics elements (0.1)
LSMAX
Maximum number of iterations for arclength to compute load level (150)
LPGNUM
The number of records of the paging file allowed in the cache (2500)
IECHO
Echoes system status to screen (1)
IPGFAC Page factor used to set maximum size of files which can be created.
IPFAC may be set to 1,2,4,8 (default),16,32 or 64. With IPGFAC=1 the
13
Chapter 3 LUSAS Data Input
max file size is 8Gb. IPGFAC =2 max file szie is 16Gb, IPGFAC=4 max file size is 32Gb etc.
MAXERR
Maximum number of times a single error will be output (50)
MAXNB
A large number which should not be exceeded by any element or node number (5000000)
MAXRSA
Maximum number of attempts allowed to set the symmetry tolerance
TOLSYM (0)
MAXSEG
Maximum number of segments defining a radiation surface (100)
MEIGSH
Maximum number of eigensolutions computed at a shift point (6)
MREFCE
Maximum number of elements sharing a common face (3)
MXEEST
Override estimate for total number of edges in structure (0)
MXELIM
Maximum number of equations to be eliminated simultaneously in the parallel frontal algorithm (6)
MXELGP
Maximum number of elements stored in an element group (Set automatically unless specified)
MXFEST
Override estimate for total number of faces in a structure (0)
MXIT
Maximum number of iterations in slideline slave search (500)
MXMNDZ
Maximum allowable frontwidth (5000)
MXSLAE
Maximum number of adjacent elements for contact nodes in slidelines or maximum number of adjacent thick shell elements at any node (64)
MXSLAN
Maximum number of adjacent nodes for contact nodes in slidelines (64)
MXWAIT
Maximum wait in seconds for DTF file before terminating analysis (900)
NCPU
Number of processors used in the parallel frontal algorithm (1)
NCITER
Iteration number at which to switch to iterative updates for multi crack concrete with crushing model (6)
NDPGSZ
Record length for any new direct access files in bytes (16384)
NIDX
Size of master index table (50000)
NLPZ
Number of real locations in the database (see on page)
NONNAT
Switch to ensure binary compatibility between PC and UNIX platforms (0, i.e., no binary compatibility)
NPGMAX
Maximum record length for direct access files in integer words (4096)
NPGS
Maximum number of records allowed in the cache (960)
PENTLY
Penalty stiffness coefficient used in constraint equations (0.0)
QMHDLM Lower limit multiplier on hardening moduli for Mohr Coulomb model
QTOL
(0.01)
Yield function convergence tolerance (1.0E6)
SHLANG
Maximum angle (in degrees) between nodal normals after which 6 degrees of freedom are assigned to a node (maximum value=90). Applicable to thick shell elements. (20)
SLFNCS Slideline normal force scale factor for contact cushioning (1.0)
SLSTCC
Slideline stiffness factor for close contact (1.0E3)
SLSTFM
Slideline surface stiffness ratio (100.0)
SLSTPC
Slideline stiffness factor for precontact (1.0)
14
Problem Definition
SSCALE
Scaling parameter for creep algorithms (1.0)
STEFAN
StefanBoltzmann constant, temperature units of the value input must be
Kelvin (5.6697E8 W/m2 K4 )
STFINP
Inplane stiffness parameter for flat shell elements (0.02)
STFSCL
Stiffness matrix scaling factor for element deactivation (1.0E6)
TOLFIJ
Environment view factor tolerance, a radiation link may be formed if the environment view factor for a surface segment exceeds this value (1.0)
TOLNOD
Tolerance distance for node on node contact in a slideline analysis (1.0E
3)
TOLSYM
Symmetry plane tolerance, a node is considered to lie in a symmetry plane if its perpendicular distance from the plane is less than this value (1.0)
IZPPRB Compression level on PROBLEM database (default 0)
IZPSHP Compression level on SHAPES database (default 0)
IZPFRN Compression level on FRONTAL database (default 0)
IZPPLT Compression level on PLOT database (default 1)
IZPRST Compression level on RESTART database (default 1)
IZPDTF Compression level on DTF database (default 0)
IZPADP Compression level on ADAPT database (default 0)
IZPSUP Compression level on SUPER database (default 0)
IZPDBM Compression level on all other database (default 0)
BBOXF
Scaling factor applied to increase bounding box which proscribes a slideline contact segment (default 1.2)
Problem Definition
The problem may be defined using the data sections for:
Problem description (mandatory)
Units definition (optional)
Options (optional)
The PROBLEM data section is mandatory (specification of UNITS and OPTIONS is optional).
Problem
The PROBLEM data section defines the start of the problem data and is mandatory for all analysis types.
PROBLEM [TITLE title]
title
Descriptive text
Notes
1. Data input for each problem must commence with the PROBLEM data section.
2. Title text can only be continued onto one additional line.
15
Chapter 3 LUSAS Data Input
Units definition
LUSAS is unit independent, hence all data quantities must be specified in a consistent set of units (irrespective of whether the UNITS data section is specified). The UNITS data section may be used to name the units used, in order that the output quantities may be annotated.
frc
lth
mas
tim
tem
UNITS frc lth mas tim tem
A word for the units of force
A word for the units of length
A word for the units of mass
A word for the units of time
A word for the units of temperature
Notes
3. All input data must be consistent with the units chosen for each problem. For dynamic analyses, if units are chosen for mass(m), length(l) and time(t), consistent units of force are given by,
F = m a = ml/t/t
4. The UNITS command enables you to choose a symbol for force, length, mass, time and temperature, that will be printed out at the top of the column headings of the results output.
5. If a symbol for force, length or mass is specified which contains more than three characters, then only the first three characters will be output.
Options
The OPTIONS data section may be used to specify user definable analysis options.
N i
OPTIONS < N i
> i=1,n
The OPTION number(s)
Notes
1. For a problem requiring more than one option, repeat the line or add option numbers (negative option numbers may be used to disable previously enabled options), as in the following example:
OPTION 40 45 55
OPTION 87
OPTION 77 55
2. There is no limit to the number of OPTION lines in the data input.
16
Data Groups
3. Options may be specified and respecified at any point in the LUSAS datafile.
Some options may be subsequently disabled by specifying a negative number; for example, the output of strains can be switched on and off at different points using
Option 55, whilst it is not permissible to reset Option 87 which defines the problem type to be Total Lagrangian.
4. A full list of user options is included in the Appendices
Data Groups
Data groups may be used to collectively assign quantities to defined sequences of elements. GROUP is a general purpose utility which can be used to replace a series of first, last, difference element sequences within certain LUSAS data chapters (see
Notes).
GROUP igroup [TITLE title]
L L last
L diff
igroup
Group reference number
title
Descriptive text
L L last
L diff
Notes
The first, last and difference between element numbers in a serie
1. The GROUP command must be specified before the ELEMENT TOPOLOGY data section.
2. The numbers defined in a group are checked to determine if a duplicate number has been specified.
3. The first and last number must be positive.
4. Groups may be utilised in GEOMETRIC ASSIGNMENTS, MATERIAL
ASSIGNMENTS and COMPOSITE ASSIGNMENTS.
Element Topology
The data section ELEMENT TOPOLOGY is used to input the node numbers of the elements. The ELEMENT TOPOLOGY data section therefore describes the connectivity of the finite element discretisation.
type ELEMENT TOPOLOGY [TITLE title]
L < N i
> i=1,n
< E i
> i=1,m
type
L
N i
E i
The element type identifier as given in the description of each element; refer to the LUSAS Element Reference Manual.
The element number allocated to the particular element being defined.
The node numbers for each node of the particular element being defined.
The moment end conditions which apply only to BEAM, BRP2, BMS3,
BTS3 and GRIL elements. Put Ei as R for a restrained rotation (default) and F for a free rotation. The BTS3 element also allows translational
17
Chapter 3 LUSAS Data Input
n
m
Notes
degrees of freedom to be released (see the element descriptions in the
LUSAS Element Reference Manual for further details).
The total number of nodes for the particular element type.
The number of end releases.
1. For problems idealised with more than one element type, the header line
ELEMENT TOPOLOGY is repeated for each element type and followed by the element number and node numbers for each element.
2. Each element must be given a unique identifying number. If an element number is repeated, the new element node numbers overwrite the previous element node numbers and an advisory message is printed out.
3. The elements should preferably be numbered in ascending order across the narrow direction of the structure (see Solution Order).
4. The element numbers may have omissions in the sequence and need not start at one. The order in which the element numbers are specified is arbitrary.
5. The element node numbers must be specified in the order shown in the element diagrams in the LUSAS Element Reference Manual.
Example 1. Element Topology
TPM3 ELEMENT TOPOLOGY
1 1 5 4
2 1 2 5
3 2 6 5
4 2 3 6
4
1
5
3
6
2
4
1
2
3
18
Element Topology
Example 2. Element Topology
QPM8 ELEMENT TOPOLOGY
FIRST 1 1 6 11 12
13 8 3 2
INC 1 2 2 2 2 2
2 2 2 2
INC 2 10 10 10 10
10 10 10 10 3
5
4
3
2
1
10
15
20
2
14
4
8
1
12
13
18
23
3
22
6
11
16
21
26
31
5
24
28
32
25
6
33
34
30
35
Example 3. Element Topology
QPM4 ELEMENT TOPOLOGY
FIRST 3 1 4 5 2
INC 2 1 1 1 1 2
INC 1 3 3 3 3 2
BAR2 ELEMENT TOPOLOGY
FIRST 1 1 4
INC 1 3 3 2
INC 6 2 2 2
3
2
1
7
5
3
1
6
5
4
8
6
4
2
9
8
7
19
Chapter 3 LUSAS Data Input
Example 4. Element Topology
BEAM ELEMENT TOPOLOGY
16 1 8 R F
FIRST 1 5 6 R R
INC 1 1 1 (3)
INC 3 4 4 (3)
FIRST 10 6 10 F R
INC 1 1 1 (3)
FIRST 13 10 14 R R
INC 1 1 1 (3)
18 17 19 R R
17 15 19 F R
12
12
15
16 20
4 8
7
3
11
11
6
14
15
9
17
19
3
2
16
6
2
10 10
5
13 14
8
18
1 4
7
1 5 9 13 17
Solution Order
The SOLUTION ORDER data section controls the efficient solution of the finite element discretisation. This command is not essential and may be omitted. However, in certain instances, a significant improvement in computation, both in time and cost may be achieved by the judicious selection of the element solution order.
SOLUTION ORDER [ASCENDING  PRESENTED  AUTOMATIC
[nopt nitopt]] [TITLE title]
{L L last
L diff
 G igroup}
nopt
Automatic optimiser selection (default=4)
=1 standard LUSAS optimiser
=2 AkhrasDhatt optimiser
=3 CuthillMcKee optimiser
=4 Sloan optimiser
nitopt
(when nopt=2) Number of optimising iterations (default=30)
(when nopt=3) Optimisation target (default=4)
1 RMS wavefront
2 Bandwidth
3 Profile
4 Max wavefront
L L last
L diff
The first, last and difference between element numbers in a series
G
Command word which must be typed to use element groups.
igroup
Element group reference number.
Notes
20
Solution Order
1. If the header line is left out the default action is SOLUTION ORDER
ASCENDING and the structure is solved according to ascending element number.
2. For SOLUTION ORDER PRESENTED the structure is solved according to the order in which the elements were presented in ELEMENT TOPOLOGY.
3. Element number data is not required for the SOLUTION ORDER PRESENTED.
4. With SOLUTION ORDER AUTOMATIC, Option 100 may be used to output the optimum element order for the frontal solution.
5. Each element number must only be specified once.
6. Fewer elements may be specified for SOLUTION ORDER than those specified in
ELEMENT TOPOLOGY. If an element is not required in the solution it should be omitted from the data input.
7. Specification of element numbers not specified in ELEMENT TOPOLOGY is illegal.
8. The standard LUSAS optimiser should not be used for unconnected structures. If this occurs, an error message is output stating that the finite element mesh has an unconnected element. Option 100 will indicate all the elements within the structure as negative, those with a positive number are outside the structure.
9. Option 282 will switch the default optimiser to the standard LUSAS optimiser for compatibility with pre LUSAS version 12 data files.
Example 1. Solution Order
24 4 8 12 16
QPM4 ELEMENT TOPOLOGY
FIRST 13 21 1 2 22
INC 1 1 1 1 1 3
FIRST 1 1 5 6 2
23
15
14
3
3
2
7
6
5
11
9
8
15
INC 1 1 1 1 1 3
INC 3 4 4 4 4 3
SOLUTION ORDER PRESENTED
22
21
13
2
1
1
6
5
4
10
9
7
14
13
21
Chapter 3 LUSAS Data Input
Example 2. Solution Order
SOLUTION ORDER
1 2 1
30
3 6 1
31
7 10 1
32
11 12 1
33 36 1
FIRST 13 16 1
INC 6 6 0 3
4
3
30
2
1
8
7
31
6
12 36 16
11
32
35
10 34
15
14
5 9 33 13
22
21
20
19
28
27
26
25
Solver Type
The SOLVER data section allows the specification of the solver to be used for the solution of the set of linear equations. This command is not essential and may be omitted, which will cause LUSAS to choose either the standard or the fast frontal solver, depending on the type of problem to be solved. However, in certain instances, a significant reduction in both computation time and memory may be achieved by choosing the iterative solver. It is also possible to assemble and write the global stiffness matrix and load vector(s) (or mass matrix, for eigenvalue problems) to binary files, without solving for the displacements.
SOLVER {FRONTAL  FAST  ASSEMBLE}
or
SOLVER CONJUGATE_GRADIENT {INCOMPLETE_CHOLESKY 
DECOUPLED  HIERARCHICAL} [droptol] [itmax]
droptol Drop tolerance parameter determining the size of the preconditioning matrix used during the conjugate gradient solution. The size of this matrix affects the nature of the iterative process, with larger preconditioning matrices giving rise to fewer, but more computationally expensive, iterations. The default value is 1.0, which produces relatively small matrices (i.e. fewer nonzero entries), which is suitable for well conditioned problems that do not require many iterations to achieve convergence. For more illconditioned problems, values in the range [1e3,
1e6] are recommended.
22
Solver Type
itmax
Maximum number of conjugate gradient iterations to be processed (default
= 5000).
Notes
1. The fast frontal solver will solve all problems except superelement analyses,
Guyan reduction and nonlinear problems using branching and bracketing.
2. For the fast frontal solver, the maximal and minimal pivots returned are based on magnitude, whereas the standard frontal solver returns pivots based on algebraic position. For example, if a problem gave rise to the three pivots 10.0, 0.1 and 1.0, the fast solver would return 10.0 and 0.1 as the maximum and minimum, respectively, whereas the standard solver would return 10.0 as the maximum and 
1.0 as the minimum.
3. For the standard frontal solver, the concept of negative pivots is synonymous with that of negative eigenvalues, which signify when a bifurcation point has been reached during a nonlinear analysis, and also whether a structure is loading or unloading. Thus warnings are given for negative pivots that are encountered during the solution phase. For the fast frontal solver, the concept of negative pivots is different from that of negative eigenvalues, and warnings of their existence are not given. For symmetric matrices, the number of negative eigenvalues is returned separately, and for nonsymmetric matrices, the determinant of the stiffness matrix is returned, from which the parity of the eigenvalues (whether there are an even or odd number of negative eigenvalues) can be deduced. LUSAS uses this information during a nonlinear analysis when using the fast solver, so the same results will be observed regardless of the solver used.
4. The conjugate gradient solver may only be used for linear, static analyses that give rise to symmetric, positivedefinite stiffness matrices.
5. The INCOMPLETE_CHOLESKY option chooses Incomplete Cholesky preconditioning, which is applicable to all analyses for which the conjugate gradient solver may be used. With a judicious choice of drop tolerance, convergence is guaranteed for most problems.
6. The DECOUPLED option chooses Decoupled Incomplete Cholesky preconditioning, and may be used for all analyses except those involving tied slidelines, thermal surfaces and Fourier elements. It generally leads to faster overall solution times than Incomplete Cholesky preconditioning, although more iterations are required for convergence. For less well conditioned problems, the conjugate gradient algorithm may not converge using this technique, so care should be taken.
7. The HIERARCHICAL option chooses Hierarchical Decoupled Incomplete
Cholesky preconditioning, which is only available for models consisting entirely of two and threedimensional, solid continuum, quadratic elements, and offers excellent convergence properties. It is by far the most effective technique for models of this type, and when used in conjunction with fine integration (OPTION
18) allows solutions to be obtained for relatively illconditioned problems. For very illconditioned problems of this type (e.g. where the average element aspect
23
Chapter 3 LUSAS Data Input
ratio is high), an extra preconditioning option exists (OPTION 323) which will often yield a solution faster than using a direct solver.
8. When using the conjugate gradient solver with hierarchical basis preconditioning, if any midside degrees of freedom are supported or prescribed, their corresponding vertex neighbours must also be supported or prescribed. For example, if a midside node is fixed in the xdirection, all nodes on the same edge of that element must also be fixed (or prescribed) in the xdirection.
9. Problems involving constraint equations cannot currently be solved with the iterative solver, since the resulting stiffness matrix is nonpositivedefinite.
10. For problems with multiple load cases, iterative solvers are less efficient since a separate iterative process is required for each load case, and the total time taken will increase in proportion to the number of load cases. By contrast, direct solvers incur very little extra cost when solving for multiple load cases.
11. Guyan reduction and superelement analyses cannot be solved iteratively, since matrix reduction does not take place.
12. The iterative solver will perform very poorly if there is not enough main memory for the solution to proceed incore. To guard against this, a data check (OPTION
51) may be performed (as with the direct solvers), which will estimate the amount of memory the iterative solver would use with the specified drop tolerance and choice of preconditioning technique.
13. If a convergence history of the iterative process is desired, OPTION 247 can be activated to write the residual norm of the solution vector to the output file after each iteration.
14. The preconditioning matrix can be stored using single precision storage (OPTION
248), which can significantly reduce the total amount of memory required for solution. For illconditioned problems, however, the rate of convergence may be affected, and the incomplete Cholesky factorisation may fail, hence this option must be used with care.
15. The iterative solver has limited error diagnostics to warn against illdefined or incompletely specified models. If this is suspected, the analysis should be run through the standard frontal solver for more comprehensive error diagnostics.
16. For the iterative solver, the convergence criterion is a tolerance value of 1e6 for the residual of the solution vector. If the solution returned by the iterative solver is deemed unsatisfactory, this tolerance can be lowered by altering the system parameter SOLTOL. It should not be raised under normal circumstances, unless an approximate solution only is required.
17. For the fast frontal and iterative solvers, the global matrix assembly involves the use of scratch files, since the size of the matrix data can be very large. For small problems which require many load increments or time steps, the global assembly process can be forced to remain incore (OPTION 17) by placing it under the control of the data manager, assuming sufficient memory is available.
18. For the ASSEMBLE option, the data can be written to ASCII files by setting the system parameter MCHOUT to 0. The matrices are written in standard compressed
24
Nodal Coordinates
row (or HarwellBoeing) format. For binary files, the order of the data written is as follows:
N
NJA
IA
(integer  number of rows and columns)
(integer  number of nonzero entries in the matrix)
(integer array, length N+1  stores row pointers for the columns
JA array JA)
(integer array, length NJA  stores column indices for the non
A zero entries)
(double precision array, length NJA  stores values for the nonzero entries)
Note that for symmetric matrices, only the upper triangular part of the matrix will be written to the file.
For vectors, the order of the data written to binary files is as follows:
N
(integer  total number of rows)
NVEC
(integer  number of load cases)
VECTOR
(double precision array, dimensioned (N, NVEC)  vector of values)
19. When using the fast frontal solver jobs sometimes fail because the presence of a large number of constraint equations causes an excessive amount of pivotting during the solution. To reduce the amount of pivotting a smaller value for the system parameter PVTTOL (default=0.01) can be specified in the data file.
Nodal Coordinates
The data chapter NODE COORDINATES is used to specify the nodal coordinates, defined in the global Cartesian system. All coordinates can be input using the NODE
COORDINATE command. Alternatively the following facilities may be used within the NODE COORDINATES data chapter in order to aid or automate nodal coordinate generation:
Local Coordinate Systems
Spacing Nodal Coordinates on a Line
Spacing Nodal Coordinates on an Arc
Spacing Nodal Coordinates in a Quadrilateral
Copying Nodes
Renumbering Nodes
Deleting Nodes
Node Coordinates
The NODE COORDINATES data section inputs the nodal coordinates in the global
Cartesian coordinates of the problem.
NODE COORDINATES [TITLE title]
N X,Y [Z]
25
Chapter 3 LUSAS Data Input
N
The node number allocated to the particular node being defined.
X,Y,Z
The global coordinates of the node. For 2D structures only X and Y need be specified.
Notes
1. If a node is repeated the new coordinate values overwrite the previous values and an advisory message is printed out.
2. LUSAS checks for nodes with same coordinates and if encountered, prints out an advisory message (Option 2 suppresses this check).
3. If several nodes are overwritten or specified in an arbitrary order, you can request output of the final node coordinates in ascending order with Option 30.
4. Extra dummy nodes, not associated with particular elements, may be specified.
These dummy nodes can, for example, be used to simplify data generation.
Y z
Node
Node z
Y y y
0
0
X x x x
2D and 3D Coordinate Definition
Local Coordinate Systems
Local Cartesian coordinates may be used to generate coordinate points in each of the local systems indicated that follow.
LOCAL {CARTESIAN  CYLINDRICAL  SPHERICAL}
COORDINATES N
0
N x
[N xy
]
N { X,Y  X,Y,Z  X,r,
x
 r,
x
,
c
}
A return to global coordinates may be obtained following the command GLOBAL
CARTESIAN COORDINATES.
26
Nodal Coordinates
GLOBAL CARTESIAN COORDINATES
No
Nx
Nxy
The node defining position of local axis origin.
The node together with No defining the positive direction of local xaxis.
The node defining the position of xy plane i.e. any point in the positive
N quadrant of the local xy plane. (Not required for 2D coordinates).
The node number allocated to the particular node being defined.
X, Y, Z Local Cartesian coordinates (see Local Cartesian Coordinates).
X, r,
x
Local cylindrical coordinates (see Local Cylindrical Coordinates).
r,
x
,
Notes c
Local spherical coordinates (see Local Spherical Coordinates).
1. After insertion of a LOCAL COORDINATE header line, LUSAS assumes that all subsequent node coordinate data refers to that local coordinate system.
2. The coordinates of the nodes, with respect to the global coordinate axes, defining the position and orientation of the local axes must be defined prior to the insertion of LOCAL COORDINATE header line.
3. Other coordinate generation procedures such as FIRST, SPACING,
QUADRILATERAL and COPY may be used in local coordinates (see subsequent commands in this section).
4. A set of LOCAL COORDINATE data must always be terminated by the
GLOBAL CARTESIAN COORDINATE command. This command transforms the local node coordinates into the global coordinates in which LUSAS operates, and outputs the global coordinate values.
5. There is no limit to the number of sets of LOCAL COORDINATE data, but each set should be terminated by the GLOBAL CARTESIAN COORDINATE command before the subsequent set of LOCAL COORDINATE data is specified.
6.
x and c are specified in degrees.
27
Chapter 3 LUSAS Data Input
Local Cartesian Coordinates
For LOCAL CARTESIAN
COORDINATES the following definitions apply: x y z distance from the local origin in the local xdirection. distance from the local origin in the local ydirection. distance from the local origin in the local zdirection.
Local Cylindrical Coordinates
For LOCAL CYLINDRICAL
COORDINATES the following definitions apply: x r qx distance from the local origin in the local xdirection. radius from the local xaxis in the local yzplane. angle in degrees from the side of the local xyplane about the local xaxis (righthand screw rule). z
0 x y x x
Y
No d e
x y r
Node z x z
28
Nodal Coordinates
Local Spherical Coordinates
For LOCAL SPHERICAL
COORDINATES the following definitions apply: r qx qc radius from the local origin angle in degrees from the positive quadrant of the local xyplane about the local xaxis. The rotation is clockwise when looking along the xaxis in the positive direction (right hand screw rule). angle in degrees from the local xaxis to the radius line. y x
Example 1. Local Cartesian Coordinates
Y
Cartesian Coordinates
c r
x
Node z y
5.0
5.0
4
5
1
2
6
3 x
101 (9.0, 4.0)
100 (3.0, 1.0)
5.0
10.0
X
NODE COORDINATES
100 3.0 1.0
101 9.0 4.0
LOCAL CARTESIAN COORDINATES 100 101
29
Chapter 3 LUSAS Data Input
FIRST 1 2 1
INC 1 1 0 3
INC 3 0 1 2
GLOBAL CARTESIAN COORDINATES
Example 2. Local Cylindrical Coordinates
x
Cylindrical Coordinates
51 (4,4,6)
Z
10
9 y z
0
NODE COORDINATES
50 4 4 0
51 4 4 6
Y z
3
4
2
5
30
52 (4,8,0)
1 y
8
7
50 (4,4,0)
6
X
Nodal Coordinates
52 4 8 0
LOCAL CYLINDRICAL COORDINATES 50 51 52
1 0 2 0
2 0 2 45
3 0 2 90
4 0 2 135
5 0 2 180
6 0 2 225
7 0 2 270
8 0 2 315
9 3 2 0
10 3 2 45
GLOBAL CARTESIAN COORDINATES
Spacing Nodal Coordinates on a Line
The SPACING command computes the coordinates of a line of nodes from the coordinates of the end nodes and the defined spacing ratios.
SPACING [ {X  Y  Z} RATIOS]
N N last
N diff
< S i
> i=1,n
N N last
N diff
The first node, last node and difference between nodes of the series of nodes to be spaced.
S i
The ratios of the spaces between consecutive nodes. For M spaces with the same value S use an asterisk to automatically repeat value as M*S. Note
n
Notes
that i 120 even when M*S format is used.
The number of spaces between consecutive nodes.
1. The coordinates of the first and last nodes of a line must be specified before the spacing data line.
2. Projections of the line connecting the N and Nlast nodes on the X, Y and Z axes may be evaluated by using the SPACING X RATIOS, SPACING Y RATIOS and
SPACING Z RATIOS commands respectively.
3. It is permissible to specify up to 120 spacing ratios. If the data will not fit on to one line use the LUSAS line continuation symbol (three dots …) to continue onto a second line.
4. Additional spacing data may be specified without repeating the header line.
31
Chapter 3 LUSAS Data Input
Example 1. Node Coordinates Spacing on a Line
This data file segment:
NODE COORDINATES
5 1 1
25 9 7
SPACING
5 25 5 1.667 1.667
1.667 5.0
Has the same effect as this one:
NODE COORDINATES
5 1 1
25 9 7
SPACING
5 25 5 3*1.667 5.0
Y
5.0
5.0
1.667
1.667
1.667
15
10
20
5 (1.0, 1.0)
5.0
25 (9.0, 7.0)
10.0
X
32
Nodal Coordinates
Example 2. Node Coordinates Spacing on a Line
This data file segment:
NODE COORDINATES
11 1.0 2.0
16 11.0 2.0
29 1.0 7.5
34 11.0 7.5
SPACING
11 29 6 2*2.0 1.5
16 34 6 2*2.0 1.5
11 16 1 3*1.25
3.75 2.5
17 22 1 3*1.25
3.75 2.5
23 28 1 3*1.25
3.75 2.5
29 34 1 3*1.25
3.75 2.5
Has the same effect as this one:
NODE COORDINATES
11 1.0 2.0
16 11.0 2.0
29 1.0 7.5
34 11.0 7.5
SPACING
FIRST 11 29 6 2*2.0 1.5
INC 5 5 (2)
FIRST 11 16 1 3*1.25
3.75 2.5
INC 6 6 (4)
Y
29 30 31 32
23
24 25 26
17
18 19 20
33
27
21
11
12 13 14
1.25
1.25 1.25
5.0
3.75
15
33
34
28
1.5
22
2.0
2.0
16
X
Chapter 3 LUSAS Data Input
Spacing Nodal Coordinates on an Arc
The SPACING ARC RATIOS data section computes the coordinates of a circular line of nodes from the coordinates of the end nodes and the defined arc ratios.
SPACING [X  Y] ARC RATIOS X c
Y c
[Z c
] [N d
]
N Nlast Ndiff < Si >i=1,n
Xc, Yc, Zc The coordinates of the centre of the circle.
Nd
The node defining the direction in which nodes are to be spaced around circle.
N Nlast Ndiff
The first node, last node and difference between nodes of the series of nodes to be spaced.
Si
The ratio of the arc spaces between consecutive nodes. For M spaces with the same value S use an asterisk to automatically repeat value as M*S.
n
Notes
Note that i 120 even when M*S format is used.
The number of arc spaces between consecutive nodes.
1. The coordinates of the first, last and centre nodes of a circular line must be specified before the spacing data line. The radius between the centre node and the
N and Nlast nodes must be equal.
2. It is permissible to specify up to 120 arc spacing ratios. If the data will not fit onto one line, use the LUSAS line continuation symbol (three dots …) to continue onto a second line.
3. Additional spacing data may be specified without repeating the header line.
4. The program will assume that the nodes will be spaced around the shortest arc length between the first and last nodes. For sweep angles greater than 180, a node, lying in the plane and direction of the circular line to be generated, must be specified on the header line. The coordinates of this direction node must be specified prior to the header line.
5. Incremental generation may be used to generate several circular lines with the same centre. For M arc spaces with the same increment value S, use the asterisk repeat facility as M*S. Zero arc spacing ratio increments need not be specified if the total number of lines are put in brackets.
6. The projection of the X or Y coordinate of the arc onto the X or Y axis is calculated using the SPACING X ARC RATIOS and SPACING Y ARC RATIOS respectively. The projected nodes lie in the same Zplane as the centre of the circle.
7. When using SPACING X (or Y) ARC RATIOS the first and last Y (or X) coordinates must not change sign over the segment of arc being generated.
34
Nodal Coordinates
Example 1. Node Coordinates Spacing on an Arc
This data file segment:
NODE COORDINATES
1 11.0 1.0
13 0.437 9.863
SPACING ARC RATIOS 2.0
1.0
1 13 3 16.67
16.67 16.67 50.0
Has the same effect as this:
NODE COORDINATES
1 11.0 1.0
13 0.437 9.863
SPACING ARC RATIOS 2.0
1.0
1 13 3 3*16.67
50.0
Y
13 (0.437, 9.863)
10
7
5.0
50°
16.67°
16.67°
16.67°
4
1 (11.0, 1.0)
5.0
X
Example 2. Node Coordinates Spacing on an Arc
This data file segment:
NODE COORDINATES
11 5.33 0.5
26 9.66 3.0
Has the same effect as this:
NODE COORDINATES
11 5.33 0.5
26 9.66 3.0
35
Chapter 3 LUSAS Data Input
15 1.0 3.0
30 1.0 8.0
SPACING
15 30 5 1.0 2.0
2.0
11 26 5 1.0 2.0
2.0
SPACING ARC RATIOS 1.0 
2.0
11 15 1 25 15
2*10
16 20 1 25 15
2*10
21 25 1 25 15
2*10
15 1.0 3.0
30 1.0 8.0
SPACING
15 30 5 1.0 2.0
2.0
11 26 5 1.0 2.0
2.0
SPACING ARC RATIOS 1.0 
2.0
FIRST 11 15 1 25 15
2*10
INC 5 5 0 (4)
Y
25
20
15
30
10.0°
29
10.0°
28
15.0°
24
23
19
18
14
13
12
17
22
27
11
16
21
25.0°
26
X
(1 .0, 2.0)
36
Nodal Coordinates
Spacing Nodal Coordinates in a Quadrilateral
The data section QUADRILATERAL SPACING generates node coordinates for plane or parabolic quadrilateral zones.
QUADRILATERAL SPACING
N { X,Y  X,Y,Z }
SIDE POINTS
N N last
N diff
[ X s
,Y s
 X s
,Y s
,Z s
]
N
A corner node number of the quadrilateral zone to be generated.
X, Y, Z The global coordinates of a corner node. For 2D structures, only X, Y are specified. Four corner node data lines are required in any order.
N Nlast Ndiff
The first node, last node and difference between nodes of the series of nodes along a side of the quadrilateral zone.
Xs, Ys, Zs The global coordinates of a point along a side of the quadrilateral zone which defines the parabolic shape and grading of the line of nodes.
This point must lie inside the central half of the side and need not be coincident with any node. Four side point data lines are required in any order.
Notes
1. If the coordinates of the side points are omitted a straight sided regularly spaced quadrilateral will be generated.
2. The angle subtended at any corner of a quadrilateral zone must be less than 180° otherwise nonuniqueness of mapping may result.
37
Chapter 3 LUSAS Data Input
Example 1. Node Coordinates Quadrilateral Spacing
Y
14
15
16 (7.0, 7.0)
13 (4.0, 5.0)
12
11
9
10
8
5
6
7
3
1 (1.0, 1.0)
2
4 (10.0, 1.0)
X
NODE COORDINATES
QUADRILATERAL SPACING
8 2 1
11 7 1
29 8 5
26 2.5 5
SIDE POINTS
8 11 1 4.5 1.6
11 29 6 7 3
26 29 1 5.25 5.6
8 26 6 1.8 3
38
Nodal Coordinates
Example 2. Node Coordinates Quadrilateral Spacing
Y
4 6 4 8 5 0 5 2
*
(3 .0 , 6 .0 )
5 4
3 4 3 6 3 8
*
(0 .0 , 3 .0 )
2 2 2 4 2 6
4 0
2 8
4 2
3 0
5 6
4 4
*
(9 .0 , 3 .0 )
3 2
1 0 1 2 1 4
*
(3 .0 , 0 .0 )
1 6 1 8 2 0
X
NODE COORDINATES
QUADRILATERAL SPACING
10 0 0
20 9 0
46 0 6
56 9 6
SIDE POINTS
10 20 2 3 0
20 56 12 9 3
46 56 2 3 6
10 46 12 0 3
The number of nodes on either side of the midnode are equal, but the spacing of the nodes will only be equal if the midnode happens to bisect the side.
39
Chapter 3 LUSAS Data Input
Example 3. Node Coordinates Quadrilateral Spacing
Y
14
15
16 (7.0, 7.0)
13 (4.0, 5.0)
12
11
9
10
8
5
6
7
3
1 (1.0, 1.0)
2
4 (10.0, 1.0)
X
NODE COORDINATES
QUADRILATERAL SPACING
1 1 1
4 10 1
13 4 5
16 7 7
SIDE POINTS
1 4 1
1 13 4
13 16 1
4 16 4
40
Nodal Coordinates
Copying Nodes
The data section COPY NODES copies the coordinates of a series of nodes to another series of nodes.
COPY NODES N1 N1 last
N1 diff
TO N2 N2 last
N2 diff
N1 N1last N1diff The first node, last node and difference between nodes of the series of node coordinates to be copied.
N2 N2last N2diff The first node, last node and difference between nodes of the recipient series of nodes.
Notes
The coordinates of the first series of nodes must be specified prior to the use of this command.
1. Any node coordinates in the second series of nodes which were previously specified will be overwritten.
2. The number of nodes in both series must be equal.
3. This command could, for example, be used in LOCAL COORDINATES to copy a repetitive pattern of nodes to a new position and orientation.
Example. Node Coordinates Copying Nodes
Y
7 y
8
6
1 1 x
5
4
3
1 0
1
2
X
NODE COORDINATES
1 1 1
2 2 1
41
Chapter 3 LUSAS Data Input
3 2 2
4 1 2
10 4 2
11 6 3
LOCAL CARTESIAN COORDINATES 10 11
COPY NODES 1 4 1 TO 5 8 1
GLOBAL CARTESIAN COORDINATES
Renumbering Nodes
The data section RENUMBER NODES renumbers a series of node numbers with a new series of node numbers.
RENUMBER NODES N1 N1 last
N1 diff
TO N2 N2 last
N2 diff
N1 N1last N1diff The first node, last node and difference between nodes of the series of node coordinates to be renumbered.
N2 N2last N2diff The first node, last node and difference between nodes of the recipient series of nodes.
Notes
1. The node coordinates of the series of nodes to be renumbered must be specified prior to the use of this command.
2. Any node coordinates of the series of new nodes which were previously specified will be overwritten.
3. The number of nodes in both series must be equal.
Deleting Nodes
The data section DELETE NODES deletes a series of node coordinates from the
LUSAS database.
DELETE NODES N N last
N diff
N Nlast Ndiff
The first node, last node and difference between nodes of the series of node coordinates to be deleted.
Note
1. If a node for deletion has not been previously specified, a warning message will be output.
Example. Node Coordinates Deleting Nodes
DELETE NODES 7 9 2
42
Geometric Properties
DELETE NODES 17 19 2
2 1 2 2 2 3
1 6 1 7 1 8
1 1 1 2 1 3
2 4
1 9
2 5
2 0
1 4 1 5
6 7 8 9 1 0
1 2 3 4 5
Geometric Properties
The data section GEOMETRIC PROPERTIES is used to define the geometric property values for the specified element type. Not all elements will require the input of geometric properties; for example, the geometric properties for a membrane element will be the element thickness at each node, whilst there is no equivalent property for the solid elements. The LUSAS Element Reference Manual should be consulted for geometric property details of each element type.
GEOMETRIC PROPERTIES are assigned to a series of elements using the
GEOMETRIC ASSIGNMENTS data section.
type GEOMETRIC PROPERTIES [CONSTANT] [nxs] [TITLE title] igmp < G i
> i=1,n
type
The element type identifier as given in the description of each element.
Refer to the LUSAS Element Reference Manual.
CONSTANT Specifies that the GEOMETRIC PROPERTIES are the same for all nodes
nxs
igmp on the element (see Notes).
The number of quadrilateral crosssections defining the total crosssection
(used for beam elements, see Notes).
The geometric property reference number (see Geometric Assignments).
43
Chapter 3 LUSAS Data Input
Gi
The geometric property values for the element type specified, see element descriptions in the LUSAS Element Reference Manual for definition of values.
Number of geometric properties to be input.
n
Notes
1. Some element types in LUSAS do not require geometric property input, in which case this section should be omitted.
2. If an element is repeated, the new geometric properties overwrite the previous values for that element and an informative message is printed in the output file.
3. When the CONSTANT parameter is used, the geometric properties for only 1 node need be defined and the others are assumed to be the same.
4. The parameter nxs can only be utilised with beam elements that require quadrilateral crosssections to be defined via the local coordinates: BMX3 element in 2D; BXS4 and BXL4 elements in 3D. The maximum number allowed for parameter nxs is 2000 (approximately 200 cross section geometries).
5. For compatibility with previous versions of LUSAS, prior to LUSAS 12, geometric properties may still be associated with elements directly using the element first, last, inc facility. To use this approach Option 117 must now be set.
The CONSTANT and nxs parameters cannot be utilised with this approach.
Examples of Geometric Properties
Input for 3D problem comprising thin beam elements with and without quadrilateral crosssections (see LUSAS Element Reference Manual for definition of values):
Example 1. Geometric Properties Without Quadrilateral CrossSections
y x
1
10
Properties defined for each node:
BS3 GEOMETRIC PROPERTIES
44
10 z
Geometric Properties
11 100.0 833.33 1666.66 0.0 0.0 0.0 ...
100.0 833.33 1666.66 0.0 0.0 0.0 ...
100.0 833.33 1666.66 0.0 0.0 0.0
Properties defined constant for all nodes:
BS3 GEOMETRIC PROPERTIES CONSTANT
12 100.0 833.33 1666.66 0.0 0.0 0.0
Example 2. Geometric Properties With Quadrilateral CrossSections
Cross section defined at each node. Input four y,z pairs at each node followed by the number of integration points in the local y and z directions respectively.
BXL4 GEOMETRIC PROPERTIES
21 0.25 0.125 0.5 0.125 0.5 0.125 0.25 0.125
0.25 0.125 0.5 0.125 0.5 0.125 0.25 0.125
0.25 0.125 0.5 0.125 0.5 0.125 0.25 0.125 3 8
Cross section defined constant for all nodes. Input four y,z pairs followed by the number of integration points in the local y and z directions respectively.
BXL4 GEOMETRIC PROPERTIES CONSTANT
21 0.25 0.125 0.5 0.125 0.5 0.125 0.25 0.125 3 8
Cross section defined as two rectangles constant for all nodes. Input four y,z pairs followed by the number of integration points in the local y and z directions respectively for each quadrilateral in the section.
BXL4 GEOMETRIC PROPERTIES CONSTANT 2
21 0.25 0.125 0.5 0.125 0.5 0.0 0.25 0.0 3 4
0.25 0.0 0.5 0.0 0.5 0.125 0.25 0.125 3 4
45
Chapter 3 LUSAS Data Input
y
0.125
4 x
1
4
2
3
2
3
0.125
z
1
1
0.125
2
0.125
Composite Geometry
The data section COMPOSITE GEOMETRY defines the thicknesses of layers used to laminate a composite material. The number of layers defined in this data section must be the same as the number of layers used in the accompanying COMPOSITE
MATERIAL section. The data is input in tabular form where rows relate to layers and columns to element nodes. The layup sequence is always defined sequentially from the lower to upper surface of the element. COMPOSITE GEOMETRY and COMPOSITE
MATERIALS are assigned to elements through the COMPOSITE ASSIGNMENT data section.
COMPOSITE GEOMETRY [TITLE title]
TABLE icgp t1
1
[< t1 i
> i=2,nnode
]
.. tnlayr
1
[< tnlayr i
> i=2,nnode
]
icgp
Composite geometry set number.
tji
Thickness of layer j at node i (see Notes).
nlayr
Total number of layers.
nnode
Number of element nodes.
Notes
1. Node order is defined by element topology. If the layer thickness is the same at each node then only the thickness at node 1 need be defined.
46
Geometric Assignments
2. The layer thickness may be specified as a ratio of the total thickness defined under
GEOMETRIC PROPERTIES for semiloof shells or of the depth defined by the element topology for composite solids.
Geometric Assignments
The data section GEOMETRIC ASSIGNMENTS is used to assign defined geometric property sets to single, groups or sequences of elements.
GEOMETRIC ASSIGNMENTS [TITLE title]
{L L last
L diff
 G igroup} igmp [igmpv]
L L last
L diff
The first, last and difference between elements with the same geometric assignment.
igmp
The geometric property reference number (see Geometric Properties)
igmpv
The varying geometric property reference number if it is defined in the
LUSAS Modeller preprocessing model. This number is saved in the
LUSAS Modeller results file for use in postprocessing.
G
A command word which must be typed to use element groups.
igroup
The element group reference number (see Defining Data Groups).
Example. Geometric Assignments
Nodal thicknesses for a single curved shell element (QSL8) with 8 nodes:
QSL8 GEOMETRIC PROPERTIES
2 2.5 2.5 2.5 3.0 3.5 3.5 3.5 3.0
GEOMETRIC ASSIGNMENTS
1 0 0 2
Material Properties
Every element declared in the model discretisation must be assigned a material property. Material property definitions may be classified into one of the following groups:
Linear Material Properties
Matrix Properties
Joint Material Properties
Mass Properties
Nonlinear Material Properties
Field Material Properties
Composite Material Properties
47
Chapter 3 LUSAS Data Input
Each set of data specified under MATERIAL PROPERTIES must have a unique material identification number associated with it. This allows a group of elements to be assigned a set of material properties under MATERIAL ASSIGNMENTS.
Material properties specified under MATERIAL PROPERTIES can be combined with the PLASTIC DEFINITION, VISCOUS DEFINITION and/or DAMAGE
PROPERTIES definitions via the MATERIAL ASSIGNMENTS data chapter.
Temperature dependent material properties may be input for both field and structural elements. In this case the TABLE command must directly follow the particular material properties command. Lines of data listing the material properties at particular reference temperatures are then input.
The following restrictions apply to the use of the temperature dependent material properties:
Limited to continuum models (von Mises, Tresca, MohrCoulomb, Drucker
Prager), i.e., not available for stress resultant model
Limited to formulations based on total strains (geometric linearity and Total
Lagrangian or Corotational geometric nonlinearity)
Hardening modulus values are not temperature dependent.
Notes
1. Superfluous properties or rigidities for elements not present in a structure may be specified.
2. For a more detailed description of each constitutive model refer to the LUSAS
Theory Manual.
3. The LUSAS Element Reference Manual defines the material properties that are applicable for each of the element types.
4. For compatibility with previous versions of LUSAS, material properties may still be associated with elements directly using the element first/last/inc facility. To use this approach Option 118 and/or 146 must be set.
Linear Material Properties
The following linear elastic material models are available:
Isotropic
Orthotropic Plane Stress
Orthotropic Plane Strain
Orthotropic Thick
Orthotropic Axisymmetric
Orthotropic Solid
48
Linear Material Properties
Anisotropic
Rigidity specification
Linear Isotropic Model
The data section MATERIAL PROPERTIES is used to define the material properties for linear elastic isotropic materials.
MATERIAL PROPERTIES [TITLE title] imat E
[ a
r
b r
T]
imat
E
ar
br
T
The material property identification number
Young‟s modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Reference temperature
Linear Orthotropic Plane Stress Model
The data section MATERIAL PROPERTIES ORTHOTROPIC is used to define the material properties for linear orthotropic plane stress materials.
MATERIAL PROPERTIES ORTHOTROPIC imat E x
E y
G xy
xy
[
x
y
xy
a r
b r
T]
imat
The material property identification number
Ex,Ey
Young‟s modulus values
Gxy
xy
Shear modulus
Poisson‟s ratio
Angle of orthotropy in degrees relative to the reference axis (see Notes).
Mass density
x, y, xy Coefficients of thermal expansion
ar
Mass Rayleigh damping constant
br
T
Notes
Stiffness Rayleigh damping constant
Reference temperature
1. Subscripts refer to the element reference axes, where reference axes may be local or global (see Local Axes in the LUSAS Element Reference Manual for the proposed element type). If q (about z) is set to zero, the reference axes are used for defining material properties.
49
Chapter 3 LUSAS Data Input
2. When using MATERIAL PROPERTIES ORTHOTROPIC care must be taken to ensure that all properties are input to sufficient numerical accuracy. Failure to do this may result in erroneous answers.
Linear Orthotropic Plane Strain Model
The data section MATERIAL PROPERTIES ORTHOTROPIC PLANE STRAIN is used to define the material properties for linear orthotropic plane strain materials.
MATERIAL PROPERTIES ORTHOTROPIC PLANE STRAIN imat E x
E y
E z
G xy
xy
yz
xz
[
x
y
xy
z
a r
b r
T]
imat
The material property identification number
Ex,Ey,Ez Young‟s modulus values
Gxy
Shear modulus
xy,yz,xz Poisson‟s ratios
Angle of orthotropy in degrees relative to the reference axis (see Notes).
Mass density
x,y,xy,z
Coefficients of thermal expansion
ar
Mass Rayleigh damping constant
br
T
Notes
Stiffness Rayleigh damping constant
Reference temperature
1. Subscripts refer to the element reference axes, where reference axes may be local or global (see Local Axes in the LUSAS Element Reference Manual for the proposed element type). If q (about z) is set to zero, the reference axes are used for defining material properties.
2. When using MATERIAL PROPERTIES ORTHOTROPIC care must be taken to ensure that all properties are input to sufficient numerical accuracy. Failure to do this may result in erroneous answers.
Linear Orthotropic Thick Model
The data section MATERIAL PROPERTIES ORTHOTROPIC THICK is used to define the material properties for linear orthotropic thick materials.
MATERIAL PROPERTIES ORTHOTROPIC THICK imat E x
E y
G xy
xy
G xz
G yz
[
x
y
xy
xz
yz
a r
b r
T]
imat
The material property identification number
Ex,Ey
Young‟s modulus values
Gxy,Gxz,Gyz Shear modulus values
xy
Poisson‟s ratio
50
Linear Material Properties
Angle of orthotropy in degrees relative to the reference axis (see Notes).
Mass density
x,y,
xy,xz,yz Coefficients of thermal expansion
ar
Mass Rayleigh damping constant
br
T
Notes
Stiffness Rayleigh damping constant
Reference temperature
1. Subscripts refer to the element reference axes, where reference axes may be local or global (see Local Axes in the LUSAS Element Reference Manual for the proposed element type). If q (about z) is set to zero, the reference axes are used for defining material properties.
2. When using MATERIAL PROPERTIES ORTHOTROPIC care must be taken to ensure that all properties are input to sufficient numerical accuracy. Failure to do this may result in erroneous answers.
Linear Orthotropic Axisymmetric Model
The data section MATERIAL PROPERTIES ORTHOTROPIC AXISYMMETRIC is used to define the material properties for linear orthotropic axisymmetric materials.
MATERIAL PROPERTIES ORTHOTROPIC AXISYMMETRIC imat E x
E y
E z
G xy
xy
yz
xz
[
x
y
xy
z
a r
b r
T]
imat
The material property identification number
Ex,Ey,Ez Young‟s modulus values
Gxy
Shear modulus
xy,yz,xz Poisson‟s ratios
Angle of orthotropy in degrees relative to the reference axis (see Notes).
Mass density
x,y,xy,z
Coefficients of thermal expansion
ar
Mass Rayleigh damping constant
br
T
Notes
Stiffness Rayleigh damping constant
Reference temperature
1. Subscripts refer to the element reference axes, where reference axes may be local or global (see Local Axes in the LUSAS Element Reference Manual for the proposed element type). If q (about z) is set to zero, the reference axes are used for defining material properties.
51
Chapter 3 LUSAS Data Input
2. When using MATERIAL PROPERTIES ORTHOTROPIC care must be taken to ensure that all properties are input to sufficient numerical accuracy. Failure to do this may result in erroneous answers.
Linear Orthotropic Solid Model
The data section MATERIAL PROPERTIES ORTHOTROPIC SOLID is used to define the material properties for linear orthotropic solid materials.
MATERIAL PROPERTIES ORTHOTROPIC SOLID imat nset E x
E y
E z
G xy
G yz
G xz
xy
yz
yz
xz
a r
b r
] T xz
[
x
y
z
xy
imat
nset
The material property identification number
The CARTESIAN SET number used to define the local axis directions.
Ex,Ey,Ez Young‟s modulus values
Gxy,Gyz,Gxz Shear modulus values
xy,yz,xz Poisson‟s ratios
Mass density
x,y,z,
xy,yz,xz Coefficients of thermal expansion
ar
br
T
Notes
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Reference temperature
1. Subscripts refer to the element reference axes, where reference axes may be local or global (see Local Axes in the LUSAS Element Reference Manual for the proposed element type). For the solid model, the orthotropy is defined by the
CARTESIAN SET command. If nset is set to zero, the orthotropy coincides with the reference axes.
2. When using MATERIAL PROPERTIES ORTHOTROPIC care must be taken to ensure that all properties are input to sufficient numerical accuracy. Failure to do this may result in erroneous answers.
Linear Anisotropic Model
The data section MATERIAL PROPERTIES ANISOTROPIC is used to define arbitrary constitutive equations relating stress to strain. The material modulus matrix is input on a component by component basis. Note that symmetry is assumed so that only the upper triangle of the matrix is required. The matrix is defined column by column.
MATERIAL PROPERTIES ANISOTROPIC {n  SOLID}
52
Linear Material Properties
imat
ar
br
T
nset
i
Di
imat {
a
r
b r
T
< D i
> i=1,n(n+1)/2
nset a
r
b r
T} <
i
> i=1,n
n
Notes
The material property identification number
Mass density
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Reference temperature
Angle of anisotropy (degrees) relative to the element reference axes (see
Notes)
The CARTESIAN SET number used to define the axes of anisotropy
(required for ANISOTROPIC SOLID only).
Coefficients of thermal expansion
Values in upper triangular half of modulus matrix.
The number of stress/strain components for element (=6 for SOLID)
1. The element reference axes may be local or global (see Local Axes in the LUSAS
Element Reference Manual for the proposed element type). If nset or q is set to zero, the anisotropy coincides with the reference axes.
2. The upper triangle components of the modulus matrix only are entered (the components are entered column by column), and:
Di The m components of the upper triangle of the modulus matrix.
m The number of components of the modulus matrix, where m may be computed from m=n(n+1)/2
Linear Rigidity Model
The data section RIGIDITIES is used to define the inplane and bending rigidities from prior explicit integration through the element thickness.
imat
n
ar
br
T
i
Di
RIGIDITIES n imat
a
r
b r
T
<
i
> i=1,n
< D i
> i=1,n(n+1)/2
The material property identification number
The number of stress/strain resultants for the element
Mass density
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Reference temperature
Angle of orthotropy relative to the reference axis (degrees)
Coefficients of thermal expansion
The values in the upper triangular half of the rigidity matrix
53
Chapter 3 LUSAS Data Input
Note
1. The element reference axes may be local or global (see Local Axes in the LUSAS
Element Reference Manual for the proposed element type). If q is set to zero, the anisotropy coincides with the reference axes.
Example 1. Membrane Behaviour
RIGIDITIES 3 imat,
, a , b , T, q, , D D
T
S
R
N
N
N x y xy
V
U
W
M
MM
L
N
D
1
D
2
D
D
2
D
3
D
D
4
D
5
D
4
5
6
PP
O
Q
P
T
S
R
S
R
T
x y xy
V
U
W
T
S
R
xo yo xyo
V
U
W
W
V
U
R
N
S
N
T
N xo yo xyo
V
U
W where:
N
D
e are the membrane stress resultants (force per unit width). membrane rigidities. membrane strains. and for isotropic behaviour, where t is the thickness:
D
1
D
3
D
4
D
5
1
0
t
2
D
2
1
t
2
D
6
t b g
The initial strains due to a temperature rise T are:
ot
R
T
S
xo yo xyo
W
V
U
R
T
T
S
1
2
3
W
V
U
Example 2. Thin Plate Flexural Behaviour
RIGIDITIES 3 imat,
, a , b , T, q, , D D
T
S
R
M
M
M x y xy
V
U
W
M
MM
L
N
D
1
D
2
D
D
2
D
3
D
D
4
D
5
D
4
5
6
PP
O
Q
P
T
S
R
S
R
T
x
y
xy
V
U
W
T
S
R
xo
yo
xyo
V
U
W
V
U
W
R
M
S
M
T
M xo yo xyo
V
U
W
54
Linear Material Properties
where:
M
D
Y are the flexural stress resultants (moments per unit width). flexural rigidities. flexural strains given by:
T
S
R
x
y
xy
V
U
W
=
S
R




T



2
x
2
2 w
y
2
w
2
2 w


W


U
V and for an isotropic plate for example, where t is the thickness:
D
1
D
3
Et
3
2
)
D
2
= D5 = 0
The initial strains due to a temperature rise T are:
ot
T
S
R
xo
yo
xyo
V
U
W
T
z T
S
R
1
2
3
V
U
W
Et
3
2
)
D
6
Et
3
24 1
)
D4
Example 3. Thick Plate Flexural Behaviour
RIGIDITIES 5

T
S
R


S
M
M
M xz
S y xy yz
imat,
, a , b , T, q, , D D x

W

V

U
N
MM
MM
L
MM
D
1
D
2
D
4
D
D
2
D
3
D
5
D
D
4
D
5
D
6
D
D
7
D
8
D
9
D
D
11
D
12
D
13
D
7
8
9
10
14
D
11
D
12
D
13
D
14
D
15
PP
Q
PP
PP
O




R
S
T


R
S

T
x y xy
xz
yz

W


U
V

T


R
S
xo
yo
xyo
xzo
yzo

W



U
V

W

U
V


T

R
S

S
M
M
M
S xo yo xyo xzo yzo

W


U
V where:
M are the flexural stress resultants (moments per unit width).
55
Chapter 3 LUSAS Data Input
S
D
Y shear stress resultants (shear force per unit width). flexural and shear rigidities. flexural strains given by:
T
S
R
x
y
xy
V
U
W

S

R


T
y
2
2 w
x
2
2 w
2
2 w


W


U
V
G
T
RS
shear strains given by: xz yz
UV
W
R
S
T
w x w y
u z v z
V
U
W and for an isotropic plate for example:
D
10
D
15
Et
) k
D
7
D
8
D
9
D
11
D
12
D
13
D
14
0 where t is the plate thickness and k is a factor taken as 1.2 which provides the correct shear strain energy when the shear strain is assumed constant through the plate thickness. D1 to D6 are the same as defined for the thin plate flexural behaviour (see
Example 2. Thin Plate Flexural Behaviour).
The initial strains due to a temperature rise T are:
T
RS
ot
ot
UV
W

T


R
S
xo
yo
xyo
xzo
yzo

W


U
V
T
z
S
R
1
2
3

U
V

W



T

R
0
T
S
0
0
4
5

W


U
V
Example 4. Shell Behaviour
RIGIDITIES 6
56
Matrix Properties
S

R



N
N
N
M
M
T
M x y
imat,
, a , b , T, q, , D D xy x y xy


W

V

U
MM
L
M
MM
N
MM
D
1
D
D
D
2
4
7
D
11
D
16
D
2
D
3
D
5
D
8
D
12
D
17
D
4
D
7
D
5
D
8
D
6
D
9
D
9
D
10
D
13
D
14
D
18
D
19
D
11
D
12
D
13
D
14
D
15
D
20
D
16
D
17
D
18
D
19
D
20
D
21
Q
O
P



R
S
PP
PP
PP

T


T

R
S

x
y xy
x
y
xy


W


U
V

R
S



T
xo
yo xyo
xo
yo
xyo

W



U
V


W

U
V




T
M
M

R
S
N
N
N
M xo yo xyo xo yo xyo


W


U
V where:
N
M
D
e are the membrane stress resultants (forces per unit width). are the flexural stress resultants (moments per unit width). flexural and shear rigidities. membrane strains.
G flexural strains.
The initial strains due to a temperature rise T are:
ot
ot
xo yo xyo xo
yo xyo
1
T
0
0
dt
0 dz
5
Matrix Properties
The data section MATRIX PROPERTIES is used to explicitly define the linear properties of the stiffness, mass and damping matrices for joint elements in the local coordinate system.
MATRIX PROPERTIES {STIFFNESS  MASS  DAMPING} [N] imat {< K i
> i=1,m
 < M i
> i=1,m
 < C i
> i=1,m
}
imat
Ki
Mi
Ci
The material property identification number
The values in upper triangular half of local element stiffness matrix.
The values in upper triangular half of local element mass matrix.
The values in upper triangular half of local element damping matrix.
57
Chapter 3 LUSAS Data Input
N
m
Size of matrix (total number of freedoms for element in question). The default value is given by twice the maximum number of freedoms at a node for the structure in question.
Number of components of the matrix where m is calculated from
m=N(N+1)/2
Notes
1. Either the stiffness, mass or damping matrix can be specified for an element. If more than one matrix is specified the last matrix overwrites all previous matrices.
To specify more than one matrix property overlay the number of elements required.
2. The force/displacement relationship is defined as:
P = T
T
K T a where:
P
T
K a
The global nodal forces
A transformation matrix relating local freedoms to global
The local element stiffness matrix stored in upper triangular form.
The global element freedoms (displacements).
Joint Material Properties
Joint material models are used to define the material properties for linear and nonlinear joint models. Ten types of joint model are available:
Standard Linear Joint Model
General Linear Joint Model
Standard Nonlinear ElastoPlastic Joint Model
General Nonlinear ElastoPlastic Joint Model
Nonlinear Joint Model For Smooth Contact
Nonlinear Joint Model For Frictional Contact
Viscoelastic Dampers
Kelvin
Four parameter solid
Hysteretic Damper For LeadRubber Bearing
Hysteretic Damper For Friction Pendulum System
UserSupplied Nonlinear Joint Properties
58
Joint Material Properties
Standard Linear Joint Model
Joint type: Spring stiffness only
The JOINT PROPERTIES data section defines linear spring stiffnesses for joints.
JOINT PROPERTIES [N] imat < K i
> i=1,N
imat
K
The material property identification number
Elastic spring stiffness corresponding to each local freedom. These local directions are defined for each joint element in the LUSAS Element
Reference Manual.
Number of springs for joint element.
N
Example. Joint Properties
JPH3 ELEMENT TOPOLOGY
2 2 3 4
JOINT PROPERTIES
1 51.2 48.9 23.1
MATERIAL ASSIGNMENT
2 0 0 1
General Linear Joint Model
Joint type: General properties
The JOINT PROPERTIES GENERAL data section defines the full joint properties of spring stiffness, mass, coefficient of linear expansion and damping factor.
JOINT PROPERTIES GENERAL [N] imat < K i
M i
C i
i
a ri
b ri
> i=1,N
[mcode]
imat
Material property identification number
K
M
Elastic spring stiffness corresponding to (i)th local freedom.
Mass corresponding to (i)th local freedom.
C
a
Viscocity coefficient  damping corresponding to the (i)th local freedom
Coefficient of thermal expansion corresponding to (i)th local freedom.
Mass Rayleigh damping constant corresponding to (i)th local freedom
b
Stiffness Rayleigh damping constant corresponding to (i)th local freedom
mcode
An integer number which determines the position of a mass or masses.
= 0 for mass between nodes (default)
= 1 for mass at 1st node.
= 2 for mass at 2nd node.
59
Chapter 3 LUSAS Data Input
N
Notes
The number of springs for joint element.
1. In order to input the damping values Ci OPTION 324 must be specified.
2. Modeller will automatically set OPTION 324 .
3. If all the Ci input values are specified as zero the Rayleigh damping parameters will be used to form the element damping matrix.
Standard Nonlinear ElastoPlastic Joint Model
Joint type: Elastoplastic (tension and compression equal)
The JOINT PROPERTIES NONLINEAR 31 data section defines the material properties for the standard elastoplastic joint model. The model incorporates elastoplasticity with isotropic hardening. Equal tension and compression yield conditions are assumed.
JOINT PROPERTIES NONLINEAR 31 [N] imat < K i
M i
i
a ri
b ri
F yldi
i
> i=1,N
[mcode]
N
imat
K
M
a
b
Material property identification number
Elastic spring stiffness corresponding to (i)th local freedom.
Mass corresponding to (i)th local freedom.
Coefficient of thermal expansion corresponding to (i)th local freedom.
Mass Rayleigh damping constant corresponding to (i)th local freedom
Stiffness Rayleigh damping constant corresponding to (i)th local freedom
F yld
Yield force
Hardening stiffness
mcode
An integer number which determines the position of a mass or masses.
= 0 for mass between nodes (default)
= 1 for mass at 1st node.
= 2 for mass at 2nd node.
The number of springs for joint element.
60
Joint Material Properties
+ : tension
 : compression
F
+Yield force
+
strain hardening stiffness
K  elastic spring stiffness
Yield force
=
2 
1

strain hardening stiffness
Standard Nonlinear ElastoPlastic Joint Model (Model 31)
General Nonlinear ElastoPlastic Joint Model
Joint type: Elastoplastic (tension and compression unequal)
The JOINT PROPERTIES NONLINEAR 32 data section defines the material properties for the general elastoplastic joint model. The model incorporates elastoplasticity with isotropic hardening. Unequal tension and compression yield conditions are assumed.
JOINT PROPERTIES NONLINEAR 32 [N] imat < K i
M i
i
a ri
b ri
+F yldi
+
i
F yldi

i
> i=1,N
[mcode]
imat
K
M
Material property identification number
Elastic spring stiffness corresponding to the (i)th local freedom.
Mass corresponding to (i)th local freedom.
Coefficient of thermal expansion corresponding to the (i)th local freedom.
a
b
Mass Rayleigh damping constant corresponding to (i)th local freedom
Stiffness Rayleigh damping constant corresponding to (i)th local freedom
+F yld
Tensile yield force
+
Tensile strain hardening stiffness
F yld
Compressive yield force (value is always positive)

Compressive strain hardening stiffness (value is always positive)
61
Chapter 3 LUSAS Data Input
mcode
An integer number which determines the position of a mass or masses.
= 0 for mass between nodes (default)
= 1 for mass at 1st node.
N
= 2 for mass at 2nd node
The number of springs for joint element.
F
+ : tension
 : compression
+
strain hardening stiffness
Tensile Yield Force
K  elastic spring stiffness
=
2 
1
Compressive Yield force

strain hardening stiffness
General Nonlinear ElastoPlastic Joint Model (Model 32)
Nonlinear Joint Model For Smooth Contact
The JOINT PROPERTIES NONLINEAR 33 data section defines the material properties for the nonlinear joint model for smooth contact with an initial gap.
JOINT PROPERTIES NONLINEAR 33 [N] imat < K ci
M i
i
a ri
b ri
F yldi
i
gap i
> i=1,N
[mcode]
imat
The material property identification number
Kci
Mi
i
The contact spring stiffness corresponding to (i)th local freedom.
The mass corresponding to (i)th local freedom.
The coefficient of linear expansion corresponding to (i)th local freedom.
ari
Mass Rayleigh damping constant corresponding to (i)th local freedom
bri
Stiffness Rayleigh damping constant corresponding to (i)th local freedom
Fyldi
Liftoff force
62
Joint Material Properties
i
gapi
Liftoff stiffness
The initial gap (see Notes)
mcode
An integer number which determines the position of a mass or masses.
N
= 0 for mass between nodes (default)
= 1 for mass at 1st node.
= 2 for mass at 2nd node
The number of springs for joint element.
F
 liftoff stiffness
Liftoff force
Gap
=
2 
1
=
2 
1
K  contact spring stiffness
Nonlinear Joint Model for Smooth Contact (Model 33)
Note
1. If an initial gap is used in a spring, then the positive local axis for this spring must go from node 1 to 2. If nodes 1 and 2 are coincident the relative displacement of the nodes in a local direction (d2 d1) must be negative to close an initial gap in that direction.
Nonlinear Joint Model For Frictional Contact
Joint type: Friction contact
The JOINT PROPERTIES NONLINEAR 34 data section defines the material properties for the nonlinear joint model for frictional contact with an initial gap.
imat
K
M
JOINT PROPERTIES NONLINEAR 34 [N] imat < K ci
M i
i
a ri
b ri
> i=1,N
gap [mcode]
Material property identification number
Contact spring stiffness corresponding to (i)th local freedom.
Mass corresponding to (i)th local freedom.
63
Chapter 3 LUSAS Data Input
a
b
Coefficient of thermal expansion corresponding to (i)th local freedom.
Mass Rayleigh damping constant corresponding to (i)th local freedom
Stiffness Rayleigh damping constant corresponding to (i)th local
gap freedom
Coefficient of friction.
Initial gap in x The initial gap in the local xdirection.
mcode
An integer number which determines the position of a mass or masses.
= 0 for mass between nodes (default)
N
Notes
= 1 for mass at 1st node.
= 2 for mass at 2nd node
The number of springs for joint element.
1. If an initial gap is used in a spring, then the positive local x axis for this spring must go from node 1 to 2. If nodes 1 and 2 are coincident the relative displacement of the nodes in the local x direction (dx2 dx1) must be negative to close an initial gap.
Fx
Fy or Fz
Fo
Gap
xx =
x2 
x1
Kcy or Kcz  contact spring stiffness
xy =
y2 
y1 or
xz =
z2 
z1
K  contact spring stiffness
Fo
 coeff. of friction
Fo
Fx
Nonlinear Joint Model for Frictional Contact (Model 34)
64
Joint Material Properties
ViscoElastic Dampers
Joint type: Viscous damper – Kelvin
Joint type: Viscous damper  Four parameter solid
The JOINT PROPERTIES NONLINEAR 35 data section defines the material properties for a general preloaded viscoelastic damper joint model. The model consists of three springs and a dashpot in the socalled fourparameter solid model arrangement.
Selectively setting the appropriate stiffnesses to zero allows the model to degenerate to a Kelvin (K2=0, K3=0) or Maxwell (K1=0, K2 or K3=0) unit.
JOINT PROPERTIES NONLINEAR 35 [N] imat < K1 i
M i
C i
i
v i
Fp i
K2 i
K3 i
> i=1,N
[mcode]
N
imat
K1
M
C
Fp
K2
Material property identification number
Spring stiffness corresponding to (i)th local freedom (see below).
Mass corresponding to (i)th local freedom.
Viscosity coefficient Damping corresponding to the (i)th local freedom
Coefficient of thermal expansion corresponding to (i)th local freedom.
Velocity exponent corresponding to (i)th local freedom
Preload force corresponding to (i)th local freedom
Spring stiffness corresponding to (i)th local freedom in parallel with damper (see below).
K3
Spring stiffness corresponding to (i)th local freedom in series with damper (see below).
mcode
An integer number which determines the position of a mass or masses.
= 0 for mass between nodes (default)
= 1 for mass at 1st node.
= 2 for mass at 2nd node.
The number of springs for joint element.
K
3
C
F
K
1
K
2
F
Four parameter solid model for viscoelasticity (Model 35)
65
Chapter 3 LUSAS Data Input
Notes
1. Stiffnesses, mass and preload force can be set to zero in order to create a viscous damper only.
2. The preload force represents the force that must be exceeded to cause movement of the damper piston (typically the initial pressure in hydraulic fluid).
3. If a Kelvin unit is defined the damping force is computed from
F
Cv
v
.
4. The viscosity coefficient is typically evaluated from
C
/
v
where
Fn
and
Vn
are the maximum force and velocity that are expected to occur in the damper.
LeadRubber Bearing with Hysteretic damping
Joint type: Lead rubber bearing
Leadrubber bearings (LRBs) are generally constructed of lowdamping natural rubber with a preformed central hole, into which a lead core is pressfitted. The central lead core provides an additional means of energy dissipation and the energy absorbed by the core reduces the lateral displacement of the isolator. This system provides the combined features of vertical load support, horizontal flexibility, restoring force and damping in a single unit.
Under lateral deformation, the lead core deforms in almost pure shear, yields at low level of stress (approximately 8 to 10 MPa in shear at normal temperature), and produces hysteretic behavior that is stable over many cycles. Unlike mild steel, lead recrystallizes at normal temperature (about 20°C), so that repeated yielding does not cause fatigue failure. LRBs generally exhibit characteristic strength that ensures rigidity under service loads.
JOINT PROPERTIES NONLINEAR 36 [N] imat
K i
M i
C
i
a ri
b ri
F yldi
i
A s
i=1,N
[mcode] imat
Material property identification number
K i
M i
Elastic spring stiffness corresponding to the ith local freedom
Mass corresponding to the ith local freedom
C
i a ri b ri
Viscosity coefficient Damping corresponding to the (i)th local freedom
Coefficient of thermal expansion corresponding to the ith local freedom
Mass Rayleigh damping constant corresponding to the ith local freedom
Stiffness Rayleigh damping constant corresponding to the ith local
F
i yldi
freedom
Yield force (only applicable to the 1 st
local freedom in 2D and the 1 st
and
2 nd
local freedoms in 3D)
Postyield stiffness (only applicable to the 1 st
1 st
and 2 nd
local freedoms in 3D)
local freedom in 2D and the
66
Joint Material Properties
A
Hysteretic parameter A (only applicable to the 1 st and the 1 st
and 2 nd
local freedoms in 3D)
local freedom in 2D
s
cp
Hysteretic parameter s (see Notes)
Biaxial coupling coefficient used in evolution of hysteretic variables
(only applicable for the 3D case – see Notes)
Hysteretic parameter beta
Hysteretic parameter gamma
mcode
An integer number which determines the position of a mass or masses.
N
=0 for mass between nodes (default) st
=1 for mass at 1
=2 for mass at 2 nd
node
node
Number of springs for joint element
Force
 postyield stiffness
F yld
Lead Core
Rubber
Steel
Plate
Displacement
Lead Rubber Bearing
K  elastic spring stiffness
Schematic LRB and hysteretic behaviour (Model 36)
Notes
1. The input parameters are utilised in the following manner; for the 3D case, the forces in the damper are computed from:
F x
F y
x y
u v
1
1
y x
/K
/K y x
F
F yld yld y x z z y x where the evolution of the hysteretic terms is given by:
y v z x y
A x
z s x x
z z
hysteretic variables bounded by values
A y
z
1
. z z s y y
where, u y
and v y
are displacements when yield occurs. For the 3D uncoupled case
(
=0), the values for s
x
and s
y
are taken as the specified input parameters. For the coupled case (
>0) the values are fixed, s
x
=s
y
=2. z x y
and z y are dimensionless
When working in 2D, the input parameter s
x
should take a value > 1, where it is used to define the following hysteretic term:
67
Chapter 3 LUSAS Data Input
z x
s x
1
Note that the value for the hysteretic coupling parameter,
, must lie within the limits of 0 and 1; a value of 0 leads to fully uncoupled hysteretic equations and a value of 1 fully coupled equations. For more information please consult the LUSAS
Theory Manual.
2. The input parameters F
yld
,
, A, s and the other hysteretic control parameters are only applicable to the joint local x translation in 2D and the local x and y translation in 3D.
3. Liftoff does not occur in this model and the vertical stiffness is taken as the local y direction in 2D and the local z direction in 3D.
4. If all the C i
input values are specified as zero the Rayleigh damping parameters will be used to form the element damping matrix.
Sliding/Frictional Pendulum System with Hysteretic
Damping
Joint type: Friction pendulum system
A friction pendulum system (FPS) bearing consists of a spherical sliding surface and an articulated slider which is faced with a high pressure capacity bearing material. The bearing may be installed as shown below or upside down with the spherical surface facing downwards. Irrespective of the installation method, the behaviour is identical.
JOINT PROPERTIES NONLINEAR 37 [N] imat
K i
M i
C
i
a ri
b ri
μ μ μ max0 i maxp i min i
A s
i
i=1,N
A R
[mcode] imat
K i
M i
C
i a ri b ri
Material property identification number
Elastic spring stiffness corresponding to the ith local freedom
Mass corresponding to the ith local freedom
Viscosity coefficient Damping corresponding to the (i)th local freedom
Coefficient of thermal expansion corresponding to the ith local freedom
Mass Rayleigh damping constant corresponding to the ith local freedom
Stiffness Rayleigh damping constant corresponding to the ith local freedom
μ
Friction coefficient at zero pressure (only applicable to the 1 st
local max0 i freedom in 2D and the 1 st
and 2 nd
local freedoms in 3D).
μ maxp i
Friction coefficient at high pressure (only applicable to the 1 st
local freedom in 2D and the 1 st
and 2 nd
local freedoms in 3D).
68
Joint Material Properties
μ
Friction coefficient at (near) zero velocity (only applicable to the 1 st min i local freedom in 2D and the 1 st
and 2 nd
local freedoms in 3D).
Coefficient of velocity Parameter controlling the variation of the coefficient of friction with velocity (only applicable to the 1 freedom in 2D and the 1 st
and 2 nd
local freedoms in 3D). st
local
A
Pressure coefficient Parameter used to determine the variation of the friction coefficient with pressure (only applicable to the 1 st
local freedom in 2D and the 1 st
and 2 nd
local freedoms in 3D)
Hysteretic parameter A (only applicable to the 1 st
local freedom in 2D and the 1 st
and 2 nd
local freedoms in 3D)
s
Hysteretic parameter s (see Notes)
A c
R
cp
Contact area of FPS
Radius of sliding surface (spherical) Specify R=0 for a flat surface.
Biaxial coupling coefficient Parameter used in evolution of hysteretic variables (only applicable for the 3D case – see Notes)
Hysteretic parameter beta
Hysteretic parameter gamma
mcode
An integer number which determines the position of a mass or masses.
N
=0 for mass between nodes (default)
=1 for mass at 1 st
node
=2 for mass at 2 nd
node
Number of springs for joint element
Force
Bearing Material
Spherical Sliding
Surface
N
Displacement
Friction Pendulum Bearing
FPS layout and schematic representation (Model 37)
Notes
1. The input parameters are utilised in the following manner; for the 3D case, the forces in the FPS element, including the restorative forces, are given by:
69
Chapter 3 LUSAS Data Input
F x
F y
N u
μ Nz x
R
N v
μ Nz y
R where the normal force N is evaluated as follows
N=K w where K z
and w are stiffness and compressive deformation in the contact direction.
The friction coefficient
s
is given by:
μ s
μ max
μ max
μ min
exp
u
where
max
is computed from:
μ max
μ max0
μ max0
μ maxp
and the bearing pressure is given by:
P=N/A c
For the 3D case the evolution of the hysteretic terms is given by:
x y
A x
z s x x
z z
z z
sgn vz
A y
z s y y
where, u y
and v y
are displacements when yield occurs. For the 3D uncoupled case
(
=0), the values for s
x
and s
y
are taken as the specified input parameters. For the coupled case (
>0) the values are fixed, s
x
=s
y
=2. z x and z y are dimensionless hysteretic variables bounded by values
1
.
When working in 2D, the input parameter s
x
should take a value > 1, where it is used to define the following hysteretic term:
1 z x
s x
Note that the value for the hysteretic coupling parameter,
, must lie within the limits of 0 and 1; a value of 0 leads to fully uncoupled hysteretic equations and a value of 1 fully coupled equations. For more information please consult the LUSAS
Theory Manual.
2. The input parameters
max0
,
maxp
,
min
,
,
A, s and the other hysteretic control parameters are only applicable to the joint local x translation in 2D and the local x and y translation in 3D.
3. Liftoff occurs when the local vertical strain (
y
in 2D,
z
in 3D) is greater than zero. If liftoff occurs the vertical stiffness is set to zero and the hysteretic terms are also initialised in readiness for recontact. In a compressive state the vertical stiffness is taken as the input value K y
in 2D and K z
in 3D.
4. If all the C
i
input values are specified as zero the Rayleigh damping parameters will be used to form the element damping matrix.
70
Joint Material Properties
UserSupplied Nonlinear Joint Properties
Joint type: Nonlinear user
The USER joint model facility allows usersupplied joint property subroutines to be used from within LUSAS. This facility provides controlled access to the pre and postsolution constitutive processing and nonlinear state variable output via these usersupplied subroutines.
By default these routines are supplied as empty routines with defined interfaces that are unchangeable. The externally developed code should be placed into these routines which is then linked into the LUSAS system. Source code access is available to these interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised. See Appendix C: Solver User Interface
Routines.
Since user specification of a constitutive model involves the external development of source FORTRAN code, as well as access to LUSAS code, this facility is aimed at the advanced LUSAS user.
The required joint properties input for the usersupplied joint model is completely general. However, the properties M
i
,C i
,
i
,
a ri
,b ri
along with mcode are reserved for LUSAS internal use: you only need to utilise them if other features of the program are required (e.g. dynamic and thermal analyses). The data section JOINT
PROPERTIES NONLINEAR USER is used to define all the joint property parameters for usersupplied joint models.
JOINT PROPERTIES NONLINEAR USER LPTUSR N NPRZS NPRZJ
NSTAT imat
K i
M i
C i
i
a ri
b ri
{u j
} j=1,nprzs6
[mcode] i=1,N
{p k
} k=1,nprzj
LPTUSR
User model number
N
Number of springs for joint element
NPRZS
Total number of joint properties per spring
NPRZJ
Number of properties per joint (common to all springs)
NSTAT
Number of state variables
imat
Material property identification number
K i
M i
C i
Elastic spring stiffness corresponding to the ith local freedom
Mass corresponding to the ith local freedom
Viscocity coefficient Damping coefficient corresponding to the ith local freedom
i a ri b ri
Coefficient of thermal expansion corresponding to the ith local freedom
Mass Rayleigh damping constant corresponding to the ith local freedom
Stiffness Rayleigh damping constant corresponding to the ith local freedom
71
Chapter 3 LUSAS Data Input u j
User defined material properties for individual component directions
P k
User defined joint properties common to all directions
mcode
An integer number which determines the position of a mass or masses.
=0 for mass between nodes (default)
=1 for mass at 1
=2 for mass at 2 st nd
node
node
Notes
1. The total number of joint properties, NPRZ, will be computed from N*NPRZS +
NPRZJ + 1.
2. The number of material properties input must be equal to that specified in the data.
3. When no state variables are required (i.e. when nstat is specified as zero) a warning message will be invoked.
4. The properties M
i
,C i
,
i
,
a ri
,b ri
along with mcode are required by LUSAS in order to perform other types of analyses: for example thermal problems require the coefficients of thermal expansion
i
and a dynamic analysis requires the mass M
i
and possibly damping via C
i
or a
ri
and b
ri
along with mcode.
5. If all the C i
input values are specified as zero the Rayleigh damping parameters will be used to form the element damping matrix.
6. Option 179 can be set for argument verification within the user routines.
Material Properties Mass
The data section MATERIAL PROPERTIES MASS is used to specify the element nodal masses in the local coordinate system for nonstructural mass elements.
MATERIAL PROPERTIES MASS naxes nnode imat mx i
my i
{mz i
} ... mx nnod
my nnod
{mz nnode
}
imat
The material property identification number
naxes
Number of axes in structure (2D or 3D)
nnode
Number of nodes to element
mx i
Mass at node i in local x direction
my i mz i
Notes
Mass at node i in local y direction
Mass at node i in local z direction (only if naxes=3)
1. MATERIAL PROPERTIES MASS must only be assigned to nonstructural mass elements. Only translational masses in the x, y and z directions are available.
Rotational masses are not available.
2. For point elements the nodal (point) mass is input. For line elements the mass per unit length is input. For surface elements the mass per unit area is input.
3. By default nodal masses are defined with respect to local element axes. However, it is also possible to define the mass orientation with respect to any CARTESIAN
SET. This is specified under MATERIAL ASSIGNMENTS.
72
Nonlinear Material Properties
Nonlinear Material Properties
The nonlinear models may be used to model yielding of materials such as metals, concrete, rubber, soils and rocks etc.. The following types of nonlinear material models are available (described in detail in the LUSAS Theory Manual):
Plasticity Models
Plastic Definition (von Mises, Hill, Hoffman)
Optimised Von Mises Model
DruckerPrager Model
Tresca Model
NonAssociative MohrCoulomb Model
Multi Crack Concrete Model
ElastoPlastic Stress Resultant Model
UserSupplied Nonlinear Material Properties
Viscous Definition (Creep, Viscoelasticity)
Damage Model
Composite Matrix Failure Model
Two Phase Material Model
Rubber Model
Volumetric Crushing Model
Concrete Creep Models
CEBFIP Model Code 1990
Chinese Creep Code for Dams
Generic Polymer Model
2D Interface Model / 3D Interface Model
Delamination Model
Resin Cure Model
Shrinkage
A full section (stress resultant) yield criterion is available for some of the shell and beam elements. Other elastoplastic models for Gauss point stress evaluations are applicable to shell, membrane and solid elements. Various yield criteria with isotropic and kinematic hardening are available. Implicit integration of the elastoplastic constitutive equations is also implemented for some of the models. The pressure dependent material models allow for different properties in tension and compression.
In addition to the standard element data output, the following details of the nonlinear material model behaviour are also output (at the Gauss points):
YFUNC
The value of the yield function. zero: stress on the yield surface.
73
Chapter 3 LUSAS Data Input
negative: stress within the yield surface.
CURYS
The value of the equivalent yield stress.
EPSTN
The value of the equivalent plastic strain.
IYLD
The value of the yield flag.
0  elastic
1  plastic
NSTEPS
The number of sub increments used to integrate the elastoplastic strain increment (explicit integration), or the number of NewtonRaphson iterations used to satisfy the elastoplastic constitutive relations (implicit integration).
Plastic Definition
The PLASTIC DEFINITION data chapter allows more flexibility in the way that plastic properties for a nonlinear material can be defined. In particular, the following options may be used to define a hardening curve by specifying the following pairs of values:
the gradient of the curve together with the plastic strain limit for which the gradient applies
the yield stress together with a plastic strain value
the yield stress together with a total strain value
A PLASTIC DEFINITION should be used in conjunction with a linear material property; the linear and nonlinear sets of properties are then assigned to elements using the MATERIAL ASSIGNMENTS or COMPOSITE MATERIAL data chapters. The following linear material property types can be assigned to the same elements as a
PLASTIC DEFINITION data set:
MATERIAL PROPERTIES
MATERIAL PROPERTIES ORTHOTROPIC
MATERIAL PROPERTIES ORTHOTROPIC PLANE STRAIN
MATERIAL PROPERTIES ORTHOTROPIC THICK
MATERIAL PROPERTIES ORTHOTROPIC AXISYMMETRIC
MATERIAL PROPERTIES ORTHOTROPIC SOLID
Note. If an orthotropic linear material is used to define the linear elastic properties, then any accompanying plastic data set must include an orthotropic stress potential.
STRESS POTENTIAL {VON_MISES  HILL  HOFFMAN} ipls [
xx
yy
zz
xy
yz
zx
T 
xy
yz
xz
T] xx t
xx c
yy t
yy c
zz t
zz c
YIELD STRESS [n
] ipls
yo t
[
yo c
] [T]
74
Nonlinear Material Properties
HARDENING CURVE [HARDENING_GRADIENT  PLASTIC_STRAIN 
TOTAL_STRAIN] N t
[N c
] ipls < H i t
S i t
> i=1,Nt
[< H i c
S i c
> i=1,Nc
] [T]
HEAT FRACTION ipls h f
[T]
ipls
The plastic definition set identification number, see Notes.
ij
Stresses defining the yield surface for Hill model.
ijt(c) Stresses defining the yield surface in tension (compression) for Hoffman model.
T
Reference temperature.
N
Number of yield stresses to be specified, see Notes. (Default=1).
y0t(c) Initial reference tensile (compressive) yield stress.
Nt(c)
Number of points/sections defining the tensile (compressive) hardening curve.
Hit(c)
First value defining the hardening curve for tension (compression), see
Notes.
Sit(c)
Second value defining the hardening curve for tension (compression), see
hf
Notes
Notes.
Heat fraction.
1. Data sections specified under the PLASTIC DEFINITION data chapter, which are used to build up the definition of a particular material, must be allocated the same plastic definition identification number, ipls.
2. The STRESS POTENTIAL data section must always be used. A stress potential must be specified for every set of plastic material properties defined.
3. The data sections under the PLASTIC DEFINITION chapter may be specified in any order.
4. When using the HARDENING CURVE, YIELD STRESS or HEAT FRACTION data sections a linear material model must be specified to define the linear material properties.
5. The PLASTIC DEFINITION data must be combined with other material data to define the required nonlinear material using the MATERIAL ASSIGNMENTS or
COMPOSITE MATERIAL data chapters.
6. The PLASTIC DEFINITION data chapter is intended to be used in conjunction with linear material models (e.g. MATERIAL PROPERTIES ORTHOTROPIC).
7. If tables of properties in the separate data sections defining a particular material are inconsistent, an amalgamated table is assembled for interpolation. Tables are inconsistent if they are made up of a different number of lines of data or use different reference temperatures. If this is the case, a value may need to be interpolated which is outside the temperature bounds of the table defined in a particular data section. If this occurs the appropriate extreme value in the table is
75
Chapter 3 LUSAS Data Input
used. If Option 227 is invoked by the user, this occurrence will cause a data error and the analysis will be terminated.
8. For additional information see:
Stress Potential
Yield Stress
Hardening Curve
Heat Fraction
Stress Potential
The use of nonlinear material properties applicable to a general multiaxial stress state requires the specification of yield stresses in each direction of the stress space when defining the yield surface (see the LUSAS Theory Manual). These stresses are specified under the STRESS POTENTIAL command and are assigned to appropriate elements through the MATERIAL ASSIGNMENTS or COMPOSITE MATERIAL data chapters. Hill, von Mises and Hoffman nonlinear material models are available.
Notes
1. The STRESS POTENTIAL data section must always be used. A stress potential must be specified for every set of plastic material properties defined.
2. If a stress potential type is not specified then von Mises is set as default.
3. The yield surface must be defined in full, irrespective of the type of analysis undertaken. This means that none of the stresses defining the yield surface can be set to zero. For example, in a plane stress analysis, the out of plane direct stress
zz, must be given a value which physically represents the model to be analysed.
4. The von Mises stress potential does not require the input of any parameters.
5. The stresses defining the yield surface in both tension, ijt, and compression,
ijc, for the Hoffman potential must be positive.
6. An orthotropic material property must be assigned with the Hill or Hoffman stress potentials.
7. The LUSAS Theory Manual should be consulted if further information on these stress potential parameters is required.
8. The STRESS POTENTIAL data section can be specified under the PLASTIC
DEFINITION or VISCOUS DEFINITION data chapters. If specified under the
VISCOUS DEFINITION data chapter, the material properties must be linear and the STRESS POTENTIAL parameters are applied to the creep properties only. If creep is defined together with a nonlinear material property, the STRESS
POTENTIAL parameters will be applied to both the creep and plasticity; in this instance, the parameters must only be specified under the PLASTIC DEFINITION data chapter.
76
Nonlinear Material Properties
Yield Stress
The stress or stresses specified under the YIELD STRESS data section define an initial uniaxial yield stress. For orthotropic material models, this value is only required for the definition of isotropic hardening; the current stress state for such models is computed using the yield surface defined under the STRESS POTENTIAL data section.
Notes
1. The number of yield stresses to be specified depends on the material model defined. If different yield stresses are required in tension and compression, then n must be set to 2. (Default n=1).
2. There are some occasions when there is no need to use the YIELD STRESS data section:
3. When using the PLASTIC_STRAIN or TOTAL_STRAIN options to define the hardening curve. (The first stress in the curve data is taken as the uniaxial yield stress).
4. When using an orthotropic material property without specifying a hardening curve.
In this instance LUSAS sets an arbitrary value of 1 and writes it to the output file.
5. When using the YIELD STRESS data section a linear material model must be used to specify the linear material properties.
6. The YIELD STRESS data section must always be used if the
HARDENING_GRADIENT option is used to define the hardening curve.
Hardening Curve
The isotropic hardening behaviour for a nonlinear material can be defined under the
HARDENING CURVE data section. There are three options available for defining the curve by using the HARDENING_GRADIENT, PLASTIC_STRAIN or
TOTAL_STRAIN data sections. The data input required for each option is described below.
Notes
1. The values used to define the hardening curve depend upon the option chosen for input.
HARDENING_GRADIENT:
Hit(c) the slope of the (i)th section of the reference tensile
(compressive) yield stress against effective plastic strain curve.
Sit(c) the limit on the effective plastic strain up to which the (i)th section of the hardening curve for tension (compression) is valid.
PLASTIC_STRAIN:
77
Chapter 3 LUSAS Data Input
Hit(c) the (i)th tensile (compressive) uniaxial yield stress defining the hardening curve.
Sit(c) the effective plastic strain corresponding with the (i)th tensile
(compressive) uniaxial yield stress.
TOTAL_STRAIN:
Hit(c) the (i)th tensile (compressive) uniaxial yield stress defining the hardening curve.
Sit(c) the total strain corresponding with the (i)th tensile
(compressive) uniaxial yield stress.
2. When using the PLASTIC_STRAIN or TOTAL_STRAIN options the first pair of values defining the curve must relate to the initial yield point. In this instance the
YIELD STRESS data section can be omitted.
3. All values defined under PLASTIC_STRAIN or TOTAL_STRAIN data sections must be positive, even when defining values for compression.
4. When using the HARDENING CURVE data section a linear material model must be used to specify the linear material properties.
5. The YIELD STRESS data section must always be used if the
HARDENING_GRADIENT option is used to define the hardening curve.
Heat Fraction
The heat fraction is only applicable in thermomechanical coupled analyses where the heat produced due to the rate of generation of plastic work is of interest. The HEAT
FRACTION data section is used to define the fraction of plastic work that is converted to heat.
Notes
1. When using the HEAT FRACTION data section a linear material model must be used to specify the linear material properties.
2. The heat fraction should take a value between 0.0 and 1.0.
Example of Plastic Definition
Example. Plastic Definition
MATERIAL PROPERTIES
1 2E9 0.25 7E3 2E5 5.0 1E3
PLASTIC DEFINITION
STRESS POTENTIAL VON_MISES
23
78
Nonlinear Material Properties
HARDENING CURVE HARD 4 4
23...
200.0 0.005 190.0 0.01 150.0 0.015 100.0 0.02...
250.0 0.005 230.0 0.01 200.0 0.015 160.0 0.02
YIELD STRESS 2
23...
2E8 1.9E8
HEAT FRACTION
23...
0.9
MATERIAL ASSIGNMENTS
1 10 1 1 0 23
Optimised Von Mises Model
The elastoplastic von Mises yield surface models may be used to represent ductile behaviour of materials which exhibit little volumetric strain (for example, metals).
In the optimised implicit (backward Euler) model the direction of plastic flow is evaluated from the stress return path. The implicit method allows the proper definition of a tangent stiffness matrix which maintains the quadratic convergence of the Newton
Raphson iteration scheme otherwise lost with the explicit method. This allows larger load steps to be taken with faster convergence. For most applications, the implicit method should be preferred to the explicit method.
The data section MATERIAL PROPERTIES NONLINEAR 75 is used to define the material properties for the optimised implicit backward Euler von Mises material model. The model incorporates linear isotropic and kinematic hardening.
imat
E
ar
br
hf
T
MATERIAL PROPERTIES NONLINEAR 75 N imat E
a
r
b r
h f
T
yo
H
I1
H
K1
L
1
The material property identification number
Young‟s modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Heat fraction coefficient (see Notes)
Reference temperature
79
Chapter 3 LUSAS Data Input
yo
HI1
HK1
L1
Initial uniaxial yield stress
Isotropic hardening parameter (see Notes)
Kinematic hardening parameter (see Notes)
The limit on the equivalent plastic strain up to which the hardening parameters are valid
The number of straight line approximations to the hardening curve (N must equal 1 for this model)
N
Notes
1. See Nonlinear Material Hardening Convention for an example of how to convert from the elastoplastic modulus, Ep, to the slope of the uniaxial yield stress against equivalent plastic strain curve when specifying a hardening curve.
2. The heat fraction coefficient represents the fraction of plastic work which is converted to heat and takes a value between 0 and 1. For compatibility with pre
LUSAS 12 data files specify Option 235.
Uniaxial Yield
Stress
= tan
1
C
1
yo
L
1
Equivalent Plastic
Strain,
p
Nonlinear Hardening Curve for the Backward Euler von Mises and Hill Models
(Model 75)
DruckerPrager Model
The DruckerPrager elastoplastic model (see figures below) may be used to represent the ductile behaviour of materials which exhibit volumetric plastic strain (for example, granular materials such as concrete, rock and soils). The model incorporates isotropic hardening.
The data section MATERIAL PROPERTIES NONLINEAR 64 is used to define the material properties.
MATERIAL PROPERTIES NONLINEAR 64 N
80
Nonlinear Material Properties imat E
a
r
b r
h f
T c
0
0
C1
1
C2
1
L
1
imat
E
ar
br
hf
T
c0
f0
C11
C21
L1
N
The material property identification number
Young‟s modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Heat fraction coefficient (see Notes)
Reference temperature
Initial cohesion (see Notes)
Initial friction angle (degrees)
The slope of the cohesion against the equivalent plastic strain
The slope of the friction angle against the equivalent plastic strain
The limit to which the hardening curve is valid
The number of straight line approximations to the hardening curve (N must equal 1)
Notes
1. The heat fraction coefficient represents the fraction of plastic work which is converted to heat and takes a value between 0 and 1. For compatibility with pre
LUSAS 12 data files specify Option 235.
2. Setting the initial cohesion (c0) to zero is not recommended as this could cause numerical instability under certain loading conditions.
Cohes ion
C
0
1
1
=tan
1
C1
1
L
1 Equivalent Plas tic
Strain
p
Cohesion Definition for the DruckerPrager Yield Model
(Model 64)
81
Chapter 3 LUSAS Data Input
Friction
Angle
0
2
2
=tan
1
C2
1
L
1 Equivalent Plas tic
Strain
p
Friction Angle Definition for the DruckerPrager Yield Model
(Model 64)
Tresca Model
The elastoplastic Tresca yield surface model may be used to represent ductile behaviour of materials which exhibit little volumetric strain (for example, metals). The model incorporates elastoplastic behaviour with isotropic hardening. The data section
MATERIAL PROPERTIES NONLINEAR 61 is used to define the material properties for the Tresca yield surface model.
MATERIAL PROPERTIES NONLINEAR 61 N imat E
a
r
b r
h f
T
yo
C
1
L
1
imat
E
ar
br
hf
T
yo
C1
The material property identification number
Young‟s modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Heat fraction coefficient (see Notes)
Reference temperature
Initial uniaxial yield stress
The slope of the uniaxial yield stress against equivalent plastic strain (see
Notes)
82
Nonlinear Material Properties
L1
N
The limit on the equivalent plastic strain up to which the hardening curve is valid
The number of straight line approximations to the hardening curve (N must equal 1 for this model)
Notes
1. See Nonlinear Material Hardening Convention for an example of how to convert from the elastoplastic modulus, Ep, to the slope of the uniaxial yield stress against equivalent plastic strain curve when specifying a hardening curve.
2. The heat fraction coefficient represents the fraction of plastic work which is converted to heat and takes a value between 0 and 1. For compatibility with pre
LUSAS 12 data files specify Option 235.
Uniaxial Yield
Stress
yo
=tan
1
C
1
L
1
Equivalent Plastic
Strain,
p
Hardening Curve Definition for the Tresca and von Mises Yield Models
(Models 61 & 62)
NonAssociated MohrCoulomb Model
The nonassociated MohrCoulomb elastoplastic model (see figures below) may be used to represent dilatant frictional materials which increasing shear strength with increasing confining stress (for example, materials such as granular soils and rock).
The model incorporates isotropic hardening.
The data section MATERIAL PROPERTIES NONLINEAR 65 is used to define the material properties.
83
Chapter 3 LUSAS Data Input
MATERIAL PROPERTIES NONLINEAR 65 imat E
a
r
b r
T c i
i
f
h
c
f
imat
E
ar
br
T
ci
i
f
hc
f
Notes
The material property identification number
Young‟s modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Reference temperature
Initial cohesion
Initial friction angle (degrees)
Final friction angle (degrees)
Dilation angle (degrees)
Cohesion hardening parameter
Limiting equivalent plastic strain
1. The nonassociated MohrCoulomb model may be used with 2D and 3D continuum elements, 2D and 3D explicit dynamics elements, solid composite elements and semiloof or thick shells.
2. The nonsymmetric solver (Option 64) is automatically switched on when using the nonassociated MohrCoulomb model.
3. A system parameter may also be modified when using the nonassociated Mohr
Coulomb model.
QMHDLM (default=0.01)
To prevent solution instabilities a lower positive limit is applied on the hardening moduli used to form the D matrix. The default value is set at E/100 by may be altered using the system parameter QMHDLM. The value QMHDLM*E will then be used.
84
Nonlinear Material Properties
Cohes ion
C i
1
1
=tan
1 h c
f
Equivalent Plas tic
Strain
p
Cohesion Definition for the NonAssociated MohrCoulomb Model
(Model 65)
Friction
Angle
f
i
f
Equivalent Plas tic
Strain
p
Friction Angle Definition for the NonAssociated MohrCoulomb Model
(Model 65)
85
Chapter 3 LUSAS Data Input
ElastoPlastic Stress Resultant Model
The elastoplastic stress resultant model may be used for beams, plates and shells (see the LUSAS Element Reference Manual). It is based on a von Mises yield criterion. The data section MATERIAL PROPERTIES NONLINEAR 29 is used to define the material properties for the elastoplastic stress resultant model.
MATERIAL PROPERTIES NONLINEAR 29 imat E
ar br T
y
ifcode
imat
E
ar
br
The material property identification number
Young‟s modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
T
y
Reference temperature
Uniaxial yield stress
ifcode
Yield function code (refer to individual elements in the LUSAS Element
Reference Manual)
Notes
1. Temperature dependent material properties are not applicable for this model.
2. The yield criteria, when used with beam elements, includes the effects of nonlinear torsion. Note that the effect of torsion is to uniformly shrink the yield surface.
3. The stressstrain curve is elastic/perfectly plastic.
4. The fully plastic torsional moment is constant.
5. Transverse shear distortions are neglected.
6. Plastification is an abrupt process with the whole crosssection transformed from an elastic to fully plastic stress state.
7. Updated Lagrangian (Option 54) and Eulerian (Option 167) geometric nonlinearities are not applicable with this model. The model, however, does support the total strain approach given by Total Lagrangian and Corotational geometric nonlinearities, Option 87 and Option 229, respectively.
UserSupplied Nonlinear Material Properties
The USER constitutive model facility allows the usersupplied constitutive routines to be used from within LUSAS. This facility provides completely general access to the
LUSAS property data input via the MATERIAL PROPERTIES NONLINEAR USER and MATERIAL PROPERTIES NONLINEAR RESULTANT USER data sections and provides controlled access to the pre and postsolution constitutive processing and nonlinear state variable output via these usersupplied subroutines.
86
Nonlinear Material Properties
By default these routines are supplied as empty routines with defined interfaces that are unchangeable. The externally developed code should be placed into these routines which is then linked into the LUSAS system. Source code access is available to these interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised. See Solver User Interface Routines.
Since user specification of a constitutive model involves the external development of source FORTRAN code, as well as access to LUSAS code, this facility is aimed at the advanced LUSAS user.
Material Properties Nonlinear User
The required material properties input for the usersupplied constitutive model is completely general. The first 15 properties are reserved for LUSAS internal use: you only need to utilise them if other features of the program are required (e.g. dynamic and thermal analyses). The data section MATERIAL PROPERTIES NONLINEAR USER is used to define all the material parameters for the usersupplied constitutive models.
MATERIAL PROPERTIES NONLINEAR USER lptusr nprz nstat imat E
x
y
z
< U i
> i=1,(nprz15)
xy
yz
xz
ar br hf T {
lptusr
A user defined material model number
nprz
The total number of material input parameters provided
nstat
The number of nonlinear state dependent constitutive variables
imat
The material assignment reference number
E
x
y
z
Young‟s modulus
Poisson‟s ratio
Mass density
xy
yz
xz
ar
br
hf
T
Coefficients of thermal expansion (see Notes)
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Heat fraction coefficient (see Notes)
Reference temperature
Angle of anisotropy relative to the reference axes (degrees) Option 207 must be set (see Notes)
nset
The CARTESIAN SET number used to define the local reference axes
spare
Unused parameter at present (set = 0.0)
Ui
Notes
The userdefined material parameters
1. LUSAS will check and diagnose erroneous or improbable data.
2. The number of material properties input must be equal to that specified on the data section header line (i.e. nprz). Failure to match the requested and supplied number of properties will invoke a LUSAS error message.
87
Chapter 3 LUSAS Data Input
3. When no state variables are required (i.e. when nstat is specified as zero) a warning message will be invoked.
4. Usersupplied constitutive models may be used as part of a composite element material assembly.
5. The first 15 material properties are required by LUSAS in order to perform other types of analyses: for example thermal problems require the coefficients of thermal expansion
(4th to 9th properties) and/or the temperature T (13th property), and a dynamic analysis requires the density
(3rd property) and the Rayleigh damping parameters ar, br (10th, 11th properties).
6. The user is required to input appropriate
values for the element type to be used and zeroes for the remainder. For example:
Plane stress elements:
x
y
xy
Plane strain and axisymmetric elements:
x
y
z
xy
Thick shell elements:
x
y
xy
yz
zx
Solid elements:
x
y
z
xy
yz
zx
If an isotropic model is required then the input must be specified accordingly, e.g. for plane strain elements this would require
x
=
y
=
z
and
xy
= 0.
7. If temperature dependent properties are input via the TABLE format T, the 13th property, must be specified so that the values can be interpolated for the actual temperatures at the Gauss points.
8. The 15 reserved properties can all be set to zero if you do not require other LUSAS facilities
9. Option 207 allows you to control how the local reference axes are to be determined; if the angle of anisotropy is determined by the angle q, Option 207 must be set, otherwise the reference axes must be determined by a CARTESIAN
SET.
10. Option 179 can be set for argument verification within the user routines.
11. The heat fraction coefficient represents the fraction of plastic work which is converted to heat in a coupled analysis and takes a value between 0 and 1.
12. A user defined nonlinear material model which results in a nonsymmetric modulus matrix can only be used with the following element types: 3D continuum
(excluding explicit dynamics elements), 2D continuum (excluding Fourier and explicit dynamics elements), bar elements and axisymmetric membrane elements.
Material Properties Nonlinear Resultant User
The general form of the input for this chapter has been tailored to allow the specification of nonlinear momentcurvature curves. However, the parameters required for any other type of user defined nonlinear resultant model may be specified via this data chapter. The first 10 properties are reserved for LUSAS internal use: you only
88
Nonlinear Material Properties
need to utilise some of them if other features of the program are required (e.g. dynamic and thermal analyses). The user subroutines supplied contain code that defines the momentcurvature relationship to be a function of the axial force in the member. The code in these routines can be overwritten with user defined code or alternatives added by utilising different lptusr parameters.
MATERIAL PROPERTIES NONLINEAR RESULTANT USER lptusr nprz ndcrve nstat imat E
a
r
b r
spare T spare spare …
F
1
< M
1,j
,C
1,j
> j=1,(nprz1)
…
. …
.
.
…
…
F ndcrve
< M ndcrve,j
,C ndcrve,j
> j=1,(nprz1)
lptusr
A user defined material model number
nprz
The number of material input parameters for each curve
ndcrve
The number of material data curves defined
E
nstat
The number of nonlinear state dependent constitutive variables
imat
The material assignment reference number
Young‟s modulus
ar
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
br
Stiffness Rayleigh damping constant
spare
Unused parameter at present (set = 0.0)
T
Reference temperature
spare
Unused parameter at present (set = 0.0)
spare
Unused parameter at present (set = 0.0)
F n
M n,j
Axial force for n th
curve (could be +ve, ve or zero)
,C n,j
Moment and curvature for point j on the n th
curve
Notes
1. LUSAS will check and diagnose erroneous or improbable data.
2. The number of material data curves defined must equal the number specified, ndcrve.
3. All data curves must be defined by the same number of parameters which must equal the number specified, nprz1.
4. Some of the first 10 material properties are required by LUSAS in order to perform other types of analyses: for example thermal problems require the coefficients of
89
Chapter 3 LUSAS Data Input
thermal expansion
(4th property) and/or the temperature T (8th property), and a dynamic analysis requires the density
(3rd property) and the Rayleigh damping parameters ar, br (5th and 6th properties).
5. When no state variables are required (i.e. when nstat is specified as zero) a warning message will be invoked.
6. Option 179 can be set for argument verification within the user routines.
7. If temperature dependent properties are input via the TABLE format T, the 8th property, must be specified so that the values can be interpolated for the actual temperatures at the Gauss points.
Further Notes
These notes apply if the MATERIAL PROPERTIES NONLINEAR RESULTANT
USER subroutines are used with the nonlinear momentcurvature facility as supplied:
1. It is recommended that the curvature values used to define the points on each individual curve be defined reasonably consistently for all curves, i.e. the curvature range used to define point j in all n curves should be reasonably small. This will lead to better interpolation between curves.
2. For 3D beam elements, all curves relating to Iyy must be specified first followed by the curves for Izz. The same number of curves must be specified for both Iyy and Izz.
3. All moment and curvature values specified for a curve must be positive. The slope of the curve segments must always be greater than zero.
4. If the computed axial force is outside the bounds of the forces defined for the data curves, the curve relating to the maximum (or minimum) axial force will be used and a warning message printed to the output file.
5. If the computed curvature exceeds the maximum value specified in the data curves, the last section of the curve will be used to compute the bending moment and a warning message will be printed to the output file.
Viscous Definition
Nonlinear viscous behaviour occurs when the relationship between stress and strain is time dependent. The viscous response is usually a function of the material together with the stress, strain and temperature history. Unlike time independent plasticity where a limited set of yield criteria may be applied to many materials, the creep response differs greatly for many materials.
To provide for the analysis of particular materials, user defined creep laws and viscoelastic models may be specified by replacing the CREEP PROPERTIES and
VISCO ELASTIC PROPERTIES data sections with CREEP PROPERTIES USER and
VISCO ELASTIC PROPERTIES USER respectively.
90
Nonlinear Material Properties
Viscous Definition
This data chapter contains the input for creep and viscoelastic material models.
VISCOUS DEFINITION
STRESS POTENTIAL {VON_MISES  HILL} ipls [
xx
yy
zz
xy
yz
xz
T]
CREEP PROPERTIES lctp icrp
f i
i=1,ncprp
T
CREEP PROPERTIES USER lctp nprzc nstat icrp T spare spare < f i
> i=1,nprzc3
VISCO ELASTIC PROPERTIES [1] ivse G v
T
For further information see:
Stress Potential
Creep Properties
Creep Properties User
Visco Elastic Properties
Visco Elastic Properties User
Stress Potential
The definition of creep properties requires that the shape of the yield surface is defined
(see the LUSAS Theory Manual). The stresses defining the yield surface are specified under the STRESS POTENTIAL command and are assigned to appropriate elements through the MATERIAL ASSIGNMENTS or COMPOSITE MATERIAL data chapters. The STRESS POTENTIAL should only be defined under VISCOUS
DEFINITION if linear material properties are to be used, otherwise, it should be defined under the PLASTIC DEFINITION data chapter. Note that the Hoffman potential is not applicable if the STRESS POTENTIAL is specified under VISCOUS
DEFINITION.
STRESS POTENTIAL {VON_MISES  HILL} ipls [
xx
yy
zz
xy
yz
xz
T]
ipls
ij
T
The stress potential set identification number
Stresses defining the yield surface (Hill)
Reference temperature
91
Chapter 3 LUSAS Data Input
Notes
1. If a stress potential type is not specified then von Mises is set as default.
2. The stress potential must be defined in full irrespective of the analysis type, except for the von Mises stress potential which, being isotropic, does not require the input of any parameter.
3. None of the stresses defining the stress potential may be set to zero. For example, in a plane stress analysis, the out of plane direct stress must be given a value which physically represents the model to be analysed.
4. STRESS POTENTIAL HOFFMAN is not applicable within the VISCOUS
DEFINITION data chapter.
5. The LUSAS Theory Manual should be consulted if further information on these stress potential parameters is required.
6. The STRESS POTENTIAL data section can be specified under the PLASTIC
DEFINITION or VISCOUS DEFINITION data chapters. If specified under the
VISCOUS DEFINITION data chapter, the material properties must be linear and the STRESS POTENTIAL parameters are applied to the creep properties only. If creep is defined together with a nonlinear material property, the STRESS
POTENTIAL parameters will be applied to both the creep and nonlinear material property; in this instance, the parameters must only be specified under the
PLASTIC DEFINITION data chapter.
7. The STRESS POTENTIAL data is combined with other material data to define an elastoplastic and/or a creep material model within the MATERIAL
ASSIGNMENTS or COMPOSITE MATERIAL data chapters.
Creep Properties
There are three uniaxial creep laws available in LUSAS and a time hardening form is available for all laws. The power creep law is also available in a strain hardening form.
Fully 3D creep strains are computed using the differential of the von Mises or Hill stress potential. The CREEP PROPERTIES data section is used to describe the creep data for these models.
CREEP PROPERTIES lctp icrp
f i
i=1,ncprp
T
lctp
icrp
fi
The creep model type:
1  Power law (time dependent form)
2  Power law (strain hardening form)
3  Exponential law
4  Eight parameter law
The creep property identification number
Creep properties
92
Nonlinear Material Properties
ncprp
Number of parameters defining the creep law:
3  Power law
6  Exponential law
T
8  Eight parameter law
Temperature
Example. Creep Properties
MATERIAL PROPERTIES
1 2E5 0.3
VISCOUS DEFINITION
STRESS POTENTIAL VON_MISES
23
CREEP PROPERTIES 1
100 1E7 5 0.5
MATERIAL ASSIGNMENTS
80 1 1 0 23 100
Notes
1. The required creep properties for each law are:
Power law
c
f q f 2 t f 3
Exponential law
c
L
NM
1
e
Eight parameter law
f
4
QP
O
e
c
f q f
2 t f
3
f
5
f t f
7 e
f
8
/ T where:
c q
= uniaxial creep strain
= von Mises or Hill equivalent deviatoric stress t
= current time
T
= temperature (Kelvin)
Further information on these creep laws may be found in the LUSAS Theory
Manual.
2. Creep properties must be defined under the VISCOUS DEFINITION data chapter
93
Chapter 3 LUSAS Data Input
3. The definition of creep properties requires that the shape of the yield surface is defined (see the LUSAS Theory Manual). The stresses defining the yield surface are specified under the STRESS POTENTIAL command and are assigned to appropriate elements through the MATERIAL ASSIGNMENTS or COMPOSITE
MATERIAL data chapters.
4. If combined plasticity and creep is utilised then the creep and plasticity must adopt the same form of stress potential i.e. either isotropic or anisotropic.
5. Creep properties may be combined with other material properties and damage properties under the MATERIAL ASSIGNMENT or COMPOSITE MATERIAL data chapters.
6. Creep data is sometimes provided for the creep law in rate form. The time component of the law must be integrated so that the law takes a total form before data input. For example the rate form of the Power law
c
integrates to
c
b g
A m
1 q t
1
The properties specified as input data then become f
1
m
A
1 f
2
n f
3
1 where A, n and m are temperature dependent constants.
7. NONLINEAR CONTROL must be specified with creep materials unless explicit integration and linear materials are specified (see Viscous Control).
8. DYNAMIC CONTROL may be utilised with creep properties if required.
User Supplied Creep Properties
The USER creep property facility allows user supplied creep law routines to be used from within LUSAS. This facility provides completely general access to the LUSAS property data input via the CREEP PROPERTIES USER data section and provides controlled access to the pre and postsolution constitutive processing and nonlinear state variable output via these usersupplied subroutines.
CREEP PROPERTIES USER must replace CREEP PROPERTIES within the
VISCOUS DEFINITION data chapter. The appropriate STRESS POTENTIAL must also be specified under VISCOUS DEFINITION, if a linear material is to be used, or
94
Nonlinear Material Properties
the PLASTIC DEFINITION data chapter if an allowable nonlinear material property is defined.
Source code access is available to interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised.
Contact FEA for full details of this facility. Since user specification of a creep law involves the external development of source FORTRAN code, as well as access to
LUSAS code, this facility is aimed at the advanced LUSAS user.
CREEP PROPERTIES USER lctp nprzc nstat icrp T spare spare < f i
> i=1,nprzc3
lctp
A user defined creep model type
nprzc
The number of properties for the creep model
nstat
The number of creep state variables (see Notes)
icrp
T
The creep property identification number
Reference temperature
spare
Unused parameter at present (set=0.0)
f i
Notes
Creep properties
1.
nstat must be an integer value greater than zero.
2. The number of creep properties input must be equal to that specified on the data section header line (i.e. nprzc). Failure to match the requested and supplied number of properties will invoke a LUSAS error message.
3. If temperature dependent properties are input using the TABLE format, T, the 1st property must be specified so that the values can be interpolated for the actual temperatures at the Gauss points. If the creep properties are not temperature dependent, the 1st property may be set to zero.
4. The usersupplied subroutine permits creep laws defined as:
where
q
t
T
= rate of uniaxial. equivalent creep strain
= equivalent deviatoric stress
= time
= temperature
5. The usersupplied routine must return the increment in creep strain. Further, if implicit integration is to be used then the variation of the creep strain increment with respect to the equivalent stress and also with respect to the creep strain increment, must also be defined.
6. If the function involves time dependent state variables they must be integrated in the usersupplied routine.
95
Chapter 3 LUSAS Data Input
7. If both plasticity and creep are defined for a material, the creep strains will be processed during the plastic strain update. Stresses in the user routine may therefore exceed the yield stress.
8. Usersupplied creep laws may be used as part of a composite element material assembly.
9. Option 179 can be set for argument verification within the user routines
10. Viscoelastic properties must be defined under the VISCOUS DEFINITION data chapter.
11. The definition of creep properties requires that the shape of the yield surface is defined (see the LUSAS Theory Manual). The stresses defining the yield surface are specified under the STRESS POTENTIAL command and are assigned to appropriate elements through the MATERIAL ASSIGNMENTS or COMPOSITE
MATERIAL data chapters.
12. If combined plasticity and creep is utilised then the creep and plasticity must adopt the same form of stress potential i.e. either isotropic or anisotropic.
13. Creep properties may be combined with other material properties and damage properties under the MATERIAL ASSIGNMENT or COMPOSITE MATERIAL data chapters.
Visco Elastic Properties
The viscoelastic facility can be coupled with the linear elastic and nonlinear plasticity, creep and damage models currently available in LUSAS. The model restricts the viscoelastic effects to the deviatoric component of the material response. This enables the viscoelastic material behaviour to be represented by a viscoelastic shear modulus
G v
and a decay constant
. Viscoelasticity imposed in this way acts like a springdamper in parallel with the elasticplastic, damage and creep response. Coupling of the viscoelastic and the existing nonlinear material behaviour enables hysteresis effects to be modelled.
There is currently one viscoelastic model implemented in LUSAS. The VISCO
ELASTIC PROPERTIES data section is used to describe the viscoelastic data for this model.
VISCO ELASTIC PROPERTIES [1] ivse Gv
T
ivse
Gv
T
The viscoelastic property identification number
Viscoelastic shear modulus (see Notes)
Viscoelastic decay constant (see Notes)
Reference temperature
96
Nonlinear Material Properties
Notes
1. It is assumed that the viscoelastic effects are restricted to the deviatoric component of the material response. The deviatoric viscoelastic components of stress are obtained using a stress relaxation function G(t), which is assumed to be dependent on the viscoelastic shear modulus and the decay constant.
' v t b g z
0 t
2 G t b g s d
ds
' ds G t b g
G e
2. The viscoelastic shear modulus
G v can be related to the instantaneous shear modulus, G0, and long term shear modulus,
G
0 , using .
G v
G
0
G
3. When viscoelastic properties are combined with isotropic elastic properties, the elastic modulus and Poisson‟s ratio relate to the long term behaviour of the material, that is,
E
and
.At each iteration, the current deviatoric viscoelastic stresses are added to the current elastic stresses. The deviatoric viscoelastic stresses are updated using;
' v b t
g t
' v b g t e
t
2 G v e
1
e
t j
'
t where
v
= deviatoric viscoelastic stresses
G
v
= viscoelastic shear modulus
= viscoelastic decay constant
t
= current time step increment
= incremental deviatoric strains
4. When viscoelastic properties are coupled with a nonlinear material model it is assumed that the resulting viscoelastic stresses play no part in causing the material to yield and no part in any damage or creep calculations. Consequently the viscoelastic stresses are stored separately and deducted from the total stress vector at each iteration prior to any plasticity, creep or damage computations. Note that this applies to both implicit and explicit integration of the creep equations.
5. Viscoelastic properties must be defined under the VISCOUS DEFINITION data chapter.
6. Viscoelastic properties may be combined with other material properties, creep and damage properties under the MATERIAL ASSIGNMENT and COMPOSITE
MATERIAL data chapters.
7. NONLINEAR CONTROL must always be specified when viscoelastic properties are assigned. In addition either DYNAMIC CONTROL or VISCOUS CONTROL must also be specified to provide a time step increment for use in the viscoelastic
97
Chapter 3 LUSAS Data Input
constitutive equations. If no time control is used the viscoelastic properties will be ignored.
User Supplied Viscoelastic Properties
The VISCO ELASTIC PROPERTIES USER facility enables a user supplied viscoelastic model to be invoked from within LUSAS. This facility provides completely general access to the LUSAS property data input via this data section and provides controlled access to the pre and postsolution constitutive processing and nonlinear state variable output via these user supplied routines. VISCO ELASTIC
PROPERTIES USER must replace VISCO ELASTIC PROPERTIES in the VISCOUS
DEFINITION data chapter.
Source code access is available to interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised.
Contact LUSAS for full details of this facility. Since user specification of a viscoelastic model involves the external development of a FORTRAN source code, as well as access to the LUSAS code, this facility is aimed at the advanced LUSAS user.
VISCO ELASTIC PROPERTIES USER lvse nprzv nstat ivse
f i
i=1,nprzv
T
lvse
A user defined viscoelastic model type
nprzv
The number of properties for the viscoelastic model
nstat
The number of user defined viscoelastic state variables
f i
T
Viscoelastic properties
Reference temperature
Notes
1.
nstat must be an integer greater than or equal to zero.
2. The number of viscoelastic properties input must be equal to that specified on the data section header line (i.e. nprzv). Failure to match the requested and supplied number of properties will invoke a LUSAS error message.
3. If temperature dependent properties are input using the TABLE format, T, the last property must be specified so that the values can be interpolated for the actual temperatures at the Gauss points.
4. A viscoelastic model can be combined with any of the elastic material models and the following nonlinear models:
Tresca (model 61)
Mohr Coulomb (model 65)
DruckerPrager (model 64)
98
Nonlinear Material Properties
VonMises (model 75)
Hill
Hoffman
User Defined Nonlinear Material Model
5. VISCO ELASTIC PROPERTIES USER must be defined under the VISCOUS
DEFINITION data chapter and assigned using MATERIAL ASSIGNMENTS or
COMPOSITE MATERIAL.
6. Option 179 can be set for argument verification within the user routines.
7. Viscoelastic properties may be combined with other material properties, creep and damage properties under the MATERIAL ASSIGNMENT or COMPOSITE
MATERIAL data chapters.
8. The current viscoelastic stresses must be evaluated at each iteration and added to the current Gauss point stresses. These viscoelastic stresses are subsequently subtracted at the next iteration, internally within LUSAS, before any plasticity, creep or damage calculations are performed.
Damage Material
Damage is assumed to occur in a material by the initiation and growth of cavities and microcracks. The DAMAGE PROPERTIES data chapter allows parameters to be defined which control the initiation of damage and post damage behaviour. In LUSAS a scalar damage variable is used in the degradation of the elastic modulus matrix. This means that the effect of damage is considered to be nondirectional or isotropic. Two
LUSAS damage models are available (Simo and Oliver) together with a facility for a usersupplied model. For further details of these damage models the LUSAS Theory
Manual should be consulted.
Damage Properties
DAMAGE PROPERTIES [SIMO  OLIVER] idam {r0 A B  r0 A n} T
idam
r0
A
B
n
T
Notes
Damage properties set identification number
Initial damage threshold (see Notes)
Characteristic material parameter (see Notes)
Characteristic material parameter (see Notes)
Ratio of the stresses that cause initial damage in tension and compression
=
cd/
td (see Notes)
Reference temperature
1. The initial damage threshold, r0, can be considered to carry out a similar function to the initial yield stress in an analysis involving an elastoplastic material.
99
Chapter 3 LUSAS Data Input
However, in a damage analysis, the value of the damage threshold influences the degradation of the elastic modulus matrix. A value for r0 may be obtained from: r o
t
b g
/ d
1 2 where
is the uniaxial tensile stress at which damage commences and E is the undamaged Young‟s modulus. The damage criterion is enforced by computing the elastic complementary energy function as damage progresses: e
T
D e
j r 0 where
is the vector of stress components, D the elastic modulus matrix and r the current damage norm. The factor
is taken as 1 for the Simo damage model, while for the Oliver model takes the value:
HG
F
1
n
I
KJ where
1
2
3

1
 
2  
3  n
t d c d
Only positive values are considered for <
i>, any negative components are set to zero. The values
and
t d
represent the stresses that cause initial damage in compression and tension respectively (note that if
=
t d
,
=1). The damage accumulation functions for each model are given by:
Simo:
G r b g t r b g r t
A exp B r b
0
r g t
Oliver:
G r b g
r
0 r t exp
NM
L
A
HG
F
1
r
0 r t
I
KJ
O
QP
For no damage, G(r
t
)=0. The characteristic t material parameters, A and B, would generally be obtained from experimental data. However, a means of computing A has been postulated for the Oliver model:
A
l
MM
N
MM
L ch e j
2
0
1
2
PP
O
Q
PP
1 where G
f
is the fracture energy per unit area, l
ch
is a characteristic length of the finite element which can be approximated by the square root of the element area.
100
Nonlinear Material Properties
These damage models are explained in greater detail in the LUSAS Theory
Manual.
2. The damage criterion for the Oliver model introduces a factor which is invoked if different stress levels cause initial damage in tension and compression.
3. A damage analysis can be carried out using any of the elastic material models and the following nonlinear models:
von Mises
Hill
Hoffman
4. CREEP PROPERTIES and/or VISCO ELASTIC PROPERTIES may be included in a damage analysis. See Viscous Definition
5. DAMAGE PROPERTIES must be assigned using MATERIAL ASSIGNMENTS or COMPOSITE MATERIAL.
User Supplied Damage Properties
The DAMAGE PROPERTIES USER facility allows routines for implementing a user supplied damage model to be invoked from within LUSAS. This facility provides completely general access to the LUSAS property data input via this data section and provides controlled access to the pre and postsolution constitutive processing and nonlinear state variable output via these usersupplied subroutines.
Source code access is available to interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised.
Contact LUSAS for full details of this facility. Since user specification of a damage model involves the external development of source FORTRAN code, as well as access to LUSAS code, this facility is aimed at the advanced LUSAS user.
DAMAGE PROPERTIES USER ldtp nprzd nstat idam < P i
> i=1,nprzd
T
ldtp
User defined damage model identification number
nprzd
Number of parameters used in defining the damage model
nstat
Number of damage state variables (see Notes)
idam
Pi
T
Notes
Damage properties set identification number
User supplied parameters for damage model
Reference temperature
1.
nstat must be an integer value greater than zero.
2. The number of damage properties input must be equal to that specified on the data section header line (i.e. nprzd). Failure to match the requested and supplied number of properties will invoke a LUSAS error message.
101
Chapter 3 LUSAS Data Input
imat
E
t
ar
br
T
fc
ft
c
3. If temperature dependent properties are input using the TABLE format, T, the last property must be specified so that the values can be interpolated for the actual temperatures at the Gauss points.
4. A damage analysis can be carried out using any of the elastic material models and the following nonlinear models:
von Mises
Hill
Hoffman
5. CREEP PROPERTIES and/or VISCOELASTIC PROPERTIES may be included in a damage analysis. See Viscous Definition
6. DAMAGE PROPERTIES USER must be assigned using MATERIAL
ASSIGNMENTS or COMPOSITE MATERIAL.
7. Option 179 can be set for argument verification within the user routines
8. Damage properties may be combined with other material properties and creep properties under the MATERIAL ASSIGNMENT or COMPOSITE MATERIAL data chapters.
MultiCrack Concrete Model
This concrete model is a plasticdamagecontact model in which damage planes form according to a principal stress criterion and then develop as embedded rough contact planes. The basic softening curve used in the model may be controlled via a fixed softening curve or a fractureenergy controlled softening curve that depends on the element size. The former, distributed fracture model, is applicable to reinforced concrete applications, while the latter localised fracture model is applicable to unreinforced cases.
MATERIAL PROPERTIES NONLINEAR 94 imat E,
,
,
t
, a r
, b r
, T, f c
, f t
,
c m g
, m hi
, m ful
, r
,
,
d
,
0
, G f
,
r
,
0
,
,
The material property identification
Young‟s modulus. Only
Poisson‟s ratio.
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping coefficient
Stiffness Rayleigh damping coefficient
Reference temperature
Uniaxial compressive strength (e.g. 40N/mm
2
)
Uniaxial tensile strength (e.g. 3.0 N/mm
2
)
Strain at peak uniaxial compression (e.g. 0.0022)
102
Nonlinear Material Properties
o
Gf
r
o
mg
mhi
mful
r
Strain at effective end of softening curve for distributed fracture (e.g.
0.0035, or 0.0 if G f
0)
Fracture energy per unit area (e.g. 0.1 N/mm or 0.0 if
0
0)
Biaxial to uniaxial peak principal stress ratio (e.g. 1.15 Range = 1.0 to
1.25)
Initial relative position of yield surface (e.g. 0.6. Range = 0.1 to 1.0 )
Dilatancy factor giving plastic potential slope relative to that of yield surface (e.g. 0.1 Range 0.25 to 1.0 )
Constant in interlock state function (e.g. 0.425 Range 0.3 to 0.6)
Contact multiplier on
0
for 1 st
opening stage (e.g. 0.5 Range 0.25 to 2.0)
Final contact multiplier on
0
(e.g. 5.0 Range 1.0 to 20)
Shear intercept to tensile strength ratio for local damage surface (e.g. 1.25
Range 0.5 to 2.5)
Slope of friction asymptote for local damage surface (e.g. 1.0 Range 0.5
to 1.5 Note
< r
)
Angular limit between crack planes (e.g. 1.0 (radians))
d
Notes
1. The model can be used with 2D and 3D continuum elements, 2D and 3D explicit dynamics elements, solid composite elements and semiloof or thick shell elements.
1. All stresses and strains should be entered as positive values.
2. If no data for the strain at peak compressive stress,
c
, is available it can be estimated from
c
.
for
c
should lie in the range
.
(
f cu
45
c
15 )
where
f cu
1 25
f c
. Any value
. As a guide, a reasonable value for most concretes is 0.0022.
3.
It is important that the initial Young‟s modulus, E, is consistent with the strain at peak compressive stress,
c
. A reasonable check is to ensure that
E
. (
f c
/
c
)
.
4. For concrete that contains reinforcement, distributed fracture will be the dominant fracture state. In this case a value for the strain at the end of the tensile softening curve,
0
, should be entered and G f
set to zero. If no data is available then a value of
0
0 0035
is reasonable to use for most concretes.
5. For unreinforced concrete the strains will tend to localise in crack zones, leading to localised fracture. The value for
0
must be set to 0.0 and the fracture energy per unit area, G f
, given a positive value. G f
varies with aggregate size but not so much with concrete strength. Typical values for various maximum coarse aggregate sizes are:
16 mm aggregate: G f
= 0.1N/mm
20 mm aggregate: G f
= 0.13N/mm
103
Chapter 3 LUSAS Data Input
32 mm aggregate: G f
= 0.16N/mm
Damage evolution function
If the effective end of the softening curve parameter, calculated from
0
5
G f
/
W f c t
element; if a finite value is given for
where W
c
is a characteristic length for the
0
,
G f
0
, is set to zero, it will be
will be ignored.
6. The initial position of the yield surface is governed by the value of
0
. For most situations in which the degree of triaxial confinement is relatively low, a value of between 0.5 and 0.6 is considered appropriate for
0
however, for higher confinements a lower value of 0.25 is better.
7. The parameter
is used to control the degree of dilatancy. Associated plastic flow is achieved if
=1, but it was found that
values in the range 0.1 to –0.3 were required to match experimental results. Generally
is set to –0.1, but for high degrees of triaxial confinement –0.3 provides a better match to experimental data.
8. The constant m g
can be obtained from experimental data from tests in which shear is applied to an open crack. The default value for m g
is taken as 0.425 but it is considered that a reasonable range for m g
for normal strength concrete is between
0.3 and 0.6. However, it was found that a low value of 0.3 could lead to second cracks forming at shallow angles to the first, due to the development of relatively large shear forces.
9. It is assumed that there is a crack opening strain beyond which no further contact can take place in shear, e ful.
, where e ful
is a multiple of
0
, i.e. e ful
=m ful
0
. Trials suggest that when concrete contains relatively large coarse aggregate i.e. 20 to
30mm, a value of m ful
in the range 1020 is appropriate, whereas for concrete with relatively small coarse aggregate, i.e. 5 to 8mm, a lower value is appropriate, in the range 3 to 5. This variation is necessary because the relative displacement at the end of a tensionsoftening curve (related via the characteristic dimension to
0
) is not in direct proportion to the coarse aggregate size, whereas the clearance
104
Nonlinear Material Properties
displacement is roughly in proportion to the coarse aggregate size. Thus e in a fixed ratio to
0
. ful
is not
10. A POD is formed when the principal stress reaches the fracture stress (f t
); the POD is formed normal to the major principal axis. Thereafter, it is assumed that damage on the plane can occur with both shear and normal strains.
y
r s t
x z
POD Local and Global coordinate systems
Local damage surface
The constants r
and
are the strain equivalents of the material input parameters r
and r
c / f t
. The relative shear stress intercept to tensile strength ratio
where c is the shear stress intercept.
11. Fine integration and the nonsymmetric solver are always set by default with this material model.
12. It is recommended that the following LUSAS options are used with this model:
252 Suppress pivot warnings
62 Allow negative pivots
105
Chapter 3 LUSAS Data Input
Composite Matrix Failure Model
The Hashin composite damage model has been implemented within LUSAS to model matrix/fibre failure in composite materials. The model can be used with HX16C &
PN12C elements and linear material models MATERIAL PROPERTIES or
MATERIAL PROPERTIES ORTHOTROPIC SOLID. A set of failure criteria have been used to represent fibre and matrix failure. These failure criteria result in a degradation of the Young‟s modulus, shear modulus and Poisson‟s ratio where the damage has occurred.
DAMAGE PROPERTIES HASHIN imat Sxt Sxc Sxy Syt Syc T
where
imat
Sxt
Sxc
Sxy
Syt
Syc
T
Notes
Assignment reference number
Ply tensile strength in fibre direction
Ply compressive strength in fibre direction
Ply shear strength measured from a cross ply laminate
Ply transverse (normal to fibre direction) tensile strength
Ply transverse compressive strength
Reference Temperature
1. This damage model can only be used with the solid composite elements HX16C and PN12C
2. This model may only be used with linear material types MATERIAL
PROPERTIES and MATERIAL PROPERTIES ORTHOTROPIC SOLID.
3. Nonlinear material properties and creep cannot be used with this damage model.
4. All strength values specified are positive.
TwoPhase Material
The data chapter TWO PHASE MATERIAL allows the input of twophase material properties.
TWO PHASE MATERIAL iptm K s
K f
n
k
x
k y
k z
T
iptm
K s
K f
n
The twophase material identification number
Bulk modulus of solid phase (particle)
Bulk modulus of fluid phase
Porosity of medium
Unit weight of fluid phase
106
Nonlinear Material Properties k x k y k z
T
Notes
Permeability in global x direction
Permeability in global y direction
Permeability in global z direction (not used at present)
Reference temperature
1. Usually, the value of K
s
is quite large compared to K
f
and not readily available to the user. If K
s
is input as 0, LUSAS assumes an incompressible solid phase. K
f
is more obtainable, eg. for water K
f
= 2200 Mpa [N1]
2. Twophase material properties can only be assigned to geotechnical elements, that is, TPN6P and QPN8P.
3. When performing a linear consolidation analysis TRANSIENT CONTROL must be specified. DYNAMIC, VISCOUS or NONLINEAR CONTROL cannot be used.
4. In an undrained analysis twophase material properties may be combined with any other material properties, and creep, damage and viscoelastic properties under the
MATERIAL ASSIGNMENT data chapter. In a drained analysis only linear material properties may be used.
5. The twophase material properties are assigned to the twophase continuum elements using MATERIAL ASSIGNMENTS.
Rubber Material Properties
Rubber materials maintain a linear relationship between stress and strain up to very large strains (typically 0.1  0.2). The behaviour after the proportional limit is exceeded depends on the type of rubber (see diagram below). Some kinds of soft rubber continue to stretch enormously without failure. The material eventually offers increasing resistance to the load, however, and the stressstrain curve turns markedly upward prior to failure. Rubber is, therefore, an exceptional material in that it remains elastic far beyond the proportional limit.
Rubber materials are also practically incompressible, that is, they retain their original volume under deformation. This is equivalent to specifying a Poisson's ratio approaching 0.5.
107
Chapter 3 LUSAS Data Input
Hard Rubber
Soft Rubber
Rubber Material Models
The strain measure used in LUSAS to model rubber deformation is termed a stretch and is measured in general terms as: l = dnew/dold where:
dnew is the current length of a fibre
dold is the original length of a fibre
Several representations of the mechanical behaviour for hyperelastic or rubberlike materials can be used for practical applications. Within LUSAS, the usual way of defining hyperelasticity, i.e. to associate the hyperelastic material to the existence of a strain energy function that represents this material, is employed. There are currently four rubber material models available:
Ogden
MooneyRivlin
NeoHookean
Hencky
MATERIAL PROPERTIES RUBBER OGDEN N imat <
ri
ri
> i=1,N
k r
[
a
r
b r
T]
MATERIAL PROPERTIES RUBBER MOONEY_RIVLIN imat C
1
C
2
k r
[
a
r
b r
T]
MATERIAL PROPERTIES RUBBER NEO_HOOKEAN
108
Nonlinear Material Properties imat C
0
k r
[
a
r
b r
T]
MATERIAL PROPERTIES RUBBER HENCKY imat G k r
[
a
r
b r
T]
imat
The material property identification number
ri, ri Ogden rubber model constants
N
The number of pairs of constants for the Ogden rubber model
C1, C2
MooneyRivlin rubber model constants
C0
NeoHookean rubber model constant
G
kr
ar
br
Shear modulus
Bulk modulus (see Notes)
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
T
Reference temperature
The constants r, r, C1, C2 and C0 are obtained from experimental testing or may be estimated from a stressstrain curve for the material together with a subsequent curve fitting exercise.
The NeoHookean and MooneyRivlin material models can be regarded as special cases of the more general Ogden material model. In LUSAS these models can be reformulated in terms of the Ogden model.
The strain energy functions used in these models includes both the deviatoric and volumetric parts and are, therefore, suitable to analyse rubber materials where some degree of compressibility is allowed. To enforce strict incompressibility (where the volumetric ratio equals unity), the bulk modulus tends to infinity and the resulting strain energy function only represents the deviatoric portion. This is particular useful when the material is applied in plane stress problems where full incompressibility is assumed. However, such an assumption cannot be used in plane strain or 3D analyses because numerical difficulties can occur if a very high bulk modulus is used. In these cases, a small compressibility is mandatory but this should not cause concern since only nearincompressibility needs to be ensured for most of the rubberlike materials.
Rubber is applicable for use with the following element types at present:
2D Continuum QPM4M, QPN4M
3D Continuum HX8M
2D Membrane
BXM2, BXM3
109
Chapter 3 LUSAS Data Input
Notes
1. For membrane and plane stress analyses, the bulk modulus kr is ignored because the formulation assumes full incompressibility. The bulk modulus has to be specified if any other 2D or 3D continuum element is used.
2. Ogden, MooneyRivlin and NeoHookean material models must be run with geometric nonlinearity using either the total Lagrangian formulation (for membrane elements) or the corotational formulation (for continuum elements).
The Hencky material model is only available for continuum elements and must be run using the corotational formulation. The large strain formulation is required in order to include the incompressibility constraints into the material definition.
3. Option 39 can be specified for smoothing of stresses. This is particularly useful when the rubber model is used to analyse highly compressed plane strain or 3D continuum problems where oscillatory stresses may result in a "patchwork quilt" stress pattern. This option averages the Gauss point stresses to obtain a mean value for the element.
4. When rubber materials are utilised, the value of det F or J (the volume ratio) is output at each Gauss point. The closeness of this value to 1.0 indicates the degree of incompressibility of the rubber model used. For totally incompressible materials
J=1.0. However, this is difficult to obtain due to numerical problems when a very high bulk modulus is introduced for plane strain and 3D analyses.
5. Subsequent selection of variables for displaying will include the variable PL1 which corresponds to the volume ratio.
6. Rubber material models are not applicable for use with the axisymmetric solid element QAX4M since this element does not support the corotational geometric nonlinear formulation. The use of total Lagrangian would not be advised as an alternative.
7. There are no associated triangular, tetrahedral or pentahedral elements for use with the rubber material models at present.
8. The rubber material models are inherently nonlinear and, hence, must be used in conjunction with the NONLINEAR CONTROL command.
9. The rubber material models may be used in conjunction with any of the other
LUSAS material models.
Volumetric Crushing Model
Material behaviour can generally be described in terms of deviatoric and volumetric behaviour which combine to give the overall material response. The crushable foam material model accounts for both of these responses. The model allows you to define the volumetric behaviour of the material by means of a piecewise linear curve of pressure versus the logarithm of relative volume. An example of such a curve is shown in the diagram below, where pressure is denoted by p and relative volume by V/V
0
.
From this figure, it can also be seen that the material model permits two different unloading characteristics volumetrically.
110
Nonlinear Material Properties
Unloading may be in a nonlinear elastic manner in which loading and unloading take place along the same nonlinear curve
Volumetric crushing may be included in which unloading takes place along a straight line defined by the unloading/tensile bulk modulus K which is, in general, different from the initial compressive bulk modulus defined by the initial slope of the curve.
Volumetric crushing is indicated by the ivcrush parameter.
In both cases, however, there is a maximum (or cutoff) tensile stress pcut that is employed to limit the amount of stress the material may sustain in tension.
The deviatoric behaviour of the material is assumed to be elasticperfectly plastic. The plasticity is governed by a yield criterion that is dependent upon the volumetric pressure (compared with the classical von Mises yield stress dependency on equivalent plastic strain) and is defined as:
2 a
0
1
a p
2 where p is the volumetric pressure, t is the deviatoric stress and a
0
a
1
a
2
are user defined constants. Note that, if a
1
= a
2
= 0 and a
0
=
2 yld
/ 3
, then classical von Mises yield criterion is obtained.
MATERIAL PROPERTIES NONLINEAR 81 N imat K G
a
r
b r
h f
T pcut a
0
a
1
a
2
ivcrush < ln(V/V
0
) i
p i
> i=1,N
imat
The material property identification number
K
G
ar
br
Bulk modulus used in tension and unloading (see figure below)
Shear modulus
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
hf
T
Heat fraction coefficient (see Notes)
Reference temperature
pcut
Cutoff pressure (see Notes and figure below)
a0..etc Parameters defining pressure dependent yield stress (see Notes)
ivcrush Volumetric crushing indicator (see Notes):
0  no volumetric crushing
1  volumetric crushing.
111
Chapter 3 LUSAS Data Input
N
The number of points defining the pressurelogarithm of relative volume curve in compression
ln(V/Vo) i
Natural logarithm (loge, not log
10
) of relative volume coordinate for ith
pi point on the pressurelogarithm of relative volume curve (see Notes and figure below)
Pressure coordinate for ith point on the pressurelogarithm of relative volume curve (see Notes and figure below)
Notes
1. The heat fraction coefficient represents the fraction of plastic work which is converted to heat and takes a value between 0 and 1.
2. The pressurelogarithm of relative volume curve is defined in the compression regime hence logarithms of relative volume must all be zero or negative and the pressure coordinates must all be zero or positive.
3. The cutoff pressure should be negative (i.e. a tensile value).
4. Parameters a
0
and a
1
should be positive.
5. The volumetric crushing indicator effectively defines the unloading behaviour of the material. If there is no volumetric crushing, the same pressurelogarithm of relative volume curve is used in loading and unloading and if volumetric crushing takes place the alternative unloading/reloading curve is used (see figure below). pressure
Compression
K  Bulk m odulus
K  Bulk m odulus
Tension
ln (V/V0) cutoff pressure
Pressure  Logarithm of Relative Volume Curve
6. The yield surface defined is quadratic with respect to the pressure variable.
Therefore it can take on different conical forms (see figure below), either elliptic
(a2<0), parabolic (a2=0) or hyperbolic (a2>0). The parabolic form is comparable to the modified von Mises material model while the elliptic form can be considered to be a simplification of the critical state soil and clay material behaviour. For all
112
Nonlinear Material Properties
values of a2 the yield criterion is taken as a
0
when p is ve (tension). For an elliptic surface (a2<0) the square of the yield stress is maintained at a constant maximum value (a0a12/4a2) when the compressive pressure exceeds a1/2a2.
hyperbolic a
2
>0 parabolic a
2
=0
a
0
a
0
a
2
1
/ 4 a
2 elliptic a
2
< 0
ve = tension P max
=a
1
/2a
2
Yield Surface Representation For Different a
2
Values
7. The relationship between the elastic modulus values in shear, G, and tension, E, assuming small strain conditions, is given by:
G
E
8. The relationship between the elastic bulk (or volumetric) modulus, K, and tensile modulus, E, is given by:
K
E
Concrete Creep Models
LUSAS accommodates two concrete creep codes, CEBFIP Model Code 1990 and the
Chinese Creep Code for Dams. The CEBFIP model is valid for ordinary structural concrete (1280 Mpa) that has been loaded in compression to less than 40% of its compressive strength at the time of loading. Relative humidities in the range 40100% and temperatures in the range 530 degrees C are assumed.
Although CEBFIP Model Code 1990 is only applicable to beams, it has been extended in LUSAS to cover multiaxial stress states. The assumptions made in the derivation of this extension can be found in the LUSAS Theory Manual.
113
Chapter 3 LUSAS Data Input b r
H f
T
a r
imat
E
MATERIAL PROPERTIES NONLINEAR 86 [CEBFIP  CHINESE]
,
,
, a r
, b r
, H f
, T, [f r f
1
, g
1
, p
1
, r
1
, f
2
, g
2
, p
2
, r
2
, f
3
, r
3
, C
] t
, RH, hr  a, b,
The material property identification number
Modulus of elasticity:
CEBFIP = E ci
= modulus at 28 days (see Notes)
Chinese =
E
= long term modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping coefficient (not used)
Stiffness Rayleigh damping coefficient (not used)
Heat fraction (not used)
Reference temperature
CEBFIP: f
r fcm/fcmo where fcm is the mean concrete compressive strength at 28 days and fcmo is a reference strength which is the equivalent of 10 Mpa in the chosen units.
C t
RH
h r
Cement type (default=2, see Notes)
Relative humidity (%) of the ambient environment (default = 70%) h/ho where h is the nominal member size (see Notes) and ho is a reference
Chinese:
length which is the equivalent of 100mm in the chosen units.
a,b
Parameters for controlling evolution of elastic modulus with time (see
f ,g
p ,r
Notes)
Parameters for controlling variation of creep coefficient with time (see
Notes)
Parameters for controlling variation of creep coefficient with time (see
Notes)
Notes
1. The CEBFIP Code states that the modulus of elasticity at 28 days may be estimated from
E ci
x
4
x
f cm
1/ 3
10
2. In the CEBFIP code, the cement type C
t
is defined as:
114
Nonlinear Material Properties
1 for slowly hardening cements SL
2 for normal or rapid hardening cements N and R
3 for rapid hardening high strength cements RS
3. In the CEBFIP code, the nominal size of member, h, is computed from 2
A c
/ u
where A
c
is the area of cross section and u the length of the perimeter of the cross section that is in contact with the atmosphere. It should be noted that the CEBFIP code has only been written to cover a uniaxial stress state (beams). The equations in CEBFIP have been extended in LUSAS to cover multiaxial stress states, however, an appropriate value for hr must still be defined.
4. In the Chinese code, the evolution of elastic modulus with time is defined by:
E
E
1
e
a
b
where
E
, a and b are parameters fitted from experimental data
5. In the Chinese code, the variation of creep coefficient with time is defined by:
t
,
C
f
1
g
1
p
1
1
e
f
2
g
2
p
2
1
e
r
3
1
e
where f
i
, g
i
, and p
i
, r
i
are parameters fitted from experimental data.
6. In the Chinese code, parameters a, b and p parameters r
i i
are assumed to be dimensionless while
are inverted retardation times and are therefore specified in days
1
.
Parameters f
i
and g
i
take the units of (
E)
1 .
7. The creep models must be run with NONLINEAR CONTROL and VISCOUS
CONTROL. The time steps and total response time must be specified in days. An option exists under the INCREMENTATION chapter of VISCOUS CONTROL to use an exponent to increase the time step as the analysis progresses.
8. These material models can be combined with SHRINKAGE PROPERTIES CEB
FIP_90 to combine the effects of creep and shrinkage.
Generic Polymer Model
The polymer material model is defined using an linear spring an Eyring damper and a number of parallel Maxwell elements. Model 88 is used when behaviour differs in tension and compression.
MATERIAL PROPERTIES NONLINEAR 87 n imat <G i
i
> i=1,n
A t
t
T G spr
K
MATERIAL PROPERTIES NONLINEAR 88 n imat <<G i
i
> i=1,n
A t
K
a r
b r
T t
, G spr
> ten
<<G i
i
> i=1,n
A t
t
G spr
>> comp
115
Chapter 3 LUSAS Data Input
n
imat
G i
i
A t
t
T
G
spr
ten comp
K
a r b r
Number of Maxwell elements
Material property identification number
Shear modulus of spring in i‟th Maxwell element
Maxwell element Newtonian dashpot viscous parameter
Constant related to the activation energy of the Eyring dashpot
Activation volume of the Eyring dashpot
Reference temperature
Shear modulus of external spring
Properties in tension
Properties in compression
Bulk Modulus
Density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
If some of the units are not required for a particular analysis, the material parameters for these should be defined as zero.
Notes
1. NONLINEAR CONTROL with VISCOUS or DYNAMIC CONTROL should always be specified with this material model.
2. The number of Maxwell elements, n, has no restriction although the model requires at least one Maxwell element to be specified.
3. The bulk modulus, K, can be evaluated from values of Young‟s Modulus and
Poisson ratio.
4. The Eyring parameters, A
t
,
t, can be set to zero for a reduction to a linear viscoelastic material.
5. The reference temperature is for future use and has no bearing on the model.
6. The density should be specified if DYNAMIC CONTROL is used.
7. The external spring can be removed by setting G
spr
to zero.
Generic Polymer Model with Damage
The polymer material model with damage consists of a linear spring, a spring that includes damage, an Eyring dashpot and a number of parallel Maxwell elements.
Different sets of material properties can be defined to model tensile and compressive behaviour, except for the ViscoScram damage model whose properties apply in both tension and compression.
116
Nonlinear Material Properties
Model 90 (see below) includes two additional features. The first feature is a set of failure criteria that are used to remove individual Maxwell elements when the criteria are met. The second is a switch between tensile and compressive material properties based on the stress state in an individual Maxwell element.
MATERIAL PROPERTIES NONLINEAR 89 n imat
<<G i
i
> i=1,n
A t
idam {a c K q i t o
m V
> i=1,ntpfc
<e i c t
G spr
> ten
<<G i
q i max c
c max
s i
> i=1,n
A t
t
G spr
> comp
 itdam ntpfc icdam ncpfc <e
> i=1,ncpfc
} icrit s u ten
e u ten
s u
comp
e u
comp i t
c
1 c
2
c
3
c
4
c
5
c
6
c
7
c
8
K
a r
b r
T
MATERIAL PROPERTIES NONLINEAR 90 n imat
<<G i
i
> i=1,n
A t
t
G spr
> ten
<<G i
i
> i=1,n
A t
t
G spr
> comp idam {a c K o
m V max
c max
s
 itdam ntpfc icdam ncpfc <e i t q i t
> i=1,ntpfc
<e i c
q i c
> i=1,ncpfc
 a c K o
m y min
er min
y max
er max c max
s
} icrit s u ten
e u ten
K
a r
b r
T iswtch
s u
comp
e u
comp
c
1
c
2
c
3
c
4
c
5
c
6
c
7
c
8
n
imat
G i
i
i
A t
t
G spr ten comp idam
Number of Maxwell elements
Material property identification number
Shear modulus of spring in i‟th Maxwell element
Viscous constant of Newtonian dashpot in i‟th Maxwell element
Retardation time of Newtonian dashpot for i‟th Maxwell element
Constant related to the activation energy of the Eyring dashpot
Activation volume of the Eyring dashpot
Shear modulus of external spring
Properties in tension
Properties in compression
Damage model
=1 ViscoScram model with constant V max
=2 Strainbased damage model
=3 ViscoScram model with strain rate dependant V max
Visco Scram damage model with constant V max
(idam=1)
a
c
K o
Initial flaw size
Average crack growth
Threshold value of stress intensity
117
Chapter 3 LUSAS Data Input
m
V max c max
s
Cracking parameter
Maximum value of rate of growth of average crack radius
Maximum crack length
Static coefficient of friction
Strainbased damage model (idam=2)
itdam
Tension function identifier
=1 User defined
=2 No damage
ntpfc
Number of points on damage curve for tensile damage function
icdam
Compression function identifier
=1 User defined
=2 No damage
ncpfc
Number of points on damage curve for compressive damage function
e q i i
xcoordinate of damage function
ycoordinate of damage function (“Q”)
Visco Scram damage model with strain rate dependant V max
(idam=3)
a
c
K o
m
Initial flaw size
Average crack growth
Threshold value of stress intensity
y min er min y max
Cracking parameter
The value
max
min
(see notes)
The value
The value
min
(see notes) max
max
(see notes)
er max c max
s
The value
max
(see notes)
Maximum crack length
Static coefficient of friction
Failure properties
icrit
Failure criteria
= 1 Maximum shear stress criterion
= 2 Von Mises criterion
= 3 Maximum normal stress criterion
= 4 Mohr‟s theory
= 5 Maximum strain theory
= 6 Critical strain theory
s u ten
Ultimate stress in tension
e s e u ten u comp u comp
Ultimate strain in tension
Ultimate stress in compression
Ultimate strain in compression
c
1
Gradient of ultimate stress vs. log e
(effective strain rate) graph (tension)
118
Nonlinear Material Properties c c c
2
3
4
Intercept of ultimate stress vs. log e
(effective strain rate) graph with ultimate stress axis (tension)
Gradient of ultimate strain vs. log e
(effective strain rate) graph (tension)
Intercept of ultimate strain vs. log e
(effective strain rate) graph with ultimate strain axis (tension)
c c
5
6
Gradient of ultimate stress vs. log e
(effective strain rate) graph
(compression)
Intercept of ultimate stress vs. log e
(effective strain rate) graph with ultimate stress axis (compression)
Gradient of ultimate strain vs. log e
(effective strain rate) graph
c
7 c
8
(compression)
Intercept of ultimate strain vs. log e
(effective strain rate) graph with ultimate strain axis (compression)
Generic properties
K
a r
Bulk Modulus
Density
Coefficient of thermal expansion
Mass Rayleigh damping constant
b r
T
Stiffness Rayleigh damping constant
Reference temperature
Iswtch Tensile/compressive material property switch
=0 switch on mean stress
=1 switch on individual Maxwell element
Notes
1. NONLINEAR CONTROL with either VISCOUS or DYNAMIC CONTROL should always be specified when using this material model.
2. At least one Maxwell element must be specified. However, there is no upper limit to n, the number of Maxwell elements.
3. The Newtonian damper in any Maxwell element can be turned off. For Model 89 this is achieved by setting the Maxwell element‟s viscous constant,
i
, to zero, while for Model 90 the retardation time,
i
, must be set to zero. The Maxwell element will then behave as a spring in parallel with the other Maxwell elements.
4. The strain rate across the Eyring dashpot is related to the Eyring parameters via the equation
eyr
A sinh
where
e
is the effective deviatoric stress.
5. The Eyring parameters, A t
and
t
, can be set to zero to remove the effect of the
Eyring dashpot.
119
Chapter 3 LUSAS Data Input
6. Properties for the Maxwell elements and the Eyring dashpot must be specified for both tension and compression.
7. There are two ViscoScram damage models, idam=1,3. With idam=1 a constant value for V max
is used, whilst with idam=3 a loglog relationship between V max and the strain rate is used (see below).
8. For the Viscoscram damage model that uses a strain rate dependent V max
(idam=3), the following relationship between V max
and the effective strain rate,
, applies.
max
max
min
max ln
max
max
ln V ln
max min
min
ln
ln
min
where
V max
min
Maximum rate of growth of the average crack radius, V max
, at the minimum valid strain rate,
min
V max
max
Maximum rate of growth of the average crack radius, V max
, at the maximum valid strain rate
max
min
Minimum effective strain rate at which the loglog
max relationship with V max
is valid
Maximum effective strain rate at which the loglog relationship with V max
is valid
The relationship between V max
and
applies in the range value of
max
max
is bounded as follows. ln V max
min
for
min
min
max
max
max
max
for
max
. The
The relationship between V max
and
is shown as a graph in the figure below.
120
Nonlinear Material Properties
ln V max
ln V max
max
ln V max
min
ln
min
) ln
max
) ln
9. The damage deviatoric strain in both ViscoScram damage models (idam=1,3) is defined as e dam ij
ij and the damage deviatoric strain rate is defined as e dam ij
2
3 c c s
2G
a
1 c
3 s ij
G where
G
is the sum of the Maxwell shear modulii.
10. If no damage is required with the ViscoScram damage models (idam=1,3), the value for a, the initial flaw size, should be set to zero.
11. For the ViscoScram damage models (idam=1,3) only one set of damage properties is specified to cover both tensile and compressive cases.
12. With failure, if any of the terms c
1
c
8
are nonzero then the ultimate stresses and strains, s u
and e u
, in tension and compression are computed from the following equations. s ten u
s comp u
c
2
c
6 e ten u
e comp u
c
4 c
8
is the effective strain rate, ten indicate tensions and comp indicates compression. The values computed above override any specification for s u
and e u in the data input. The sign convention for the data input is that the ultimate stresses/strains in tension are positive and in compression are negative.
The terms c
1
 c
8
are determined from graphs of ultimate stress/strain vs. the natural logarithm of the strain rate in tension and compression. The figure below
121
Chapter 3 LUSAS Data Input
shows an example for the ultimate stress in tension. The graph shows the quantities c
1
and c
2
that define the relationship between s u ten
and ln
. s ten u
gradient = c
2 c
1 ln
13. The bulk modulus, K, can be computed from standard isotropic relations using the
Young‟s Modulus, E, and the Poisson ratio,
, of the material.
K
E
2
14. The density,
, must be specified if DYNAMIC CONTROL is used.
15. The parameter iswtch determines when a switch between tensile and compressive material properties occurs. With iswtch=0, the criteria is based on the mean stress. With iswtch=1, each Maxwell element has its tensile/compressive material properties selected based on the stress state within that Maxwell element.
16. The units of some GPM variables can be expressed in base dimensions M (mass),
L (length), T (time) and
(temperature).
GPM unit
Maxwell
Eyring
ViscoScram
Generic
Parameter
G i
A t a c
K
0 m
K
Miscellaneous Stress
Units
M.L
1
.T
2
T
1
L
L
M.L
1/2
.T
2
Parameter Units
i
t
T
M
1
.L.T
2
L.T
1
V max c max
s
L
Dimensionless
Dimensionless
M
1
.L.T
2 a r
M.L
3 b r
1/
T
M.L
1
.T
2
Strain rate
Dimensionless
Dimensionless
T
1
122
Nonlinear Material Properties
GPM unit Parameter Units
Strain Dimensionless
Parameter Units
2D ElastoPlastic Interface Model
The elastoplastic interface models may be used to represent the frictioncontact relationship within planes of weakness between two discrete 2D bodies. The model is available in plane stress and plane strain elements (see the LUSAS Element Reference
Manual), a line of which must lie between the two bodies in the finite element discretisation.
The elastic material properties are defined in the local basis, permitting differing values to be specified normal and tangential to the plane of the interface. The nonlinear behaviour is governed by an elastoplastic constitutive law, which is formulated with a limited tension criterion normal to the interface plane, and a MohrCoulomb criterion tangential to the interface plane.
The data section MATERIAL PROPERTIES NONLINEAR 27 is used to define the material properties for the 2D elastoplastic interface model.
MATERIAL PROPERTIES NONLINEAR 27 imat E in
E out
G
a
r
b r
h f
T c
y
imat
E in
E out
G
ar
br
hf
T
c
y
Notes
The material property identification number
Young‟s modulus inplane
Young‟s modulus outofplane
Shear modulus
Poisson‟s ratio
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Heat fraction coefficient (see Notes)
Reference temperature
Cohesion
Friction angle
Uniaxial yield stress
1. The model cannot be used within a geometrically nonlinear analysis.
2. The tangential (inplane) direction is in the element x direction and the normal (out of plane) is in the element h direction. The x direction is defined from the vector between nodes 1 and 3 in the following diagram:
123
Chapter 3 LUSAS Data Input
7
5
6
8
4
1
2
3
3. The heat fraction coefficient represents the fraction of plastic work which is converted to heat and takes a value between 0 and 1. For compatibility with pre
LUSAS 12 data files specify Option 235.
3D ElastoPlastic Interface Model
The elastoplastic interface models may be used to represent the frictioncontact relationship within planes of weakness between two discrete 3D bodies. The model is available in solid continuum elements (see the LUSAS Element Reference Manual), a line of which must lie between the two bodies in the finite element discretisation.
The elastic material properties are defined in the local basis, permitting differing values to be specified normal and tangential to the plane of the interface. The nonlinear behaviour is governed by an elastoplastic constitutive law, which is formulated with a limited tension criterion normal to the interface plane, and a MohrCoulomb criterion tangential to the interface plane.
The data section MATERIAL PROPERTIES NONLINEAR 26 is used to define the material properties for the 3D elastoplastic interface model.
imat
Ein
Eout
Gin
Gout
in
out
MATERIAL PROPERTIES NONLINEAR 26 imat E in
E out
G in
G out
in
out
a
r
b r
h f
T c
y
The material property identification number
Young‟s modulus inplane
Young‟s modulus outofplane
Inplane shear modulus
Outofplane shear modulus
Inplane Poisson‟s ratio
Outofplane Poisson‟s ratio
124
Nonlinear Material Properties
ar
br
hf
T
c
y
Notes
Mass density
Coefficient of thermal expansion
Mass Rayleigh damping constant
Stiffness Rayleigh damping constant
Heat fraction coefficient (see Notes)
Reference temperature
Cohesion
Friction angle
Uniaxial yield stress
1. The model cannot be used within a geometrically nonlinear analysis
2. The tangential (inplane) direction lies in the element xh plane and the normal
(out of plane) in the element z direction.
7
8
6
5
3
4
1
2
3. The heat fraction coefficient represents the fraction of plastic work which is converted to heat and takes a value between 0 and 1. For compatibility with pre
LUSAS 12 data files specify Option 235.
Delamination Interface Properties
The nonlinear material model 25 is used to define the delamination interface properties
MATERIAL PROPERTIES NONLINEAR 25 idim imat (Gi
t
i mode) i=1,idim
where
idim
imat number of dimensions of model (IPN6 =2, IS16 = 3) material number
125
Chapter 3 LUSAS Data Input
G i
t
i
mode critical fracture energy tension threshold/interface strength maximum relative displacement unloading model
1  reversible unloading
2  unloading on secant towards origin
3  coupling model
Notes
1. It is recommended that the arc length procedure is adopted with the option to select the root with the lowest residual norm OPTION 261
2. It is recommended that fine integration is selected for the parent elements using
OPTION 18
3. The nonlinear convergence criteria should be selected to converge on the residual norm.
4. OPTION 62 should be selected to continue if more than one negative pivot is encountered and OPTION 252 should be used to suppress pivot warning messages from the solution process.
5. The nonsymmetric solver is selected automatically when mixed mode delamination is specified.
6. The critical fracture energies should be the measured GIc, and GIIc
7. The tension threshold /interface strength is the stress at which delamination is initiated. This should be a good estimate of the actual delamination tensile strength but, for many problems the precise value has little effect on the computed response. If convergence difficulties arise it may be necessary to reduce the threshold values to obtain a solution.
8. The maximum relative displacement is used to define the stiffness of the interface before failure. Provided it is sufficiently small to simulate an initially very stiff interface it will have little effect. Typically its value should be defined as 10 7.
9. Although the solution is largely independent of the mesh discretisation, to avoid convergence difficulties it is recommended that a least two elements are placed in the process zone.
Resin Cure Model
This model is used for predicting the deformations of thermoset composites that occur during a hot cure manufacturing process. The effects of chemical shrinkage (via
SHRINKAGE PROPERTIES) and thermal expansion are accounted for along with the evolution of material properties during the cure cycle. This facility is intended for use within the framework of a semicoupled thermomechanical analysis. However, a simplified solution without thermomechanical coupling can be computed for the situation in which the cure proceeds uniformly within a part by prescribing the resin
126
Nonlinear Material Properties
state plus accompanying shrinkage, at discrete points within the cure process. To fully utilise this model the High Precision Moulding product is required.
Either layer or basic fibre/resin properties can be entered. Properties are required in both the glassy and rubbery states. Additionally, properties in the liquid state are required for layer properties. The basic fibre/resin properties are fed into a micromechanics analysis to produce the corresponding layer values. Full laminate values may also be entered.
MATERIAL PROPERTIES NONLINEAR CURE LAYER [DIBENEDETTO 
GENERAL  USER ] [npnts] [nstate]
Imat
33
G
E
22
R
E
33
R
E
11
G
E
22
G
11
G
22
G
G
12
R
G
E
33
G
G
12
G
G
23
G
G
13
G
33
G
23
R
G
13
R
12
R
23
R
13
R
12
G
23
G
11
R
22
R
22
R
G
23
L
G
33
R
13
L
12
L
23
L
13
L
11
L
22
L
33
L
E
11
L
13
G
11
G
22
G
11
L
E
22
L
22
L
33
R
E
33
L cGel
a r
b r
< f i
> i=1,npnts
33
L
E
11
R
G
11
R
12
L
MATERIAL PROPERTIES NONLINEAR CURE FIBRE_RESIN
[DIBENEDETTO  GENERAL  USER ] [npnts] [nstate] imat
mat
G
E fib1
E fib2
E mat
R
mat
R
G fib12
G fib23
mat
R
cGel
fib
fib1
fib2
fib
E mat
G
mat mat
a r
b r
ftype WarpU
FillU FibH FibW Wc Fc Acl nGP Atype
> i=1,npnts
G
< f i
DIBENEDETTO DiBenedetto glass transition model, see Notes
GENERAL
Piecewise linear description of glass transition temperature, see
USER
Notes
User defined glass transition function, see Notes
*
G
*
R
glassy property rubbery property
*
L
liquid property
npnts number of data parameters which define glass transition equation
(not required if a glass transition function is not declared)
nstate number of user state variables (minimum of 1 if user model
imat
E
E
E ii fib1 fib2
specified)
The material property identification number
Young‟s modulus of the laminar in the longitudinal, transverse and thickness directions.
Young‟s modulus of the fibre in the longitudinal direction
Young‟s modulus of the fibre in the transverse direction
127
Chapter 3 LUSAS Data Input
E mat
G ij
G fib12
G fib23
G mat
ij fib
mat
ii
Young‟s modulus of the matrix
Shear moduli for the laminar
Shear modulus along fibre
Shear modulus across fibre
Shear modulus of the matrix
Poisson‟s ratios of the laminar
Poisson‟s ratio of the fibre
Poisson‟s ratio of the matrix
fib1
fib2
mat
ii
cGel
mat a r
degree of cure at which matrix gels
Mass density of the laminar
Mass density of the resin
Rayleigh mass damping constant
b r
Rayleigh stiffness damping constant
ftype
Fabric type, see Notes
WarpU
Warp undulation fraction (recommended 1.0)
FillU
Fill undulation fraction (recommended 1.0)
FibH
Fibre height fraction of layer height (recommended 1.0)
FibW
Wc
Fibre width fraction (recommended 1.0)
Warp count, fibre bundles per unit length in the warp direction
Fc
Acl
Fill count, fibre bundles per unit length in the weft direction
Aerial density of the fabric
nGP
Number of Gauss points (111) (recommended 8)
Atype
Woven fabric analysis type (1 = isostrain (recommended), 2 =
< f i
>
Coefficients of thermal expansion in the longitudinal, transverse and thickness directions of the laminar
Coefficients of thermal expansion along the fibre
Coefficients of thermal expansion across the fibre
Coefficient of thermal expansion of the matrix
Coefficients of shrinkage, with respect to degree of cure, in the isostress)
Functional values which depend on the form of the Glass transition equation selected, see Notes
Notes
1. The resin cure models are intended for use with the High Precision Moulding product.
2. These models are utilised in a thermomechanical coupled analysis where the degree of cure is computed in the thermal analysis.
3. The shrinkage of the resin is introduced via the SHRINKAGE PROPERTIES
GENERAL or USER chapters.
128
Nonlinear Material Properties
4. No glass transition function need be entered if the material states are defined using the STATE command in VISCOUS CONTROL.
5. The following options are available for ftype, the fabric type.
6
7
4
5 ab
2
3
ftype
1
Description
Plain
Leno
Mock Leno
ftype
8
9
10
Description
Satin 5H
Satin 8H
Satin 12H
Twill 2x1
Twill 3x1
11
12
Basket 2x2
Basket 4x4
Twill 2x2 13 Basket 8x8
Twill 4x4 14 0/90 UD (noncrimp)
UD Tape where „a‟ is the mechanical model and „b‟ the thermal model. For example to use the CCA model to define the mechanical properties and Chamis the thermal „ab‟ = „215‟
4
5
6
a
1
2
3
Mech.Model
Rule of mixtures
CCA
Puck
Chamis
Halpin Tsai (circ)
Halpin Tsai (rect)
b Therm.Model
11 Rule of mixtures
12 CCA
13 Schneider
14 Shapery
15 Chamis
16 Chamberlain (hexag)
17 Chamberlain (square)
6. The functional values which depend on the form of the Glass transition equation selected are defined as follows
DiBenedetto equation, npnts=3 f
1
= TgI glass transition temperature of fully cured polymer f
2
= Tg0 glass transition temperature before cure lambda = material parameter
General piecewise linear, npnts = number of points defining linear sections
< DOC i
Tg i
> i=1,npnts
DOC degree of cure, Tg glass transition temperature
User equation defined via user interface, npnts=number of user input parameters
< f i
> i=1,npnts
where
129
Chapter 3 LUSAS Data Input
f
1
= LTGUSR – identifier passed into user routine fi (i=2,npnts) = parameters passed to user routine
7. The User defined glass transition function is introduced via externally developed
FORTRAN source code. Source code access is available to interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised. Contact LUSAS for full details of this facility.
8. A minimum data solution is available which is applicable to thin composites in which the state of cure is constant or nearly constant at every point. This approach requires use of the STATE command in VISCOUS CONTROL and does not involve a coupled analysis.
9. The coupled analysis solution requires the use of NONLINEAR CONTROL in both the thermal and structural analysis. The thermal analysis also requires the
TRANSIENT CONTROL chapter and the structural analysis VISCOUS
CONTROL. A semicoupled analysis with data transfer at every time step should be used.
Shrinkage
The cure of concrete and thermoset resins is accompanied by an isotropic shrinkage which in concrete‟s case depends on time, temperature and other environmental factors whilst for thermoset resins the shrinkage is normally described with respect to its degree of cure. LUSAS provides for the shrinkage of concrete using equations defined in the design code CEB FIP 90 and also a more general routine in which shrinkage is defined using a piecewise linear curve. Using the latter, shrinkage can be a function of either time or degree of cure. Additionally a user facility is available which provides a means of interfacing LUSAS with externally developed code.
Shrinkage Properties CEBFIP 90
SHRINKAGE PROPERTIES CEB_FIP_90
fr
ishr C t
RH h r
f r
ishr
Ct
RH
hr
Shrinkage property identification number
Cement type (see notes)
Relative humidity (%) of the ambient environment h/h o
where h is the nominal member size (see notes) and h o is the equivalent of 100mm in the chosen units. f cm
/f cmo
where f cm
is the mean concrete compressive strength at 28 days and f cmo
is a reference strength which is the equivalent of 10 MPa in the chosen units.
Notes
1. The cement type, Ct, is defined as:
130
Nonlinear Material Properties
1 for slowly hardening cements SL
2 for normal or rapid hardening cements N and R
3 for rapid hardening high strength cements RS
2. The nominal size of member, h, is computed from 2Ac/u where Ac is the area of cross section and u the length of the perimeter of the cross section that is in contact with the atmosphere. The CEBFIP Model Code 1990 is only strictly applicable to a uniaxial stress state but the law has been extended in LUSAS to accommodate multiaxial stress states. Care should be taken when estimating a value to use for h when applying CEBFIP shrinkage to concrete members that are not beamlike in nature. In general, the larger the value for h, the longer the time taken for shrinkage strains to reach a final value; for large values of h, it must be decided whether this behaviour is reasonable. An illustration of the effect on shrinkage of varying the input parameter hr is shown below. As CEBFIP creep and shrinkage input parameters can be defined separately, it is possible, if necessary, to use different hr values for creep and shrinkage on the same assignment.
3. The CEBFIP shrinkage model can be used with the CEBFIP creep model.
4. Shrinkage is calculated from the time of activation of the element.
Shrinkage Properties General
SHRINKAGE PROPERTIES GENERAL [TIME  DEGREE_OF_CURE] npnts ishr < f i
V s i
> i=1.npnts
131
Chapter 3 LUSAS Data Input
TIME
Interpolate linear shrinkage using time measured from the element‟s activation
Degree_of_cure
Interpolate linear shrinkage from degree of cure
npnts
Number of points defining piecewiselinear linear shrinkage curve
fi time or degree of cure at point i
Vsi
Notes
Linear shrinkage at time/degree of cure at point i.
1. The linear shrinkage value V
s i
is the shrinkage in the coordinate direction. It is applied equally in the x, y and z coordinate directions according to the particular element stress type.
2. The degree of cure is calculated from a coupled thermal analysis which takes account of the variation of temperature throughout the model.
3. Shrinkage is calculated from the time of activation of the element. That is the interpolation time is taken to be zero on activation.
Shrinkage Properties User
The SHRINKAGE PROPERTIES USER facility provides routines for implementing a user supplied shrinkage model to be invoked from within LUSAS. This facility provides completely general access to the LUSAS property data input via this data section and controlled access to the presolution processing and nonlinear state variable output.
Source code access is available to interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised.
Contact LUSAS for full details of this facility. Since user specification of a shrinkage model involves the external development of source FORTRAN code, as well as access to LUSAS code, this facility is aimed at the advanced LUSAS user.
SHRINKAGE PROPERTIES USER lstp nprzs nstat ishr < f i
> i=1,nprzs lstp
User defined shrinkage model identification number
nprzs
Number of parameters used in definition of shrinkage model
nstat
Number of shrinkage state variables (see Notes)
fi
Notes
User supplied parameters for shrinkage model
1.
nstat must be an integer greater than zero
2. The number of damage properties input must be equal to that specified on the data section header line (i.e. nprzs).
3. Option 179 can be set for argument verification within the user routines
132
Field Material Properties
Field Material Properties
The following section contains field element material properties, one of which must be defined for each field element; these material properties are not applicable to any other element type. The following types of field material properties are available:
Isotropic Field Model
Orthotropic Plane Field Model
Orthotropic Solid Field Model
If temperature dependent material properties are specified, the linear problem becomes nonlinear and NONLINEAR CONTROL will need to be specified to obtain a correct solution. TEMP and TMPE loading may be used to provide an initial thermal field for the evaluation of temperature dependent properties. Further iterations will use the evaluated thermal field.
Note that for temperature dependent thermal boundary conditions, such as radiation, it is computationally more efficient to use thermal links to model the boundary heat transfer than to apply it directly to the elements as a load type.
Isotropic Field Model
The isotropic field model may be used to represent field properties which are identical in each direction. The data section MATERIAL PROPERTIES FIELD ISOTROPIC is used to specify the material properties for the isotropic field model.
MATERIAL PROPERTIES FIELD ISOTROPIC n imat k T [C H]
imat
n
k
T
C
H
Notes
The material property identification number
Phase change type:
=0 Phase change not required (default)
=1 Del Giudice
=2 Lemmon
Thermal conductivity
Reference temperature
Specific heat coefficient
Enthalpy
1. The specific heat coefficient(s) must be multiplied by the density prior to input.
2. Isotropic field properties are applicable to all field elements except thermal links
(see the LUSAS Element Reference Manual).
3. It is recommended that Option 105 (lumped specific heat) is used with phase change analyses.
4. Specific heat coefficient is only required for transient analyses.
133
Chapter 3 LUSAS Data Input
5. Enthalpy is only required for phase change analyses.
Plane Orthotropic Field Model
The data section MATERIAL PROPERTIES FIELD ORTHOTROPIC is used to define the material properties for the plane orthotropic field model. The model is valid for 2D plane field problems.
MATERIAL PROPERTIES FIELD ORTHOTROPIC n imat k x
k y
T [C H]
imat
n
The material property identification number
Phase change type:
=0 Phase change not required (default)
=1 Del Giudice
=2 Lemmon
kx, ky
Thermal conductivity in x and y directions
angle of orthotropy (degrees) relative to global Xaxis (positive in an anticlockwise direction)
Reference temperature.
T
C
H
Notes
Specific heat coefficient (only required for transient analysis).
Enthalpy (only required for phase change analysis).
1. The specific heat coefficient(s) must be multiplied by the density prior to input.
2. It is recommended that Option 105 (lumped specific heat) is used with phase change analyses.
Orthotropic Solid Field Model
The data section MATERIAL PROPERTIES FIELD ORTHOTROPIC SOLID is used to define the material properties for orthotropic solid field problems. The model is valid for 3D solid field problems.
MATERIAL PROPERTIES FIELD ORTHOTROPIC SOLID n imat nset k x
k y
k z
T [C H]
imat
n
The material property identification number
Phase change type:
nset
=0 Phase change not required (default)
=1 Del Giudice
=2 Lemmon
CARTESIAN SET number used to define local axes direction. If nset=0, the local axes coincide with global axes.
kx, ky, kz Thermal conductivity in x, y and z directions
134
Field Material Properties
T
C
H
Reference temperature.
Specific heat coefficient (only required for transient analysis).
Enthalpy (only required for phase change analysis).
Notes
1. The specific heat coefficient(s) must be multiplied by the density prior to input.
2. It is recommended that Option 105 (lumped specific heat) is used with phase change analyses.
Isotropic Concrete Heat of Hydration Model
The data section MATERIAL PROPERTIES FIELD ISOTROPIC CONCRETE is used to define the heat of hydration for different concrete types. This depends on the chemical composition of the cement. Cement types I, II, III and V are catered for. Note that cement type IV is no longer widely used as admixtures tend to be used instead, therefore no data is available for this type. Provision has been made for a user defined chemical composition which is defined as cement type VI.
MATERIAL PROPERTIES FIELD ISOTROPIC CONCRETE n imat k T C H icem wcem wcra wslg wpfa pfacao Tr conv itime
[C3S C2S C3A C4AF FreeCaO SO3 MgO Blaine]
imat
n
nset
The material property identification number
Phase change type:
=0 Phase change not required (default)
=1 Del Giudice
=2 Lemmon
CARTESIAN SET number used to define local axes direction. If nset=0, the local axes coincide with global axes.
kx, ky, kz Thermal conductivity in x, y and z directions
T
Reference temperature.
C
Specific heat coefficient (only required for transient analysis).
H
icem
Enthalpy (only required for phase change analysis).
Cement type (1= Type I, 2= Type2 II, 3= Type III, 5=Type V, 6=user
wcem
wcra defined)
Weight of cement per unit volume (must be defined in kg/m
3
)
wslg
wpfa
Water/cementitious ratio (weight of water per unit volume/(wcem+wslg+wpfa))
Weight of GGBF slag per unit volume (must be defined in kg/m
3
)
Weight of fly ash per unit volume (must be defined in kg/m
3
)
135
Chapter 3 LUSAS Data Input
pfacao CaO content of fly ash (defined as %) Values usually lie in the range 2
30%, class C fly ash = 24% and class F = 11%
Tr
conv
Temperature at which concrete is assumed to cure (degrees C)
Factor to convert heat (computed in J/m
itime
Time unit identifier (1=hrs,2=days)
3
) to model unit system
C3S
C2S
User defined C
User defined C
3
2
S content (defined as %)
S content (defined as %)
C3A
C4AF
User defined C
3
A content (defined as %)
User defined C
4
AF content (defined as %)
FreeCaO User defined Free CaO content (defined as %)
SO3
User defined SO
3
content (defined as %)
MgO
User defined MgO content (defined as %)
Blaine
User defined Blaine index (must be defined in m
2
/kg)
Notes
1. The time step and any termination response times must be specified in hours or days. If the timescale is in days; the thermal conductivity and heat transfer coefficients should be defined wrt days, i.e. J/day/m.C and J/day/m
2
.C.
2. The parameters C3S, C2S, C3A, C4AF, FreeCaO, SO3, MgO and Blaine are only required for the user defined cement type, that is, icem=6.
3. The heat of hydration properties in the data file must be specified in kg/m/ o
C units.
The model itself can be in any units and Modeller will tabulate the appropriate conversion factor to convert J/m
3
to the User‟s model units. In other words, the
User defines their data in consistent units for their model, Modeller transforms these to kg/m/
o
C on tabulation and also tabulates the conversion factor.
4. The CaO content for fly ash must be specified if fly ash is to be included. Some typical values are Class C fly ash (24%) and Class F fly ash (11%).
5. Other typical thermal properties for concrete:
Specific heat capacity = 1020 J/kg.C (mature concrete).
Conductivity = 28804680 J/hr/m.C
Convective heat transfer coefficient = 360072000 J/hr/m
2
.C.
Orthotropic Concrete Heat of Hydration Model
The data section MATERIAL PROPERTIES FIELD ORTHOTROPIC CONCRETE is used to define the material properties for the plane orthotropic concrete/resin field model. The model is valid for 2D plane field problems.
MATERIAL PROPERTIES FIELD ORTHOTROPIC CONCRETE n imat k x
k y
T C H icem wcem wcra wslg wpfa pfacao Tr conv itime
136
Field Material Properties
[C3S C2S C3A C4AF FreeCaO SO3 MgO Blaine]
All terms are as defined for the Isotropic Concrete Heat of Hydration Model.
Orthotropic Solid Concrete Heat of Hydration Model
The data section MATERIAL PROPERTIES FIELD ORTHOTROPIC SOLID
CONCRETE is used to define the material properties for orthotropic solid concrete field problems. The model is valid for 3D solid field problems.
MATERIAL PROPERTIES FIELD ORTHOTROPIC SOLID CONCRETE n imat nset k x
k y
k z
T C H icem wcem wcra wslg wpfa pfacao Tr conv itime
[C3S C2S C3A C4AF FreeCaO SO3 MgO Blaine]
All terms are as defined for the Isotropic Concrete Heat of Hydration Model.
Linear Variation Convection/Radiation Model
Field link elements permit the variation of conductive, convective and radiative heat transfer to be related to an initial value at full closure, and a linear change in value with increasing gap opening.
The data section MATERIAL PROPERTIES FIELD LINK 18 is used to define the material properties for the linear variation convection/radiation model.
MATERIAL PROPERTIES FIELD LINK 18 imat ko [hco hro dk/dl dhc/dl dhr/dl T]
imat
Ko
hco
The material property identification number
Gap conductance at origin
Convective heat transfer coefficient at origin
hro
Radiative heat transfer coefficient at origin
dk/dL
Variation of gap conductance with opening distance
dhc/dL
Variation of gap convective heat transfer coefficient with opening distance
dhr/dL
Variation of radiative heat transfer coefficient with opening distance
T
Notes
Reference temperature.
1. If a negative value of a material property is calculated, then the material property is set to zero.
2. The figure below shows heat transfer coefficients/gap distance relationship for the linear variation convection/radiation model.
137
Chapter 3 LUSAS Data Input
3. When a radiative heat transfer coefficient is specified the temperature units for the problem will be Kelvin by default. Option 242 allows temperatures to be input and output in Celsius (Centigrade) for problems involving radiative heat transfer.
K, hc, hr dhc/dL hc o dK/dL
K o dhr/dL hr o
Gap distance L
Heat Transfer Coefficients/Gap Distance Relationship for the Linear Variation
Convection/Radiation Model
Nonlinear Variation Convection/Radiation Model
The nonlinear convection/radiation field model permits the variation of conductive, convective and radiative heat transfer to be related to the gap opening distance in an arbitrary manner, by defining the variation of property with distance as a sequential series of straight line segments.
The data section MATERIAL PROPERTIES FIELD LINK 19 is used to define the material properties for the nonlinear variation convection/radiation model.
MATERIAL PROPERTIES LINK 19 N imat < K i
hc i
hr i
L i
> i=1,N
T
imat
N
ki
hci
hri
Li
T
The material property identification number
The number of points used to define the material properties
Gap conductance for point i
Convective heat transfer coefficient for point i
Radiative heat transfer coefficient for point i
Total distance for point i from origin
Reference temperature.
138
Material Assignments
Notes
1. The figure below shows the heat transfer coefficients/gap distance relationship for the nonlinear variation convection/radiation model.
2. When a radiative heat transfer coefficient is specified the temperature units for the problem will be Kelvin by default. Option 242 allows temperatures to be input and output in Celsius (Centigrade) for problems involving radiative heat transfer.
K, hc, hr hc o hc o hc o
K o
K o
K o hr o hr o hr o
L
1
L
2
Gap distance L
Heat Transfer Coefficients/Gap Distance Relationship for the Nonlinear Variation
Convection/Radiation Model
Material Assignments
Material specified using MATERIAL PROPERTIES, PLASTIC DEFINITION,
VISCOUS DEFINITION, DAMAGE PROPERTIES and SHRIHKAGE is assigned to elements using the MATERIAL ASSIGNMENTS data chapter.
MATERIAL ASSIGNMENTS [TITLE title]
{L L last
L diff
 G igroup} imat [nset ipls icrp idam imatv ivse iptm ishr]
L Llast Ldiff
First, last and difference between elements with the same element group number
G
Command word which must be typed to use element groups (see Group).
igroup
The element group reference number.
imat
The material identification number.
139
Chapter 3 LUSAS Data Input
nset
The Cartesian set number defining orthotropy of material properties (see
Cartesian Sets and Notes).
ipls
The stress potential set identification number. See Plastic Definition
icrp
idam
The creep property identification number. See Viscous Definition
The damage property identification number.
imatv
The varying material identification number if it is defined in the preprocessing LUSAS Modeller model. This number is saved in the LUSAS
Modeller results file for postprocessing.
The viscoelastic property identification number. See Viscous Definition
ivse
iptm
ishr
Notes
The twophase material identification number.
The shrinkage property identification number.
1.
nset is only applicable to material models using nset in their material input parameters. When nset is included in the MATERIAL ASSIGNMENT command the value input using MATERIAL PROPERTIES is overridden.
2. If an element is repeated the new properties/rigidities overwrite the previous values for that element.
3. Material properties may only be modified for a transient, dynamic or nonlinear problems subject to the following conditions:
Only the material assignment respecified will be modified
Further assignments may only use material properties datasets defined at the beginning of the problem.
Composite Material
Composite material input may be used to laminate a variety of materials together within a single element. In this lamination procedure, the composite layup sequence is always defined sequentially from the lower to upper surfaces of the element. Any appropriate LUSAS material model (see Notes) may be assigned to any defined layer within the element; hence combinations of material assignments may be used within a single element to achieve a numerical model of the laminated or composite material.
The composite material data is input in three stages.
1. The constitutive materials are defined using MATERIAL PROPERTIES,
PLASTIC DEFINITION, VISCOUS DEFINITION and/or DAMAGE
PROPERTIES.
2. The composite layup is defined using the COMPOSITE MATERIAL command.
3. The defined composite material property sets are assigned to elements using
COMPOSITE ASSIGNMENTS.
The data section COMPOSITE MATERIAL is used to define the layup sequence for each composite property set. Data is specified in tabular form with each row relating to a particular layer in the sequence. The columns contain property set numbers relating to
140
Composite Material
previously defined MATERIAL PROPERTIES, STRESS POTENTIAL, CREEP
PROPERTIES, DAMAGE PROPERTIES, VISCO ELASTIC PROPERTIES and
SHRINKAGE. The STRESS POTENTIAL property set must have been previously defined under either the PLASTIC DEFINITION or VISCOUS DEFINITION data chapters.
COMPOSITE MATERIAL [TITLE title]
TABLE icmp imat i
[angle i
ipls ivse i
ishr i
] i
icrp i
idam i
lname i
icmp
Composite material set number
nlayr
Number of layers in the composite property set ( i=1 to nlayr )
imat i
Material property set number for layer i
angle i
Material direction angle for layer i (see Notes)
ipls i
Stress potential set number for layer i
icrp i
Creep property set number for layer i
idam i
Damage property set number for layer i
iname i
Layer name for layer
ivse i
Viscoelastic property set number for layer i
ishr Shrinkage property set number for layer i
Notes
1.
angle is applicable to orthotropic material models. The value for angle defined using the COMPOSITE MATERIAL command overrides the value input with
MATERIAL PROPERTIES.
2. The number of layers defined in a COMPOSITE MATERIAL table must equal the number of layers defined in the corresponding COMPOSITE GEOMETRY table when assigning values to elements.
3. A composite property set may consist of up to 99 layers.
4. Layer stresses are output by requesting output at Gauss points. All layers will then be output.
5. Composite material data and geometry is allocated to elements using the
COMPOSITE ASSIGNMENTS command.
6. The composite layup defined within this data chapter is orientated with respect to either the local element axes or with respect to a CARTESIAN SET defined within the COMPOSITE ASSIGNMENTS data chapter. Note that an angle of 0 aligns with the appropriate x axis and an angle of 90 with the y axis.
7. For shell elements an appropriate plane stress material model must be used while for solid elements a 3D continuum model should be used (see the LUSAS Element
Reference Manual).
141
Chapter 3 LUSAS Data Input
Composite Assignments
Composite material and geometry sets are assigned to elements using the COMPOSITE
ASSIGNMENTS data chapter.
COMPOSITE ASSIGNMENTS [TITLE title]
{L L last
L diff
 G igroup} icpm icpg [ns
1
ns j
, j=2,nnode
]
L Llast Ldiff
First, last and difference between elements with the same
G element group number.
Command word which must be typed to use element groups (see Group).
igroup
The element group reference number.
icpm
The composite material identification number (see Composite Material).
icpg
The composite geometry identification number (see Composite Geometry).
nsj
The orientation of the composite layup at node j (see Notes).
= 0 for composite orientation with respect to local element axes (see
LUSAS Element Reference Manual for element axes definitions)
= h for composite orientation with respect to a defined CARTESIAN
SET (see Cartesian Sets).
nnode
Number of nodes
Notes
1. The number of layers defined by the COMPOSITE MATERIAL set and the
COMPOSITE GEOMETRY set must be identical when used in the same assignment.
2. The composite layup orientation can be defined at each node where the node ordering is defined by the element topology. If the composite orientation is the same for all nodes then only the composite orientation for node 1 need be specified.
3. If the orientations of the composite layup are omitted then orientation with respect to the element local axes is assumed (nsj = 0 for j=1,nnode).
4. Orientations with respect to local element axes cannot be mixed with orientations with respect to CARTESIAN SETS for a particular element: either all nodes must have orientations with respect to the local element axes or with respect to
CARTESIAN SETS (although the CARTESIAN SET numbers may be different for each of the nodes).
Element Ages
The element ages data chapter is used to define the time in days between casting and activation when using the CEBFIP material model.
ELEMENT AGES
142
Activate/Deactivate Elements
L L last
L diff
L Llast Ldiff
age
age
First, last and difference between elements numbers
Element age in days (default=0 days, see Notes)
Note
The element age should be defined as the time in days between casting and the time at which an element is activated. For example, an element could be 40 days old but activated in the analysis on day 28.
Activate/Deactivate Elements
The activation and deactivation facility accounts for the addition or removal of parts of a model as required by the simulation process. Also known as birth and death, rather than add or remove elements, the facility activates and deactivates elements to model their presence and absence. Staged construction processes, such as tunnelling, are an example of its use with structural analyses.
All elements to be used in the model are specified at the start of the analysis. To model the absence of a part of the model, elements defining it are deactivated. In structural analyses, these elements have their stiffness matrix reduced in magnitude, while for field analysis the conductivity matrix (or other analogous quantity) is reduced. This ensures the deactivated elements have a negligible effect on the behaviour of the remaining model. The element stresses and strains, fluxes and gradients and other analogous quantities are all set to zero.
To model the addition of a part to the model, the elements defining it are activated. In structural analyses, an unmodified stiffness matrix is computed for these elements and the activated elements are introduced in a stress/strain free state, except for any initial stresses or strains that have been defined. Strains are incremented from the point of activation and the current geometry is used to define the activated element‟s initial geometry. In field analyses activation works in the same manner, except that the quantities affected are the conductivity matrix (or other analogous quantity), the fluxes and the gradients.
By default, all loads applied to deactivated elements are initialised to zero and concentrated loads at nodes common to both active and inactive elements are shuffled to the active element. By setting option 385, however, loads applied to deactivated elements are preserved to enable reapplication if and when the elements are reactivated.
DEACTIVATE ELEMENTS
L L last
L diff
[ninc rdfact]
L Llast Ldiff
The first element, last element and difference between elements of the series of elements to be deactivated.
143
Chapter 3 LUSAS Data Input
ninc
The number of increments over which the fraction of residual force is to be redistributed, see Notes (default=1).
rdfact
The fraction of residual force to be redistributed, see Notes (default=0.0).
ACTIVATE ELEMENTS
L L last
L diff
[ninc]
L Llast Ldiff
The first element, last element and difference between elements of the series of elements to be activated.
ninc
The number of increments over which any remaining residual force is to be redistributed, see Notes (default=1).
Notes
1. Restrictions on use. Elements cannot be activated or deactivated in the following circumstances:
In explicit dynamics analyses.
In Fourier analyses.
When using updated Lagrangian or Eulerian geometric nonlinearity.
Elements adjacent to slideline surfaces cannot be activated or deactivated.
2. Option 272 and NONLINEAR CONTROL must be specified when elements are to be activated or deactivated.
3. For rdfact=0.0, all internal forces associated with deactivated elements will remain in the system (i.e. the stresses, displacements, etc., for the remaining elements in a static structural analysis will remain unchanged if the external load remains constant. The same applies to temperature, fluxes, etc., in a static field analysis)‟
For rdfact=1.0, all internal forces associated with deactivated elements are removed from the system (i.e. the stresses, displacements, etc., for the remaining elements in a structural analysis will change. The same applies to temperature, fluxes, etc., in a field analysis)
For 1.0>rdfact>0.0, a fraction of the internal forces in deactivated elements is removed with the remainder retained in the system for subsequent redistribution
(e.g. in a structural analysis with rdfact=0.1, 10% of internal force is removed so that some stress redistribution takes place on the deactivation stage, 90% is retained for redistribution when the element is subsequently reactivated).
4. When deactivated elements are reactivated, any remaining internal forces associated with the reactivated elements (forces retained from deactivation stage) will be removed from the system so that a stress/flux redistribution takes place.
5. Deactivation and activation can take place over several increments if convergence difficulties are encountered by specifying the parameter ninc. For example, if
ninc=3 and rdfact=0.3, then 10% of the internal force will be removed on the first increment, 20% on the second and 30% on the third. The TERMINATION section in NONLINEAR CONTROL (or alternative CONTROL chapter if
144
Activate/Deactivate Elements
applicable) would then have to be defined to cover at least 3 increments (time steps). See the example on Data Input Examples for Tunnel Excavation.
6. Deactivated elements remain in the solution but with a scaled down stiffness/conductivity/etc., so that they have little effect on the residual structure.
The scaling is performed using SYSTEM parameter STFSCL (default=1E6) which can be changed by the user. In dynamic analyses, the mass and damping matrices are initialised to zero.
7. When an element is deactivated, by default all loads associated with that element are removed from the system and will not be reapplied if an element is subsequently activated. This includes concentrated loads, unless the load is applied to a boundary between active and inactive elements when the load is shuffled to the active element. The only exceptions are prescribed loads (displacement, temperature or other analogous quantity) which can be applied to inactive elements. Accelerations may also be applied in a dynamic analysis but this is not recommended.
Setting option 385 overrides the default load initialisation, preserving loads applied to deactivated elements to enable their reapplication if and when the elements are reactivated.
8. When an element is activated in a subsequent stage of a structural analysis, it is introduced in an unstressed/unstrained state and the initial element geometry is taken as the current geometry. Strains are incremented from the time at which the element is activated. Initial stresses/strains and residual stresses may be defined for an element at the reactivation stage. The same applies to field analyses with analogous quantities of flux and gradient, although a geometry update does not take place.
9. The activation of an element that is currently active results in the initialisation of stresses, strains, fluxes and gradients along with an update of the initial geometry to the current geometry. The element is considered to have just become active. The internal equilibrating forces that currently exist in the element will be immediately redistributed throughout the mesh. This provides a simplified approach to redistribute all the element forces of this newly activated element in one increment, for cases in which no relaxation of the remaining structure was required. See example on Data Input Examples for Tunnel Excavation.
10. The direction of local element axes can change during an analysis when elements are deactivated and reactivated. In particular, 3noded beam elements that use the central node to define the local axes should be avoided as this can lead to confusion. For such elements the sign convention for bending moments for a particular element may change after reactivation (e.g. it is recommended that
BSL4 should be preferred to BSL3 so that the 4th node is used to define the local axes and not the initial element curvature).
11. Care should be taken when deactivating elements in a geometrically nonlinear analysis, especially if large displacements are present. It may be necessary to apply prescribed displacements to deactivated elements in order to attain a required configuration for reactivation.
145
Chapter 3 LUSAS Data Input
12. It should be noted that the internal forces in the elements will not balance the applied loading until all residual forces in activated/deactivated elements have been redistributed.
Data Input Examples for Tunnel Excavation
T unnel lining Elem ents 238255
T hese elem ents are used in the
3rd exam ple only. T hey have com m on nodes at the exterior boundary with elem ents 3855 but the interior boundary nodes form a free surface using unique node num bers which define the tunnel void.
T unnel void
Elem ents
2337
T unnel lining
Elem ents 3855
T hese elem ents are used in all three exam ples
Element Numbers Defining the Tunnel Lining and Void
Example 1. Residual Force Redistribution in Increments During Deactivation
.
.
MATERIAL PROPERTIES
C concrete properties
1 14E9 0.3 2400
C soil properties
2 15E7 0.3 2000
MATERIAL ASSIGNMENTS
C assign all elements with soil material properties
1 200 1 2
SUPP NODE
1 59 1 R R
C Apply load to set up initial stress state in soil and maintain constant (however load
C does not have to remain constant)
146
Activate/Deactivate Elements
LOAD CASE
C surface surcharge
CL
60 95 1 0 5000
C soil self weight
CBF
1 200 1 0 2000
NONLINEAR CONTROL
ITERATION 10
CONVERGENCE 0.1 0 0.1 0 0 0
OUTPUT 0 1 1
C Deactivate the elements representing the excavated material.
DEACTIVATE ELEMENTS
C f l i number of increments redistribution factor
C
(default=1)
23 55 1 3
(default=0.0)
0.5
C This will have the effect of deactivating elements 23 to 55 and redistributing 0.5 of
C the equilibrating forces to the remaining mesh prior to the activation of elements. This
C can be interpreted as a relaxation of the stresses around the tunnel excavation, i.e
C displacements and stresses will change so that the boundary of the excavation changes
C shape. If factor=0.0 then all the residual force will be stored for subsequent
C redistribution. This redistribution stage will take place over the next 3 increments.
C i.e. Residual force = (1  0.5*1/3)Fr inc 2
C
(1  0.5*2/3)Fr 3
C
(1  0.5)Fr 4
C More than one increment will only be required if convergence difficulties occur. For
C linear elastic materials the same final result will be obtained irrespective of the
147
Chapter 3 LUSAS Data Input
C number of increments used to redistribute the residual. For nonlinear materials it may
C not be possible to redistribute the force in one increment. Allowing a staged
C redistribution gives the opportunity to change the applied loading during this process.
C Redistribution increments (initial loading is preserved except for load on deactivated
C elements):
NONLINEAR CONTROL
TERMINATION 0 3
MATERIAL ASSIGNMENTS
C Redefine material properties for tunnel lining
38 55 1 1
C Reactivate elements modelling the tunnel lining
ACTIVATE ELEMENTS
C f l i number of increments (default=1)
38 55 1 4
C This command will reactivate elements 38 to 55 in an unstressed/unstrained state and
C any remaining residual equilibrating force associated with these elements will be
C redistributed throughout the mesh over the next 4 increments.
C i.e. Residual force = 0.75*Fr’ inc 5
C
0.5*Fr’ 6
C
C
0.25*Fr’
0.0*Fr’
7
8
C where Fr’= (10.5)Fr (from above)
C Redistribute the remaining residual forces
NONLINEAR CONTROL
TERMINATION 0 4
END
148
Activate/Deactivate Elements
Example 2. Simplified Version with No Redistribution at the Deactivation Stage
.
.
MATERIAL PROPERTIES
C concrete properties
1 14E9 0.3 2400
C soil properties
2 15E7 0.3 2000
MATERIAL ASSIGNMENTS
C assign all elements with soil material properties
1 200 1 2
SUPP NODE
1 59 1 R R
C Apply load to set up initial stress state in soil
LOAD CASE
C surface surcharge
CL
60 95 1 0 5000
C soil self weight
CBF
1 200 1 0 2000
NONLINEAR CONTROL
ITERATION 10
CONVERGENCE 0.1 0 0.1 0 0 0
OUTPUT 0 1 1
MATERIAL ASSIGNMENTS
C Redefine material properties for tunnel lining
38 55 1 1
C Activate elements modelling the tunnel lining
ACTIVATE ELEMENTS
C f l i number of increments (default=1)
38 55 1 1
C This command will activate elements 38 to 55 and restore them to an unstressed/
149
Chapter 3 LUSAS Data Input
C unstrained state while the internal equilibrating force associated with these elements
C will be redistributed throughout the mesh. If it is not required to allow some
C relaxation of the boundary of the excavation prior to installing the tunnel lining, then
C the activation of the tunnel lining can be done in one step. The activation of an
C element which is currently active results in a resetting of the stresses/strains to zero
C and the element is considered to have just become active.
C Deactivate the elements that represent the tunnel void
(i.e. the area inside the lining)
DEACTIVATE ELEMENTS
C f l i number of increments redistribution factor
C
(default=1)
23 37 1 1
(default=0.0)
1.0
C This will have the effect of deactivating elements 23 to 37 which form the tunnel void
C and redistributing all residual force associated with these elements
END
Example 3. Alternative Method of Defining the Tunnel Lining
.
.
MATERIAL PROPERTIES
C concrete properties
1 14E9 0.3 2400
C soil properties
2 15E7 0.3 2000
C At the outset, deactivate the elements that will represent the tunnel lining on re
C activation.
DEACTIVATE ELEMENTS
150
Activate/Deactivate Elements
C f l i number of increments redistribution factor
C
(default=1)
238 255 1 1
(default=0.0)
1.0
C For simplicity, these elements may be thought of as being superimposed on elements 38 to
C 55 which formed the tunnel lining in the previous analyses. However, only the external
C boundary nodes of the tunnel lining must be common with nodes in theunderlying mesh.
C In other words, these elements are connected to the elements which represent the soil at
C the external boundary but the internal element boundaries are discretised with different
C node numbers to form a free surface i.e. the tunnel void.
MATERIAL ASSIGNMENTS
C assign soil material properties
1 200 1 2
C assign lining elements with concrete material properties
238 255 1 1
SUPP NODE
1 59 1 R R
C fix the additional nodes defining the internal boundary of the tunnel lining (i.e.
C located on the elements that are deactivated from the outset). This permits the internal
C dimensions of the tunnel opening to be preserved if critical. Note that prescribed
C displacements could also be applied to these nodes to dictate the shape of the internal
C surface prior to activating the tunnel lining.
201 289 1 R R
C Apply load to set up initial stress state in soil.
LOAD CASE
C surface surcharge
151
Chapter 3 LUSAS Data Input
CL
60 95 1 0 5000
C soil self weight
CBF
1 200 1 0 2000
NONLINEAR CONTROL
ITERATION 10
CONVERGENCE 0.1 0 0.1 0 0 0
OUTPUT 0 1 1
C Activate elements modelling the tunnel lining
ACTIVATE ELEMENTS
C f l i number of increments (default=1)
238 255 1 1
C Deactivate the elements that represent the overall tunnel excavation
DEACTIVATE ELEMENTS
C f l i number of increments redistribution factor
C
(default=1)
23 55 1 1
(default=0.0)
1.0
SUPP NODE
C Release the nodes modelling the interior walls of the lining
201 289 1 F F
END
Damping Properties
The data section DAMPING PROPERTIES is used to define the frequency dependent
Rayleigh damping parameters for elements which contribute to the damping of the whole structure. This section is valid for viscous (modal) and structural (hysteretic) damping and may be utilised when distributed viscous and/or structural damping factors are required using MODAL_DAMPING CONTROL (see Modal Damping
Control).
DAMPING PROPERTIES [VISCOUS  STRUCTURAL]
L L last
L diff
< (a r
b r
)
i
> i=1,n
152
Slidelines
L Llast Ldiff
First, last and difference between elements with identical damping properties.
ar
br
n
Mass Rayleigh damping parameter.
Stiffness Rayleigh damping parameter.
Circular frequency at which the damping parameters apply.
Number of frequencies for which Rayleigh parameters are specified. If more than one set of parameters are specified linearly interpolated parameters will be computed at the required frequency.
Notes
1. If only a and b are input it is assumed the Rayleigh parameters are the same for all frequencies.
2. The Rayleigh parameters are interpolated at the required frequency.
3. If this data chapter is omitted and distributed damping factors are required, then
Rayleigh parameters from material properties are used.
Slidelines
Slidelines may be used to model contact and impact problems, or to tie dissimilar meshes together. Several slideline options are available:
Tied sliding
General sliding without friction
General sliding with friction
Sliding only (without friction or lift off)
Null
The tied slideline option allows meshes of differing degrees of refinement to be connected without the need of a transition zone between the meshes. It can be very useful in creating a highly localised mesh in the region of high stress gradients.
The friction/nofriction slideline types model the finite relative deformation of contacting bodies in two or three dimensions where the contact is stationary or sliding, constant or intermittent. The sliding only option is similar but does not permit intermittent contact, i.e. the surfaces are kept in contact, allowing frictionless sliding contact without liftoff to be modelled. A null slideline is ignored during the analysis, useful when performing a preliminary check on a model.
Each slideline comprises two surfaces  the master surface and the slave surface. These surfaces are specified using nodes in the region where contact is expected to occur. The nodes are ordered to form contact segments where each segment is a boundary face of an underlying element.
153
Chapter 3 LUSAS Data Input
Note that, except for tied slidelines, the slideline contact facility is inherently nonlinear and must be used in a nonlinear analysis. This requires the use of the NONLINEAR
CONTROL data chapter.
The slideline facility requires the following data input:
Slideline property definition
Slideline surface definition
Slideline assignments
The SLIDELINE PROPERTIES command specifies the properties of each slideline, such as the stiffness scale factor and the coefficient of friction. The topology of each slideline surface is specified using the SLIDELINE_SURFACE DEFINITION data section. The segment ordering defined in this section should be checked before a full analysis is undertaken. Alternatively, or in conjunction with SLIDELINE_SURFACE
DEFINITION, the AUTOMATIC SURFACE command can be used to define all valid external surfaces as possible contact surfaces. The slideline surfaces are associated with the required slideline properties using the SLIDELINE ASSIGNMENT data section.
With automatically generated contact surfaces, The SLIDELINE ASSIGNMENT
MATERIAL data section must be used.
The slideline type, (e.g. tied, general sliding with friction), can be redefined during an analysis. This involves respecifying the SLIDELINE ASSIGNMENT data chapter.
SLIDELINE PROPERTIES can also be redefined and assigned.
Temperature dependent SLIDELINE PROPERTIES can also be specified. In this case the TABLE command must follow the SLIDELINE PROPERTIES command. Lines of data listing the slideline properties at particular reference temperatures are then input.
The stiffness scale factors and the coefficient of friction are linearly interpolated across the reference temperatures. All other properties remain unchanged.
A nonlinear friction law can be introduced by using the SLIDELINE PROPERTIES
USER command. This command allows a set of friction parameters to be defined that can vary with the temperature, velocity and acceleration of the contacting surfaces.
These properties may also be specified as temperature dependent.
The following features are available with slidelines
Contact constraint enforcement By default the penalty method is used. The augmented Lagrangian method is also available.
Geometric definition Slideline surfaces can be modelled using linear/bilinear segments, or as curved contact surfaces using quadratic patches. With quadratic patches the curved contact geometry is constructed from a patch of slideline segments, while the contact forces are distributed to the closest segment. The quadratic patches and the curved geometry are setup automatically within LUSAS Solver. The standard patch consists of two linear segments in 2D and four bilinear segments (quadrilateral or triangular) in 3D.
154
Slidelines
Where a patch definition is not possible the standard linear/bilinear definition is used instead.
Rigid surfaces Rigid slideline surfaces are available for modelling contact with rigid bodies. Rigid surfaces can be assigned to valid structural elements as well as to special rigid surface elements R2D2, R3D3 and R3D4. The latter are recommended for modelling rigid bodies since they remove the need for defining structural elements, hence speeding up the solution. All nodes on a rigid surface should be completely restrained. Rigid surfaces cannot contact each other so only one slideline surface can be defined as rigid – master or slave.
Close contact This defines a region above a slideline surface within which a soft spring is applied, but with no force. The stiffness of this spring is applied to all nodes that lie within the closecontact region, thus softening the transition between incontact and outofcontact states. This can help the nonlinear convergence when incontact/outofcontact chatter is experienced.
Contact cushioning This facility applies a contact force and stiffness above a surface that increases exponentially as a node moves closer to the surface.
This cushions the impact of a node with the surface and softens the transition between incontact and outofcontact states. This can help stabilise incontact/outofcontact chatter and any consequent nonlinear convergence difficulties.
Slideline extensions The boundary of a slideline segment can be expanded by specifying a slideline extension. Points outside the segment but within the extended boundary are considered valid for contact. This is particularly useful near the edges of a slideline surface, where a node could be on a segment in one nonlinear iteration and off the segment in the next iteration – a form of chatter that can cause nonlinear convergence difficulties.
Precontact This facility brings two bodies into initial contact using interface forces that act between the slideline surfaces. One of the surfaces must be free to move as a rigid body and the direction of movement is dictated by the interface forces (which act normal to the surface), applied loading and support conditions.
Precontact can be used to overcome problems encountered when applying an initial load (other than prescribed displacement) to a discrete body that, without the slideline, would undergo unrestrained rigid body motion. This is particularly the case when an initial gap exists between the contacting surfaces and a load is applied to bring them into contact. Precontact is only applicable to static analyses.
Warning. Incorrect use of this procedure could lead to initial straining in the bodies or to an undesired starting configuration.
The following table gives a list of elements valid for use with slidelines.
155
Chapter 3 LUSAS Data Input
Element type
Engineering beams
Thick shells
Plane stress continuum
Plane strain continuum
Axisymmetric solid continuum
Solid continuum
Continuum twophase
2D interface
3D interface
2D rigid surface
3D rigid surface
LUSAS elements
BMS3, BTS3
TTS3, QTS4
TPM3, TPM3E, TPK6, TPM6, QPM4, QPM4E,
QPM4M, QPK8, QPM8
TNK6, TPN3, TPN3E, TPN6, QNK8, QPN4,
QPN4E, QPN4L, QPN4M, QPN8
TAX3, TAX3E, TAX6, TXK6, QAX4, QAX4E,
QAX4L, QAX4M, QAX8, QXK8,
TH4, TH4E, TH10, TH10K, PN6, PN6E,
PN6L, PN12, PN12L, PN15, PN15K, PN15L,
HX8, HX8E, HX8L, HX8M, HX16, HX16L,
HX20, HX20K, HX20L
TH10P, TPN6P, PN12P, PN15P, HX16P, HX20P,
QPN8P
IAX4, IAX6, IPN4, IPN6
IS6, IS8, IS16, IS12
R2D2
R3D3, R3D4
Slideline Properties
The data section SLIDELINE PROPERTIES is used to define the overall features of each slideline, such as the interface stiffness scale factor and friction coefficient. If a table of temperature dependent properties is specified under this data chapter, linear interpolation will be applied to all material data. It is possible to redefine and assign the
SLIDELINE PROPERTIES as an analysis progresses.
SLIDELINE PROPERTIES [TITLE title] isprop M scale
S scale
r
extn T C cont
Pentol
Pupfac T
Z
isprop
Slideline property assignment number
M scale
Interface stiffness scale factor for master surface (see Notes)
For automatic surfaces factor is applied to IMAT1, where IMAT1 is a material property identifier
Explicit solution schemes (default = 0.1)
Implicit/static solution schemes (default = 1.0)
Tied slidelines (default=100.0)
S scale
Interface stiffness scale factor for slave surface
For automatic surfaces factor is applied to IMAT2, where IMAT2 is a material property identifier
156
Slidelines
r
extn
Explicit solution schemes (default = 0.1)
Implicit/static solution schemes (default = 1.0)
Tied slidelines (default=100.0)
Coulomb friction coefficient (default = 0.0) (see Notes)
Zonal contact detection parameter (default=0.01) (see Notes)
Slideline extension distance (default = 0.0)
The extension eliminates interpenetration for slideline surfaces which are significantly irregular. More details may be found in the LUSAS Theory
Manual.
T
C cont
Reference temperature (default = 0.0)
Close contact detection parameter, see Notes (default=0.001)
Pentol
Penetration tolerance with augmented Lagrangian method (see Notes)
Pupfac
Penalty update factor with augmented Lagrangian method (default=10.0)
T
Z
Notes
(see Notes)
Tied slideline detection zone (default a large number) (see Notes)
1. The stiffness scale factors control the amount of interpenetration between the two slideline surfaces. Increasing these factors will decrease the relative penetration.
2. The zonal contact detection parameter in conjunction with the system parameter
BBOXF controls the extent of the contact detection test. In the first phase a bounding box is defined around each body or contact surface in turn permitting an efficient check for their overlap. BBOXF is a scaling factor applied to this box, the default value of 1.2 is sufficient for most analyses. For the first iteration of precontact analyses BBOXF is replaced by the system parameter BBOXFP whose default value is 10.0. Then overlap is checked between bounding boxes containing individual surface segments and a nodal volume around the contacting node. The zonal detection distance sets the size of the nodal volume for a node and is calculated by multiplying the zonal detection parameter and the largest dimension of the model in the coordinate directions. A value of 1 will force a search of every single possible contact segment. The default value of 0.01 searches a zone which is
1% of the model size centred on the contacting node.
3. The close contact detection parameter, Ccont, is used to check if a node is threatening to contact a slideline surface. The surface tolerance used is the product of the detection parameter and the length of the surface segment where the node is threatening to penetrate. If the distance between the surfaces is less than the surface tolerance a spring is included at that point just prior to contact. By default, the stiffness of the spring is taken as 1/1000 of the surface stiffness. The factor of
1/1000 can be changed by redefining the SYSTEM parameter SLSTCC. The inclusion of springs in this manner helps to stabilise the solution algorithm when surface nodes come in and out of contact during the iteration process. The close contact detection facility is not available for explicit dynamics.
4. Slideline properties can be redefined at selected stages in an analysis by respecifying SLIDELINE PROPERTIES.
157
Chapter 3 LUSAS Data Input
5. The explicit tied slideline option is more robust when the mesh with the greatest node density is designated the slave surface.
6. Scaling of the slideline surface stiffnesses is automatically invoked at the beginning of each analysis if the ratio of the average stiffness values for each constituent slideline surface differ by a factor greater than 100 (a default value, modifiable using the SLSTFM SYSTEM parameter). In this manner account is made for bodies having significantly different material properties. Option 185 will suppress this facility.
7. The Coulomb friction can only be specified for slideline type 2.
8. The augmented Lagrangian scheme aims to reduce penetrations to below the penetration tolerance Pentol. If 0.0 is specified for the penetration tolerance, a machine dependant nearzero value is used. On 32bit Windows PCs, the default is
1x10
9
.
9. If the penetrations are not reducing quickly enough in the augmented Lagrangian scheme, the penalty update procedure can be used to increase the penalty parameters (contact stiffnesses) in order to accelerate the reduction. The procedure identifies nodes where the reduction in penetration is slow and updates the penalty parameter in the following manner.
k
N
1
k
N
1 k
N k
N if if
HG
F
HG
F g k
N g k1
N g k
N g k1
N
KJ
I
KJ
I
where
N
is the penalty parameter (contact stiffness), g
N
is the penetration, k is the augmented Lagrangian update number,
is Pupfac and
=0.25.
10. The penetration tolerance Pentol and penalty update factor Pupfac are only valid with the augmented Lagrangian method
11. The tied slideline detection zone T
Z
is a dimensional value that sets the maximum distance from a node to the adjacent surface beyond which no contact element will be formed. For instance if a body is 1m long a value of 1mm will probably be acceptable. Contact elements will only be formed for nodes which are within 1mm of the surface.
UserDefined Slideline Properties
The data section SLIDELINE PROPERTIES USER allows user supplied subroutines defining a nonlinear friction law to be called from within LUSAS. This allows you to introduce a friction law which may depend on the velocity, acceleration or temperature of the contacting surfaces. The user subroutines can only be used to compute the friction parameters and the allowable tangential frictional force on a surface. The remaining input data is treated in the same way as data specified under SLIDELINE
PROPERTIES. As temperatures are passed into the user routines, together with a table
158
Slidelines
of friction parameters, you can override interpolation of the friction parameters if necessary. It is possible to redefine SLIDELINE PROPERTIES USER as an analysis progresses.
Source code access is available to these interface routines and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised.
Contact FEA for full details of this facility. Since user specification of a nonlinear friction law involves the external development of source FORTRAN code, as well as access to LUSAS code, this facility is aimed at the advanced LUSAS user.
SLIDELINE PROPERTIES USER nfric [TITLE title] isprop M scale
S scale
<
i
Pentol Pupfac T z
> i=1,nfric
r
extn T C cont
nfric
Number of friction parameters
isprop
Slideline property assignment number
M scale
Interface stiffness scale factor for master surface
For automatic surfaces factor is applied to material IMAT1, where IMAT1 is a material property identifier
Explicit solution schemes (default = 0.1)
Implicit/static solution schemes (default = 1.0)
Tied slidelines (default=100.0)
S scale
Interface stiffness scale factor for slave surface
For automatic surfaces factor is applied to material IMAT2, where IMAT2 is a material property identifier
Explicit solution schemes (default = 0.1)
Implicit/static solution schemes (default = 1.0)
Tied slidelines (default=100.0)
i
r
extn
Friction parameters for user defined friction law
Zonal contact detection parameter (default = 0.01)
Slideline extension distance (default = 0.0)
The extension eliminates interpenetration for slideline surfaces which are significantly irregular. See Notes (more details may be found in the LUSAS
T
Theory Manual).
Reference temperature (default = 0.0)
C cont
Close contact detection parameter, see Notes (default=0.001)
Pentol
Penetration tolerance with augmented Lagrangian method (see Notes)
Pupfac
Penalty update factor with augmented Lagrangian method (default=10.0)
T
Z
Notes
(see Notes)
Tied slideline detection zone (default a large number) (see Notes)
1. The stiffness scale factors control the amount of interpenetration between the two slideline surfaces. Increasing these factors will decrease the relative penetration.
159
Chapter 3 LUSAS Data Input
2. The zonal contact detection parameter in conjunction with the system parameter
BBOXF control the extent of the contact detection test. In the first phase a bounding box is defined around each body or contact surface in turn permitting an efficient check for their overlap. BBOXF is a scaling factor applied to this box, the default value of 1.2 is sufficient for most analyses. For the first iteration of precontact analyses BBOXF is replaced by the system parameter BBOXFP whose default value is 10.0. Then overlap is checked between bounding boxes containing individual surface segments and a nodal volume around the contacting node. The zonal detection distance sets the size of the nodal volume for a node and is calculated by multiplying the zonal detection parameter and the largest dimension of the model in the coordinate directions. A value of 1 will force a search of every single possible contact segment. The default value of 0.01 searches a zone which is
1% of the model size centred on the contacting node.
3. The number of friction parameters defined must agree with the number expected
nfric. All data values must be specified when using this data chapter, default values for data items other than the friction parameters will be set if D is specified in the required locations.
4. Slideline properties can be redefined at selected stages in an analysis by respecifying SLIDELINE PROPERTIES USER.
5. The close contact detection parameter, Ccont, is used to check if a node is threatening to contact a slideline surface. The surface tolerance used is the product of the detection parameter and the length of the surface segment where the node is threatening to penetrate. If the distance between the surfaces is less than the surface tolerance a spring is included at that point just prior to contact. By default, the stiffness of the spring is taken as 1/1000 of the surface stiffness. The factor of
1/1000 can be changed by redefining the SYSTEM parameter SLSTCC. The inclusion of springs in this manner helps to stabilise the solution algorithm when surface nodes come in and out of contact during the iteration process. The close contact detection facility is not available for explicit dynamics.
6. The augmented Lagrangian scheme aims to reduce penetrations to below the penetration tolerance Pentol. If 0.0 is specified for the penetration tolerance, a machine dependant nearzero value is used. On 32bit Windows PCs, the default is
1x10
9
.
7. If the penetrations are not reducing quickly enough in the augmented Lagrangian scheme, the penalty update procedure can be used to increase the penalty parameters (contact stiffnesses) in order to accelerate the reduction. The procedure identifies nodes where the reduction in penetration is slow and updates the penalty parameter in the following manner.
k
N
1 k
N
1
k
N k
N if if
HG
F
HG
F g k
N g k1
N g k
N g k1
N
KJ
I
KJ
I
160
Slidelines
where
N
is the penalty parameter (contact stiffness), g
N
is the penetration, k is the augmented Lagrangian update number,
is Pupfac and
=0.25.
8. The tied slideline detection zone T
Z
is a dimensional value that sets the maximum distance from a node to the adjacent surface beyond which no contact element will be formed. For instance if a body is 1m long a value of 1mm will probably be acceptable. Contact elements will only be formed for nodes which are within 1mm of the surface.
9. The penetration tolerance Pentol and penalty update factor Pupfac are only valid with the augmented Lagrangian method
Slideline Surface Definition
The data sections SLIDELINE_SURFACE DEFINITION is used to define the topology of each slideline surface.
SLIDELINE_SURFACE DEFINITION nsurf [TITLE title]
< N i
> i=1,nseg
nsurf
The surface number to be defined
N i
nseg
The node numbers defining each segment
The number of nodes defining each segment
SLIDELINE_SURFACE DEFINITION RIGID nsurf [TITLE title]
< N i
> i=1,nseg
nsurf
The surface number to be defined
N i
nseg
The node numbers defining each segment
The number of nodes defining each segment
Notes
1. A segment is defined as an element face which forms part of the possible contact surface. Two nodes are required to define the slideline for 2D analyses. Three or four nodes, are required to define a segment for a 3D problem, depending on the particular element face. The segments must be located along the object boundary with segment node ordering defined in a consistent direction, however, segments may be specified in an arbitrary order.
2. For 2D surfaces, the master surface segment node ordering must be defined such that outward normals are defined. The slave surface node ordering must then be in the same direction. If Option 61 is used, both the master and slave surface segment node ordering must be defined such that outward normals are defined. The examples below show these cases.
3. For 2D slidelines the positive local x axis for the master surface coincides with the direction of segment node ordering. A right hand screw rule is then applied with a
161
Chapter 3 LUSAS Data Input
positive local z axis pointing out of the page. The positive local y axis defines the direction of the surface normal, see Example 1. 2D Slideline Surface Definition.
4. For 3D surfaces, the node definition for each surface segment must be labelled in an anticlockwise direction (when looking towards the structure along the outward normal to the slideline surface). The numbering convention obeys the right hand screw rule. See the examples below.
5. Sharp corners (of approximately 90) are generally best described by the use of two surfaces.
6. Coarse mesh discretisation in the region of contact should be avoided.
10. A slideline extension of the order of the anticipated allowable penetration is recommended for 3D slide surfaces.
7. The coordinates of all contact nodes which are determined to have penetrated prior to the commencement of the analysis are reset normally to the contacted surface.
Option 186 will suppress this facility as required. This resetting of coordinates is not available for tied slidelines.
8. SLIDELINE_SURFACE DEFINITION RIGID is used to define a rigid surface.
Such a surface is nondeformable and all nodes on it must be fully restrained.
These restraints should be defined in the
SUPPORT NODES
data section.
9. Standard nodeonsegment contact assumes an equal weighting of force and stiffness at each contact node. Specifying isldst=1 uses a weighting based on contacted areas, which should improve the accuracy of the results.
10. Standard nodeonsegment contact assumes an equal weighting of force and stiffness at each contact node. Specifying isldst=1 uses a weighting based on contacted areas, which should improve the accuracy of the results.
Slideline Surface Automatic
The slideline contact surfaces can be defined automatically by including the command
SLIDELINE_SURFACE AUTOMATIC
Notes
1. All the external faces corresponding to valid underlying element types are extracted and united to form the contact surfaces. A valid element type is one that has edges or faces that can be used in a SLIDELINE SURFACE DEFINITION, however, elements with quadratic edges or faces are not currently supported.
2. The material identifiers, IMAT1 and IMAT2, belonging to the elements which have come into contact are used to identify the correct contact conditions set by the
SLIDELINE ASSIGNMENTS MATERIAL command.
3. Care must be taken to avoid unintended contact when shells are present. A node is above the surface when it lies in the direction of the positive normal of the shell.
4. Manual slideline surfaces (defined by SLIDELINE_SURFACE DEFINITION) can be used in conjunction with the automatic surfaces. Nodes lying on a manually
162
Slidelines
defined surface can only come in contact with the corresponding master or slave surface. However, a node on an automatically generated surface can come in contact with a manually defined surface.
5. The external surface data is saved in a .ASL file. In the event of resolving the problem the nodal topology data is checked against the data stored in this file and if there are no changes the surface data is reused.
6. If the angle between two adjacent segments is less than or equal to the system parameter ANGLEC then it is deemed to be an edge. Slideline extensions can be applied at this point if they have been defined. ANGLEC has a default value of
120
.
7. The contact surfaces must be defined using linear geometry, i.e. curved quadratic patches (islgem = 2) are not currently supported.
Slideline Assignments
The data section SLIDELINE ASSIGNMENTS assembles manually defined slideline surfaces into the required slidelines.
SLIDELINE ASSIGNMENTS [TITLE title] numsl M nsurf
S nsurf
isprop isltyp [P cont
islcsh islpss islgem isldst islaug islpup alstat alsymf]
numsl
The slideline number
M nsurf
The master slideline surface number
S nsurf
The slave slideline surface number
isprop
Slideline property number specified in SLIDELINE PROPERTIES data chapter
isltyp
Type of slideline treatment required for this surface (see Notes) :
=0 for a null slideline
=1 for general sliding without friction (default)
=2 for general sliding with friction
=3 for tied slidelines
P cont
=4 for sliding only (without friction or lift off)
Precontact detection flag : no precontact process precontact required
islcsh
Contact cushioning parameter
= 0 (default)
= 1 (see Notes)
No contact cushioning = 0 (default)
Contact cushioning required = 1 (see Notes)
islpss Number of contact check passes (see Notes) :
Two pass
One pass
islgem Contact surface geometric definition :
Linear (2D), bilinear (3D)
Curved quadratic patches
= 2 (default)
= 1
= 1 (default)
= 2 (see Notes)
163
Chapter 3 LUSAS Data Input
isldst
Use of distributed force/stiffness using contact areas (see Notes)
0 (off, default), 1 (on)
islaug
Use of the augmented Lagrangian method (see Notes)
0 (off, default), 1 (on)
islpup
Use of the penalty update procedure with the augmented Lagrangian method (see Notes)
0 (off, default), 1 (on)
alstat
Contact status with the augmented Lagrangian method (see Notes)
Uzawa‟s method
Powell‟s method
= 1 (default)
= 2
alsymf
Symmetrised Coulomb friction with the augmented Lagrangian method
(see Notes)
0 (off, default), 1 (on)
Notes
1. The slideline surface numbers specified must be previously defined in the
SLIDELINE_SURFACE DEFINITION command.
2. A slideline surface may only be used once.
3. Specifying a friction coefficient with isltyp=1 or 3 is invalid.
4. For 3D slideline surfaces the assignment of the master and slave surfaces is immaterial.
5. A null slideline may be specified if a slideline is defined in the data file but not required for a particular analysis.
6. Assignments can be changed at selected stages in an analysis by respecifying
SLIDELINE ASSIGNMENTS. However, assignments must remain unchanged for master and slave surface numbers, precontact detection, geometric definition and symmetrised Coulomb friction with the augmented method. When changing between frictional and other types of slideline the SLIDELINE PROPERTIES command will also be required to modify the friction coefficient.
1
P
2
P
7. The precontact detection flag, Pcont, is used to overcome problems encountered when applying an initial load to a discrete body which would be subjected to
164
Slidelines
unrestrained rigid body motion. This procedure is only applicable to static analyses and it is required when an initial gap exists between the slideline surfaces and a loading type other than PDSP or TPDSP is to be applied. When this facility is invoked the surfaces of the slidelines are brought together using interface forces
(which act at right angles to the surfaces) and the applied loading. One of the surfaces must be defined on a discrete part of the structure which is free to move as a rigid body and the direction of movement is dictated by the interface forces, applied loading and support conditions. Incorrect use of this procedure could lead to initial straining in the bodies or to an undesired starting configuration. By selecting specific slidelines for the precontact process (i.e. slidelines where initial contact is expected) minimum initial straining will occur and more control over the direction of rigid body movement can be exercised. In the example above precontact is defined for slideline 1 but not for slideline 2. The force used to bring the bodies together (in addition to the applied loading) is computed from the product of the slideline stiffness and gap distance between the surfaces. This force can be factored using the SYSTEM parameter SLSTPC, (default=1.0). It is possible to define all slidelines for precontact and to specify a small value for SLSTPC
(typically 1E6), however, the initial applied loading must be small so that unrestrained rigid body motion does not occur and in general this approach tends to be less stable and is not recommended. It should be noted that if this procedure is used correctly any initial straining caused by the precontact process will disappear after the iterations for the first increment have lead to convergence.
8. Contact cushioning is designed to remove discontinuities in force and stiffness between in and out of contact states via an exponential function, thus aiming to reduce associated problems such as chatter. It can only be specified for general sliding with and without friction slideline types.
Compared to the basic penalty method, however, contact cushioning regards every node on every slideline as being active and may therefore increase processing time depending upon the number of slidelines and slideline nodes. If it is possible to make an assessment of potential areas where chatter may occur in a problem, contact cushioning should be used selectively on slidelines in those areas, although there is no harm in specifying it for all valid slidelines.
Contact cushioning uses an estimate of the normal contact force scalar in the exponential function. Where it is felt that the estimate of the normal contact force scalar is going to be consistently computed as either being too high or too low, the
SYSTEM parameter SLFNCS (default = 1.0) can be used to factor those estimates.
9. Number of contact check passes is controlled by islpss. Currently this value only functions for rigid surfaces. For nonrigid surfaces, the default value of 2 will be used.
10. If islpss is set to one for a rigid surface, only the penetration of deformable surface into the rigid surface is prevented (and not visa versa).
11. Because rigid surfaces can not contact each other, only one of the slideline surfaces in a slideline assignment can be a rigid surface.
165
Chapter 3 LUSAS Data Input
12. Curved slidelines (islgem=2) are defined using quadratic patches. These use information from a patch of slideline segments to define the curved geometry, while the contact forces are distributed to the closest segment. The quadratic patches and the curved geometry are setup automatically within LUSAS Solver with no additional user specification. The standard patch configuration consists of two linear segments in 2D and four bilinear segments (quadrilateral or triangular) in 3D. Where a patch definition is not possible the standard linear/bilinear definition is used instead.
13. The quadratic patch formulation has a nonsymmetric tangent stiffness matrix. The nonsymmetric solver is therefore set automatically by LUSAS Solver.
14.
Large mesh „bias‟ with quadratic patches should be avoided to ensure a reasonable curve fit of the curved contact surface.
15. The standard slideline formulation applies an equal weighting to the force and stiffness at all contact nodes. With isldst=1, the weighting is based on the contacted area, accounting for effects at the edge of the contact area and for a nonuniform mesh.
16. The augmented Lagrangian method uses both penalty parameters and Lagrangian multipliers to reduce contact penetrations to below the tolerance specified under
SLIDELINE PROPERTIES. The Lagrangian multipliers are introduced without increasing the number of variables in the solution. If at convergence the penetrations are not acceptable, the Lagrangian multipliers are updated using the penalty parameters, and the solution is rerun. This process is repeated until either the penetrations are acceptable or the maximum updates is reached (See Nonlinear
Control).
An augmented Lagrangian solution may therefore take longer than the standard penalty solution, but will be less sensitive to the penalty parameter and does not generate additional variables from the Lagrangian multipliers.
17. If the augmented Lagrangian solution is not reducing penetrations quickly enough, the penalty update procedure can be used to increase the penalty parameters
(contact stiffnesses) in order to accelerate the reduction. Details of the procedure can be found under SLIDELINE PROPERTIES. The procedure only works with the augmented Lagrangian method.
18. The augmented Lagrangian criterion for determining whether a node is in contact is based on the sign of the Lagrangian multiplier rather than whether a node has penetrated. A positive value means a node is under tension and must therefore be out of contact, while a negative values means the node is under compression and therefore in contact. There are two techniques for employing this criterion. With
Powell‟s method, the status of a node is only updated at the end of a Lagrangian loop, while with Uzawa‟s method the status is updated during each iteration.
19. The standard penalty and augmented Lagrangian formulations for Coulomb friction involve a nonsymmetric stiffness matrix. Specifying alsymf=1 invokes a formulation that generates a symmetric stiffness matrix. This uses the Lagrangian multiplier from the previous update, rather than the current normal force, when
166
Slidelines
computing the frictional force. Although the solution is quicker, it can lag behind the nonsymmetric version by one Lagrangian update.
Example 1. 2D Slideline Surface Definition
Without Option 61:
SLIDELINE PROPERTIES 1
1 D D D D 0
SLIDELINE DEFINITION 1
FIRST 1 2
INC 1 1 5
SLIDELINE DEFINITION 2
FIRST 11 12
INC 1 1 4
SLIDELINE ASSIGNMENT
1 1 2 1 D
With Option 61:
SLIDELINE PROPERTIES 1
1 D D D D 0
SLIDELINE DEFINITION 1
FIRST 1 2
INC 1 1 5
SLIDELINE DEFINITION 2
FIRST 12 11
INC 1 1 4
SLIDELINE ASSIGNMENT
1 1 2 1 D
2
1 1
1 5
1 4
1 y x
2
1 2
3
1 3 y
4 5 6
1
167
Chapter 3 LUSAS Data Input
Example 2. 3D Slideline Surface Definition
1 3
1 0
1
1 2
1
4
7
2
1 1
5
No rmal
8
3
No rmal
6
9
2
SLIDELINE PROPERTIES 1
1 D D D D 0
SLIDELINE DEFINITION 2
FIRST 1 2 5 4
INC 1 1 1 1 2
INC 3 3 3 3 2
SLIDELINE DEFINITION 1
10 13 12 11
SLIDELINE ASSIGNMENT
1 2 1 1 D
Slideline Assignments Materials
The data section SLIDELINE ASSIGNMENTS MATERIALS complements the
SLIDELINE ASSIGNMENT command but is used specifically with automatically generated surfaces for which a slideline surface number is not available.
SLIDELINE ASSIGNMENTS MATERIALS [TITLE title] numsl IMAT1 IMAT2 isprop isltyp [P cont islgem]
islcsh islpss
numsl
The slideline number
IMAT1 The master slideline surface material identifier IMAT
168
Thermal Surfaces
IMAT2
The slave slideline surface material identifier IMAT
isprop
Slideline property number specified in SLIDELINE PROPERTIES data chapter
isltyp
Type of slideline treatment required for this surface :
=0 for a null slideline
=1 for general sliding without friction (default)
=2 for general sliding with friction
=3 for tied slidelines
=4 for sliding only (without friction or lift off)
P cont
Precontact detection flag : no precontact process precontact required
islcsh
Contact cushioning parameter
= 0 (default)
= 1
No contact cushioning = 0 (default)
Contact cushioning required = 1
islpss Number of contact check passes (see Notes) :
Two pass = 2 (default)
One pass = 1
Islgem
Contact surface geometric definition : = 1
Notes
1. Automatically generated contact surfaces are not formally identified prior to solving the problem. In the absence of a specific surface identifier contact conditions are specified using the material identifiers IMAT corresponding to the elements on the contacted and contacting surface.
2. A node may come in contact with more than one surface but a contact element is only formed with the surface for which the contact node has penetrated least.
3. The contact surface geometry must be linear (islgem = 1), i.e. curved quadratic patches (islgem = 2) are not currently supported.
4. All parameters are as defined in SLIDELINE ASSIGNMENTS. Further details should are given in this data chapter.
Thermal Surfaces
Heat flow across the gap between two surfaces is modelled in LUSAS by the specification of links which define both the path of the heat flow as well as the gap‟s conductivity. The thermal surface data chapter describes a framework in which these links can be automatically generated and updated. In addition to direct heat flow between two points, defined by a link, indirect heat flows are possible by the formation of a link to an environmental node. Heat may also be lost directly to the general environment.
169
Chapter 3 LUSAS Data Input
Heat Transfer by Conduction and Convection
The surfaces are discretised as a series of segments defined by the external nodes of the structure. In generating the links, heat flowing through an area of each segment is
"lumped" to each of the segment nodes. The contributing portion of the segment surface assigned to a node is defined, for the following discussion, as a nodal area. It is then assumed that this heat flows in a direction normal to the nodal area. The origin of the normal flow vector is taken to be at a point one quarter the distance from the node to the segment centroid as this more fairly represents the source of the flow as being from an area rather than a node. To determine the heat flow from a nodal area to an opposing segment, the intercept of its nodal normal with that segment is sought. The size of the gap is defined as the magnitude of the intercept vector.
Environmental nodes may be used to represent the medium which separates the thermal surfaces between which heat is flowing. As the length of a link directly connecting two surfaces increases, the validity of the assumed flow becomes more tenuous.
Alternatively, instead of forming a link, heat could flow directly to the surroundings, but in this case, the heat is lost from the solution. This, in some cases, is a poor approximation to reality, particularly when the thermal surfaces form an enclosure. In this instance an environmental node can be used to model the intervening medium, with all nodal areas which are not directly linked to other areas linked to the environmental node. The environmental node then redistributes heat from the hotter surfaces of the enclosure to the cooler ones without defining the exact process of the transfer.
More than one environmental node may be defined and they may be connected together using links so that a better approximation to the behaviour of medium may be obtained.
The precise form of the link depends on the specified data, with the possibility of links forming between two surfaces, or a segment forming a link to either an environmental node or to the general environment, or finally, the surface may be considered to be insulated without any associated links. However, the order of priority of formulation of link type is well defined, and is set out below (the commands, which are written in capitals, are detailed in subsequent sections):
For nodal area normals which have intercepted another surface segment: a. If a nodal area has penetrated another surface and THERMAL
CONTACT PROPERTIES have been specified a link is formed using these properties. b. If a nodal area has penetrated another surface and no THERMAL
CONTACT PROPERTIES have been specified and if THERMAL GAP
PROPERTIES LINEAR or THERMAL GAP PROPERTIES GENERAL have been specified then these properties are used. c. If no penetration has occurred and if THERMAL GAP PROPERTIES
LINEAR or THERMAL GAP PROPERTIES GENERAL have been specified then these properties are used.
170
Thermal Surfaces
d. If the length of the normal vector is less than or equal to the maximum permissible gap size defined by the properties in b. or c. then a link is formed otherwise it is considered that the surfaces are out of the range of influence and no link is formed.
For nodal areas not linked to a surface segment by not having met conditions a. to d. above or not having intercepted another segment, and with THERMAL
ENVIRONMENTAL PROPERTIES assigned: e. If the nodal area is associated to an environmental node then a link is formed to the node. f. If the nodal area is not associated to an environmental node, a link is formed to the general environment.
If none of the conditions a. to f. apply then no link is formed.
Updated geometry is calculated in a structural analysis and is transferred to the thermal analysis using the thermomechanical coupling commands. If contact pressures are required, a slideline analysis must be run.
For conduction and convection the thermal surface input requires the following data: a. Specification of gap properties using the commands
THERMAL GAP PROPERTIES LINEAR
THERMAL GAP PROPERTIES GENERAL
THERMAL CONTACT PROPERTIES b. Specification of thermal surface segments using the command
THERMAL_SURFACE DEFINITION c. Assignment of both surfaces and gap properties to a gap using the commands
THERMAL ASSIGNMENT
GAP SURFACE DEFINITION
Additionally, the following data may also be prescribed: d. Environmental surface properties (these define the conductivity between a surface and the environment) using the commands
THERMAL ENVIRONMENT PROPERTIES
THERMAL_SURFACE PROPERTY ASSIGNMENT e. Environmental nodes may be defined and assigned to thermal surfaces using the commands:
ENVIRONMENTAL NODE DEFINITION
ENVIRONMENTAL NODE ASSIGNMENT and are effective if THERMAL ENVIRONMENT PROPERTIES and
THERMAL_ SURFACE PROPERTY ASSIGNMENTS have been specified.
171
Chapter 3 LUSAS Data Input
Heat Transfer by Diffuse Radiation
Heat transfer by diffuse radiation is modelled by defining the thermal surfaces that are engaged in radiative exchange. The thermal surfaces are then assigned to a radiation surface. The radiation surface defines those thermal surfaces that will exchange heat by radiation, since radiative heat transfer will only take place between thermal surfaces that define the same radiation surface. The geometry of the thermal surfaces is used to calculate the view factors between the segments that define the thermal surfaces.
A view factor between two segments expresses the fraction of radiative energy leaving one segment that is directly incident on the other segment. If two segments do not have a direct view of each other, for example they may face in opposite directions or there may be other segments blocking the direct view, then the view factor is zero. However two segments with a zero view factor may still exchange heat by reflection off other segments in the thermal surfaces defining the complete radiation surface. If the thermal surfaces defining a radiation surface form an enclosure then the sum of the view factors for any surface segment must be 1.0. The view factors for each radiation surface are calculated in a data check run as well as a full solution run. All the thermal surfaces are assumed to be opaque so that the reflectivity is given by (1.0 emissivity) and the emissivity may be input by the user and assigned to each thermal surface.
The emissivity is a fraction between 0.0 and 1.0 and describes the emissive power of a surface as a fraction of the blackbody emissive power. The blackbody emissive power is given by T4, where
= Stefan Boltzmann constant = 5.6697e8 W/m2/K4
= temperature of the body in Kelvin
If you are working in units other than Watts and metres then the StefanBoltzmann constant will need to be set using the SYSTEM parameter STEFAN. By default all temperature data input and output by LUSAS will be in Kelvin, however you can choose to work in Celsius (Centigrade) by using Option 242. The temperature units of the Stefan Boltzmann constant must always be input in Kelvin.
Using the view factors and emissivity data LUSAS can assemble a matrix that describes all the possible paths for heat to be radiated around the radiation surface. If the radiation surface does not form an enclosure then the segments may optionally radiate to the environment as well as each to other.
If you have a symmetric problem in which the plane(s) of symmetry cut through a radiation surface then it is necessary to define the plane(s) of symmetry. This enables
LUSAS to impose the zero flux condition necessary along a plane of symmetry in a thermal model.
For diffuse radiation the thermal surface input requires the following data:
1. Specification of surface radiation properties using the command:
172
Thermal Surfaces
THERMAL RADIATION PROPERTIES
2. Specification of thermal surface segments using the command:
THERMAL_SURFACE DEFINITION
3. Assignment of radiation properties to thermal surfaces using the command:
THERMAL_SURFACE PROPERTY ASSIGNMENT
4. Assignment of thermal surfaces to form a radiation surface using the commands:
THERMAL ASSIGNMENT
RADIATION SURFACE
Additionally the following data may be specified if the model contains planes of symmetry that cut through thermal surfaces defining a radiation surface:
1. Specification of planes of symmetry using the command:
THERMAL RADIATION SYMMETRY
2. Assignment of symmetry planes to a symmetry surface using the command:
THERMAL_SURFACE SYMMETRY ASSIGNMENT
3. Assignment of a symmetry surface to a radiation surface using the commands:
THERMAL ASSIGNMENT
RADIATION SURFACE
Thermal Gap Properties Linear
The data section THERMAL GAP PROPERTIES LINEAR is used to define thermal properties which may take a linear variation across a gap opening. It is possible to redefine the properties as an analysis progresses, however, the properties must also be reassigned using the THERMAL ASSIGNMENT data chapter.
THERMAL GAP PROPERTIES LINEAR [TITLE title] gmat k o
[h co
dk/dl dh/dl L max
T]
gmat
ko
hco
Gap properties identifier
Gap conductance for a closed gap
Convective heat transfer coefficient for a closed gap
dk/dL
Variation of gap conductance with gap opening
dh/dL
Variation of convective heat transfer coefficient with gap opening
Lmax
Maximum link length beyond which a link will not be created
T
Notes
Reference temperature
1. If the gap opening is such that a negative gap conductance or convective coefficient is calculated, then that gap property is set to zero.
2. The maximum length, Lmax, limits the range of validity of the link element to which these gap properties will be applied. If the length of the link is calculated to be greater than Lmax, then heat will flow either to an environmental node, to the
173
Chapter 3 LUSAS Data Input
general environment or the surface will be considered to be insulated, depending on the ENVIRONMENTAL SURFACE PROPERTIES input.
3. Gap openings are calculated by evaluating the intersection of the surface normal, originating from a point 1/4 the distance from a segment node to the segment centroid, with an opposing surface.
4. Gap properties are assigned to a gap using the THERMAL ASSIGNMENT data chapter.
Thermal Gap Properties General
The data section THERMAL GAP PROPERTIES GENERAL is used to define thermal properties which can vary according to the size of the gap opening. It is possible to redefine the properties as an analysis progresses, however, the properties must also be reassigned using the THERMAL ASSIGNMENT data chapter.
THERMAL GAP PROPERTIES GENERAL [TITLE title] gmat < k i
h ci
L i
> i=1,n
T
n
gmat
ki
hci
Li
T
Notes
Number of gap openings for which properties will be defined
Gap properties identifier
Gap conductance for gap opening Li
Convective heat transfer coefficient for gap opening Li
Size of the ith gap opening
Reference temperature
1.
Lmax and Lmin are defined as the maximum and minimum of Li (i=1,n).
2. If the actual gap opening is less than the minimum value of gap opening, Lmin, the gap properties are assumed to be those corresponding to Lmin. If the gap opening is such that a negative gap conductance or convective coefficient is calculated, then that gap property is set to zero.
3. If the actual gap opening is greater than the maximum value of gap opening,
Lmax, then heat will flow either to an environmental node, or to the general environment or the surface will be considered to be insulated, depending on the
ENVIRONMENTAL SURFACE PROPERTIES input.
4. If only 1 point is input, n=1, Lmax is taken to be L1 and the gap properties are constant over a gap opening of 0 to L1.
5. Gap openings are calculated by evaluating the intersection of the surface normal, originating from a point 1/4 the distance from a segment node to the segment centroid, with an opposing surface.
6. Gap properties are assigned to a gap using the THERMAL ASSIGNMENT data chapter.
174
Thermal Surfaces
Thermal Contact Properties
The data section THERMAL CONTACT PROPERTIES is used to define thermal properties which can vary according to the surface pressure between two contacting surfaces. The surface pressures must be evaluated using the slideline facility and introduced to the thermal analysis via thermomechanical coupling. It is possible to redefine the properties as an analysis progresses, however, the properties must also be reassigned using the THERMAL ASSIGNMENT data chapter.
THERMAL CONTACT PROPERTIES n [TITLE title] cmat < k i
h ci
P i
> i=1,n
T
n
cmat
ki
hci
Pi
T
Notes
Number of contact pressures for which properties will be defined
Contact properties identifier
Gap conductance for contact pressure Pi
Convective heat transfer coefficient for contact pressure Pi
The ith contact pressure defined
Reference temperature
1.
Pmax and Pmin are defined as the maximum and minimum of Pi (i=1,n).
2. If the surface pressure lies outside the range bounded by Pmax and Pmin, then the value taken is Pmin if the surface pressure is less than Pmin and correspondingly the value of Pmax is taken if the surface pressure exceeds Pmax. If the gap opening is such that a negative gap conductance or convective coefficient is calculated, then that gap property is set to zero.
3. Contact pressures can only be calculated using contact forces evaluated from a slideline analysis. The thermomechanical coupling option must be used to transfer this data to the thermal analysis.
4. Contact forces in a slideline analysis are computed if a node penetrates the opposing surface, whilst in a thermal analysis a contact area is calculated if a point
1/4 the distance from the node to the segment centroid has penetrated the opposing surface. This can occasionally lead to different contact predictions between the analyses, particularly at the ends of surfaces or if a sharp surface impacts on a smooth surface.
5. Contact pressure is calculated by dividing the nodal force by the area of all adjacent surfaces which are in contact with opposing surfaces.
6. If a surface is not in contact, a thermal link will be established either to an opposing surface, an environmental node, the general environment or the surface may be considered to be insulated, depending on the ENVIRONMENTAL
SURFACE PROPERTIES input.
7. Contact properties are assigned to a gap using the THERMAL ASSIGNMENT data chapter.
175
Chapter 3 LUSAS Data Input
Thermal Radiation Properties
The data section THERMAL RADIATION PROPERTIES is used to define the emissivity of thermal surfaces engaged in heat transfer by radiation.
THERMAL RADIATION PROPERTIES [TITLE title] rmat
T
rmat
T
Notes
Radiation property identifier
Emissivity
Reference temperature
1. All surfaces are diffuse and opaque so the reflectivity is given by (1emissivity).
2. The radiation properties are assigned to a thermal surface using the
THERMAL_SURFACE PROPERTY ASSIGNMENT data chapter.
3. By default all temperatures input and output in heat transfer problems involving radiation will be in Kelvin. Option 242 may be set to allow temperatures to be input and output in Celsius (Centigrade).
4. Option 131 cannot be used with radiation properties. This is because Option 131 relies on a symmetric matrix and radiation is nonsymmetric.
Thermal Environment Properties
The data section THERMAL ENVIRONMENT PROPERTIES is used to define the heat transfer coefficients for the interface of a surface and a bounding medium. The thermal environmental properties are properties of a surface, not a gap, and are assigned directly to a surface using the THERMAL_SURFACE PROPERTY
ASSIGNMENT data chapter. Properties may be redefined as an analysis progresses, however, to invoke the redefinition the properties must also be reassigned.
THERMAL ENVIRONMENT PROPERTIES [TITLE title] emat k [h c
[
env] envtmp T]
emat
k
hc
env
Environment properties identifier
Surface conductance to environment
Surface convective heat transfer coefficient
Environment emissivity (see Notes)
envtmp
Environmental temperature
T
Reference temperature
Notes
1. A surface segment will try to establish a link with another surface segment. If it fails to do so, heat can flow to an environmental node or to the general environment. The conduction properties for this flow are defined using
176
Thermal Surfaces
THERMAL ENVIRONMENT PROPERTIES. If these properties are not assigned to a surface and a link is not formed, and the surface does not define a
RADIATION SURFACE, then surface is treated as though it is insulated.
2. If the surface has an associated environmental node, a link is established to this node with a conductivity defined using the THERMAL ENVIRONMENT
PROPERTIES; the environmental temperature, envtmp, is ignored. If there is not an associated environmental node, heat is lost directly to the environment using a conductivity defined using the THERMAL ENVIRONMENT PROPERTIES; the environment takes a temperature of envtmp.
3. To specify the environment emissivity Option 253 must be set. The environment emissivity is only used if a segment within a RADIATION SURFACE has a view factor to the environment that exceeds a defined tolerance. The view factor to the environment for a surface segment is defined by 1.0  (sum of the view factors from the segment to all the other segments defining the RADIATION SURFACE).
The tolerance may be set by the system variable TOLFIJ.
4. Thermal environment properties are assigned to a surface using the
THERMAL_SURFACE PROPERTY ASSIGNMENT data chapter.
Thermal Radiation Symmetry
The data section THERMAL RADIATION SYMMETRY is used to define lines or planes of symmetry that cut through radiation surfaces.
THERMAL RADIATION SYMMETRY [TITLE title]
LINE nsym {NODES N1 N2  EQUATION LX LY L}
PLANE nsym {NODES N1 N1 N3  EQUATION CX CY CZ C}
nsym
Symmetry line or plane identifier
N1, N2, N3 Node numbers defining a line or plane of symmetry
LX, LY, L
Coefficients in the line equation LX.x + LY.y = L
CX, CY, CZ, C
Notes
Coefficients in the plane equation CX.x + CY.y + CZ.z = C
1. A line of symmetry must always lie in the global XY plane of the model.
2. A line of symmetry may be used in either a 2D, axisymmetric or 3D analysis. In an axisymmetric analysis a line of symmetry must be perpendicular to the axis about which the model is spun. In a 3D analysis a line of symmetry is converted to a plane of symmetry passing through the defined line and parallel to the global Z axis of the model.
3. A plane of symmetry may be used in either a 2D, axisymmetric or 3D analysis. In a 2D analysis the plane of symmetry must be parallel to the global Z axis of the model. In an axisymmetric analysis a plane of symmetry must be perpendicular to the axis about which the model is spun and parallel to the global Z axis of the model.
177
Chapter 3 LUSAS Data Input
4. Radiation symmetry lines and planes only need to be defined when the plane(s) of symmetry in a model cuts through a radiation surface. Symmetry planes are not required if no radiation surfaces are defined.
5. The symmetry planes are assigned to a symmetry surface using the
THERMAL_SURFACE SYMMETRY ASSIGNMENT data chapter.
Thermal Surface Symmetry Assignment
The data section THERMAL_SURFACE SYMMETRY ASSIGNMENT is used to assign THERMAL RADIATION SYMMETRY lines and planes to a symmetry surface.
THERMAL_SURFACE SYMMETRY ASSIGNMENT isym [TITLE title]
< nsym i
> i=1,npln
isym
npln
nsym
Notes
Symmetry surface identifier
Number of lines and/or planes of symmetry defining symmetry surface
npln symmetry line and/or plane identifiers defining symmetry surface
1. The number of symmetry planes assigned to a symmetry surface must be sufficient to enable LUSAS to generate the full radiation surface by mirroring the defining thermal surfaces successively in each symmetry plane in the order in which the symmetry identifiers are specified in the assignment command.
2. The symmetry surface is assigned to a radiation surface using the RADIATION
SURFACE data chapter.
Thermal Surface Definition
The data section THERMAL_SURFACE DEFINITION is used to define the topology of each thermal surface. It is possible to redefine the surfaces as an analysis progresses, however, the surfaces must also be reassigned using the THERMAL GAP
ASSIGNMENT or the THERMAL_SURFACE PROPERTY ASSIGNMENT data chapters.
THERMAL_SURFACE DEFINITION ntsurf [TITLE title]
< Ni >i=1,nseg
ntsurf
Thermal surface identifier
nseg
Number of nodes defining each segment
Ni
Notes
nseg node numbers defining segment
178
Thermal Surfaces
1. A segment is defined as an element face which forms part of the thermal surface.
Two nodes are required to define the surface for 2D analyses. Three or four nodes are required to define a segment for a 3D problem, depending on the particular element face. The segments must be located along the object boundary with segment node ordering defined in a consistent direction, however, segments may be specified in an arbitrary order.
2. The heat flow from a surface is along a vector which is normal to the surface of the segment. For segments in two dimensions, the normal is defined using a righthand screw rule with the local xaxis running from the first node to the second, the yaxis defines the surface normal with the zaxis coming out of the problem plane.
For 3D surfaces, the node definition for surface segments must be labelled in an anticlockwise direction (when looking towards the structure along the outward normal to the thermal surface).
3. If two 2D elements of different thickness are connected to a segment node, the thickness of the thermal segment is taken as the average of the two element thicknesses.
4. Thermal surface definitions are assigned using the THERMAL ASSIGNMENT data chapter.
Thermal Surface Property Assignments
The data section THERMAL_SURFACE PROPERTY ASSIGNMENTS assigns the
THERMAL ENVIRONMENT PROPERTIES and THERMAL RADIATION
PROPERTITES to a thermal surface previously defined using the
THERMAL_SURFACE DEFINITION command.
THERMAL_SURFACE PROPERTY ASSIGNMENT [TITLE title] ntsurf emat rmat [npnts]
ntsurf
Thermal surface identifier
emat
Thermal environment properties identifier
rmat
Thermal radiation properties identifier
npnts
Number of subsegments to use in the calculation of radiation view factors.
A default value of 2 will be used if not input by the user and if the thermal surface defines a radiation surface, otherwise default=0
Notes
1. THERMAL ENVIRONMENT PROPERTIES are not mandatory. If specified then they are used by surface segments that do not form a conduction or convection link to another surface segment, or they may be used by a thermal surface that defines a radiation surface to establish a radiation link to the environment depending on the surface segment environment view factor.
2. THERMAL RADIATION PROPERTIES are mandatory for any thermal surface that defines a radiation surface.
179
Chapter 3 LUSAS Data Input
3. If Option 131 is specified when radiation surfaces are defined, the option is switched off and a warning message is issued. (Option 131 is switched on by default).
4. The number of subsegments will default to a value of 2 if not specified for any thermal surfaces that define radiation surfaces. The number of subsegments is used in the view factor calculations to subdivide each surface segment into a series of smaller segments. The accuracy of the view factors will increase as more subsegments are used but the calculation time will also increase. Try to run with the minimum number of subsegments that give the required accuracy. The maximum number of subsegments allowed in 2D and axisymmetric models is 50 and in 3D models the maximum allowed is 30.
5. THERMAL ENVIRONMENT PROPERTIES and the THERMAL_SURFACE
DEFINITION may be redefined and reassigned at any point in the solution.
Thermal Assignment
The data section THERMAL ASSIGNMENT is used to define the thermal gaps, their surfaces, properties and processing, and thermal radiation surfaces.
THERMAL ASSIGNMENT [TITLE title]
GAP DEFINITION [UPDATE  NO_UPDATE] [NO_SHADING 
SHADING] [ACTIVE  INACTIVE]
GAP PROPERTIES igap gmat [cmat]
GAP SURFACE DEFINITION igap ntsurf
1
[ntsurf
2
]
RADIATION SURFACES irad isym [TITLE title]
< itsurf i
> i=1,nsurf
igap
Thermal gap identifier
UPDATE
Update geometry from coupled structural analysis (default)
NO_UPDATE
Prevent processing of updated geometry from coupled structural analysis (default UPDATE geometry)
NO_SHADING No checks for shading of elements defining a thermal gap (default
SHADING)
SHADING Check for shading of surface segments defining a thermal gap (default)
ACTIVE
Process gap (default)
INACTIVE Suppress further processing of thermal surface (default ACTIVE)
gmat
Gap property identifier (default=0, see Notes)
cmat
Contact property identifier (default=0, see Notes)
ntsurf1 Thermal surface identifier (see Notes)
ntsurf2 Thermal surface identifier (see Notes)
irad
isym
Radiation surface identifier
Symmetry surface identifier
nsurf
Number of thermal surfaces defining radiation surface
180
Thermal Surfaces
itsurf nsurf Thermal surfaces defining the radiation surface (see Notes)
Notes
1. Gaps may be defined and redefined at any point in the solution.
2. GAP PROPERTIES and GAP SURFACE DEFINITIONS may be reassigned at any point in the solution.
3. The NO_UPDATE flag can be set to prevent the update and subsequent recalculation of thermal links when geometry is read from a coupled structural analysis. The default is to UPDATE geometry.
4. The SHADING parameter forces a complete search of all possible segments. The nearest segment with which it is possible to form a link is then taken as the linkage segment. By default the parameter is enabled.
5. The INACTIVE command suspends further processing of the thermal gap, which has the effect of insulating flow across it. A gap may be reactivated at a later stage in the solution by reissuing the GAP DEFINITION command with the ACTIVE parameter.
6. The use of the GAP DEFINITION command resets the UPDATE, SHADING and
ACTIVE parameters to their default or defined values.
7. Either a gap property identifier, gmat, or a contact property identifier, cmat, must be specified if a gap, igap, is defined. Specification of a 0 or D for an identifier will indicate that no property identifier is to be used.
8.
ntsurf1, ntsurf2 and itsurf are the identifiers defined with the
THERMAL_SURFACES DEFINITION data chapter.
9. At least one surface, ntsurf1, must be specified if a gap, igap, is defined.
Links will then be set up between segments of this surface alone.
10. Only one thermal surface need be defined in a thermal gap. The specification of a second surface, ntsurf2, is for numerical efficiency. The search for linkage between the two defined segments commences with segments on the second surface; if no possible link is found, the first surface is then checked.
11. 0 or D should be input for the symmetry surface, isym, if the radiation surface,
irad, has no symmetry assignment.
12. Any number of thermal surfaces may be used to define a radiation surface and the thermal surfaces do not have to form a continuous line/surface or enclosure.
13. Radiative heat transfer will only take place between thermal surfaces used in the definition of the same radiation surface.
14. The radiation view factors are only dependent on the geometry of the segments defining the radiation surface. So the view factors are only calculated on the very first iteration of a thermal analysis and are recalculated each time the nodal coordinates are updated in a thermal coupled analysis. Option 256 may be used to suppress the recalculation of the view factors in a coupled analysis.
181
Chapter 3 LUSAS Data Input
15. By default all temperatures input and output in heat transfer problems involving radiation will be in Kelvin. Option 242 may be set to allow temperatures to be input and output in Celsius(Centigrade).
16. If radiation surfaces have been defined and the problem units are not Watts and metres then the Stefan Boltzmann constant must be set in the appropriate problem units using the system variable STEFAN.
Radiation Shading
The RADIATION SHADING data chapter allows the user to specify which of the thermal surfaces defining a radiation surface are shading surfaces, partially or fully blocking the view between other thermal surfaces in the radiation surface
RADIATION SHADING irad [TITLE title]
< itshad > i=1,nshad
irad
Radiation surface identifier
nshad
Number of shading thermal surfaces
itshad
Thermal surfaces that obstruct the view between the thermal surfaces that define the radiation surface.
itshad = 1: all thermal surfaces defining the radiation surface are assumed to obstruct the view between segments in the radiation surface.
itshad = 0: no thermal surfaces obstruct any view between any of the thermal surfaces defining the radiation surface, for example the inside of a cube.
Note. If the radiation shading chapter is omitted then all thermal surfaces defining the radiation surface are assumed to obstruct the view between segments in the radiation surface.
If you are in any doubt about shading within a radiation surface then the fully obstructed option, itshad = 1, should be used. This is because the correct view factors are obtained even if a thermal surface is declared as a shading surface when it is not, but a shading surface not declared will lead to incorrect view factors. However you should always try to correctly identify the shading surfaces as this does speed up the view factor calculation.
Radiation View Factor Read
The RADIATION VIEW FACTOR READ chapter allows you to specify which radiation surface view factors are to be read from a file.
RADIATION VIEW FACTOR READ [TITLE title] irad
irad
Radiation surface identifier
The filenames for the radiation surfaces must follow the convention:
182
Thermal Surfaces jnnmm.rvf
where:
j =
nn =
mm = job name radiation surface counter, =01 for the first radiation surface defined, 02 for the second etc. file counter only required if the radiation surface view factors do not all fit in the default file size of 1Mbyte, =blank for the first file, 01 for the second file, etc.
For example, imagine job radt contains two radiation surfaces with identifiers 3 and
4, then the view factors would be read from files:
radt01.rvf, radt0101.rvf, radt0102.rvf ... for radiation surface
3, and
radt02.rvf, radt0201.rvf, radt0202.rvf ... for radiation surface 4
Radiation view factor file format
Number of integer words
Description
Single
Precision
Double
Precision Convex
Geometry type
1 = axisymmetric
2 = 2D planar
3 = 3D
Number of segments
Calculation type =
1
(100*number of records/file) + number of bytes/integer
Number of bytes/real
Segment areas
Direct interchange area matrix (Ai *
Fij)
1
1
1
1
1
N
N*N
2
2
2
2
2
2N
4*N*N
1
1
1
1
1
N
N*N
Note. Option 255 creates the view factor transfer files for each radiation surface if they do not already exist. These files are very useful if the job is rerun, because the addition of the RADIATION VIEW FACTOR READ chapter makes LUSAS read in the view factors from these files instead of repeating the view factor calculations.
183
Chapter 3 LUSAS Data Input
View Factor Output
The data section VIEW_FACTOR OUTPUT is used to control the detail of view factor output in the LUSAS output file.
VIEW_FACTOR OUTPUT [TITLE title] irad irad last
irad diff
[iout] irad iradlast
iraddiff The first, last and difference defining a series of radiation surfaces with
iout identical output control
Radiation surface view factor output number
=0 no view factor output
=1 print the sum of the view factors for each surface segment in the radiation surface and, print the largest deviation in any segment sum from
1.0
=2 print all the individual view factors from each surface segment to all the other segments defining the radiation surface and, print the sum of the view factors for each surface segment in the radiation surface and, print the largest deviation in any segment sum from 1.0
=3 print just the largest deviation in any surface segment view factor sum from 1.0
Notes
1. The default control value for all radiation surfaces is 1.
Environmental Node Definition
The data section ENVIRONMENTAL NODE DEFINITION defines environmental nodes to be used with the thermal surfaces. They are used to distribute heat transferred to the medium separating the thermal surfaces. Heat will flow, via the medium, from hotter surfaces to cooler surfaces without the direct formation of thermal links between these surfaces. The medium is assumed to be of constant temperature as defined by the temperature of the environmental node.
ENVIRONMENTAL NODE DEFINITION [TITLE title] encode [k C a r
envtmp]
enode
Environmental node number (see Notes).
k
Conductance from the environmental node to an external environment of
C constant temperature.
Specific heat capacity multiplied by the mass of the medium associated to
ar the environmental node (used in transient thermal analysis).
Association radius. Segment nodes lying outside this radius are not associated to the environmental node (default = infinity, see Notes).
envtmp
External environmental temperature.
184
Thermal Surfaces
Notes
1. Environmental nodes are assigned to gaps using ENVIRONMENTAL NODE
ASSIGNMENTS command.
2. All environmental nodes must be defined in the initial data section prior to the first solution. Their node number and position are defined in NODE COORDINATES.
Unassigned and disassociated environmental nodes will take the temperature of the external environment envtmp.
3. Environmental nodes may be connected together using other elements such as thermal links and bars. Care must be taken in ensuring that environmental nodes connected to links have the proper boundary conditions.
4. Environmental nodes may be assigned to more than one gap. More than one environmental node may be assigned to one gap.
5. Environmental nodes may be supported and temperatures prescribed using either the SUPPORT or PDSP commands.
6. Concentrated loads (i.e. thermal fluxes) may not be applied directly to environmental nodes. However, thermal bars may be connected to the environmental node and concentrated loads applied to the end of the thermal bar.
7. The associated radius will be ignored if this value is set to D. This effectively means that all nodes may be associated with this environmental node.
8. An example on the definition and usage of environmental nodes is given below.
Environmental Node Assignments
The data section ENVIRONMENTAL NODE ASSIGNMENTS assigns environmental nodes to thermal gaps.
ENVIRONMENTAL NODE ASSIGNMENTS [TITLE title]
N N last
N diff
igap
N Nlast Ndiff
The first node, last node and difference between nodes of the series of environmental nodes.
igap
Identifier defining the gap to which the environmental nodes are to be assigned (see Notes).
Notes
1. All previous assignments are overwritten if the command ENVIRONMENTAL
NODE ASSIGNMENTS is reissued in the solution.
2.
igap is defined in the THERMAL GAP DEFINITION data chapter.
3. An example of the assignment and usage of environmental nodes is given below.
185
Chapter 3 LUSAS Data Input
Example. Use of Environmental Nodes
Shown below is an enclosure with a possible distribution of heat flow: heat flows across the gap
A
C
B
heat flows to the environmental node heat flows to the environmental node
Heat flows directly across the enclosure at its narrowest point B and via an environmental node at its widest point A. At C heat flow is to the environmental node, as the length of its link is beyond the maximum permitted.
Meshing the enclosure surround as shown below:
186
Thermal Surfaces
46
37
47
38
48
39
49
40
50
41
51
42
52
43
53
44
54
45
28
19
10
29
20
11
30
21
12
31
22
13
32
23
14
24
15
35
26
17
36
27
18 16
1 2 3 4 5 6 7 8 9 where node 24 is the environmental node. The thermal surface data would take the form:
:
THERMAL GAP PROPERTIES LINEAR: define gap properties
44 100 0 0 0 2 0
THERMAL ENVIRONMENT PROPERTIES: define surface/gas interface properties
66 50
THERMAL_SURFACE DEFINITION 88: define surface as inside of enclosure
FIRST 11 12
INC 1 1 6
FIRST 17 26
INC 9 9 3
FIRST 44 43
INC 1 1 3
FIRST 41 32
INC 9 9 2
FIRST 23 22
INC 1 1 3
20 11
187
Chapter 3 LUSAS Data Input
THERMAL_SURFACE PROPERTY ASSIGNMENTS: assign surface properties to surface
88 66
THERMAL GAP ASSIGNMENT: assign properties and surfaces to gap 1
GAP DEFINITION 1
GAP PROPERTY 1 44
GAP SURFACES DEFINITION 1 88
ENVIRONMENTAL NODE DEFINITION: define node 24 as environmental node
24
ENVIRONMENTAL NODE ASSIGNMENTS: assign environmental node 24 to gap 1
24 0 0 1
:
Nodal Freedoms
The NODAL FREEDOMS data chapter optionally defines the freedoms at a node when using thick shell elements (TTS3, QTS4, TTS6, QTS8). This command allows five or six degrees of freedom to be specified for a node where either two „local‟ or three global rotations will apply. This facility may be used in conjunction with
TRANSFORMED FREEDOMS to specify loading or boundary conditions in more convenient directions.
NODAL FREEDOMS
N N last
N diff
n free
N N last
N diff
The first node, last node and difference between nodes of the series
n free
Notes
of nodes with identical nodal freedoms.
The number of freedoms (must be 5 or 6)
1. Five degrees of freedom will automatically be assigned to a node unless:
Another type of element with six global degrees of freedom is connected to the same node.
The maximum angle between adjacent shell element normals at the node is greater than the SYSTEM parameter SHLANG (default = 20).
2. If six degrees of freedom are specified for a node, care should be taken that the rotation about the element normal is restrained IF NECESSARY to prevent
188
Freedom Template
singularities. Circumstances in which singularities may occur if this rotation is not restrained are:
When only one element is connected to the node.
When the surface modelled by the elements is quite flat.
3. It is recommended that five degrees of freedom are used whenever possible.
4.
A description of the two „local‟ rotations is given in the LUSAS Element Reference
Manual.
Freedom Template
The FREEDOM TEMPLATE command optionally defines the list of freedoms for which values are defined in SUPPORT CONDITIONS, CONSTRAINT EQUATIONS,
RETAINED FREEDOMS, MODAL SUPPORTS and LOADCASE data chapters.
FREEDOM TEMPLATE
< fretyp
(i)
> i=1,nfrtmp fretyp
(i)
Freedom type for each freedom in template.
nfrtmp
Number of freedoms in template.
Valid freedom types are:
U  displacement in global Xdirection.
V
W
 displacement in global Ydirection.
 displacement in global Zdirection.
THX  rotation about the global Xaxis.
THY  rotation about the global Yaxis.
THZ  rotation about the global Zaxis.
THL1  local rotation about the first loof point.
THL2  local rotation about the second loof point.
DU  hierarchical displacement
DTHX  hierarchical local rotation
PHI  field variable
THA  rotation about first local axis for thick shells
THB  rotation about second local axis for thick shells
Notes
1. If FREEDOM TEMPLATE is not specified then the values input on the
SUPPORT CONDITIONS, CONSTRAINT EQUATIONS, RETAINED
FREEDOMS and LOADCASE will be applied to the freedoms at the node in the order that they occur.
2. The FREEDOM TEMPLATE command must be input when MODAL
SUPPORTS are specified.
3. The following LOADCASE options utilise the FREEDOM TEMPLATE information:
TPDSP, PDSP, CL, VELOCITY, ACCELERATION
189
Chapter 3 LUSAS Data Input
4. If superelements are used without any standard elements the FREEDOM
TEMPLATE command must be specified.
5. If superelements are used that have more freedoms than the standard elements, and values are to be prescribed for these freedoms, then the FREEDOM TEMPLATE must be specified.
Example. Freedom Templates
If an analysis uses 3D beam elements with freedoms U, V, W, THX, THY, THZ and the template freedoms are defined as:
FREEDOM TEMPLATE
U V THZ
Then the support data would be of the form:
SUPPORT CONDITIONS
1 1 0 R F R
which defines U and THZ as fixed and V as free; the other freedoms (i.e. W, THX,
THY) will be considered as free.
Cartesian Sets
Cartesian coordinate sets may be used to define a set of local xyzaxes relative to the global axes. The data section CARTESIAN SETS is used to define the required local
Cartesian coordinate axes.
CARTESIAN SETS [CYLINDRICAL] [TITLE title] nset N
0
[N
1
N
2
]
CARTESIAN SETS MATRIX [TITLE title] nset < R i
> i=1,nmatrix
nset
N
0
N
1
N
2
R i
The Cartesian set identification number.
The node defining the Cartesian set origin.
Additional node required to uniquely define set.
Additional node required to uniquely define set.
The matrix terms (row by row) defining the Cartesian set transformation
(see Notes).
nmatrix The number of terms in the Cartesian set transformation matrix (4 for 2D problems and 9 for 3D problems).
Notes
1. The nodes required to define a Cartesian set are as follows (see figures below):
190
Cartesian Sets
2D problem:
The N1 node defines the local xaxis.
The local yaxis is determined using the righthand screw rule, with the zaxis coming out of the plane of the mesh
3D problem:
The N1 node defines the local xaxis.
The N2 node is any point lying in the positive quadrant of the local xyplane.
The local zaxis is defined using the righthand screw rule.
2. Cylindrical Cartesian sets define the radial, tangent and normal axes transformations. The tangent vector is positive in the direction of a clockwise rotation when looking along the local normal axis from the origin N0. The local axes are evaluated at an arbitrary point within the domain. The nodes used to define a Cylindrical Cartesian set are as follows (see figures below):
2D problem:
No additional data is required.
The local normal axis is directed out of the plane of the mesh.
If a node is coincident with N0 the radial axis will coincide with the xaxis and the tangential axis will coincide with the yaxis.
3D problem:
The N1 node defines the axis from which the cylindrical vectors are evaluated.
The local normal axis is defined as being positive in the direction from
N0 to N1.
If a node lies on the local normal axis, by 1 default the radial axis will lie in the xyplane and the tangential axis will complete the corresponding righthand coordinate system.
Order of axes r´, t´, n´.
3. The Cylindrical Cartesian set is evaluated at the centre point of an element when determining material properties. The centre point is defined as the average of the nodal x, y and z coordinates.
4. The Cartesian set transformation matrix defines the 2D or 3D transformation from local to global coordinate systems as: where {u´} is a vector in the local coordinate system and {U} is the vector in the global coordinate system. [R] is the transformation matrix. The dimensions of [R] are 2x2 for 2D problems and 3x3 for 3D problems. [R] may be constructed by defining the orthogonal vector directions which define the local coordinate directions. For example:
191
Chapter 3 LUSAS Data Input
where {x´}, {y´} and {z´} are vectors defining the local coordinate directions (see figure below for a 2D example).
5. The Cartesian set transformation matrix will be checked for orthogonality and each vector will be automatically normalised.
6. Any number of CARTESIAN SET data chapters may be defined, but if duplicate
nset values are specified the last definition will be used.
(a) 2D Cartesian Set (b) Cylindrical Cartesian Set y y t' y' r'
N
0
N
0 x'
N
1
0 x y
(c) 3D Cartesian Set
0 y
(d) 3D Cylindrical Set t' r' n'
N
1 x z z'
0
N
0 x' y'
N
2
0 x
N
1 z
Definition of Cartesian Sets
N
0 x
192
Transformed Freedoms
Y y' x'
(3.0, 5.0)
(0.0, 0.0)
(10.0, 6.0)
X
10.0
6.0
3.0 5.0
or
cos
sin
sin
cos
Cartesian Set Matrix Definition for 2D Example
Transformed Freedoms
Transformed freedoms may be used to rotate the global degrees of freedom at a node to a new orientation defined by the CARTESIAN SET command. The procedure is useful for applying loading values or boundary conditions in local coordinates directions.
The data section TRANSFORMED FREEDOMS is used to define the nodes to which a predefined local Cartesian coordinate set applies.
TRANSFORMED FREEDOMS [TITLE title]
N N last
N diff
nset
N N last
N diff
The first node, last node and difference between nodes of the series
nset of nodes with identical transformed freedoms.
The number of the Cartesian Set defining the directions or transformation of the transformed freedoms (see Cartesian Sets).
Notes
1. All concentrated loads, prescribed displacements, support conditions and constraint equations applied to a nodal freedom which has been transformed, act in the transformed directions.
2. Default output is in the global direction. Option 115 outputs values in the transformed directions.
3. The order of the transformed directions for cylindrical sets is defined as r´, t´, n´.
193
Chapter 3 LUSAS Data Input
Constraint Equations
Nodal freedoms can be linked by a linear equation. Such constraint equations are useful in defining boundary conditions. For example, if an edge of a structure is to move as an integral unit, the appropriate translational degree of freedom at each node can be forced to act in a relative manner via constraint equations.
The data section CONSTRAINT EQUATIONS is used to define the equation coefficients and the nodes to which the specified constraint equation applies.
CONSTRAINT EQUATIONS [TITLE title]
EQUATION C
N N last
N diff
N v
C f
where:
C
The constraint equation constant
N N last
N diff
The first node, last node and difference between nodes of the series of nodes with identical variables and coefficients.
N v
The degree of freedom variable number at the node. For example, u=1,
C f
Notes
v=2 for plane stress elements (refer to LUSAS Element Reference Manual).
See Notes on FREEDOM TEMPLATE.
The coefficient corresponding to the node and variable number.
1. The general form of the equation is:
C1V1+C2V2+ … +CiVi=C where Vi represents the variables and i the total number of coefficients
2. Each new equation starts with an EQUATION line followed by the corresponding constraint equation data lines.
3. If a node and variable number are repeated, the new coefficient overwrites the previous coefficient for that equation.
4. Constraint equations must not be oversufficient for a unique solution. For example:
U21 = U25, U25 = U30, U30 = U21 is over sufficient
U21 = U25, U25 = U30 is sufficient
5. When using CONSTRAINT EQUATIONS with eigenvalue extraction, the constant C must be specified as zero.
6. If nonstructural nodes or unconnected parts of a structure are to be constrained, the SYSTEM variable PENTLY should be specified to invoke the penalty constraint technique within the constraint equation. PENTLY should be specified as a small number to avoid numerical problems, but to ensure the reduction process within the solution does not break down.
194
Constraint Equations
7. Constrained variables which have been transformed will be constrained in their transformed directions.
8. If the FREEDOM TEMPLATE data chapter has been specified the values specified for Nv relate to the modified freedom list.
9. Freedoms featuring in constraint equations will not be candidates for use as automatic masters.
10. Care should be taken when specifying constraint equations so that ill conditioning of the equations does not result. For example, for some analyses it may be better to define:
U21 = U25, U21 = U26, U21 = U27, U21 = U28 rather than:
U21 = U25, U25 = U26, U26 = U27, U27 = U28
11. If constraint equations are defined in a Guyan analysis or eigenvalue analysis, a
Sturm sequence check cannot be carried out.
12. If constraint equations have been defined the Eigenvalue/Frequency Range facility cannot be used in an Eigenvalue analysis.
13. Constraint equations are not permissible for use with explicit dynamics elements.
Example. Constraint Equations
Plane stress problem with U displacements at nodes 9,11 and 15 constrained to be equal.
U9 = U11 U9 = U15
CONSTRAINT EQUATIONS
EQUATION 0.0
9 0 0 1 1.0
11 0 0 1 1.0
EQUATION 0.0
9 0 0 1 1.0
15 0 0 1 1.0
Plane stress problem with a general constraint relationship.
U9 + U11 + 0.5U6  3.0V14 = 12.5
CONSTRAINT EQUATIONS
EQUATION 12.5
195
Chapter 3 LUSAS Data Input
9 11 2 1 1.0
6 0 0 1 0.5
14 0 0 2 3.0
Y,v
13
9
7
14
8
15
8
11
4 5
5 6 7
X,u
Support Conditions
The data section SUPPORT NODES is used to define the boundary conditions of finite element discretisation. Note that prescribed nodal displacements may also be defined using this data section.
SUPPORT NODES [TITLE title]
N N last
N diff
< type i
> i=1,n
[< V i
> i=1,n
]
N N last
N diff
The first node, last node and difference between nodes of the series of nodes with identical supports.
type i
The support type for each global freedom at a node.
V i
=R for a restrained support freedom or a restrained support freedom with prescribed displacement.
=F for a free support freedom.
=S for spring freedom. (see Note on use of FREEDOM TEMPLATE)
The corresponding values of prescribed displacement or spring stiffness
n for each global freedom at a node. Rotational displacements and rotational spring stiffnesses should be prescribed in radians and stiffness/radian, respectively. (see Note on use of FREEDOM TEMPLATE)
The MAXIMUM number of freedoms at a node for the structure being solved.
Notes
1. If a node number is repeated the new support (types and values) overwrites the previous support and an advisory message is printed out.
196
Support Conditions
2. The freedom associated with a prescribed displacement must be restrained using this data section.
3. If support values Vi are specified, the total number of values must be equal to the
MAXIMUM number of freedoms at any node of the structure. Support values corresponding to free freedoms must be given values, say Vi=0.
4. Ensure that the structure is restrained against translation and rotation in all global directions for all static analyses.
5. For a skew support use TRANSFORMED FREEDOMS, or a joint element with the appropriate orientation, spring stiffness (K=0 for free freedom) and initial strain (prescribed displacement).
6. Support nodes may only be modified between increments of a transient/dynamic nonlinear problem subject to the following conditions:
Only the support conditions for the nodes respecified will be modified.
A support condition may be respecified only for a node specified as a support in the first set of SUPPORT NODES. A dummy support may be specified i.e. all variables free, for nodes that are subsequently restrained.
7. Ensure that nodes are not free to rotate when attached to beam elements with free ends. For example, node 1 in the diagram below must be restrained against rotation as well as displacement otherwise the element will be free to rotate as a rigid body.
R
F
1
2
8. Support nodes may be omitted for eigenvalue analyses provided a shift is used in the EIGENVALUE CONTROL data chapter.
If the FREEDOM TEMPLATE data chapter has been used care should be taken that the required support conditions relate to the modified freedom list.
For nonlinear problems it is recommended that prescribed displacements are specified using the PDSP or TPDSP loading data chapters.
The PDSP values supersede the values specified on the SUPPORT NODES data line. If a spring support is defined at a variable then any subsequent PDSP applied to that variable is read as the spring stiffness.
9. In a axisymmetric analysis the nodes on the axis of symmetry must be restrained to prevent translation across the syemmtry axis. i.e. For symmetry about Y displacement in x must be restrained.
10. For axisymmetric Fourier problems the restrictions shown below are applied to the freedoms of nodes lying on the axis of symmetry. These conditions are automatically imposed on the centreline nodes.
axisymmetric about X axis
harmonic
axisymmetric about Y axis
restraint harmonic restraint
197
Chapter 3 LUSAS Data Input
n=0 n=1 n>1 v, w=0 u=0 u, v, w=0 n=0 n=1 n>1
Example 1. Support Conditions
SUPPORT NODES
1 10 3 R R
2 0 0 F S 0.0 23.1
3 12 3 R F 0.35 0.0
u, w=0 v=0 u, v, w=0
Y,v
10 11 12
7 8 9
4 5 6
1
Spring constant
K=23.1 N/ mm
2 3
Prescribed displacement d=0.35mm
X,u
Example 2. Support Conditions
SUPPORT NODES
198
Coupled Analysis
1 13 3 R R R F F
3 15 3 F R R F F
Z,w
Y,v
14
13
15
10 12
8
7
9
4 6
2
1
3
X,u
Coupled Analysis
In a thermomechanically coupled analysis the control of data to and from an external datafile generally requires three operations
Generation and initialisation of the Coupled Datafile
Reading from the Coupled Analysis Datafile
Writing to the Coupled Analysis Datafile
For further information, refer to Coupled Analyses.
Initialisation of the Coupled Datafile
The data section COUPLE controls both the generation of the external coupled analysis datafile in the primary analysis and the file name specification in the secondary analysis
COUPLE [OPEN] [PARALLEL] fname
OPEN
Specifies that the analysis is to open the data transfer file. If omitted, the analysis will expect to find the data transfer file in its work area.
PARALLEL Specifies that a second analysis is running. If information is requested from the data transfer file and it is not located, an error is signalled if no other analysis is running, otherwise the current analysis will wait for new
199
Chapter 3 LUSAS Data Input
data to become available. Note that the specification of PARALLEL without the second analysis running may cause the system to wait indefinitely for information that will not be available. The SYSTEM parameter MXWAIT determines the waiting time in seconds before an error is printed and the analysis terminated.
fname
The name of data transfer file. The name must be less than 65 characters with a 3 letter extension, or 61 without an extension (an extension .DTF will automatically be added).
Reading from the Coupled Analysis Datafile
The data section COUPLE READ controls the reading from the coupled analysis datafile. The command is used to initialise the read condition at the start of an analysis
(mandatory) and may, if required, be specified at later stages of the analysis.
COUPLE READ [nstepr timerd ndatr nitemr]
nstepr
The step number in the current analysis at which the first data read will occur. This parameter is to be used for static analyses (default = previous step [0], set to 1 to disable ).
timerd
The time in the current analysis at which data should be read. This parameter is to be used for dynamic/transient analyses (default = time end of previous step, set to 1 to disable).
ndatr
The index number for the next dataset to be read (see Notes) (default = 1).
nitemr
The type of data to be transferred
=1 for nodal coordinates
=2 for nodal temperatures
=3 to initialise nodal reference temperatures to those of the previous step
(automatically switches to type 2 on subsequent steps).
=4 for heat flux due to plastic work and nodal coordinates
(default value: Structural analysis = 2, Thermal analysis = 1).
Notes
1. If the reference temperature of the structure is to be initialised with zero temperature nitemr type 3 should be used at the commencement of the analysis
(the first specification of the COUPLE READ command).
2. Option 70 switches on the data echo. All data read into the analysis is echoed to the output file.
3. Each dataset that is written to the coupled datafile is given an integer index number which is automatically incremented by 1 on each write to the coupled analysis datafile. This number corresponds to ndatr specified in the COUPLE READ data line.
4. Further reading from the coupled datafile is controlled by the INCREMENTAL
COUPLE READ data line within the respective analysis control data chapters.
200
Structural Loading
Writing to the Coupled Analysis Datafile
The data section COUPLE WRITE controls writing to the coupled analysis datafile.
The command is used to initialise the write conditions at the start of an analysis
(mandatory) and may, if required, be specified at later stages of the analysis.
COUPLE WRITE [nstepw timewt ndatw nitemw]
nstepw
The step number in the current analysis at which the first data write will occur. This parameter is to be used for static analyses (default = current step [1], set to 1 to disable).
timewt
The time in the current analysis at which data should be written.
This parameter is to be used for dynamic/transient analyses
(default = time at end of current step, set to 1 to disable).
ndatw
The index number for the next dataset to be written (default = 1).
nitemw
The type of data to be transferred
= 1 for nodal coordinates
= 2 for nodal temperatures
= 4 for heat flux due to plastic work and nodal coordinates
(default value: Structural analysis = 1, Thermal analysis = 2).
Notes
1. Each dataset that is written to the coupled datafile is given an integer index number which is automatically incremented by 1 on each write to the coupled analysis datafile. This number corresponds to ndatw specified in the COUPLE WRITE data line.
2. Further writing to the coupled datafile is controlled by the INCREMENTAL
COUPLE WRITE data line within the respective analysis control data chapters.
Structural Loading
LUSAS incorporates a variety of loading types. The loading types available are classified into the following groups (the abbreviations for each loading type are shown in brackets):
Prescribed variables (PDSP, TPDSP)
Concentrated loads (CL)
Element loads (ELDS, DLDL, DLDG, DLEL, DLEG, PLDL, PLDG)
Distributed loads (UDL, FLD)
Body forces (CBF, BFP, BFPE)
Velocities and accelerations (VELOCITY, ACCELERATION)
Initial stresses and strains (SSI, SSIE, SSIG)
Residual stresses (SSR, SSRE, SSRG)
Temperature loads (TEMP, TMPE)
Field loads (ENVT, TDET, RIHG)
201
Chapter 3 LUSAS Data Input
It is important for you to consult the individual element description in the LUSAS
Element Reference Manualin order to check that the required loading is available for that particular element.
Two forms of nodal loading are possible. Firstly, a load may be applied at a node. This load will act on all elements which are connected to the node. Secondly, a load may be applied on an element node, where the load is applied at the node of the prescribed element only. If the required direction of a global load does not lie in the global axes then transformed freedoms can be used to transform the loads to the required local directions (this applies to CL, PDSP, TPDSP, VELOCITY and ACCELERATION loads only).
For some of the loading types it is possible to abbreviate a long line of data input. Such loading definitions make use of two parameters. The first, the loading data list pointer
„l‟, indicates the position in the loading list of the first required component. The second, „n‟, indicates the total number of loading components which are required. For example, the full loading data list of temperature loading (TEMP) for an isoflex plate element contains the 8 components:
T
T x
T y
T z
T
0
T
0
x
T
0
y
T
0
z where only
T
z and
T
0
z are applicable.
Hence, final and initial temperature gradients of 10.5 and 5.6 may be applied by specifying the full loading list (that is 8 required components) as:
LOAD CASE
TEMP 8
0 0 0 10.5 0 0 0 5.6
or, using the abbreviated loading input (using 5 components, and a position pointer of
4), as:
LOAD CASE
TEMP 5 4
10.5 0 0 0 5.6
Note. The default pointer position is 1 (that is, the start of the loading list). Note also that the values not required within the abbreviated loading list must be specified (as zeros).
202
Structural Loading
Load Case Definition
The data section LOAD CASE is used to define the loading types which belong to a particular load case group. For linear analyses each specified LOAD CASE data section defines a new set of loading which are to be applied individually to the structure. For nonlinear analyses the LOAD CASE data section may also be used to define the incrementation of a set of applied loads.
LOAD CASE [TITLE title]
Notes
1. Each new load case must start with this header line.
2. Each LOAD CASE line must be followed by a load type line and corresponding load data lines; see subsequent sections.
3. Each LOAD CASE may consist of a number of load types.
4. Multiple linear LOAD CASES are processed simultaneously.
Prescribed Variables
Nodal variables can be prescribed in an incremental manner (PDSP) or in total form
(TPDSP). In each case the variable to be prescribed must be restrained under the
SUPPORT NODES data chapter.
Incremental Prescribed Variables (PDSP)
The data section PDSP is used to define incremental prescribed nodal variables.
PDSP n [l] [TITLE title]
N N last
N diff
< V i
> =1,n
n
l
The required number of prescribed values.
The starting location of the first input value in the prescribed displacement data list (default l=1)
N N last
N diff
The first node, last node and difference between nodes of the series of nodes with identical prescribed values.
V i
Notes
The prescribed values (see Note on FREEDOM TEMPLATE).
1. The number of prescribed values must not exceed the number of freedoms for any node.
2. Prescribed values will function only if the corresponding freedoms are specified as restrained (R) in SUPPORT NODES.
3. If the FREEDOM TEMPLATE data chapter has been specified prescribed values will relate to the modified freedom list.
203
Chapter 3 LUSAS Data Input
4. Prescribed nodal variables may also be defined via the SUPPORT NODES data chapter (this is not recommended for nonlinear analyses). In this case the prescribed velocities will apply to all loadcases.
5. Incremental and total prescribed displacements (see Total prescribed variables
(TPDSP) below) should not be applied in the same analysis if load curves have been defined. It is recommended that total prescribed displacements are used with load curves.
6. Incremental and total prescribed displacements must not be combined to prescribe values for variables at the same node.
7. Rotational displacements should be specified in radians.
8. In a linear analysis, multiple PDSP load cases may be defined but there must be no change in the degrees of freedom that are loaded.
Total Prescribed Variables (TPDSP)
The data section TPDSP is used to define total prescribed nodal variables.
TPDSP n [l] [TITLE title]
N N last
N diff
< V i
> =1,n
n
l
The required number of prescribed values.
The starting location of the first input value in the prescribed displacement data list (default l=1).
N N last
N diff
The first node, last node and difference between nodes of the series of nodes with identical prescribed values.
V i
Notes
The prescribed values (see Note on FREEDOM TEMPLATE).
1. The number of prescribed values must not exceed the number of freedoms for any node.
2. Prescribed values will function only if the corresponding freedoms are specified as restrained (R) in SUPPORT NODES.
3. If the FREEDOM TEMPLATE data chapter has been specified prescribed values will relate to the modified freedom list.
4. Total and incremental prescribed displacements (see Incremental prescribed
variables (PDSP) above) should not be applied in the same analysis if load curves have been defined. It is recommended that total prescribed displacements are used with load curves.
5. Total and incremental prescribed displacements must not be combined to prescribe values for variables at the same node.
6. Rotational displacements should be specified in radians.
7. In a linear analysis, multiple PDSP load cases may be defined but there must be no change in the degrees of freedom that are loaded.
204
Structural Loading
Concentrated Loads (CL)
The data section CL is used to define concentrated forces and/or moments which are applied directly to structural nodes.
CL [TITLE title]
N N last
N diff
< P i
> i=1,n
N N last
N diff
The first node, last node and difference between nodes of the series
P i
n
Notes of nodes with identical values.
The nodal forces/moments in global X, Y or Z directions (see Notes).
The number of nodal forces/moments
1. If the FREEDOM TEMPLATE data chapter has been specified concentrated loading must relate to the modified freedom list.
Element Loads
Four types of internal element loads may be applied:
Element loads (ELDS)
Distributed loads (DLDL,DLDG)
Distributed element loads (DLEL,DLEG)
Element point loads (PLDL,PLDG)
Consult the relevant element section in the LUSAS Element Reference Manual for details of the required loading components.
Element Loads (ELDS)
The data section ELDS is used to define the element load type and components.
ELDS m [l] [TITLE title]
L L last
L diff
ltype < V i
> i=1,n
m
Maximum number of element loads applied to any one element per load case.
l
The starting location of the first input value in the element load data list
(default l=1).
L L last
L diff
The first element, last element and difference between elements of the series of elements with identical element loading values.
ltype
The element load type number. The element loading types available are:
11 Point loads and moments in local directions
12 Point loads and moments in global directions
21 Uniformly distributed loads in local directions
22 Uniformly distributed loads in global directions
205
Chapter 3 LUSAS Data Input
V i
n
23 Uniformly ditributed projected loads in global directions
31 Distributed element loads in local directions
32 Distributed element loads in global directions
33 Distributed element projected loads in global directions
41 Trapezoidal loads in local directions
42 Trapezoidal loads in global directions
43 Trapozoidal projected loads in global directions
The element internal distances and load values.
The number of element internal distances and load values for the loaded element type (see Loading section in the LUSAS Element Reference
Manual).
Distributed Loads Local/Global (DLDL,DLDG)
The data sections DLDL and DLDG are used to define the distributed load components in local and global directions respectively.
n
l
L
N
NL
q i
Notes
{DLDL  DLDG} n [l] [TITLE title]
L N NL < q i
> i=1,n
The required number of values in the distributed load data list.
The starting location of the first input value in the distributed load data list
(default l=1).
The element number.
The element node number as defined in ELEMENT TOPOLOGY.
The distributed load sequential number (see Notes).
The distributed load values.
1. Use the header line DLDL for local, or DLDG for global, distributed loads.
2. A unique sequential number must be assigned to each distributed load that is applied to an element for a given load case.
3. If an element has a sequential number that is repeated for a given load case, the new loads overwrite the previous values.
Distributed Element Loads Local/Global (DLEL,DLEG)
The data sections DLEL and DLEG are used to define the element distributed load components in local and global directions respectively.
n
{DLEL  DLEG} n [l] [TITLE title]
L L last
L diff
NL < q i
> i=1,n
The required number of values in the distributed internal element load data list.
206
Structural Loading
l
The starting location of the first input value in the distributed internal element load array (default l=1).
L L last
L diff
The first element, last element and difference between elements of
NL
q i
Notes
the series of elements with identical distributed internal element load.
The distributed internal load number (see Notes).
The distributed internal load values.
1. Use the header line DLEL for local, or DLEG for global, distributed internal element loads.
2. A unique internal load number must be assigned to each distributed load that is applied to an element for a given load case.
3. If an element has an internal load number that is repeated for a given load case, the new loads overwrite the previous values.
Element Point Loads Local/Global (PLDL,PLDG)
The data sections PLDL and PLDG are used to define the loading components for element point loads in local and global directions respectively.
{PLDL  PLDG} n [l] [TITLE title]
L L last
L diff
NL < p i
> i=1,n
n
l
The required number of values in the internal element point load data list.
The starting location of the first input value in the internal element point load list (default l=1).
L L last
L diff
The first element, last element and difference between elements of the series of elements with identical internal element point loads.
NL
P i
Note
The element internal point load sequential number.
The element internal point load values.
1. Use the header line PLDL for local, or PLDG for global, point loads.
Distributed Loads
Two types of distributed loads are available:
Uniformly Distributed Loads (UDL)
Face Loads (FLD)
Uniformly Distributed Loads (UDL)
The data section UDL is used to define the loading intensity components for uniformly distributed loads.
UDL [TITLE title]
207
Chapter 3 LUSAS Data Input
L L last
L diff
< W i
> i=1,n
L L last
L diff
The first element, last element and difference between elements of
W
n
i
Note
the series of elements with UDL loads.
The uniformly distributed load (applied in the element local directions, see the LUSAS Element Reference Manual).
The number of uniformly distributed load components.
1. All values applied to elements are accumulative within each LOAD CASE.
Face Loads (FLD)
The data section FLD is used to define the loading components and associated element faces for face loading. The element face numbering conventions are shown in the
LUSAS Element Reference Manual.
n
l
L
LF
N
FL i
Notes
FLD n [l] [TITLE title]
L LF N < FL i
> i=1,n
The required number of values in the element face load data list.
The starting location of the first input value in the element face load data list (default l=1).
The element number.
The element face number (see the LUSAS Element Reference Manual).
The element face node number as input in element topology.
The face load values.
1. If zero element face node N, is specified, then the face load will be applied to all nodes on the face.
2. When using Option 123 for clockwise node numbering, care should be taken to ensure that loading is applied in the correct direction.
Body Forces
Three types of body force loading are available:
Constant Body Forces (CBF)
Body Force Potentials (BFP)
Element Body Force Potentials (BFPE)
Constant Body Forces (CBF)
The data section CBF is used to define the loading components for constant body force loading (specified as forces per unit volume).
208
Structural Loading
CBF [n] [l] [TITLE title]
L L last
L diff
< q i
> i=1,n
n
l
The number of constant body forces/angular velocities/angular accelerations.
The starting location of the first input value in the element load data list
(default l=1).
L L last
L diff
The first element, last element and difference between elements of
q i
the series of elements with identical constant body forces.
The constant body forces/angular velocities (see Notes)/angular accelerations in/about the global X, Y and Z directions/axes (see the
LUSAS Element Reference Manual).
Notes
1. Option 48 switches the constant body force input to linear acceleration input. The angular velocities and accelerations remain unchanged.
2. All values applied to elements are accumulative within each LOAD CASE.
3. Option 102 switches off the load correction stiffness matrix due to centripetal acceleration.
4. Centripetal stiffening effects are limited to 2Dcontinuum, axisymmetric solid, 3Dcontinuum, semiloof shells, thick shells and 3D numerically integrated beam elements. They are only included in nonlinear analyses via the Total Lagrangian geometrically nonlinear facility.
5. Element loading will be a function of the square of any angular velocity specified.
If auto incrementation is used in a nonlinear analysis the load factor, TLAMDA, will be applied to the equivalent element loading and not the angular velocity. If
LUSAS Solver detects this combination an error message will be written to the output file and the analysis terminated. To override this error check OPTION 340 can be specified in the data file and the analysis will continue giving a warning message only. To directly control the magnitude of the angular velocity applied to the structure in a nonlinear analysis manual incrementation or load curves should be utilised.
Body Force Potentials (BFP)
The data section BFP is used to define the loading components for body force potential loading (specified as forces at nodes).
BFP [TITLE title]
N N last
N diff
< q i
> i=1,n
N N last
N diff
The first node, last node and difference between nodes of the series of nodes with force potentials.
q i
The body force potentials/pore water pressure/constant body forces at nodes in global and/or local directions (see Notes).
209
Chapter 3 LUSAS Data Input
n
Notes
The number of body force potentials/pore water pressure/constant body forces.
1. BFP values at a node apply to all elements connected to that node.
2. The LUSAS Element Reference Manual must be consulted to find out which values can be specified under BFP loading for a particular element. Unless otherwise stated, the values are defined as force/unit area or volume and consist of qi where:
i=1 to 3 body force potentials, applied in local element directions
i=4 pore water pressure, applied in global directions
i=5 to 7 constant body forces, applied in global directions
3. All values applied to elements are accumulative within each LOAD CASE.
Element Body Force Potentials (BFPE)
The data section BFPE is used to define the loading components for elemental body force potential loading (specified as forces at element nodes).
n
l
L
N
i
BFPE n [l] [TITLE title]
L N <
i
> i=1,n
The required number of values in the body force potential data list.
The starting location of the first input value in the body force potential data list (default l=1).
The element number.
The element node number as defined in ELEMENT TOPOLOGY.
The body force potential values at the element node in global and/or local directions (see Notes).
Notes
1. The LUSAS Element Reference Manual must be consulted to find out which values can be specified under BFPE loading for a particular element. Unless otherwise stated, the values are defined as force/unit area or volume and consist of:
i:
i=1 to 3 body force potentials, applied in local element directions
i=4 pore water pressure, applied in global directions
i=5 to 7 constant body forces, applied in global directions
2. All values applied to elements are accumulative within each LOAD CASE.
210
Structural Loading
Velocity and Acceleration
In dynamic analyses, velocities or accelerations at a nodal variable can be defined.
These values can be used to specify an initial starting condition or they may be prescribed for the whole analysis. If values are to be prescribed throughout the analysis load curves must be used (see Curve Definition) and the appropriate freedom must be restrained in the SUPPORT NODES data chapter.
Prescribed Velocities (VELOCITY)
Prescribed Accelerations (ACCELERATION)
Examples of Acceleration and Velocity Curves
Prescribed Velocities (VELOCITY)
The data section VELOCITY may be used to define the components of an initial velocity or to prescribe velocities throughout a dynamic analysis.
VELOCITY n [l] [TITLE title]
N N last
N diff
< V i
> i=1,n
n
l
The required number of velocity values in the data list.
The starting location of the first input value in the velocity data list
(default l=1).
N N last
N diff
The first node, last node and difference between nodes of the series
V i
Notes
of nodes with identical velocities.
The velocity components (see Notes).
1. If a component of velocity is to be prescribed throughout an analysis the appropriate freedom must be specified as restrained (R) in support nodes. If an initial velocity is defined without using load curves the support condition for the variable must be free.
2. The number of velocities must not exceed the number of freedoms for any node.
3. Prescribed or initial velocities are only applicable to dynamic analyses.
4. Initial velocities should only be applied to the first load case (i.e. at time=0).
5. If the FREEDOM TEMPLATE data chapter has been specified velocities will relate to the modified freedom list.
6. In general, load curves (see Curve Definition) must be used to prescribe velocities in an analysis. However, initial velocities may be defined without using load curves if no other load type is controlled by a load curve.
7. In general, it is not reasonable to prescribe velocities and accelerations (see
ACCELERATION below) for the same variable at the same point in time; if this does occur in an analysis the acceleration will overwrite the velocity and a warning message will be output. An exception to this rule occurs for implicit dynamics
211
Chapter 3 LUSAS Data Input
analyses where an initial velocity and acceleration may be used to define an initial condition for the same variable.
8. If initial conditions are to be applied, refer to Transient Dynamic Analysis for details on how to compute the data input required for the appropriate dynamics integration scheme.
9. In explicit dynamics, if an initial velocity is to be followed by subsequent prescribed values (velocities, accelerations or displacements) at the same variable, the appropriate freedom must be restrained from the outset.
10. Velocities defined in load curves for explicit dynamics will be written to the output file one time step later than the time at which they were defined. This time lag is a consequence of the central difference integration scheme.
11. It is possible to switch from a prescribed velocity to a prescribed acceleration (or viceversa) for the same variable by manipulating load curve data. Care should be taken when doing this to avoid any discontinuity which could excite a high frequency response in the model. An example of manipulating load curve data in this way is given on Examples of Acceleration and Velocity Curves.
Prescribed Accelerations (ACCELERATION)
The data section ACCELERATION may be used to define the components of an initial acceleration or to prescribe accelerations throughout a dynamic analysis. It should be noted however that an initial acceleration cannot be used to define the starting conditions for an explicit dynamic analysis.
ACCELERATION n [l] [TITLE title]
N N last
N diff
< V i
> i=1,n
n
l
The required number of acceleration values in the data list.
The starting location of the first input value in the acceleration data list
(default l=1).
N N last
N diff
The first node, last node and difference between nodes of the series
V i
Notes
of nodes with identical accelerations.
The acceleration components (see Notes).
1. If a component of acceleration is to be prescribed throughout an analysis the appropriate freedom must be specified as restrained (R) in support nodes. If an initial acceleration is defined in an implicit dynamic analysis without using load curves the support condition for the variable can be free or restrained.
2. The number of accelerations must not exceed the number of freedoms for any node.
3. Prescribed or initial accelerations are only applicable to dynamic analyses.
4. Initial accelerations should only be applied to the first load case (i.e. at time=0) and are only valid for implicit dynamic analyses.
212
Structural Loading
5. If the FREEDOM TEMPLATE data chapter has been specified accelerations will relate to the modified freedom list.
6. In general, load curves (see Curve Definition) must be used to prescribe accelerations in an analysis. However, initial accelerations may be defined without using load curves in an implicit dynamic analysis if no other load type is controlled by a load curve.
7. In general, it is not reasonable to prescribe accelerations and velocities (see
VELOCITY above) for the same variable at the same point in time; if this does occur in an analysis the acceleration will overwrite the velocity and a warning message will be output. An exception to this rule occurs for implicit dynamics analyses where an initial velocity and acceleration may be used to define an initial condition for the same variable.
8. If initial conditions are to be applied, refer to Transient Dynamic Analysis for details on how to compute the data input required for the appropriate dynamics integration scheme.
9. In explicit dynamics, accelerations defined in load curves will be written to the output file one time step later than the time at which they were defined. This time lag is a consequence of using the central difference integration scheme.
10. It is possible to switch from a prescribed acceleration to a prescribed velocity (or viceversa) for the same variable by manipulating load curve data. Care should be taken when doing this to avoid any discontinuity which could excite a high frequency response in the model. An example of manipulating load curve data in this way is given below.
Examples of Acceleration and Velocity Curves
This example shows two methods for defining curves which alternate the prescribing of velocities and accelerations at the same freedom. In the first method, all load curves are assigned from time step 0 and zero sections in a curve allow control to be passed from one curve to another. In the second method, curves are reassigned at appropriate points in the analysis. Either method can be used in implicit dynamics analyses but only the first method should be used for explicit dynamics.
Example. Load Curves Method 1
Velocity
Load Curve 1
Prescribe velocity between times 0.0 and
1.0 and from time 2.0 onwards
0.0
1.0
2.0
Time
213
Chapter 3 LUSAS Data Input
Acceleration
0.0
1.0
2.0
Loading section from data file:
LOAD CASE
VELOCITY 2
1 2 1 0.0 200.0
LOAD CASE
ACCELERATION 2
1 2 1 0.0 300.0
CURVE DEFINITION 1 USER
0.0
1.0
1.0
1.5
1.00001 0.0
1.99999 0.0
2.0 3.0
10.0 5.0
CURVE DEFINITION 2 USER
0.0 0.0
0.99999 0.0
1.0 1.0
2.0 1.0
2.00001 0.0
10.0 0.0
CURVE ASSIGNMENT
1 1.0 1
2 1.0 2
214
Time
Load Curve 2
Prescribe acceleration between times 1.0 and
2.0
Structural Loading
DYNAMIC CONTROL
INCREMENTATION 0.01
CONSTANTS
OUTPUT 1
TERMINATION
END
D
30
Combining curves with zero sections in this manner is only required if it is necessary to alternate the specification of velocities and accelerations at the same freedom. In explicit dynamics (with a varying time step size) the results near discontinuity points in the load curves should be checked to ensure that the tolerance used for defining zero sections is adequate enough to prevent erroneous values being prescribed. For implicit analyses the time step size is fixed and this potential problem will not arise if the load curves are defined correctly.
Example. Load Curves Method 2
Acceleration
Load Curve 1
Prescribe velocity profile completely
0.0
Acceleration
1.0
2.0
Time
Load Curve 2
Prescribe acceleration profile completely
0.0
1.0
2.0
Time
Note. Method 2 should only be used for implicit dynamic analyses.
Loading section from data file:
LOAD CASE
215
Chapter 3 LUSAS Data Input
VELOCITY 2
1 2 1 0.0 100.0
LOAD CASE
ACCELERATION 2
1 2 1 0.0 100.0
CURVE DEFINITION 1 USER
0.0
1.0
2.0
10.0
2.0
3.0
6.0
10.0
CURVE DEFINITION 2 USER
0.0 1.0
0.99999 1.0
1.0
2.0
3.0
3.0
2.00001 0.5
10.0 0.5
CURVE ASSIGNMENT
1 1.0 1
DYNAMIC CONTROL
INCREMENTATION 0.01
CONSTANTS
OUTPUT 1
TERMINATION
CURVE ASSIGNMENT
D
10
2 1.0 2
DYNAMIC CONTROL
TERMINATION
CURVE ASSIGNMENT
1 1.0 1
DYNAMIC CONTROL
TERMINATION
10
10
216
Structural Loading
END
Initial Stresses and Strains
Three types of initial stress and strain loading are available:
Initial stresses and strains at nodes (SSI)
Initial stresses/strains for elements (SSIE)
Initial stresses and strains at gauss points (SSIG)
Initial stresses and strains are applied as the first load case and subsequently included into the incremental solution scheme for nonlinear problems.
Initial stresses and strains are only applicable to numerically integrated elements. Refer to the individual element descriptions in the LUSAS Element Reference Manual for details of the initial stress and strain components.
Initial Stresses and Strains at Nodes (SSI)
The data section SSI is used to define the initial stress and strain components at nodes.
SSI n [l] [TITLE title]
N N last
N diff
< V i
> i=1,n
n
l
The required number of initial stresses or strains at a node.
The starting location of the first input value in the element stress/strain data list (default, l=1 for stress input). The value l=ndse + 1 gives the starting location for strain input, where ndse is the number of stress components for the loaded element type.
N N last
N diff
The first node, last node and difference between nodes of the series
V i
of nodes with identical initial stresses/strains.
The initial stress, stress resultant or initial strain values at a node, relative to the reference axis.
Note
1. The initial stress/strain values at a node, apply to all elements connected to that node.
Example. Initial Stress
To apply an initial stress resultant (Mxy) of magnitude 2 to node number 10 of a QSI4 element would require the following command:
SSI 6
10 0 0 0 0 0 0 0 2
217
Chapter 3 LUSAS Data Input
and for a strain (yxy) at the same node of magnitude 0.001
SSI 6
10 0 0 0 0 0 0 0 0 0 0 0 0 0 0.0001
or
SSI 6 7
10 0 0 0 0 0 0 0 0.0001
Initial Stresses/Strains for Elements (SSIE)
The data section SSIE is used to define the initial element stress and strain components.
SSIE n [l] [TITLE title]
L N < V i
> i=1,n
n
l
L
N
V i
Example. Initial Stress
The required number of initial stresses or strains at an element node.
The starting location of the first input value in the element stress/strain data list (default, l=1 for stress input). The value l=ndse + 1 gives the starting location for strain input, where ndse is the number of stress components for the loaded element type.
The element number.
The element node number as defined in ELEMENT TOPOLOGY.
The initial stress, stress resultant or strain values at the element node.
To apply an initial stress (sy) of magnitude 2 to node number 7 of QPM8 element number 3 would require the following command:
SSIE 3
3 7 0 2 0
and for a strain (ey) at the same node of magnitude 0.001
SSIE 3
3 7 0 0 0 0 0.0001 0
or
SSIE 3 4
3 7 0 0.0001 0
218
Structural Loading
Initial Stresses and Strains at Gauss Points (SSIG)
The data section SSIG is used to define the initial stress and strain components at
Gauss points.
SSIG n [l] [TITLE title]
L L last
L diff
NGP < V i
> i=1,n
n
l
The required number of initial stresses or strains at an element Gauss point.
The starting location of the first input value in the element stress/strain data list (default, l=1 for stress input). The value l=ndse + 1 gives the starting location for strain input, where ndse is the number of stress components for the loaded element type.
L L last
L diff
The first element, last element and difference between elements of a
NGP
V i
series of elements with identical initial stress/strains.
The Gauss point number.
The initial stress, stress resultant or strain value at the element Gauss point relative to the reference axis.
Example. Initial Stress
To apply an initial stress (sxy) of magnitude 2 to Gauss point number 2 of QAX4 element number 10 would require the following command:
SSIG 4
10 0 0 2 0 0 2 0
and for a strain (exy) at the same node of magnitude 0.001
SSIG 4
10 0 0 2 0 0 0 0 0 0 0.0001 0
or
SSIG 4 5
10 0 0 2 0 0 0.0001 0
Residual Stresses
Three types of residual stress loading are available:
Residual stresses at nodes (SSR)
Residual stresses for elements (SSRE)
Residual stresses at gauss points (SSRG)
219
Chapter 3 LUSAS Data Input
Residual stresses (unlike initial stresses) are assumed to be in equilibrium with the undeformed geometry and are not treated as a load case as such. They are considered as a starting position for stress for a nonlinear analysis. Failure to ensure that the residual stresses are in equilibrium will result in an incorrect solution.
Refer to the individual element descriptions in the LUSAS Element Reference Manual
for details of the residual stress components.
Residual Stresses at Nodes (SSR)
The data section SSR is used to define the components of residual stress at nodes.
SSR n [l] [TITLE title]
N N last
N diff
<
ri
> i=1,n
n
l data list (default l=1).
N N last
N diff
The first node, last node and difference between nodes of the series
ri
The required number of residual stresses at a node.
The starting location of the first input value in the element residual stress of nodes with identical residual stresses.
The residual stress or stress resultant values at a node, relative to the reference axis.
Note
1. The residual stress value at a node applies to all elements connected to that node.
Example. Residual Stress
To apply a residual stress resultant (Mxy) of magnitude 2 to node number 10 of a QSI4 element would require the following command:
SSR 6
10 0 0 0 0 0 0 0 2
Residual Stresses for Elements (SSRE)
The data section SSRE is used to define the element residual stress components.
n
l
L
N
SSRE n [l] [TITLE title]
L N <
ri
> i=1,n
The required number of residual stresses at an element node.
The starting location of the first value in the element residual stress data list (default l=1).
The element number.
The element node number as defined in ELEMENT TOPOLOGY.
220
Structural Loading
ri
The residual stress or stress resultant values at the element node, relative to the element reference axis.
Example. Residual Stress
To apply a residual stress (sy) of magnitude 2 to node number 7 of QPM8 element number 3 would require the following command:
SSRE 3
3 7 0 2 0
Residual Stresses at Gauss Points (SSRG)
The data section SSRG is used to define the components of residual stress at Gauss points.
SSRG n [l] [TITLE title]
L L last
L diff
NGP <
ri
> i=1,n
n
l
The required number of residual stresses at an element Gauss point.
The starting location of the first input value in the element residual stress data list (default l=1).
L L last
L diff
The first element, last element and difference between elements of
NGP
ri
the series of elements with identical residual stresses.
The Gauss point number.
The residual stress or stress resultant values for the element, relative to the element reference axis.
Example. Residual Stress
To apply a residual stress (sxy) of magnitude 2 to Gauss point number 2 of QAX4 element number 10 would require the following command:
SSIG 4
10 0 0 2 0 0 2 0
Temperature Loads
Two types of temperature loading are available:
Temperature loads at nodes (TEMP)
Temperature loads for elements (TMPE)
Consult the individual element descriptions in the LUSAS Element Reference Manual
for details of the temperature components.
221
Chapter 3 LUSAS Data Input
Temperature Loads at Nodes (TEMP)
The data section TEMP is used to define the loading components for nodal temperature loads.
TEMP n [l] [TITLE title]
N N last
N diff
< T i
> i=1,n
n
l
The required number of values in the temperature data list.
The starting location of the first input value in the temperature data list
(default l=1).
N N last
N diff
The first node, last node and difference between nodes of the series
T i
Notes
of nodes with identical temperature values.
The temperature values at a node.
1. The temperature values at a node apply to all elements connected to that node, except joints, in which temperature loading is invoked using Option 119.
2. For step by step problems, the initial temperature values need only be specified on the first load step.
3. The TEMP data section may be used to provide a temperature field for computing initial material properties in a nonlinear analysis. To initialise the temperature field in a nonlinear field analysis, the temperature loading must be applied using a manual loading increment.
4. In a stress analysis, temperature loading will only induce stresses if the coefficient of thermal expansion is specified in the material properties.
5. To initialise the temperature field in a nonlinear field analysis, the temperature loading must be applied using a manual load increment.
Temperature Loads for Elements (TMPE)
The data section TMPE is used to define the loading components for element temperature loads.
n
l
L
N
Ti
TMPE n [l] [TITLE title]
L N < T i
> i=1,n
The required number of values in the temperature data list.
The starting location of the first input value in the temperature data list
(default l=1).
The element number.
The element node number as defined in ELEMENT TOPOLOGY.
The temperature values at the element node.
Notes
222
General Point/Patch Loads
1. Temperature is only applied to the node of the element specified.
2. For step by step problems, the temperature values need only be specified on the first load step.
3. The TMPE data section may be used to provide a temperature field for computing initial material properties in a nonlinear analysis. To initialise the temperature field in a nonlinear field analysis, the temperature loading must be applied using a manual loading increment.
4. In a stress analysis, temperature loading will only induce stresses if the coefficient of thermal expansion is specified in the material properties.
5. To initialise the temperature field in a nonlinear field analysis, the temperature loading must be applied using a manual load increment.
General Point/Patch Loads
Since loading may not always conveniently be applied directly to the finite element mesh, the general point and patch load facilities provide a means of calculating the equivalent loads which are applied at the nodes to model loading which may lie within a single element or straddle several elements. By rotation of the vertical loading vector, inplane loading may also be modelled.
General loading can be applied across the finite element mesh by the definition of a
search area. The search area overlies the finite element mesh and is composed of equivalent 3 and 4 noded, or 6 and 8 noded triangular and quadrilateral elements, connected into an area which conveniently covers all or part of the structure to be loaded. The loading is applied to this overlying mesh and converted into equivalent nodal loads using the shape functions of the search elements. These nodal loads are then applied directly to the underlying structural mesh. Note that the nodal loads correctly represent the vertical and inplane components but do not account for any equivalent bending moments.
To ensure a correct transfer of loading, the search area node numbers must coincide with the structural mesh. It is important to note that the loads are only applied to the nodes which are common to both the mesh and the search area.
The definition of general point and patch loads therefore generally involves four data sections:
Search area definition
General point load definition
General patch load definition
Assigning point or patch loads to the structure
An example showing the usage of these data sections is given on General Point and
Patch Loading Assignment.
223
Chapter 3 LUSAS Data Input
Search Area Definition
The data section SEARCH AREA is used to define the general point and patch loading search area.
SEARCH AREA isarea nelt < node i
> i=1,n
isarea
The search area reference number.
nelt
The element number allocated to the particular search element being defined.
nodei
Node numbers for each node of the particular search element being
n
Notes
defined.
The number of nodes required to define the search element.
1. Each search element must be given a unique identifying number. The element numbers may, but not necessarily, be the same as those used in the ELEMENT
TOPOLOGY.
2. Node numbers must be the same as those used for the structural mesh (defined in
NODE COORDINATES).
3. The search element numbers may have omissions in the sequence and need not start at one. The order in which the elements are specified is arbitrary.
4. Nodes must be numbered in an anticlockwise manner.
5. Linear three and four noded elements may be combined or similarly six and eight noded elements may be combined to mesh the search area.
6. A search area must form a continuous surface irrespective of the element types used to mesh the structure.
7. A search area may be defined on any face of an element.
General Point Load Definition
The data section POINT DEFINITION is used to define a series of point loads of arbitrary magnitude in a local zcoordinate system. The loading is applied to the structure by using the ASSIGN command. A CARTESIAN SET is used to define the local xy coordinate system in which the position of the load is defined; the local axes for the load are also assigned using the ASSIGN command.
POINT DEFINITION ldefn x y P
ldefn
The load reference number.
x
The local xcoordinate of point load.
y
P
The local ycoordinate of point load.
The magnitude of the point load acting in the local zdirection.
224
General Point/Patch Loads
Notes
1. The x and y coordinates are defined in local coordinates with a user defined origin and orientation (see ASSIGN data chapter)
2. A load may include any number of point loads which are allowed to be defined in an arbitrary order.
3. A positive P is applied in the positive local z direction.
General Patch Load Definition
The data section PATCH DEFINITION is used to define general patch loads. These are converted to a series of point loads which are then treated in the same fashion as the point loading. The loading is applied to the structure by the specification of the node of the origin of the local xy coordinate system and its orientation with respect to the global axes using the ASSIGN command. Each different load can be applied at a different point and orientation, where the orientation of the local axes is defined using the CARTESIAN SET command.
PATCH DEFINITION ldefn ndivx ndivy x y P
ldefn
The patch reference number
ndivx
The number of patch divisions in local xdirection
ndivy
The number of patch divisions in local ydirection
x
The local xcoordinate of point
y
P
Notes
The local ycoordinate of point
The magnitude of the patch load acting in the local zdirection (see Notes).
1. The type of patch is defined by the number of points:
points = Straight line knife edge load
points = quadrilateral straight boundary patch
8 points = curved boundary patch
2. For knife edge patch loads, the direction of P corresponds with the local z direction
(i.e. a positive P is applied in the positive local z direction). For 4 and 8 point patch loads the direction of point ordering for the patch is important. If the patch points are defined in an anticlockwise direction (when looking from positive to negative local z) the direction of loading corresponds with the positive local z direction. If the patch points are defined in a clockwise direction, a positive P will be applied in the negative local z direction.
3. The angle subtended at any corner of a quadrilateral zone must be less than 180° otherwise nonuniqueness of mapping may result.
225
Chapter 3 LUSAS Data Input
4. For the eight noded patch the midnodes must lie inside the central half of the sides.
5. The PATCH load is transformed to an equivalent summation of ndivx*ndivy point loads; the more divisions used the more realistic the patch load.
6. For line loads the ndivx parameter defines the number of load divisions used.
General Point and Patch Loading Assignment
Defined general point and patch loading is applied to the structure via the ASSIGN data section. This incorporates a transformation which allows the loads, defined in local coordinates, to be orientated at any angle to the global axes. Firstly, the local point or patch loading is orientated with respect to the main structure. The vertical loading can then be rotated to give an inplane loading component (for example, to represent a vehicle braking or cornering load).
ASSIGN norg ldfen nset isarea lset factor
norg
The node number of the origin of the point or patch loading local coordinate system.
ldfen
The load definition number (see Point Definition and Patch Definition
nset above).
The Cartesian set defining the orientation of the local point or patch loading coordinates to the global system (see Cartesian Sets). By default the load will be applied in global directions.
isarea
The search area definition number (see Search Area Definition).
lset
The Cartesian set defining the orientation of the applied vertical loading with respect to the global axes (see Cartesian Sets).
factor
The factor to be applied to the vertical load (default = 1.0).
Notes
1. Any number of point or patch loads may be applied in an arbitrary order.
2. The origin of the local axes for point or patch loads may be placed on any node defined in the NODE COORDINATE data chapter. This node may be defined outside the boundary of the structure.
3. The orientation of point or patch loads may be varied using different Cartesian sets
 (nset varies the patch orientation, lset varies the vertical load orientation). If zero is specified for the Cartesian set number, the orientation of point or patch loads is assumed to be with respect to the global axes.
4. Loading applied outside of the search area are ignored.
5. The translation degrees of freedom of the structural elements must agree with the resolved loading applied to the nodes; if the structure has, for instance, only a lateral freedom w, it is not possible to apply inplane loading in the u and v
226
General Point/Patch Loads
direction which arise if the lateral load applied to the loading mesh is reoriented about either the x or y axes.
Example. Lorry Loading on Bridge Deck
The bridge deck is discretised using a regular mesh of square planar elements:
602
501
401
301
201
101
102 103
1 2 3 4 5
 wheel loading positions
99
1. Definition of orientation of local coordinate.
CARTESIAN SET
1 2 103 102
2. Definition of a search area 2 using 4 noded elements.
SEARCH AREA 2
FIRST 1 1 2 102 101
INC 1 1 1 1 1 (5)
INC 4 100 100 100 100 (5)
3. Definition of point loads to represent a 6 wheeled lorry load (local origin at node
102) with lorry at 45 to the global axes.
POINT DEFINITION 4
0 0 3
1 0 3
3 0 2
700
600
500
400
300
200
100
227
Chapter 3 LUSAS Data Input
0 2 3
1 2 3
3 2 2
4. Assign point loads to structure.
LOAD CASE
ASSIGN
102 4 1 2 0 1
Field Loading
Three types of loading are available for field analyses:
Environmental temperature loading (ENVT)
Temperature dependent environmental temperature loading (TDET)
Temperature dependent rate of internal heat generation (RIHG)
The prescription of temperature dependent or radiation loading turns a linear field problem into a nonlinear field problem. Note that other loading types such as face loads, constant body force, body force potentials, etc. are also applicable to field problems.
Related commands are:
Temperature load case
Temperature Load Assignments
Environmental temperature loading (ENVT)
The data section ENVT is used to define the environmental temperature and convective and radiative heat transfer coefficients for environmental temperature loading.
n
l
L
LF
N
V1
V2
ENVT n [l] [TITLE title]
L LF N < V i
> i=1,n
The required number of values in the element environmental temperature data list (2 or 3).
The starting location of the first input value in the element environmental temperature data list (default l=1).
The element number.
The element face number.
The element face node number as defined in ELEMENT TOPOLOGY.
The environmental temperature.
The convective heat transfer coefficient.
228
Field Loading
V3
Notes
The radiation heat transfer coefficient.
1. If heat transfer coefficients vary on a specified face the values will be interpolated using the shape functions to the Gauss points.
2. If a zero element face node number is specified, then the environmental load will be applied to all nodes on the face.
3. If a nonzero radiation heat transfer coefficient is specified, the problem is nonlinear and NONLINEAR CONTROL must be used.
4. When a radiation heat transfer coefficient is specified the temperature units for the problem will be Kelvin by default. Option 242 allows temperatures to be input and output in Celsius (Centigrade) for problems involving radiative heat transfer.
5. Load curves can be used to maintain or increment the environmental temperature as a nonlinear analysis progresses.
6. Automatic load incrementation within the NONLINEAR CONTROL data chapter can be used to increment ENVT loading.
7. When using load curves or auto incrementation with ENVT loading, the envionmental temperature may be incremented but the heat coefficients remain constant. This means that the heat coefficients will be applied even if the load curve defines a zero environmental temperature. If the heat coefficients and ENVT load are to be introduced or removed during an analysis, then the first (or last) point defining the load curve must coincide with the time at which the ENVT is to be introduced (or removed). Note that if the ENVT is inactive, the heat coefficients are not applied.
8. If the boundary heat transfer conditions can be adequately represented by nontemperature dependent convection and radiation heat transfer coefficients, the
ENVT command may be used to input the data. ENVT loading modifies the stiffness matrix and, consequently, for linear field problems, only one load case may be solved in any one analysis when this loading is applied.
Temperature load case
The TEMPERATURE LOAD CASE data section is used to define a new temperature dependent (that is, nonlinear) temperature load case.
TEMPERATURE LOAD CASE [TITLE title]
Notes
1. The TEMPERATURE LOAD CASE data section must be issued if TDET or
RIHG loading are required.
2. Each TEMPERATURE LOAD CASE definition must be directly followed by either TDET, RIHG and/or TEMPERATURE LOAD ASSIGNMENTS data sections.
3. Each load case may consist of any number of load types.
229
Chapter 3 LUSAS Data Input
4. NONLINEAR CONTROL must be specified if temperature dependent loading is used.
5. The order of data input is first to list the temperature dependent data in the form of a table using the TEMPERATURE LOAD CASE followed by subcommands
TDET and/or RIHG. These tables are then assigned to the elements using the
TEMPERATURE LOAD ASSIGNMENTS followed by the subcommands TDET and/or RIHG.
6. If TDET or RIHG loading is to be combined with other load types such as CL or
PDSP, the TEMPERATURE LOAD CASE must precede the LOAD CASE data chapter.
Temperature dependent environmental temperature loading (TDET)
The data section TDET is used to define the environmental temperature, convective and radiative heat transfer coefficients, and reference temperature for temperature dependent environmental temperature loading.
n
l
ilod
Vi
T
Notes
TDET n [l] [TITLE title]
TABLE ilod
< V i
> i=1,n
T
The required number of values in the environmental temperature data list
(must currently =3).
The starting location of the first input value in the environmental data list
(default l=1).
The table reference number.
The list of values:
V1  Environmental temperature
V2  Convective heat transfer coefficient
V3  Radiative heat transfer coefficient
Reference temperature.
1. When a radiation heat transfer coefficient is specified the temperature units for the problem will be Kelvin by default. Option 242 allows temperatures to be input and output in Celsius (Centigrade) for problems involving radiative heat transfer.
2. Load curves can be used to maintain or increment the environmental temperature as a nonlinear analysis progresses.
3. When using load curves incrementation with TDET loading, the environmental temperature may be incremented but the heat coefficients remain constant. This means that the heat coefficients will be applied even if the load curve defines a zero environmental temperature. If the heat coefficients and TDET load are to be introduced during an analysis, then the first (or last) point defining the load curve
230
Field Loading
must coincide with the time at which the ENVT is to be introduced (or removed).
Note that if the ENVT is inactive, the heat coefficients are not applied.
4. Automatic load incrementation under the NONLINEAR CONTROL data chapter cannot be used with TDET loading.
Temperature dependent rate of internal heat generation
(RIHG)
The data section RIHG is used to define the rate of internal heat generation and reference temperature for temperature dependent internal heat generation loading.
RIHG n [l] [TITLE title]
TABLE ilod
V T
n
l
ilod
V
T
Notes
The number of values of data in the table (must currently =1)
The starting location of the first input value in the table (default l=1).
The table reference number.
Rate of internal heat generation.
Reference temperature.
1. Load curves can be used to maintain or increment the RIHG as a nonlinear analysis progresses.
2. Automatic load incrementation under the NONLINEAR CONTROL data chapter cannot be used with RIHG loading.
User defined rate of internal heat generation (RIHG
USER)
The USER defined rate of internal heat generation facility allows a usersupplied subroutine to be used from within LUSAS. This facility provides access to the LUSAS property data input via the RIHG USER data section and provides controlled access to the pre and postsolution element processing via the usersupplied subroutine.
By default the routine is supplied as an empty routine with a defined interface that is unchangeable. The externally developed code should be placed into this routine which is then linked into the LUSAS system. Source code access is available to the interface routine and object library access is available to the remainder of the LUSAS code to enable this facility to be utilised. See Solver User Interface Routines.
Since user specification of rate of internal heat generation involves the external development of source FORTRAN code, as well as access to LUSAS code, this facility is aimed at the advanced LUSAS user.
231
Chapter 3 LUSAS Data Input
The data section RIHG USER provides the interface to User supplied subroutines for computing the rate of internal heat generation.
RIHG USER n [TITLE title]
TABLE ilod
< U i
> i=1,(n1)
T
n
ilod
U
T
Notes
The number of values of data in the table
The table reference number.
The userdefined input parameters
Reference temperature.
1. NONLINEAR and TRANSIENT CONTROL chapters must be defined when using RIHG USER loading.
2. Load curves can be used to maintain or increment the RIHG USER as a nonlinear transient analysis progresses.
3. The number of input parameters must be equal to that specified on the data section header line (i.e. n). Failure to match the requested and supplied number of parameters will invoke a LUSAS error message.
4. Option 179 can be set for argument verification within the user routines.
Temperature Load Assignments
The TEMPERATURE LOAD ASSIGNMENTS data section is used to assign temperature dependent field loading (that is TDET and RIHG) to the associated elements.
TEMPERATURE LOAD ASSIGNMENTS [TITLE title]
Notes
1. Each load assignment list must start with this header.
2. The TEMPERATURE LOAD ASSIGNMENTS data section must be immediately followed by a TDET or RIHG assignment data section.
3. Load assignments must be used if temperature dependent field loads are specified.
TDET Load Assignments
The TDET assignment data section is used to assign the defined temperature dependent environmental temperature field loading to the associated elements.
L
TDET
L LF N ilod
The element number.
232
Curve Definition
LF
N
ilod
The element face number.
The element (face) node number as defined in ELEMENT TOPOLOGY.
The load table reference number (see Temperature dependent environmental temperature loading (TDET).
RIHG Load Assignments
The RIHG assignments data section is used to assign the defined temperature dependent and User defined rate of internal heat generation to the associated elements.
RIHG [USER]
L N ilod
L
N
ilod
The element number.
The element node number as defined in ELEMENT TOPOLOGY.
The load table reference number (see Temperature dependent rate of internal heat generation (RIHG)).
Curve Definition
General curves may be defined in order to describe loads that vary with time in a dynamic analysis or to describe loads that vary with the angle around the circumference for a Fourier analysis. Curves may also be used to define the variation of load with increment number in a static analysis. A selection of predefined LUSAS system curves is available, or more generally, curves may be described completely by the user. The description of the curve (or curves) is done by using the CURVE DEFINITION command. The CURVE ASSIGNMENT command then associates load cases to a particular curve.
Curve Definition
The definition of a curve is controlled by the CURVE DEFINITION command.
CURVE DEFINITION [lcurve] [USER  SINE  COSINE 
SQUARE]
for USER curve definition:
< t i
F(t i
) > i=1,n
for SINE, COSINE, SQUARE curve definition:
amplitude frequency [phase_angle t
0
]
lcurve
Load curve number (default is the order of CURVE DEFINITION input).
ti
Interpolation variable (e.g. time, angle, increment number).
F(ti)
The value of the function at ti (positive or negative as required).
amplitude
The peak value of the wave (positive or negative as required).
frequency
The frequency of the wave (i.e. the inverse of the time period).
233
Chapter 3 LUSAS Data Input
phase_angle The offset in degrees applied to t.
t0
Notes
The value of the interpolation parameter at which the curve is activated.
1. The USER curve is assumed to be linear between defined points F(ti). It should be noted that each data point is input on a separate line. The USER curve is the default input.
2. Data should be input in order of increasing value of the interpolation parameter.
The curve should, in general, only assume 1 value at each interpolation point.
However, for Fourier static analysis a vertical segment may be used to define a stepfunction in the load distribution (see figure below).
3. If a point lies outside the USER defined curve no load is applied.
4. The LUSAS system curves are defined by:
A curve amplitude
F curve frequency
phase offset (degrees) t
0
starting value.
SINE curve t
0
0 t
0
t
0
For Fourier analysis:
A sin ft
COSINE curve t
0
0 t
0
t
0
For Fourier analysis:
A cos ft
Note. If f=0 then
A cos
for all t
SQUARE curve t
0
0 t
0
A
A
0
Note. If f=0 then if if if
A
for all t.
t
0
0
t
0
0
t
0
0
234
Curve Definition
5. Any number of curves may be specified. In the special case of an ENVT load in a thermal analysis, the temperature and heat coefficients are not applied.
6. For nonlinear static analysis the step increment number will be used to interpret the data. The INCREMENTATION data section must not be specified.
7. For Fourier analysis the load must only be applied over the angular range of 0° to
360°. Sine and cosine harmonics (without phase angle and constant specification) can be used to apply sinusoidal loading.
8. If load curves are used with NONLINEAR CONTROL the TERMINATION line must be specified to define the number of load steps to be applied. (See example below.)
F(t) F(t)
0
F(t)
(a) Fourier Single Load t
F(t)
0
(b) Fourier Multiple Loads t
0 t
0
(d) NonFourier Multiple Loads t
(c) NonFourier Single Load
Definition of Step Functions for a Fourier Static Analysis
(Black circles indicate points that must be defined)
235
Chapter 3 LUSAS Data Input
Curve Assignment
The CURVE ASSIGNMENT command assigns loads defined by the LOAD CASE commands to a particular curve which has been described using the CURVE
DEFINITION command.
CURVE ASSIGNMENT
L fac lcurve
L
Load case number (see Notes)
fac
The load factor to be applied to the load case
lcurve
The load curve number
Notes
1. If the CURVE ASSIGNMENT command is not utilised the load cases are applied as for a standard analysis.
2. If the CURVE ASSIGNMENT command is used, unassigned load cases will not be applied.
3. Curve data, both user and system, once input, cannot be overwritten, extended or amended. However, new load curves may be added. Once the CURVE
ASSIGNMENT command has been used, load curves are activated and loading is applied via factored load cases. If the CURVE ASSIGNMENT command is respecified, all existing assignments are overwritten.
4. Each curve assignment must start on a new line.
5. The load case number is defined by the order in which the LOAD CASES are input. The first load case is defined as 1, the second 2 and so on. If, during the analysis, further load cases are defined then the internal load case counter is reset to 1. In this instance, existing load cases will be overwritten.
6. The standard function of prescribed displacements and spring stiffnesses input using the SUPPORT facility is preserved. If PDSP loading is used, this data overwrites previously input data. Note that PDSP input determines the incremental displacements and not the total displacements even if LOAD CURVES are utilised. To define total displacements using load curves TPDSP should be used.
7. General curves can be used in the following applications: dynamic transient nonlinear
Fourier
Analysis Type Interpolation Variable
linear/nonlinear/explicit/implicit current response time linear/nonlinear/explicit/implicit current response time static (not arc length) increment number static circumferential angle (degrees)
236
Curve Definition
Example 1. Load Curves
The commands used to double the intensity of a face load over a period of 10 units are
LOAD CASE
FLD
1 1 0 8.
CURVE DEFINITION 3 USER
0 1 :assign a value of 1 at time/increment zero
10 2 :assign a value of 2 at time/increment ten
CURVE ASSIGNMENT
1 2 3 to load case 1.
:assign load curve 3 with a factor of 2
Example 2. Load Curves
The following example shows how to superimpose three load curves to give a combined loading of one „dead‟ load and two „live‟ loads in a static nonlinear analysis.
Unfactored loading:
4.0
1.0
7
8
1.0
9
4 6
1 2
3
237
Chapter 3 LUSAS Data Input
Load curves to be superimposed:
Factor
1.0
25
Increment
Factor
1.5
Load Curve 1
Dead load
Load Curve 2
Live load 1
Factor
1.4
9 25
Increment
Load Curve 3
Live load 2
9 13
Loading section from data file:
LOAD CASE
CL
7 9 2 0.0 1.0
8 8 0 0.0 4.0
CURVE DEFINITION 1 USER
1 1.0
21 25
Increment
238
Retained Freedoms
25 1.0
CURVE DEFINITION 2 USER
1 0.0
9 1.5
25 1.5
CURVE DEFINITION 3 USER
9 0.0
13 0.4
21 1.4
25 1.4
CURVE ASSIGNMENT
1 1.0 1
1 1.0 2
1 1.0 3
NONLINEAR CONTROL
ITERATIONS 12
CONVERGENCE 0.0 0.0 0.8 0.8
OUTPUT 0 1 4
TERMINATION 0 25
END
The use of Load Curves with Fourier Elements
Fourier loading should be input using the load curve commands to define its circumferential variation. The curve data must use q values lying between 0° and 360°.
Both system and USER curve data may be utilised. For dynamic and harmonic response analyses the Fourier load component must be input explicitly.
Retained Freedoms
The RETAINED FREEDOMS data section is used to manually define master and
slave freedoms. The definition of master and slave freedoms is required for Guyan reduced eigenvalue extraction. RETAINED FREEDOMS are also required to define the master freedoms for a superelement during the generation phase of an analysis involving superelements.
Within the Guyan reduction phase the number of master freedoms may automatically be generated to compute the correct number of iteration vectors required, nivc. This
239
Chapter 3 LUSAS Data Input
depends upon the number of master freedoms already specified in the RETAINED
FREEDOMS data section, nmastr. The number of automatically generated master freedoms would therefore be namast = nivc  nmastr.
RETAINED FREEDOMS [TITLE title]
N N last
N diff
< type i
> i=1,n
N N last
N diff
The first, last and difference between nodes of the series of nodes with identical retained freedoms.
typei
The freedom type for each global freedom at a node.
n
Notes
=M for a master degree of freedom (default)
=S for a slave degree of freedom.
The number of freedoms at a node for the structure being solved.
1. If a node number is repeated the new set of freedom types overwrites the previous set and an advisory message is printed out.
2. The master and slave codes must be separated by a space (for example M S M not
MSM).
3. Master freedoms may also be selected automatically for Guyan reduction using the
GUYAN CONTROL data chapter.
4. If the FREEDOM TEMPLATE data chapter has been utilised the freedom types specified in this section will relate to the modified freedom list.
5. If Option 131 is specified in your data file when retained freedoms are present,
(Guyan reduction and superelement generation phases), the option is switched off and a warning message is issued. (Option 131 is switched on by default).
Output Control
The location of LUSAS output may be controlled in two ways:
Element output
Node output
Stresses and strains at Gauss points and nodes are output using the ELEMENT
OUTPUT command. Nodal displacements and reactions are output using the NODE
OUTPUT command.
The frequency of output is controlled using the OUTPUT data sections in the
NONLINEAR, DYNAMIC, TRANSIENT and VISCOUS CONTROL data chapters.
Further control is provided using the OPTION facility. The relevant output control options are:
No. Output options
26 Reduce number of lines output in coordinates
240
Output Control
39
40
42
44
46
No.
32
33
34
Output options
Suppress stress output but not stress resultant output
Output direction cosines of local Cartesian systems for interface
Output element stress resultants
Stress smoothing for rubber material models
Output nodal displacement increments for nonlinear analyses
Output nodal residual forces for nonlinear
Suppress expanded input data printout except load cases
Suppress page skip between output stages
55
59
77
Output strains as well as stresses
Output local direction cosines for shells
Output principal stresses for solids
115 Output displacements and reactions in transformed axes
116 Suppress the output of internal constraint forces
143 Output shear forces in plate bending elements.
This option will produce results on an elementbyelement basis, but will not include the shear stresses in the averaged nodal results.
144 Output element results for each load case separately
147 Omit output phase
169 Suppress extrapolation of stress to nodes for semiloof shell
181 Output required results in Polar system for harmonic response analysis
208 Write plot file for pre version 10.0 LUSAS Modeller
259 Save nodal stresses in plot file to avoid stress extrapolation in
LUSAS Modeller
Element Output Control
The ELEMENT OUTPUT data section is used to define the order and contents of the element output.
ELEMENT OUTPUT [ASCENDING  SPECIFIED  SOLUTION]
[TITLE title]
L L last
L diff
iout [iavgp] [ifrmgp] [inthis]
L Llast Ldiff
The first element, last element and difference between elements of the series of elements with identical output control.
iout
The element output number
=0 for no output
=1 for nodal output
241
Chapter 3 LUSAS Data Input
=2 for Gauss point output
=3 for nodal and Gauss point output
iavgp
The averaged nodal value group number (see Notes).
ifrmgp
Parameter to control the grouping of the summation of element forces and moments for the model summary.
inthis
Parameter to control element output to the history file. Options are:
= 0 for no output.
= 1 for output.
Notes
1. If this data chapter is excluded nodal results will be output for all elements in ascending order.
2. Element numbers not specified are not output.
3. For linear problems ELEMENT OUTPUT control must be placed immediately after all loading data. The output control cannot be varied from load case to load case.
4. For nonlinear/stepbystep problems ELEMENT OUTPUT control may be placed after each LOAD CASE to change output between load increments. Once specified the ELEMENT OUTPUT control will remain active throughout the problem until respecified.
5. For load combinations ELEMENT OUTPUT control may be respecified after any
LOAD COMBINATIONS data chapter. ELEMENT OUTPUT then controls the output of the preceding load combinations and remains in force unless respecified further on.
6. If ELEMENT OUPUT is not specified after LOAD COMBINATIONS, the
ELEMENT OUTPUT control currently in force for LOAD CASES is used.
7. For enveloping ELEMENT OUTPUT control may be specified after the
ENVELOPE FINISH data line to control the output of results from an envelope.
8. Elements may be output in ascending, specified or solution order. The specified order is the order in which elements appear or are generated in the ELEMENT
OUTPUT PECIFIED data chapter. It should be noted that when assembling the output order LUSAS, firstly, groups together all elements with the same averaged nodal value grouping, secondly, groups all similar elements (that is, all solids shells, etc.) and thirdly, sorts out the specified order.
9. If averaged nodal values are required then a positive integer must be specified for
iavgp. This allows complete control to be exercised over which element nodal values are averaged together; a particularly useful facility where stresses are in local directions, i.e. shells. Any number of different groups may be specified and only elements with the same group number are averaged together.
10. The parameter ifrmgp should be specified as a positive integer that defines the group number for the summation of element forces and moments in the model summary.
242
Output Control
11. The averaged nodal values produced with ELEMENT OUTPUT do not include the thin isoflex plate shear stresses that appear in the elementbyelement output with
Option 143.
12. All element data is always written to the LUSAS Modeller post processing file.
Node Output Control
The data section NODE OUTPUT is used to control the location and content of the nodal output.
NODE OUTPUT [TITLE title]
N N last
N diff
int [inthis]
N N last
N diff
The first node, last node and difference between nodes of the series
int of nodes with identical output control.
The node output number
=0 for no output
=1 for displacements at nodes
=2 for reactions at nodes
=3 for displacements and reactions at nodes.
inthis
Parameter to control element output to the history file. Options are:
Notes
=0 for no output.
=1 for output.
1. If this data chapter is excluded nodal results will be output for all nodes in ascending order.
2. Node numbers not specified are not output
3. For linear problems NODE OUTPUT must be placed immediately after all loading data. The output control cannot be varied from load case to load case.
4. For nonlinear/stepbystep problems, NODE OUTPUT control may be placed after each LOAD CASE to change output between load increments. Once specified, the
NODE OUTPUT control will remain active throughout the problem until respecified.
5. For load combinations, NODE OUTPUT control may be respecified after any
LOAD COMBINATION data chapter. NODE OUTPUT then controls the output of the preceding load combinations and remains in force unless respecified further on.
6. If NODE OUTPUT is not specified after LOAD COMBINATIONS, the NODE
OUTPUT control currently in force for LOAD CASES is used.
7. For enveloping, NODE OUTPUT control may be specified after the ENVELOPE
FINISH data line to control the output of results from an envelope.
8. Note that for field analyses, the displacement output (int=1 or 3) will be replaced by field values, thermal gaps or radiation surface flows.
243
Chapter 3 LUSAS Data Input
9. All nodal data is always written to the LUSAS Modeller post processing file.
Example 1. Element and Node Output with Load Combination
Y,v
13 14 15
Load case 1 Load case 2
12.
5
12.
5
7 8
9 8 11
12.
5
4
5
5 6 7
12.
5
12.
5
X,u
Plane stress problem:
LOAD CASE
CL
7 15 4 12.5
LOAD CASE
CL
7 0 0 12.5
15 0 0 12.5
ELEMENT OUTPUT ASCENDING
4 5 1 1
8 0 0 1
NODE OUTPUT
5 7 1 3
13 15 1 3
LOAD COMBINATION
244
Output Control
5.0 1
2.5 2
LOAD COMBINATION
3.0 1
4.5 2
ELEMENT OUTPUT SPECIFIED
4 7 3 3
5 8 3 2
LOAD COMBINATION
1.5 2
1.5 1
ELEMENT OUTPUT ASCENDING
5 0 0 1
Example 2. Element and Node Output for a Single Load Case (Linear)
Y,v
13 14 15
12.5
7 8
9 8 11
12.5
4 5
5 6 7
12.5
X,u
LOAD CASE
CL
7 15 4 12.5
ELEMENT OUTPUT
245
Chapter 3 LUSAS Data Input
C Gauss point stresses for element 4
4 0 0 2
NODE OUTPUT
C Displacement and reaction output
C for nodes 5, 6 and 7
5 7 1 3
Example 3. Element and Node Output for Single Load Case (Nonlinear)
LOAD CASE
CL
7 15 4 12.5
ELEMENT OUTPUT
4 0 0 3 : gives Gauss point and nodal stresses for element number 4
: the omition of the NODE OUTPUT command gives displacements and
: reactions for all nodes
NONLINEAR CONTROL
Load Combinations
The data section LOAD COMBINATIONS may be used to combine the results obtained from individually defined load cases.
LOAD COMBINATIONS [N] [TITLE title] fac L
N
fac
L
Notes
The load combination number (default sequential, starting with load combinations 1).
The multiplication factor for load case.
The load case to be factored.
1. Only results from LOAD CASES initially specified in the data input may be factored.
2. There is no limit on the number of LOAD COMBINATIONS which may be processed.
246
Enveloping Results
3. There is no limit on the number of LOAD CASES which may be factored to create a LOAD COMBINATION.
4. If a load case is specified more than once in the LOAD COMBINATION data the factors are accumulated.
5. The load case number is implicitly assigned in the order of declaration of the
LOAD CASES in the datafile. It must not be specified with the LOAD CASE data section.
6. A PLOT FILE cannot be specified after LOAD COMBINATION.
7. The results of a LOAD COMBINATION and the combination data itself is not transferred to the LUSAS Modeller postprocessing file.
8. LOAD COMBINATION can also be carried out in LUSAS Modeller.
Enveloping Results
The ENVELOPE data section may be used to extract the maximum and minimum values from a series of enveloped linear analyses.
A particular load envelope is specified between the commands ENVELOPE START and ENVELOPE FINISH. The LOAD COMBINATION commands appear between the envelope commands. Output control for the envelope is specified immediately after the ENVELOPE FINISH command. Specification of nodal and element output within the envelope will be applied to the preceding LOAD COMBINATIONS.
ENVELOPE {START  FINISH}
Notes
1. Enveloping is available for all elements in the LUSAS Element Reference Manual.
2. The enveloping facility may be used in conjunction with the RESTART facility if required.
3. Enveloping must be used in conjunction with the LOAD COMBINATION facility.
4. Enveloping can also be carried out in LUSAS Modeller.
Superelements
Large finite element models may be divided into smaller, more manageable components which are added together to form the complete structure in a subsequent analysis. These components are referred to as „superelements‟. A superelement may be defined as an assembly of individual elements together with a list of master freedoms that will represent the superelement once it has been reduced. The SUPERELEMENT family of commands provides this facility in LUSAS for linear static, eigenvalue, nonlinear and transient dynamic analyses. An option also exists to evaluate the natural frequencies of a large structure from the eigen solutions of the individual superelements using modal synthesis.
247
Chapter 3 LUSAS Data Input
In addition a component for which the user modal data (frequencies and eigenvectors) is available can be utilised to obtain the natural frequencies of a large structure. This component will be referred to as a user modal superelement. A detailed explanation of these facilities can be found in the LUSAS Theory Manual.
Analyses involving superelements may be divided into three basic stages:
Opening databases and creating superelement data.
Using superelements and/or user modal data in an analysis (i.e. solving the complete structure). This stage could involve user modal data only if superelements are not used.
Recovering displacements and stresses within the superelements.
The superelement data may be created in one or several analyses and stored in several databases. Once generated, the superelements may be used in either static, natural frequency, nonlinear or transient dynamic analysis. The recovery procedure permits the displacements, stresses and strains of a superelement to be recovered. Additional concentrated loads and prescribed displacements are permitted during the combination pass of an analysis. In the create phase, both static and natural frequency analyses of an individual superelement may be performed to validate the data.
The following restrictions apply to the use of superelements:
1. If nonlinear analysis are undertaken the super elements will behave linearly.
2. Superelements cannot be generated from Fourier elements.
3. User modal data may only be used for natural frequency analyses
4. Material properties must be constant. If temperature dependent properties are input then the values corresponding to the initial temperature will be used.
5. Superelement generation/recovery is limited to one superelement per analysis run.
6. When a superelement connects to other nonsuperelements, the connecting node locations associated with the nonsuperelements must have the same relative locations as originally used in generating the superelement. In addition, the
Cartesian sets for the nodes must coincide.
7. If superelements are used without any standard elements the FREEDOM
TEMPLATE data chapter must be included.
8. If superelements are used that have more freedoms than the standard elements, and any values are to be prescribed for these freedoms, then the FREEDOM
TEMPLATE data chapter must be included. These values may be defined in
SUPPORT CONDITIONS, CONSTRAINT EQUATIONS, RETAINED
FREEDOMS or LOADCASE data chapters.
9. User modal data eigenvectors must be in the structure global axes.
How to use Superelements
The general approach for using the SUPERELEMENT facility in LUSAS is explained through a description of input data files required at each stage of a typical analysis
248
Superelements
using superelements. The output files provided at each stage are also listed and their use in subsequent stages of the analysis is defined. The figure on Recovery Phase gives a schematic diagram of a complete superelement analysis together with the input and output files at each stage. An example of data files required for each phase of the analysis is provided on Examples of Using Superelements.
Creating Superelements
A typical data file for creating superelements would contain SUPERELEMENT
ASSIGN and SUPERELEMENT DEFINE commands. The master freedoms for the superelement would be specified using the RETAINED FREEDOMS data chapter.
This analysis would then create:
A superelement database
An output file
A restart file (optional)
The contents of the files created would depend upon the control parameters specified under the subcommands of SUPERELEMENT DEFINE. Only one superelement can be generated in a single analysis.
Using Superelements in an Analysis
A typical data file for using superelements in an analysis to solve the complete structure would contain the SUPERELEMENT USE command and may also contain
SUPERELEMENT DEFAULT or DISTRIBUTE commands. These commands would reference databases created in the superelement creation phase. Additional elements, boundary conditions or loading may be specified at this stage. This analysis would then create:
Superelement result database(s)
An output file
A restart file (optional)
A LUSAS Modeller plot file (optional)
Several superelement databases may be used in this stage of the analysis. In addition user modal superelements may be included to form the complete structure using the
SUPERELEMENT MODAL_DATA command. User modal superelements can also be used in isolation (see Utilising User Modal Data in an Analysis below). If a LUSAS
Modeller plot file is created it will NOT contain the superelement results.
Recovering Superelement Results
A data file for recovering superelement results using output from the previous analysis stage would contain the SUPERELEMENT RECOVER command and may also contain a SUPERELEMENT DEFAULT command. These commands would reference
249
Chapter 3 LUSAS Data Input
output databases created during solution of the complete structure. This analysis would then create:
An output file
A restart file (optional)
A LUSAS Modeller plot file (optional)
If the superelement generation restart file is not available recovery may be performed using the original data file. Only one superelement may be recovered in each analysis.
Utilising User Modal Data in an Analysis
A typical data file for utilising user modal data in an analysis to solve the complete structure would contain the SUPERELEMENT MODAL_DATA command. This command would reference a neutral file containing the component connectivity nodes and freedoms, frequencies and references to result files containing the eigenmodes.
Additional user modal data components, elements, superelements or boundary conditions may be specified at this stage. The analysis would then create:
An output file
A restart file (optional)
A LUSAS Modeller plot file (optional)
If a LUSAS Modeller plot file is created it will NOT contain the user modal data results.
A Typical Superelement Analysis
A typical analysis sequence to generate two superelements and use them with a user modal superelement and a group of LUSAS elements in the complete structure would be as follows (see figure on Recovery Phase):
Generation Phase
Analysis 1
Input
define1.dat
Output
define1.out define1.mys (optional) define1.rst (optional) define1.sfr (rename to recov1.sfr or delete) dbname1.sda
Analysis 2
Input Output
define2.dat define2.out
250
Superelements
Analysis 2
Input Output
define2.mys (optional) define2.rst (optional) define2.sfr (rename to recov2.sfr or delete) dbname2.sda
Solution Phase
Analysis 3
Recovery Phase
Analysis 4
Input
use1.dat dbname1.sda dbname2.sda use1.def use1.adp
Output
use1.out use1.rst (optional) use1.mys (optional) dbname1.srs dbname2.srs
Input
recov1.dat define1.rst
(optional) recov1.sfr
(optional) dbname1.sda
Output
recov1.out recov1.mys (optional) recov1.rst (optional) dbname1.srs
Analysis 5
Input
recov2.dat define2.rst
(optional) recov2.sfr
(optional)
Output
recov2.out recov2.mys (optional) recov2.rst (optional) dbname2.sda dbname2.srs
The file extensions .sda and .srs relate to superelement data and results databases respectively. The extension .sfr indicates a file containing the reduced frontal matrices.
If the appropriate .sfr file is accessible during the recovery phase, the solution is recovered from the back substitution of the equations leading to a more efficient solution. To take advantage of this facility the .sfr file must have the same prefix as the
251
Chapter 3 LUSAS Data Input
data file used in the recovery, i.e. copy define1.sfr to recov1.sfr in above example. If a superelement restart file (.rst) is not available, recovery may be performed by redefining the superelement in the datafile (i.e. as in the superelement creation phase).
Note. The .mys, .rst, .sfr, .sda and .srs files are all binary files. The .dat and the .out files are ASCII files which can be read and edited directly by the user. The user modal data files (.def and .adp) are ASCII files.
dat out dat out define1 rst sfr sda mys define2 dat def/adp sda sfr rst mys use1 dat recov1 srs rst out srs mys recov2 dat mys out rst out mys rst
process (or analysis phase)
ASCII files (extension shown) binary files (extension shown) necessary input/output data paths optional input/output data paths
Main Stages of an Analysis Involving Superelements
Component Mode Synthesis Using Superelements
Component mode synthesis provides a method of evaluating the natural frequencies of a large structural system by utilising the eigen solutions of the component parts.
Additional generalised freedoms (or modal coordinates) are introduced which enable an enhanced representation of the reduced mass and stiffness to be computed for each superelement. The superelement matrices are then combined and the eigensolution for
252
Superelements
the complete structure is evaluated. More details can be found in the LUSAS Theory
Manual.
The eigenvalues evaluated using this method of analysis will always be an upper bound on the corresponding exact values of the system. The accuracy of each eigenvalue and corresponding eigenvector is dependent upon how accurately the boundary conditions are represented in the eigenanalysis of each of the components.
The component mode reduction can be carried out whilst defining a superelement, or as an updating procedure if the superelement has already been defined. During this phase
LUSAS calculates the natural frequencies of the superelement. Using this eigensolution the reduced stiffness and mass are computed for the superelement, in terms of the master freedoms and generalised coordinates. For these computations the required number of generalised coordinates must be defined in the data input.
Generalised coordinates are extra (fictitious) degreesoffreedom that are utilised to enhance the stiffness and mass of the superelement and allow a more accurate dynamic (eigen or transient) solution of the complete structure to be computed without the specification of extra retained (or master) freedoms.
In addition, the modal supports for the master freedoms must also be specified as
„fixed‟, „free‟ or „spring stiffness and mass‟.
For many structures the alternatives „fixed‟ or „free‟ are not sufficient for accurate modelling. In order to improve modelling it is possible to:
Introduce spring stiffnesses and masses on the exterior freedoms to represent the effects of the remaining structure. This requires you to estimate the stiffness and mass of the remaining structure.
Automatically reduce the stiffness and mass of the remaining structure to the master freedoms. This can be achieved in two ways:
once the component mode reduction has been carried out for each superelement the complete structure can be assembled and the natural frequencies computed. At this stage it is also possible to automatically distribute the mass and stiffness of the complete structure to each superelement.
alternatively the stiffness and mass can be distributed before any natural frequencies are calculated at the superelement level. Once this redistribution has been carried out the natural frequencies of the individual superelements can be computed more accurately.
Opening Superelement Files
Superelement databases are opened using the SUPERELEMENT ASSIGN command.
SUPERELEMENT {ASSIGN dbname filename  DEFAULT dbname}
253
Chapter 3 LUSAS Data Input
ASSIGN
Opens a new superelement database.
DEFAULT Changes the default superelement database.
dbname
Internal name of database.
filename External name of file containing database.
Notes
1. If a filename is not provided, the filename will default to dbname.
2. Several superelement databases may be used at any one time. Use of the
DEFAULT option changes the default database for subsequent operations.
3. ASSIGN sets the database defined as the default database.
Superelement Creation
The superelement to be created will contain information on element topology and usually requires specification of boundary freedoms, loading and reduction options.
The SUPERELEMENT DEFINE command defines the name and title associated with the superelement.
Superelement Definition
SUPERELEMENT DEFINE defines the superelement name and internal database that is used to store the superelement information.
SUPERELEMENT DEFINE sname [dbname] [TITLE title]
sname
Superelement name.
dbname
Internal name of database.
Notes
1. Each superelement in an analysis must have a unique identification name.
2. If dbname is not specified then either:
3. The current default database will be used if available, or
4. The database will default to sname if a default database is not available.
Constants
The CONSTANTS data section defines the control parameters for the superelement creation phase. A list of valid names defines the output required.
CONSTANTS [LOAD] [STIF] [MASS] [STAT] [EIGN]
LOAD
STIF
MASS
Save the reduced load vector.
Save the reduced stiffness matrix.
Save the reduced mass matrix.
254
Superelements
STAT
EIGN
Notes
Perform a static analysis using superelement.
Perform an eigenanalysis using superelement.
1. If the CONSTANTS command is not specified LOAD and STIF will be invoked by default. However, if Option 90 is set then LOAD, STIF and MASS will be the default control parameters.
2. If the command GENERALISED COORDINATES is specified the following default operations will be carried out:
The reduced mass matrix will be saved.
An eigenanalysis will be performed to compute the eigenvectors required.
The enhanced reduced stiffness and mass will be computed and saved.
Output
The OUTPUT command defines the information to be presented in the results output file.
OUTPUT [MAST] [LOAD] [STIF] [MASS] [DRCO] [CORD]
MAST
LOAD
STIF
MASS
DRCO
CORD
Notes
Master freedom description.
Reduced load vector.
Reduced stiffness matrix.
Reduced mass matrix.
Nodal direction cosine matrices.
Nodal coordinates.
1. By default, only a summary of the superelement data will be provided.
Generalised Coordinates
The GENERALISED COORDINATES command defines the number of generalised coordinates to be utilised in the exterior freedom set for the superelement. These additional freedoms allow an enhanced representation of the superelement mass and stiffness to be computed thereby providing a more accurate solution when the complete structure is analysed.
m
GENERALISED COORDINATES m
Number of generalised coordinates
255
Chapter 3 LUSAS Data Input
Notes
1. If the GENERALISED COORDINATES command is specified an eigenvalue analysis will be performed to compute max(m,nroot) eigenvalues and corresponding eigenvectors using either Subspace iteration or Guyan reduction.
2. If the eigenvalue solution method is not specified subspace iteration will be used by default.
Modal Supports
The MODAL SUPPORT command defines the support conditions for the master freedoms for local superelement eigenanalysis. This information is also used for computation of the eigenmodes associated with generalised coordinates. Further additional master freedoms may be specified for a local eigenvalue analysis using
Guyan reduction.
MODAL SUPPORT [STIF] [MASS]
N N last
N diff
< type i
> i=1,n
< stif i
> i=1,n
< mass i
> i=1,n
STIF
Stiffness flag.
MASS
Mass flag.
N N last
N diff
The first node, last node and difference between nodes of the series of nodes with identical modal supports.
typei
Modal support code for each freedom at the nodes. Valid types are:
R  Master freedom restrained.
F  Master freedom free.
S  Spring support for master freedom.
G  Denotes interior freedoms as masters for local eigenvalue analysis (see
Notes).
stifi
Stiffness for spring support.
massi
Mass for spring support.
n
Notes
Total number of degreesoffreedom at the node.
1.
By default, master freedoms are restrained („R‟) in a local eigenvalue analysis.
2. MODAL SUPPORT has no influence in static analyses.
3. Retained freedoms of type „G‟ should only be specified if Guyan reduction is being used to compute the eigensolution of the superelement. The freedoms are not used in subsequent superelement operations.
4. The FREEDOM TEMPLATE data chapter must be used when MODAL
SUPPORTS are specified.
256
Superelements
Using Superelements
Superelements are utilised for two reasons:
to solve the complete structure
to redistribute the masses and stiffnesses for eigenanalyses.
The SUPERELEMENT USE command is used in both of these cases.
When solving the complete structure additional elements, loading, boundary conditions and user modal data may also be added directly with the complete structure. The complete structure is defined as the combination of the lowest level superelements.
When the complete structure is solved, the displacements relating to all master freedoms are written to the appropriate superelement database(s).
The masses and stiffnesses of the complete structure can be redistributed to the boundaries of each of the superelements using the SUPERELEMENT DISTRIBUTE
COMMAND (see Distribution of Mass and Stiffness in Modal Synthesis). In order to do this the complete structure must be formed by utilising the SUPERELEMENT USE command.
SUPERELEMENT USE sname dbname
sname
Name of superelement to be solved.
dbname
Database where superelement is stored.
Notes
1. Several superelements may be included in the complete structure.
2. If dbname is not specified then either:
3. the current default database will be used if available, or
4. the database will default to sname if a default database is not available.
5. If SUPERELEMENT ASSIGN has not been defined the filename which contains the superelement database, dbname, will be assumed to be the filename.
6. Additional loads and boundary conditions may only be added to the nodes specified as masters in the creation phase.
7. Additional load conditions permitted are concentrated loads (CL) only. Elements loads are not permitted at this stage.
Utilising User Modal Data
The SUPERELEMENT MODAL_DATA command is used to define modal data for a component of the complete structure. This command is only valid for natural frequency analyses.
SUPERELEMENT MODAL_DATA uname
OUTPUT {STIFF  MASS}
257
Chapter 3 LUSAS Data Input
uname
Name of neutral file containing user modal data.
STIF
Reduced stiffness matrix to be output.
MASS
Note
Reduced mass matrix to be output.
1. Several user modal superelements may be included in the complete structure.
User Modal Data Neutral File
The user modal data neutral file (with a file extension .def) has two lines for a title
(packet type 25) followed by two lines for a subtitle (packet type 26 usually date, time and version). This is followed by the user modal data (packet type 27). This file can be in free format or in fixed format and the format type is specified on the first line of the neutral file. The results files (with a file extension of .adp) utilised in this neutral file must also be in this format.
The file format type for the neutral file and associated result files is specified on the first line of the neutral file as free or fixed. In free format you can input data in any column with a spacing between descriptors or numbers. fixed format requires the numbers to be input in certain columns. If this line is omitted or an unrecognised format type is encountered free format is assumed.
FORMAT
FORMAT
FORMAT
Format (A)
= File format type (FREE or FIXED)
The header line for each data packet contains the following information:
HEADER
Fixed Format (I2,8I8) or FREE format
IT ID IV KC N1 N2 N3 N4 N5
IT
ID
IV
= packet (or Entity) type
= identification number. A “0” value means not applicable
= additional ID. A “0” value means not applicable
KC
= line count (number of lines of data after the header)
N1 to N5 Supplemental integer values used and defined as needed.
PACKET TYPE 25: TITLE
HEADER
Fixed Format (I2,8I8) or FREE format
258
Superelements
25 0 0
ID = 0 (n/a)
IV = 0 (n/a)
KC = 1
1
USER TITLE Format (A)
TITLE
TITLE = identifying title, may be up to 80 characters
PACKET TYPE 26: SUMMARY DATA
HEADER
26 0
ID
IV
KC
= 0 (n/a)
= 0 (n/a)
= 1
Fixed Format (I2,8I8) or FREE format
0 1
SUMMARY DATA
Format (A)
DATA
DATA = character string containing Date:Time:Version
PACKET TYPE 27: USER MODAL DATA
HEADER
Fixed Format (I2,8I8) or FREE format
27 0
ID
IV
N1
N2
N3
KC
0 KC N1 N2 N3
= 0 (n/a)
= 0 (n/a)
= maximum number of freedoms to a node
= total number of boundary nodes i.e. connectivity to complete structure
= number of eigenmodes
= 1 + N2 + (N3 + 4) / 5 + N3
259
Chapter 3 LUSAS Data Input
TEMPLATE Fixed Format (20A4) or FREE format
FRETYP
FRETYP
= freedom types at a node (N1 values specified)
For valid freedom types (see Freedom Template)
NODAL FREEDOM Fixed Format (10I8) or free format
NNODE
NF9
NF1 NF2 NF3 NF4 NF5 NF6 NF7 NF8
NNODE = boundary node number  this node must exist in the structure and the results files
NF1 to NF9 nodal freedoms (results column number in results file)  do not specify more than N1 freedoms
FREQUENCIES
Fixed Format (5E16.9) or FREE format
FREQ
FREQ = natural frequencies for each mode
RESULTS FILE
Format (A)
EIGFLE
EIGFLE
= name of results file for this mode number
 this file contains the mass normalised eigenvectors and can be in free or fixed each format as specified on the first line in the neutral file, this line is repeated for mode
See Examples of Using Superelements for an example of a user modal data neutral file.
User Modal Data Results Files
The user modal data results file (with a file extension .adp) has one line for a title followed by a line for nodal information. This is followed by two lines for subtitles,
260
Superelements
followed by nodal displacements (a line for each node). This file must be in free or fixed format as specified in the user modal data neutral file.
RESULTS FILE DATA
TITLE
Format (A)
TITLE
TITLE = identifying title, may be up to 80 characters
NODAL INFORMATION
Fixed Format (2I9,E15.6,2I9) or free format
NNODES MAXNOD
NNODES
MAXNOD
DEFMAX
NDMAX
NWIDTH displacements
DEFMAX
= number of nodes
= highest node number
= maximum absolute displacement
NDMAX NWIDTH
= node number where maximum displacement occurs
= number of result columns after NODID for nodal freedom
SUBTITLE1 Format (A)
SUBTITLE
SUBTITLE
= identifying subtitle, may be up to 80 characters
SUBTITLE2 Format (A)
SUBTITLE
SUBTITLE
= identifying subtitle, may be up to 80 characters
DISPLACEMENTS Fixed Format (I8,5E13.7) or free format (for each node)
NODID (DATA(J),J=1,NWIDTH)
NODID = node number
DATA = nodal freedom displacements
261
Chapter 3 LUSAS Data Input
See Examples of Using Superelements for an example of a user modal data results file.
Recovery of Superelement Data and Results
The SUPERELEMENT RECOVER command permits superelement results to be recovered from the database. This process involves reflation of the reduced solution for a superelement to obtain the solution of the constituent elements. The superelement database will contain the displacements relating to the exterior freedoms computed in the solution of the complete structure. In the recovery stage of the analysis these displacements will be used to compute internal displacements, stresses and strains for the superelement.
SUPERELEMENT RECOVER sname dbname
CONSTANTS {STAT  EIGN  NONL inc  DYNA nt }
sname
Name of superelement to be solved.
dbname
Database where superelement is stored.
STAT
EIGN
Recover information from static analysis (see Notes).
Recover information from eigenanalysis (see Notes).
NONL inc Recover information from nonlinear analysis on specified increment.
DYNA nt Recover information from dynamic analysis on specified time step.
Notes
1. If dbname is not specified then either:
The current default database will be used if available, or database will default to sname if a default database is not available.
2. If SUPERELEMENT ASSIGN has not been defined the filename which contains the superelement database, dbname, will be assumed to be the filename.
3. If the CONSTANTS command is not specified the results from the most recent analysis will be recovered.
4. A more efficient solution can be obtained if the appropriate file containing the reduced frontal matrices is utilised in the recovery stage. These files can be recognised by the extension .sfr and are produced during the superelement creation phase. To take advantage of this facility, the previously created .sfr file must be renamed to fname.sfr, where fname is the name of the data file used in the recovery. Using this approach the reassembly of the reduced frontal matrices is avoided and the solution is achieved directly from the back substitution. However, it should be noted that the .sfr files are generally quite large and may require a considerable amount of storage.
5. When recovering problems in which generalised coordinates have been used the sfr file should be used in the recover process to maintain consistancy.
262
Superelements
Distribution of Mass and Stiffness in Modal Synthesis
Generally, the master freedoms of a superelement are assumed to be either fixed or free. A better approximation is usually obtained by utilising point masses and stiffnesses to represent the effects of the remaining structure. This is accomplished by reducing the mass and stiffness of the complete structure to the boundary nodes of each chosen superelement. To achieve this, the master freedom codes for each superelement are modified and a Guyan reduction analysis is performed. This provides the reduced stiffness and mass from which the superelement stiffness and mass are subtracted to give the boundary mass and stiffness.
The SUPERELEMENT DISTRIBUTE command specifies that an analysis is to be performed to distribute mass and stiffness from the complete structure to each superelement in modal synthesis analysis. The complete structure must be formed by utilising the SUPERELEMENT USE command for each superelement that is to be included.
SUPERELEMENT DISTRIBUTE sname dbname
sname
Name of superelement to be solved.
dbname
Database where superelement is stored.
Notes
1. Several superelements may be included in the complete structure (see Using
Superelements).
2. If dbname is not specified the data will be recovered from the default database set using the SUPERELEMENT ASSIGN/DEFAULT command.
3. If SUPERELEMENT ASSIGN has not been defined the filename which contains the superelement database, dbname, will be assumed to be the filename.
Examples of Using Superelements
This section provides an example of the data files required to execute the basic phases of an analysis using superelements.
Example 1. Superelement Generation Phase
PROBLEM TITLE Superelement generation phase
BEAM ELEMENT TOPOLOGY
FIRST 1 1 2
INC 1 3 3 3
NODE COORDINATES
FIRST 1 0 0
263
Chapter 3 LUSAS Data Input
INC 1 5 0 2
INC 3 0 5 5
BEAM GEOMETRIC PROPERTIES
1 0.01 0.0001 1.0
GEOMETRIC ASSIGNMENTS
1 3 1 1
MATERIAL PROPERTIES
2 210E9 0.3
MATERIAL ASSIGNMENTS
1 3 1 2
FREEDOM TEMPLATE
U V THZ
SUPPORT NODES
1 7 3 R R R
RETAINED FREEDOMS
2 8 3 M M M
C
C Open a superelement database SEDBSE in an external file SEEXTF
SUPERELEMENT ASSIGN SEDBSE
C
SEEXTF
C Define the name of this superelement as SENAME and store in the default database SEDBSE
TITLE First SUPERELEMENT DEFINE SENAME superelement
C
C Save the reduced stiffness and mass for SENAME in
SEDBSE
CONSTANTS
C
STIF MASS
C Present the master freedom description and reduced stiffness in the results output file
OUTPUT MAST STIF
264
Superelements
C This restart file will be referred to as SEREST
RESTART WRITE
END
Example 2. Superelement Mass and Stiffness Distribution Phase
PROBLEM TITLE Superelement mass and stiffness distribution phase
C
C Open the superelement database SEDBSE in the external file SEEXTF
SUPERELEMENT ASSIGN SEDBSE
C
SEEXTF
C Include the superelement SENAME (which is stored in database SEDBSE) into the analysis.
SUPERELEMENT USE
C
SENAME SEDBSE
C Include other superelements into the complete structure
C
C Distribute mass and stiffness to superlement
SUPERELEMENT DISTRIBUTE
END
SENAME SEDBSE
Example 3. Superelement Solution Phase
PROBLEM TITLE Superelement solution phase
QPM4 ELEMENT TOPOLOGY
FIRST 1 2 3 6 5
INC 1 3 3 3 3 4
NODE COORDINATES
FIRST 2 5 0
INC 1 5 0 2
INC 3 0 5 5
QPM4 GEOMETRIC PROPERTIES
265
Chapter 3 LUSAS Data Input
1 0.01 0.01 0.01 0.01
GEOMETRIC ASSIGNMENTS
1 4 1 1
MATERIAL PROPERTIES
2 210E9 0.3
MATERIAL ASSIGNMENTS
1 4 1 2
FREEDOM TEMPLATE
U V THZ
SUPPORT NODES
2 3 1 F R R
14 15 1 F R R
LOAD CASE
CL
3 15 12 10 0 10
6 12 3 20
C
C Open the superelement database SEDBSE in the external file SEEXTF
SUPERELEMENT ASSIGN SEDBSE
C
SEEXTF
C Include the superelement SENAME (which is stored in database SEDBSE) into the analysis.
SUPERELEMENT USE
C
SENAME SEDBSE
C Include other superelements into the complete structure
C Include user modal data USE1 into the analysis.
SUPERELEMENT MODAL_DATA USE1
C
C Include other user modal superelements into the complete structure
EIGENVALUE CONTROL
266
Superelements
CONSTANTS 5 D D 1
PLOT FILE
END
Example 4. Superelement Recovery Phase
RESTART READ 1 SEREST
C Recover the superelement SENAME results for the most recent analysis
C
C Open the superelement database SEDBSE in the external file SEEXTF
SUPERELEMENT ASSIGN SEDBSE
C
SEEXTF
C Recover the superelement results
SUPERELEMENT RECOVER SENAME SEDBSE
RESTART WRITE
PLOT FILE
END
Example 5. User Modal Neutral File
FREE FORMAT
25 0 0 1
User modal data for two beams with total of six freedoms
26 0 0 1
220993:12:00:V11.0
27 0 0 11 3 2 6
U V THZ
11 1 2 3
14 1 2 3
0.145609E+02 0.162796E+02 0.141941E+03
0.158695E+03 357.302
399.476
267
Chapter 3 LUSAS Data Input use1.adp use2.adp use3.adp use4.adp use5.adp use6.adp
99
Example 6. User Modal Results File
USE1  Two beams with total of six freedoms (One of six result files)
10 14 0.127609 14 3 use1 GLOBAL DISPLACEMENTS
MODE = 1
1 0.0000000E+00 0.0000000E+0 0.0000000E+00
2 0.0000000E+00 0.8983746E17 0.2475554E17
4 0.0000000E+00 0.0000000E+00 0.0000000E+00
5 0.0000000E+00 0.5336911E16 0.1470636E16
7 0.0000000E+00 0.0000000E+00 0.0000000E+00
8 0.0000000E+00 .1740663E15 .4773746E16
10 0.0000000E+00 0.0000000E+00 0.0000000E+00
11 0.0000000E+00 .1007247E14 .2966510E15
13 0.0000000E+00 0.0000000E+00 0.0000000E+00
14 0.0000000E+00 0.1276092E+00 0.3516390E01
Analysis Control
The following types of analysis control data chapters are available for the control of specific LUSAS analysis types:
NONLINEAR CONTROL
DYNAMIC CONTROL
TRANSIENT CONTROL
VISCOUS CONTROL
EIGENVALUE CONTROL for nonlinear analysis for stepbystep dynamic analysis for transient field analysis for creep analysis for eigenvalue extraction analysis
268
Nonlinear Control
GUYAN CONTROL for Guyan reduced eigenvalue analysis
MODAL_DAMPING CONTROL for computation of distributed damping
SPECTRAL CONTROL for spectral response analysis
HARMONIC_RESPONSE CONTROL for forced vibration analysis
FOURIER CONTROL for Fourier analysis
Nonlinear Control
The NONLINEAR CONTROL data chapter is used to control the solution procedure for nonlinear analyses. For further information regarding the solution of nonlinear problems refer to Nonlinear Analysis, and the LUSAS Theory Manual.
NONLINEAR CONTROL
Incrementation
The INCREMENTATION data section specifies how an automatic solution is to proceed. Input only if using an automatic procedure.
Manual load incrementation Manual incrementation may be specified by repetition of the LOAD CASE data chapter after the
NONLINEAR CONTROL chapter, hence explicitly defining the required loading parameters. The general form of manual incrementation is therefore:
LOAD CASE
NONLINEAR CONTROL
LOAD CASE
LOAD CASE
LOAD CASE etc.
Where loads are being specified, the total values at each step must be input. In contrast, displacement increments are additive, and hence the incremental change should be specified. It should be noted that, when using manual incrementation, since the incrementation and final levels are defined explicitly, the INCREMENTATION and TERMINATION sections of the
NONLINEAR CONTROL data chapter are redundant.
Automatic load incrementation Automatic incrementation for nonlinear problems is controlled via the INCREMENTATION section of the
NONLINEAR CONTROL data chapter. In this case, only the initial LOAD
CASE is specified and the incrementation is controlled by the
INCREMENTATION and TERMINATION sections of the NONLINEAR
CONTROL data chapter. The general form of automatic incrementation is therefore:
LOAD CASE
NONLINEAR CONTROL
269
Chapter 3 LUSAS Data Input
INCREMENTATION
TERMINATION
When using automatic incrementation, the initial loading components specified in the LOAD CASE data chapter are multiplied by the current load factor. The starting load factor is specified as the parameter slamda in the
INCREMENTATION data section.
INCREMENTATION slamda [dlamdx isurfc itd cstifs dellst delsmx]
slamda
Starting reference load factor (default = 1.0 on first increment, default =
0.0 on subsequent increments).
This is the factor by which the reference load level will be multiplied for the predictor, or first iteration, of the next load increment. This load level will remain constant if
isurfc=0 (constant load level). Must be nonzero at the first increment but may subsequently be respecified as zero if the new load factor is to be computed from the previous convergence history (i.e. using itd).
dlamdx
The maximum absolute change in the load factor on iteration zero of any load increment.
This parameter is used when the load level is automatically adjusted following consideration of the iterations desired for convergence against those achieved. The effect of the parameter is to limit the rate of change of load in an increment. If zero is input, no limit will be applied. If a D is input, the default value of dlamdx =
2.0*(tlamda  slamda) is taken; tlamda is the total load factor at the end of the previous increment.
Note. If a nonzero value of dellst is specified in an analysis controlled by the arclength method (isurfc=1 or 2) then:
the maximum incremental arclength parameter delsmx will be used to limit the step size of subsequent increments, and
slamda will have no effect (i.e. dellst will be used to control the new increment).
isurfc
The constant load level or arclength control parameter (default=0)
If specified as zero, the loading will remain constant during the iteration process (that is, the „constant load level procedure‟). If input as one or two, the loading will vary during the iterations (that is, an „arclength‟ procedure, see Notes on TERMINATION).
Two algorithms based on the arclength method are available in LUSAS:
Crisfield‟s modified approach
itd
Rheinboldt‟s arclength method
The number of desired iterations per load increment (default = 4)
270
Nonlinear Control
When using automatic incrementation, the loading variable (load or arclength) is varied according to the number of iterations taken to converge on the preceding step. If the number of iterations taken for convergence exceeded the desired number, specified by itd, then the loading variable is decreased; conversely, if the number of iterations taken to converge was less than the desired number, the step length is increased. Hence the rate of change of loading variable is adjusted depending on the degree of nonlinearity present. If zero is input, the load variable will remain constant.
cstifs
The current stiffness parameter value at which the solution will switch from a constant load level to an arclength procedure (default = 0.4). The current stiffness parameter varies between 1.0 (initially) and 0.0 at a horizontal limit point. It is therefore a useful measure of structural collapse. One may wish to start with load control (isurfc=0) and have the program automatically switch to arclength control as structural collapse is neared. Measuring structural stiffness with the current stiffness parameter, once the current stiffness parameter falls below the threshold value of cstifs the program automatically switches to arclength control. If zero is input, the parameter is ignored.
Note. itd must be given a positive value to use this facility, and isurfc must equal zero.
dellst
The incrementallength value required to restart an analysis under arclength control. When applying a restart with the structure near to collapse, it is advisable to use arclength control (isurfc=1). If the loaddeflection response is very flat, it is impractical to restart (as normal) by specifying a load factor, slamda.
Instead, it is better to specify an „arclength increment‟, dellst. An appropriate value for dellst can be obtained by looking at output values of the arc length in the iterative log or output files, of prior arclength increments, deltl. If dellst is nonzero this value will be used for the new load increment instead of slamda no matter what value of slamda is specified.
delsmx
The maximum value of dellst for subsequent increments (default is calculated as delsmx =2*dellst).
If delsmx is nonzero this value will be used to limit the size of subsequent increments instead of dlamdx no matter what value of dlamdx is specified.
Step Reduction
The STEP_REDUCTION data section defines how a load increment will be reduced if convergence difficulties occur. This section is only applicable when values have been specified under INCREMENTATION.
STEP_REDUCTION [mxstrd stpred stpfnl]
271
Chapter 3 LUSAS Data Input
mxstrd
The maximum number of times a step reduction can occur on a single increment (default = 5). If input as zero step reduction will be suppressed.
stpred
The factor used to reduce the load increment on a step reduction (default =
0.5).
stpfnl
The factor used to increase the original load increment if mxstrd step reductions have failed to achieve a solution (default = 2.0).
If mxstrd step reductions have failed to lead to convergence then a final attempt is made to achieve a solution by increasing the original increment using stpfnl. This procedure has the potential to „step over‟ a difficult point in an analysis (e.g. a bifurcation point) so that the solution can continue.
Iterations
ITERATIONS specifies how the iteration strategy is to proceed.
ITERATIONS nit [nalps toline ampmx etmxa etmna isilcp] itype
nit
The maximum number of iterations for each load increment (default = 12).
nalps
The maximum number of line searches to be carried out on each iteration
(default = 2)
toline
The line search tolerance factor (default = 0.75).
ampmx
The maximum amplification factor in a line search (default = 5.0).
etmxa
The maximum step length in a line search (default = 25.0).
etmna
The minimum step length in a line search (default = 0.0).
isilcp
Separate iterative loop for contact procedure
No separate iterative loop for contact = 0 (default)
Separate iterative loop for contact = 1
Line searches are carried out if the absolute value of epsln on the nonlinear iterative log exceeds the value toline. The aim is to make epsln reasonably small on each iteration to speed convergence and prevent divergence.
itype
The type of iteration to be carried out for each iteration (default = NR)
Each iteration is specified on a separate line. There must be nit + 1 iteration types specified to include iteration zero. The type may be NR for NewtonRaphson or MNR for modified NewtonRaphson iterations. (If not included, the default is NR for all iterations). Note that FIRST, INC, INC can be used to generate this input.
For example, to apply „standard modified NR‟ with the calculation of the stiffness matrix at the beginning of each increment the first iteration must be specified as NR.
Notes
If arclength is to be used, it is advisable to ensure that the stiffness is calculated at least at the beginning of the increment.
272
Nonlinear Control
To specify the separate contact iterative loop procedure the variable isilcp on the ITERATIONS data chapter should be set to one. This will invoke the procedure for relevant material models. Since the procedure is designed to deal with contact and nonlinear material interaction it only applies to those elements that can be used with slidelines. Other elements not attached to the slideline are dealt with in the normal manner.
Bracketing
BRACKETING can be used to locate a limit or bifurcation point during a geometrically nonlinear analysis (omit this command if bracketing is not required).
When using the BRACKETING command, NONLINEAR CONTROL should be followed by EIGENVALUE CONTROL STIFFNESS. After the critical point in the nonlinear analysis has been found, the eigenvalue analysis is invoked. The scalar product of the lowest eigenmode extracted from the current tangent stiffness matrix and the applied load vector will indicate whether a limit or bifurcation point has been found. It is only possible to bracket the first critical point encountered in an analysis.
BRACKETING [ibrac irevsb brtol]
ibrac
Method used to locate limit/bifurcation point:
1 bisection (default)
2 interpolation
3 Riks semidirect approach
irevsb
Reversible (elastic) or irreversible (plastic or path dependent) analysis:
0 reversible (default)
1 irreversible
brtol
Bracketing tolerance (default = 0.01).
Depending on the type of arclength solution selected, the bracketing tolerance can depend upon:
the ratio of the current and initial minimum pivots and the ratio of the total and incremental load factors, or
the ratio of the arclength prior to bracketing and the subsequent increment in arclength
The value specified for brtol should be small enough to accurately locate the critical point; too tight a tolerance will eventually lead to ill conditioning of the tangent stiffness. Trial solutions using various values for brtol will inevitably be required to obtain a solution of sufficient accuracy.
Branching
BRANCHING can be used to „branch switch‟ onto a secondary path after a bifurcation point has been located using the BRACKETING command (omit this command if branching is not required). This procedure forces the analysis to leave the stable equilibrium path and follow an unstable secondary path. Two options exist for guiding the solution on to the secondary path:
273
Chapter 3 LUSAS Data Input
Eigenvalue injection
Artificial force with Rheinboldt‟s arclength
This facility should only be used by restarting a successfully completed bracketing analysis using the RESTART data chapter.
BRANCHING [ibrnch dellst]
ibrnch
Method used to branch on to secondary path:
1 eigenmode injection; used with isurfc=1 (default)
2 artificial force and Rheinboldt‟s arclength; used with (isurfc=2)
dellst
Starting arclength scaling factor (default=0.01)
If the BRANCHING command is specified the appropriate value of isurfc, the type of solution algorithm to be adopted, will be set automatically to suit the branching method selected.
Note. Values assigned for isurfc and dellst under the BRANCHING command will override those specified using INCREMENTATION. Any previous value specified for dellst will also be overwritten with the default value if the dellst data location in BRANCHING is left blank.
Convergence
The CONVERGENCE data section specifies at which stage the iterative corrections can be assumed to have restored the structure to equilibrium. It is compulsory on the first occurrence of NONLINEAR CONTROL. The solution has converged if the values of all the following criteria computed after an iteration are less than those specified. If a parameter is input as zero, the corresponding criteria is ignored.
CONVERGENCE rmaxal [rnoral dlnorm rlnorm wlnorm dtnrml]
rmaxal
The limit for the maximum absolute value of any residual (mar) (default = a large number).
rnoral
The limit for the square root of the mean value of the squares of all residuals (rms) (default = a large number).
dlnorm
The limit for the sum of the squares of the iterative displacements as a percentage of the sum of the squares of the total displacements (dpnrm).
Only translational degrees of freedom are considered by default but all degrees of freedom can be included by specifying Option 187. (default =
1.0)
rlnorm
The limit for the sum of the squares of all residual forces as a percentage of the sum of the squares of all external forces, including reactions
(rdnrm). Only translational degrees of freedom are considered but all degrees of freedom can be included by specifying Option 187. (default =
0.1)
274
Nonlinear Control
wlnorm
The limit for the work done by the residuals acting through the iterative displacements as a percentage of the work done by the loads on iteration zero of the increment (wdnrm) (default = a large number).
dtnrml
The limit for the sum of the squares of the iterative displacements as a percentage of the sum of the squares of the incremental displacements
(dtnrm). Only translational degrees of freedom are considered by default but all degrees of freedom can be included by specifying Option 187.
(default = 1.0)
Output
The OUTPUT data section specifies how often output is required. Insert zero to ignore a particular output option. On the last increment a PLOT FILE will automatically be written, overriding any specification in the OUTPUT command. This is also the case for output to the LUSAS output file and the LUSAS log file.
OUTPUT nitout [incout incplt incrst nrstsv inclog inchis]
nitout
The iteration interval for output of results (default =0).
incout
The increment interval for output of results (default = 1).
incplt
The increment interval for writing of plotting data to the plot file (default =
1). PLOT FILE does not need to be specified.
incrst
The increment interval for writing of problem data to the restart file
(default = 0). RESTART WRITE does not need to be specified.
nrstsv
The maximum number of restart dumps to be saved (default = 0). (to save the latest 2 dumps throughout the problem, set nrstsv = 2).
inclog
The increment interval for writing the iterative log (default=1).
inchis
The increment interval for writing the selective results history file.
(default=1 and will only be invoked if selective results output is specified).
In problems where the restart facility is used, a separate history file is created for each analysis.
Incremental Couple Read
The INCREMENTAL COUPLE READ data section controls the frequency of reading from the coupled datafile for thermomechanically coupled analyses (omit command if not performing a coupled analysis). See ThermoMechanically Coupled Analyses for more details.
INCREMENTAL COUPLE READ [nffrd dtfrd niterr]
nfrrd
The number of steps between data reads (default = 1)
dtfrd
The increment of time between data reads (default = 0)
niterr
The number of iterations between data reads (default = 0)
275
Chapter 3 LUSAS Data Input
Incremental Couple Write
The INCREMENTAL COUPLE WRITE data section controls the frequency of writing to the coupled datafile for thermomechanically coupled analyses (omit command if not performing a coupled analysis). See ThermoMechanically Coupled Analyses for more details.
INCREMENTAL COUPLE WRITE [nfrwt dtfwrt ndsave niterw]
nfrwt
The number of steps between writes (default = 1)
dtfwrt
The time increment between writes (default = 0)
ndsave
The number of datasets retained on disk. It is recommended that at least two datasets are saved. (default = all)
niterw
The number of iterations between writes (default = 0)
Termination
The TERMINATION data section specifies when an automatic incrementation solution is to terminate. It is compulsory if INCREMENTATION has been specified. If more than one termination criterion has been specified, termination will occur following the first criterion to be satisfied. Insert zero to ignore a particular option.
TERMINATION tlamdx [maxinc maxnod mxvar rmxdsp]
tlamdx
The maximum total load factor to be applied (default = 0)
maxinc
The maximum number of further increments to be applied from the time of specification of this NONLINEAR CONTROL (default = 1).
mxnod
The node number of displacement to be limited (default = 0).
mxvar
The variable number of displacement to be limited at node mxnod (default
= 0).
rmxdsp
The maximum displacement of node mxnod variable mxvar (default =
0).
When automatic incrementation has been specified the analysis will terminate exactly at the specified value of tlamdx for analyses that are controlled by non arclength automatic incrementation (i.e. isurfc = 0).
Notes
1. The INCREMENTATION and TERMINATION data sections are only used in conjunction with automatic load incrementation.
2. The INCREMENTAL COUPLE READ and INCREMENTAL COUPLE WRITE data sections are only used in thermomechanically coupled analyses.
3. Automatic load step reduction will not take place in coupled analyses.
4. Throughout NONLINEAR CONTROL, where stated, you may input a D for a particular input variable to obtain the default value.
5. When performing a nonlinear transient, dynamic or creep analysis, the
NONLINEAR CONTROL chapter must be used to specify ITERATION and
276
Nonlinear Control
CONVERGENCE only. Parameters controlling the number of problem steps, incrementation of loading etc. must be set using the commands in the
TRANSIENT, DYNAMIC or VISCOUS CONTROL chapters.
6. When carrying out a nonlinear analysis the plot and restart dumps should be requested by specifying the appropriate parameters in the OUTPUT data section.
However, a PLOT or a RESTART command may appear after this data chapter.
7. The nonlinear solution may be continued after the solution has failed to converge at a particular increment by setting Option 16.
8. TERMINATION must be used in conjunction with load curves to set the desired number of load increments.
9. When using an arclength procedure, Option 164 forces the arclength solution to be guided by the current stiffness parameter, cstifs, instead of using the minimum pivot, pivmn. If a bifurcation point is encountered, the arclength procedure could cause the solution to oscillate about this point with no further progress being made. Option 164 allows the solution to continue on the fundamental path and overcomes any such oscillations if a bifurcation point is encountered. Note that Option 164 is not valid when using the BRACKETING command.
10. BRANCHING and BRACKETING must not be specified if they are not required in an analysis.
11. STEP_REDUCTION is only applicable if values have been specified under the
INCREMENTATION data section.
12. Specifying Option 62 forces the solution to continue if more than two pivots are encountered during an analysis.
13. Option 131 is switched off by default for a nonlinear analysis, but this may be set to on in the data file if required. If Option 131 is set to on a warning message is issued and the analysis will continue with the option switched on.
14. The following nonlinear parameters are output:
MAR
RMS
The maximum absolute residual
The root mean square of the residuals
DPNRM
The displacement norm as a percentage of the total displacements
RDNRM
The residual force norm as a percentage of the total reactions
WDNRM
The work done by the residual forces as a percentage of the work done by the loads on iteration zero
DTNRM
The displacement norm as a percentage of the total displacements for the increment
EPSLN
The line search tolerance parameter
ETA
The final line search step length
DELTL
The incremental displacement length (arclength)
DELTW
The work done by the external loads during the current increment
DLMDA
The change in load factor on the current iteration
277
Chapter 3 LUSAS Data Input
TLMDA
The total load factor
LTDSP
The value of the displacement at the node and variable number specified in the TERMINATION criteria
MXSTP
The maximum number of plasticity steps used (if MXSTP 1 plasticity has occurred in that iteration)
NLSCH
The number of line searches carried out on the current iteration
CSTIF
The current stiffness parameter
PENMX
The maximum penetration on slidelines
NDPMX
The slideline node at which maximum penetration occurs
KDSMX
The node: variable number at which the maximum incremental displacement occurs
ISURF
The load/arclength control parameter
ENGY
Total strain energy
PLWRK
Total plastic work
PIVMN
The minimum pivot value from the tangent stiffness
PIVMX
The maximum pivot value from the tangent stiffness
NSCH
The number of negative pivots found during the solution
KPVMN
The node: variable number at which the minimum pivot occurs
KPVMX
The node: variable number at which the maximum pivot occurs
Slideline
The augmented Lagrangian method with slidelines employs both penalty parameters
(contact stiffnesses) and Lagrangian multipliers to reduce contact penetrations. At convergence, the method checks the penetrations against a tolerance. If any are outside the tolerance the Lagrangian multipliers, and if the penalty update procedure is specified, the contact stiffnesses are updated at the relevant nodes and the solution is rerun.
The progress of the solution is controlled by the SLIDELINE data section, which places a limit on the number of Lagrangian multiplier and penalty parameter updates.
SLIDELINE NAGLMX NPUPMX
Naglmx
Maximum number of augmented Lagrangian updates per increment
(default = 2).
Npupmx
Maximum number of penalty parameter (contact stiffness) updates per increment (default = 1).
Application of Loads with Nonlinear Control
The stress state is always 'remembered' on iteration zero after a change of control. In a nonlinear analysis the stresses will be updated based on the external loads until convergence is achieved. If the load is reduced to zero in a subsequent loadcase, then the resulting stresses may also reduce to zero while any plastic strains will remain.
278
Nonlinear Control
The type of loading is important when determining whether a load level from one increment is "remembered" or " forgotten" in subsequent increments when using manual or automatic load incrementation (see also General Loading Rules). Some loading types are total in nature whilst other are incremental. All of the loading types in
LUSAS are total with the exception of the Incremental Prescribed Displacement loading type (PDSP)
Total
These apply only the specified loading magnitude to the structure. This means that any previously specified loading at a node or element is overwritten by the current specification of load.
Consider an automatic, fixed load increment in which a concentrated load magnitude of 5.0 is to be incremented from a reference load factor of 0.2 over
3 increments. The initial load applied will be calculated according to 0.2*5.0.
The subsequent two load increments will be calculated as 0.4*5.0 and 0.6*5.0
Incremental
The specified loading magnitude is applied in addition to the load already applied to the structure.
Consider the example above but with incremental prescribed displacement loading. The initial load applied will be calculated according to 0.2*5.0. The subsequent two load increments will be calculated incrementally as (previous load + next increment of load), i.e.
2nd Increment: 0.2*5.0 + (0.4  0.2)*5.0
3rd Increment: 0.4*5.0 + (0.6  0.4)*5.0
The following examples illustrate different orders in the command formats for
NONLINEAR CONTROL. These examples are not affected by the presence of:
Material nonlinearity
Geometric nonlinearity
Arclength procedures
Line search procedures
Dynamic analyses
Static analyses
Note. Automatic nonlinear control is not applicable for use with a transient dynamic analysis.
Application Of Force Loading
Force loading is any loading EXCEPT incremental or total prescribed displacement loading.
279
Chapter 3 LUSAS Data Input
Example. Automatic Incrementation Followed by Automatic
CL
1 0 0 10.0
NONLINEAR CONTROL
INCREMENTATION 0.5
TERMINATION 0 3
Giving a load at the end of this control of 15.
CL
1 0 0 20.0
NONLINEAR CONTROL
INCREMENTATION 1.0
TERMINATION 0 3
Giving a load at the end of this control of 60.
The load is applied in steps 5, 10, 15, 20, 40, 60. In this sense it could be said that the previous load is 'forgotten'.
Example. Manual Incrementation Followed by Manual
CL
1 0 0 10.0
NONLINEAR CONTROL
ITERATION 12
CONVERGENCE 0 0 D D
Giving a load at the end of this control of 10.
CL
1 0 0 20.0
NONLINEAR CONTROL
ITERATION 12
CONVERGENCE 0 0 D D
Giving a load at the end of this control of 20.
280
Nonlinear Control
Example. Automatic Incrementation Followed by Manual
CL
1 0 0 10.0
NONLINEAR CONTROL
INCREMENTATION 0.5
TERMINATION 0 3
Giving a load at the end of this control of 15
CL
1 0 0 10.0
NONLINEAR CONTROL
ITERATION 12
CONVERGENCE 0 0 D D
Giving a load at the end of this control of 10.
Example. Manual Incrementation Followed by Automatic
This is the only case where a load is remembered. The application of a manual increment will remain throughout the analysis until any further manual increment.
Additional load is applied from the current automatic incrementation.
CL
1 0 0 10.0
NONLINEAR CONTROL
ITERATION 12
CONVERGENCE 0 0 D D
Giving a load at the end of this control of 10.
CL
1 0 0 2.0
NONLINEAR CONTROL
INCREMENTATION 1.0
TERMINATION 0 3
Giving a load at the end of this control of 16 (10 + 6).
281
Chapter 3 LUSAS Data Input
Dead Load and Live Load
A typical nonlinear analysis would require the application of a dead load, typically selfweight, as a constant load for the analysis, together with the live load which is gradually applied over a number of increments. The following examples show this can be achieved.
Example 1. Dead Load and Incremented Live Load
Using the characteristics of an automatic nonlinear loading following a manual load application:
CL
1 0 0 10.0
NONLINEAR CONTROL
ITERATION 12
CONVERGENCE 0 0 D D
Which, at the end of this control, applies a dead load of 10.
CL
1 0 0 2.0
NONLINEAR CONTROL
INCREMENTATION 1.0
TERMINATION 0 3
Which, at the end of the second control, applies a dead load of 10 and a live load of 6 giving a total load of 16.
Manual Load Application
CL
1 0 0 10.0
NONLINEAR CONTROL
ITERATION 12
CONVERGENCE 0 0 D D
Which, at the end of this control, applies a dead load of 10.
CL
1 0 0 10.0
1 0 0 2.0
282
Nonlinear Control
CL
1 0 0 10.0
1 0 0 4.0
CL
1 0 0 10.0
1 0 0 6.0
Which, at the end of the second control, applies a dead load of 10 and a live load of 6 giving a total of 16.
Using Load Curves
The load curve facility allows two load variations to be applied. One constant and one variable as required.
CL
1 0 0 10.0
CL
1 0 0 2.0
CURVE DEFINITION 1 COSINE
1.0 0.0
CURVE DEFINITION 2 USER
1 0.0
4 3.0
CURVE ASSIGNMENT
1 1.0 1
2 1.0 2
NONLINEAR CONTROL
TERMINATION 0 4
Which applies a constant load level of 10 and a varying live load of 6 giving a total load of 16.
Follower Forces
In general, follower forces are available in LUSAS when the loading type is either
UDL (Uniformly Distributed Load) or FLD (Face Load) and Eulerian geometric nonlinearity option (Option 167) is selected. For certain elements additional follower loading is also available using Option 36 (see the LUSAS Element Reference Manual).
283
Chapter 3 LUSAS Data Input
Explicit dynamics elements will also give follower forces when using the FLD load facility.
General Loading Rules
1. In switching from manual to automatic control, any loading input under the manual control is remembered and held constant while the automatic procedure is operating
2. In switching from automatic back to manual control, any loading accumulated under automatic control is forgotten and only the manual load is applied. To include the final load level from the automatic load increments, the load datasets from which it comprises must be assigned to this manual load case
3. In switching from manual to manual control, any loading accumulated under previous manual controls is forgotten and only the current manual load is applied.
4. In switching from automatic to automatic control, any loading accumulated under the previous automatic control is forgotten and only the current automatic load is applied. To include the final load level from the previous automatic load increment, an additional loadcase must be inserted prior to the next automatic increment and the load datasets from the previous automatic increment assigned to this manual load case.
5. If incremental prescribed displacements are being used then, in any switching from one type of control to another, the effect of prescribed displacements will be remembered and will not need to be input again. This is not the case for total prescribed displacements which are total loads
6. The stress and strain state will always be remembered whatever loading is applied on iteration zero after the change of control. In a nonlinear analysis the stresses/strains will be updated based on the external loads until convergence is achieved. If the load is reduced to zero in a subsequent loadcase, then the resulting stresses may also reduce to zero while any plastic strains will remain. Additionally, if the same load magnitude is maintained across a change of control, convergence will be achieved in one iteration because the stress state and the equilibrium internal forces do not change.
Dynamic Control
The DYNAMIC CONTROL data chapter is used to control the solution procedure for transient dynamic analyses. For further information regarding the solution of transient dynamics problems refer to Dynamic Analysis, and the LUSAS Theory Manual.
DYNAMIC CONTROL
Incrementation
The INCREMENTATION data section controls the applied time step interval.
INCREMENTATION dt [tsfac dtincf inctyp dtmin dtmax]
284
Dynamic Control
dt
The initial time step.
tsfac
The scale factor for computing the time step for explicit dynamic analyses
(default = 0.9 for 3D and 2/3 for 2D)
dtincf
The time step increment restriction factor for dynamic analyses (default =
1.0 for explicit analysis, default = 10.0 for implicit analysis). Note that stability conditions must be taken into account when setting dtincf. The default value may lead to instability in some cases.
inctyp
Set to 1 for a driven coupled analysis. This means that the time step for this analysis is calculated by the thermal analysis. Note that a driven coupled analysis is not permitted when coupling iteratively. (default = 0).
dtmin
Minimum time step for explicit dynamic analyses (default = 0.0). Note that stability conditions must be taken into account when setting dtmin since solution instability may occur.
dtmax
Maximum time step for explicit dynamic analyses (default = no limit)
Constants
The CONSTANTS data section specifies the time integration factors to be used. If not specified, the default or previous user defined data are assumed. If explicit dynamic elements have been specified then the default constants will be those for an explicit dynamic analysis and this command may be omitted.
Implicit dynamics (HilberHughes integration scheme)
CONSTANTS alpha [beta gamma]
alpha
Integration factor (default = 0).
beta
Integration factor (default = 1/4).
gamma
Integration factor (default = 1/2).
Note. For an unconditionally stable, second order accurate scheme, alpha must lie between the limits:
3 a 0 and beta and gamma are defined as:
1
4
2
,
2
If beta and gamma are not specified they will be computed automatically using the above equations. Setting alpha to zero reduces the algorithm to the Newmark method
(this is the default).
285
Chapter 3 LUSAS Data Input
Explicit dynamics
alpha
Integration factor = 0
beta
Integration factor = 0
gamma
Integration factor = ½
Note. For an explicit dynamic analysis the above integration factors are mandatory and the CONSTANTS data section may be omitted in this case. Only explicit dynamics elements may be used with the explicit dynamics constants.
Incremental Couple Read
The INCREMENTAL COUPLE READ data section controls the frequency of reading from a coupled datafile for a coupled analysis (omit if not performing a coupled analysis). See Coupled Analysis for more information.
INCREMENTAL COUPLE READ [nffrd dtfrd niterr]
nfrrd
The number of steps between data reads (default = 1)
dtfrd
The increment of time between data reads (default = 0)
niterr
The number of iterations between data reads (default = 0)
Incremental Couple Write
The INCREMENTAL COUPLE WRITE data section controls the frequency of writing a coupled datafile for a coupled analysis (omit if not performing a coupled analysis).
See Coupled Analysis for more information.
INCREMENTAL COUPLE WRITE [nfrwt dtfwrt ndsave niterw]
nfrwt
The number of steps between writes (default = 1)
dtfwrt
The time increment between writes (default = 0)
ndsave
The number of datasets retained on disk (default = all)
niterw
The number of iterations between writes (default = 0)
Output
The OUTPUT data section specifies how often output is required. If not specified, the default or previously defined user data are assumed. On the last increment a PLOT
FILE will automatically be written, overriding any specification in the OUTPUT command. This is also the case for output to the LUSAS output file and the LUSAS log file.
OUTPUT incout [incplt incrst nrstsv inclog inchis]
incout
Increment interval for output of results (default = 1)
incplt
Increment interval for writing of plotting data to the plot file (default = 1).
PLOT FILE does not need to be specified.
incrst
The increment interval for writing of problem data to the restart file
(default = 0). RESTART WRITE does not need to be specified.
286
Dynamic Control
nrstsv
The maximum number of restart dumps to be saved (default =0). (to save the latest 2 dumps throughout the problem, set nrstsv = 2)
inclog
The increment interval for writing the time step log (default=1).
inchis
The increment interval for writing the selective results history file.
(default=1 and will only be invoked if selective results output is specified).
In problems where the restart facility is used, a separate history file is created for each analysis.
Termination
The TERMINATION data section specifies when the analysis terminates. If not specified, the default or previously defined user data are assumed.
TERMINATION maxinc [ttime dtterm]
maxinc
The maximum number of time steps to be applied (default = 1).
ttime
The total response time at which the analysis should terminate (default = a large number).
dtterm
The minimum time step below which the analysis should terminate
(default = 0.0)
Notes
1. To start a dynamic analysis, a knowledge of the initial conditions is required. For example, initial displacements may be computed from a static preanalysis and initial velocities calculated. These velocities can then be specified by the user in the dynamic analysis using the VELOCITY data chapter.
2. For an analysis using explicit dynamic elements only dt is taken as the smaller of the user input and the calculated values (dt may be entered, in this instance, as zero). Further steps are automatically adjusted according to mesh deformation.
3.
dtterm will terminate an analysis if the step size is reduced below this value.
4. If inctyp is set to 1 for a driven coupled analysis, dt is reinterpreted as the maximum step size permitted, and the new step size is calculated to be as close to, but not exceeding dt, as possible. The variable step size is always selected to ensure that the next data transfer takes place at the next dataset.
5. If both maxinc and ttime are specified, termination occurs with the minimum response time.
6. If the problem is nonlinear, the convergence and the iteration details must be set by the NONLINEAR CONTROL commands.
7. Automatic time stepping is mandatory for explicit dynamic analyses.
8. The INCREMENTAL COUPLE READ and INCREMENTAL COUPLE WRITE data sections should be omitted if a thermomechanically coupled analysis is not being performed.
9. Automatic load step reduction will not take place in a coupled analysis.
287
Chapter 3 LUSAS Data Input
10. When carrying out a DYNAMIC analysis the plot and restart dumps should be requested by specifying the appropriate parameters in the OUTPUT data section.
However, a PLOT or a RESTART command may appear after this data chapter.
11. For large explicit dynamic analyses the output files may be enormous if default values are chosen for output.
12. Throughout DYNAMIC CONTROL, where stated, you can input a D for a particular input variable to obtain the default value.
13. If no output or plot dump is requested, the stress computation is automatically bypassed during a linear dynamic analysis.
Example. Static Starting Conditions for Dynamic Analyses
In the following examples, nonessential data has been omitted.
Linear for the simple case of a constant dead load (simulated using constant body
force loading), followed by a constant live load (using the concentrated loading type):
SUPPORT NODE
LOAD CASE
CL
ELEMENT OUTPUT
1 0 0 0
LOAD CASE
CL
DYNAMIC CONTROL
END
For the more complex case of a constant dead load followed by a varying live load:
SUPPORT NODES
LOAD CASE
CBF
ELEMENT OUTPUT
1 0 0 0
LOAD CASE
CBF
LOAD CASE
288
Dynamic Control
CL
CURVE DEFINITION 1 USER
CURVE DEFINITION 2 USER
CURVE ASSIGNMENT
1 1 1
2 1 2
DYNAMIC CONTROL HILBER
END
Nonlinear Similarly, a constant dead load (simulated using constant body force
loading), followed by a constant live load (using the concentrated loading type):
SUPPORT NODE
LOAD CASE
CL
ELEMENT OUTPUT
1 0 0 0
NONLINEAR CONTROL
LOAD CASE
CL
DYNAMIC CONTROL
END
For a varying live load using load curves
SUPPORT NODES
LOAD CASE
CBF
LOAD CASE
PDSP 2
CURVE DEFINITION 1 COSINE
CURVE DEFINITION 2 COSINE
CURVE ASSIGNMENT
1 1 1
289
Chapter 3 LUSAS Data Input
ELEMENT OUTPUT
1 0 0 0
NONLINEAR CONTROL
CURVE ASSIGNMENT
1 1 1
2 1 2
DYNAMIC CONTROL HILBER
END
Dynamic Integration Schemes
alpha Integration Scheme
Central Difference
HilberHughesTaylor

0
0
¼ beta
½ gamma
½
The table shows the integration schemes available and the default integration parameters for each. The parameter values listed are set by default where the Central
Difference scheme applies for explicit dynamic elements. The parameters are defined under the CONSTANTS data section of DYNAMIC CONTROL.
The constant alpha is used to control the amount of numerical damping within the
HilberHughesTaylor solution scheme; it is not used in the explicit Central Difference scheme.
Selecting the Time Step
The time step for dynamic analysis is specified using the INCREMENTATION section of the DYNAMIC CONTROL data chapter. The selection of the time step is governed by stability and accuracy. When using explicit algorithms, stability requires that the time step is less than or equal to a critical value where: t cr
1
T max
2
max where w max
and T max
are the circular frequency and period of the highest mode of vibration in the uncoupled system.
Transient Control
The TRANSIENT CONTROL data chapter is used to control the solution procedure for transient field analyses. For further information regarding the solution of transient
290
Transient Control
field problems refer to Transient and Dynamic Analyses, and the LUSAS Theory
Manual.
TRANSIENT CONTROL
Incrementation
The INCREMENTATION data section controls the time step value for a transient field analysis.
INCREMENTATION dt [inctyp] dtincf dtmin dtmax
dt
Initial time step value.
inctyp
Set to 1 for a driven coupled analysis. This means that the time step for this analysis is calculated by the structural analysis. Note that a driven coupled analysis is not permitted when coupling iteratively (default = 0).
dtincf
The time step increment factor (default=1 for constant time step)
dtmin
The minimum permissible time step size (default=dt)
dtmax
The maximum permissible time step size (default=dt)
Constants
The CONSTANTS data section is used to specify the time integration factor. If not specified, the default or previously defined user data are assumed. See Thermo
Mechanically Coupled Analyses for more details.
CONSTANTS beta
beta
The time integration factor
=1/2 for the CrankNicholson scheme
=1 for the backward difference scheme.
(default = 2/3 for linear analysis).
(default = 1 for nonlinear analysis, this value may not be overwritten).
Incremental Couple Read
The INCREMENTAL COUPLE READ data section is used to control reading from the coupled datafile for thermomechanically coupled analyses (omit command if not performing a coupled analysis). See ThermoMechanically Coupled Analyses for more details.
INCREMENTAL COUPLE READ [nffrd dtfrd niterr]
nffrd
The number of steps between data reads (default = 1)
dtfrd
The increment of time between data reads (default = 0)
niterr
The number of iterations between data reads (default = 0)
291
Chapter 3 LUSAS Data Input
Incremental Couple Write
The INCREMENTAL COUPLE WRITE data section is used to control writing to the coupled datafile for thermomechanically coupled analyses (omit command if not performing a coupled analysis). See ThermoMechanically Coupled Analyses for more details.
INCREMENTAL COUPLE WRITE [nfrwt dtfwrt ndsave niterw]
nfrwt
The number of steps between writes (default = 1)
dtfwrt
The time increment between writes (default = 0)
ndsave
The number of datasets retained on disk (default = all)
niterw
The number of iterations between writes (default = 0)
Output
The output frequency control. If not specified, the default or previously defined user data are assumed. On the last increment a PLOT FILE will automatically be written, overriding any specification in the OUTPUT command. This is also the case for output to the output file and the log file.
OUTPUT incout [incplt incrst nrstsv inclog inchis]
incout
The increment interval for output of results (default = 1)
incplt
The increment interval for writing of plotting data to the plot file (default =
1). PLOT FILE does not need to be specified.
incrst
The increment interval for writing of problem data to the restart file
(default = 0). RESTART WRITE does not need to be specified.
nrstsv
The maximum number of restart dumps to be saved (default =0). (to save the latest 2 dumps throughout the problem, set nrstsv= 2)
inclog
The increment interval for writing the time step log (default=1).
inchis
The increment interval for writing the selective results history file.
(default=1 and will only be invoked if selective results output is specified).
In problems where the restart facility is used, a separate history file is created for each analysis.
Termination
The TERMINATION data section is used to specify when the analysis terminates. If not specified, the default or previously defined user data are assumed.
TERMINATION maxinc [ttime]
maxinc
The maximum number of time steps to be applied (default = 1).
ttime
The total response time at which the analysis should terminate (default = a large number).
292
Viscous Control
Notes
1. Transient analysis is applicable to field problems only.
2. The INCREMENTAL COUPLE READ and INCREMENTAL COUPLE WRITE data sections should be omitted if the problem is not a thermomechanical coupled analysis.
3. Automatic load step reduction will not take place in a coupled analysis.
4. The support conditions and loading data specified prior to the first TRANSIENT
CONTROL chapter provide the static steady state solution at time equals zero.
5. For a coupled analysis only, if inctyp is set to a nonzero value for a driven coupled analysis, dt is reinterpreted as the maximum step wise permitted, and the new step wise is calculated to be as close to, but not exceeding dt. The variable step wise is always selected to ensure that the next data transfer takes place exactly at the next dataset.
6. If both maxinc and ttime are specified, termination occurs with the minimum response time.
7. If the problem is nonlinear, the convergence and the iteration details must be set by the NONLINEAR CONTROL commands.
8. When carrying out a TRANSIENT analysis the plot and restart dumps should be requested by specifying the appropriate parameters in the OUTPUT data section.
However, a PLOT or a RESTART command may appear after this data chapter.
9. Throughout TRANSIENT CONTROL, where stated, you can input a D for a particular input variable to obtain the default value.
10. Oscillatory response may be seen when using the default beta constant with step type loading. Increasing beta will reduce these oscillations (as would a more gradual ramping of the load).
Viscous Control
The VISCOUS CONTROL data chapter is used to control the solution procedure for creep analyses. For further information regarding the solution of problems involving rate dependent material nonlinearity refer to the LUSAS Theory Manual.
VISCOUS CONTROL
Incrementation
The INCREMENTATION data section controls the applied time step interval.
INCREMENTATION [dt dtincf inctyp dtmin dtmax exptim]
dt
Time step (default = 0.001)
dtincf
Time step increment restriction factor (default = 10.0).
inctyp
Set to 1 for a driven coupled analysis. This means that the time step for this analysis is calculated by the thermal analysis. Note that a driven coupled analysis is not permitted when coupling iteratively (default = 0).
dtmin
Minimum time step (default = 0.0)
dtmax
Maximum time step (default = no limit)
293
Chapter 3 LUSAS Data Input
exptim Exponent used to increase time step when using the CEBFIP creep model
(see Notes)
Automatic Viscous Control
The AUTOMATIC VISCOUS_CONTROL data section specifies the automatic timestepping criterion to be applied and the factors to be used for each criterion.
AUTOMATIC VISCOUS_CONTROL [OFF] ictol toler control factor
ictol
Toler
Control
factor
Notes
Control criterion (see below).
Tolerance factor for controlling the automatic time step (see below).
The way in which this factor is used is dependent upon the chosen control criterion.
May have one of two meanings depending on the criterion used (see
Notes below):
Permitted difference between the time step evaluated at the beginning of a step and that calculated once values at t+dt are established. If the error tolerance is exceeded the time step is halved.
Switch for explicit time step calculation.
Definition of automatic time stepping criteria:
1.
ictol = 1
toler
control
factor
= dcrpmx = incremental creep strain
= Permitted difference between the time step evaluated at the beginning of a step and that calculated once values at t+dt are established.
Limit of change of creep strain rate dec/dt calculated at time t and t+dt: d t
dcrpmx c
c t
2. If the gradient is almost constant, then a large dt will be predicted; conversely, if the difference in gradients is large a small time step will be predicted.
ictol = 2
toler = restriction factor
control
factor
= 0 (deactivate explicit step calculation)
1 (activate explicit step calculation)
The explicit time step is calculated using the creep strain rate dec/dt:
294
Viscous Control
dt
3 E
)
x restriction factor d
c dq where E is the Elastic modulus and n is Poisson‟s ratio of the material and q is the equivalent stress.
3.
ictol = 3
toler = scale factor a
control
factor
= Permitted difference between the time step evaluated at the beginning of a step and that calculated once values at t+dt are established.
dt is calculated as a function of the total strain
and the creep strain rate
dec/dt: dt
NM
L
c
QP
O 1
2
4.
ictol = 4
toler = scale factor a
control
factor
= Permitted difference between the time step evaluated at the beginning of a step and that calculated once values at t+dt are established.
5.
dt is calculated as a function of the critical total elastic strain components
i
e and the critical creep strain rate de
i
c/dt component: dt
min
i e i c
i=1, number of strain components
Typical values of a are as following:
0.01< a<0.15 a<10 explicit analysis implicit analysis
Default values are:
ictol
1
2
3
4
toler
0.001
1.000
0.000
0.000
control factor
0.1
1.0 (initialised for first step of implicit analysis then deactivated)
0.0
0.0
295
Chapter 3 LUSAS Data Input
Rate Dependent
The RATE_DEPENDENT data section specifies whether implicit or explicit integration is to be used. If this section is omitted the default of implicit integration is invoked.
RATE_DEPENDENT {IMPLICIT  EXPLICIT}
State
The STATE data section can be used with the RESIN CURE MODEL, which is used for predicting the deformations of thermoset composites that occur during a hot cure manufacturing process. The use of the STATE data section simplifies the analysis so that only a structural analysis is required. This approach is restricted to thin parts in which the state of cure is constant, or nearly constant at every point. A globally defined state is then valid which can be evaluated from a basic knowledge of the cure cycle and cure kinetics. The cure is modelled by splitting it into sections in which a single material state is valid. As the material is linear within each state the shrinkage and thermal strains need only be considered at the end of the step.
STATE < iState i
> i=1,maxinc
iState
The state of the resin, (liquid = 1, rubbery = 2, glassy = 3).
maxinc
The maximum number of time steps to be applied.
This procedure requires a pseudo time step of 1, in other words, using
INCR 1
each iState is associated with a pseudo time multiple of 1 which is used to synchronise both the shrinkage and thermal data corresponding to the step, see Notes.
Incremental Couple Read
The INCREMENTAL COUPLE READ data section controls the frequency of reading from a coupled datafile for a coupled analysis (omit if not performing a coupled analysis).
INCREMENTAL COUPLE READ [nffrd dtfrd niterr]
nfrrd
The number of steps between data reads (default = 1)
dtfrd
The increment of time between data reads (default = 0)
niterr
The number of iterations between data reads (default = 0)
Incremental Couple Write
The INCREMENTAL COUPLE WRITE data section controls the frequency of writing a coupled datafile for a coupled analysis (omit if not performing a coupled analysis).
INCREMENTAL COUPLE WRITE [nfrwt dtfwrt ndsave niterw]
296
Viscous Control
nfrwt
The number of steps between writes (default = 1)
dtfwrt
The time increment between writes (default = 0)
ndsave
The number of datasets retained on disk (default = all)
niterw
The number of iterations between writes (default = 0)
Output
The OUTPUT data section specifies how often output is required. If not specified, the default or previously defined user data are assumed. On the last increment a PLOT
FILE will automatically be written, overriding any specification in the OUTPUT command. This is also the case for output to the LUSAS output file and the LUSAS log file.
OUTPUT [incout incplt incrst nrstsv inclog inchis]
incout
Increment interval for output of results (default = 1)
incplt
Increment interval for writing of plotting data to the plot file (default = 1).
PLOT FILE does not need to be specified.
incrst
The increment interval for writing of problem data to the restart file
(default = 0). RESTART WRITE does not need to be specified.
nrstsv
The maximum number of restart dumps to be saved (default = 0). For example, to save the latest 2 dumps throughout the problem, set nrstsv
= 2.
inclog
The increment interval for writing the time step log (default = 1).
inchis
The increment interval for writing the selective results history file.
(default=1 and will only be invoked if selective results output is specified).
In problems where the restart facility is used, a separate history file is created for each analysis.
Termination
The TERMINATION data section specifies when the analysis terminates. If not specified, the default or previously defined user data are assumed.
TERMINATION [maxinc ttime dtterm steady]
maxinc
The maximum number of time steps to be applied (default = 1).
ttime
The total response time at which the analysis should terminate (default = a large number).
dtterm
The minimum time step below which the analysis should terminate
(default = 0.0).
steady
Value to terminate analysis relating the current displacement increment to the displacement increment directly following a new control data section. incremental displacement on current step
steady incremental displacement norm on first step
297
Chapter 3 LUSAS Data Input
Notes
1. The starting time step for both explicit and implicit analyses is automatically calculated using the explicit step stability criterion. On subsequent steps, for implicit analyses, the step size is determined by the active automatic control criterion. The other active criteria are also evaluated on the first step and if any prove more critical than the explicit time step, then this value will be applied.
2. For many functions the creep rate is infinite at t=0 and therefore dt/2 is used to evaluate the creep strain rate and various derivatives required in the automatic step evaluation. The choice of dt determines the particular gradients and hence the calculation of the initial time step.
3. dtincf limits the growth of the time step. The default value allows the step to grow an order of magnitude with each time step, thus if the explicit time step is too conservative for the implicit analysis it does not take many time steps to adjust.
4. For an analysis using explicit dynamic elements, explicit integration must be specified.
5. If inctyp is set to a nonzero value for a driven coupled analysis, dt is reinterpreted as the maximum step wise permitted, and the new step wise is calculated to be as close to, but not exceeding dt, as possible. The variable step wise is always selected to ensure that the next data transfer takes place at the next dataset.
6. If both maxinc and ttime are specified, termination occurs with the minimum response time.
7. If the problem is nonlinear, the convergence and the iteration details must be set by the NONLINEAR CONTROL commands.
8. The INCREMENTAL COUPLE READ and INCREMENTAL COUPLE WRITE data sections should be omitted if a thermomechanically coupled analysis is not being performed.
9. Automatic load step reduction will not take place in a coupled analysis. When carrying out a VISCOUS analysis the plot and restart dumps should be requested by specifying the appropriate parameters in the OUTPUT data section. However, a
PLOT or a RESTART command may appear after this data chapter.
10. Throughout VISCOUS CONTROL, where stated, you can input a D for a particular input variable to obtain the default value.
11. DYNAMIC CONTROL may be utilised with VISCOUS CONTROL if required.
12. NONLINEAR CONTROL must be specified with VISCOUS CONTROL unless linear materials are used with an explicit creep integration scheme (i.e. ratedependent = explicit).
13. An example of using the STATE command to control resin shrinkage and thermal strains is given below.
SHRINKAGE PROPERTIES GENERAL TIME 3 ishr …
0
1
0.035
0.045
:
2
LOAD CASE 1
0.046
TEMP
298
Viscous Control
1
1.0
1 USER
First Last Inc
:
CURVE DEFINITION
0
1
0
0
:
2 160
VISCOUS CONTROL
STATE 2 3 3
The preceding data results in three load steps. On the first the composite is in its rubbery state (=2) and the shrinkage is 3.5%. Note that we are commencing the analysis when the resin is in its rubbery state at a temperature of 180
C; the load curve defines the cure temperature changes. On the second step the composite will have vitrified (glassy = 3) and a further 1% shrinkage will occur. Finally on step 3, the composite is cooled from 180
C to room temperature 20
C. A further 0.1% shrinkage occurs during cool down.
The STATE command can be entered more than once. On definition maxinc is set to the number of entered states. If maxinc is subsequently input under
TERMINATION it will overwrite the value set by the STATE command. If, whilst running, all the STATE variables are processed, LUSAS will stop, independently of the value of maxinc.
14. To use the parameter exptim the total response time, ttime, and the maximum number of time steps, maxinc, must be specified under TERMINATION. The initial time step is taken as 1 day and increases according to the value of the exponential, the number of time steps (maxinc) and the total response time. The parameter exptim is only applicable to analyses using the CEBFIP creep and shrinkage model.
299
Chapter 3 LUSAS Data Input
Figure 2.2 Time step number vs time step growth for an exponent of 3.0
Figure 2.3 Response time vs time step growth for an exponent of 3.0
300
Eigenvalue Control
Eigenvalue Control
The EIGENVALUE CONTROL data chapter is used to control the solution procedure for eigenvalue extraction and eigenvalue buckling analyses, using either the subspace iteration method, the inverse iteration method with shifts, or the Lanczos method
(standard or fast). For eigenvalue extraction using Guyanreduced eigenvalues, see
Guyan Control. The subspace iteration method is used to compute either the lowest or highest eigenmodes, while the inverse iteration method with shifts is used to compute the eigenmodes that exist within a specified eigenvalue or frequency range of interest.
The Lanczos method can compute the lowest or highest eigenvalues or a specified range. For further information regarding the solution of eigenvalue problems refer to
Eigenvalue Analysis, and the LUSAS Theory Manual.
EIGENVALUE CONTROL
either:
{CONSTANTS  SUBSPACE  LANCZOS  FAST}
or:
[INVERSE  LANCZOS  FAST] {EIGENVALUE  FREQUENCY}
RANGE
[CONVERGENCE]
Eigenvalue Control
EIGENVALUE CONTROL {BUCKLING  STIFFNESS  DAMPING}
BUCKLING The BUCKLING command word is used to specify that an eigenvalue buckling problem is to be solved. This facility can only be used in conjunction with element types that support geometrically nonlinear solutions (see the LUSAS Element Reference Manual).
STIFFNESS
The STIFFNESS command word is used to specify that an eigenvalue analysis of the stiffness matrix should be performed.
DAMPING
The DAMPING command word is used to specify that the damping matrix is to be included in the analysis leading to a complex eigensolution.
With no other command words on this line (e.g. buckling/stiffness) an eigenvalue analysis using both stiffness and mass matrices will be carried out (a natural frequency analysis).
Maximal/Minimal Eigenvalues
This data section is used to specify the options for the chosen eigenvalue solution method that will solve for the lowest or highest eigenmodes in the structure. If this data section is used, the EIGENVALUE/FREQUENCY RANGE data section must be omitted. With the exception of nroot, default values will be assumed for all parameters that are not specified. If the CONSTANTS keyword is specified, LUSAS will select the default eigenvalue solver, which is the fast Lanczos solver unless the
301
Chapter 3 LUSAS Data Input
analysis contains superelements, or is a branching and bracketing analysis, in which case the subspace iteration solver will be used.
{CONSTANTS  SUBSPACE} nroot [nivc shift norm sturm eigsol maxmin buckl]
or:
LANCZOS nroot [shift norm sturm maxmin buckl]
or:
FAST nroot [shift norm maxmin buckl]
or for DAMPING:
FAST nroot [shiftr shifti norm]
nroot
The number of eigenvalues required (must be less than or equal to the number of free nodal variables for the structure).
nivc
The number of starting iteration vectors to be used (default is taken as min
{(2*nroot), (nroot+8), (number of structure free variables)}. Only used for subspace iteration.
shift
The shift to be applied to the stiffness matrix (default = 0.0).
shiftr The real shift to be used in a complex (DAMPING) eigensolution (= 0.0  not available at present).
shifti
The imaginary shift to be used in a complex (DAMPING) eigensolution (=
norm
0.0  not available at present).
The normalisation procedure required for the eigenvectors (default=0).
=0 normalisation with respect to unity
=1 normalisation with respect to the global mass
=2 normalisation with respect to the global stiffness
sturm
Determines if a Sturm sequence check is to be applied (default=1).
Automatically performed for the fast solver.
=0 no Sturm sequence check
=1 Sturm sequence to be carried out
eigsol
Type of eigensolver required (default=0). Only used for subspace iteration.
=0 Generalised Jacobi method
=1 HouseholderQL method
maxmin
Determines whether minimum or maximum eigenvalues are required
(default=0).
=0 minimum eigenvalues required
=1 maximum eigenvalues required
buckl
Type of buckling required (default=0).
=0 normal buckling
=1 alternative buckling (all eigenvalues will be positive. See Notes on Eigenvalue Output)
302
Eigenvalue Control
Eigenvalue/Frequency Range
The EIGENVALUE RANGE or FREQUENCY RANGE data sections (for specifying eigenvalues or natural frequencies, respectively) are used to specify the options for the chosen eigenvalue solution method that will solve for a range of eigenmodes or frequencies. If this data section is used the CONSTANTS data section must be omitted.
With the exception of Rmin and Rmax, default values will be assumed for all other parameters that are not specified. If neither the INVERSE, LANCZOS nor FAST keywords appear on the command line, LUSAS will select the default eigenvalue solver, which is the fast Lanczos solver unless the analysis contains superelements, or is a branching and bracketing analysis, in which case the inverse iteration solver will be used.
[INVERSE  LANCZOS  FAST] {EIGENVALUE  FREQUENCY}
RANGE Rmin Rmax [nreq norm]
Rmin
Rmax
nreq
norm
The minimum eigenvalue or frequency for the defined range.
The maximum eigenvalue or frequency for the defined range (must be larger than Rmin).
The number of eigenvalues required (default = total number of eigenvalues within the specified range).
The normalisation procedure required for the eigenvectors (default=0).
=0 normalisation with respect to unity
=1 normalisation with respect to the global mass
=2 normalisation with respect to the global stiffness
Convergence
The CONVERGENCE data section is used to specify the internal convergence tolerance used for the subspace and inverse iteration solvers, and controls the maximum number of iterations to be used for the standard Lanczos solver. It is not used for the fast Lanczos solver. If this data section is not specified, the default values are assumed.
CONVERGENCE rtol [nitem]
or:
CONVERGENCE nitem
rtol
The iterative tolerance to be satisfied (not used for either Lanczos solver)
(default for subspace iteration = 1.0E7)
(default for inverse iteration with shifts = 1.0E4).
For subspace iteration, this measure is defined as the absolute value of (current eigenvalue  previous eigenvalue)/current eigenvalue. This must be satisfied for all eigenvalues before convergence is assumed. For inverse iteration with shifts, this measure is defined as the tolerance for mass orthogonality.
303
Chapter 3 LUSAS Data Input
nitem
The maximum number of iterations/steps to be carried out (not used for the fast Lanczos solver)
(default for subspace iteration = 10)
(default for inverse iteration with shifts = 30)
(default for standard Lanczos = 100).
The inverse iteration procedure should always converge quickly, since the shift point is automatically updated to improve convergence if convergence difficulties are detected.
The maximum number of iterations is, therefore, set to 30, since this should never be required by the algorithm. It is provided merely as a safety measure, and the default value may be changed by specifying the parameter nitem in the CONVERGENCE data section.
Eigenvalue Output
Eigenvalue analyses output the following results:
Eigenvalues, frequencies and error norms for each mode requested, for example:
MODE EIGENVALUE FREQUENCY ERROR NORM
1 81.7872 1.43934 0.2189E11
The total mass of the structure in the three global, translational directions, e.g.,
TOTAL MASS ACTING IN X DIRECTION = 3510.00 KG
TOTAL MASS ACTING IN Y DIRECTION = 3510.00 KG
Modal displacement shapes for each mode in turn. Note that these eigenvectors have no physical meaning except to indicate the mode shape.
Total reactions for each mode in turn (again, these have no physical meaning, since they are derived from the displacements).
Mass participation factors are output to indicate the proportion of mass acting in each mode. Note that this is calculated automatically and there is no requirement for this factor to sum to unity. Mass participation will always be
Notes
positive.
1. Combinations of the lowest, highest and a range of eigenvalues can be extracted in a single LUSAS run if required, by specifying additional EIGENVALUE
CONTROL data chapters with the relevant data sections. If using the fast Lanczos solver, this must be specifed for each eigenvalue extraction, since it requires the assembly of global matrices. The standard Lanczos solver can be used during the same run as the subspace and inverse iteration solvers, if desired. If the highest eigenvalues are required, this must be specified in the last EIGENVALUE
CONTROL data chapter, unless the fast Lanczos solver is in use. For example, to find the lowest two eigenvalues, the highest six eigenvalues and all frequencies in the range [0, 20] using the fast Lanczos solver, the following commands should be specified:
304
Eigenvalue Control
EIGENVALUE CONTROL
FAST 2
EIGENVALUE CONTROL
FAST 6 D D 1
EIGENVALUE CONTROL
FAST FREQUENCY RANGE 0 20
2. Combinations of eigenvalues can also be specified for stiffness and buckling analyses by specifying additional EIGENVALUE CONTROL STIFFNESS and
EIGENVALUE CONTROL BUCKLING data chapters, respectively. The same strictures apply as for the EIGENVALUE CONTROL data chapter.
3. In case the requested eigenmodes turn out not to be the ones actually needed, choosing OPTION 279 will cause the reduced stiffness and mass matrices to be saved to a restart file. They can then be accessed during a separate analysis, and more eigenmodes retrieved without needing to reduce the matrices again. Note that this facility is not available for the fast Lanczos solver.
4. The stresses from the eigenvectors may be output using ELEMENT and NODE
OUTPUT CONTROL.
5. If nmastr master freedoms are specified within the RETAINED FREEDOMS data section, a Guyan reduction analysis will be carried out in order to obtain a first approximation to the starting iteration vectors for the subspace iteration method. Note namast automatically generated master freedoms will be used if
nivc is greater than nmast (i.e. namast = nivc  nmastr).
6. If an EIGENVALUE CONTROL (including STIFFNESS and BUCKLING) data chapter using subspace iteration follows immediately after a GUYAN CONTROL data chapter, the solution from the Guyan reduction analysis will automatically be used as the first approximation to the starting iteration vectors required for the subspace iteration. This enables the Guyan solution to be improved by using the subspace iteration algorithm.
7. If an EIGENVALUE CONTROL data chapter and the GUYAN CONTROL data chapter are separated by any other data chapters, then each will be treated as a separate analysis. The same applies if a GUYAN CONTROL data chapter is immediately preceded by an EIGENVALUE CONTROL data chapter.
8. Throughout EIGENVALUE CONTROL, where a default value is shown, a D may be entered for a particular input variable to obtain the default value.
9. Within the subspace iteration method the eigenvalue solution may be continued after the Jacobi iteration method has failed to converge by setting Option 16, but the results should be used with caution.
10. If nreq is defined in the RANGE section the eigenvalues found will not always be the first eigenvalues of the system, unless the Fast Lanczos solver is used.
11. Option 230 will suppress the computation during an eigenvalue analysis. For reasonable size jobs this has the effect of reducing the plot file size to 1/3 of its original size which speeds up the analysis.
12. The Eigenvalue/Frequency Range facility cannot be used if constraint equations have been defined, unless the Fast Lanczos solver is used.
305
Chapter 3 LUSAS Data Input
13. The Sturm sequence check may prove unreliable if constraint equations are defined in the analysis, unless the Fast Lanczos solver is used.
14. For buckling analyses involving constraint equations, the Fast Lanczos solver will only find eigenvalues either side of zero, i.e. in the range (
, 0) or (0,
). If a range of eigenvalues is required in an interval which contains zero, two separate data chapters must be specified, where the interval is divided into two subintervals either side of zero.
15. The inverse iteration procedure should always converge quickly since the shift point is automatically updated to improve convergence if this is not the case. The maximum number of iterations is therefore set, by default, at 30 since this should never be required by the algorithm. It is provided merely as a safety measure and the default value may be changed by specifying the parameter nitem in the
CONVERGENCE data section.
Guyan Control
The GUYAN CONTROL data chapter is used to control the solution procedure for
Guyan reduced eigenvalue extraction analyses (for eigenvalue analyses using subspace iteration see Eigenvalue Control). For further information regarding the solution of eigenvalue problems by Guyan reduction refer to Guyan Reduction, and the LUSAS
Theory Manual.
GUYAN CONTROL [BUCKLING  STIFFNESS]
BUCKLING The BUCKLING command word is used to specify that the eigenvalue buckling problem is to be solved using Guyan reduction. This facility must only be used in conjunction with element types that support nonlinear solutions (see the LUSAS Element Reference Manual).
STIFFNESS
The STIFFNESS command word is used to specify that an eigenvalue analysis of the stiffness matrix is to be carried out using Guyan reduction.
Constants
The CONSTANTS data section is used to specify the constants for the Guyan reduction as well as to define the options available to the user. This section is compulsory, and with the exception of nroot default values will be assumed for all parameters that are not specified.
CONSTANTS nroot [namast shift norm sturm eigsol maxmin buckl]
nroot
The number of eigenvalues required (must be less than or equal to the number of free nodal variables of the reduced structure).
namast
The number of automatically generated master freedoms (default=0) (see
Retained Freedoms).
shift
The shift to be applied to the eigenvalue procedure (default = 0.0).
306
Guyan Control
norm
The normalisation procedure required for the eigenvectors (default=0).
=0 normalisation with respect to unity
=1 normalisation with respect to the global mass
=2 normalisation with respect to the global stiffness
sturm
Determines if a Sturm sequence check is to be applied (default=1).
=0 no Sturm sequence check
=1 Sturm sequence to be carried out
eigsol
Type of eigensolver required (default=0).
=0 Generalised Jacobi method
=1 HouseholderQL method
maxmin
Determines whether minimum or maximum eigenvalues are required
(default=0).
=0 minimum eigenvalues required
=1 maximum eigenvalues required
buckl
Type of buckling required (default=0).
=0 normal buckling
=1 alternative buckling (all eigenvalues will be positive) (see Notes).
Notes
1. Specified master freedoms may also be input via the RETAINED FREEDOM data chapter.
2. Master freedom selection may be either totally specified, or totally automatic, or a combination of the two. LUSAS will confirm the type of master freedoms used in the operation, and in the case of wholly specified or wholly automatic, will warn to that effect.
3. If LUSAS is unable to create the full requested number of masters a warning to that effect will be invoked, and the solution will proceed with the reduced number of automatic master freedoms. Note that this is equivalent to carrying out an eigenanalysis of the full problem.
4. The solution obtained by a Guyan reduction can be improved upon by employing the subspace iteration algorithm. This will be done if an EIGENVALUE
CONTROL data chapter follows immediately after a GUYAN CONTROL data chapter; the Guyan reduction solution will automatically be used as the first approximation to the starting iteration vectors required for the subspace iteration.
5. If an EIGENVALUE CONTROL data chapter and the GUYAN CONTROL data chapter are separated by any other data chapter then each will be treated as a separate analysis. The same applies if a GUYAN CONTROL data chapter is immediately preceded by an EIGENVALUE CONTROL data chapter.
6. Throughout GUYAN CONTROL, where stated, a D may be entered for a particular input variable to obtain the default value.
7. The nonlinear solution may be continued after the Jacobi iteration method has failed to converge by setting Option 16.
8. Freedoms featuring in constraint equations will not be considered for use as automatic masters.
307
Chapter 3 LUSAS Data Input
9. The Sturm sequence check may prove unreliable if constraint equations are defined in the analysis.
Modal Damping Control
The MODAL_DAMPING CONTROL data chapter is used to control the computation of viscous or structural distributed damping factors where element contributions towards damping vary within the structure. This data chapter should always follow an eigenvalue analysis since this analysis depends upon the eigensolutions that should have already been obtained. This section is valid for viscous (modal) and structural
(hysteretic) damping. After this section LUSAS computes the distributed viscous and/or structural damping factors and echoes the damping factors to the LUSAS output file. These damping factors may subsequently be used in a harmonic or spectral response analysis or a LUSAS Modeller modal analysis session.
MODAL_DAMPING CONTROL [VISCOUS  STRUCTURAL]
Constants
The CONSTANTS data section is used to specify the default damping factor for a mode if the distributed damping factor is not to be computed (i.e. mode omitted from
MODES section). If this section is not specified the system default values will apply.
CONSTANTS damp
damp
The overriding default damping factor if the distributed damping factor is not to be computed (default=0.05 for VISCOUS damping, default=0.00 for
STRUCTURAL damping)
Material Properties
This line is optional and is only required if the damping parameters from the
MATERIAL PROPERTY data chapter and not the DAMPING PROPERTIES data chapter are to be used for the computation of the distributed damping factors. By default Rayleigh parameters from the DAMPING PROPERTIES section are used. If no
DAMPING PROPERTIES are input then Rayleigh parameters from the MATERIAL
PROPERTIES section are used.
MATERIAL PROPERTIES
Modes
This section is optional and is used when the distributed damping is to be computed for only some modes. By default distributed damping factors will be computed for all modes.
MODES modei
308
Modal Damping Control
modei
Number of the (i)th mode for which distributed damping must be computed. This line must be repeated for each mode but may be generated by using the LUSAS data generation structure FIRST, INC, INC etc.
Distributed damping factors will not be computed for modes omitted here but these modes will take the default damping factor as specified in the CONSTANTS data section.
Notes
1. The parameter norm in EIGENVALUE or GUYAN control must be set to 1 in the eigenvalue analysis to normalise the eigenvectors with respect to global mass before computation of distributed modal damping factors.
2. After computing the distributed viscous and/or structural damping factors LUSAS will write the values to the output file.
Example. Damping Properties
:
C Table of viscous damping properties
DAMPING PROPERTIES VISCOUS
C a i
, b i
,
i
, a b i
,
I
(Hz) i
, b i
,
i
, a i
,
1 3 1 0.1 0.05 0 0.1 0.05 0.2
0.3 0.2 0.3 ...
0.1 0.05 0.5 0.1 0.05 0.6 0.3
0.2 0.7 ...
0.3 0.2 0.9 0.1 0.05 1.0 0.1
0.05 1.5
C Table of structural damping properties
DAMPING PROPERTIES STRUCTURAL
C a i
, b i
,
i
, a b i
,
I
(Hz) i
, b i
,
i
, a i
,
1 0 0 0.1 0.05 0.1 0.1 0.05 0.2
0.3 0.4 0.4 ...
0.1 0.05 0.5 0.1 0.05 0.6 0.5
0.2 0.7 ...
0.7 0.2 0.9 0.1 0.05 1.0 0.1
0.05 1.5
309
Chapter 3 LUSAS Data Input
2 0 0 0.1 0.05 0.1 0.1 0.05 0.2
0.3 0.4 0.4 ...
0.1 0.05 0.5 0.1 0.05 0.6 0.5
0.2 0.7 ...
0.7 0.2 0.9 0.1 0.05 1.0 0.1
0.05 1.5
3 0 0 0.1 0.05 0.1 0.1 0.05 0.2
0.3 0.4 0.4 ...
0.1 0.05 0.5 0.1 0.05 0.6 0.5
0.2 0.7 ...
0.7 0.2 0.9 0.1 0.05 1.0 0.1
0.05 1.5
:
LOAD CASE
CL
4 16 4 5./32.**.5
C Eigenvalue analysis (3 modes)
EIGENVALUE CONTROL
CONST 3 3 D 1
C Compute distributed viscous damping factors for all three modes. Rayleigh
C parameters from the DAMPING PROPERTIES VISCOUS table will be used in the
C computation.
MODAL_DAMPING CONTROL VISCOUS
C Compute distributed structural damping factors for modes 1 and 3. Use the
C overriding default damping constant of 0.33 for mode
2. Rayleigh parameters from
C the DAMPING PROPERTIES STRUCTURAL table will be used in the computation.
MODAL_DAMPING CONTROL STRUCTURAL
CONSTANTS 0.33
MODES
1 3 2
310
Spectral Control
C Harmonic response analysis using distributed viscous damping factors and system
C factors (no distributed structural damping factors will be used).
C Default values for structural damping are used.
HARMONIC_RESPONSE CONTROL
CONSTANTS 3 0.1
VISCOUS DAMPING DISTRIBUTED
FREQUENCIES
0.01
0.175
0.477
HARMONIC LOADING REAL 1
HARMONIC LOADING IMAGIN 1
END
Spectral Control
The SPECTRAL CONTROL data chapter is used to control the solution procedure for spectral response analyses. This data chapter must always follow an eigenvalue analysis since the analysis depends upon the eigensolutions that should have already been obtained. For further information regarding the solution of spectral response problems refer to Spectral Response Analysis, and the LUSAS Theory Manual.
SPECTRAL CONTROL
Constants
The CONSTANTS data section is used to specify certain constants for the spectral response procedure. This data section is mandatory.
CONSTANTS nmod icmb [dampm]
nmod
icmb
The number of modes to be processed. Must be less than or equal to the number of eigenvalues previously extracted (default = number of eigenvalues previously solved for, i.e. nroot).
The spectral combination type.
=0 for no combination required (default)
=1 for SRSS (square root of the sum of the squares)
=2 for CQC (complete quadratic combination)
=3 for Absolute Sum
311
Chapter 3 LUSAS Data Input
dampm
The overriding default value for the modal damping coefficients not specified in the MODAL DAMPING data section. (default = 0.05, that is
5%).
Modal damping
The MODAL DAMPING data section is used to specify the damping of each system mode of vibration as a portion of the critical damping for that mode. Modal damping may be input for each mode directly (LUSAS will then assign the modal damping value to the modal frequency when it has been determined by the eigenvalue analysis) using MODES, or may be input at known frequencies (LUSAS will then interpolate to the modal frequencies computed in the eigenvalue analysis) using FREQUENCIES.
Alternatively the physical distribution of damping in a structure may be modelled using
MODAL DAMPING DISTRIBUTED, where the computed modal damping factors from MODAL_DAMPING CONTROL VISCOUS (see Modal Damping Control) is used.
The following apply only for MODES and FREQUENCIES keywords:
MODAL DAMPING {DISTRIBUTED  MODES RAYLEIGH 
FREQUENCIES RAYLEIGH}
{Mi 
i} ai [bi]
Mi
i
ai
bi
The (i)th mode number.
The (i)th specified frequency.
The modal damping value for the (i)th mode or (i)th specified frequency, or the mass Rayleigh damping constant when the RAYLEIGH option is invoked.
The stiffness Rayleigh damping constant when the RAYLEIGH option is invoked.
Excitation
The EXCITATION data section specifies the excitation direction and is compulsory.
EXCITATION Xdir Ydir Zdir
Xdir
Ydir
The excitation factor in the global Xdirection
The excitation factor in the global Ydirection
Zdir
The excitation factor in the global Zdirection
Note. The above factors are the components of the vector defining the direction of excitation.
Spectral Curve
The SPECTRAL CURVE data section is used to specify the frequencydisplacement, frequencyvelocity or frequencyacceleration curve.
312
Harmonic Response Control
SPECTRAL CURVE nspts icurve
< freq i
value i
> i=1,n
nspts
The number of points defining the spectral curve.
Icurve
The spectral curve type:
=1 for frequencydisplacement curve
=2 for frequencyvelocity curve
=3 for frequencyacceleration curve
=4 for period displacement curve
=5 for period velocity curve
=6 for period acceleration curve
freq i
The frequency for the (i)th point on the spectral curve.
value i
The value of the displacement/velocity/acceleration for the (i)th point on the spectral curve in ascending order.
Notes
1. The parameter norm in EIGENVALUE or GUYAN CONTROL must be set to 1 in the eigenvalue analysis to normalise the eigenvectors to global mass before a spectral analysis can be carried out.
2. To use distributed damping factors MODAL DAMPING DISTRIBUTED must be specified, otherwise the current direct input damping factors will be used.
3. When MODAL DAMPING is specified it must follow CONSTANTS.
4. If PLOT FILE is placed after the SPECTRAL CONTROL chapter the spectral results are transferred to the LUSAS Modeller plot file for subsequent plotting.
5. Damping is only taken into account for spectral combination type CQC.
6. Spectral response may also be carried out in LUSAS Modeller.
Harmonic Response Control
The HARMONIC_RESPONSE CONTROL data chapter is used to control the solution procedure for forced vibration or harmonic response analysis. This data chapter should always follow an eigenvalue analysis since this analysis depends upon the eigensolutions that should have already been obtained. For further information regarding the solution of forced vibration problems refer to Harmonic Response
Analysis, and the LUSAS Theory Manual.
HARMONIC_RESPONSE CONTROL
Constants
The CONSTANTS data section is used to specify the harmonic response control parameters and the user defined default damping values. This section may only be specified once in an analysis; once these constants have been defined they are unchangeable.
313
Chapter 3 LUSAS Data Input
CONSTANTS nmod dampm damps
nmod
The number of system eigenmodes which are to be utilised in the harmonic response analysis. (default = number of eigenvalues previously solved for, i.e. nroot)
dampm
The overriding default value for the viscous damping coefficients not specified in the VISCOUS DAMPING data section. (default = 0.05, that is
5%)
damps
The overriding default value for structural damping coefficients not specified in the STRUCTURAL DAMPING data section. (default = 0.0, that is 0%)
Frequencies
The FREQUENCY data section is used to specify the loading (or sampling) frequencies for which the harmonic analysis will be carried out.
FREQUENCIES freqi
freqi
Value of the (i)th sampling frequency. This line must be repeated for each frequency but may be generated by using the LUSAS data generation structure FIRST, INC, INC.
Viscous Damping
The VISCOUS DAMPING data section is used to specify the damping of each system mode of vibration as a portion of the critical damping for that mode. Viscous damping may be input for each mode directly using the MODES keyword (LUSAS will then assign the viscous damping value to the modal frequency when it has been determined by the eigenvalue analysis) or may be input at known frequencies (LUSAS will then interpolate to the modal frequencies computed in the eigenvalue analysis) using the
FREQUENCIES keyword. Alternatively the physical distribution of damping in a structure may be modelled using VISCOUS DAMPING DISTRIBUTED, where the computed viscous damping factors from MODAL_DAMPING CONTROL VISCOUS are used (see section on Modal Damping Control).
The following apply only for MODES and FREQUENCIES keywords:
Mi
i
ai
VISCOUS DAMPING {DISTRIBUTED  MODES RAYLEIGH 
FREQUENCIES RAYLEIGH}
{M i

i
} a i
[b i
]
The (i)th mode number.
The (i)th specified frequency.
The modal damping value for the (i)th mode or (i)th specified frequency, or the mass Rayleigh damping constant when the RAYLEIGH option is invoked.
314
Harmonic Response Control
bi
The stiffness Rayleigh damping constant when the RAYLEIGH option is invoked.
Structural Damping
The STRUCTURAL DAMPING data section specifies the damping of each system mode of vibration via the hysteretic damping value; this value may be different for each system mode but is constant for the structure for each mode. Structural damping may be input for each mode directly (LUSAS will then assign the structural damping value to the modal frequency when it has been determined by the eigenvalue analysis) using the MODES keyword or may be input at known frequencies using the FREQUENCIES keyword (LUSAS will then interpolate to the modal frequencies computed in the eigenvalue analysis). Alternatively the physical distribution of damping in a structure may be modelled using STRUCTURAL DAMPING DISTRIBUTED, where the computed modal damping factors from MODAL_DAMPING CONTROL
STRUCTURAL are used (see section on Modal Damping Control).
The following apply only for MODES and FREQUENCIES keywords:
STRUCTURAL DAMPING {DISTRIBUTED  MODES  FREQUENCIES}
{Mi 
i} i
Mi
i
i
The (i)th mode number.
The (i)th specified frequency.
The structural damping value for the (i)th mode or (i)th specified frequency.
Harmonic Loading
The HARMONIC LOADING data section specifies the harmonic loads in terms of their real and imaginary components. By specifying both components the phase difference of the loads can be specified.
HARMONIC LOADING {REAL  IMAGINARY} lnum
lnum
The LOAD CASE number which describes the harmonic loading component.
The HARMONIC LOADING defaults are defined as follows:
If no HARMONIC LOADING is defined or if the HARMONIC LOADING command is specified without any parameters then the default loading is assumed:
LOAD CASE number 1 is used as the real component and the imaginary component is assumed to be zero;
If only the real component of load is specified then the imaginary component is assumed to be zero;
If only the imaginary component of load is specified then the real component is assumed to be zero.
315
Chapter 3 LUSAS Data Input
Notes
1. The parameter norm in EIGENVALUE or GUYAN CONTROL must be set to 1 in the eigenvalue analysis to normalise the eigenvectors to global mass before a harmonic response analysis can be carried out.
2. Modal and structural damping values for unspecified system modes for direct input of damping using VISCOUS DAMPING MODES or FREQUENCIES will be interpreted as the default values in the CONSTANTS data section.
3. Modal and structural damping values specified at known FREQUENCIES will be interpolated at the nmod selected system frequencies: interpolation to system frequencies within the range specified in the relevant DAMPING data section will be linear, while interpolation to system frequencies beyond the range specified will be constant and will invoke a warning message.
4. Original and interpolated damping will be echoed.
5. When Rayleigh damping constants are specified the corresponding modal damping is computed from: modal damping
HG
F a r w
2 w b r
KJ
I where w is either the natural frequency corresponding to the particular mode or the frequency that is input on the data line. This conversion is done before the interpretation of the damping is carried out.
6. When the RAYLEIGH option is used notes 3. and 4. will still apply.
7. To use distributed damping factors VISCOUS and/or STRUCTURAL DAMPING
DISTRIBUTED must be specified otherwise the current direct input damping factors will be used.
8. LOAD CASE numbering is assumed to be consecutive. After a RESTART command has been used the new LOAD CASES start renumbering from 1 again.
9. The harmonic loading must be respecified with every new
HARMONIC_RESPONSE data command.
10. Throughout HARMONIC_RESPONSE CONTROL, where a default is given, you can input a D for a particular input variable to invoke the default value.
11. Option 181 provides output in the polar coordinate system.
12. PDSP loading is not permitted with this facility.
Fourier Control
The FOURIER CONTROL data chapter controls the input of the Fourier components for use with Fourier elements. This data chapter must be used if Fourier elements are
316
Fourier Control
utilised. For further information regarding the solution of Fourier problems refer to the section titled Fourier Analysis, and the LUSAS Theory Manual.
FOURIER CONTROL
HARMONIC [symmetry]
H Hlast Hdiff
symmetry The harmonic components to be analysed (default = 0):
= 0 both symmetric and asymmetric components
= 1 only the asymmetric components
= 2 only the symmetric components
H Hlast Hdiff
The first harmonic, last harmonic and difference in harmonics of the Fourier expansion.
Example. Fourier Control
In order to apply a line load with an intensity of 8 per unit length of the structure over an arc from 10° to 20° and to solve for the first 4 harmonics (symmetric), the datafile will have the following form:
LOAD CASE
CL
1 0 0 16. 0. 0.
CURVE DEFINITION 4 USER :define User curve 4
10 1
20 1
:assign a value of 1 at 10°
:assign a value of 1 at 20°
CURVE ASSIGNMENT
1 0.5 4 of 0.5 to loadcase 1
:assign load curve 4 with a factor
FOURIER CONTROL
HARMONICS 2
0 3 1
:solve symmetric components only
:evaluate harmonics 0,1,2 and 3.
Concentrated loads, constant body forces and body force potentials are applied in the global XYZ directions, as opposed to surface tractions, initial stresses, initial strains and thermal loading which are all applied in the local xyz directions. Note that concentrated loads/nodal reactions are input and output as forces per unit length.
Concentrated loads may also be applied in the cylindrical coordinate system by setting
Option 202.
317
Chapter 3 LUSAS Data Input
Notes
1. Both the symmetric and the asymmetric components will be calculated unless overridden by the symmetry input parameter.
2. The HARMONIC data line applies to all H, Hlast, Hdiff series following the specification of this command. HARMONIC may be respecified in this data chapter if required.
3. All loads for a static analysis will be decomposed into the defined harmonic components.
4. If a dynamic, eigenvalue or harmonic response analysis is required the harmonic series should only contain 1 term.
5. Concentrated loads may be applied in the local cylindrical coordinate system by using Option 202.
Creating a Plot File
The PLOT FILE data section writes the analysis mesh data and results to secondary storage for subsequent plotting using LUSAS Modeller. For nonlinear, dynamic, transient and viscous analyses the frequency of plot file generation is controlled via the
OUTPUT data sections (in these cases the PLOT FILE data section is not required).
PLOT FILE
Notes
1. For linear analyses PLOT FILE must be placed after all the LOAD CASE and
ELEMENT/NODAL OUTPUT commands.
2. PLOT FILE should be specified prior to ENVELOPE and LOAD
COMBINATION.
3. To save eigenvalue results, place the PLOT FILE command prior to the harmonic or spectral commands.
4. The structural definition can be saved (and subsequently viewed) when using a preanalysis data check (Option 51).
5. When carrying out a nonlinear, dynamic, transient or a viscous analysis the plot file should be requested by setting the incplt parameter within the OUTPUT data section in the appropriate data chapter. However, the PLOT FILE command may still be specified at the end of the analysis.
6. If a nonlinear, dynamic, transient or a viscous analysis terminates and plot files have been requested a plot file will always be created for the last increment.
Restart Facilities
Data can be written to disk to enable a nonlinear, dynamic, transient or viscous problem to be restarted from additional steps or a load combination to be carried out.
318
Restart Facilities
Note that for nonlinear, dynamic, transient or viscous analyses the frequency of restart file generation is controlled via the OUTPUT data sections of the appropriate
CONTROL data chapter.
Writing to a Restart File
The data section RESTART WRITE is used to control writing of the LUSAS database to disk for subsequent processing.
RESTART WRITE [BRIEF] [ndump]
ndump
The number of the restart dump to be written.
Notes
1. Restart files are written to a file of the same name as the data file but with an extension of .rst.
2. May be placed after any LOAD CASE data chapter for nonlinear problems.
3. The RESTART WRITE BRIEF command will dump sufficient information to enable a problem to be restarted for LOAD COMBINATIONS. This option cannot be used for restarting any other problem.
4. If no dump number is specified the dump number will be incremented by one from the previous highest value.
5. If a dump number is specified that already exists, a warning message will be printed and the dump will be overwritten.
6. In a nonlinear problem a dump will only be written if the solution converged.
7. When carrying out a nonlinear, dynamic, transient or a viscous analysis the restart write file should be requested by setting the incrst parameter within the
OUTPUT data section in the appropriate data chapter.
8. If a nonlinear, dynamic, transient or a viscous analysis terminates and restart dumps have been requested a restart dump will always be created for the last increment.
9. Selecting Option 251 will generate a restart file from a data check phase. To complete the analysis after a successful data check, initiate the restart file and
LUSAS will recommence the analysis at the equation solution phase. This particular restart facility is only valid for a linear static problem and is not available for other types of analyses.
Reading from a Restart File
The data section RESTART READ is used to control reading of the written LUSAS database from disk for subsequent processing.
RESTART READ [ndump] [fname]
ndump
The number of the RESTART WRITE dump to be recovered
(default = last saved dump).
319
Chapter 3 LUSAS Data Input
fname
The file name of the restart file (without extension).
(default = name of data file).
Notes
1. The filename extension .rst is used for all restart files.
2. The RESTART READ data command must be the first line of any restart processing (unless a SYSTEM command is present in which case the RESTART
READ will follow this).
3. Further data may be stored in the restart file after a RESTART READ.
4. A new LUSAS Modeller plot file will be created in a nonlinear, dynamic, transient or viscous analysis if required after a RESTART READ. The existing plot file can be used by setting Option 204 either in the previous analysis or in the restart data file.
5. Any system parameters specified in the previous analysis must be respecified on restart.
6. A RESTART analysis can be utilised to create a LUSAS Modeller plot file only.
Example. Restart Read
To create a plot file only:
RESTART READ
PLOT FILE
END
To continue a nonlinear analysis:
RESTART READ
LOADCASE
...
NONLINEAR CONTROL
...
END
To perform a presolution restart analysis created using Option 251:
RESTART READ filename
PLOT FILE
END
320
ReSolution
ReSolution
The reduced stiffness matrices for linear elastic analyses can be saved to disk by specifying option 279 when using the restart facility. This allows subsequent analyses to process additional load cases using the matrix stored on disk to reduce solution times. The stiffness file takes a default .stf extension, and the location of the stored stiffness file can be changed using the STIFFNESS environment variable. The stiffness file changes during the resolution phase. The highest load case from the previous resolution is stored in the file. Loadcases will be numbered in ascending order if not otherwise specified on the LOAD CASE line, as is the default when the data file is tabulated by Modeller. The stiffness file must have the same name as the restart file, but with a .stf extension.
The stiffness matrix is accessed for resolution using the RESTART READ command, and it must be available when the restart file is read if option 279 was used when the restart file was created. If LUSAS cannot locate a stiffness file while reading the restart file, an error will be issued. If the stiffness file has accidentally been erased or corrupted, it should be recreated by rerunning the original analysis.
The data syntax for creating a stiffness file using the restart write command is as follows:
problem title resolution options 279
... load case
... restart write end
The stiffness file is read using the restart read command and subsequent load cases are processed by specifying the following syntax:
restart read filename load case
... load case
... load case
... end
321
End
Chapter 3 LUSAS Data Input
Notes
1. It is advisable to always work on a backup copy of the stiffness file as it can become corrupted if LUSAS terminates with an error while accessing the file.
2. The stiffness file cannot be split using the method outlined for splitting the frontal file.
The data section END is used to terminate the current problem data file and is mandatory.
END
Notes
1. The END statement must be the last data section in the analysis datafile.
322
LUSAS User Options
Appendix A LUSAS
User Options
For usability LUSAS User Options are listed by option number and also by Category
LUSAS User Options
No. Effect of option (plus related notes where applicable)
2 Suppress node coordinate checks for similar coordinates
4 and missing nodes
No overwriting present in data exit on first occurrence
14 Compute element stresses and strains (plates/flat shells)
16 Continue nonlinear/eigenvalue solution when failed to converge
17 Keep global matrix assembly incore for fast/iterative solvers
18 Invokes finer numerical integration rules for elements
19 Invokes coarse numerical integration rule for semiloof
20 Invokes nonorthogonal concrete crack model (concrete model 24)
22 Invokes fracture energy strainsoftening model (concrete model 24)
23 Invokes strainvariable shear retention model (concrete model 24)
26 Reduce number of lines output in coordinates
30 Output final node coordinates in ascending order
32 Suppresses stress output but not stress resultant output
33 Output direction cosines of local cartesian systems for interface
34 Output element stress resultants
36 Follower loads (available for selected elements)
39 Stress smoothing for rubber material models
40 Output nodal displacement increments for nonlinear analyses
42 Output nodal residual forces (nonlinear)
Category
INPUT
INPUT
PROCESSING
NONLINEAR /
EIGENVALUES
NONLINEAR
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
OUTPUT
OPTIMISATION
OUTPUT
OUTPUT
OUTPUT
NONLINEAR
OUTPUT
OUTPUT
OUTPUT
323
Appendix A LUSAS User Options
No. Effect of option (plus related notes where applicable)
44 Suppress expanded input data printout except load cases
45 Suppress expanded input data printout for load cases
46 Suppress page skip between output stages
Category
OUTPUT
INPUT
OUTPUT
47 Axisymmetry about the global Xaxis INPUT
48 Switch CBF input from Force/unit volume to acceleration INPUT
49 Automatic correction of midside nodes INPUT
51
53
Data processing only
Positive definite/singularity check on modulus matrix at each Gauss point
54 Updated Lagrangian geometric nonlinearity
55 Output strains as well as stresses
INPUT
PROCESSING
NONLINEAR
OUTPUT
59 Output local direction cosines for shells
61 All 2D slideline surfaces defined with outward normals
OUTPUT
INPUT
62 Continue solution if more than one negative pivot occurs NONLINEAR
64 Nonsymmetric frontal solution
66 Calculate element internal forces
70 Echo nodal data read from data transfer file
72 Suppress machine code inner loops
SOLVER
PROCESSING
COUPLED
OPTIMISATION
77
87
91
93
Output principal stresses and directions for solids
Total Lagrangian geometric nonlinearity
Formulate element mass with fine integration
Suppress intermediate eigenvalue output for Subspace or bracketing methods
100 Output optimum frontal solution order
102 Switch off load correction stiffness matrix due to centripetal acceleration
OUTPUT
NONLINEAR
INTEGRATION
EIGENVALUES
OPTIMISATION
LOADING
DYNAMICS
PROCESSING
105 Lumped mass matrix
110 Use assumed shear strain field for QTS8 thick shell elements
111 Don't include superelement generation load
115 Output displacements and reactions in transformed axes
116 Suppress the output of internal constraint forces
117 Invokes geometric assignments input
118 Invokes material assignments input
119 Invokes temperature input for joints (by default no temperature in joints)
123 Clockwise node numbering
124 Save shape function array for restarts
131 Parallel frontal solver algorithm
134 Gauss to NewtonCotes integration for elements
136 Stress resultants by f=Kd and cubic interpolation
137 Stress resultants by f=Kd and equilibrium
138 Output yield flags only
PROCESSING
OUTPUT
OUTPUT
INPUT
INPUT
INPUT
INPUT
RESTART
SOLVER
INTEGRATION
PROCESSING
PROCESSING
NONLINEAR
324
LUSAS User Options
No. Effect of option (plus related notes where applicable)
139 Output yielded, cracked or crushed integration points only for MNL
143 Output shear forces in plate bending elements.
Category
NONLINEAR
144 Output element results for each load case separately
146 Include stiffness (second) Rayleigh damping parameter
147 Omit output phase
OUTPUT
OUTPUT
DYNAMICS
OUTPUT
155 14 point integration rule for HX20
156 13 point integration rule for HX20
157 Material Model 29 required (mandatory with noncrosssection elements)
INTEGRATION
INTEGRATION
NONLINEAR
164 Guide arclength solution with current stiffness parameter NONLINEAR
167 Eulerian geometric nonlinearity NONLINEAR
169 Suppress extrapolation of stress to nodes for semiloof shell OUTPUT
170 Suppress storage of shapes OPTIMISATION
INTEGRATION 171 Use standard shear strain field for QTS4 thick shell elements
172 Formulate modulus matrix by integrating across the crosssection
INTEGRATION
179 Verify arguments to usersupplied constitutive model routines
181 Harmonic response/complex mode output required in polar system
183 Double convergence check on coupled analyses running
184
185 concurrently
Suppress stringent slave search for slideline problems
Suppress initial slideline_surface stiffness check
NONLINEAR
OUTPUT
COUPLED
SLIDELINES
SLIDELINES
186 Suppress initial penetration check for slidelines
187 Include all variables in convergence norm computations
SLIDELINES
NONLINEAR
197 Fast element stiffness formulation without sparsity checks OPTIMISATION
202 Apply CLs in local cylindrical coordinates with Fourier LOADING elements
204 Use existing Plot file after restarting an analysis
207 Use angle in degrees to define direction of anisotropy for userdefined materials
208 Write plot file in pre version 11.0 format (not valid for explicit dynamics)
225 Use alternative number of parameters for enhanced strain interpolation function
RESTART
INPUT
OUTPUT
INTEGRATION
227 Error if a value is outside the bounds of a table of values PROCESSING
229 Corotational nonlinear geometric formulation NONLINEAR
230 Suppress stress calculation for eigenvalue analysis OPTIMISATION
PROCESSING 231 Error for material direction cosines not in plane of semiloof elements
235 Heat fraction specified for thermal softening INPUT
325
Appendix A LUSAS User Options
No. Effect of option (plus related notes where applicable)
242 Temperatures input and output in degrees Celsius
247 Extra output for iterative solvers
248 Single precision preconditioning for PCG solver
250 Datafile has been created by Modeller
251 Data processing and create a restart file (linear static analyses only)
Category
INPUT
SOLVER
SOLVER
252 Suppress pivot warning messages from frontal solution algorithm
SOLVER
253 Emissivity specified in thermal environment properties INPUT
254 Output all eigensolutions computed using inverse iteration EIGENVALUE
255 Output all radiation surface view factors to FACET file. OUTPUT
256 Suppress recalculation of radiation view factors in coupled analyses
259 Save nodal stresses in plot file to avoid stress extrapolation
INPUT
INPUT
COUPLED
OUTPUT in Modeller
261 Switch for selecting root with lowest residual norm (arclength method)
266 Layer by layer computation of mass matrix for solid composites
272 Activate or deactivate elements
273 Contact penalty stiffness update for augmented Lagrangian and slidelines
274 Use Uzawa rather than Powell method for node activity
NONLINEAR
INTEGRATION
PROCESSING
NONLINEAR
275 Automatic time step calculation for implicit dynamics
278 Assign six degrees of freedom to all thick shell element nodes
279 Save the reduced stiffness for further use in a linear analysis
281 Autoloader file
289 Plastic work is to be transferred in a coupled analysis
308 Arclength solution using local relative displacements
(interface elements)
310 Output results to userdefined output file
311 Compute number of eigenvalues in specified range and
PROCESSING
DYNAMICS
PROCESSING
SOLVER
PROCESSING
COUPLED
290 Write element stiffness and mass matrices to plot file OUTPUT
303 Exclude incompatible modes for solid composite elements PROCESSING
304 Plot/restart databases open until end of analysis. Speeds subsequent dumps.
OUTPUT
NONLINEAR
OUTPUT
EIGENVALUE terminate analysis
318 Adaptive Analysis: Overwrite disp's with interpolated disp's from old mesh
319 Invokes eccentricity input for QTS4 thick shell family
320 Global matrix (and righthand side) assembly and output only
PROCESSING
INPUT
OUTPUT
326
LUSAS User Options
No. Effect of option (plus related notes where applicable)
323 Extra preconditioning for iterative solver with a hierarchical basis
324 Specify damping properties for joint properties general explicitly
340 Allow application of angular velocities with nonlinear auto incrementation
342
344
345
346
347
Always output progress information during solution
Suppress condition number estimate in fast solvers
Separate plot file for each analysis step
Single segment contact from beginning of problem
Single segment contact from beginning of second
Category
SOLVER
INPUT
NONLINEAR
OUTPUT
SOLVER
OUTPUT
PROCESSING
PROCESSING increment
348 Slideline summary output
350 Invokes product moment of inertia (Iyz) input for BTS3
OUTPUT
INPUT nonlinear thick beam elements
352 Turn off consistently linearised formulation for slidelines SLIDELINES
353 Use of a fixed penalty parameter with slidelines
355 Slideline Cohesion with Coulomb friction in 2D
SLIDELINES
SLIDELINES
OUTPUT 363 Suppress echo of computed laminate properties in output file (woven fabric material)
364 Write element stiffness, mass and damping matrices to plot file
370 Strain hardening approach to modified von Mises and
OUTPUT
NONLINEAR
Hoffman material models (77/78)
373 Extended input data diagostics for CEBFIP creep and shrinkage model
376 Suppress use of METIS ordering for fast solvers
377 Use minimum amount of memory for BCS solvers
380 Output stress resultants relative to beam axes for eccentric
BTS3 elements
OUTPUT
SOLVER
SOLVER
OUTPUT
381 Apply CBF,ELDS,UDL loads along beam axes with
BMS3 elements
385 Preserve loading assigned to deactivated elements for subsequent application on activation
389 Echo thermal link elements to output file
390 Include selected results in plot file for dataonlyprocessing
LOADING
LOADING
386 Use of weighted force/stiffness distribution with slidelines SLIDELINES
387 Redefine NSET to angle in element xyplane for use in PROCESSING orthotropic material properties
388 Use duplicate nodes facility for collapsed elements PROCESSING
OUTPUT
OUTPUT
394 Lamina directions supported
395 Use 14point fine integration rule for mass matrix of TH10 family (used together with 91)
PROCESSING
INTEGRATION
327
Appendix A LUSAS User Options
No. Effect of option (plus related notes where applicable)
396 Improved top/middle/bottom transverse shear stress calculation for thick shell elements
397 With dataonlyprocessing, compute memory requirements for solution of equations
398 Use all 27/18 integration points for stress extrapolation for
20/16 node solids with fine integration
399 Retain inactive elements in birth and death solution (old analysis type)
Category
INTEGRATION
PROCESSING
INTEGRATION
PROCESSING
328
LUSAS User Options by Category
LUSAS User Options by Category
No. Effect of option (plus related notes where applicable)
70 Echo nodal data read from data transfer file
183 Double convergence check on coupled analyses running
Category
COUPLED
COUPLED concurrently
256 Suppress recalculation of radiation view factors in coupled analyses
289 Plastic work is to be transferred in a coupled analysis
COUPLED
COUPLED
105 Lumped mass matrix
146 Include stiffness (second) Rayleigh damping parameter
DYNAMICS
DYNAMICS
275 Automatic time step calculation for implicit dynamics DYNAMICS
254 Output all eigensolutions computed using inverse iteration EIGENVALUE
EIGENVALUE 311 Compute number of eigenvalues in specified range and terminate analysis
93 Suppress intermediate eigenvalue output for Subspace or bracketing methods
EIGENVALUES
2 Suppress node coordinate checks for similar coordinates and missing nodes
4 No overwriting present in data exit on first occurrence
45 Suppress expanded input data printout for load cases
INPUT
INPUT
INPUT
47 Axisymmetry about the global Xaxis INPUT
48 Switch CBF input from Force/unit volume to acceleration INPUT
49 Automatic correction of midside nodes
51 Data processing only
INPUT
INPUT
61 All 2D slideline surfaces defined with outward normals
117 Invokes geometric assignments input
118 Invokes material assignments input
119 Invokes temperature input for joints (by default no temperature in joints)
123 Clockwise node numbering
207 Use angle in degrees to define direction of anisotropy for
INPUT
INPUT
INPUT
INPUT
INPUT
INPUT userdefined materials
235 Heat fraction specified for thermal softening
242 Temperatures input and output in degrees Celsius
250 Datafile has been created by Modeller
251 Data processing and create a restart file (linear static analyses only)
253 Emissivity specified in thermal environment properties
319 Invokes eccentricity input for QTS4 thick shell family
324 Specify damping properties for joint properties general explicitly
350 Invokes product moment of inertia (Iyz) input for BTS3 nonlinear thick beam elements
INPUT
INPUT
INPUT
INPUT
INPUT
INPUT
INPUT
INPUT
329
Appendix A LUSAS User Options
No. Effect of option (plus related notes where applicable)
18 Invokes finer numerical integration rules for elements
19 Invokes coarse numerical integration rule for semiloof
20 Invokes nonorthogonal concrete crack model (concrete model 24)
22 Invokes fracture energy strainsoftening model (concrete model 24)
23 Invokes strainvariable shear retention model (concrete model 24)
91 Formulate element mass with fine integration
134 Gauss to NewtonCotes integration for elements
155 14 point integration rule for HX20
156 13 point integration rule for HX20
171 Use standard shear strain field for QTS4 thick shell elements
172 Formulate modulus matrix by integrating across the crosssection
225 Use alternative number of parameters for enhanced strain interpolation function
266 Layer by layer computation of mass matrix for solid composites
395 Use 14point fine integration rule for mass matrix of TH10 family (used together with 91)
396 Improved top/middle/bottom transverse shear stress calculation for thick shell elements
398 Use all 27/18 integration points for stress extrapolation for
20/16 node solids with fine integration
Category
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
INTEGRATION
102 Switch off load correction stiffness matrix due to centripetal acceleration
202 Apply CLs in local cylindrical coordinates with Fourier elements
381 Apply CBF,ELDS,UDL loads along beam axes with
BMS3 elements
385 Preserve loading assigned to deactivated elements for subsequent application on activation
LOADING
LOADING
LOADING
LOADING
17 Keep global matrix assembly incore for fast/iterative solvers
36 Follower loads (available for selected elements)
54 Updated Lagrangian geometric nonlinearity
NONLINEAR
NONLINEAR
NONLINEAR
62 Continue solution if more than one negative pivot occurs NONLINEAR
87 Total Lagrangian geometric nonlinearity NONLINEAR
138 Output yield flags only NONLINEAR
139 Output yielded, cracked or crushed integration points only for MNL
NONLINEAR
330
LUSAS User Options by Category
No. Effect of option (plus related notes where applicable)
167 Eulerian geometric nonlinearity
179 Verify arguments to usersupplied constitutive model routines
Category
157 Material Model 29 required (mandatory with noncrosssection elements)
NONLINEAR
164 Guide arclength solution with current stiffness parameter NONLINEAR
NONLINEAR
NONLINEAR
187 Include all variables in convergence norm computations
229 Corotational nonlinear geometric formulation
261 Switch for selecting root with lowest residual norm (arclength method)
273 Contact penalty stiffness update for augmented Lagrangian and slidelines
308 Arclength solution using local relative displacements
(interface elements)
NONLINEAR
NONLINEAR
NONLINEAR
NONLINEAR
NONLINEAR
340 Allow application of angular velocities with nonlinear auto incrementation
370 Strain hardening approach to modified von Mises and
Hoffman material models (77/78)
16 Continue nonlinear/eigenvalue solution when failed to converge
30 Output final node coordinates in ascending order
72 Suppress machine code inner loops
100 Output optimum frontal solution order
NONLINEAR
NONLINEAR
NONLINEAR /
EIGENVALUES
OPTIMISATION
OPTIMISATION
OPTIMISATION
170 Suppress storage of shapes OPTIMISATION
197 Fast element stiffness formulation without sparsity checks OPTIMISATION
230 Suppress stress calculation for eigenvalue analysis OPTIMISATION
26 Reduce number of lines output in coordinates
32 Suppresses stress output but not stress resultant output
33 Output direction cosines of local cartesian systems for interface
34 Output element stress resultants
39 Stress smoothing for rubber material models
40 Output nodal displacement increments for nonlinear analyses
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
42 Output nodal residual forces (nonlinear)
44 Suppress expanded input data printout except load cases
46 Suppress page skip between output stages
55 Output strains as well as stresses
59 Output local direction cosines for shells
77 Output principal stresses and directions for solids
115 Output displacements and reactions in transformed axes
116 Suppress the output of internal constraint forces
143 Output shear forces in plate bending elements.
144 Output element results for each load case separately
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
331
Appendix A LUSAS User Options
No. Effect of option (plus related notes where applicable) Category
147 Omit output phase OUTPUT
169 Suppress extrapolation of stress to nodes for semiloof shell OUTPUT
181 Harmonic response/complex mode output required in polar OUTPUT system
208 Write plot file in pre version 11.0 format (not valid for explicit dynamics)
255 Output all radiation surface view factors to FACET file.
259 Save nodal stresses in plot file to avoid stress extrapolation in Modeller
290 Write element stiffness and mass matrices to plot file
304 Plot/restart databases open until end of analysis. Speeds
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT subsequent dumps.
310 Output results to userdefined output file
320 Global matrix (and righthand side) assembly and output only
342 Always output progress information during solution
345 Separate plot file for each analysis step
348 Slideline summary output
363 Suppress echo of computed laminate properties in output file (woven fabric material)
364 Write element stiffness, mass and damping matrices to plot file
373 Extended input data diagostics for CEBFIP creep and shrinkage model
380 Output stress resultants relative to beam axes for eccentric
BTS3 elements
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
OUTPUT
389 Echo thermal link elements to output file
390 Include selected results in plot file for dataonlyprocessing
14 Compute element stresses and strains (plates/flat shells)
53 Positive definite/singularity check on modulus matrix at each Gauss point
66 Calculate element internal forces
110 Use assumed shear strain field for QTS8 thick shell
OUTPUT
OUTPUT
PROCESSING
PROCESSING
PROCESSING
PROCESSING elements
111 Don't include superelement generation load
136 Stress resultants by f=Kd and cubic interpolation
137 Stress resultants by f=Kd and equilibrium
PROCESSING
PROCESSING
PROCESSING
227 Error if a value is outside the bounds of a table of values PROCESSING
231 Error for material direction cosines not in plane of PROCESSING semiloof elements
272 Activate or deactivate elements
274 Use Uzawa rather than Powell method for node activity
PROCESSING
PROCESSING
332
LUSAS User Options by Category
No. Effect of option (plus related notes where applicable)
278 Assign six degrees of freedom to all thick shell element nodes
281 Autoloader file
Category
PROCESSING
303 Exclude incompatible modes for solid composite elements PROCESSING
318 Adaptive Analysis: Overwrite disp's with interpolated PROCESSING disp's from old mesh
346 Single segment contact from beginning of problem
347 Single segment contact from beginning of second increment
387 Redefine NSET to angle in element xyplane for use in orthotropic material properties
PROCESSING
PROCESSING
PROCESSING
PROCESSING
388 Use duplicate nodes facility for collapsed elements
394 Lamina directions supported
397 With dataonlyprocessing, compute memory requirements for solution of equations
399 Retain inactive elements in birth and death solution (old analysis type)
124 Save shape function array for restarts
PROCESSING
PROCESSING
PROCESSING
PROCESSING
RESTART
204 Use existing Plot file after restarting an analysis
184 Suppress stringent slave search for slideline problems
185 Suppress initial slideline_surface stiffness check
186 Suppress initial penetration check for slidelines
RESTART
SLIDELINES
SLIDELINES
SLIDELINES
352 Turn off consistently linearised formulation for slidelines SLIDELINES
353 Use of a fixed penalty parameter with slidelines
355 Slideline Cohesion with Coulomb friction in 2D
SLIDELINES
SLIDELINES
386 Use of weighted force/stiffness distribution with slidelines SLIDELINES
64 Nonsymmetric frontal solution
131 Parallel frontal solver algorithm
247 Extra output for iterative solvers
248 Single precision preconditioning for PCG solver
SOLVER
SOLVER
SOLVER
SOLVER
SOLVER 252 Suppress pivot warning messages from frontal solution algorithm
279 Save the reduced stiffness for further use in a linear analysis
323 Extra preconditioning for iterative solver with a hierarchical basis
344 Suppress condition number estimate in fast solvers
376 Suppress use of METIS ordering for fast solvers
377 Use minimum amount of memory for BCS solvers
SOLVER
SOLVER
SOLVER
SOLVER
SOLVER
333
Appendix A LUSAS User Options
334
Nonlinear Hardening Material Convention
Appendix B
Nonlinear
Hardening Material
Convention
Nonlinear Hardening Material Convention
(engineering stress)
2
e
2
p
2
1
e
1
p
1
E p1
y
E p2
E
y
1
2
(engineering strain)
Using the slope of the uniaxial yield stress against equivalent plastic strain:
335
Appendix B Nonlinear Hardening Material Convention
C
HG
F
1
E p
E p
E
KJ
I we have:
E p 1
1
y
1
y
and
E p2
2
2
1
1 where:
y
y
E
1
e
1
p
1
2
e
2
p
2 which may be substituted into the top equation to give the corresponding C values for each section:
C
HG
F
1
E p
E p
E
KJ
I
(Ep < E)
Now the strain values required by LUSAS are the
1 p
,
2 p
, etc. The limit on the equivalent plastic strain up to which the hardening curve is valid are, thus:
L
1
1
e
1
1
1
E
and
L
2
2
e
2
2
2
E
The converted curve for LUSAS use would, therefore, be as follows:
336
Stress
2
1
y
C
1
Nonlinear Hardening Material Convention
C
2
L
1
L
2
Equivalent plastic strain
337
Solver User Interface Routines
Appendix C Material
Model Interface
Solver User Interface Routines
A number of interface facilities are available within the LUSAS Solver. Since the specification of these facilities requires both external development of FORTRAN source code and access to the Solver object libraries, these facilities are aimed at the advanced user.
The object libraries and userinterface routines needed for external code development are provided in the LUSAS MMI kit. The kit also includes workspace and project files that allow the development of external code in a visual environment on a PC, and which enable the compilation and linking of that code into Lusas Solver. Please contact your local distributor for further details.
User Defined Constitutive Models
For continuum based models the user is required to define three subroutines in
FORTRAN to carry out the following tasks:
USRKDM defines the modulus matrix.
USRSTR defines the current stress and material state and state variables.
USRSVB outputs evaluated nonlinear state variables.
For resultant based models the user is required to define the following subroutines:
USRRDM defines the modulus matrix.
USRRST defines the current stress and material state and state variables.
USRSVB outputs evaluated nonlinear state variables.
See Material Properties Nonlinear User and Material Properties Nonlinear Resultant
User for data syntax details.
User Defined Creep Models
This facility allows the specification of a creep law for a particular material if the creep models available in LUSAS Solver are inappropriate. The usersupplied subroutine
339
Appendix C Material Model Interface
USRCRP allows specification of creep laws that are a function of stress, strain and temperature history.
See Creep Properties User for data syntax details.
User Defined Damage Models
The usersupplied damage subroutine USRDAM permits external computation of the damage variable and its derivative with respect to the current elastic complementary energy norm.
See Damage Properties User for data syntax details.
User Defined Viscoelastic Models
This facility permits an externally developed viscoelastic material model to be used within Lusas. The usersupplied viscoelastic subroutine USRDMV is used to compute the viscoelastic contribution to the modulus matrix.
See Visco Elastic Properties User for data syntax details.
User Defined Friction Models
The usersupplied subroutine USRSLF permits a nonlinear friction law to be utilised in a slideline analysis. The friction law may be a function of the surface temperatures, the relative velocities and/or accelerations of adjacent surfaces and a set of userdefined friction parameters.
See Slideline Properties User for data syntax details.
User Defined Rate of Internal Heat Generation
The usersupplied subroutine USRRHG permits the way in which internal heat is generated in a thermal analysis to be defined. This can be defined to be a function of temperature, time and chemical reaction. The parameters used to control the chemical reaction are specified under the RIHG USER data chapter. In a thermomechanical coupled analysis, variables defining the degree and rate of chemical reaction (or cure) may be transferred to the structural analysis where they can be accessed in the user interface routines USRKDM and USRSTR. The modulus matrix and stress computations may then become a function of degree or rate of cure.
See RIHG User for data syntax details.
340
Programming Rules
Software Required
A compatible FORTRAN compiler is required to include userdefined subroutines. Call your LUSAS distributor for details.
Programming Rules
Modification of External Arguments
It is important that only those arguments indicated in the userprogrammable routines are modified. All other arguments may be manipulated as required, but must remain unchanged.
Although LUSAS contains a large number of system error traps, specifically designed to detect internally corrupted variables and artificially terminate the analysis procedure in a controlled manner, this process cannot generally be guaranteed. Hence, illegal modification of arguments may lead to unpredictable analysis termination or corrupt solutions. LUSAS can accept no responsibility in such circumstances.
For the same reason it is important that the DIMENSION, CHARACTER and
LOGICAL declarations within the userprogrammable subroutines are not modified or deleted. Only code between the lines indicated may be modified externally. These subroutines are described in detail in the following chapters.
Verification
The incoming and outgoing arguments to the userprogrammable subroutines may be verified via lower level subroutines that are also provided. Access to the verification subroutines is activated by specification of Option 179 in the analysis data file. The arguments to these routines should not be altered.
The logical variable FEA is for LUSAS/FEA use only. These verification routines are described in detail in the following chapters.
External Error Diagnosis
The logical error flag (ERROR) is initialised to .FALSE., and may be used to detect a fatal error within the externally supplied FORTRAN code. On exit from the userprogrammable subroutines detection of ERROR=.TRUE. will activate a controlled termination of the analysis procedure.
341
Appendix C Material Model Interface
Argument Definition Codes
In the descriptions of all subroutines in the sections that follow, abbreviations are used to differentiate between variables and arrays for integer, real logical and character variables. These definitions are shown in the table right.
Code Variable type Code Array type
IV integer variable IA integer array
RV real variable RA real array
LV logical variable LA logical array
CV character variable
CA character array
Declaration
FEA Ltd can accept no responsibility whatsoever for any analysis or programming results obtained through use of the userprogrammable
CONSTITUTIVE MODELS, CREEP, DAMAGE, NONLINEAR FRICTION or
MODELLER RESULTS. Whilst FEA Ltd can validate that the arguments are passed correctly through the interfaces to the userprogrammable subroutines,
FEA Ltd cannot be held responsible for any programming or alterations carried out by the user within these routines.
FEA Ltd cannot guarantee that the interfaces to the abovenamed user routines will continue to remain in the form described in this manual.
342
User Defined Constitutive Models
User Defined Constitutive Models
Continuum models
All constitutive models defined under MATERIAL PROPERTIES NONLINEAR
USER utilise continuum stresses and strains and the user defined routines interface with code at the material integration point level. For continuum based elements (for example, bars, 2D and 3D continuum) this is within a Gauss point loop. For resultant based elements (for example semiloof beams and shells) this is at a fibre or layer sampling position within the Gauss point loop.
The constitutive relationship is assumed to be of the form: l q
D l q where l q
are the increments of continuum stress, l q
are the increments of continuum strain and
D
is the constitutive or modulus matrix. The modulus matrix is explicitly defined by the user via the externally developed FORTRAN subroutine,
USRKDM, and is of the form:
D
L
MM
MM
N
D
D
11
D
21 ndse , 1
D
D
12
D
22 ndse ,2
D
13
D
23
D ndse ,3
D
D
1 , ndse
D
2 , ndse
PP
Q
PP
O where ndse is the number of continuum stresses or strains at a material sampling point.
The number of continuum stresses or strains at a point is related to the LUSAS model number mdl, and is a constant for each element type.
343
Appendix C Material Model Interface
The continuum stress and strain components, and their associated model number (mdl) are tabulated for each applicable LUSAS element group below:
mdl Model type
1 Uniaxial
2 Plane stress
2 Semiloof shell
3 Plane strain
(approximate)
4 Axisymmetric
5 3D beams
6 Solids
Components
xx xx, yy, xy xx, yy, xy xx, yy, xy xx, yy, xy, zz xx, xy, xz xx, yy, zz, xy, yz, zx xx, xy, xz, yz xx, yy
7 3D semiloof beams
8 Axisymmetric sheet and shell
9 Axisymmetric thick shell
10 Thick plane beam
11 Plane strain
12 Thick shells
User Material Properties Input
xx, xy, zz xx, xy xx, yy, xy, zz xx, yy, xy, yz, zx
ndse
1
3
3
3
2
4
5
4
3
6
4
2
3
The user material properties are input in a similar manner as the other LUSAS material types.
The user material input consists of a total of nprz material parameters, the first 15 of which are specifically for LUSAS use. These 15 properties are required should the user wish to utilise some of the other LUSAS analysis types (e.g. thermal or dynamic analyses) for which material parameters are required. The temperature is specified should the user wish to use temperature dependent properties. Material properties 16 to
nprz must be supplied by the user in the order required by the usersupplied routines. It should be noted however, that all nprz properties can be used within the user routines.
These properties, relating to the current temperature, are stored in the array ELPR.
Values for the complete table of reference temperatures are stored in array ELPRT.
344
User Defined Constitutive Models
The 15 specific properties are:
1
Young‟s modulus (E)
2
Poisson's ratio (
)
3
Mass density (
)
49 Coefficients of thermal expansion (
x
y
z
xy
yz
xz
)
10
Mass Rayleigh damping parameter (a r
)
11
Stiffness Rayleigh damping parameter (b r
)
12
Heat fraction (h f
)
13
Reference temperature (T)
14
Angle of anisotropy (
) measured in degrees relative to the reference axes (with Option 207 set), or the Cartesian set number (nset) defining the local reference axes.
15
Not used at present.
Together with the user material properties the user also needs to specify the following integer numbers for the specific material defined:
lptusr a number which identifies the particular user material model.
nprz the total number of material properties used.
nstat the number of nonlinear state variables that are used in the material model
(these variables will be output together with the Gauss point stresses/strains). The value of nstat must not be less than 1.
The numbers are specified on the data input line for the user material model as follows:
MATERIAL PROPERTIES NONLINEAR USER lptuser nprz nstat
See the UserSupplied Nonlinear Material Properties section for more details.
Evaluation of the Modulus Matrix
The modulus matrix
D
is explicitly defined via the externally supplied FORTRAN subroutine USRKDM. The routine is called at the material integration point level, from both the LUSAS Solver presolution and postsolution analysis modules. On entry to
USRKDM, the modulus matrix
D
is fully initialised (each array component set to floating point real zeros). Hence, only the nonzero components of the modulus matrix need be evaluated. The returned modulus matrix must be symmetrical about the leading diagonal.
345
Appendix C Material Model Interface
Nonlinear Stress Recovery
The stress recovery algorithm is defined explicitly via the externally supplied
FORTRAN subroutine USRSTR, and is concerned with the evaluation of:
Stress State the current stress state,
Material State the current material state (as indicated by the nonlinear state variables),
Nonlinear Variables additional associated nonlinear variables.
The routine is called at the material integration point level, from the LUSAS Solver postsolution analysis module. Stresses, strains and nonlinear state variables are available as current values, values at the end of the previous iteration, and values at the start of the current increment.
The procedure for updating incremental and iterative variables from the evaluated current values is automatically performed by LUSAS Solver. Consequently, modifications should be restricted to current values only.
Stress/Strain Formulation
For the Eulerian formulation and GreenNaghdi rate formulation, the stress components have been rotated to the initial configuration using the rotation matrix evaluated using polar decomposition. The stress rotation matrix is therefore that of the current configuration.
For the Jaumann rate formulation, the stress components at time t have been rotated to the current configuration. The stress rotation matrix is then the incremental spin matrix.
In addition, no total strain is evaluated for the Jaumann rate.
Nonlinear State Variable Output
The output of the evaluated nonlinear state variables is controlled via the externally supplied FORTRAN subroutine, USRSVB. The routine is called at the material integration point level, from the LUSAS Solver output analysis module.
Default nonlinear state variable output for user supplied constitutive models is of the form shown below (6 variables to a line, to a total of nstat values. Nonlinear state variables for usersupplied models are output by default and are not subject to LUSAS
Solver Options 138 and 139.
NL STATE VARIABLES 0.0000E+00 0.0000E+00 0.0000E+00
(contd.)
0.0000E+00 0.0000E+00 0.0000E+00
346
User Defined Constitutive Models
The output of stresses, and optionally strains, follows the normal pattern for the particular element type, i.e. it is subject to the usual LUSAS frequency and location controls. All output must be written to the recognised LUSAS output channel defined by integer NT6.
Verification
Three routines USRVF1, USRVF2 and USRVF3 are supplied to enable the user to verify the incoming and outgoing arguments to the userprogrammed subroutines
USRKDM, USRSTR and USRSVB respectively. These subroutines may be utilised by the user but no alterations are permitted.
SUBROUTINE USRKDM
Purpose
Explicit definition of the modulus matrix D for userdefined material. This routine may be programmed by the user but the argument list must not be altered in any way.
Note. For static nonlinear analysis failure to code this routine will result in slower convergence. For transient dynamic analysis however it is important that this routine defines the nonlinear modulus matrix as failure to do so may result in incorrect results.
SUBROUTINE USRKDM
A( LPTUSR ,MDL ,NAXES ,NDSE ,NEL ,
B NG ,NPRZ ,NSTAT ,NT6 ,NTAB ,
C NACTVE ,DINT ,DT ,TEMPC ,RSPTM ,
D DOCT ,DOCC ,RDOC ,TEMPR ,VERIF ,
E NWINC ,REPAS ,ERROR ,INIACT ,FEA ,
F ELPR ,EPST ,EPSC ,STVBT ,STVBC ,
G STRST ,STRSC ,XYZ ,D ,ELPRT ,
H DRCMGP )
DIMENSION
A ELPR(NPRZ) ,EPST(NDSE) ,EPSC(NDSE) ,
B STVBT(NSTAT) ,STVBC(NSTAT) ,STRST(NDSE) ,
C STRSC(NDSE) ,XYZ(NAXES) ,D(NDSE,NDSE) ,
D ELPRT(NPRZ,NTAB),DRCMGP(NAXES,NAXES)
Name
LPTUSR
MDL
Argument Description
User supplied constitutive model reference number
LUSAS reference code for stress model type
347
Type
IV
IV
Modify


Appendix C Material Model Interface
Name
NAXES
NDSE
NEL
NG
NPRZ
NSTAT
NT6
NTAB
NACTVE
DINT
DT
TEMPC
RSPTM
DOCT
DOCC
RDOC
TEMPR
VERIF
NWINC
REPAS
ERROR
INIACT
FEA
ELPR
EPST
EPSC
Argument Description
Number of system axes (dimensions)
Number of continuum stress components at a Gauss point for the stress model type MDL
Current element number
Current Gauss point number
Number of material parameters for the constitutive model
Number of state dependent variables
Type
IV
IV
IV
IV
IV
LUSAS results output channel
Number of temperature dependent property tables
Element activation status
0Standard element 1activating 2deactivated
Characteristic length or area of the current Gauss point
Current time step increment (dynamic analysis)
Current temperature
Current total response time (dynamic analysis)
Degree of cure at the start of the current increment
(thermomechanical coupled analysis via user defined interface USRRHG)
Current degree of cure (thermomechanical coupled analysis via user defined interface USRRHG)
Current rate of cure (thermomechanical coupled analysis via user defined interface USRRHG)
Reference or initial temperature
RV
RV
RV
RV
Logical incoming/outgoing argument verification flag LV
Logical flag, TRUE denoting the start of a new increment
LV
Logical flag, TRUE denoting a repass
Logical flag for fatal error and program termination
LV
LV
RV
RV
RV
RV
IV
IV
IV
IV
Logical flag for initial activation of element
Logical flag for FEA use only
Material properties for current element (evaluated at the current temperature)
Total strain components at the start of the current increment
Current total strain components
LV
LV
RA
RA
RA
348






 yes










Modify


User Defined Constitutive Models
Name
STVBT
STVBC
STRST
STRSC
XYZ
Argument Description
State variables at the start of the current increment
Current state variables
Stress components at the start of the current increment
Current stress components
Coordinates for the current Gauss point
D
ELPRT
Modulus matrix (Dmatrix)
Table of temperature dependent material properties
DRCMGP Direction cosine matrix for the material
RA
RA
RA
RA
RA
Type
RA
RA
RA

 yes


Modify



SUBROUTINE USRSTR
Purpose
Stress recovery algorithm for userdefined material. This subroutine may be programmed by the user but the argument list may not be altered in any way.
Note. For a static nonlinear analysis, failure to code routine USRKDM will result in slower convergence. For a transient dynamic analysis, however, it is important that the routine USRKDM defines the nonlinear modulus matrix as failure to do so may result in incorrect results.
SUBROUTINE USRSTR
A( IMAT ,LPTUSR ,MDL ,NAXES ,NDSE ,
B NEL ,NG ,NPRZ ,NSTAT ,NT6 ,
C NTAB ,DINT ,DISEN ,DT ,STREN ,
D TEMPC ,RSPTM ,VIHG ,DOCT ,DOCC ,
E RDOC ,VERIF ,STHLV ,REPAS ,ERROR ,
F BOUNDS ,NWINC ,INIACT ,FEA ,
G ELPR ,EPST ,EPSI ,EPSC ,STVBT ,
H STVBI ,STVBC ,STRST ,STRSI ,STRSC ,
I XYZ ,D ,ELPRT ,ROTAC ,ROTAT ,
J DRCMGP )
DIMENSION
A ELPR(NPRZ) ,EPST(NDSE) ,EPSI(NDSE) ,
B EPSC(NDSE) ,STVBT(NSTAT) ,STVBI(NSTAT) ,
349
Appendix C Material Model Interface
C STVBC(NSTAT) ,STRST(NDSE) ,STRSI(NDSE) ,
D STRSC(NDSE) ,XYZ(NAXES) ,D(NDSE,NDSE) ,
E ELPRT(NPRZ,NTAB) ,ROTAC(NAXES,NAXES) ,
F ROTAT(NAXES,NAXES) ,DRCMGP(NAXES,NAXES)
NSTAT
NT6
NTAB
DINT
DISEN
DT
STREN
TEMPC
RSPTM
VIHG
DOCT
Name
IMAT
LPTUSR
MDL
NAXES
NDSE
NEL
NG
NPRZ
DOCC
RDOC
Argument Description
Material assignment reference number
User supplied constitutive model reference number
LUSAS reference code for stress model type
Number of system axes (dimensions)
Number of continuum stress components at a
Gauss point for the stress model type MDL
Type
IV
IV
IV
IV
IV
Current element number
Current Gauss point number
Number of material parameters for the constitutive model
IV
IV
IV
Number of state dependent variables
LUSAS results output channel
IV
IV
Number of temperature dependent property tables IV
RV Characteristic length or area of the current Gauss point
Energy dissipated by inelastic processes
Current time step increment (dynamic analysis)
Increment of elastic strain energy
Current temperature
Current total response time (dynamic analysis)
RV
RV
RV
RV
RV
RV Volumetric internal heat generation due to mechanical work
Degree of cure at the start of the current increment (thermomechanical coupled analysis via user defined interface USRRHG)
Current degree of cure (thermomechanical coupled analysis via user defined interface
USRRHG)
Current rate of cure (thermomechanical coupled analysis via user defined interface USRRHG)
RV
RV
RV yes
 yes

 yes










Modify


350
User Defined Constitutive Models
EPST
EPSI
EPSC
STVBT
STVBI
STVBC
STRST
STRSI
STRSC
XYZ
D
ELPRT
ROTAC
ROTAT
DRCMGP
Name
VERIF
STHLV
REPAS
ERROR
BOUNDS
NWINC
INIACT
FEA
ELPR
Argument Description
Logical incoming/outgoing argument verification flag
Logical increment step halving flag
Type
LV
Material properties for current element (evaluated at the current temperature
LV
Logical flag for repass through subroutine
Logical flag for fatal error and program termination
LV
LV
Flag to error if temperature out of bounds of table LV
Logical flag, TRUE denoting the start of a new increment
LV
Logical flag for initial activation of element
Logical flag for FEA use only
LV
LV
RA
Total strain components at the start of current increment
Total strain components at the end of the previous iteration
Current total strain components
Stress components at the start of the current increment
Stress components at the end of the previous iteration
RA
RA
State variables at the start of the current increment
RA
RA
State variables at the end of the previous iteration RA
On entry: State variables at start of the current increment, on exit: Current state variables
RA
RA
RA
RA On entry: Stress components at start of current increment. On exit: Current stress components
Coordinates of the current Gauss point
Modulus matrix (Dmatrix)
Table of temperature dependent material properties
RA
RA
RA
Stress rotation matrix (current)
Stress rotation matrix (at time t)
RA
RA
Direction cosine matrix for the material RA


 yes
 yes







 yes



Modify
 yes
 yes
351
Appendix C Material Model Interface
SUBROUTINE USRSVB
Purpose
Output of nonlinear state variables for userdefined material. This subroutine may be programmed by the user but the argument list must not be altered in any way.
SUBROUTINE USRSVB
A( LPTUSR ,NSTAT ,NDSE ,NT6 ,VERIF ,
B ERROR ,FEA ,
C STVBC )
DIMENSION
A STVBC(NSTAT)
Name
LPTUSR
NSTAT
NDSE
Argument Description Type Modif y



NT6
VERIF
ERROR
FEA
STVBC
User supplied constitutive model reference number
Number of state dependent variables
Number of continuum stress components at a Gauss point for the stress model type MDL
LUSAS results output channel
Logical incoming/outgoing argument verification flag
IV
IV
IV
IV
LV
Logical flag for fatal error and program termination LV
Logical flag for FEA use only LV
Current state variables for constitutive model RA

 yes


SUBROUTINE USRVF1
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutine
USRKDM. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVF1
A( LPTUSR ,MDL ,NAXES ,NDSE ,NEL ,
B NG ,NPRZ ,NSTAT ,NT6 ,NTAB ,
C NACTVE ,DINT ,DT ,TEMPC ,RSPTM ,
D DOCT ,DOCC ,RDOC ,TEMPR ,VERIF ,
E NWINC ,REPAS ,ERROR ,INIACT ,FEA ,
352
User Defined Constitutive Models
F ARGIN ,
G ELPR ,EPST ,EPSC ,STVBT ,STVBC ,
H STRST ,STRSC ,XYZ ,D ,ELPRT ,
I DRCMGP )
DIMENSION
A ELPR(NPRZ) ,EPST(NDSE) ,EPSC(NDSE) ,
B STVBT(NSTAT) ,STVBC(NSTAT) ,STRST(NDSE) ,
C STRSC(NDSE) ,XYZ(NAXES) ,D(NDSE,NDSE) ,
D ELPRT(NPRZ,NTAB),DRCMGP(NAXES,NAXES)
The argument list is the same as that for subroutine USRKDM, except for one argument. The additional argument is the logical variable ARGIN (see continuation line F in the above subroutine statement) that is used in this subroutine. If
ARGIN=.TRUE. verification of incoming arguments will be carried out and if
ARGIN=.FALSE. verification of outgoing arguments will take place.
SUBROUTINE USRVF2
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutine
USRSTR. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVF2
A( IMAT ,LPTUSR ,MDL ,NAXES ,NDSE ,
B NEL ,NG ,NPRZ ,NSTAT ,NT6 ,
C NTAB ,DINT ,DISEN ,DT ,STREN ,
D TEMPC ,RSPTM ,VIHG ,DOCT ,DOCC ,
E RDOC ,VERIF ,STHLV ,REPAS ,ERROR ,
F BOUNDS ,NWINC ,INIACT ,FEA ,ARGIN ,
G ELPR ,EPST ,EPSI ,EPSC ,STVBT ,
H STVBI ,STVBC ,STRST ,STRSI ,STRSC ,
I XYZ ,D ,ELPRT ,ROTAC ,ROTAT ,
J DRCMGP )
DIMENSION
A ELPR(NPRZ) ,EPST(NDSE) ,EPSI(NDSE) ,
B EPSC(NDSE) ,STVBT(NSTAT) ,STVBI(NSTAT) ,
C STVBC(NSTAT) ,STRST(NDSE) ,STRSI(NDSE) ,
D STRSC(NDSE) ,XYZ(NAXES) ,D(NDSE,NDSE) ,
353
Appendix C Material Model Interface
E ELPRT(NPRZ,NTAB) ,ROTAC(NAXES,NAXES) ,
F ROTAT(NAXES,NAXES) ,DRCMGP(NAXES,NAXES)
The argument list is the same as that for subroutine USRSTR, except for one argument.
The additional argument is the logical variable ARGIN (see continuation line F in the above subroutine statement) that is used in this subroutine. If ARGIN=.TRUE. verification of incoming arguments will be carried out and if ARGIN=.FALSE. verification of outgoing arguments will take place.
SUBROUTINE USRVF3
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutine
USRSVB. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVF3
A( LPTUSR ,NSTAT ,NDSE ,NT6 ,VERIF ,
B ERROR ,FEA ,ARGIN ,
C STVBC )
DIMENSION
A STVBC(NSTAT)
The argument list is the same as that for subroutine USRSVB, except for one argument.
The additional argument is the logical variable ARGIN (see continuation line B in the above subroutine statement) that is used in this subroutine. If ARGIN=.TRUE. verification of incoming arguments will be carried out and if ARGIN=.FALSE. verification of outgoing arguments will take place.
User Defined Resultant Models
Resultant Models
All constitutive models defined under MATERIAL PROPERTIES NONLINEAR
RESULTANT USER utilise stress resultants and strains/curvatures. The user defined routines interface with code at the element gauss point level. This facility may be used with 2D and 3D beam elements which have a nonlinear capability, namely BM3,
BMX3,BTS3, BSL3/4, BXL4, BS3/4 and BSX4
The constitutive relationship is assumed to be of the form: where l q l q
D l q
are the increments of stress resultants,
are the increments of strains and curvatures and
D
is the constitutive or modulus matrix. The modulus matrix is
354
User Defined Resultant Models
explicitly defined by the user via the externally developed FORTRAN subroutine,
USRRDM, and is of the form:
D
L
MM
MM
N
D
D
11
D
21 ndse , 1
D
D
12
D
22 ndse ,2
D
13
D
23
D ndse ,3
D
D
1 , ndse
D
2 , ndse
PP
Q
PP
O where ndse is the number of stress resultants or strains and curvatures at an element gauss point. The number of stress resultants at a point can be ascertained from the
LUSAS element type number nelt.
The stress resultant and strain components, and their associated element type number
(nelt) are tabulated for each applicable LUSAS beam element below:
nelt
54,43
205
97,170,171
98,176,177
Element name
BM3,BMX3
BTS3
BS3,BS4,BSX4
BSL3,BSL4,BXL4
Stress resultants
Fx,Mz
Fx,Fy,Fz,Mx,My,Mz
Fx,My,Mz,Txz,Txy,Fy
Fx,My,Mz,Txz,Txy,Fy
ndse
2
6
6
6
Resultant User Material Properties Input
The user material properties are input in a similar manner to the other LUSAS material types.
The resultant user material input consists of a total of nprz material parameters, the first 10 of which are specifically for LUSAS use. These 10 properties are required should the user wish to utilise some of the other LUSAS analysis types (e.g. thermal or dynamic analyses) for which material parameters are required. The temperature is specified should the user wish to use temperature dependent properties. Material properties 11 to nprz must be supplied by the user in the order required by the usersupplied routines. It should be noted however, that all nprz properties can be used within the user routines. These properties, relating to the current temperature, are stored in the array ELPR. Values for the complete table of reference temperatures are stored in array ELPRT.
355
Appendix C Material Model Interface
The 10 specific properties are:
1
Young‟s modulus (E)
2
Poisson's ratio (
)
3
Mass density (
)
4
Coefficients of thermal expansion (
5
Mass Rayleigh damping parameter (ar)
6
Stiffness Rayleigh damping parameter (br)
7
Not used at present
8
Reference temperature (T)
9
Not used at present
10 Not used at present.
Together with the user material properties the user also needs to specify the following integer numbers for the specific material defined:
lptusr a number which identifies the particular user material model.
nprz the total number of material properties used.
ndcrve the number of material data curves defined. This allows the user to input a table of values that vary with reference to something other than temperature. For example, a table of momentcurvature profiles may be defined where each profile relates to a particular axial force in the element.
nstat the number of nonlinear state variables that are used in the material model
(these variables will be output together with the Gauss point stresses/strains). The value of nstat must not be less than 1.
The numbers are specified on the data input line for the user material model as follows:
MATERIAL PROPERTIES NONLINEAR RESULTANT USER lptuser nprz ndcrve nstat
See the UserSupplied Nonlinear Material Properties section for more details.
Evaluation of the Modulus Matrix
The modulus matrix
D
is explicitly defined via the externally supplied FORTRAN subroutine USRRDM. The routine is called at the element gauss point level, from both the LUSAS Solver presolution and postsolution analysis modules. On entry to
USRRDM, the modulus matrix
D
is fully initialised (each array component is set to a floating point real zero). Hence, only the nonzero components of the modulus matrix
356
User Defined Resultant Models
need be evaluated. The returned modulus matrix must be symmetrical about the leading diagonal.
Nonlinear Stress Recovery
The stress recovery algorithm is defined explicitly via the externally supplied
FORTRAN subroutine USRRST, and is concerned with the evaluation of:
Stress State the current stress state,
Material State the current material state (as indicated by the nonlinear state variables),
Nonlinear Variables additional associated nonlinear variables.
The routine is called at the element gauss point level, from the LUSAS Solver postsolution analysis module. Stress resultants, strains and curvatures, and nonlinear state variables are available as current values, values at the end of the previous iteration, and values at the start of the current increment.
The procedure for updating incremental, and iterative variables from the evaluated current values, is automatically performed by LUSAS Solver. Consequently, modifications should be restricted to current values only.
Nonlinear State Variable Output
The output of the evaluated nonlinear state variables is controlled via the externally supplied FORTRAN subroutine, USRSVB. The routine is called at the element gauss point level from the LUSAS output analysis module.
Default nonlinear state variable output for user supplied constitutive models is of the form shown below (6 variables to a line, to a total of nstat values). Nonlinear state variables for usersupplied models are output by default and are not subject to LUSAS
Solver Options 138 and 139.
NL STATE VARIABLES 0.0000E+00 0.0000E+00 0.0000E+00
(contd.)
0.0000E+00 0.0000E+00 0.0000E+00
The output of stress resultants, and optionally strains and curvatures, follows the normal pattern for the particular element type, i.e. it is subject to the usual LUSAS frequency and location controls. All output must be written to the recognised LUSAS output channel defined by integer NT6.
Verification
Two routines USRVF4 and USRVF3 are supplied to enable the user to verify the incoming and outgoing arguments to the userprogrammed subroutines USRRDM and
USRRST, and USRSVB respectively. This subroutine may be utilised by the user but no alterations are permitted.
357
Appendix C Material Model Interface
SUBROUTINE USRRDM
Purpose
Explicit definition of the modulus matrix D for userdefined material. This routine may be programmed by the user but the argument list must not be altered in any way.
SUBROUTINE USRRDM
A( NEL ,NELT ,NDSE ,NGP ,NG ,
B LPTUSR ,NDCRVE ,NPRZ ,NTAB ,NLGPR ,
C NSTAT ,NT6 ,IMAT ,INC ,ELEN ,
D DLENTH ,DT ,TEMPC ,RSPTM ,ELTAGE ,
E ACTIM ,VERIF ,NWINC ,REPAS ,ERROR ,
F FEA ,BOUNDS ,
G ELGPR ,ELPR ,EPST ,EPSC ,STRST ,
H STRSC ,STVBT ,STVBC ,PLSPRP ,STRSI ,
I STRSR ,EPSTH ,EPSI ,DUMMY ,ELPRT ,
J SHRNKT ,SHRNKC ,D )
DIMENSION
A ELGPR(NLGPR) ,ELPR(NPRZ) ,EPST(NDSE) ,
B EPSC(NDSE) ,STRST(NDSE) ,STRSC(NDSE) ,
C STVBT(NSTAT) ,STVBC(NSTAT) ,PLSPRP(NDSE) ,
D STRSI(NDSE) ,STRSR(NDSE) ,EPSTH(NDSE) ,
E EPSI(NDSE) ,DUMMY(NDSE) ,ELPRT(NPRZ,NTAB),
F SHRNKT(NDSE) ,SHRNKC(NDSE) ,D(NDSE,NDSE)
Name
NEL
NELT
NDSE
NGP
NG
LPTUSR
NDCRVE
NPRZ
NTAB
NLGPR
Argument Description
Current element number
Element type number
Number of stress components at a Gauss point
Number of gauss points
Current Gauss point number IV
User supplied constitutive model reference number IV
Number of material data curves defined
Number of material parameters for each material
IV
IV
Number of lines in a table of material properties
Number of element geometric properties
IV
IV
Type
IV
IV
IV
IV









Modify

358
User Defined Resultant Models
Name
NSTAT
NT6
IMAT
Argument Description
Number of state dependent model variables
LUSAS results output channel
Material assignment number
INC
ELEN
Load increment number
Element length
DLENGTH Characteristic length of the current Gauss point
DT Current time step increment (dynamic analysis)
TEMPC
RSPTM
ELTAGE
ACTIM
VERIF
Current temperature
Current total response time (dynamic analysis)
Age of an element at activation
NWINC
REPAS
ERROR
FEA
BOUNDS
ELGPR
ELPR
EPST
EPSC
STRST
STRSC
STVBT
STVBC
PLSPRP
STRSI
STRSR
IV
RV
RV
RV
RV
RV
RV
Time of element activation
Logical incoming/outgoing argument verification flag
Logical flag, TRUE denoting the start of a new increment
Logical flag, TRUE denoting a repass
RV
LV
LV
LV
Logical flag for fatal error and program termination LV
Logical flag denoting FEA or external code use
(FOR FEA INTERNAL USE ONLY)
Flag to error if a value is outside the bounds of a table of values (OPTION 227)
LV
LV
Element geometric properties
Material properties for current element
(evaluated at the current temperature)
Total strain components at the start of the current increment
RA
RA
RA
Current total strain components
Stress resultant components at the start of the current increment
Stress resultant components
State variables at the start of current increment
Current state variables
Vector of plastic geometric properties (defined using OPTION 157)
Initial stresses (these have already been added to the incoming STRSC/STRST values)
Residual stresses (these have already been added to the incoming STRSC/STRST values)
RA
RA
RA
RA
RA
RA
RA
RA
Type
IV
IV
IV
359











 yes









Modify




Appendix C Material Model Interface
Name
EPSTH
EPSI
DUMMY
ELPRT
SHRNKT
SHRNKC
D
Argument Description
Total thermal strains
Initial strains
Unused vector
Table of temperature dependent material properties RA
Shrinkage strain vector at start of current increment RA
Current shrinkage strain vector
Modulus matrix (Dmatrix)
RA
RA
Type
RA
RA
RA
 yes
Modify



SUBROUTINE USRRST
Purpose
Stress recovery algorithm for userdefined material. This subroutine may be programmed by the user but the argument list may not be altered in any way.
SUBROUTINE USRRST
A( NEL ,NELT ,NDSE ,NGP ,NG ,
B LPTUSR ,NDCRVE ,NPRZ ,NTAB ,NLGPR ,
C NSTAT ,NT6 ,IMAT ,INC ,ELEN ,
D DLENTH ,DT ,TEMPC ,RSPTM ,ELTAGE ,
E ACTIM ,VERIF ,NWINC ,REPAS ,ERROR ,
F FEA ,BOUNDS ,
G ELGPR ,ELPR ,EPST ,EPSC ,STRST ,
H STRSC ,STVBT ,STVBC ,PLSPRP ,STRSI ,
I STRSR ,EPSTH ,EPSI ,DEPS ,ELPRT ,
J SHRNKT ,SHRNKC ,D )
DIMENSION
A ELGPR(NLGPR) ,ELPR(NPRZ) ,EPST(NDSE) ,
B EPSC(NDSE) ,STRST(NDSE) ,STRSC(NDSE) ,
C STVBT(NSTAT) ,STVBC(NSTAT) ,PLSPRP(NDSE) ,
D STRSI(NDSE) ,STRSR(NDSE) ,EPSTH(NDSE) ,
E EPSI(NDSE) ,DEPS(NDSE) ,ELPRT(NPRZ,NTAB),
F SHRNKT(NDSE) ,SHRNKC(NDSE) ,D(NDSE,NDSE)
360
User Defined Resultant Models
Name
NEL
NELT
NDSE
NGP
NG
LPTUSR
NDCRVE
NPRZ
NTAB
NLGPR
Argument Description
Current element number
Element type number
Number of stress components at a Gauss point
Number of gauss points
Current Gauss point number
User supplied constitutive model reference number
Number of material data curves defined
Number of material parameters for each material
Number of lines in a table of material properties
Number of element geometric properties
NSTAT
NT6
IMAT
Number of state dependent model variables
LUSAS results output channel
Material assignment number
INC
ELEN
Load increment number
Element length
DLENGTH Characteristic length of the current Gauss point
DT Current time step increment (dynamic analysis)
TEMPC
RSPTM
ELTAGE
ACTIM
VERIF
NWINC
Current temperature
Current total response time (dynamic analysis)
Age of an element at activation
Time of element activation
REPAS
ERROR
FEA
BOUNDS
ELGPR
ELPR
EPST
EPSC
Logical incoming/outgoing argument verification flag LV
Logical flag, TRUE denoting the start of a new increment
LV
Logical flag, TRUE denoting a repass LV
LV Logical flag for fatal error and program termination
Logical flag denoting FEA or external code use
(FOR FEA INTERNAL USE ONLY)
Flag to error if a value is outside the bounds of a table of values (OPTION 227)
Element geometric properties
Material properties for current element
(evaluated at the current temperature)
Total strain components at the start of the current increment
LV
LV
RA
RA
RA
Current total strain components RA
RV
RV
RV
RV
IV
IV
IV
IV
RV
RV
RV
IV
IV
IV
IV
IV
IV
IV
Type
IV
IV
IV


















Modify








 yes

361
Appendix C Material Model Interface
Name
STRST
STRSC
STVBT
STVBC
Argument Description
Stress resultant components at the start of the current increment
On entry: Stress resultant components at start of current increment. On exit: Current stress resultant components
State variables at the start of current increment
On entry: State variables at start of the current increment, on exit: Current state variables
Vector of plastic geometric properties (defined using OPTION 157)
Initial stresses (these have already been added to the incoming STRSC/STRST values)
Residual stresses (these have already been added to the incoming STRSC/STRST values)
Total thermal strains
Initial strains
Incremental strains after deduction of initial and thermal strains
Table of temperature dependent material properties
Shrinkage strain vector at start of current increment
Current shrinkage strain vector
Modulus matrix (Dmatrix)
Type
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
Modify
 yes
 yes
PLSPRP
STRSI
STRSR
EPSTH
EPSI
DEPS
ELPRT
SHRNKT
SHRNKC
D
SUBROUTINE USRVF4
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutines
USRRDM and USRRST. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVF4
A( NEL ,NELT ,NDSE ,NGP ,NG ,
B LPTUSR ,NDCRVE ,NPRZ ,NTAB ,NLGPR ,
C NSTAT ,NT6 ,IMAT ,INC ,ELEN ,
D DLENTH ,DT ,TEMPC ,RSPTM ,ELTAGE ,
E ACTIM ,VERIF ,NWINC ,REPAS ,ERROR ,
F FEA ,BOUNDS ,ARGIN ,RNAME ,
G ELGPR ,ELPR ,EPST ,EPSC ,STRST ,
362






 yes
User Defined Joint Models
H STRSC ,STVBT ,STVBC ,PLSPRP ,STRSI ,
I STRSR ,EPSTH ,EPSI ,DEPS ,ELPRT ,
J SHRNKT ,SHRNKC ,D )
DIMENSION
A ELGPR(NLGPR) ,ELPR(NPRZ) ,EPST(NDSE) ,
B EPSC(NDSE) ,STRST(NDSE) ,STRSC(NDSE) ,
C STVBT(NSTAT) ,STVBC(NSTAT) ,PLSPRP(NDSE) ,
D STRSI(NDSE) ,STRSR(NDSE) ,EPSTH(NDSE) ,
E EPSI(NDSE) ,DEPS(NDSE) ,ELPRT(NPRZ,NTAB),
F SHRNKT(NDSE) ,SHRNKC(NDSE) ,D(NDSE,NDSE)
The argument list is the same as that for subroutine USRRST, except for the additional arguments ARGIN and RNAME. The logical variable ARGIN (see continuation line F in the above subroutine statement) is used in this subroutine. If ARGIN=.TRUE. verification of incoming arguments will be carried out and if ARGIN=.FALSE. verification of outgoing arguments will take place. The character variable RNAME indicates the routine for which verification is taking place, i.e. USRRDM or USRRST.
User Defined Joint Models
All joint models defined under JOINT PROPERTIES NONLINEAR USER utilise forces and strains/curvatures. The user defined routines interface with code at the element level. This facility may be used with any 2D or 3D joint element.
The constitutive relationship is assumed to be of the form:
where are the increments in joint forces, l q
are the increments of strains and curvatures and
D
is the diagonal modulus matrix. The modulus matrix is explicitly defined by the user via the externally developed FORTRAN subroutine,
USRKJN, and is of the form:
D
11
0
0
D
0
0
22
0
0
0
D
0
0
where ndse is the number of joint forces or strains and curvatures.
363
Appendix C Material Model Interface
User Joint Properties Input
The user joint properties are input in a similar manner to the other LUSAS joint property types.
The user joint properties input consists of nprz parameters where nprz =
nprzs*N+nprzj+1. The value nprzs is the number of parameters per spring, N is the number of springs and nprzj is the number of parameters common to all springs. The properties M
i
,C i
,
i
,
a ri
,b ri
along with mcode are reserved for LUSAS internal use: they are only utilisd if other features of the program are required (e.g. dynamic and thermal analyses). It should be noted however, that all nprz properties can be used within the user routines.
Together with the user joint parameters the user also needs to specify the following integer numbers for the specific joint model defined:
lptusr a number which identifies the particular user joint model.
nprzs the number of input parameters per spring
N the number of springs in the joint
nprzj the number of input parameters common to each spring
nstat the number of nonlinear state variables that are used in the joint model.
The value of nstat must not be less than 1.
The numbers are specified on the data input line for the user material model as follows:
JOINT PROPERTIES NONLINEAR USER lptusr N nprzs nprzj nstat
Evaluation of the Modulus Matrix
The modulus matrix
D
is explicitly defined via the externally supplied FORTRAN subroutine USRKJN. The routine is called at the element level, from both the LUSAS
Solver presolution and postsolution analysis modules. On entry to USRKJN, the modulus matrix
D
is fully initialised (each array component is set to a floating point real zero). Hence, only the nonzero components of the modulus matrix need be evaluated.
Nonlinear Stress Recovery
The stress recovery algorithm is defined explicitly via the externally supplied
FORTRAN subroutine USRSJN, and is concerned with the evaluation of:
Stress State the current stress state,
Material State the current material state (as indicated by the nonlinear state variables),
Nonlinear Variables additional associated nonlinear variables.
364
User Defined Joint Models
The routine is called at the element level, from the LUSAS Solver postsolution analysis module. Forces, strains and curvatures, and nonlinear state variables are available as current values, values at the end of the previous iteration, and values at the start of the current increment.
The procedure for updating incremental, and iterative variables from the evaluated current values, is automatically performed by LUSAS Solver. Consequently, modifications should be restricted to current values only.
Verification
Two routines USRJN1 and USRJN2 are supplied to enable the user to verify the incoming and outgoing arguments to the userprogrammed subroutines USRKJN and
USRSJN respectively.
SUBROUTINE USRKJN
Purpose
Explicit definition of the modulus matrix D for userdefined joint properties. This routine may be programmed by the user but the argument list must not be altered in any way.
SUBROUTINE USRKJN
A( LNODZ ,LPTUSR ,NACTVE ,NAXES ,ND ,
B NDSE ,NEL ,NPRZ ,NSTAT ,NT6 ,
C ACTIM ,ELTAGE ,DT ,TEMPC ,RSPTM ,
D TEMPR ,ERROR ,FEA ,INIACT ,NWINC ,
E REPAS ,VERIF ,
F B ,D ,DC ,DISPT ,DISPC ,
G ELPR ,EPST ,EPSC ,STVBT ,STVBC ,
H STRST ,STRSC ,XYZ ,VELCTY )
DIMENSION
A B(NDSE,NDF) ,D(NDSE,NDSE) ,DC(NAXES,NAXES),
B DISPT(NDF) ,DISPC(NDF) ,ELPR(NPRZ) ,
C EPST(NDSE) ,EPSC(NDSE) ,STVBT(NSTAT) ,
D STVBC(NSTAT) ,STRST(NDSE) ,STRSC(NDSE) ,
E XYZ(NAXES,LNODZ),VELCTY(NDF)
365
Appendix C Material Model Interface
Name
LNODZ
LPTUSR
NACTVE
NAXES
NDF
NDSE
NEL
NPRZ
NSTAT
NT6
ACTIM
ELTAGE
DT
TEMPC
RSPTM
TEMPR
ERROR
FEA
INIACT
NWINC
REPAS
VERIF
B
D
DC
DISPT
DISPC
ELPR
EPST
EPSC
Argument Description
Number of nodes
User supplied constitutive model reference number
Element activation status 0Standard element 1activating 2deactivated
Number of system axes (dimensions)
Number of degrees of freedom
Number of continuum stress components at a Gauss point for the stress model type MDL.
Current element number
Number of material parameters for the constitutive model
Number of state dependent model variables
LUSAS results output channel
Element activation time
Element age
Current time step increment (dynamic analysis)
Current temperature
Current total response time (dynamic analysis)
Reference temperature
Logical flag for fatal error and program termination
Logical flag denoting FEA or external code use
Logical flag for initial activation of element
Logical flag, TRUE indicating the start of a new increment
Logical flag, TRUE for repass
Logical incoming argument verification flag
Strain displacement matrix
Modulus matrix (Dmatrix)
Direction cosine matrix for the local axes system
Array of displacements at the start of the current increment
Array of current displacements
Material properties for current element
Total strain components at the start of the current increment
Current total strain components
366
RA
RA
RA
RA
RV
LV
LV
LV
LV
IV
IV
RV
RV
RV
RV
RV
LV
LV
RA
RA
RA
RA
IV
IV
IV
IV
IV
Type
IV
IV
IV
Modify














 yes












 yes
User Defined Joint Models
Name
STVBT
STVBC
STRST
STRSC
XYZ
VELCTY
Argument Description Type
State variables at the start of current increment
Current state variables
RA
RA
Stress components at the start of the current increment RA
Stress components
Coordinates for the nodes
Current velocity vector
RA
RA
RA



Modify



SUBROUTINE USRSJN
Purpose
Stress recovery algorithm for userdefined joint properties. This subroutine may be programmed by the user but the argument list may not be altered in any way.
SUBROUTINE USRSJN
A( LNODZ ,LPTUSR ,NACTVE ,NAXES ,ND ,
B NDSE ,NEL ,NPRZ ,NSTAT ,NT6 ,
C LSTATM ,IP ,ACTIM ,ELTAGE ,DT ,
D TEMPC ,RSPTM ,TEMPR ,DYNAM ,ERROR ,
E FEA ,INIACT ,NWINC ,REPAS ,STEPRD ,
F VERIF ,
G B ,D ,DC ,DISPT ,DISPC ,
H ELPR ,EPST ,EPSC ,STVBT ,STVBC ,
I STRST ,STRSC ,XYZ ,VELCTY )
DIMENSION
A B(NDSE,NDF) ,D(NDSE,NDSE) ,DC(NAXES,NAXES),
B DISPT(NDF) ,DISPC(NDF) ,ELPR(NPRZ) ,
C EPST(NDSE) ,EPSC(NDSE) ,STVBT(NSTAT) ,
D STVBC(NSTAT) ,STRST(NDSE) ,STRSC(NDSE) ,
E XYZ(NAXES,LNODZ),VELCTY(NDF)
Name
LNODZ
LPTUSR
Argument Description
Number of nodes
User supplied constitutive model reference number
Type
IV
IV
Modify


367
Appendix C Material Model Interface
Name
NACTVE
NAXES
NDF
NDSE
NEL
NPRZ
NSTAT
NT6
LSTATM
IP
ACTIM
ELTAGE
DT
TEMPC
RSPTM
TEMPR
DYNAM
ERROR
FEA
INIACT
NWINC
REPAS
STEPRD
VERIF
B
D
DC
DISPT
DISPC
ELPR
Argument Description
Element activation status 0Standard element 1activating 2deactivated
Number of system axes (dimensions)
Number of degrees of freedom
Number of continuum stress components at a Gauss point for the stress model type MDL.
Current element number
Number of material parameters for the constitutive model
Number of state dependent model variables
LUSAS results output channel
Length of state variable array
Pointer to start of plastic strains
Element activation time
Element age
Current time step increment (dynamic analysis)
Current temperature
Current total response time (dynamic analysis)
Reference temperature
HHT step by step dynamics
Logical flag for fatal error and program termination
Logical flag denoting FEA or external code use
Logical flag for initial activation of element
Logical flag, TRUE indicating the start of a new increment
Logical flag, TRUE for repass
Step reduction flag
Logical incoming argument verification flag
Strain displacement matrix
Modulus matrix (Dmatrix)
Direction cosine matrix for the local axes system
Array of displacements at the start of the current increment
Array of current displacements
Material properties for current element
IV
IV
RV
RV
RV
RV
LV
LV
LV
LV
LV
IV
IV
IV
IV
RV
RV
LV
LV
LV
RA
RA
RA
RA
RA
RA
Type
IV
Modify

IV
IV
IV





 yes



 yes








 yes







368
User Defined Joint Models
Name
EPST
EPSC
STVBT
STVBC
STRST
STRSC
XYZ
VELCTY
Argument Description
Total strain components at the start of the current increment
Current total strain components
Type
RA
RA
State variables at the start of current increment
Current state variables
RA
RA
Stress components at the start of the current increment RA
Stress components
Coordinates for the nodes
Current velocity vector
RA
RA
RA
Modify


 yes
 yes


SUBROUTINE USRJN1
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutine
USRKJN. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRJN1
A( LNODZ ,LPTUSR ,NACTVE ,NAXES ,NDF ,
B NDSE ,NEL ,NPRZ ,NPRZC ,NSTAT ,
C NT6 ,ACTIM ,ELTAGE ,DT ,RSPTM ,
D ERROR ,FEA ,INIACT ,NWINC ,REPAS ,
E VERIF ,ARGIN ,
F B ,D ,DC ,DISPT ,DISPC ,
G ELPR ,EPST ,EPSC ,STVBT ,STVBC ,
H STRST ,STRSC ,XYZ ,VELCTY ,TEMPR ,
I TEMPC )
DIMENSION
A B(NDSE,NDF) ,D(NDSE,NDSE) ,DC(NAXES,NAXES),
B DISPT(NDF) ,DISPC(NDF) ,ELPR(NPRZ) ,
C EPST(NDSE) ,EPSC(NDSE) ,STVBT(NSTAT) ,
D STVBC(NSTAT) ,STRST(NDSE) ,STRSC(NDSE) ,
E XYZ(NAXES,LNODZ),VELCTY(NDF),TEMPR(NDSE ,
F TEMPC(NDSE)
369
Appendix C Material Model Interface
The argument list is the same as that for subroutine USRKJN, except for one argument.
The additional argument is the logical variable ARGIN (see continuation line E in the above subroutine statement) that is used in this subroutine. If ARGIN=.TRUE. verification of incoming arguments will be carried out and if ARGIN=.FALSE. verification of outgoing arguments will take place.
SUBROUTINE USRJN2
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutine
USRSJN. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRJN2
A( LNODZ ,LPTUSR ,NACTVE ,NAXES ,NDF ,
B NDSE ,NEL ,NPRZ ,NSTAT ,NT6 ,
C LSTATM ,IP ,ACTIM ,ELTAGE ,DT ,
D TEMPC ,RSPTM ,TEMPR ,DYNAM ,ERROR ,
E FEA ,INIACT ,NWINC ,REPAS ,STEPRD ,
F VERIF ,ARGIN ,
G B ,D ,DC ,DISPT ,DISPC ,
H ELPR ,EPST ,EPSC ,STVBT ,STVBC ,
I STRST ,STRSC ,XYZ ,VELCTY )
DIMENSION
A B(NDSE,NDF) ,D(NDSE,NDSE) ,DC(NAXES,NAXES),
B DISPT(NDF) ,DISPC(NDF) ,ELPR(NPRZ) ,
C EPST(NDSE) ,EPSC(NDSE) ,STVBT(NSTAT) ,
D STVBC(NSTAT) ,STRST(NDSE) ,STRSC(NDSE) ,
E XYZ(NAXES,LNODZ),VELCTY(NDF)
The argument list is the same as that for subroutine USRSJN, except for one argument.
The additional argument is the logical variable ARGIN (see continuation line F in the above subroutine statement) that is used in this subroutine. If ARGIN=.TRUE. verification of incoming arguments will be carried out and if ARGIN=.FALSE. verification of outgoing arguments will take place.
370
User Defined Creep Models
User Defined Creep Models
Introduction
Several creep models are available in LUSAS, but if the provided models are inappropriate this facility will enable the definition of a creep material using a userdefined creep law.
The usersupplied creep routine USRCRP allows creep laws to be specified that are a function of stress, strain and temperature history.
Creep Laws
The usersupplied subroutine permits creep laws defined as: c
b g where:
c
Rate of uniaxial equivalent creep strain q
Equivalent deviatoric stress
Creep Properties Input
t
Time
T
Temperature
The user creep properties are input in a manner similar to that used for the other creep laws available in LUSAS.
The input for userdefined creep properties consists of a total of nprzc creep parameters, the first 3 of which are reserved specifically for use by LUSAS. The temperature is specified should the user wish to utilise temperature dependent properties. Creep properties 4 to nprzc must be given in the order expected by the usersupplied routines.
The 3 reserved locations are:
1. Reference temperature (T)
2. Not used at present.
3. Not used at present.
Together with the user creep properties you also need to specify the following integer numbers for the specific creep law defined:
ictp a number which identifies the particular user creep model.
nprzc the total number of creep properties used.
371
Appendix C Material Model Interface
nstat the number of nonlinear creep state variables that are used in the creep model (these variables will be output together with the Gauss point stresses/strains). The value of nstat must not be less than 1.
Evaluation of Creep Strains
The following points should be considered when coding the usersupplied routine
USRCRP for evaluating the creep strains:
The usersupplied routine must return the increment in creep strain. Further, if implicit integration is to be used, the variation of the creep strain increment with respect to the equivalent stress and with respect to the creep strain increment must also be defined.
If the function involves time dependent state variables, they must be integrated in the usersupplied routine.
If both plasticity and creep are defined for a material, the creep strains will be processed during the plastic strain update. Stresses in the user routine may therefore exceed the yield stress.
Verification
Routine USRVFC is supplied to enable the user to verify the incoming and outgoing arguments to the userprogrammed subroutine USRCRP. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRCRP
Purpose
Computes the creep strain increment.
The variations of creep strain DCRPDC, DCRPDQ, DCRPDP, DCRPDS are only required for implicit integration. This subroutine may be programmed by the user but the argument list may not be altered in any way.
SUBROUTINE USRCRP
A( LCTUSR ,NEL ,NG ,NCRPP ,NT6 ,
B NSTAT ,NDSE ,DISEN ,DT ,RSPTIM ,
C TEMP ,PRESS ,STREQV ,CRPSTN ,SWLSTN ,
D DCRP ,DCRPDC ,DCRPDQ ,DCRPDS ,DCRPDP ,
E VERIFY ,ERROR ,FEA ,EXPCRP ,STEPRD ,
F TIMEDP ,
G STATVC ,STATVP ,CRPMDL ,STRESS )
DIMENSION
372
User Defined Creep Models
A STATVC(NSTAT) ,STATVP(NSTAT) ,CRPMDL(NCRPP) ,
B STRESS(NDSE)
Name
LCTUSR
NEL
NG
NCRPP
NT6
NSTAT
NDSE
DISEN
DT
RSPTIM
TEMP
PRESS
STREQV
CRPSTN
SWLSTN
DCRP
DCRPDC
DCRPDQ
DCRPDS
DCRPDP
VERIFY
ERROR
FEA
EXPCRP
STEPRD
Argument Description
User supplied creep model reference number
Element number
Gauss point number
Number of parameters defining user creep model
LUSAS results output channel
Number of creep state dependent model variables
Number of stress components
Energy dissipated by inelastic process (not currently used)
Time step
Response time t  note time at beginning of step=t, time at end of step=t+dt
Gauss point temperature
Current pressure (not currently used)
Equivalent uniaxial stress (Hill or von Mises)
Creep strain at time t
Swelling strain at time t (not currently used)
Rate of change of creep strain with time
RV
RV
Rate of change of creep strain rate with creep increment
Rate of change of creep strain rate with equivalent stress
Rate of change of creep strain rate with swelling strain (not currently used)
Rate of change of creep strain rate with pressure (not currently used)
RV
RV
RV
RV
Logical incoming/outgoing argument verification flag LV
Logical flag for fatal error and program termination LV
Logical flag for FEA use only LV
Explicit creep. If .TRUE. use time=RSPTIM for evaluations and if .FALSE. use time=RSPTIM+DT.
For an implicit analysis EXPCRP will be .TRUE. in the presolution and .FALSE. in the postsolution
Step reduction flag
LV
LV
RV
RV
RV
RV
RV
RV
Type
IV
IV
IV
IV
IV
IV
IV
RV


 yes






 yes yes





Modify

 yes

 yes
373
Appendix C Material Model Interface
Name Argument Description
TIMEDP
STATVC
Time dependent creep flag
On entry: State variables at end of last step
On exit: Current state variables
STATVP State variables at end of last step
CRPMDL Creep model parameters
STRESS Current stress tensor
Type
LV
RA
RA
RA
RA



Modify
yes yes
SUBROUTINE USRVFC
Purpose
Verifies the incoming and outgoing arguments to the userprogrammed subroutine
USRCRP. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVFC
A( LCTUSR ,NEL ,NG ,NCRPP ,NT6 ,
B NSTAT ,NDSE ,DISEN ,DT ,RSPTIM ,
C TEMP ,PRESS ,STREQV ,CRPSTN ,SWLSTN ,
D DCRP ,DCRPDC ,DCRPDQ ,DCRPDS ,DCRPDP ,
E VERIFY ,ERROR ,FEA ,EXPCRP ,STEPRD ,
F TIMEDP ,MODE ,
G STATVC ,STATVP ,CRPMDL ,STRESS )
DIMENSION
A STATVC(NSTAT) ,STATVP(NSTAT) ,CRPMDL(NCRPP) ,
B STRESS(NDSE)
The argument list is the same as that for subroutine USRCRP, except for the additional integer variable MODE (see continuation line F in the above subroutine statement).
This variable is used in this subroutine: MODE=1 is for verification of incoming arguments, MODE=(any other value) is for verification of outgoing arguments.
374
User Defined Damage Models
User Defined Damage Models
Introduction
The usersupplied damage routine USRDAM permits external computation of the damage variable and its derivative with respect to the current elastic complementary energy norm.
The temperature, the damage threshold at the previous converged position, the damage model parameters and the damage state variables at the current and previous converged positions are available for this computation.
This facility allows the user to specify a damage law for a particular material if the damage models available in LUSAS are inappropriate.
Damage Variable
The damage variable is used to define the degradation of the elastic modulus matrix.
This means that the effective stress vector may be expressed as:
1
1 d t t b g{ }
Effective stress vector at time t
. t e
Cauchy stress vector at time t
. t c d t b g
Damage variable at time t
. Note that for no damage, d t b g
0
.
Further information on the use of damage models can be found in the LUSAS Theory
Manual.
Damage Properties Input
The user damage properties are input in a manner similar to that used for the other damage laws available in LUSAS.
The user damage properties input consists of a total of nprzd damage parameters, the first of which is reserved specifically for LUSAS use. This is the temperature that is specified, should the user wish to utilise temperature dependent properties. Damage properties 2 to nprzd must be supplied by the user in the order required by the usersupplied routines.
375
Appendix C Material Model Interface
The reserved location is:
Reference temperature. (T)
Together with the user damage properties, the following integer numbers for the specific damage law defined also need to be specified.
idtp Number which identifies the particular user damage model.
nprzd Total number of damage properties used.
nstat Number of nonlinear state variables that are used in the damage model
(these variables will be output together with the Gauss point stresses/strains). The value of nstat must not be less than 1.
Verification
Routine USRVFD is supplied to enable the user to verify the incoming and outgoing arguments to the userprogrammed subroutines USRDAM. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRDAM
Purpose
Computes the damage variable and its derivative with respect to the current elastic complementary energy norm. This subroutine may be programmed by the user but the argument list may not be altered in any way.
SUBROUTINE USRDAM
A( LDTUSR ,NEL ,NG ,NDAMP ,NT6 ,
B NSTAT ,TEMP ,TAUC ,HDAMA ,DDAMA ,
C TDAMA ,ERROR ,VERIFY ,FEA ,
D DAMCUR ,DAMPRV ,DAMMDL )
DIMENSION
A DAMCUR(NSTAT) ,DAMPRV(NSTAT) ,DAMMDL(NDAMP)
Name
LCTUSR
NEL
NG
NDAMP
NT6
Argument Description
User supplied damage model reference number
Element number
Gauss point number
Number of parameters defining user damage model
LUSAS results output channel
Type
IV
IV
IV
IV
IV
Modify





376
User Defined Damage Models
Name
NSTAT
TEMP
TAUC
HDAMA
DDAMA
TDAMA
ERROR
VERIFY
FEA
DAMCUR
DAMPRV
DAMMDL
Argument Description
Number of damage state dependent model variables
Gauss point temperature
Logical flag for fatal error and program termination
Logical incoming/outgoing argument verification flag
Logical flag for FEA use only
Current damage state variables
Damage state variables at end of last step
Damage model parameters
Type
RV
Norm of current elastic complementary energy
Derivative of damage variable with respect to
TAUC
RV
RV
Damage variable RV
Damage threshold at previous converged position RV
LV
LV
LV
RA
RA
RA
Modify

 yes yes
 yes

 yes


SUBROUTINE USRVFD
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutine
USRDAM. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVFD
A( LDTUSR ,NEL ,NG ,NDAMP ,NT6 ,
B NSTAT ,TEMP ,TAUC ,HDAMA ,DDAMA ,
C TDAMA ,ERROR ,VERIFY ,FEA ,MODE ,
D DAMCUR ,DAMPRV ,DAMMDL )
DIMENSION
A DAMCUR(NSTAT) ,DAMPRV(NSTAT) ,DAMMDL(NDAMP)
The argument list is the same as that for subroutine USRDAM, except for the additional integer variable MODE (see continuation line C in the above subroutine statement). This variable is used in this subroutine: MODE=1 is for verification of incoming arguments, MODE=(any other value) is for verification of outgoing arguments.
377
Appendix C Material Model Interface
User Defined Friction Models
Introduction
The usersupplied routine USRSLF permits a nonlinear friction law to be utilised in a slideline analysis. The friction law may be a function of the surface temperature, the relative velocities and/or accelerations of the adjacent surfaces and a set of user defined friction parameters. The friction law can be used with the normal interface force to return an allowable tangential frictional force.
Temperature dependent parameters are entered using the standard tabular input. All the values in the slideline properties table are interpolated at the temperature of the point of contact on the contacted surface prior to passing into the user routine.
Nonlinear Friction Law
The nonlinear friction law can take the form:
F allow
b
,
2
,
i g where:
F
N
allow i
Allowable tangential frictional force
Normal interface force
Relative velocities of the contacting surfaces
Relative accelerations of the contacting surfaces
Temperatures of contacting surfaces User defined friction parameters
T
The components of velocity and acceleration supplied to the user routine are in the direction of the tangential frictional force on the slideline surface being processed.
Note that in the routine USRSLF, the adjacent surface is the current surface being processed. To provide further useful information, the current response time, the contacting node number and the node numbers defining the current segment of the adjacent surface are also passed into USRSLF.
Nonlinear Friction Parameter Input
The nonlinear friction parameters are input using the SLIDELINE PROPERTIES
USER data section.
Input for the SLIDELINE PROPERTIES USER data section follows the same form as the standard SLIDELINE PROPERTIES data section, except the number of friction
378
User Defined Friction Models
parameters (nfric) must be defined. The friction parameters must be supplied in the order required by the usersupplied routines.
Verification
Routine USRVSF is supplied to enable the user to verify the incoming and outgoing arguments to the userprogrammed subroutines USRSLF. This subroutine may be utilised but no alterations are permitted.
SUBROUTINE USRSLF
Purpose
Computes the allowable tangential force using a nonlinear friction law. This subroutine may be programmed by the user but the argument list may not be altered in any way.
SUBROUTINE USRSLF
A( ISPROP ,NODC ,NFRIC ,NT6 ,ISURF ,
B JSURF ,NDSEG ,NPROPS ,TMPND ,TMPSF ,
C VNOD ,VSUR ,ANOD ,ASUR ,FORCEN ,
D FTALLW ,RSPTIM ,VERIFY ,ERROR ,FEA ,
E NODSEG ,SLPROP )
DIMENSION
A NODSEG(NSEGN) ,SLPROP(NPROPS)
Name
ISPROP
NODC
NFRIC
NT6
ISURF
JSURF
NDSEG
TMPND
TMPSF
VNOD
Argument Description
Slideline property assignment number
Contact node number
Number of friction parameters
LUSAS output channel
Surface number containing contact node
Cntacted surface number
Number of nodes on the current segment of the contacted surface
Current temperature at contacting node
Current temperature at contact point on adjacent surface
Velocity component of contacting node in direction of total tangential force on adjacent surface
IV
IV
IV
IV
Type
IV
IV
IV
RV
RV
RV






Modify




379
Appendix C Material Model Interface
Name
VSUR
ANOD
ASUR
FORCEN
FTALLW
RSPTIM
VERIFY
ERROR
FEA
NODSEG
SLPROP
Argument Description
Velocity component of adjacent surface in direction of total tangential force
Acceleration component of contacting node in direction of total tangential force on adjacent surface
Acceleration component of adjacent surface in direction of total tangential force
Magnitude of the normal force
Allowable tangential force
Current response time
Logical flag for verification of arguments
Logical flag for fatal error and program termination
For LUSAS/FEA internal use only
Node numbers for segment of adjacent surface
Slideline properties evaluated at contacted surface temperature TMPSF
Type
RV
RV
RV
RV
RV
RV
LV
LV
LV
IA
RA



Modify



 yes

 yes
SUBROUTINE USRVSF
Purpose
Verify the incoming and outgoing arguments to the userprogrammed subroutine
USRSLF. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVSF
A( ISPROP ,NODC ,NFRIC ,NT6 ,ISURF ,
B JSURF ,NDSEG ,NPROPS ,TMPND ,TMPSF ,
C VNOD ,VSUR ,ANOD ,ASUR ,FORCEN ,
D FTALLW ,RSPTIM ,VERIFY ,ERROR ,FEA ,
E MODE ,
F NODSEG ,SLPROP )
DIMENSION
A NODSEG(NSEGN) ,SLPROP(NPROPS)
The argument list is the same as that for subroutine USRSLF, except for the additional integer variable MODE (see continuation line E in the above subroutine statement).
This variable is used in this subroutine: MODE=1 is for verification of incoming arguments, MODE=(any other value) is for verification of outgoing arguments.
380
UserDefined Rate of Internal Heat Generation
UserDefined Rate of Internal Heat Generation
Introduction
The usersupplied subroutine USRRHG permits the user to define the way in which internal heat is generated in a thermal analysis. This can be defined to be a function of temperature, time and chemical reaction. The parameters used to control the chemical reaction are specified under the RIHG USER data chapter. In a thermomechanical coupled analysis, variables defining the current degree and rate of chemical reaction (or cure) may be transferred to the structural analysis where they can be accessed in the user interface routines USRKDM and USRSTR. The modulus matrix and stress computations may then become a function of degree or rate of cure.
User RIHG Parameter Input
The parameters controlling the rate of internal heat generation are specified under the user RIHG chapter in a similar manner to the way standard RIHG parameters are defined in LUSAS. The RIHG User data section takes the following form:
TEMPERATURE LOAD CASE
RIHG USER n
TABLE ilod
<P i
> i=1,n
TEMPERATURE LOAD ASSIGNMENTS
RIHG USER
L N ilod
Where n is the number of parameters to be defined, ilod the table identifier, P
i
the
RIHG control parameters, one of which could be a reference temperature, L the element number and N the node number of that element for which the parameters are to be applied. Note that the table could consist of many lines of parameters each one relating to a particular reference temperature. The complete table is accessible in the user routine USRRHG so that temperature dependent control parameters can be specified if necessary.
Evaluation of RIHG
The following points should be considered when coding the usersupplied routine
USRRHG for evaluating the rate of internal heat generation:
1. The user supplied routine USRRHG is called from within the element gauss point loop.
2. The routine must return the rate of internal heat generation at the nodes stored in the vector RIHG. In addition, the degree and rate of cure at the nodes can also be computed, stored in array DOCCND and returned. As this routine is called from within a gauss point loop and the information required to compute the nodal values
381
Appendix C Material Model Interface
is always available for an element, the nodal values need only be computed and returned on the first pass for each element, e.g. when the gauss point loop counter,
NG=1.
3. The current degree and rate of cure (or some other chemical reaction) can also be computed at the gauss points on each pass through the routine and stored in vector
DOCCGP. The values at the start of the time step are also available.
4. In a thermomechanical coupled analysis, the gauss point cure values (or any other chemical reaction which influences mechanical behaviour) may be transferred to the structural analysis and are accessible in the user defined material routines
USRKDM and USRSTR.
Verification
Routine USRVFR is supplied to enable the user to verify the incoming and outgoing arguments to the userprogrammed subroutines USRRHG. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRRHG
Purpose
Computes the rate of internal heat generation at nodes, RIHG, the degree of cure at nodes, DOCCND and at gauss points, DOCCGP. This subroutine may be programmed by the user but the argument list may not be altered in any way.
SUBROUTINE USRRHG
A( NEL ,LNODZ ,NTAB ,NRHGD ,NG ,
B INC ,NT ,NAXES ,NGP ,NT6 ,
C NDOC ,DT ,RSPTM ,DINT ,TEMPIN ,
D ACTIM ,ELTAGE ,USRGPC ,USRGPP ,ERROR ,
E BOUNDS ,PRESOL ,VERIF ,NWINC ,FEA ,
F TMPFLG ,REPAS ,
G TINIT ,TEMPC ,TEMPP ,TEMPI ,NTABLD ,
H SHAPES ,XYZ ,DOCCGP ,DOCPGP ,DOCIGP ,
I RIHG ,RHGDAT ,XYZN ,DOCCND ,DOCPND ,
J DOCIND ,USRNDC ,USRNDP )
DIMENSION
A TINIT(LNODZ) ,TEMPC(LNODZ) ,
B TEMPP(LNODZ) ,TEMPI(LNODZ) ,
C NTABLD(LNODZ) ,SHAPES(LNODZ) ,
D XYZ(NAXES) ,DOCCGP(NDOC) ,
382
UserDefined Rate of Internal Heat Generation
NG
INC
NT
NAXES
NGP
NT6
NDOC
DT
RSPTM
DINT
Name
NEL
LNODZ
NTAB
NRHGD
TEMPIN
ACTIM
ELTAGE
USRGPC
USRGPP
ERROR
BOUNDS
E DOCPGP(NDOC) ,DOCIGP(NDOC) ,
F RIHG(LNODZ) ,RHGDAT(NRHGD,NTAB,LNODZ),
G XYZN(NAXES,LNODZ) ,DOCCND(NDOC,LNODZ) ,
H DOCPND(NDOC,LNODZ) ,DOCIND(NDOC,LNODZ) ,
I USRNDC(LNODZ) ,USRNDP(LNODZ)
PRESOL
Argument Description Type
Current element number
Number of element nodes
IV
IV
Maximum number of lines in any RIHG USER table IV
IV Maximum number of parameters in any line of RIHG
USER data
Current Gauss point number
Current increment number
Current time step number
IV
IV
IV
Number of system axes (dimensions)
Number of gauss points
LUSAS results output channel
First dimension of degree of cure arrays (=2)
Current time step increment
Current total response time
Characteristic length or area of the current Gauss point
Temperature at the current gauss point  interpolated from nodal values (can be used if TMPFLG.is true  currently only applicable for composite brick elements)
Time of element activation
Element age on loading
User defined gauss point value (current)
IV
IV
IV
IV
RV
RV
RV
RV
RV
RV
RV
User defined gauss point value (start of time step) RV
Logical flag for fatal error and program termination LV
Logical to error if the current temperature is outside the bounds of a table of values
(OPTION 227)
LV
Logical flag, TRUE for presolution (forming thermal stiffness) and FALSE in postsolution
(computation of thermal gradients and flows)
LV yes yes

Modify
















383
Appendix C Material Model Interface
Name
VERIF
NWINC
FEA
TMPFLG
REPAS
TINIT
TEMPC
TEMPP
TEMPI
NTABLD
SHAPES
XYZ
DOCCGP
DOCPGP
DOCIGP
RIHG
RHGDAT
XYZN
DOCCND
DOCPND
DOCIND
USRNDC
USRNDP
Argument Description
Logical incoming/outgoing argument verification flag
Logical flag, TRUE denoting the start of a new increment
Logical flag denoting FEA or external code use
(FOR FEA INTERNAL USE ONLY)
Logical flag, if true indicates that the current gauss point temperature has been interpolated from nodal values and is available in the arguments list
Logical flag, TRUE denoting a repass
Initial nodal temperatures  only applicable on very first pass when specified as TMPE or
TEMP loading case
Current nodal temperatures
Nodal temperatures at previous increment or time step
Nodal temperatures at previous iteration
Number of lines in the load table for each node
Shape function values for current gauss point
Current gauss point coordinates
Current degree of cure at current gauss point
Degree of cure at previous increment or time step at current gauss point
Degree of cure at previous iteration at current gauss point
Rate of internal heat generation at nodes
Input parameters defined in RIHG USER data chapter
Nodal coordinates
Current degree of cure at nodes
Nodal degree of cure at previous increment or time step
Nodal degree of cure at previous iteration
User defined nodal values (current)
User defined nodal values (start of time step)
Type
LV
LV
LV
LV
LV
RA
RA
RA
RA
IA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA
RA


Modify





 yes

 yes

 yes



 yes


384
UserDefined Rate of Internal Heat Generation
SUBROUTINE USRVFR
Purpose
Verifies the incoming and outgoing arguments to the userprogrammed subroutine
USRRHG. This subroutine may be utilised by the user but no alterations are permitted.
SUBROUTINE USRVFR
A( NEL ,LNODZ ,NTAB ,NRHGD ,NG ,
B INC ,NT ,NAXES ,NGP ,NT6 ,
C NDOC ,DT ,RSPTM ,DINT ,TEMPIN ,
D ACTIM ,ELTAGE ,USRGPC ,USRGPP ,ERROR ,
E BOUNDS ,PRESOL ,VERIF ,NWINC ,FEA ,
F TMPFLG ,REPAS ,ARGIN ,
G TINIT ,TEMPC ,TEMPP ,TEMPI ,NTABLD ,
H SHAPES ,XYZ ,DOCCGP ,DOCPGP ,DOCIGP ,
I RIHG ,RHGDAT ,XYZN ,DOCCND ,DOCPND ,
J DOCIND ,USRNDC ,USRNDP )
DIMENSION
A TINIT(LNODZ) ,TEMPC(LNODZ) ,
B TEMPP(LNODZ) ,TEMPI(LNODZ) ,
C NTABLD(LNODZ) ,SHAPES(LNODZ) ,
D XYZ(NAXES) ,DOCCGP(NDOC) ,
E DOCPGP(NDOC) ,DOCIGP(NDOC) ,
F RIHG(LNODZ) ,RHGDAT(NRHGD,NTAB,LNODZ),
G XYZN(NAXES,LNODZ) ,DOCCND(NDOC,LNODZ) ,
H DOCPND(NDOC,LNODZ) ,DOCIND(NDOC,LNODZ) ,
I USRNDC(LNODZ) ,USRNDP(LNODZ)
The argument list is almost the same as that of subroutine USRRHG, except for the additional logical ARGIN (see continuation line F in the above subroutine statement).
This variable is used in this subroutine. If ARGIN=.TRUE. verification of incoming arguments will be carried out and if ARGIN=.FALSE. verification of outgoing arguments will take place.
385
Appendix C Material Model Interface
Utility Routines
Introduction
In addition to the userprogrammable subroutines, access is available to the following
LUSAS utility subroutines and functions. A full description of the operation and arguments of each of these routines can be found on the pages that follow.
Name Routine Function and Description
DVSTSN
INTPRP
KMVEQS
Form deviatoric stress matrix from total stress matrix and evaluate the first stress invariant
Interpolate the current material properties from the table
Transform stress/strain vector to equivalent matrix or vice versa
Compute the principal values of stress/strain vector in 2D
PRNSTR
PRSTR3
TEGV2
Compute the principal values of stress/strain vector in 3D
Compute eigenvalues and eigenvectors of a 2*2 matrix
Compute eigenvalues and eigenvectors of a 3*3 matrix
MTEGV3
MTINV2
MTINV3
Invert a 2*2 matrix explicitly
Invert a 3*3 matrix using Cramer's rule
MTINVT
Invert a matrix of any order using Gaussian elimination
KTRNLG
Transform stress/strains between local and global systems at a point
In order to avoid the duplication of existing LUSAS subroutine names, any externally developed subroutines (at a lower level to the userprogrammable subroutines) must adhere to the naming convention:
SUBROUTINE USR___
It is also recommended that site dependent constraints regarding subroutine name length, variable names, and machine precision be considered when developing external
FORTRAN code.
SUBROUTINE DVSTSN
Purpose
Calculates the deviatoric stress matrix and then evaluates the first stress invariant. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE DVSTSN
A( NMSMX ,SMEAN ,
B SMX ,DEVSMX )
DIMENSION
386
Utility Routines
A SMX(NMSMX,NMSMX) ,DEVSMX(NMSMX,NMSMX)
Name
NMSMX
SMEAN
SMX
DEVSMX
Argument Description
Dimensions of matrices (always=3)
Mean stress/strain
Stress/strain matrix
Deviatoric stress tensor
Type
IV
RV
RA
RA
Modified
 yes
 yes
SUBROUTINE INTPRP
Purpose
Interpolates temperature dependent properties from a table. The temperature property values within which the temperature load lies are found and the column numbers of these properties in the element material property table array are extracted. These properties are then interpolated as a linear variation of temperature and stored in the element material property array. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE INTPRP
A( NEL ,IMAT ,LPTP ,NPRZ ,NTAB ,
B NG ,ILOC ,TEMP ,BOUNDS ,ERROR ,
C ELPR ,ELPRT )
DIMENSION
A ELPR(NPRZ) ,ELPRT(NPRZ,NTAB)
Name
NEL
IMAT
LPTP
NPRZ
Argument Description
Element number
Material assignment reference number
Material model reference number
Maximum number of properties for defined property type
Number of lines of property data in table NTAB
NG
ILOC
Gauss point number
Location of temperature property in ELPR or
ELPRT for material defined
TEMP Temperature at this point
BOUNDS Flag for error if temperature out of bounds
Type
IV
IV
IV
IV
IV
IV
IV
RV
LV


Modified





 yes
387
Appendix C Material Model Interface
Name
ERROR
ELPR
ELPRT
Argument Description
Logical flag for fatal error and program termination
Interpolated element material properties
Table of temperature dependent material properties
Type
LV
RA
RA
Modified
yes yes

SUBROUTINE KMVEQS
Purpose
This subroutine sets up the stress/strain tensor as a 3*3 matrix or NDSE*1 vector for any stress model. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE KMVEQS
A( MDL ,NDSE ,NMS ,STRFLG ,MTXFLG ,
B SM ,SV )
DIMENSION
A SM(NMS,NMS) ,SV(NDSE)
Name Argument Description
MDL
NDSE
NMS
STRFLG
Reference code for stress model type
Number of continuum stresses/strains at a point
Dimension of stress/strain matrix
Flag indicating stress or strain to be used,
.TRUE.=Stress, .FALSE.=Strain
MTXFLG Flag indicating matrix or vector form is required,
.TRUE.=Matrix, .FALSE.=Vector
SM
SV
Stress/strain matrix
Stress/strain vector
Type
IV
IV
IV
LV
LV
RA
RA
Modified




 yes yes
SUBROUTINE PRNSTR
Purpose
Computes the principal stresses or strains for 2dimensional problems using Mohr's circle. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE PRNSTR
388
Utility Routines
A( S ,SMAX ,SMIN ,ANGD ,MODE )
DIMENSION
A S(3)
Name
S
SMAX
SMIN
ANGD
MODE
Argument Description
Vector in the form Sx, Sy, Sxy
Maximum principal value
Minimum principal value
Angle of maximum principal value in degrees clockwise from the X axes
Flag indicating stress or strain, 1 = Stress, 2 = Strain
Type
RA
RV
RV
RV
IV
Modified
 yes yes yes

SUBROUTINE PRSTR3
Purpose
This subroutine finds the principal stresses/strains in 3D by computing the eigenvectors of a symmetric tridiagonal matrix using inverse iteration. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE PRSTR3
A( NDSE ,NPRIN ,MDL ,STRFLG
B STRESS ,STRSP ,SVEC )
DIMENSION
A STRESS(NDSE) ,STRSP(NPRIN) ,
B SVEC(NPRIN,NPRIN)
Name
NDSE
NPRIN
STRESS
STRSP
SVEC
Argument Description
Number of continuum stress/strain components
Dimension of tridiagonal matrix (must equal 3)
Stress array: Sx, Sy, Sz, Sxy, Syz, Sxz
Principal stress array
Final eigenvectors
Type
IV
IV
RA
RA
RA
Modified


 yes yes
389
Appendix C Material Model Interface
SUBROUTINE MTEGV2
Purpose
Computes the explicit solution in terms of eigenvalues and eigenvectors of the 2dimensional eigen problem. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE MTEGV2
A( IS ,CM ,EVALUS ,EVECTS ,ERROR )
DIMENSION
A CM(IS,IS) ,EVALUS(IS) ,EVECTS(IS,IS)
Name
IS
CM
EVALUS
EVECTS
ERROR
Argument Description
Dimension of eigenproblem (must = 2)
Coefficient matrix (must be positive definite)
Array of eigenvalues
Matrix of eigenvectors
Flag returned .TRUE. on error
Type
IV
RA
RA
RA
LV
Modified

 yes yes yes
SUBROUTINE MTEGV3
Purpose
Compute the solution in terms of eigenvalues and eigenvectors of a symmetric 3dimensional eigen problem using Jacobi rotation. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE MTEGV3
A( IS ,CM ,EVALUS ,EVECTS )
DIMENSION
A CM(IS,IS) ,EVALUS(IS) ,EVECTS(IS,IS)
Name
IS
CM
EVALUS
EVECTS
Argument Description
Dimension of eigenproblem (must = 3)
Coefficient matrix (must be positive definite)
Array of eigenvalues
Matrix of eigenvectors
Type
IV
RA
RA
RA
Modified

 yes yes
390
Utility Routines
SUBROUTINE MTINV2
Purpose
Invert a 2*2 matrix explicitly. A mode switch is available so that only the determinant can be computed. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE MTINV2
A( A ,B ,DET ,IS ,MODE ,
B IERR )
DIMENSION
A A(IS,IS) ,B(IS,IS)
Name
A
B
DET
IS
MODE
IERR
Argument Description
Matrix to be inverted
Inverse matrix
Determinant of A
Dimension of matrix (must equal 2)
Mode switch, 1= evaluate determinant only
Error flag, returned nonzero on error
Type
RA
RA
RV
IV
IV
IV
Modified
 yes yes

 yes
SUBROUTINE MTINV3
Purpose
Invert a 3*3 matrix explicitly. A mode switch is available so that only the determinant can be computed. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE MTINV3
A( A ,B ,DET ,IS ,MODE ,
B IERR )
DIMENSION
A A(IS,IS) ,B(IS,IS)
Name
A
B
Argument Description
Matrix to be inverted
Inverse matrix
Type
RA
RA
Modified
 yes
391
Appendix C Material Model Interface
Name
DET
IS
MODE
IERR
Argument Description
Determinant of A
Dimension of matrix (must = 3)
Mode switch, 1=evaluate determinant only
Error flag, returned nonzero on error
Type
RV
IV
IV
IV
Modified
yes

 yes
SUBROUTINE MTINVT
Purpose
Invert a N*N matrix (or a submatrix) by using the GaussJordan method. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE MTINVT
A( A ,IS ,NA )
DIMENSION
A A(IS,IS)
Name
A
IS
NA
Argument Description
On input : matrix to be inverted
Dimension of matrix
The dimension of the submatrix that must be inverted
Type
RA
IV
IV
Modified

 yes. On exit: the inverse of the original matrix
SUBROUTINE KTRNLG
Purpose
Transform local stresses or strains at a point to global values. This subroutine may be utilised by the user but no alterations are permissible.
SUBROUTINE KTRNLG
A( NEL ,NDSE ,NAXES ,MODE ,TYPE ,
B MDL ,
C DRCGGP ,STRORI ,STRNEW )
DIMENSION
392
Utility Routines
A DRCGGP(NAXES,NAXES) ,STRORI(NDSE) ,
B STRNEW(NDSE)
Name
NEL
NDSE
NAXES
MODE
TYPE
MDL
DRCGGP
STRORI
Argument Description Type
Element number
Number of stresses/strains at a point
Number of axes for a problem
If .TRUE. then local to global else global to local
Logical for results type .TRUE. for stresses otherwise strains
LV
Stress model number IV
Direction cosines defining local Cartesian axes RA
IV
IV
IV
LV
Original stresses or strains
STRNEW Transformed stresses or strains
RA
RA


 yes
Modified





393
Appendix C Material Model Interface
394
* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project