Keywords Reference Manual Volume II: I–Z Version 6.
ABAQUS Keywords Reference Manual Volume II Version 6.
Trademarks and Legal Notices CAUTIONARY NOTICE TO USERS: This manual is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the ABAQUS Software. The ABAQUS Software is inherently complex, and the examples and procedures in this manual are not intended to be exhaustive or to apply to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses. ABAQUS, Inc.
ABAQUS Offices and Representatives ABAQUS, Inc. ABAQUS Europe BV Rising Sun Mills, 166 Valley Street, Providence, RI 02909–2499, Tel: +1 401 276 4400, Fax: +1 401 276 4408, support@Abaqus.com, http://www.abaqus.com Gaetano Martinolaan 95, P. O. Box 1637, 6201 BP Maastricht, The Netherlands, Tel: +31 43 356 6906, Fax: +31 43 356 6908, info.europe@abaqus.
Preface This section lists various resources that are available for help with using ABAQUS. Support ABAQUS, Inc., offers both technical engineering support (for problems with creating a model or performing an analysis) and systems support (for installation, licensing, and hardware-related problems) for ABAQUS through a network of local support offices. Contact information is listed in the front of each ABAQUS manual.
CONTENTS Contents — Volume I A *ACOUSTIC FLOW VELOCITY *ACOUSTIC MEDIUM *ACOUSTIC WAVE FORMULATION *ADAPTIVE MESH *ADAPTIVE MESH CONSTRAINT *ADAPTIVE MESH CONTROLS *AMPLITUDE *ANNEAL *ANNEAL TEMPERATURE *AQUA *ASSEMBLY *ASYMMETRIC-AXISYMMETRIC *AXIAL 1.1 1.2 1.3 1.4 1.5 1.6 1.7 1.8 1.9 1.10 1.11 1.12 1.
CONTENTS C *C ADDED MASS *CAPACITY *CAP CREEP *CAP HARDENING *CAP PLASTICITY *CAST IRON COMPRESSION HARDENING *CAST IRON PLASTICITY *CAST IRON TENSION HARDENING *CAVITY DEFINITION *CECHARGE *CECURRENT *CENTROID *CFILM *CFLOW *CFLUX *CHANGE FRICTION *CLAY HARDENING *CLAY PLASTICITY *CLEARANCE *CLOAD *COHESIVE SECTION *COMBINED TEST DATA *COMPLEX FREQUENCY *CONCRETE *CONCRETE COMPRESSION DAMAGE *CONCRETE COMPRESSION HARDENING *CONCRETE DAMAGED PLASTICITY *CONCRETE TENSION DAMAGE *CONCRETE TENSION STIFFENING
CONTENTS *CONNECTOR LOAD *CONNECTOR LOCK *CONNECTOR MOTION *CONNECTOR PLASTICITY *CONNECTOR POTENTIAL *CONNECTOR SECTION *CONNECTOR STOP *CONSTRAINT CONTROLS *CONTACT *CONTACT CLEARANCE *CONTACT CLEARANCE ASSIGNMENT *CONTACT CONTROLS *CONTACT CONTROLS ASSIGNMENT *CONTACT DAMPING *CONTACT EXCLUSIONS *CONTACT FILE *CONTACT FORMULATION *CONTACT INCLUSIONS *CONTACT INTERFERENCE *CONTACT OUTPUT *CONTACT PAIR *CONTACT PRINT *CONTACT PROPERTY ASSIGNMENT *CONTACT RESPONSE *CONTOUR INTEGRAL *CONTROLS *CORRELATION *
CONTENTS D *D ADDED MASS *DAMAGE EVOLUTION *DAMAGE INITIATION *DAMAGE STABILIZATION *DAMPING *DASHPOT *DEBOND *DECHARGE *DECURRENT *DEFORMATION PLASTICITY *DENSITY *DEPVAR *DESIGN GRADIENT *DESIGN PARAMETER *DESIGN RESPONSE *DETONATION POINT *DFLOW *DFLUX *DIAGNOSTICS *DIELECTRIC *DIFFUSIVITY *DIRECT CYCLIC *DISPLAY BODY *DISTRIBUTION *DISTRIBUTING *DISTRIBUTING COUPLING *DLOAD *DRAG CHAIN *DRUCKER PRAGER *DRUCKER PRAGER CREEP *DRUCKER PRAGER HARDENING *DSA CONTROLS *DSECHARGE *DSECURRENT *DSFLOW *DSFLUX
CONTENTS E *EL FILE *EL PRINT *ELASTIC *ELCOPY *ELECTRICAL CONDUCTIVITY *ELEMENT *ELEMENT MATRIX OUTPUT *ELEMENT OUTPUT *ELEMENT PROPERTIES *ELEMENT RESPONSE *ELGEN *ELSET *EMBEDDED ELEMENT *EMISSIVITY *END ASSEMBLY *END INSTANCE *END LOAD CASE *END PART *END STEP *ENERGY FILE *ENERGY OUTPUT *ENERGY PRINT *EOS *EOS COMPACTION *EOS SHEAR *EPJOINT *EQUATION *EXPANSION *EXTREME ELEMENT VALUE *EXTREME NODE VALUE *EXTREME VALUE 5.1 5.2 5.3 5.4 5.5 5.6 5.7 5.8 5.9 5.10 5.11 5.12 5.13 5.14 5.15 5.16 5.17 5.
CONTENTS *FILE OUTPUT *FILM *FILM PROPERTY *FILTER *FIXED MASS SCALING *FLOW *FLUID BEHAVIOR *FLUID BULK MODULUS *FLUID CAVITY *FLUID DENSITY *FLUID EXCHANGE *FLUID EXCHANGE ACTIVATION *FLUID EXCHANGE PROPERTY *FLUID EXPANSION *FLUID FLUX *FLUID INFLATOR *FLUID INFLATOR ACTIVATION *FLUID INFLATOR MIXTURE *FLUID INFLATOR PROPERTY *FLUID LEAKOFF *FLUID LINK *FLUID PROPERTY *FOUNDATION *FRACTURE CRITERION *FRAME SECTION *FREQUENCY *FRICTION 6.8 6.9 6.10 6.11 6.12 6.13 6.14 6.15 6.16 6.17 6.18 6.19 6.20 6.
CONTENTS H *HEADING *HEAT GENERATION *HEAT TRANSFER *HEATCAP *HOURGLASS STIFFNESS *HYPERELASTIC *HYPERFOAM *HYPOELASTIC *HYSTERESIS 8.1 8.2 8.3 8.4 8.5 8.6 8.7 8.8 8.
CONTENTS Contents — Volume II I *IMPEDANCE *IMPEDANCE PROPERTY *IMPERFECTION *IMPORT *IMPORT CONTROLS *IMPORT ELSET *IMPORT NSET *INCIDENT WAVE *INCIDENT WAVE FLUID PROPERTY *INCIDENT WAVE INTERACTION *INCIDENT WAVE INTERACTION PROPERTY *INCIDENT WAVE PROPERTY *INCIDENT WAVE REFLECTION *INCLUDE *INCREMENTATION OUTPUT *INELASTIC HEAT FRACTION *INERTIA RELIEF *INITIAL CONDITIONS *INSTANCE *INTEGRATED OUTPUT *INTEGRATED OUTPUT SECTION *INTERACTION OUTPUT *INTERACTION PRINT *INTERFACE *ITS 9.1 9.2 9.3 9.4 9.
CONTENTS L *LATENT HEAT *LOAD CASE 12.1 12.2 M *MAP SOLUTION *MASS *MASS DIFFUSION *MASS FLOW RATE *MATERIAL *MATRIX *MATRIX ASSEMBLE *MATRIX INPUT *MEMBRANE SECTION *MODAL DAMPING *MODAL DYNAMIC *MODAL FILE *MODAL OUTPUT *MODAL PRINT *MODEL CHANGE *MOHR COULOMB *MOHR COULOMB HARDENING *MOISTURE SWELLING *MOLECULAR WEIGHT *MONITOR *MOTION *MPC *MULLINS EFFECT *M1 *M2 13.1 13.2 13.3 13.4 13.5 13.6 13.7 13.8 13.9 13.10 13.11 13.12 13.13 13.14 13.15 13.16 13.17 13.18 13.19 13.20 13.21 13.22 13.23 13.
CONTENTS *NODE FILE *NODE OUTPUT *NODE PRINT *NODE RESPONSE *NONSTRUCTURAL MASS *NORMAL *NSET 14.9 14.10 14.11 14.12 14.13 14.14 14.15 O *ORIENTATION *ORNL *OUTPUT 15.1 15.2 15.
CONTENTS *PRINT *PSD-DEFINITION 16.28 16.29 *RADIATE *RADIATION FILE *RADIATION OUTPUT *RADIATION PRINT *RADIATION SYMMETRY *RADIATION VIEWFACTOR *RANDOM RESPONSE *RATE DEPENDENT *RATIOS *REBAR *REBAR LAYER *REFLECTION *RELEASE *RESPONSE SPECTRUM *RESTART *RETAINED EIGENMODES *RETAINED NODAL DOFS *RIGID BODY *RIGID SURFACE *ROTARY INERTIA 17.1 17.2 17.3 17.4 17.5 17.6 17.7 17.8 17.9 17.10 17.11 17.12 17.13 17.14 17.15 17.16 17.17 17.18 17.19 17.
CONTENTS *SIMPEDANCE *SIMPLE SHEAR TEST DATA *SLIDE LINE *SLOAD *SOILS *SOLID SECTION *SOLUBILITY *SOLUTION TECHNIQUE *SOLVER CONTROLS *SORPTION *SPECIFIC HEAT *SPECTRUM *SPRING *SRADIATE *STATIC *STEADY STATE CRITERIA *STEADY STATE DETECTION *STEADY STATE DYNAMICS *STEADY STATE TRANSPORT *STEP *SUBMODEL *SUBSTRUCTURE COPY *SUBSTRUCTURE DELETE *SUBSTRUCTURE DIRECTORY *SUBSTRUCTURE GENERATE *SUBSTRUCTURE LOAD CASE *SUBSTRUCTURE MATRIX OUTPUT *SUBSTRUCTURE PATH *SUBSTRUCTURE PROPERTY *SURFACE *SURFACE BEHAVI
CONTENTS T *TEMPERATURE *TENSILE FAILURE *TENSION STIFFENING *THERMAL EXPANSION *TIE *TIME POINTS *TORQUE *TORQUE PRINT *TRACER PARTICLE *TRANSFORM *TRANSPORT VELOCITY *TRANSVERSE SHEAR STIFFNESS *TRIAXIAL TEST DATA *TRS 19.1 19.2 19.3 19.4 19.5 19.6 19.7 19.8 19.9 19.10 19.11 19.12 19.13 19.14 U *UEL PROPERTY *UNDEX CHARGE PROPERTY *UNIAXIAL TEST DATA *USER DEFINED FIELD *USER ELEMENT *USER MATERIAL *USER OUTPUT VARIABLES 20.1 20.2 20.3 20.4 20.5 20.6 20.
I 9.
* IMPEDANCE 9.1 *IMPEDANCE: Define impedances for acoustic analysis. This option is used to provide boundary impedances or nonreflecting boundaries for acoustic and coupled acoustic-structural analyses. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step References: • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.9.1 of the ABAQUS Analysis User’s Manual • • • “Acoustic loads,” Section 27.4.
* IMPEDANCE Optional parameter: OP Set OP=MOD (default) to modify existing impedances or to define additional impedances. Set OP=NEW if all existing impedances applied to the model should be removed. To remove only selected impedances, use OP=NEW and respecify all impedances that are to be retained. Data line to define an impedance for PROPERTY, NONREFLECTING=PLANAR, or NONREFLECTING=IMPROVED: First (and only) line: 1. Element number or element set label. 2.
* IMPEDANCE 8. X-component of the direction cosine of the major axis of the ellipse or prolate spheroid defining the radiating surface. The components of this vector need not be normalized to unit magnitude. 9. Y-component of the direction cosine of the major axis of the ellipse or prolate spheroid defining the radiating surface. 10. Z-component of the direction cosine of the major axis of the ellipse or prolate spheroid defining the radiating surface. 9.
* IMPEDANCE PROPERTY 9.2 *IMPEDANCE PROPERTY: boundary. Define the impedance parameters for an acoustic medium This option is used to define the proportionality factors between the pressure and the normal components of surface displacement and velocity in acoustic analysis. The *IMPEDANCE PROPERTY option must be used in conjunction with the *IMPEDANCE or *SIMPEDANCE option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • “Acoustic loads,” Section 27.4.
* IMPEDANCE PROPERTY Data lines to define an impedance using DATA=ADMITTANCE (default): First line: 1. , the proportionality factor between pressure and displacement of the surface in the normal direction. This quantity is the imaginary part of the complex admittance, divided by the angular frequency; see “Acoustic loads,” Section 27.4.5 of the ABAQUS Analysis User’s Manual. (Units of F−1 L3 .) 2. , the proportionality factor between pressure and velocity of the surface in the normal direction.
* IMPERFECTION 9.3 *IMPERFECTION: Introduce geometric imperfections for postbuckling analysis. This option is used to introduce a geometric imperfection into a model for a postbuckling analysis. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • “Introducing a geometric imperfection into a model,” Section 11.3.1 of the ABAQUS Analysis User’s Manual “Unstable collapse and postbuckling analysis,” Section 6.2.
* IMPERFECTION NSET Set this parameter equal to the node set to which the geometric imperfection values are to be applied. If this parameter is omitted, the imperfection will be applied to all nodes in the model. Optional parameter if the FILE parameter is omitted: SYSTEM Set SYSTEM=R (default) to specify the imperfection as perturbation values of Cartesian coordinates. Set SYSTEM=C to specify the imperfection as perturbation values of cylindrical coordinates.
* IMPERFECTION Z (X,Y,Z) Y X Rectangular Cartesian (SYSTEM=R) (default) Z Z (R,θ,Z) (R,θ, φ) Y Y φ R θ θ X X Cylindrical (SYSTEM=C) Spherical (SYSTEM=S) (θ and φ are given in degrees) Figure 9.3–1 Coordinate systems. 9.
* IMPORT 9.4 *IMPORT: Import information from a previous ABAQUS/Explicit or ABAQUS/Standard analysis. If this is an ABAQUS/Explicit analysis, this option is used to define the time in a previous ABAQUS/Standard analysis at which the specified node and element information is imported. If this is an ABAQUS/Standard analysis, this option is used to define the time in a previous ABAQUS/Standard or ABAQUS/Explicit analysis at which the specified node and element information is imported.
* IMPORT the analysis is to be imported. If this parameter is omitted, the analysis is imported from the last available interval of the specified step. ITERATION This parameter is relevant only when the results are imported from a previous direct cyclic ABAQUS/Standard analysis.
* IMPORT CONTROLS 9.5 *IMPORT CONTROLS: Specify tolerances used in importing model and results data. This option is used to specify the tolerance for error checking on shell normals in ABAQUS/Standard or ABAQUS/Explicit when the *IMPORT, UPDATE=YES option is used. If the *IMPORT CONTROLS option is used, it must appear after the *IMPORT option.
* IMPORT ELSET 9.6 *IMPORT ELSET: Import element set definitions from a previous ABAQUS/Explicit or ABAQUS/Standard analysis. This option is used to import element set definitions that were defined in a previous ABAQUS/Explicit or ABAQUS/Standard analysis. If the *IMPORT ELSET option is used, it must appear after the *IMPORT option. If this option is omitted or is specified without any data lines, all the element sets relevant to the analysis will be imported.
* IMPORT NSET 9.7 *IMPORT NSET: Import node set definitions from a previous ABAQUS/Explicit or ABAQUS/Standard analysis. This option is used to import node set definitions that were defined in a previous ABAQUS/Explicit or ABAQUS/Standard analysis. If the *IMPORT NSET option is used, it must appear after the *IMPORT option. If this option is omitted or is specified without any data lines, all the node sets relevant to the analysis will be imported.
* INCIDENT WAVE 9.8 *INCIDENT WAVE: boundary. Define incident wave loading for a blast or scattering load on a The preferred interface for applying incident wave loading is the *INCIDENT WAVE INTERACTION option used in conjunction with the *INCIDENT WAVE INTERACTION PROPERTY option. The alternative interface uses the *INCIDENT WAVE option to apply incident wave loading. The alternative interface will be removed in a subsequent release.
* INCIDENT WAVE PRESSURE AMPLITUDE Set this parameter equal to the name of the amplitude curve defining the fluid pressure time history at the standoff point (“Amplitude curves,” Section 27.1.2 of the ABAQUS Analysis User’s Manual). The corresponding fluid traction, if required, will be computed from the pressure amplitude reference. Data lines to define an incident wave: First line: 1. Surface name. 2. Reference magnitude.
* INCIDENT WAVE FLUID PROPERTY 9.9 *INCIDENT WAVE FLUID PROPERTY: incident wave. Define the fluid properties associated with an The preferred interface for defining the fluid properties for an incident wave is the *INCIDENT WAVE INTERACTION PROPERTY option used in conjunction with the *INCIDENT WAVE INTERACTION option. The alternative interface uses the *INCIDENT WAVE FLUID PROPERTY option to define the fluid properties used to define an incident wave.
* INCIDENT WAVE INTERACTION 9.10 *INCIDENT WAVE INTERACTION: scattering load on a surface. Define incident wave loading for a blast or This option is used to apply incident wave loading. The *INCIDENT WAVE INTERACTION PROPERTY option must be used in conjunction with the *INCIDENT WAVE INTERACTION option. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be modeled with the *INCIDENT WAVE REFLECTION option.
* INCIDENT WAVE INTERACTION PRESSURE AMPLITUDE Set this parameter equal to the name of the amplitude curve defining the fluid pressure time history at the standoff point (“Amplitude curves,” Section 27.1.2 of the ABAQUS Analysis User’s Manual). The corresponding fluid traction, if required, will be computed from the pressure amplitude reference. UNDEX Include this parameter to define a spherical incident wave using the *UNDEX CHARGE PROPERTY option.
* INCIDENT WAVE INTERACTION PROPERTY 9.11 *INCIDENT WAVE INTERACTION PROPERTY: properties describing an incident wave. Define the geometric data and fluid This option defines the geometric data and fluid properties used to define incident waves. Each *INCIDENT WAVE INTERACTION option must refer to an *INCIDENT WAVE INTERACTION PROPERTY definition. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • “Acoustic loads,” Section 27.4.
* INCIDENT WAVE PROPERTY 9.12 *INCIDENT WAVE PROPERTY: wave. Define the geometric data describing an incident The preferred interface for defining the geometric data for an incident wave is the *INCIDENT WAVE INTERACTION PROPERTY option used in conjunction with the *INCIDENT WAVE INTERACTION option. The alternative interface uses the *INCIDENT WAVE PROPERTY option to define the geometric data for incident waves. The alternative interface will be removed in a subsequent release.
* INCIDENT WAVE PROPERTY 4. X-component of , the velocity of the incident wave standoff point. 5. Y-component of , the velocity of the incident wave standoff point. 6. Z-component of , the velocity of the incident wave standoff point. Second line: 1. X-coordinate of , the position of the incident wave source point. Alternatively, specify the name of an *AMPLITUDE definition describing the time history of this coordinate. 2. Y-coordinate of , the position of the incident wave source point.
* INCIDENT WAVE REFLECTION 9.13 *INCIDENT WAVE REFLECTION: incident wave fields. Define the reflection load on a surface caused by This option is used to define reflected incident wave fields. It must be used in conjunction with the *INCIDENT WAVE INTERACTION option (preferred interface for applying incident wave loading) or the *INCIDENT WAVE option (alternative interface). The alternative interface will be removed in a subsequent release.
* INCLUDE 9.14 *INCLUDE: Reference an external file containing ABAQUS input data. This option is used to reference an external file containing a portion of the ABAQUS input file. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model or history data Level: Part, Part instance, Assembly, Model, Step Reference: • “Defining a model in ABAQUS,” Section 1.3.1 of the ABAQUS Analysis User’s Manual Required parameter: INPUT Set this parameter equal to the name of the file containing the input data.
* INCREMENTATION OUTPUT 9.15 *INCREMENTATION OUTPUT: incrementation data. Define output database requests for time This option is used to write incrementation variables to the output database. It must be used in conjunction with the *OUTPUT, HISTORY option. Product: ABAQUS/Explicit Type: History data Level: Step References: • • “Output to the output database,” Section 4.1.
* INELASTIC HEAT FRACTION 9.16 *INELASTIC HEAT FRACTION: Define the fraction of the rate of inelastic dissipation that appears as a heat source. This option is used to provide for inelastic energy dissipation to act as a heat source in adiabatic thermo-mechanical problems. It is relevant when the ADIABATIC parameter is included on the *DYNAMIC or the *STATIC option.
* INERTIA RELIEF 9.17 *INERTIA RELIEF: Apply inertia-based load balancing. This option is used to apply inertia-based loads on a free or partially constrained body. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Inertia relief,” Section 11.1.1 of the ABAQUS Analysis User’s Manual “Distributed loads,” Section 27.4.
* INERTIA RELIEF There are no data lines when the FIXED or REMOVE parameters are specified. 9.
* INITIAL CONDITIONS 9.18 *INITIAL CONDITIONS: Specify initial conditions for the model. This option is used to prescribe initial conditions for an analysis. Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/Aqua Type: Model data Level: Model Reference: • “Initial conditions,” Section 27.2.
* INITIAL CONDITIONS Set TYPE=PORE PRESSURE to give initial pore fluid pressures for a coupled pore fluid diffusion/stress analysis in ABAQUS/Standard. Set TYPE=POROSITY to give initial porosity values for materials defined with the *EOS COMPACTION option in ABAQUS/Explicit. Set TYPE=PRESSURE STRESS to give initial pressure stresses for a mass diffusion analysis in ABAQUS/Standard.
* INITIAL CONDITIONS Set TYPE=TEMPERATURE to give initial temperatures. The STEP and INC parameters can be used in conjunction with the FILE parameter to define initial temperatures from the results or output database file of a previous ABAQUS/Standard heat transfer analysis. Set TYPE=VELOCITY to prescribe initial velocities. Initial velocities should be defined in the global directions, regardless of the use of the *TRANSFORM option. STEP This parameter is used only with the FILE parameter.
* INITIAL CONDITIONS INPUT Set this parameter equal to the name of the alternate input file containing the data lines for this option. See “Input syntax rules,” Section 1.2.1 of the ABAQUS Analysis User’s Manual, for the syntax of such file names. If this parameter is omitted, it is assumed that the data follow the keyword line. INTERPOLATE Include this parameter in conjunction with the FILE, STEP, and INC parameters to indicate that the temperature field needs to be interpolated between dissimilar meshes.
* INITIAL CONDITIONS SECTION POINTS This parameter is used only with TYPE=PLASTIC STRAIN, TYPE=STRESS, and TYPE=HARDENING to specify plastic strains, stresses, and hardening variables at individual section points through the thickness of a shell element. This parameter can be used only when shell properties are defined using the *SHELL SECTION option. It cannot be used when properties are defined using the *SHELL GENERAL SECTION option. UNBALANCED STRESS This parameter is used only with TYPE=STRESS.
* INITIAL CONDITIONS 7. X-coordinate of the second reference point. 8. Y-coordinate of the second reference point. 9. Z-coordinate of the second reference point. Data lines for TYPE=CONCENTRATION: First line: 1. Node set or node number. 2. Initial normalized concentration value at the node. Repeat this data line as often as necessary to define the initial normalized concentration at various nodes or node sets. Data lines for TYPE=CONTACT: First line: 1. Slave surface name. 2. Master surface name. 3.
* INITIAL CONDITIONS to read for any node is based on the maximum number of field variable values for all the nodes in the model. These trailing initial values will be zero and will not be used in the analysis. Repeat this set of data lines as often as necessary to define initial temperatures at various nodes or node sets. No data lines are required for TYPE=FIELD, VARIABLE=n, FILE=file, STEP=step, INC=inc. Data lines for TYPE=FLUID PRESSURE: First line: 1.
* INITIAL CONDITIONS Data lines for TYPE=HARDENING, REBAR: First line: 1. Element number or element set label. 2. Rebar name. If this field is left blank, the initial conditions will be applied to all rebars in the model. . 3. Initial equivalent plastic strain, . (Only relevant for the kinematic hardening models.) 4. Initial backstress, Repeat this data line as often as necessary to define the hardening parameters for rebars in various elements or element sets.
* INITIAL CONDITIONS 2. Initial mass flow rate per unit area in the x-direction or total initial mass flow rate in the crosssection for one-dimensional elements. 3. Initial mass flow rate per unit area in the y-direction (not needed for nodes associated with one-dimensional convective flow elements). 4. Initial mass flow rate per unit area in the z-direction (not needed for nodes associated with one-dimensional convective flow elements).
* INITIAL CONDITIONS 5. Value of third plastic strain component, . Give the initial plastic strain components as defined for this element type in Part VI, “Elements,” of the ABAQUS Analysis User’s Manual. In any element for which an *ORIENTATION option applies, the plastic strain components must be given in the local system (“Orientations,” Section 2.2.5 of the ABAQUS Analysis User’s Manual).
* INITIAL CONDITIONS No data lines are required for TYPE=PRESSURE STRESS, FILE=file, STEP=step, INC=inc. Data lines for TYPE=RATIO if the USER parameter is omitted: First line: 1. Node set or node number. 2. First value of void ratio. 3. Vertical coordinate corresponding to the above value. 4. Second value of void ratio. 5. Vertical coordinate corresponding to the above value. Omit the elevation values and the second void ratio value to define a constant void ratio distribution.
* INITIAL CONDITIONS Data lines for TYPE=RELATIVE DENSITY: First line: 1. Node set or node number. 2. Initial relative density. Repeat this data line as often as necessary to define initial relative density at various nodes or node sets. Data lines for TYPE=ROTATING VELOCITY: First line: 1. Node set or node number. 2. Angular velocity about the axis defined from point a to point b, where the coordinates of a and b are given below. 3. Global X-component of translational velocity. 4.
* INITIAL CONDITIONS Subsequent lines (only needed if more than seven solution-dependent state variables exist in the model): 1. Value of eighth solution-dependent state variable. 2. Etc., up to eight solution-dependent state variables per line.
* INITIAL CONDITIONS 2. Initial specific energy. Repeat this data line as often as necessary to define initial specific energy in various elements or element sets. Data lines for TYPE=SPUD EMBEDMENT: First line: 1. Element set or element number. 2. Spud can embedment, . Repeat this data line as often as necessary to define initial embedment for various elements or element sets. Data lines for TYPE=SPUD PRELOAD: First line: 1. Element set or element number. . 2.
* INITIAL CONDITIONS 3. Vertical coordinate corresponding to the above value. 4. Second value of vertical component of (effective) stress. 5. Vertical coordinate corresponding to the above value. 6. First coefficient of lateral stress. This coefficient defines the x-direction stress components. 7. Second coefficient of lateral stress. This coefficient defines the y-direction stress component in three-dimensional cases and the thickness or hoop direction component in plane or axisymmetric cases.
* INITIAL CONDITIONS No data lines are required for TYPE=STRESS, USER. Data lines for TYPE=TEMPERATURE: First line: 1. Node set or node number. 2. First initial temperature value at the node or node set. For shells and beams several values (or a value and the temperature gradients across the section) can be given at each node (see “Using a beam section integrated during the analysis to define the section behavior,” Section 23.3.
* INITIAL CONDITIONS Data lines for TYPE=VELOCITY: First line: 1. Node set or node number. 2. Degree of freedom. 3. Value of initial velocity. Repeat this data line as often as necessary to define the initial velocity at various nodes or node sets. 9.
* INSTANCE 9.19 *INSTANCE: Begin an instance definition. This option is used to instance a part within an assembly. It must be used in conjunction with the *ASSEMBLY and *END INSTANCE options. If the instance is not imported from a previous analysis, the *INSTANCE option must be used in conjunction with the *PART option. When importing a part instance from a previous analysis, the *INSTANCE option must be used in conjunction with the *IMPORT option.
* INSTANCE Data line to translate an instance that is not imported from a previous analysis: First (and only) line: 1. Value of the translation to be applied in the X-direction. 2. Value of the translation to be applied in the Y-direction. 3. Value of the translation to be applied in the Z-direction. Data lines to translate and/or rotate an instance that is not imported from a previous analysis: First line: 1. Value of the translation to be applied in the X-direction. 2.
* INSTANCE b θ θ a Figure 9.19–1 Rotation of an instance. 9.
* INTEGRATED OUTPUT 9.20 *INTEGRATED OUTPUT: the output database. Specify variables integrated over a surface to be written to This option is used to write integrated quantities over a surface, such as the total force transmitted across a surface, to the output database. It must be used in conjunction with the *OUTPUT, HISTORY option. Product: ABAQUS/Explicit Type: History data Level: Step References: • • • • • “Output to the output database,” Section 4.1.
* INTEGRATED OUTPUT Data lines to request integrated output: First line: 1. Specify the identifying keys for the output variables to be written to the output database. The keys are defined in “ABAQUS/Explicit output variable identifiers,” Section 4.2.2 of the ABAQUS Analysis User’s Manual. Repeat this data line as often as necessary to define the list of variables to be written to the output database. 9.
* INTEGRATED OUTPUT SECTION 9.21 *INTEGRATED OUTPUT SECTION: Define an integrated output section over a surface with a local coordinate system and a reference point. This option is used to associate a surface with a coordinate system and/or a reference node to track the average motion of the surface. It can also be used in conjunction with an integrated output request to obtain output of quantities integrated over a surface.
* INTEGRATED OUTPUT SECTION Set POSITION=CENTER if the reference node is to be relocated from the user-defined location to the center of the surface in the initial configuration. PROJECT ORIENTATION Set PROJECT ORIENTATION=NO (default) if the initial coordinate system of the section should not be projected onto the section surface. If the ORIENTATION parameter is included, this choice results in an initial coordinate system that matches the defined orientation.
* INTERACTION OUTPUT 9.22 *INTERACTION OUTPUT: output database. Specify spot weld interaction variables to be written to the This option is used to write spot weld interaction variables to the output database. It must be used in conjunction with the *OUTPUT, HISTORY option. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step References: • • • “Output to the output database,” Section 4.1.3 of the ABAQUS Analysis User’s Manual “Mesh-independent fasteners,” Section 28.3.
* INTERACTION PRINT 9.23 *INTERACTION PRINT: Define print requests for spot weld interaction variables. This option is used to provide tabular printed output of spot weld interaction variables. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Output to the data and results files,” Section 4.1.2 of the ABAQUS Analysis User’s Manual “Mesh-independent fasteners,” Section 28.3.
* INTERACTION PRINT Data lines to request spot weld interaction variable output to the data file: First line: 1. Give the identifying keys for the variables to be written to the data file. The keys are defined in “ABAQUS/Standard output variable identifiers,” Section 4.2.1 of the ABAQUS Analysis User’s Manual. Repeat this data line as often as necessary: each line defines a table. If this line is omitted, the default variables will be output. 9.
* INTERFACE 9.24 *INTERFACE: Define properties for contact elements. This option is used to assign element section properties to ITT-, ISL-, IRS-, and ASI-type contact elements. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance, Assembly References: • • • • “Acoustic interface elements,” Section 26.14.1 of the ABAQUS Analysis User’s Manual “Tube-to-tube contact elements,” Section 31.3.1 of the ABAQUS Analysis User’s Manual “Slide line contact elements,” Section 31.4.
* INTERFACE Data line for ASI1 elements: First (and only) line: 1. Area associated with the elements. Enter the direction cosine, in terms of the global Cartesian coordinate system, of the interface normal that points into the acoustic fluid: 2. X-direction cosine. 3. Y-direction cosine. 4. Z-direction cosine. Data line for ASI-type elements for use with 2-D elements: First (and only) line: 1. Element thickness. The default is unit thickness.
* ITS 9.25 *ITS: Define properties for ITS elements. This option is used to define the properties for ITS-type elements. The *DASHPOT, *FRICTION, and *SPRING options must immediately follow this option. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • • • “Rigid surface contact elements,” Section 31.5.
* ITS 2. Diameter of the hole in the support plate. 3. X-direction cosine of the axis of the tube. 4. Y-direction cosine of the axis of the tube. 5. Z-direction cosine of the axis of the tube. 9.
J 10.
* JOINT 10.1 *JOINT: Define properties for JOINTC elements. This option is used to define the properties for JOINTC elements. The *DASHPOT and *SPRING options must immediately follow this option. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • • “Flexible joint element,” Section 26.3.
* JOINT ELASTICITY 10.2 *JOINT ELASTICITY: Specify elastic properties for elastic-plastic joint elements. This option is used to define linear elastic moduli for elastic-plastic joint elements. It can be used only in conjunction with the *EPJOINT option. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • “Elastic-plastic joints,” Section 26.11.1 of the ABAQUS Analysis User’s Manual *EPJOINT Required parameters: MODULI Set MODULI=SPUD CAN to define spud can moduli.
* JOINT ELASTICITY 5. 6. 7. 8. Temperature. First field variable. Second field variable. Third field variable. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than three): 1. Fourth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the elastic behavior as a function of temperature and other predefined field variables. Data lines for MODULI=SPUD CAN and NDIM=3: First line: 1.
* JOINT ELASTICITY 7. Temperature. 8. First field variable. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than one): 1. Second field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the elastic behavior as a function of temperature and other predefined field variables. Data lines for MODULI=GENERAL and NDIM=3: First line: 1. 2. 3. 4. 5. 6. 7. 8. . . . . . . . . Second line: 1. 2. 3. 4. 5. 6. 7. 8.
* JOINT ELASTICITY 7. First field variable. 8. Second field variable. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than two): 1. Third field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the elastic behavior as a function of temperature and other predefined field variables. 10.
* JOINT PLASTICITY 10.3 *JOINT PLASTICITY: Specify plastic properties for elastic-plastic joint elements. This option is used to define the plastic behavior for elastic-plastic joint elements. It can be used only in conjunction with the *EPJOINT option. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • “Elastic-plastic joints,” Section 26.11.
* JOINT PLASTICITY 7. First field variable. 8. Second field variable. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than two): 1. Third field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the plastic behavior as a function of temperature and other predefined field variables. Data lines for TYPE=CLAY: First line: 1. 2. 3. 4. 5. 6. 7. 8. , undrained shear strength of the clay. a, hardening parameter.
* JOINT PLASTICITY Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than three): 1. Fourth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the plastic behavior as a function of temperature and other predefined field variables. 10.
* JOINTED MATERIAL 10.4 *JOINTED MATERIAL: Specify the jointed material model. This option is used to define a failure surface and the flow parameters for a single joint system or for bulk material failure in the elastic-plastic model of a jointed material, or it can be used to define shear retention in open joints. Up to three joint systems can be defined for each material point. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Jointed material model,” Section 18.4.
* JOINTED MATERIAL Data lines defining failure surface and flow parameters (SHEAR RETENTION omitted): First line: 1. Angle of friction, , for this system. Give the value in degrees. 2. Dilation angle, , for this system. Give the value in degrees. 3. Cohesion, d, for this system. (Units of FL−2 .) 4. Temperature. 5. First field variable. 6. Second field variable. 7. Etc., up to four field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than four): 1.
* JOULE HEAT FRACTION 10.5 *JOULE HEAT FRACTION: Define the fraction of electric energy released as heat. This option is used to specify the fraction of dissipated electrical energy released as heat in coupled thermalelectrical problems. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Coupled thermal-electrical analysis,” Section 6.6.2 of the ABAQUS Analysis User’s Manual There are no parameters associated with this option.
K 11.
* KAPPA 11.1 and for mass diffusion driven by *KAPPA: Specify the material parameters gradients of temperature and equivalent pressure stress, respectively. This option is used to introduce temperature- and pressure-driven mass diffusion. It must appear immediately after the *DIFFUSIVITY option. For each use of the *DIFFUSIVITY option, *KAPPA can be used once with TYPE=TEMP and once with TYPE=PRESS. The *KAPPA, TYPE=TEMP and *DIFFUSIVITY, LAW=FICK options are mutually exclusive.
* KAPPA Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define temperature, and other predefined field variables. as a function of concentration, Data lines to define the pressure stress factor, k p (TYPE=PRESS): First line: 1. Pressure stress factor, . (Units of LF−1/2 .) 2. Concentration, c. 3. Temperature, . 4.
* KINEMATIC 11.2 *KINEMATIC: Define a kinematic coupling constraint. This option is used to define a kinematic coupling constraint. It must be used in conjunction with the *COUPLING option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly References: • • “Coupling constraints,” Section 28.3.2 of the ABAQUS Analysis User’s Manual *COUPLING There are no parameters associated with this option.
* KINEMATIC COUPLING 11.3 *KINEMATIC COUPLING: Constrain all or specific degrees of freedom of a set of nodes to the rigid body motion of a reference node. This option is used to impose constraints between degrees of freedom of a node or node set and the rigid body motion defined by a reference node. The preferred method of providing a kinematic constraint of this type is the *COUPLING option used in conjunction with the *KINEMATIC option.
* KINEMATIC COUPLING 3. Last degree of freedom constrained. If this field is left blank, the degree of freedom specified in the second field will be the only one constrained. Repeat this data line as often as necessary to specify constraints at different nodes and degrees of freedom. When the ORIENTATION parameter is specified, the degrees of freedom are in the referenced local system in the initial configuration; otherwise, they are in the global system.
L 12.
* LATENT HEAT 12.1 *LATENT HEAT: Specify latent heats. This option is used to specify a material’s latent heat. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model Reference: • “Latent heat,” Section 20.2.4 of the ABAQUS Analysis User’s Manual There are no parameters associated with this option. Data lines to define a material’s latent heat: First line: 1. Latent heat per unit mass. (Units of JM−1 .) 2. Solidus temperature. 3. Liquidus temperature.
* LOAD CASE 12.2 *LOAD CASE: Begin a load case definition for multiple load case analysis. This option is used to begin each load case definition. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Multiple load case analysis,” Section 6.1.3 of the ABAQUS Analysis User’s Manual *END LOAD CASE Required parameter: NAME Set this parameter equal to a label that will be used to refer to the load case. There are no data lines associated with this option. 12.
M 13.
* MAP SOLUTION 13.1 *MAP SOLUTION: Map a solution from an old mesh to a new mesh. This option is used to transfer solution variables from an earlier analysis to a new mesh that occupies the same space. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Mesh-to-mesh solution mapping,” Section 12.4.1 of the ABAQUS Analysis User’s Manual Optional parameters: INC Set this parameter equal to the increment number from which the old solution will be read.
* MAP SOLUTION 2. Value of the translation to be applied in the Y-direction. 3. Value of the translation to be applied in the Z-direction. Enter values of zero to apply a pure rotation. Second line: 1. X-coordinate of point a on the axis of rotation (see Figure 13.1–1). 2. Y-coordinate of point a on the axis of rotation. 3. Z-coordinate of point a on the axis of rotation. 4. X-coordinate of point b on the axis of rotation. 5. Y-coordinate of point b on the axis of rotation. 6.
* MASS 13.2 *MASS: Specify a point mass. This option is used to define lumped mass values associated with MASS elements. For ABAQUS/Standard analyses this option is also used to define mass proportional damping (for directintegration dynamic analysis) and composite damping (for modal dynamic analysis) associated with MASS elements. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly Reference: • “Point masses,” Section 24.1.
* MASS Data line to define the mass magnitude: First (and only) line: 1. Mass magnitude. Mass, not weight, should be given. ABAQUS does not use any specific physical units, so the user’s choice must be consistent. 13.
* MASS DIFFUSION 13.3 *MASS DIFFUSION: Transient or steady-state uncoupled mass diffusion analysis. This option is used to control uncoupled transient or steady-state mass diffusion analysis. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Mass diffusion analysis,” Section 6.8.1 of the ABAQUS Analysis User’s Manual Optional parameters: DCMAX Set this parameter equal to the maximum normalized concentration change to be allowed in an increment.
* MASS DIFFUSION If a value is given, ABAQUS/Standard will use the minimum of the given value and 0.8 times the suggested initial time step. 4. Maximum time increment. If this value is omitted, no upper limit is imposed. This value is used only for automatic time incrementation. 5. Rate of change of normalized concentration (normalized concentration per time) used to define steady state; only needed if END=SS is chosen.
* MASS FLOW RATE 13.4 *MASS FLOW RATE: Specify fluid mass flow rate in a heat transfer analysis. This option is used to specify the mass flow rate per unit area (or through the entire section for one-dimensional elements) for forced convection/diffusion elements in a heat transfer analysis. This option cannot be used with hydrostatic fluid elements. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Uncoupled heat transfer analysis,” Section 6.5.
* MASS FLOW RATE Data lines to define mass flow rates: First line: 1. Node number or node set label. 2. Mass flow rate per unit area in the x-direction (units of ML−2 T−1 ) or total mass flow rate in the cross-section (units of MT−1 ) for one-dimensional elements. 3. Mass flow rate per unit area in the y-direction (not needed for nodes associated with onedimensional elements). 4. Mass flow rate per unit area in the z-direction (not needed for nodes associated with onedimensional elements).
* MATERIAL 13.5 *MATERIAL: Begin the definition of a material. This option is used to indicate the start of a material definition. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model Reference: • “Material data definition,” Section 16.1.2 of the ABAQUS Analysis User’s Manual Required parameter: NAME Set this parameter equal to a label that will be used to refer to the material in the element property options. Material names in the same input file must be unique.
* MATERIAL Set STRAIN RATE REGULARIZATION=LINEAR to use a linear regularization for strain rate-dependent material data. There are no data lines associated with this option. 13.
* MATRIX 13.6 *MATRIX: Read in the stiffness or mass matrix for a linear user element. This option can be used only in conjunction with the *USER ELEMENT, LINEAR option. It is used to read in the stiffness or mass matrix for the user element. It can be used once if only a stiffness or mass is required or twice to give both matrices. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance, Model References: • • “User-defined elements,” Section 26.15.
* MATRIX ASSEMBLE 13.7 *MATRIX ASSEMBLE: Define stiffness or mass matrices for a part of the model. This option can be used to identify a stiffness or a mass matrix that will be assembled into the corresponding global finite element matrix. This matrix must have been input previously by using the *MATRIX INPUT option. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Defining matrices,” Section 2.10.
* MATRIX INPUT 13.8 *MATRIX INPUT: Read in a matrix for a part of the model. This option can be used to input a matrix in sparse format. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Defining matrices,” Section 2.10.1 of the ABAQUS Analysis User’s Manual *MATRIX ASSEMBLE Required parameter: NAME Set this parameter equal to a label that will be used to refer to this matrix.
* MATRIX INPUT 4. Degree of freedom number for column node. 5. Matrix entry. Give data to define a symmetric matrix in lower triangular, upper triangular, or square format. For a square matrix to be symmetric, corresponding entries above and below the diagonal must have exactly the same values. Repeat this data line as often as necessary. 13.
* MEMBRANE SECTION 13.9 *MEMBRANE SECTION: Specify section properties for membrane elements. This option is used to assign section properties to a set of membrane elements. Section properties include thickness, thickness change behavior, material definition, and material orientation. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance Reference: • “Membrane elements,” Section 23.1.
* MEMBRANE SECTION NODAL THICKNESS Include this parameter to indicate that the membrane thickness should not be read from the data lines but should be interpolated from the thickness specified at the nodes with the *NODAL THICKNESS option. ORIENTATION Set this parameter equal to the name given for the *ORIENTATION option to be used to define a local coordinate system for material calculations in the elements in this set. POISSON This parameter is relevant only in a large-deformation analysis.
* MODAL DAMPING 13.10 *MODAL DAMPING: Specify damping for modal dynamic analysis. This option is used to specify damping for mode-based procedures. It is usually used in conjunction with the *SELECT EIGENMODES option for selecting eigenmodes for modal superposition. If the *SELECT EIGENMODES option is not used, all eigenmodes extracted in the prior *FREQUENCY step will be used with the damping values specified under the *MODAL DAMPING option.
* MODAL DAMPING analysis,” Section 6.3.11 of the ABAQUS Analysis User’s Manual). The value of the damping constant, s, that multiplies the internal forces is entered on the data line. Optional parameter: DEFINITION Set DEFINITION=MODE NUMBERS (default) to indicate that the damping values are given for the specified mode numbers. Set DEFINITION=FREQUENCY RANGE to indicate that the damping values are given for the specified frequency ranges. Frequency ranges can be discontinuous.
* MODAL DAMPING Data lines to define structural damping by specifying mode numbers (STRUCTURAL and DEFINITION=MODE NUMBERS): First line: 1. Mode number of the lowest mode of a range. 2. Mode number of the highest mode of a range. (If this entry is left blank, it is assumed to be the same as the previous entry so that values are being given for one mode only.) 3. Damping factor, s. Repeat this data line as often as necessary to define modal damping for different modes.
* MODAL DYNAMIC 13.11 *MODAL DYNAMIC: Dynamic time history analysis using modal superposition. This option is used to provide dynamic time history response as a linear perturbation procedure using modal superposition. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Transient modal dynamic analysis,” Section 6.3.
* MODAL FILE 13.12 *MODAL FILE: Write generalized coordinate (modal amplitude) data or eigendata to the results file during a mode-based dynamic or eigenvalue extraction procedure. This option is used during mode-based dynamic or eigenvalue extraction procedures to control the writing of generalized coordinate (modal amplitude and phase) values or eigendata to the ABAQUS/Standard results file.
* MODAL OUTPUT 13.13 *MODAL OUTPUT: Write generalized coordinate (modal amplitude) data to the output database during a mode-based dynamic or complex eigenvalue extraction procedure. This option is used during a mode-based dynamic or complex eigenvalue extraction procedure to write generalized coordinate (modal amplitude and phase) values to the ABAQUS/Standard output database. It must be used in conjunction with the *OUTPUT, HISTORY option.
* MODAL PRINT 13.14 *MODAL PRINT: Print generalized coordinate (modal amplitude) data during a modebased dynamic procedure. This option is used during mode-based dynamic procedures to control the printed output of generalized coordinate (modal amplitude and phase) values. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Output to the data and results files,” Section 4.1.
* MODEL CHANGE 13.15 *MODEL CHANGE: Remove or reactivate elements and contact pairs. This option is used to remove or reactivate elements or contact pairs during an analysis. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Element and contact pair removal and reactivation,” Section 11.2.1 of the ABAQUS Analysis User’s Manual “Removing/reactivating ABAQUS/Standard contact pairs,” Section 29.2.
* MODEL CHANGE Data lines to remove/reactivate elements (TYPE=ELEMENT): First line: 1. Give a list of element numbers and/or element set names that are involved in the removal or reactivation. Repeat this data line as often as necessary. Data lines to remove/reactivate contact pairs (TYPE=CONTACT PAIR): First line: 1. Slave surface name used in the contact pair being removed or reactivated. 2. Master surface name used in the contact pair being removed or reactivated.
* MOHR COULOMB 13.16 *MOHR COULOMB: Specify the Mohr-Coulomb plasticity model. This option is used to define the yield surface and flow potential parameters for elastic-plastic materials that use the Mohr-Coulomb plasticity model. It must be used in conjunction with the *MOHR COULOMB HARDENING option. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Mohr-Coulomb plasticity,” Section 18.3.
* MOHR COULOMB 2. Dilation angle, , at high confining pressure in the p– plane. Give the value in degrees. 3. Temperature. 4. First field variable. 5. Second field variable. 6. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line.
* MOHR COULOMB HARDENING 13.17 *MOHR COULOMB HARDENING: model. Specify hardening for the Mohr-Coulomb plasticity This option is used to define piecewise linear hardening/softening behavior for a material defined by the MohrCoulomb plasticity model. It must be used in conjunction with the *MOHR COULOMB option. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Mohr-Coulomb plasticity,” Section 18.3.
* MOHR COULOMB HARDENING 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of the cohesion yield stress on plastic strain and, if needed, on temperature and other predefined field variables. 13.
* MOISTURE SWELLING 13.18 *MOISTURE SWELLING: Define moisture-driven swelling. This option is used to define the moisture-driven swelling of the solid skeleton in a partially saturated porous medium. It can be used in the analysis of coupled wetting liquid flow and porous medium stress. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Moisture swelling,” Section 20.7.6 of the ABAQUS Analysis User’s Manual There are no parameters associated with this option.
* MOLECULAR WEIGHT 13.19 *MOLECULAR WEIGHT: Define the molecular weight of an ideal gas species. This option is used to define the molecular weight of an ideal gas species. It can be used only in conjunction with the *FLUID BEHAVIOR option. Product: ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • • • “Defining fluid cavities,” Section 11.6.2 of the ABAQUS Analysis User’s Manual “Defining inflators,” Section 11.6.
* MONITOR 13.20 *MONITOR: Define a degree of freedom to monitor. This option is used to choose a node and degree of freedom to monitor the progress of the solution in the status file. In ABAQUS/Standard the information will also be written to the message file. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step Reference: • “Output,” Section 4.1.
* MOTION 13.21 *MOTION: Specify motions as a predefined field. This option is used to specify motions of node sets or individual nodes during cavity radiation heat transfer analysis, to define the motion of a reference frame in steady-state transport analysis, or to define the velocity of the material transported through the mesh during a static analysis. Product: ABAQUS/Standard Type: History data Level: Step References: • • • • “Cavity radiation,” Section 32.1.
* MOTION is given with TYPE=VELOCITY, the default is a STEP function for cavity radiation analysis and a RAMP function for steady-state transport analysis. TYPE This parameter is used to specify whether the magnitude is in the form of a displacement or a velocity. Set TYPE=DISPLACEMENT (default for cavity radiation analysis) to give translational or rotational displacement values.
* MOTION The following data are required only for three-dimensional cases: 5. Global z-component of point a on the axis of rotation. 6. Global x-component of point b on the axis of rotation. 7. Global y-component of point b on the axis of rotation. 8. Global z-component of point b on the axis of rotation. Repeat this data line as often as necessary to define rotational motion for different nodes. Data lines to define motion in user subroutine UMOTION (USER): First line: 1. Node set label or node number.
* MPC 13.22 *MPC: Define multi-point constraints. This option is used to impose constraints between different degrees of freedom of the model. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly References: • • “General multi-point constraints,” Section 28.2.2 of the ABAQUS Analysis User’s Manual “MPC,” Section 1.1.
* MPC the following nodes on this line. Any number of continuation lines are allowed. Exactly 15 nodes or node sets must be given on each line except the last line. 13.
* MULLINS EFFECT 13.23 *MULLINS EFFECT: Specify Mullins effect material parameters for elastomers. This option is used to define material constants for the Mullins effect in filled rubber elastomers or for modeling energy dissipation in elastomeric foams. It can be used only with the *HYPERELASTIC or the *HYPERFOAM options. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • • • • • • “Hyperelastic behavior of rubberlike materials,” Section 17.5.
* MULLINS EFFECT cannot be specified if both the R and M parameters are also specified (use the data line instead to specify all three parameters). If this parameter is omitted, will be determined from a nonlinear, least-squares fit of the test data. Allowable values of BETA are . The M and BETA parameters cannot both be zero. DEPENDENCIES Set this parameter equal to the number of field variables, in addition to temperature, on which the material parameters depend.
* MULLINS EFFECT Data lines to define the material constants if both the TEST DATA INPUT and USER parameters are omitted: First line: 1. . 2. 3. . (If this entry is left blank, the default value is taken to be 0.0 in ABAQUS/Standard and 0.1 in ABAQUS/Explicit.) 4. Temperature. 5. First field variable. 6. Etc., up to four field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than four): 1. Fifth field variable. 2. Etc., up to eight field variables per line.
* M1 13.24 *M1: Define the first bending moment behavior of beams. This option is used to define the first bending moment behavior of beams. It can be used only in conjunction with the *BEAM GENERAL SECTION, SECTION=NONLINEAR GENERAL option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • “Using a general beam section to define the section behavior,” Section 23.3.
* M1 Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than six): 1. Seventh field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the bending stiffness as a function of temperature and other predefined field variables. Data lines if the LINEAR parameter is omitted: First line: 1. Bending moment. 2. Curvature. 3. Temperature. 4. First field variable. 5. Second field variable. 6. Etc.
* M2 13.25 *M2: Define the second bending moment behavior of beams. This option is used to define the second bending moment behavior of beams. It can be used only in conjunction with the *BEAM GENERAL SECTION, SECTION=NONLINEAR GENERAL option and is needed only for beams in space. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • “Using a general beam section to define the section behavior,” Section 23.3.
* M2 Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than six): 1. Seventh field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the bending stiffness as a function of temperature and other predefined field variables. Data lines if the LINEAR parameter is omitted: First line: 1. Bending moment. 2. Curvature. 3. Temperature. 4. First field variable. 5. Second field variable. 6. Etc.
N 14.
* NCOPY 14.1 *NCOPY: Create nodes by copying. This option is used to copy a node set to create a new node set. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance Reference: • “Node definition,” Section 2.1.1 of the ABAQUS Analysis User’s Manual Required parameters: CHANGE NUMBER Set this parameter equal to an integer that will be added to each of the existing node numbers to define the node numbers of the nodes being created.
* NCOPY Optional parameters: MULTIPLE This parameter is used with the SHIFT parameter to define the number of times the rotation should be applied. The default is MULTIPLE=1. NEW SET Set this parameter equal to the name of the node set to which the nodes created by the operation will be assigned. This new node set will be unsorted if the OLD SET was unsorted and if the NEW SET does not already exist. Otherwise, this new node set will be a sorted set.
* NCOPY 2. Y-coordinate of the first point defining the reflection plane. 3. Z-coordinate of the first point defining the reflection plane. 4. X-coordinate of the second point defining the reflection plane (point b in Figure 14.1–3). 5. Y-coordinate of the second point defining the reflection plane. 6. Z-coordinate of the second point defining the reflection plane. Second line: 1. X-coordinate of the third point defining the reflection plane (point c in Figure 14.1–3). 2.
* NCOPY b a Figure 14.1–1 *NCOPY, SHIFT option. a New Set b Old set a, b define the line Figure 14.1–2 *NCOPY, REFLECT=LINE option. 14.
* NCOPY New Set Old Set c b a a, b, c define the mirror plane Figure 14.1–3 *NCOPY, REFLECT=MIRROR option. a Old set New Set a is the point through which the nodes are reflected Figure 14.1–4 *NCOPY, REFLECT=POINT option. 14.
* NCOPY L L pole node a old set Figure 14.1–5 *NCOPY, POLE option. 14.
* NFILL 14.2 *NFILL: Fill in nodes in a region. This option is used to generate nodes for a region of a mesh by filling in nodes between two bounds. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance Reference: • “Node definition,” Section 2.1.1 of the ABAQUS Analysis User’s Manual Optional parameters: BIAS Include this parameter to bias the spacing of the nodes being generated toward one end of the line of nodes being generated.
* NFILL Data lines to fill in nodes between two bounds: First line: 1. Name of the node set defining the first bound of the region. 2. Name of the node set defining the second bound of the region. 3. Number of intervals along each line between bounding nodes. 4. Increment in node numbers from the node number at the first bound set end. The default is 1. Repeat this data line as often as necessary, one line per region to be filled by this option. 14.
* NGEN 14.3 *NGEN: Generate incremental nodes. This option is used to generate nodes incrementally. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance Reference: • “Node definition,” Section 2.1.1 of the ABAQUS Analysis User’s Manual Optional parameters: LINE Set LINE=P to generate the nodes along a parabola. In this case the user must define an extra point, the midpoint between the two end points. Set LINE=C to generate the nodes along a circular arc.
* NGEN 6. Second coordinate of the extra point (if required). 7. Third coordinate of the extra point (if required). The following entries are used only for a circular arc equal to or larger than 180°: 8. First component of a normal to the circular arc. 9. Second component of a normal to the circular arc. 10. Third component of a normal to the circular arc. Repeat this data line as often as necessary.
* NMAP 14.4 *NMAP: Map nodes from one coordinate system to another. This option is used to map a set of nodes from one coordinate system to another. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: This option is not supported in a model defined in terms of an assembly of part instances. Reference: • “Node definition,” Section 2.1.1 of the ABAQUS Analysis User’s Manual Required parameters: NSET Set this parameter equal to the name of the node set containing the nodes to be mapped.
* NMAP by the distance between points a and b. The line between points a and b defines the position. For every value of the -coordinate is defined in a plane perpendicular to the plane defined by the points a, b, and c and perpendicular to the axis of the toroidal system. lies in the plane defined by the points by a, b, and c. Set TYPE=BLENDED to map via blended quadratics in an ABAQUS/Standard analysis. Data lines for TYPE=RECTANGULAR, CYLINDRICAL, DIAMOND, SPHERICAL, or TOROIDAL: First line: 1. 2. 3. 4.
* NMAP 3. Y-coordinate of the point to which this control node is to be mapped. 4. Z-coordinate of the point to which this control node is to be mapped. Second line: 1. Node number of the second control node. 2. X-coordinate of the point to which this control node is to be mapped. 3. Y-coordinate of the point to which this control node is to be mapped. 4. Z-coordinate of the point to which this control node is to be mapped.
* NMAP ^ Z ^ Z d ^ Y z z a y x b y x ^ X b rectangular a ^ X skewed Cartesian ^ Z ^ Z b ^ Y c a c b (R, θ, φ) φ R θ (R, θ, Z) z y x z (θ = 0) ( φ = 0) c a y x spherical R θ c (θ = 0) cylindrical c (r, θ, φ) r θ z φ a y x R b (φ = 0) toroidal Figure 14.4–1 Coordinate systems; angles are in degrees. 14.
* NO COMPRESSION 14.5 *NO COMPRESSION: materials). Introduce a compressive failure theory (tension only This option is used to modify the elasticity definition so that no compressive stress is allowed. It can be used only in conjunction with the *ELASTIC option. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “No compression or no tension,” Section 17.2.2 of the ABAQUS Analysis User’s Manual *ELASTIC There are no parameters or data lines associated with this option. 14.
* NO TENSION 14.6 *NO TENSION: Introduce a tension failure theory (compression only material). This option is used to modify the elasticity definition so that no tensile stress is allowed. It can be used only in conjunction with the *ELASTIC option. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “No compression or no tension,” Section 17.2.2 of the ABAQUS Analysis User’s Manual *ELASTIC There are no parameters or data lines associated with this option. 14.
* NODAL THICKNESS 14.7 *NODAL THICKNESS: Define shell or membrane thickness at nodes. This option is used to define variable shell or membrane thicknesses on a nodal basis. The thickness data defined with this option will be ignored unless the NODAL THICKNESS parameter is included on either the *SHELL GENERAL SECTION or the *SHELL SECTION options for shell elements or on the *MEMBRANE SECTION option for membrane elements.
* NODAL THICKNESS Data lines when the GENERATE parameter is omitted: First line: 1. Node set label or node number. 2. Thickness. Repeat this data line as often as necessary to define the variation in shell or membrane thickness. Data lines when the GENERATE parameter is included: First line: 1. Node number or node set label that defines the first bound for the generate operation. 2. Node number or node set label that defines the second bound for the generate operation. 3.
* NODE 14.8 *NODE: Specify nodal coordinates. This option is used to define a node directly by specifying its coordinates. Nodal coordinates given in this option are in a local system if the *SYSTEM option is in effect when this option is used. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly Reference: • “Node definition,” Section 2.1.
* NODE 4. Third coordinate of the node. 5. First direction cosine of the normal at the node (optional). 6. Second direction cosine of the normal at the node (optional). For nodes entered in a cylindrical or spherical system, this entry is an angle given in degrees. 7. Third direction cosine of the normal at the node (optional). For nodes entered in a spherical system, this entry is an angle given in degrees. The normal will be used only for element types with rotational degrees of freedom.
* NODE FILE 14.9 *NODE FILE: Define results file requests for nodal data. This option is used to choose the nodal variables that will be written to the results (.fil) file in an ABAQUS/Standard analysis or to the selected results (.sel) file in an ABAQUS/Explicit analysis. In an ABAQUS/Explicit analysis it must be used in conjunction with the *FILE OUTPUT option.
* NODE FILE The default value is LAST MODE=N, where N is the number of modes extracted. If the MODE parameter is used, the default value is LAST MODE=M, where M is the value of the MODE parameter. MODE This parameter applies only to ABAQUS/Standard analyses. This parameter is useful only during eigenvalue extraction for natural frequencies and for eigenvalue buckling estimation. Set this parameter equal to the first mode number for which output is required. The default is MODE=1.
* NODE OUTPUT 14.10 *NODE OUTPUT: Define output database requests for nodal data. This option is used to write nodal variables to the output database. It must be used in conjunction with the *OUTPUT option. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step References: • • “Output to the output database,” Section 4.1.
* NODE OUTPUT Optional parameter: VARIABLE Set VARIABLE=ALL to indicate that all nodal variables applicable to this procedure and material type should be written to the output database. Set VARIABLE=PRESELECT to indicate that the default nodal output variables for the current procedure type should be written to the output database. Additional output variables can be requested on the data lines. If this parameter is omitted, the nodal variables requested for output must be specified on the data lines.
* NODE PRINT 14.11 *NODE PRINT: Define print requests for nodal variables. This option is used to provide tabular printed output of nodal variables (displacements, reaction forces, etc.) in the data file. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Output to the data and results files,” Section 4.1.2 of the ABAQUS Analysis User’s Manual Optional parameters: FREQUENCY Set this parameter equal to the output frequency in increments.
* NODE PRINT output is required. The default is MODE=1. See also the LAST MODE parameter. When performing a *FREQUENCY analysis, the normalization will follow the format set by the NORMALIZATION parameter. Otherwise, the normalization is such that the largest displacement component in the mode has a magnitude of 1.0. NSET Set this parameter equal to the name of the node set for which this output request is being made.
* NODE RESPONSE 14.12 *NODE RESPONSE: Define nodal responses for design sensitivity analysis. This option is used to write nodal response sensitivities to the output database. It must be used in conjunction with the *DESIGN RESPONSE option. Product: ABAQUS/Design Type: History data Level: Step References: • • “Design sensitivity analysis,” Section 14.1.
* NONSTRUCTURAL MASS 14.13 *NONSTRUCTURAL MASS: nonstructural features. Specify mass contribution to the model from This option is used to include the mass contribution from nonstructural features in the model. The nonstructural mass can be applied over an element set that contains solid, shell, membrane, surface, beam, or truss elements. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly Reference: • “Nonstructural mass definition,” Section 2.6.
* NONSTRUCTURAL MASS Set DISTRIBUTION=VOLUME PROPORTIONAL to distribute the total nonstructural mass among the members of the element set region in proportion to the element volume in the initial configuration. A uniform value is added to the underlying structural density over the element set region; therefore, if the region has nonuniform structural density, the center of mass for the element set region may be altered. Data line for UNITS=TOTAL MASS: First (and only) line: 1.
* NORMAL 14.14 *NORMAL: Specify a particular normal direction. This option is used to define alternative nodal normals for elements. In an ABAQUS/Standard analysis it can also be used to define alternative normals for contact surfaces. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly Reference: • “Normal definitions at nodes,” Section 2.1.
* NSET 14.15 *NSET: Assign nodes to a node set. This option assigns nodes to a node set. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model or history data Level: Part, Part instance, Assembly, Model, Step Reference: • “Node definition,” Section 2.1.1 of the ABAQUS Analysis User’s Manual Required parameter: NSET Set this parameter equal to the name of the node set to which the nodes will be assigned.
* NSET INTERNAL ABAQUS/CAE uses the INTERNAL parameter to identify sets that are created internally. The INTERNAL parameter is used only in models defined in terms of an assembly of part instances. The default is to omit the INTERNAL parameter. UNSORTED If this parameter is included, the nodes in this node set will be assigned to the set (or added to the set if it already exists) in the order in which they are given. This parameter will be ignored if the ELSET parameter is used.
O 15.
* ORIENTATION 15.1 *ORIENTATION: Define a local axis system for material or element property definition, for kinematic coupling constraints, for free directions for inertia relief loads, or for connectors. This option is used to define a local coordinate system for definition of material properties; for material calculations at integration points; for element property definitions (e.g.
* ORIENTATION SYSTEM Set SYSTEM=RECTANGULAR (default) to define a rectangular Cartesian system by the three points a, b, and c shown in Figure 15.1–1. Point c is the origin of the system, point a must lie on the -axis, and point b must lie on the - plane. Although not necessary, it is intuitive to select point b such that it is on or near the local -axis. Set SYSTEM=CYLINDRICAL to define a cylindrical system by giving the two points a and b on the polar axis of the cylindrical system (Figure 15.1–1).
* ORIENTATION Data lines to define an orientation using DEFINITION=NODES: First line: 1. Node number of the node at point a. 2. Node number of the node at point b. The next item, specification of point c (the origin), is optional and relevant only for SYSTEM=RECTANGULAR and SYSTEM=Z RECTANGULAR. The default location of the origin, c, is the global origin. 3. Node number of the node at point c. Second line (mandatory for shells, membranes, gaskets, composite solid sections, and contact pairs): 1.
* ORIENTATION Z Y b Z SYSTEM = RECTANGULAR Y c a X (global) X Y X b SYSTEM = Z RECTANGULAR Z c Y a Z X (global) X (radial) SYSTEM = CYLINDRICAL b Z Z Y a Y (tangential) X (global) b SYSTEM = SPHERICAL Z (meridional) Y (circumferential) Z Y a X (radial) X (global) Figure 15.1–1 Orientation systems. 15.
* ORNL 15.2 *ORNL: Specify constitutive model developed by Oak Ridge National Laboratory. This option is used to provide plasticity and creep calculations for type 304 and 316 stainless steel according to the specification in Nuclear Standard NEF 9–5 T, “Guidelines and Procedures for Design of Class I Elevated Temperature Nuclear System Components.” It can be used only with the *PLASTIC option and/or the *CREEP, LAW=STRAIN option.
* OUTPUT 15.3 *OUTPUT: Define output requests to the output database. This option is used to write contact, element, energy, nodal, or diagnostic output to the output database. In an ABAQUS/Standard analysis it is also used to write modal or radiation output to the output database. In an ABAQUS/Explicit analysis it is also used to write incrementation output to the output database.
* OUTPUT HISTORY Include this parameter to indicate that the output requests used in conjunction with the *OUTPUT option will be written to the output database as history-type output. Optional parameters: FREQUENCY Set this parameter equal to the output frequency, in increments. The output will always be written to the output database at the last increment of each step. Set FREQUENCY=0 to suppress the output.
* OUTPUT types except *DYNAMIC and *MODAL DYNAMIC; output will be written every 10 increments for these procedure types. The FREQUENCY, NUMBER INTERVAL, TIME INTERVAL, and TIME POINTS parameters are mutually exclusive. The following parameters are optional and valid only if the FIELD or HISTORY parameter is included: OP Set OP=NEW (default) to indicate that all output database requests defined in previous steps should be removed. New output database requests can be defined.
* OUTPUT Using *OUTPUT in an ABAQUS/Explicit analysis References: • • • • • • • • • “Output to the output database,” Section 4.1.3 of the ABAQUS Analysis User’s Manual “ABAQUS/Explicit output variable identifiers,” Section 4.2.2 of the ABAQUS Analysis User’s Manual “Overview of job diagnostics,” Section 23.
* OUTPUT TIME POINTS Set this parameter equal to the name of the *TIME POINTS option that defines the time points at which output is to be written. If this parameter and the NUMBER INTERVAL parameter are omitted, field output will be written at 20 equally spaced intervals throughout the step. The NUMBER INTERVAL and TIME POINTS parameters are mutually exclusive.
* OUTPUT VARIABLE Set VARIABLE=ALL to indicate that all variables applicable to this procedure and material type should be written to the output database. Set VARIABLE=PRESELECT to indicate that the default output variables for the current procedure type should be written to the output database. Additional output requests can be defined with the output options used in conjunction with the *OUTPUT option, listed previously.
P, Q 16.
* PARAMETER 16.1 *PARAMETER: Define parameters for input parametrization. This option is used to define parameters that can be used in place of ABAQUS input quantities. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly, Model, Step References: • • “Parametric input,” Section 1.4.1 of the ABAQUS Analysis User’s Manual “Parametric shape variation,” Section 2.1.
* PARAMETER DEPENDENCE 16.2 *PARAMETER DEPENDENCE: parameters. Define dependence table for tabularly dependent This option is used to define the dependence table that specifies the relationship between tabularly dependent and independent parameters. Product: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly, Model, Step References: • • “Parametric input,” Section 1.4.1 of the ABAQUS Analysis User’s Manual “Parametric shape variation,” Section 2.1.
* PARAMETER SHAPE VARIATION 16.3 *PARAMETER SHAPE VARIATION: Define parametric shape variations. This option is used to define parametric shape variations. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • “Parametric shape variation,” Section 2.1.2 of the ABAQUS Analysis User’s Manual “Design sensitivity analysis,” Section 14.1.
* PARAMETER SHAPE VARIATION Optional parameters if the FILE parameter is used: INC Set this parameter equal to the increment number (in the analysis whose results file is being used as input to this option) from which the displacement data are to be read. If this parameter is omitted, ABAQUS will read the data from the last increment available for the specified step on the results file.
* PARAMETER SHAPE VARIATION Z (X,Y,Z) Y X Rectangular Cartesian (SYSTEM=R) (default) Z Z (R,θ,Z) (R,θ, φ) Y Y φ R θ θ X X Cylindrical (SYSTEM=C) Spherical (SYSTEM=S) (θ and φ are given in degrees) Figure 16.3–1 Coordinate systems. 16.
* PART 16.4 *PART: Begin a part definition. This option is used to begin a part definition. It must be used in conjunction with the *ASSEMBLY, *END PART, and *INSTANCE options. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • “Defining an assembly,” Section 2.9.1 of the ABAQUS Analysis User’s Manual *END PART Required parameter: NAME Set this parameter equal to a label that will be used to refer to the part.
* PERIODIC 16.5 *PERIODIC: Define periodic symmetry for a cavity radiation heat transfer analysis. This option is used to define cavity symmetry by periodic repetition in a given direction. It can be used only following the *RADIATION SYMMETRY option. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Cavity radiation,” Section 32.1.
* PERIODIC is assumed to apply both in the positive and negative directions of the distance vector. The default value is NR=2. Data line to define periodic symmetry of a two-dimensional cavity (TYPE=2D): First (and only) line: 1. x-coordinate of point a (see Figure 16.5–1). 2. y-coordinate of point a. 3. x-coordinate of point b. 4. y-coordinate of point b. 5. x-component of periodic distance vector. 6. y-component of periodic distance vector.
* PERIODIC a -2d -d d 2d b n=2 y x Figure 16.5–1 *PERIODIC, TYPE=2D option. 16.
* PERIODIC 2d d -d -2d c z n=2 y b a x Figure 16.5–2 *PERIODIC, TYPE=3D option. 16.
* PERIODIC z 2d d n=2 z = const periodic symm reference line -d -2d r Figure 16.5–3 *PERIODIC, TYPE=ZDIR option. 16.
* PERMEABILITY 16.6 *PERMEABILITY: Define permeability for pore fluid flow. This option is used to define permeability for pore fluid flow in problems involving seepage. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Permeability,” Section 20.7.2 of the ABAQUS Analysis User’s Manual Optional parameters: DEPENDENCIES Set this parameter equal to the number of field variable dependencies included in the definition of the permeability.
* PERMEABILITY Data lines to define fully saturated isotropic permeability (TYPE=ISOTROPIC): First line: 1. 2. 3. 4. 5. 6. k. (Units of LT−1 .) Void ratio, e. Temperature, . First field variable. Second field variable. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the variation.
* PERMEABILITY 6. . 7. Void ratio, e. 8. Temperature, . Subsequent lines (only needed if the DEPENDENCIES parameter is specified): 1. First field variable. 2. Second field variable. 3. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the variation. Data lines to define the dependence of permeability on saturation of the wetting liquid, ks (s) (TYPE=SATURATION): First line: 1. . (Dimensionless.) 2. Saturation, s. (Dimensionless.
* PHYSICAL CONSTANTS 16.7 *PHYSICAL CONSTANTS: Specify physical constants. This option is used to define physical constants necessary for an analysis; since ABAQUS has no built-in units, no default values are provided. If a physical constant required for the analysis is not given, ABAQUS will issue a fatal error message. The units used for the constants must be consistent with the remaining input data.
* PIEZOELECTRIC 16.8 *PIEZOELECTRIC: Specify piezoelectric material properties. This option is used to define the piezoelectric properties of a material. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Piezoelectric behavior,” Section 20.6.2 of the ABAQUS Analysis User’s Manual Optional parameters: DEPENDENCIES Set this parameter equal to the number of field variables included in the definition of the piezoelectric properties.
* PIEZOELECTRIC 2. 3. 4. 5. 6. 7. 8. . . . . . . . Third line: 1. 2. 3. 4. 5. 6. . . Temperature, . First field variable. Second field variable. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the piezoelectric properties as a function of temperature and other predefined field variables.
* PIEZOELECTRIC 3. . 4. . 5. . 6. . 7. . 8. . 1. . 2. . Third line: 3. Temperature, . 4. First field variable. 5. Second field variable. 6. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line.
* PIPE-SOIL INTERACTION 16.9 *PIPE-SOIL INTERACTION: elements. Specify element properties for pipe-soil interaction This option is used to define properties for pipe-soil interaction elements. The *PIPE-SOIL STIFFNESS option must follow immediately after this option. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • • “Pipe-soil interaction elements,” Section 26.13.1 of the ABAQUS Analysis User’s Manual “Pipe-soil interaction element library,” Section 26.13.
* PIPE-SOIL STIFFNESS 16.10 *PIPE-SOIL STIFFNESS: elements. Define constitutive behavior for pipe-soil interaction This option is used to define the constitutive behavior for pipe-soil interaction elements. It can be used only in conjunction with the *PIPE-SOIL INTERACTION option. Repeat the option as needed to define behavior in the different local directions. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • • • “Pipe-soil interaction elements,” Section 26.13.
* PIPE-SOIL STIFFNESS TYPE Set TYPE=LINEAR (default) to define a linear constitutive model. Set TYPE=NONLINEAR to define a nonlinear constitutive model. Set TYPE=CLAY to define a constitutive model using the ASCE formulae for clay. This parameter must be used in conjunction with the DIRECTION parameter. Set TYPE=SAND to define a constitutive model using the ASCE formulae for sand. This parameter must be used in conjunction with the DIRECTION parameter.
* PIPE-SOIL STIFFNESS 3. 4. 5. 6. Temperature. First field variable. Second field variable. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the force per unit length as a function of relative displacement, temperature, and other predefined field variables.
* PIPE-SOIL STIFFNESS 7. Second field variable. 8. Third field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than three): 1. Fourth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the parameters for the ASCE formulae as a function of temperature and other predefined field variables.
* PIPE-SOIL STIFFNESS Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than three): 1. Fourth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the parameters for the ASCE formulae as a function of temperature and other predefined field variables. Data lines to define constitutive behavior using the ASCE formula for sand in the horizontal direction (TYPE=SAND, DIRECTION=HORIZONTAL): First line: 1. 2.
* PIPE-SOIL STIFFNESS Data lines if the constitutive behavior is defined in user subroutine UMAT (TYPE=USER): First line: 1. Enter the data to be used as properties in user subroutine UMAT. Repeat this data line as often as necessary to define properties required in UMAT. Enter eight values per line. 16.
* PLANAR TEST DATA 16.11 *PLANAR TEST DATA: and/or tension). Used to provide planar test (or pure shear) data (compression This option is used to provide planar test (or pure shear) data. It can be used only in conjunction with the *HYPERELASTIC option, the *HYPERFOAM option, and the *MULLINS EFFECT option. This type of test does not define the hyperelastic material constants fully; at the least, uniaxial or biaxial test data should also be given.
* PLANAR TEST DATA Data lines to specify planar test data for hyperelasticity other than the Marlow model: First line: 1. Nominal stress, . 2. Nominal strain in the direction of loading, . Repeat this data line as often as necessary to give the stress-strain data. Data lines to specify planar test data for the Marlow model: First line: 1. Nominal stress, . 2. Nominal strain, . 3. Nominal lateral strain, .
* PLANAR TEST DATA 3. Nominal transverse strain, . Default is zero. Not needed if the POISSON parameter is specified on the *HYPERFOAM option. Repeat this data line as often as necessary to give the stress-strain data. Using planar test data to define the Mullins effect material model References: • • • “Mullins effect in rubberlike materials,” Section 17.6.1 of the ABAQUS Analysis User’s Manual “Energy dissipation in elastomeric foams,” Section 17.6.
* PLASTIC 16.12 *PLASTIC: Specify a metal plasticity model. This option is used to specify the plastic part of the material model for elastic-plastic materials that use the Mises or Hill yield surface. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • • “Classical metal plasticity,” Section 18.2.1 of the ABAQUS Analysis User’s Manual “Models for metals subjected to cyclic loading,” Section 18.2.
* PLASTIC Optional parameter for use with HARDENING=ISOTROPIC: RATE Set this parameter equal to the equivalent plastic strain rate, applies. , for which this stress-strain curve Optional parameter for use with HARDENING=COMBINED: DATA TYPE Set DATA TYPE=HALF CYCLE (default) to specify stress versus plastic strain values of the first half-cycle for calibrating the kinematic hardening parameters. Set DATA TYPE=PARAMETERS to specify the calibrated kinematic hardening material parameters directly.
* PLASTIC Data lines for HARDENING=COMBINED with DATA TYPE=STABILIZED: First line: 1. 2. 3. 4. 5. 6. 7. Yield stress. Plastic strain. Strain range. Temperature. First field variable. Second field variable. Etc., up to four field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than four): 1. Fifth field variable. 2. Etc., up to eight field variables per line.
* PLASTIC 2. Plastic strain. 3. Temperature, if temperature dependent. Repeat this data line a maximum of two times to define linear kinematic hardening independent of temperature. Repeat this set of data lines as often as necessary to define a variation of the linear kinematic hardening modulus with respect to temperature. Data line for HARDENING=JOHNSON COOK: First (and only) line: 1. A. 2. B. 3. n. 4. m. 5. Melting temperature, 6. Transition temperature, . .
* PLASTIC AXIAL 16.13 *PLASTIC AXIAL: Define plastic axial force for frame elements. This option can be used only in conjunction with the *FRAME SECTION option. It describes the axial force in a frame element as a function of the axial plastic displacement. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • “Frame section behavior,” Section 23.4.2 of the ABAQUS Analysis User’s Manual *FRAME SECTION There are no parameters associated with this option.
* PLASTIC M1 16.14 *PLASTIC M1: Define the first plastic bending moment behavior for frame elements. This option can be used only in conjunction with the *FRAME SECTION option. It describes the bending moment in a frame element as a function of the plastic rotation about the first cross-section direction. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • “Frame section behavior,” Section 23.4.
* PLASTIC M2 16.15 *PLASTIC M2: elements. Define the second plastic bending moment behavior for frame This option can be used only in conjunction with the *FRAME SECTION option and is available only for FRAME3D elements. It describes the bending moment in a frame element as a function of the plastic rotation about the second cross-section direction. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • “Frame section behavior,” Section 23.4.
* PLASTIC TORQUE 16.16 *PLASTIC TORQUE: elements. Define the plastic torsional moment behavior for frame This option can be used only in conjunction with the *FRAME SECTION option and is available only for FRAME3D elements. It describes the torsional moment in a frame element as a function of the plastic rotation about the element’s axis. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • “Frame section behavior,” Section 23.4.
* POROUS BULK MODULI 16.17 *POROUS BULK MODULI: Define bulk moduli for soils and rocks. This option is used to define the bulk moduli of solid grains and a permeating fluid such that their compressibility can be considered in the analysis of a porous medium. The *POROUS BULK MODULI option cannot be used with the porous metal plasticity material model. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Porous bulk moduli,” Section 20.7.
* POROUS ELASTIC 16.18 *POROUS ELASTIC: Specify elastic material properties for porous materials. This option is used to define the elastic parameters for porous materials. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Elastic behavior of porous materials,” Section 17.3.
* POROUS ELASTIC 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of the material parameters , G, and on temperature and field variables. Data lines to define the instantaneous shear modulus from the bulk modulus and Poisson’s ratio: First line: 1. Value of the logarithmic bulk modulus, . (Dimensionless.) 2. Value of Poisson’s ratio, . 3. Value of the elastic tensile limit, . (This value cannot be negative.) 4. Temperature, . 5.
* POROUS FAILURE CRITERIA 16.19 *POROUS FAILURE CRITERIA: METAL PLASTICITY model. Define porous material failure criteria for a *POROUS This option is used to specify the material failure criteria in a porous metal. Product: ABAQUS/Explicit Type: Model data Level: Model References: • • *POROUS METAL PLASTICITY “Porous metal plasticity,” Section 18.2.9 of the ABAQUS Analysis User’s Manual There are no parameters associated with this option.
* POROUS METAL PLASTICITY 16.20 *POROUS METAL PLASTICITY: Specify a porous metal plasticity model. This option is used to specify the porous part of the porous metal plasticity model. The *POROUS METAL PLASTICITY option can be used in conjunction with the *VOID NUCLEATION option to define the nucleation of voids. In an ABAQUS/Explicit analysis it can also be used in conjunction with the *POROUS FAILURE CRITERIA option to specify the material failure criteria.
* POROUS METAL PLASTICITY 6. Second field variable. 7. Etc., up to four field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than four): 1. Fifth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of temperature and other predefined field variables. 16.
* POST OUTPUT 16.21 *POST OUTPUT: Postprocess for output from the restart file. This option can be used only for postprocessing to recover additional printed (.dat), output database (.odb), and results file (.fil) output from the restart file of a previous analysis. Product: ABAQUS/Standard Type: History data Level: Model References: • • “Output,” Section 4.1.1 of the ABAQUS Analysis User’s Manual “Restarting an analysis,” Section 9.1.
* POTENTIAL 16.22 *POTENTIAL: Define an anisotropic yield/creep model. This option is used to define stress ratios for anisotropic yield and creep behavior. It can be used only in conjunction with material models defined by the *CREEP option, the *PLASTIC option (HARDENING=ISOTROPIC, KINEMATIC, or COMBINED; the *POTENTIAL option can be used in conjunction with COMBINED hardening only in ABAQUS/Explicit), and/or the *VISCOUS option.
* POTENTIAL 7. Temperature. 8. First field variable. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than one): 1. Second field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of other field variables. 16.
* PREPRINT 16.23 *PREPRINT: Select printout for the analysis input file processor. This option is used to select the printout that will be obtained from the analysis input file processor. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model Reference: • “Output,” Section 4.1.1 of the ABAQUS Analysis User’s Manual Optional parameters: CONTACT This parameter applies only to ABAQUS/Standard analyses.
* PRESSURE PENETRATION 16.24 *PRESSURE PENETRATION: contact. Specify pressure penetration loads with surface-based This option is used to prescribe pressure penetration loading simulated with surface-based contact. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Pressure penetration loading,” Section 30.1.
* PRESSURE PENETRATION OP Set OP=MOD (default) for existing pressure penetration loads to remain, with this option modifying existing pressure penetration loads or defining additional pressure penetration loads. Set OP=NEW if all existing pressure penetration loads applied to the model should be removed. New pressure penetration loads can be defined.
* PRESSURE STRESS 16.25 *PRESSURE STRESS: Specify equivalent pressure stress as a predefined field for a mass diffusion analysis. This option can be used only in a *MASS DIFFUSION analysis to specify pressure as a predefined field. The user defines equivalent pressure stresses at the nodes, and ABAQUS/Standard interpolates the pressure to the material points. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Mass diffusion analysis,” Section 6.8.
* PRESSURE STRESS are being reset to new values (not to initial conditions) via OP=NEW, the AMPLITUDE parameter described above applies. Required parameter for reading equivalent pressure stresses from the results file: FILE Set this parameter equal to the name of the results file (including the optional .fil extension) from which the data are read. See “Input syntax rules,” Section 1.2.1 of the ABAQUS Analysis User’s Manual, for the syntax of such file names.
* PRESSURE STRESS Data lines to define pressures using the data line format: First line: 1. Node set or node number. If a node set label is given, all nodes in this set must have identical initial pressures. 2. Reference pressure value (positive in compression). If the AMPLITUDE parameter is present, this value will be modified by the AMPLITUDE specification. Repeat this line as often as necessary to define the pressure at different nodes or node sets.
* PRESTRESS HOLD 16.26 *PRESTRESS HOLD: solution. Keep rebar prestress constant during initial equilibrium This option is used within a *STATIC step (“Static stress analysis,” Section 6.2.2 of the ABAQUS Analysis User’s Manual) to keep the stress in some or all of the rebar constant during the initial equilibrium solution. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Defining reinforcement,” Section 2.2.
* PRE-TENSION SECTION 16.27 *PRE-TENSION SECTION: Associate a pre-tension node with a pre-tension section. This option is used to associate a pre-tension node with a pre-tension section. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance, Assembly Reference: • “Prescribed assembly loads,” Section 27.5.
* PRE-TENSION SECTION If the data line is omitted, ABAQUS/Standard will compute an average normal to the pre-tension section for continuum elements. For truss or beam elements the default normal points from the first to the last node in the element connectivity. 16.
* PRINT 16.28 *PRINT: Request or suppress output to the message file in an ABAQUS/Standard analysis or to the status file in an ABAQUS/Explicit analysis. This option is used to obtain or suppress detailed printout in the message (.msg) file in an ABAQUS/Standard analysis or in the status (.sta) file in an ABAQUS/Explicit analysis. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step References: • “Output,” Section 4.1.
* PRINT RESIDUAL Set RESIDUAL=YES (default) if the output of equilibrium residuals is to be given during the equilibrium iterations. Set RESIDUAL=NO to suppress the output. SOLVE Set SOLVE=YES to request information regarding the actual number of equations and the memory requirement in each iteration. The default is SOLVE=NO. Optional parameters in ABAQUS/Explicit analyses: ALLKE Set ALLKE=YES to request that a column containing the total kinetic energy be printed in the status file.
* PSD-DEFINITION 16.29 *PSD-DEFINITION: response loading. Define a cross-spectral density frequency function for random This option is used to define a frequency function for reference in the *CORRELATION option to define the frequency dependence of the random loading in the *RANDOM RESPONSE analysis procedure. Product: ABAQUS/Standard Type: Model data Level: Model References: • • • • “Random response analysis,” Section 6.3.11 of the ABAQUS Analysis User’s Manual “UPSD,” Section 1.1.
* PSD-DEFINITION Set TYPE=FORCE (default) if this frequency function is given directly in power units. Set TYPE=DB if this frequency function is defined in decibel units (see below). This option cannot be used with the USER parameter. USER Include this parameter if the frequency function is defined in user subroutine UPSD. If this parameter is included, no data lines are needed. Data lines for TYPE=BASE or TYPE=FORCE: First line: 1. Real part of the frequency function, in units2 per frequency. 2.
R 17.
* RADIATE 17.1 *RADIATE: Specify radiation conditions in heat transfer analyses. This option is used to apply radiation boundary conditions between a nonconcave surface and a nonreflecting environment in fully coupled thermal-stress analysis. In ABAQUS/Standard it is also used for heat transfer and coupled thermal-electrical analyses. It must be used in conjunction with the *PHYSICAL CONSTANTS option, which is used to define the Stefan-Boltzmann constant.
* RADIATE Set REGION TYPE=LAGRANGIAN (default) to apply the radiation condition to a Lagrangian boundary region. The edge of a Lagrangian boundary region will follow the material while allowing adaptive meshing along the edge and within the interior of the region. Set REGION TYPE=SLIDING to apply the radiation condition to a sliding boundary region. The edge of a sliding boundary region will slide over the material. Adaptive meshing will occur along the edge and in the interior of the region.
* RADIATION FILE 17.2 *RADIATION FILE: Define results file requests for cavity radiation heat transfer. This option is used to write cavity radiation variables to the ABAQUS/Standard results file. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Cavity radiation,” Section 32.1.1 of the ABAQUS Analysis User’s Manual “Output,” Section 4.1.
* RADIATION OUTPUT 17.3 *RADIATION OUTPUT: variables. Define output database requests for cavity radiation This option is used to write cavity radiation variables to the output database. It must be used in conjunction with the *OUTPUT option. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Output to the output database,” Section 4.1.
* RADIATION OUTPUT Data lines to request cavity radiation output: First line: 1. Specify the identifying keys for the variables to be written to the output database. The keys are defined in “ABAQUS/Standard output variable identifiers,” Section 4.2.1 of the ABAQUS Analysis User’s Manual. Repeat this data line as often as necessary to define the cavity radiation variables to be written to the output database. 17.
* RADIATION PRINT 17.4 *RADIATION PRINT: Define print requests for cavity radiation heat transfer. This option is used to print tabular output of cavity radiation variables (radiation fluxes, viewfactor totals, and facet temperatures). Product: ABAQUS/Standard Type: History data Level: Step References: • • “Cavity radiation,” Section 32.1.1 of the ABAQUS Analysis User’s Manual “Output,” Section 4.1.
* RADIATION PRINT Data lines to request printed output: First line: 1. Give the identifying keys for the variables to be printed in a table for this request. The keys are defined in the “Surface variables” section of “ABAQUS/Standard output variable identifiers,” Section 4.2.1 of the ABAQUS Analysis User’s Manual. Repeat this data line as often as necessary: each line defines a table (or more than one table if the request is for a cavity made up of more than one surface).
* RADIATION SYMMETRY 17.5 *RADIATION SYMMETRY: analysis. Define cavity symmetries for radiation heat transfer This option must precede the *CYCLIC, *PERIODIC, and/or *REFLECTION options to specify symmetries in cavities used for cavity radiation heat transfer analysis. Product: ABAQUS/Standard Type: History data Level: Step References: • • • • “Cavity radiation,” Section 32.1.
* RADIATION VIEWFACTOR 17.6 *RADIATION VIEWFACTOR: Control cavity radiation and viewfactor calculations. This option is used to control the calculation of viewfactors during a cavity radiation analysis. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Cavity radiation,” Section 32.1.1 of the ABAQUS Analysis User’s Manual Optional parameters: BLOCKING Set BLOCKING=ALL (default) to specify that full blocking checks be performed in the viewfactor calculations.
* RADIATION VIEWFACTOR SYMMETRY Include this parameter to indicate the existence of radiation symmetries in the model. This parameter must be set equal to the name appearing in the *RADIATION SYMMETRY option where the symmetries are defined. If this parameter is omitted, it is assumed that there are no radiation symmetries in the cavity. VTOL Set this parameter equal to the acceptable tolerance for the viewfactor calculations. If this parameter is omitted, the default viewfactor tolerance is 0.05.
* RANDOM RESPONSE 17.7 *RANDOM RESPONSE: Calculate response to random loading. This option is used to give the linearized response of a model to random excitation. Product: ABAQUS/Standard Type: History data Level: Step References: • • • “Random response analysis,” Section 6.3.11 of the ABAQUS Analysis User’s Manual *CORRELATION *PSD-DEFINITION There are no parameters associated with this option. Data lines for a random response analysis: First line: 1.
* RATE DEPENDENT 17.8 *RATE DEPENDENT: Define a rate-dependent viscoplastic model. This option can be used in conjunction with the *PLASTIC option (HARDENING=ISOTROPIC only), the *DRUCKER PRAGER HARDENING option, and/or the *CRUSHABLE FOAM HARDENING option to introduce strain rate dependence in the material models. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • • • “Rate-dependent yield,” Section 18.2.
* RATE DEPENDENT Data lines to define the overstress power law parameters (TYPE=POWER LAW): First line: 1. D. 2. n. 3. Temperature. 4. First field variable. 5. Second field variable. 6. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line.
* RATIOS 17.9 *RATIOS: Define anisotropic swelling. This option is used to specify ratios that define anisotropic swelling. The *RATIOS option can be used only in conjunction with the *MOISTURE SWELLING option or the *SWELLING option, and it should appear immediately after either one. Product: ABAQUS/Standard Type: Model data Level: Model References: • • • • “Moisture swelling,” Section 20.7.6 of the ABAQUS Analysis User’s Manual “Rate-dependent plasticity: creep and swelling,” Section 18.2.
* RATIOS Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than four): 1. Fifth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of the anisotropic swelling ratios on temperature and other field variables. 17.
* REBAR 17.10 *REBAR: Define rebar as an element property. This option is used as an alternative method to define rebar as an element property in shells, membranes, and solid (continuum) elements. It must be used to define rebar in beams in ABAQUS/Standard analyses. The preferred option for defining rebar in shells, membranes, and surface elements is the *REBAR LAYER option, which must be used in conjunction with the *SHELL SECTION, the *MEMBRANE SECTION, or the *SURFACE SECTION options.
* REBAR Optional parameters: GEOMETRY This parameter is not meaningful for rebar in beams, axisymmetric shells, or axisymmetric membranes, or for single rebar in continuum elements. Set GEOMETRY=ISOPARAMETRIC (default) to indicate that the layer of rebar is parallel to a direction of the element local (isoparametric) coordinate system. Set GEOMETRY=SKEW to indicate that the rebar layer is in a skew direction with respect to the element faces.
* REBAR Rebar 2 Local beam section axes X2 X1 Figure 17.10–1 1 Rebar location in a beam section. Data lines to define isoparametric rebar in three-dimensional shell elements: First line: 1. Element number or name of the element set that contains these rebar. 2. Cross-sectional area of each rebar. 3. Spacing of the rebar in the plane of the shell. The default is 1.0. 4. Position of the rebar in the shell section thickness direction.
* REBAR 2 3 Similar to edge 1 or 3 4 2 Similar to edge 2 or 4 1 3 ;; ;; ;; ;; ;; ;; ;; ;; ;;;;;;;;;;; ;; ;;;;;;;;;;; ;; 2 Edge 1 1 2 3 4 Corner nodes 1-2 2-3 3-4 4-1 1 physical space Figure 17.10–2 4 isoparametric space “Isoparametric” rebar in a three-dimensional shell or membrane. Data lines to define skew rebar in three-dimensional shell elements: First line: 1. 2. 3. 4. Element number or name of the element set that contains these rebar. Cross-sectional area of each rebar.
* REBAR Data lines to define rebar in axisymmetric shell elements: First line: 1. 2. 3. 4. Element number or name of the element set that contains these rebar. Cross-sectional area of each rebar. Spacing of rebar in this rebar layer. The default is 1.0. Position of the rebar in the shell section thickness direction. This value is given as the distance of the rebar from the middle surface of the shell, positive in the direction of the positive normal to the shell.
* REBAR 4. Orientation of rebar in degrees. See Figure 17.10–3. 5. Fractional distance from the edge given below, f (ratio of the distance between the edge and the rebar to the distance across the element). 6. Edge number from which the rebar are defined. See Figure 17.10–4 or Figure 17.10–7. 7. Isoparametric direction (for three-dimensional elements only). 8. For axisymmetric elements only, the radial position at which the spacing of the rebar is measured.
* REBAR 5. Isoparametric direction (for three-dimensional elements only). In three-dimensional cases the fractional distances , and are given along the first two edges of the face identified in Figure 17.10–7 for the isoparametric direction chosen. Repeat this data line as often as necessary. Each line defines a single rebar. Rebar gle on ti nta an ie Or 1 4 edge 4 Positive direction from lower to higher numbered edge. y rebar spacing z edge 1 r x edge 3 θ z 2 Figure 17.
* REBAR Edge Corner nodes 1 2 3 4 rebar layer B, defined with edge 2 or 4 1-2 2-3 3-4 4-1 rebar layer B 2 3 4 4 L4 3 1 L2 L A4 1 2 1 LA2 y rebar layer A, defined with L L edge 1 and f = A2 = A4 L2 L4 x rebar layer A 2 Isoparametric mapping of element with rebar Actual element Figure 17.10–4 Rebar layer definition in solid elements with GEOMETRY=ISOPARAMETRIC. 17.
* REBAR Edge Corner nodes 1 2 3 4 1-2 2-3 3-4 4-1 rebar layer A defined with L L f1 = A1 , f2 = A2 , f3 = 0 and f4 = 0 L2 L1 rebar layer B defined with L L f1 = 0, f2 = 0, f3 = B3 and f4 = B4 L3 L4 L3 L B3 4 L4 2 3 rebar layer B 4 L B4 3 1 L2 1 L A1 L A2 1 2 rebar layer A L1 2 y Isoparametric mapping of element with rebar Actual element x Figure 17.10–5 Rebar layer definition in solid elements with GEOMETRY=SKEW. 17.
* REBAR Edge Corner nodes 1 2 single rebar defined with l l f1 = 1 and f2 = 2 L1 L2 4 1-2 2-3 2 3 4 3 1 L2 1 l2 l1 1 2 single rebar L1 2 y x Actual element Figure 17.10–6 Isoparametric mapping of element with rebar SINGLE rebar in a solid element. 17.
* REBAR 8 7 8 5 6 6 5 4 3 z 7 ⇒ 4 3 3 y 2 1 2 x 1 actual element 1 2 isoparametric mapping Isoparametric direction: 1 (parallel to the 1-2 edge of the element and intersecting face 1-4-8-5) Edge 1 2 3 4 Corner nodes 1-4 4-8 8-5 5-1 Isoparametric direction: 2 (parallel to the 1-4 edge of the element and intersecting face 1-5-6-2) Edge Corner nodes 1 2 3 4 1-5 5-6 6-2 2-1 Isoparametric direction: 3 (parallel to the 1-5 edge of the element and intersecting face 1-2-3-4) Edge Corner nod
* REBAR LAYER 17.11 *REBAR LAYER: Define layers of reinforcement in membrane, shell, surface, and continuum elements. This option is used to define one or multiple rebar layers in membrane, shell, and surface elements. It must be used in conjunction with the *MEMBRANE SECTION, the *SHELL SECTION, or the *SURFACE SECTION option.
* REBAR LAYER ORIENTATION This parameter is meaningful only for rebar in general shell, membrane, and surface elements. Set this parameter equal to the name of an orientation definition that defines the angular orientation of the rebar on the data lines. If this parameter is omitted, the angular orientation of rebar on the data lines is specified relative to the default projected local surface directions.
* REBAR LAYER 9. Radius, , of the rebar defined with GEOMETRY=LIFT EQUATION. The value is the position of the rebar in the uncured geometry, measured with respect to the axis of rotation in a cylindrical coordinate system. This entry has no meaning for rebar defined using GEOMETRY=CONSTANT or GEOMETRY=ANGULAR. Repeat the data line as often as necessary. Each data line defines a layer of rebar. 17.
* REFLECTION 17.12 *REFLECTION: analysis. Define reflection symmetries for a cavity radiation heat transfer This option is used to define a cavity symmetry by reflection through a line or a plane. It can be used only following the *RADIATION SYMMETRY option. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Cavity radiation,” Section 32.1.
* REFLECTION Data lines to define reflection of a three-dimensional cavity (TYPE=PLANE): First line: 1. 2. 3. 4. 5. 6. X-coordinate of point a (see Figure 17.12–2). Y-coordinate of point a. Z-coordinate of point a. X-coordinate of point b. Y-coordinate of point b. Z-coordinate of point b. Second line: 1. X-coordinate of point c. 2. Y-coordinate of point c. 3. Z-coordinate of point c. Data line to define reflection of an axisymmetric cavity (TYPE=ZCONST): First (and only) line: 1.
* REFLECTION n Z c Y b a X Figure 17.12–2 *REFLECTION, TYPE=PLANE option. 17.
* REFLECTION z z = const symmetry line r Figure 17.12–3 *REFLECTION, TYPE=ZCONST option. 17.
* RELEASE 17.13 *RELEASE: element. Release rotational degrees of freedom at one or both ends of a beam This option is used to release a rotational degree of freedom or a combination of rotational degrees of freedom at one or both ends of a beam element. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • “Kinematic coupling constraints,” Section 28.2.3 of the ABAQUS Analysis User’s Manual “Element end release,” Section 28.5.
* RESPONSE SPECTRUM 17.14 *RESPONSE SPECTRUM: spectra. Calculate the response based on user-supplied response This option is used to calculate estimates of peak values of displacements and stresses based on user-supplied response spectra (defined using the *SPECTRUM option) and on the natural modes of the system. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Response spectrum analysis,” Section 6.3.
* RESPONSE SPECTRUM 4. Z-direction cosine of this direction. 5. Factor multiplying the magnitudes in the response spectrum. Default is 1.0. Second line (optional): 1. Name of the response spectrum to be used in the second direction. 2. X-direction cosine of this direction. This direction must be at a right angle to the direction defined above. 3. Y-direction cosine of this direction. This direction must be at a right angle to the direction defined above. 4. Z-direction cosine of this direction.
* RESTART 17.15 *RESTART: Save and reuse data and analysis results. WARNING: This option can create a very large amount of data. The size is estimated by the analysis input file processor in an ABAQUS/Standard analysis. This option is used to control the writing and reading of restart data. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model or history data Level: Model, Step Using *RESTART in an ABAQUS/Standard analysis Reference: • “Restarting an analysis,” Section 9.1.
* RESTART If this parameter is omitted, the restart will begin at the end of the step specified on the STEP parameter. ITERATION If the new analysis is restarted from a previous direct cyclic analysis, set this parameter equal to the iteration number within the specified step of the direct cyclic analysis after which the analysis will resume.
* RESTART When the OVERLAY parameter is included, each increment written overlays the previous increment, if any, written for the same step. If this parameter is omitted, data are retained for every increment. In either case the last increment of every step is retained. There are no data lines associated with this option. Using *RESTART in an ABAQUS/Explicit analysis Reference: • “Restarting an analysis,” Section 9.1.
* RESTART Optional parameters if the WRITE parameter is used: NUMBER INTERVAL Set this parameter equal to the number of intervals during the step at which the *RESTART data are to be written. The value of this parameter must be a positive integer. The default is NUMBER INTERVAL=1. ABAQUS/Explicit will always write the restart data at the beginning and end of the step.
* RETAINED EIGENMODES 17.16 *RETAINED EIGENMODES: generation analysis. Select the modes to be retained in a substructure This option selects the modes to be used in a substructure generation analysis. The modes must be extracted in a prior *FREQUENCY step and will include residual modes if they were activated. If this option is not used, no modes will be used. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Defining substructures,” Section 10.1.
* RETAINED NODAL DOFS 17.17 *RETAINED NODAL DOFS: Specify the degrees of freedom that are to be retained as external to a substructure. This option is used to list degrees of freedom that are to be retained as external degrees of freedom on the substructure. It can be used only in a *SUBSTRUCTURE GENERATE analysis. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Defining substructures,” Section 10.1.
* RIGID BODY 17.18 *RIGID BODY: properties. Define a set of elements as a rigid body and define rigid element This option is used to bind a set of elements and/or a set of nodes and/or an analytical surface into a rigid body and assign a reference node to the rigid body, which can optionally be declared as an isothermal rigid body for fully coupled thermal-stress analysis.
* RIGID BODY PIN NSET Set this parameter equal to the name of a node set containing pin-type nodes to be assigned to the rigid body. This parameter can be used to add nodes to a rigid body or to redefine node types of nodes on elements included in the rigid body by the ELSET parameter. Pin-type nodes have only their translational degrees of freedom associated with the rigid body. A node cannot appear in more than one rigid body definition.
* RIGID BODY There are no data lines associated with this option in an ABAQUS/Standard analysis. Data line for R2D2, RB2D2, and RB3D2 elements in an ABAQUS/Explicit analysis: First (and only) line: 1. Cross-sectional area of the element. The default is 0. Data line for RAX2, R3D3, and R3D4 elements in an ABAQUS/Explicit analysis: First (and only) line: 1. Thickness of the element. The default is 0. 17.
* RIGID SURFACE 17.19 *RIGID SURFACE: Define an analytical rigid surface. This option must be used when defining the seabed for three-dimensional drag chain elements in ABAQUS/Standard analyses. For all other cases the preferred options for defining analytical rigid surfaces are the *SURFACE and the *RIGID BODY options. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance References: • • • • • “Surfaces: overview,” Section 2.3.
* RIGID SURFACE Set TYPE=CYLINDER to define a three-dimensional rigid surface by providing connected line segments and then sweeping them along a specified generator vector. Set TYPE=REVOLUTION to define a three-dimensional rigid surface by providing connected line segments, which are given in an plane and are rotated about an axis. Set TYPE=USER to define a rigid surface via user subroutine RSURFU.
* RIGID SURFACE Third line: 1. The “word” START. 2. Local x-coordinate of the starting point of the line segments. 3. Local y-coordinate of the starting point of the line segments. Fourth and subsequent data lines define the various line, circular, and parabolic segments (see below for their format) that form the profile of the rigid surface. Data lines to define surfaces created with TYPE=REVOLUTION: First line: 1. 2. 3. 4. 5. 6.
* RIGID SURFACE Data line to define a parabolic arc segment: 1. The “word” PARAB. 2. x-coordinate of the middle point along the parabolic arc. 3. y-coordinate of the middle point along the parabolic arc. 4. x-coordinate of the endpoint of the parabolic arc. 5. y-coordinate of the endpoint of the parabolic arc. For rigid surfaces created with TYPE=SEGMENTS, the x- and y-coordinates are the global X- and Ycoordinates or r- and z-coordinates.
* RIGID SURFACE local z Start n b line segment a local r circular arc segment n Figure 17.19–2 *RIGID SURFACE, TYPE=REVOLUTION. 17.
* ROTARY INERTIA 17.20 *ROTARY INERTIA: Define rigid body rotary inertia. This option is used to define rigid body rotary inertia values associated with ROTARYI elements. It is also used in ABAQUS/Standard analyses to define mass proportional damping (for direct-integration dynamic analysis) and composite damping (for modal dynamic analysis) associated with ROTARYI elements.
* ROTARY INERTIA In large-displacement analysis (an ABAQUS/Explicit analysis or when the NLGEOM parameter is included on the *STEP option in an ABAQUS/Standard analysis), the local axes of inertia rotate with the rotation of the node to which the ROTARYI element is attached. Data line to define the rotary inertia: First (and only) line: 1. Rotary inertia about the local 1-axis, . 2. Rotary inertia about the local 2-axis, . 3. Rotary inertia about the local 3-axis, . 4. Product of inertia, . 5.
S 18.
* SECTION CONTROLS 18.1 *SECTION CONTROLS: Specify section controls. WARNING: Using values larger than the default values for hourglass control can produce excessively stiff response and sometimes can even lead to instability if the values are too large. Hourglassing that occurs with the default hourglass control parameters is usually an indication that the mesh is too coarse. Therefore, it is generally better to refine the mesh than to add stronger hourglass control.
* SECTION CONTROLS Required parameter: NAME Set this parameter equal to a label that will be used to refer to the section control definition. All section control names in the same input file must be unique. Optional parameters: DISTORTION CONTROL This parameter applies only to ABAQUS/Explicit analyses. Set DISTORTION CONTROL=YES to activate a constraint that acts to prevent negative element volumes or other excessive distortion for crushable materials.
* SECTION CONTROLS ABAQUS/Standard and ABAQUS/Explicit. Any data given on the data line will be ignored for this case. Set HOURGLASS=RELAX STIFFNESS (default for ABAQUS/Explicit, except for elements with hyperelastic and hyperfoam materials) to use the integral viscoelastic form of hourglass control for all elements with reduced integration in ABAQUS/Explicit.
* SECTION CONTROLS NO. For elements other than cohesive elements, connector elements, and elements with plane stress formulations the default value is 1.0 if the element is deleted from the mesh and 0.99 otherwise. For cohesive elements, connector elements, and elements with plane stress formulations the default value is always 1.0.
* SECTION CONTROLS 3. Scaling factor, , for the hourglass stiffness for use with the out-of-plane displacement degree of freedom in small-strain shell elements in ABAQUS/Explicit. If this value is left blank, ABAQUS/Explicit will use the default value of 1.0. The suggested range for the value of is between 0.2 and 3.0. This scaling factor is not relevant for ABAQUS/Standard. 4. Scaling factor for the linear bulk viscosity in ABAQUS/Explicit.
* SECTION FILE 18.2 *SECTION FILE: Define results file requests of accumulated quantities on user-defined surface sections. This option is used to control output to the results file of accumulated quantities associated with a user-defined section. Depending on the analysis type the output may include one or several of the following: the total force, the total moment, the total heat flux, the total current, the total mass flow, or the total pore fluid volume flux associated with the section.
* SECTION FILE average rigid body motion of the surface section. This parameter is relevant only if AXES=LOCAL and the NLGEOM parameter is active in the step. Optional data lines: First line: 1. Node number of the anchor point (blank if coordinates given). 2. First coordinate of the anchor point (ignored if node number given). 3. Second coordinate of the anchor point (ignored if node number given). 4. Third coordinate of the anchor point (for three-dimensional cases only; ignored if node number given).
* SECTION FILE anchor point 1 defined section 3 b 2 a 2 a 1 Y Z Y anchor point X elements used to define the section X 2-D and axisymmetric Figure 18.2–1 defined section 3-D User-defined local coordinate system. 18.
* SECTION ORIGIN 18.3 *SECTION ORIGIN: Define a meshed cross-section origin. This option is used in conjunction with the *BEAM SECTION GENERATE option to define the location of the beam node on a meshed beam cross-section. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Meshed beam cross-sections,” Section 10.4.1 of the ABAQUS Analysis User’s Manual *BEAM SECTION GENERATE Optional parameter: ORIGIN Set ORIGIN=CENTROID to place the beam node at the section centroid.
* SECTION POINTS 18.4 *SECTION POINTS: Locate points in the beam section for which stress and strain output are required. This option is used as model data in ABAQUS/Standard and ABAQUS/Explicit in conjunction with the *BEAM GENERAL SECTION option and as history data in ABAQUS/Standard in conjunction with the *BEAM SECTION GENERATE option.
* SECTION POINTS 4. Local -position of second section point. Continue giving coordinate pairs for as many points as needed. At most four pairs of points can be specified on any data line. If the point (0,0) is specified as the last entry on a line, it will be ignored unless it is the only point requested. Data lines to locate elements and integration point numbers for meshed sections when used in conjunction with the *BEAM GENERAL SECTION, SECTION=MESHED option: First line: 1. Section point label. 2.
* SECTION PRINT 18.5 *SECTION PRINT: surface sections. Define print requests of accumulated quantities on user-defined This option is used to provide tabular output of accumulated quantities associated with a user-defined section. Depending on the analysis type the output may include one or several of the following: the total force, the total moment, the total heat flux, the total current, the total mass flow, or the total pore fluid volume flux associated with the section.
* SECTION PRINT average rigid body motion of the surface section. This parameter is relevant only if AXES=LOCAL and the NLGEOM parameter is active in the step. Optional data lines: First line: 1. Node number of the anchor point (blank if coordinates given). 2. First coordinate of the anchor point (ignored if node number given). 3. Second coordinate of the anchor point (ignored if node number given). 4. Third coordinate of the anchor point (for three-dimensional cases only; ignored if node number given).
* SECTION PRINT anchor point 1 defined section 3 b 2 a 2 a 1 Y Z Y anchor point X elements used to define the section X 2-D and axisymmetric Figure 18.5–1 defined section 3-D User-defined local coordinate system. 18.
* SELECT CYCLIC SYMMETRY MODES 18.6 *SELECT CYCLIC SYMMETRY MODES: Specify the cyclic symmetry modes in an eigenvalue analysis of a cyclic symmetric structure. This option is used to specify which cyclic symmetry modes should be used in an eigenvalue analysis. Product: ABAQUS/Standard Type: History data Level: Step References: • “Analysis of models that exhibit cyclic symmetry,” Section 10.3.
* SELECT EIGENMODES 18.7 *SELECT EIGENMODES: Select the modes to be used in a modal dynamic analysis. This option selects the modes to be used in a dynamic analysis based on modes or in a complex eigenvalue extraction analysis. Only one option per step can be used. If this option is not used, all modes extracted in the prior *FREQUENCY step will be used, including residual modes if they were activated.
* SELECT EIGENMODES Data lines if the GENERATE parameter is omitted and DEFINITION=MODE NUMBERS: First line: 1. List of modes to be used. Repeat this data line as often as necessary. Up to 16 entries are allowed per line. Data lines if the GENERATE parameter is omitted and DEFINITION=FREQUENCY RANGE: First line: 1. Lower boundary of the frequency range (in cycles/time). 2. Upper boundary of the frequency range (in cycles/time). Repeat this data line as often as necessary.
* SFILM 18.8 *SFILM: Define film coefficients and associated sink temperatures over a surface for heat transfer analysis. This option is used to provide film coefficients and sink temperatures over a surface for fully coupled thermalstress analysis. In ABAQUS/Standard it is also used in heat transfer and coupled thermal-electrical analyses. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step References: • • “Thermal loads,” Section 27.4.
* SFILM The FILM AMPLITUDE parameter is ignored if a nonuniform film coefficient is defined in user subroutine FILM or if a film coefficient is defined to be a function of temperature and field variables using the *FILM PROPERTY option. OP Set OP=MOD (default) to modify existing films or to define additional films. Set OP=NEW if all existing *SFILMs applied to the model should be removed. Data lines to define sink temperatures and film coefficients: First line: 1. Surface name. 2.
* SFLOW 18.9 *SFLOW: Define seepage coefficients and associated sink pore pressures normal to a surface. This option is used to provide seepage coefficients and sink pore pressures to control pore fluid flow normal to the surface in consolidation analysis. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Pore fluid flow,” Section 27.4.6 of the ABAQUS Analysis User’s Manual “FLOW,” Section 1.1.
* SFLOW Data lines to define drainage-only seepage: First line: 1. Surface name. 2. Seepage flow type label QD. 3. Drainage-only seepage coefficient value, . (Units of F−1 L3 T−1 .) Repeat this data line as often as necessary to define drainage-only seepage for various surfaces. Data lines to define nonuniform seepage: First line: 1. Surface name. 2. Seepage flow type label QNU. 3. Optional reference pore pressure value.
* SHEAR CENTER 18.10 *SHEAR CENTER: Define the position of the shear center of a beam section. This option can be used only in conjunction with the *BEAM GENERAL SECTION, SECTION=GENERAL or the *BEAM GENERAL SECTION, SECTION=MESHED option. It is used to define the position of the shear center of the section with respect to the local (1, 2) axis system.
* SHEAR FAILURE 18.11 *SHEAR FAILURE: Specify a shear failure model and criterion. This option is used with the Mises or the Johnson-Cook plasticity models to specify shear failure of the material. It must be used in conjunction with the option *PLASTIC, HARDENING=ISOTROPIC or JOHNSON COOK. Product: ABAQUS/Explicit Type: Model data Level: Model References: • • • • “Classical metal plasticity,” Section 18.2.1 of the ABAQUS Analysis User’s Manual “Johnson-Cook plasticity,” Section 18.2.
* SHEAR FAILURE Data lines to define the failure strain in tabular form (TYPE=TABULAR): First line: 1. Equivalent plastic strain at failure, 2. Rate of equivalent plastic strain, . . 3. Dimensionless pressure-deviatoric stress ratio, . 4. Temperature. 5. First field variable. 6. Second field variable. 7. Etc., up to four field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than four): 1. Fifth field variable. 2. Etc., up to eight field variables per line.
* SHEAR RETENTION 18.12 *SHEAR RETENTION: Define the reduction of the shear modulus associated with crack surfaces in a *CONCRETE model as a function of the tensile strain across the crack. This option is used to give a multiplying factor, , that defines the modulus for shearing of cracks as a fraction of the elastic shear modulus of the uncracked concrete. If this option is used, it should follow the *CONCRETE option.
* SHEAR RETENTION 7. Second field variable. 8. Third field variable. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than three): 1. Fourth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of the shear retention behavior on temperature and other predefined field variables. 18.
* SHEAR TEST DATA 18.13 *SHEAR TEST DATA: Used to provide shear test data. This option can be used only in conjunction with the *VISCOELASTIC option. The *SHEAR TEST DATA option cannot be used for a viscoelastic material if the *COMBINED TEST DATA option is used. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model Using shear test data to define a viscoelastic material References: • • “Time domain viscoelasticity,” Section 17.7.
* SHELL GENERAL SECTION 18.14 *SHELL GENERAL SECTION: Define a general, arbitrary, elastic shell section. This option is used to define a general, arbitrary, elastic shell section. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • • “Shell elements: overview,” Section 23.6.1 of the ABAQUS Analysis User’s Manual “Using a general shell section to define the section behavior,” Section 23.6.6 of the ABAQUS Analysis User’s Manual “UGENS,” Section 1.1.
* SHELL GENERAL SECTION controls,” Section 21.1.4 of the ABAQUS Analysis User’s Manual) or to be used in a subsequent ABAQUS/Explicit import analysis. OFFSET Include this parameter to define the distance (as a fraction of the shell thickness) from the shell midsurface to the reference surface (containing the nodes of the element). This parameter accepts positive or negative values or the labels SPOS or SNEG.
* SHELL GENERAL SECTION The following parameters are optional, mutually exclusive, and used only if the section is not defined by its general stiffness on the data lines: COMPOSITE Include this parameter to indicate that the shell is composed of layers with different linear elastic material behavior. MATERIAL Set this parameter equal to the name of the single linear elastic material of which the shell is made. USER This parameter applies only to ABAQUS/Standard analyses.
* SHELL GENERAL SECTION Optional parameter for use when the MATERIAL, the COMPOSITE, and the USER parameters are omitted: DEPENDENCIES Set this parameter equal to the number of field variable dependencies included in the definition of the scaling moduli, in addition to temperature. If this parameter is omitted, it is assumed that the moduli are constant or depend only on temperature. Data line if the MATERIAL parameter is included: First (and only) line: 1. Shell thickness.
* SHELL GENERAL SECTION 3. , temperature for these values of Y and . 4. First field variable. 5. Second field variable. 6. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define Y and other predefined field variables.
* SHELL SECTION 18.15 *SHELL SECTION: Specify a shell cross-section. This option is used to specify a shell cross-section. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • “Shell elements: overview,” Section 23.6.1 of the ABAQUS Analysis User’s Manual “Using a shell section integrated during the analysis to define the section behavior,” Section 23.6.
* SHELL SECTION DENSITY Set this parameter equal to a mass per unit surface area of the shell. If this parameter is used, the mass of the shell includes a contribution from this parameter in addition to any contribution from the material definition. NODAL THICKNESS Include this parameter to indicate that the shell thickness should not be read from the data lines but should be interpolated from the thickness specified at the nodes with the *NODAL THICKNESS option.
* SHELL SECTION In ABAQUS/Standard the default is POISSON=0.5; in ABAQUS/Explicit the default is POISSON=MATERIAL. STACK DIRECTION This parameter is relevant only for continuum shells. This parameter defines the continuum shell stack or thickness direction. Set this parameter equal to 1, 2, 3, or ORIENTATION. The default is STACK DIRECTION=3. The ORIENTATION parameter must also be used if STACK DIRECTION=ORIENTATION.
* SHELL SECTION be at least 3, except in a pure heat transfer analysis, where the number of integration points can be 1 for a constant temperature through the shell thickness. Data lines to define a composite shell (the COMPOSITE parameter is included): First line: 1. Layer thickness. This value is modified if the NODAL THICKNESS parameter is included. 2. Number of integration points to be used through the layer.
* SHELL TO SOLID COUPLING 18.16 *SHELL TO SOLID COUPLING: edge and a solid face. Define a surface-based coupling between a shell This surface-based option allows for a transition from shell element modeling to solid element modeling in a three-dimensional analysis. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly References: • • • “Defining element-based surfaces,” Section 2.3.
* SHELL TO SOLID COUPLING 2. The solid surface name. Repeat this data line as often as necessary to define all the surfaces forming the coupling definition. Each data line defines a pair of surfaces that will be coupled. 18.
* SIMPEDANCE 18.17 *SIMPEDANCE: Define impedances of acoustic surfaces. This option is used to provide surface impedance information or nonreflecting boundaries for acoustic and coupled acoustic-structural analysis. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step References: • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.9.1 of the ABAQUS Analysis User’s Manual • • • “Acoustic loads,” Section 27.4.
* SIMPEDANCE Optional parameter: OP Set OP=MOD (default) to modify existing impedances or to define additional impedances. Set OP=NEW if all existing impedances applied to the model should be removed. To remove only selected impedances, use OP=NEW and respecify all impedances that are to be retained. Data line to define an impedance for PROPERTY, NONREFLECTING=PLANAR, or NONREFLECTING=IMPROVED: First (and only) line: 1. Surface name.
* SIMPLE SHEAR TEST DATA 18.18 *SIMPLE SHEAR TEST DATA: Used to provide simple shear test data. This option is used to provide simple shear test data. *HYPERFOAM option. Products: ABAQUS/Standard It can be used only in conjunction with the ABAQUS/Explicit Type: Model data Level: Model References: • • “Hyperelastic behavior in elastomeric foams,” Section 17.5.2 of the ABAQUS Analysis User’s Manual *HYPERFOAM There are no parameters associated with this option.
* SLIDE LINE 18.19 *SLIDE LINE: interact. Specify slide line surfaces on which deformable structures may This option is relevant only for slide line and tube-to-tube contact elements. It is used to define the slide line and to specify which set of contact elements interacts with it. Product: ABAQUS/Standard Type: Model data Level: Assembly References: • • “Tube-to-tube contact elements,” Section 31.3.1 of the ABAQUS Analysis User’s Manual “Slide line contact elements,” Section 31.4.
* SLIDE LINE SMOOTH Set this parameter equal to the smoothing fraction, f, to round discontinuities between line segments of a slide line. The default is 0. The limit is . Data lines if the GENERATE parameter is omitted: First line: 1. First node number on this slide line. 2. Second node number on this slide line. 3. Third node number on this slide line. 4. Etc. Repeat this data line as often as necessary to specify the nodes forming the slide line. Enter up to 16 integer values per line.
* SLOAD 18.20 *SLOAD: Apply loads to a substructure. This option is used to activate a substructure load case defined by the *SUBSTRUCTURE LOAD CASE option. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Using substructures,” Section 10.1.1 of the ABAQUS Analysis User’s Manual *SUBSTRUCTURE LOAD CASE Optional parameters: AMPLITUDE Set this parameter equal to the name given to an amplitude defined by the *AMPLITUDE option (“Amplitude curves,” Section 27.1.
* SOILS 18.21 *SOILS: Effective stress analysis for fluid-filled porous media. This option is used to specify transient (consolidation) or steady-state response analysis of partially or fully saturated fluid-filled porous media. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1 of the ABAQUS Analysis User’s Manual “Rate-dependent plasticity: creep and swelling,” Section 18.2.
* SOILS FACTOR Set this parameter equal to the damping factor to be used in the automatic damping algorithm (see “Solving nonlinear problems,” Section 7.1.1 of the ABAQUS Analysis User’s Manual) if the problem is expected to be unstable due to local instabilities and the damping factor calculated by ABAQUS/Standard is not suitable.
* SOILS 5. The rate of change of pore pressure with time, used to define steady state: only needed if END=SS is chosen. When all nodal wetting liquid pressures are changing at rates below this value, the solution terminates. 18.
* SOLID SECTION 18.22 *SOLID SECTION: elements. Specify element properties for solid, infinite, acoustic, and truss This option is used to define properties of solid (continuum) elements, infinite elements, acoustic finite and infinite elements, and truss elements. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • • “Solid (continuum) elements,” Section 22.1.1 of the ABAQUS Analysis User’s Manual “Infinite elements,” Section 22.2.
* SOLID SECTION Required parameter for anisotropic materials optional parameter for isotropic materials: ORIENTATION Set this parameter equal to the name given for the *ORIENTATION option (“Orientations,” Section 2.2.5 of the ABAQUS Analysis User’s Manual) to be used to define a local coordinate system for material calculations in the elements in this set. This parameter is required when the material is anisotropic.
* SOLID SECTION Data line to define homogeneous solid elements, infinite elements, acoustic elements, or truss elements: First (and only) line: 1. Enter any attribute values required. The default for the first attribute is 1.0. See the description in Part VI, “Elements,” of the ABAQUS Analysis User’s Manual of the element type being used for a definition of the data required. Data lines to define a composite solid: First line: 1. Layer thickness.
* SOLUBILITY 18.23 *SOLUBILITY: Specify solubility. This option is used to define the solubility for a material diffusing through a base material. It must be used in conjunction with the *DIFFUSIVITY option. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Solubility,” Section 20.5.
* SOLUTION TECHNIQUE 18.24 *SOLUTION TECHNIQUE: Specify alternative solution methods. This option is used to specify the quasi-Newton method instead of the standard Newton method for solving nonlinear equations, to specify a separated solution scheme for *COUPLED TEMPERATUREDISPLACEMENT and *COUPLED THERMAL-ELECTRICAL procedures, or to specify that contact iterations should be executed instead of regular severe discontinuity iterations.
* SOLUTION TECHNIQUE Data line for TYPE=CONTACT ITERATIONS: First (and only) line: 1. Correction factor on the maximum number of right-hand-side solutions during any contact iteration. The default is 1. The actual number of allowed right-hand-side solutions with the correction factor accounted for is printed in the message file if *PRINT, CONTACT=YES is specified. 2. Maximum number of contact iterations allowed before new global matrix assemblage and factorization. The default is 30. 18.
* SOLVER CONTROLS 18.25 *SOLVER CONTROLS: Specify controls for the iterative linear solver. This option is used to set the control parameters for the iterative linear equation solver. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Iterative linear equation solver,” Section 6.1.5 of the ABAQUS Analysis User’s Manual Optional parameter: RESET Include this parameter to reset all of the solver controls to their default values.
* SORPTION 18.26 *SORPTION: Define absorption and exsorption behavior. This option is used to define absorption and exsorption behaviors of a partially saturated porous medium in the analysis of coupled wetting liquid flow and porous medium stress. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Sorption,” Section 20.7.4 of the ABAQUS Analysis User’s Manual Optional parameters: LAW Set LAW=LOG to define the absorption or exsorption behavior by the analytical logarithmic form.
* SORPTION 3. 4. . This value must lie in the range . This value must lie in the range small positive number (since cannot be equal to . The default is 0.01. . The default is 0.01 plus a very ). Data line for TYPE=SCANNING: First (and only) line: 1. Slope of the scanning line, . This slope must be positive and larger than the slope of any segment of the absorption or exsorption behavior definitions. 18.
* SPECIFIC HEAT 18.27 *SPECIFIC HEAT: Define specific heat. This option is used to specify a material’s specific heat. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model Reference: • “Specific heat,” Section 20.2.3 of the ABAQUS Analysis User’s Manual Optional parameter: DEPENDENCIES Set this parameter equal to the number of field variables included in the definition of specific heat.
* SPECTRUM 18.28 *SPECTRUM: Define a response spectrum. This option is used to define a spectrum to be used in a *RESPONSE SPECTRUM analysis. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Response spectrum analysis,” Section 6.3.10 of the ABAQUS Analysis User’s Manual *RESPONSE SPECTRUM Required parameter: NAME Set this parameter equal to a label that will be used to refer to the spectrum. This label is used to cross-reference a spectrum on the *RESPONSE SPECTRUM option.
* SPECTRUM Date lines to define a spectrum: First line: 1. Magnitude of the spectrum. 2. Frequency, in cycles per time, at which this magnitude is used. 3. Associated damping, given as ratio of critical damping. Repeat this data line as often as necessary to define the spectrum at all frequencies at each damping value. 18.
* SPRING 18.29 *SPRING: Define spring behavior. This option is used to define the spring behavior for spring elements. In ABAQUS/Standard analyses it is also used to define the spring behavior for ITS and JOINTC elements. If the *SPRING option is being used to define part of the behavior of ITS or JOINTC elements, it must be used in conjunction with the *ITS or *JOINT options and the ELSET and ORIENTATION parameters should not be used.
* SPRING system. Set this parameter equal to the name of the *ORIENTATION definition (“Orientations,” Section 2.2.5 of the ABAQUS Analysis User’s Manual). RTOL This parameter applies only to ABAQUS/Explicit analyses. Set this parameter equal to the tolerance to be used for regularizing the material data. The default is RTOL=0.03. See “Material data definition,” Section 16.1.2 of the ABAQUS Analysis User’s Manual, for a discussion of data regularization.
* SPRING 5. Second field variable. 6. Etc., up to five field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the spring stiffness as a function of temperature and other predefined field variables. Data lines to define linear spring behavior for SPRING1, SPRING2, or JOINTC elements: First line: 1.
* SPRING 2. For SPRING2 elements give the degree of freedom with which the springs are associated at their second nodes. If the ORIENTATION parameter is included on the *SPRING option when defining spring elements or on the *JOINT option when defining joint elements, the degrees of freedom specified here are in the local system defined by the *ORIENTATION option referenced. Second line: 1. Force. 2. Relative displacement. 3. Temperature. 4. First field variable. 5. Second field variable. 6. Etc.
* SRADIATE 18.30 *SRADIATE: Specify surface radiation conditions in heat transfer analysis. This option is used to apply surface radiation boundary conditions between a nonconcave surface and a nonreflecting environment in fully coupled thermal-stress analysis. In ABAQUS/Standard it is also used for heat transfer and coupled thermal-electrical analyses. It must be used in conjunction with the *PHYSICAL CONSTANTS option, which is used to define the Stefan-Boltzmann constant.
* SRADIATE 4. Emissivity, . Repeat this data line as often as necessary to define radiation conditions for different surfaces. 18.
* STATIC 18.31 *STATIC: Static stress/displacement analysis. This option is used to indicate that the step should be analyzed as a static load step. Product: ABAQUS/Standard Type: History data Level: Step References: • • • • • “Static stress analysis,” Section 6.2.2 of the ABAQUS Analysis User’s Manual “Unstable collapse and postbuckling analysis,” Section 6.2.4 of the ABAQUS Analysis User’s Manual “Adiabatic analysis,” Section 6.5.
* STATIC by ABAQUS is not suitable. This parameter must be used in conjunction with the STABILIZE parameter and overrides the automatic calculation of the damping factor based on a value of the dissipated energy fraction. This parameter cannot be used if the RIKS parameter is included. FULLY PLASTIC This parameter is relevant only for cases where “fully plastic” analysis is required with deformation theory plasticity.
* STATIC 3. Minimum time increment allowed. Only used for automatic time incrementation. If ABAQUS/Standard finds it needs a smaller time increment than this value, the analysis is terminated. If this entry is zero, a default value of the smaller of the suggested initial time increment or 10−5 times the total time period is assumed. 4. Maximum time increment allowed. Only used for automatic time incrementation. If this value is not specified, no upper limit is imposed.
* STEADY STATE CRITERIA 18.32 *STEADY STATE CRITERIA: Specify steady-state criteria for terminating a quasi-static uni-directional simulation. This option is used to specify the norms that must be satisfied to halt a quasi-static uni-directional simulation based on achieving a steady-state condition. It must be used in conjunction with the *STEADY STATE DETECTION option. Product: ABAQUS/Explicit Type: History data Level: Step References: • • • “Steady-state detection,” Section 11.8.
* STEADY STATE CRITERIA 7. First direction cosine of force or torque norm output at the reference node. 8. Second direction cosine of force or torque norm output at the reference node. 9. Third direction cosine of force or torque norm output at the reference node. Repeat this data line as often as necessary. Each line defines a criterion that must be satisfied to achieve steady state. 18.
* STEADY STATE DETECTION 18.33 *STEADY STATE DETECTION: Specify steady-state requirements for terminating a quasi-static uni-directional simulation. This option is used to define the conditions that must be satisfied to determine that steady state has been reached. It must be used in conjunction with the *STEADY STATE CRITERIA option. Product: ABAQUS/Explicit Type: History data Level: Step References: • • • “Steady-state detection,” Section 11.8.
* STEADY STATE DETECTION 3. Third direction cosine of primary direction. 4. Global X-coordinate of a point on the cutting plane. 5. Global Y-coordinate of a point on the cutting plane. 6. Global Z-coordinate of a point on the cutting plane. 18.
* STEADY STATE DYNAMICS 18.34 *STEADY STATE DYNAMICS: excitation. Steady-state dynamic response based on harmonic This option is used to calculate the system’s linearized steady-state response to harmonic excitation. Product: ABAQUS/Standard Type: History data Level: Step References: • • • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 of the ABAQUS Analysis User’s Manual “Mode-based steady-state dynamic analysis,” Section 6.3.
* STEADY STATE DYNAMICS Set SUBSPACE PROJECTION=EIGENFREQUENCY if the projections onto the modal subspace of the dynamic equations are to be performed at each eigenfrequency within the requested ranges and at the eigenfrequencies immediately outside these ranges. The projections are then interpolated at each frequency requested on the data lines. The interpolation is done on a logarithmic or linear scale depending on the value of the FREQUENCY SCALE parameter.
* STEADY STATE DYNAMICS Data lines for a steady-state dynamics analysis: First line: 1. Lower limit of frequency range or a single frequency, in cycles/time. 2. Upper limit of frequency range, in cycles/time. If this value is given as zero, it is assumed that results are required at only one frequency and the remaining data items on the line are ignored. 3. Number of points in the frequency range at which results should be given.
* STEADY STATE TRANSPORT 18.35 *STEADY STATE TRANSPORT: Steady-state transport analysis. This option is used to indicate that the step should be analyzed as a steady-state transport analysis. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Steady-state transport analysis,” Section 6.4.1 of the ABAQUS Analysis User’s Manual “Symmetric model generation,” Section 10.3.
* STEADY STATE TRANSPORT parameter and overrides the automatic calculation of the damping factor based on a value of the dissipated energy fraction. INERTIA Include this parameter to indicate that inertia effects must be accounted for. Set INERTIA=NO (default) to ignore inertia effects. Set INERTIA=YES to include inertia effects. LONG TERM Include this parameter to indicate that there is no viscoelastic or viscoplastic material response during this step.
* STEADY STATE TRANSPORT terminated. If this entry is zero, a default value of the smaller of the suggested initial time increment or 10−5 times the total time period is assumed. 4. Maximum time increment allowed. Only used for automatic time incrementation. If this value is not specified, no upper limit is imposed. 18.
* STEP 18.36 *STEP: Begin a step. This option is used to begin each step definition. It must be followed by a procedure definition option. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Model Beginning a step in an ABAQUS/Standard analysis References: • • • • “Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User’s Manual “Convergence criteria for nonlinear problems,” Section 7.2.3 of the ABAQUS Analysis User’s Manual “Design sensitivity analysis,” Section 14.1.
* STEP CONVERT SDI This parameter determines how severe discontinuities (such as contact changes) are accounted for during nonlinear analysis. Set CONVERT SDI=NO (default) to force a new iteration if severe discontinuities occur during an iteration. Set CONVERT SDI=YES to estimate residual forces associated with severe discontinuities and check whether the equilibrium tolerances are satisfied.
* STEP NAME Set this parameter equal to a label that will be used to refer to the step on the output database. Step names in the same input file must be unique. Step names from the original input file can be reused in a restart input file. NLGEOM Omit this parameter or set NLGEOM=NO to perform a geometrically linear analysis during the current step.
* STEP Beginning a step in an ABAQUS/Explicit analysis References: • • “Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User’s Manual *END STEP Optional parameter: NAME Set this parameter equal to the name used to identify the step on the output database. Step names in the same input file must be unique. NLGEOM Set NLGEOM=YES (default) to indicate that geometric nonlinearity should be accounted for during the step (stress analysis and fully coupled thermal-stress analysis only).
* SUBMODEL 18.37 *SUBMODEL: Specify driven boundary nodes in submodeling analysis. This option is used to specify the total list of “driven nodes” for a submodel. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly Reference: • “Submodeling,” Section 10.2.
* SUBMODEL EXTERIOR TOLERANCE Set this parameter equal to the fraction of the average element size in the global model by which a driven node of the submodel may lie outside the region of the elements of the global model. The default is 0.05. For shell-to-solid submodeling the driven node may lie within a region defined by half the value of the SHELL THICKNESS parameter plus the exterior tolerance. If both tolerance parameters are specified by the user, ABAQUS uses the tighter tolerance.
* SUBSTRUCTURE COPY 18.38 *SUBSTRUCTURE COPY: Copy a substructure definition. This option is used to copy a substructure definition from one library to another or from one substructure identifier to another within one library. Product: ABAQUS/Standard Type: Model data Level: This option is not supported in a model defined in terms of an assembly of part instances. Reference: • “Using substructures,” Section 10.1.
* SUBSTRUCTURE DELETE 18.39 *SUBSTRUCTURE DELETE: Remove a substructure from the substructure library. This option is used to delete a substructure from a substructure library. Product: ABAQUS/Standard Type: Model data Level: This option is not supported in a model defined in terms of an assembly of part instances. Reference: • “Using substructures,” Section 10.1.
* SUBSTRUCTURE DIRECTORY 18.40 *SUBSTRUCTURE DIRECTORY: substructure library. List information about the substructures on a This option is used to provide a summary of information about the substructures stored on a substructure library. Product: ABAQUS/Standard Type: Model data Level: This option is not supported in a model defined in terms of an assembly of part instances. Reference: • “Using substructures,” Section 10.1.
* SUBSTRUCTURE GENERATE 18.41 *SUBSTRUCTURE GENERATE: Substructure generation analysis. This option is used to indicate that the step should be analyzed as a substructure generation step. Product: ABAQUS/Standard Type: History data Level: This option is not supported in a model defined in terms of an assembly of part instances. Reference: • “Defining substructures,” Section 10.1.
* SUBSTRUCTURE GENERATE PROPERTY EVALUATION Set this parameter equal to the frequency at which to evaluate frequency-dependent properties for viscoelasticity, springs, and dashpots during the substructure generation. If this parameter is omitted, ABAQUS/Standard will evaluate the stiffness associated with frequency-dependent springs and dashpots at zero frequency and will not consider the stiffness contributions from frequency-domain viscoelasticity in the *SUBSTRUCTURE GENERATE step.
* SUBSTRUCTURE LOAD CASE 18.42 *SUBSTRUCTURE LOAD CASE: Begin the definition of a substructure load case. This option is used to begin the definition of a substructure load case for the substructure currently being generated. It can be used only in a *SUBSTRUCTURE GENERATE analysis. Product: ABAQUS/Standard Type: History data Level: This option is not supported in a model defined in terms of an assembly of part instances. References: • • “Defining substructures,” Section 10.1.
* SUBSTRUCTURE MATRIX OUTPUT 18.43 *SUBSTRUCTURE MATRIX OUTPUT: Write a substructure’s recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and gravity load vectors to a file. This option is used to write a substructure’s recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and gravity load vectors to a file. It can be used only in a *SUBSTRUCTURE GENERATE analysis.
* SUBSTRUCTURE MATRIX OUTPUT Set OUTPUT FILE=USER DEFINED to write the results to a user-specified file in the format of the *USER ELEMENT, LINEAR option (“User-defined elements,” Section 26.15.1 of the ABAQUS Analysis User’s Manual). The name of the file is specified using the FILE NAME parameter. Set OUTPUT FILE=ODB to write the data to the output database (.odb) file.
* SUBSTRUCTURE PATH 18.44 *SUBSTRUCTURE PATH: Enter into a substructure to obtain output or return back from a previously entered substructure. This option is used to navigate through “levels” of substructures to obtain output of results. Product: ABAQUS/Standard Type: History data Level: This option is not supported in a model defined in terms of an assembly of part instances. Reference: • “Using substructures,” Section 10.1.
* SUBSTRUCTURE PROPERTY 18.45 *SUBSTRUCTURE PROPERTY: Translate, rotate, and/or reflect substructures. This option is used to define properties for a substructure. It is required for all substructures in a model. Product: ABAQUS/Standard Type: Model data Level: This option is not supported in a model defined in terms of an assembly of part instances. Reference: • “Using substructures,” Section 10.1.
* SUBSTRUCTURE PROPERTY 3. Value of the translation to be applied in the global Z-direction. Enter values of zero to apply a pure rotation. Second line: 1. Global X-coordinate of point a on the axis of rotation (see Figure 18.45–1). 2. Global Y-coordinate of point a on the axis of rotation. 3. Global Z-coordinate of point a on the axis of rotation. 4. Global X-coordinate of point b on the axis of rotation. 5. Global Y-coordinate of point b on the axis of rotation. 6.
* SUBSTRUCTURE PROPERTY Data lines to translate, rotate, and reflect a substructure: First line: 1. Value of the translation to be applied in the global X-direction. 2. Value of the translation to be applied in the global Y-direction. 3. Value of the translation to be applied in the global Z-direction. Second line: 1. Global X-coordinate of point a on the axis of rotation (see Figure 18.45–1). 2. Global Y-coordinate of point a on the axis of rotation. 3.
* SUBSTRUCTURE PROPERTY b θ θ a Figure 18.45–1 Substructure rotation. c b a Figure 18.45–2 Substructure reflection. Points a, b, and c cannot be colinear. 18.
* SURFACE 18.46 *SURFACE: Define a surface or region in a model. This option is used to define surfaces for contact simulations, tie constraints, fasteners, and coupling, as well as regions for distributed surface loads, acoustic radiation, acoustic impedance, and output of integrated quantities on a surface. In ABAQUS/Standard it is also used to define surfaces for cavity radiation analysis and assembly loads.
* SURFACE Set COMBINE=INTERSECTION to create a surface based on the intersection of two surfaces of the same type. Set COMBINE=DIFFERENCE to create a surface based on the difference of two surfaces of the same type (the second surface is subtracted from the first). Only the NAME parameter and, in cavity radiation simulations, the PROPERTY parameter can be used in conjunction with this parameter.
* SURFACE finite-sliding contact formulation in ABAQUS/Standard or the surface is used with the contact pair algorithm in ABAQUS/Explicit. TRIM=YES has no effect on surfaces used with the contact pair algorithm in ABAQUS/Explicit. TYPE Set TYPE=ELEMENT (default) to define a free surface automatically for the elements specified or to define a surface on the elements by using element face identifiers. Set TYPE=NODE to define a surface by specifying a list of nodes or node set labels.
* SURFACE Data lines for COMBINE=UNION: First line: 1. List of surfaces. Repeat this data line as often as necessary. Up to 16 entries are allowed per line. Data line for COMBINE=INTERSECTION or COMBINE=DIFFERENCE: First (and only) line: 1. First surface name. 2. Second surface name. For COMBINE=DIFFERENCE the second surface is subtracted from the first. Data lines to define a surface when the CROP parameter is included: First line: 1. Surface name. Second line: 1. 2. 3. 4. 5. 6.
* SURFACE 2. Face or edge identifier label (see “Defining element-based surfaces,” Section 2.3.2 of the ABAQUS Analysis User’s Manual, for the face and edge identifiers for various elements) or the “word” EDGE (optional). Repeat this data line as often as necessary to define the surface. Data lines to define a surface using nodes or node sets when the TYPE=NODE parameter is used: First line: 1. Node set name or node number. 2. Cross-sectional area or distributing weight factor.
* SURFACE 3. Global Y-coordinate or z-coordinate of the starting point of the line segments. Second and subsequent data lines define the various line, circular, and parabolic segments (see below for their format) that form the profile of the analytical surface. Data lines to define surfaces created with TYPE=CYLINDER: First line (leave blank if this surface is being defined within a part): 1. 2. 3. 4. 5. 6.
* SURFACE 3. Local z-coordinate of the starting point of the line segments. Third and subsequent data lines define the various line, circular, and parabolic segments (see below for their format) that form the profile of the analytical surface. Data lines that define the line segments that form the analytical surface for TYPE=SEGMENTS, TYPE=CYLINDER, and TYPE=REVOLUTION: Data line to define a straight line segment: 1. The “word” LINE. 2. x-coordinate of the end point of the line. 3.
* SURFACE n Outward normal n Line segment Start Circular arc segment Local y-axis c b Generator direction a Local z-axis Local x-axis Figure 18.46–1 *SURFACE, TYPE=CYLINDER. 18.
* SURFACE local z Start n b line segment a local r circular arc segment n Figure 18.46–2 *SURFACE, TYPE=REVOLUTION. 18.
* SURFACE BEHAVIOR 18.47 *SURFACE BEHAVIOR: contact. Define alternative pressure-overclosure relationships for This option is used to modify the default hard contact pressure-overclosure relationship in a mechanical contact analysis. Mechanical interactions normal to the surfaces are influenced by this option. It must be used in conjunction with the *SURFACE INTERACTION option or in an ABAQUS/Standard analysis with the *GAP option or the *INTERFACE option.
* SURFACE BEHAVIOR ABAQUS Analysis User’s Manual, for a discussion of the default penalty stiffness. You can specify or modify the penalty stiffness on the data line. Optional parameters: NO SEPARATION Include this parameter to prevent any separation of the two surfaces once contact has been established. PRESSURE-OVERCLOSURE Use this parameter to choose a contact pressure-overclosure relationship other than the default hard contact.
* SURFACE BEHAVIOR Data line for PRESSURE-OVERCLOSURE=EXPONENTIAL: First (and only) line: 1. Clearance at which the contact pressure is zero, 2. Pressure at zero clearance, (see Figure 18.47–1). . The following data item is available only in ABAQUS/Explicit analyses: . When using penalty contact, large stiffness values 3. Value of the maximum stiffness, obtained from the exponential law may significantly lower the stable time increment size.
* SURFACE BEHAVIOR Repeat this data line in ascending order of overclosure value as often as necessary to define the overclosure as a function of pressure. A minimum of two data lines are required. The pressure-overclosure relationship is extrapolated beyond the last overclosure point by continuing the same slope (see Figure 18.47–3). Contact pressure Kmax Exponential pressure-overclosure relationship Clearance p0 c0 Figure 18.47–1 Overclosure Exponential pressure-overclosure relationship.
* SURFACE BEHAVIOR Pressure p (pn,hn) (p2,h2) Clearance c Figure 18.47–3 (p3,h3) (0,h1) Overclosure h Pressure-overclosure relationship defined in tabular form. 18.
* SURFACE FLAW 18.48 *SURFACE FLAW: Define geometry of surface flaws. This option is used with line spring elements to define the geometry of the part-through crack of the shell. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance Reference: • “Line spring elements for modeling part-through cracks in shells,” Section 26.10.1 of the ABAQUS Analysis User’s Manual Required parameter: SIDE Set SIDE=POSITIVE or SIDE=NEGATIVE to indicate which surface is cracked.
* SURFACE INTERACTION 18.49 *SURFACE INTERACTION: Define surface interaction properties. This option is used to create a surface interaction property definition. The surface interaction properties will govern any contact interactions that reference this surface interaction.
* SURFACE INTERACTION Set this parameter equal to the thickness of an interfacial layer between the contacting surfaces. The value can be positive or negative. USER Include this parameter if the surface interaction model is to be defined in user subroutine UINTER in an ABAQUS/Standard analysis or in user subroutine VUINTER in an ABAQUS/Explicit analysis. When this parameter is included, the *SURFACE BEHAVIOR option and its various suboptions cannot be used under the same interaction definition.
* SURFACE INTERACTION Second line (needed only if the PROPERTIES parameter is used): 1. Enter the values of the surface interaction properties, eight per line. Repeat this data line as often as necessary to define all material constants. Data lines to define the surface interaction in an ABAQUS/Explicit analysis if the PROPERTIES parameter is used: First line: 1. Enter a blank line. Second line: 1. Enter the values of the surface interaction properties, eight per line.
* SURFACE PROPERTY 18.50 *SURFACE PROPERTY: Define surface properties for cavity radiation. This option is used to define surface properties for cavity radiation analysis. It must immediately precede the *EMISSIVITY option. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Cavity radiation,” Section 32.1.
* SURFACE PROPERTY ASSIGNMENT 18.51 *SURFACE PROPERTY ASSIGNMENT: general contact algorithm. Assign surface properties to a surface for the This option is used to modify surface properties for surfaces that are involved in general contact interactions in ABAQUS/Explicit. It must be used in conjunction with the *CONTACT option. Product: ABAQUS/Explicit Type: Model or history data Level: Model, Step References: • • “Surface properties for general contact,” Section 29.3.
* SURFACE PROPERTY ASSIGNMENT Data lines for PROPERTY=OFFSET FRACTION: First line: 1. Surface name. If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Faces specified on elements other than shell elements, membrane elements, rigid elements, and surface elements will be ignored. 2. The “word” ORIGINAL (default), the “word” SPOS, the “word” SNEG, or a value between –0.5 and 0.5.
* SURFACE SECTION 18.52 *SURFACE SECTION: Specify section properties for surface elements. This option is used to specify a surface element cross-section. It must be used in conjunction with the *REBAR LAYER option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • • “Surface elements,” Section 26.7.1 of the ABAQUS Analysis User’s Manual “Defining reinforcement,” Section 2.2.
* SWELLING 18.53 *SWELLING: Specify time-dependent volumetric swelling. This option is used to specify time-dependent metal swelling for a material. Swelling behavior defined by this option is active only during *SOILS, CONSOLIDATION; *COUPLED TEMPERATUREDISPLACEMENT; and *VISCO procedures. Product: ABAQUS/Standard Type: Model data Level: Model References: • • “Rate-dependent plasticity: creep and swelling,” Section 18.2.4 of the ABAQUS Analysis User’s Manual “CREEP,” Section 1.1.
* SWELLING 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of volumetric swelling strain rate on temperature and other predefined field variables. 18.
* SYMMETRIC MODEL GENERATION 18.54 *SYMMETRIC MODEL GENERATION: Create a three-dimensional model from an axisymmetric or partial three-dimensional model.
* SYMMETRIC MODEL GENERATION Optional parameters: ELEMENT OFFSET Set this parameter equal to an integer to define the offset for element numbering. When the REVOLVE parameter is used, the offset is added to each element number on the previous cross-section to obtain the numbering of the elements on the next cross-section, starting at the reference cross-section, . The reference cross-section uses the same numbering as the original axisymmetric model.
* SYMMETRIC MODEL GENERATION Second line: 1. Segment angle, (in degrees), of the original three-dimensional sector. . 2. Number of three-dimensional repetitive sectors, including the original sector in the generated periodic model. The default is 1. Third line (needed if the surface meshes on either side of the original sector are not matched completely): 1. The surface name on one side of the original sector. 2.
* SYMMETRIC MODEL GENERATION 2. Angular scaling factor in the circumferential direction with respect to the original sector. The default is 1.0. Repeat the third data line as often as necessary to define all the sectors of the model in the circumferential direction. Subsequent lines (needed if the surface meshes on either side of the original sector are not matched completely): 1. The surface name on one side of the original sector. 2.
* SYMMETRIC MODEL GENERATION Second line: 1. X-coordinate of point c. 2. Y-coordinate of point c. 3. Z-coordinate of point c. Data lines if the REVOLVE parameter is included: First line: 1. X-coordinate of point a. 2. Y-coordinate of point a. 3. Z-coordinate of point a. 4. X-coordinate of point b. 5. Y-coordinate of point b. 6. Z-coordinate of point b. Second line: 1. X-coordinate of point c. 2. Y-coordinate of point c. 3. Z-coordinate of point c. Third line: 1.
* SYMMETRIC MODEL GENERATION b θ a y x z Figure 18.54–1 Revolving a single three-dimensional repetitive sector to create a periodic structure. z b θ Y X z a Z c reference cross-section at θ = 0 r Figure 18.54–2 Revolving an axisymmetric cross-section. 18.
* SYMMETRIC MODEL GENERATION reflection line b 8 6+n 7 7+n 6 5 4 1 Figure 18.54–3 5+n 8+n 2+n 3 1+n 2 a 3+n 4+n Reflecting a three-dimensional model through line ab with node offset n. 18.
* SYMMETRIC MODEL GENERATION reflection plane 7 8 5 7+n 6+n 6 8+n 5+n b c 4 1 3+n 3 4+n 2 2+n 1+n a Figure 18.54–4 Reflecting a three-dimensional model through a plane abc with node offset n. 18.
* SYMMETRIC RESULTS TRANSFER 18.55 *SYMMETRIC RESULTS TRANSFER: three-dimensional analysis. Import results from an axisymmetric or partial This option is used to transfer a solution from an axisymmetric analysis to a three-dimensional model or to transfer the solution of a partial three-dimensional model to a full three-dimensional model. It can be used only in conjunction with the *SYMMETRIC MODEL GENERATION option.
* SYMMETRIC RESULTS TRANSFER Set UNBALANCED STRESS=RAMP if the stress unbalance is to be resolved linearly over the step. There are no data lines associated with this option. 18.
* SYSTEM 18.56 *SYSTEM: Specify a local coordinate system in which to define nodes. This option is used to define nodes by accepting coordinates relative to a specified local rectangular coordinate system and generating the nodal coordinates in the global coordinate system. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance Reference: • “Node definition,” Section 2.1.1 of the ABAQUS Analysis User’s Manual There are no parameters associated with this option.
* SYSTEM Z Z 1 1 Y Y c a b X (global) Figure 18.56–1 Local coordinate system. 18.
T 19.
* TEMPERATURE 19.1 *TEMPERATURE: Specify temperature as a predefined field. This option is used to specify temperature as a predefined field during an analysis. To use this option in a restart analysis of ABAQUS/Standard, either *TEMPERATURE or *INITIAL CONDITIONS, TYPE=TEMPERATURE must have been specified in the original analysis. Products: ABAQUS/Standard ABAQUS/Explicit Type: History data Level: Step References: • • “Predefined fields,” Section 27.6.
* TEMPERATURE apply. Rather, the AMPLITUDE parameter given on the *STEP option governs the behavior in an ABAQUS/Standard analysis, and the temperatures are always ramped back to their initial conditions in ABAQUS/Explicit analyses. If temperatures are being reset to new values (not to initial conditions) via OP=NEW, the AMPLITUDE parameter described above applies.
* TEMPERATURE ESTEP Set this parameter equal to the step number (of the analysis whose results or output database file is being used as input to this option) that ends the history data to be read. If no value is supplied, ESTEP is taken as equal to BSTEP. EINC Set this parameter equal to the increment number (of the analysis whose results or output database file is being used as input to this option) that ends the history data to be read.
* TEMPERATURE 2. Reference temperature value. If the AMPLITUDE parameter is present, this value and subsequent temperature values will be modified by the AMPLITUDE specification. 3. Temperature gradient in the thickness for shells. -direction for beams or temperature gradient through the 4. Temperature gradient in the -direction for beams. Repeat this data line as often as necessary to define temperatures at different nodes or node sets.
* TEMPERATURE Data lines to define temperatures using user subroutine UTEMP: First line: 1. Node set or node number. Repeat this data line as often as necessary. UTEMP will be called for each node listed. 19.
* TENSILE FAILURE 19.2 *TENSILE FAILURE: Specify a tensile failure model and criterion. This option is used with the Mises or the Johnson-Cook plasticity models or the equation of state model to specify a tensile failure model and criterion. It must be used in conjunction with the *PLASTIC, HARDENING=ISOTROPIC option; the *PLASTIC, HARDENING=JOHNSON COOK option; or the *EOS option. Product: ABAQUS/Explicit Type: Model data Level: Model References: • • • • • • “Equation of state,” Section 17.9.
* TENSILE FAILURE Set PRESSURE=DUCTILE to model the case where the pressure stress will be limited by the hydrostatic cutoff stress when the failure criterion is met. SHEAR Set SHEAR=BRITTLE to model the case where the deviatoric stresses will be set to zero when the failure criterion is met. Set SHEAR=DUCTILE to model the case where the deviatoric stresses will be unaffected when the failure criterion is met. Data lines to specify a tensile failure model: First line: 1.
* TENSION STIFFENING 19.3 *TENSION STIFFENING: *CONCRETE model. Define the retained tensile stress normal to a crack in a This option is used to define the retained tensile stress normal to a crack as a function of the deformation in the direction of the normal to the crack. It must be used with and appear after the *CONCRETE option. The *TENSION STIFFENING option can also be used in conjunction with the *SHEAR RETENTION and *FAILURE RATIOS options.
* TENSION STIFFENING 4. First field variable. 5. Second field variable. 6. Etc., up to five field variables. The first point at each value of temperature must be a stress fraction of 1.0 at a strain of 0.0. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five): 1. Sixth field variable. 2. Etc., up to eight field variables per line.
* THERMAL EXPANSION 19.4 *THERMAL EXPANSION: Define the thermal expansion behavior of beams. This option can be used only in conjunction SECTION=NONLINEAR GENERAL option. Products: ABAQUS/Standard with the *BEAM GENERAL SECTION, ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • “Using a general beam section to define the section behavior,” Section 23.3.
* TIE 19.5 *TIE: Define surface-based tie and cyclic symmetry constraints or coupled acousticstructural interactions. This option is used to impose tie constraints, cyclic symmetry constraints, or coupled acoustic-structural interactions between pairs of surfaces. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly References: • • • • • “Mesh tie constraints,” Section 28.3.1 of the ABAQUS Analysis User’s Manual “Defining element-based surfaces,” Section 2.
* TIE Optional parameters: ADJUST Set ADJUST=YES (default) to move all tied nodes on the slave surface onto the master surface in the initial configuration, without any strain. Set ADJUST=NO if the slave nodes will not be moved. This is the default if the slave surface belongs to a substructure or if one or more of the surfaces is beam element-based.
* TIME POINTS 19.6 *TIME POINTS: Specify time points at which data are written to the output database or restart files, or specify time points in the loading history at which the response of a structure will be evaluated in a direct cyclic analysis.
* TIME POINTS Data lines if the GENERATE parameter is omitted: First line: 1. List of time points; the points must be arranged in ascending order. Repeat this data line as often as necessary. Up to eight entries are allowed per line. If you use the *TIME POINTS option in conjunction with the *DIRECT CYCLIC option, the listed time points must include the starting time and ending time in a single loading cycle. The time points must be specified in the step time.
* TORQUE 19.7 *TORQUE: Define the torsional behavior of beams. This option can be used only in conjunction SECTION=NONLINEAR GENERAL option. Products: ABAQUS/Standard with the *BEAM GENERAL SECTION, ABAQUS/Explicit Type: Model data Level: Part, Part instance References: • • “Using a general beam section to define the section behavior,” Section 23.3.
* TORQUE Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than six): 1. Seventh field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the torsional stiffness as a function of temperature and other predefined field variables. Data lines if the LINEAR parameter is omitted: First line: 1. Torque. 2. Twist. 3. Temperature. 4. First field variable. 5. Second field variable. 6. Etc.
* TORQUE PRINT 19.8 *TORQUE PRINT: Print a summary of the total torque that can be transmitted across axisymmetric slide lines. This option is used to obtain a summary of the total torque that can be transmitted across all axisymmetric slide lines in a model. Product: ABAQUS/Standard Type: History data Level: Step Reference: • “Slide line contact elements,” Section 31.4.
* TRACER PARTICLE 19.9 *TRACER PARTICLE: Define tracer particles for tracking the location of and results at material points during a step. This option is used to define tracer particles and assign them to tracer sets for tracking the location of and results at material points during a step. The tracer set name is used in conjunction with the *ELEMENT OUTPUT and/or the *NODE OUTPUT options to request output for the tracer particles associated with the tracer set name.
* TRANSFORM 19.10 *TRANSFORM: Specify a local coordinate system at nodes. This option is used to specify a local coordinate system for displacement and rotation degrees of freedom at a node. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Part, Part instance, Assembly Reference: • “Transformed coordinate systems,” Section 2.1.
* TRANSFORM Z Z 1 Y1 Y b a X1 X (global) Figure 19.10–1 Cartesian transformation option. (radial) X Z 1 (axial) Z 1 b Y a 1 Y (tangential) X (global) Figure 19.10–2 Cylindrical transformation option. 19.
* TRANSFORM b 1 Z (meridional) Z 1 Y (circumferential) Y a 1 X (radial) X (global) Figure 19.10–3 Spherical transformation option. 19.
* TRANSPORT VELOCITY 19.11 *TRANSPORT VELOCITY: Specify angular transport velocity. This option is used to define the angular velocity of material transported through the mesh of a deformable body or the transport of material relative to the reference node of a rigid body during a steady-state transport analysis. Product: ABAQUS/Standard Type: History data Level: Step References: • • • “Steady-state transport analysis,” Section 6.4.
* TRANSPORT VELOCITY GENERATION option. For a rigid body of type REVOLUTION the rotation is assumed to be about the axis of revolution of the body. Repeat this data line as often as necessary to define rotational motion on nodes of different parts of the model. 19.
* TRANSVERSE SHEAR STIFFNESS 19.12 *TRANSVERSE SHEAR STIFFNESS: shells. Define transverse shear stiffness for beams and This option must be used in conjunction with the *BEAM GENERAL SECTION option, the *BEAM SECTION option, the *COHESIVE SECTION option, the *SHELL GENERAL SECTION option, or the *SHELL SECTION option.
* TRANSVERSE SHEAR STIFFNESS Data line when used with all other beam sections: First (and only) line: 1. Value of the shear stiffness of the section. 2. Value of the shear stiffness of the section. 3. Value of the slenderness compensation factor or the label SCF. If this field is left blank, a default value of 0.25 is assumed. If the label SCF is specified, the values of the shear stiffness specified by the user will be ignored.
* TRIAXIAL TEST DATA 19.13 *TRIAXIAL TEST DATA: Provide triaxial test data. This option is required if some or all of the material parameters that define the exponent form of the *DRUCKER PRAGER option are to be calibrated from triaxial test data. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “Extended Drucker-Prager models,” Section 18.3.
* TRS 19.14 *TRS: Used to define temperature-time shift for time history viscoelastic analysis. This option can be used only in conjunction with the *VISCOELASTIC option. In an ABAQUS/Standard analysis, viscoelasticity must be defined in the time domain by using the VISCOELASTIC option with the TIME parameter. * Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • “Time domain viscoelasticity,” Section 17.7.
U 20.
* UEL PROPERTY 20.1 *UEL PROPERTY: Define property values to be used with a user element type. This option is used to define the properties of a user element. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance, Model References: • • “User-defined elements,” Section 26.15.1 of the ABAQUS Analysis User’s Manual *USER ELEMENT Required parameter: ELSET Set this parameter equal to the name of the element set containing the user elements for which these property values are being defined.
* UNDEX CHARGE PROPERTY 20.2 *UNDEX CHARGE PROPERTY: Define an UNDEX charge for incident waves. This option defines parameters that create the time histories of load, displacement, and other variables used to simulate an underwater explosion. This option must be used in conjunction with the *INCIDENT WAVE INTERACTION PROPERTY option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model or history data Level: Model, Step References: • • “Acoustic loads,” Section 27.4.
* UNDEX CHARGE PROPERTY 2. Maximum number of time steps for the bubble simulation, . The bubble amplitude simulation ceases when the number of steps reaches or the time duration, , is reached. . 3. Relative step size control parameter, . 4. Absolute step size control parameter, , is decreased or increased according to the 5. Step size control exponent, . The step size, error estimate: . Fourth line: 1. Depth magnitude of charge material, . 2. X-direction cosine of fluid surface normal. 3.
* UNIAXIAL TEST DATA 20.3 *UNIAXIAL TEST DATA: tension). Used to provide uniaxial test data (compression and/or This option is used to provide uniaxial test data. It can be used only in conjunction with the *HYPERELASTIC option, the *HYPERFOAM option, and the *MULLINS EFFECT option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model Using uniaxial test data to define a hyperelastic material References: • • “Hyperelastic behavior of rubberlike materials,” Section 17.5.
* UNIAXIAL TEST DATA Data lines to specify uniaxial test data for the Marlow model: First line: 1. Nominal stress, . 2. Nominal strain, . . Not needed if the POISSON parameter is specified on the 3. Nominal lateral strain, *HYPERELASTIC option or if the *VOLUMETRIC TEST DATA option is used. 4. Temperature, . 5. First field variable. 6. Second field variable. 7. Etc., up to four field variables. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than four): 1.
* UNIAXIAL TEST DATA Using uniaxial test data to define the Mullins effect material model References: • • • “Mullins effect in rubberlike materials,” Section 17.6.1 of the ABAQUS Analysis User’s Manual “Energy dissipation in elastomeric foams,” Section 17.6.2 of the ABAQUS Analysis User’s Manual *MULLINS EFFECT There are no parameters associated with this option. Data lines to specify uniaxial test data for defining the unloading-reloading response of the Mullins effect material model: First line: 1.
* USER DEFINED FIELD 20.4 *USER DEFINED FIELD: Redefine field variables at a material point. This material option is used to allow the values of field variables at a material point to be redefined within an increment via user subroutine USDFLD. If the *USER DEFINED FIELD option is used, it must appear within a *MATERIAL definition (“Material data definition,” Section 16.1.2 of the ABAQUS Analysis User’s Manual). Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “USDFLD,” Section 1.1.
* USER ELEMENT 20.5 *USER ELEMENT: Introduce a user-defined element type. This option is used to introduce a linear or a general user-defined element. It must precede any reference to this user element on an *ELEMENT option. Product: ABAQUS/Standard Type: Model data Level: Part, Part instance, Model Introducing a linear user-defined element References: • • • • “User-defined elements,” Section 26.15.
* USER ELEMENT Required parameters if the FILE parameter is included: OLD ELEMENT Set this parameter equal to the element number that was assigned to the element whose matrices are being read. This parameter can also be set to a substructure identifier to read a substructure matrix from an ABAQUS/Standard results file. STEP Set this parameter equal to the step number in which the element matrix was written.
* USER ELEMENT Second line if the active degrees of freedom are different at subsequent nodes: 1. Enter the position in the connectivity list (node position on the element) where the new list of active degrees of freedom first applies. 2. Enter the new list of active degrees of freedom. Repeat the second data line as often as necessary. Introducing a general user-defined element References: • • • • “User-defined elements,” Section 26.15.1 of the ABAQUS Analysis User’s Manual “UEL,” Section 1.1.
* USER ELEMENT PROPERTIES Set this parameter equal to the number of real (floating point) property values needed as data in user subroutine UEL to define such an element. The default is PROPERTIES=0. UNSYMM Include this parameter if the element matrices are not symmetric. This parameter will cause ABAQUS/Standard to use its unsymmetric equation solution capability. VARIABLES Set this parameter equal to the number of solution-dependent state variables that must be stored within the element.
* USER MATERIAL 20.6 *USER MATERIAL: VUMAT. Define material constants for use in subroutine UMAT, UMATHT, or This option is used to input material constants for use in a user-defined mechanical model (user subroutine UMAT in ABAQUS/Standard or user subroutine VUMAT in ABAQUS/Explicit). In ABAQUS/Standard it is also used to input material constants for use in a user-defined thermal material model (user subroutine UMATHT).
* USER MATERIAL Include this parameter if the material stiffness matrix, , is not symmetric or when a thermal constitutive model is used and is not symmetric. This parameter causes ABAQUS/Standard to use its unsymmetric equation solution procedures. Data lines to define material constants: First line: 1. Give the material constants, eight per line. Repeat this data line as often as necessary to define all material constants. 20.
* USER OUTPUT VARIABLES 20.7 *USER OUTPUT VARIABLES: Specify number of user variables. This option is used to allow ABAQUS to allocate space at each material calculation point for user-defined output variables defined in user subroutine UVARM. If the *USER OUTPUT VARIABLES option is used, it must appear within each of the relevant material or gasket behavior definitions. Product: ABAQUS/Standard Type: Model data Level: Model Reference: • “UVARM,” Section 1.1.
V 21.
* VARIABLE MASS SCALING 21.1 *VARIABLE MASS SCALING: Specify mass scaling during the step. This option is used to specify mass scaling during the step for part or all of the model. Product: ABAQUS/Explicit Type: History data Level: Step References: • • “Mass scaling,” Section 11.7.1 of the ABAQUS Analysis User’s Manual “Output,” Section 4.1.
* VARIABLE MASS SCALING Required, mutually exclusive parameters if the DT parameter or the TYPE=ROLLING parameter is used: FREQUENCY Set this parameter equal to the frequency, in increments, at which mass scaling calculations are to be performed during the step. For example, FREQUENCY=5 will scale the mass at the beginning of the step and at increments 5, 10, 15, etc. The value of this parameter must be a positive integer.
* VIEWFACTOR OUTPUT 21.2 *VIEWFACTOR OUTPUT: Write radiation viewfactors to the results file in cavity radiation heat transfer analysis. This option is used to write cavity radiation element viewfactor matrices to the results file. This option is available only for heat transfer analysis including cavity radiation. Product: ABAQUS/Standard Type: History data Level: Step References: • • “Cavity radiation,” Section 32.1.1 of the ABAQUS Analysis User’s Manual “Output,” Section 4.1.
* VISCO 21.3 *VISCO: Transient, static, stress/displacement analysis with time-dependent material response (creep, swelling, and viscoelasticity). This option is used to obtain a transient static response in an analysis with time-dependent material behavior (creep, swelling, and viscoelasticity). Product: ABAQUS/Standard Type: History data Level: Step References: • • “Quasi-static analysis,” Section 6.2.5 of the ABAQUS Analysis User’s Manual “Rate-dependent plasticity: creep and swelling,” Section 18.
* VISCO STABILIZE Include this parameter to use automatic stabilization if the problem is expected to be unstable due to local instabilities. Set this parameter equal to the dissipated energy fraction of the automatic damping algorithm (see “Solving nonlinear problems,” Section 7.1.1 of the ABAQUS Analysis User’s Manual). If this parameter is omitted, the stabilization algorithm is not activated.
* VISCOELASTIC 21.4 *VISCOELASTIC: Specify dissipative behavior for use with elasticity. This option is used to generalize a material’s elastic response to include viscoelasticity. The viscoelasticity can be defined as a function of frequency for steady-state small-vibration analyses or as a function of reduced time for time-dependent analyses. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • • • • • “Time domain viscoelasticity,” Section 17.7.
* VISCOELASTIC TIME Use this parameter to choose the time domain definition. In this case the material’s elasticity must be defined using the *ELASTIC, the *HYPERELASTIC, or the *HYPERFOAM option. Set TIME=CREEP TEST DATA if the Prony series parameters are to be computed by ABAQUS from data taken from shear and volumetric creep tests. Set TIME=FREQUENCY DATA if the Prony series parameters are to be computed by ABAQUS from frequency-dependent cyclic test data.
* VISCOELASTIC Optional parameters when test data are given to define time domain viscoelasticity with TIME=CREEP TEST DATA or TIME=RELAXATION TEST DATA or when test data are given to define frequency domain viscoelasticity with FREQUENCY=PRONY, FREQUENCY=CREEP TEST DATA, or FREQUENCY=RELAXATION TEST DATA: ERRTOL Set this parameter equal to the allowable average root-mean-square error of the data points in the least-squares fit. The default is 0.01 (1%).
* VISCOELASTIC 3. Frequency, f, in cycles per time. 4. Uniaxial nominal strain (defines the level of uniaxial preload). Repeat this data line as often as necessary to define the uniaxial loss and storage moduli as functions of frequency and preload. Data lines to define continuum material properties for FREQUENCY=TABULAR, PRELOAD=VOLUMETRIC: First line: 1. Bulk loss modulus. 2. Bulk storage modulus. 3. Frequency, f, in cycles per time. 4.
* VISCOELASTIC 4. Closure (defines the level of preload). Repeat this data line as often as necessary to define the effective thickness-direction gasket loss and storage moduli as functions of frequency and preload. Data lines to define effective thickness-direction gasket properties if PRELOAD=UNIAXIAL is not included: First line: 1. Real part of . direction dynamic stiffness. , where . 2. Imaginary part of thickness direction dynamic stiffness.
* VISCOUS 21.5 *VISCOUS: Specify viscous material properties for the two-layer viscoplastic model. This option is used to define the viscous properties for the two-layer viscoplastic material model. It must be used in conjunction with the *ELASTIC and *PLASTIC options. Product: ABAQUS/Standard Type: Model data Level: Model References: • • • • “Two-layer viscoplasticity,” Section 18.2.
* VISCOUS 7. Second field variable. 8. Third field variable. Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than three): 1. Fourth field variable. 2. Etc., up to eight field variables per line. Repeat this set of data lines as often as necessary to define the dependence of the viscous constants on temperature and other predefined field variable. Data lines for LAW=USER: First line: 1. f. 2. Temperature. 3. First field variable. 4. Second field variable. 5. Etc.
* VOID NUCLEATION 21.6 *VOID NUCLEATION: Define the nucleation of voids in a porous material. This option is used to model the nucleation of voids in a porous material. It can be used only with the *POROUS METAL PLASTICITY option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model References: • • “Porous metal plasticity,” Section 18.2.
* VOLUMETRIC TEST DATA 21.7 *VOLUMETRIC TEST DATA: Provide volumetric test data. This option can be used only in conjunction with the *HYPERELASTIC option, the *HYPERFOAM option, or the *VISCOELASTIC option. Products: ABAQUS/Standard ABAQUS/Explicit Type: Model data Level: Model Hyperelastic material model Volumetric loading test data can be provided by this option to include user-defined material compressibility.
* VOLUMETRIC TEST DATA See “Using the DEPENDENCIES parameter to define field variable dependence” in “Material data definition,” Section 16.1.2 of the ABAQUS Analysis User’s Manual, for more information. Data lines to specify volumetric test data for hyperelasticity other than the Marlow model: First line: 1. Pressure, p. 2. Volume ratio, J (current volume/original volume). Repeat this data line as often as necessary. Data lines to specify volumetric test data for the Marlow model: First line: 1. 2. 3.
* VOLUMETRIC TEST DATA Viscoelastic material model References: • • “Time domain viscoelasticity,” Section 17.7.1 of the ABAQUS Analysis User’s Manual *VISCOELASTIC Optional parameter: VOLINF To specify creep test data, set this parameter equal to the value of the long-term, normalized . volumetric compliance, To specify relaxation test data, set this parameter equal to the value of the long-term, normalized volumetric modulus . The volumetric compliance is related to the volumetric modulus by .
W, X, Y, Z 22.
* WAVE 22.1 *WAVE: Define gravity waves for use in immersed structure calculations. This option is used to define gravity waves for use in applying loads. Product: ABAQUS/Aqua Type: Model data Level: Model Reference: • “ABAQUS/Aqua analysis,” Section 6.10.1 of the ABAQUS Analysis User’s Manual Optional parameters: INPUT Set this parameter equal to the name of the alternate input file containing the data lines for this option. See “Input syntax rules,” Section 1.2.
* WAVE Optional parameters for TYPE=GRIDDED: MINIMUM Set this parameter equal to the elevation below which point the structure is fully immersed for all time t. If this parameter is omitted, the elevation of the structure is compared against the instantaneous free surface to check for fluid surface penetration. QUADRATIC Include this parameter to indicate that quadratic interpolation of the wave data is used to determine information between grid points.
* WAVE 5. y-direction cosine defining the direction of the vector (the direction of travel for this wave component). This component is not needed in two-dimensional cases. Repeat this data line as often as necessary to define multiple wave trains; one line per wave component. Data line to define gridded wave data (TYPE=GRIDDED): First (and only) line: 1. x-coordinate of the origin of the wave data grid. 2. y-coordinate of the origin of the wave data grid. 3.
* WIND 22.2 *WIND: Define wind velocity profile for wind loading. This option is used to define a wind velocity profile for use in applying loads. Product: ABAQUS/Aqua Type: Model data Level: Model Reference: • “ABAQUS/Aqua analysis,” Section 6.10.1 of the ABAQUS Analysis User’s Manual There are no parameters associated with this option. Data line to define the wind velocity profile: First (and only) line: 1. Air density, . 2. Reference height for wind profile, . 3.
About ABAQUS, Inc. Founded in 1978, ABAQUS, Inc. is the world's leading provider of advanced Finite Element Analysis software and services that are used to solve real-world engineering problems. The ABAQUS software suite has an unsurpassed reputation for technology, quality, and reliability and provides a powerful and complete solution for both routine and sophisticated linear and nonlinear engineering problems.