3D Connexion Keywords Reference Manual Volume Ii Version 6 Owners ABAQUS Manual, Vol 2

Version 6.6 to the manual 499e08c7-d0a4-4af4-a479-8af8d400cf7f

2015-02-05

: 3D-Connexion 3D-Connexion-Keywords-Reference-Manual-Volume-Ii-Version-6-6-Owners-Manual-135660 3d-connexion-keywords-reference-manual-volume-ii-version-6-6-owners-manual-135660 3d-connexion pdf

Open the PDF directly: View PDF PDF.
Page Count: 628 [warning: Documents this large are best viewed by clicking the View PDF Link!]

Keywords Reference ManualKeywords Reference Manual
Volume II: I–Z
Version 6.6
ABAQUS Keywords
Reference Manual
Volume II
Version 6.6
ABAQUS Version 6.1 Module: ID:
Printed on:
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. will not be responsible for the accuracy or usefulness of any analysis performed using the ABAQUS Software or the procedures, examples,
or explanations in this manual. ABAQUS, Inc. shall not be responsible for the consequences of any errors or omissions that may appear in this manual.
ABAQUS, INC. DISCLAIMS ALL EXPRESS OR IMPLIED REPRESENTATIONS AND WARRANTIES, INCLUDING ANY IMPLIED WARRANTY
OF MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE OF THE CONTENTS OF THIS MANUAL.
IN NO EVENT SHALL ABAQUS, INC. OR ITS THIRD-PARTY PROVIDERS BE LIABLE FOR ANY INDIRECT, INCIDENTAL, PUNITIVE,
SPECIAL, OR CONSEQUENTIAL DAMAGES (INCLUDING, WITHOUT LIMITATION, DAMAGES FOR LOSS OF BUSINESS PROFITS,
BUSINESS INTERRUPTION, OR LOSS OF BUSINESS INFORMATION) EVEN IF ABAQUS, INC. HAS BEEN ADVISED OF THE POSSIBILITY
OF SUCH DAMAGES.
The ABAQUS Software described in this manual is available only under license from ABAQUS, Inc. and may be used or reproduced only in accordance
with the terms of such license.
This manual and the software described in this manual are subject to change without prior notice.
No part of this manual may be reproduced or distributed in any form without prior written permission of ABAQUS, Inc.
© 2006 ABAQUS, Inc. All rights reserved.
Printed in the United States of America.
U.S. GOVERNMENT USERS: The ABAQUS Software and its documentation are “commercial items,” specifically “commercial computer software” and
“commercial computer software documentation” and, consistent with FAR 12.212 and DFARS 227.7202, as applicable, are provided with restricted rights
in accordance with license terms.
TRADEMARKS
The trademarks and service marks (“trademarks”) in this manual are the property of ABAQUS, Inc. or third parties. You are not permitted to use these
trademarks without the prior written consent of ABAQUS, Inc. or such third parties.
The following are trademarks or registered trademarks of ABAQUS, Inc. or its subsidiaries in the United States and/or other countries:
ABAQUS, ABAQUS/Standard, ABAQUS/Explicit, ABAQUS/CAE, ABAQUS/Viewer, ABAQUS/Aqua, ABAQUS/Design, ABAQUS/Foundation,
ABAQUS/AMS, ABAQUS for CATIA V5, VCCT for ABAQUS, DDAM for ABAQUS, Unified FEA, and the ABAQUS Logo. The 3DS logo and
SIMULIA are trademarks of Dassault Systèmes.
Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information
concerning trademarks, copyrights, and licenses, see the Legal Notices in the ABAQUS Version 6.6 Release Notes and the notices at
http://www.abaqus.com/products/products_legal.html.
Cover image: bolted joint in an aircraft brake courtesy Honeywell Landing Systems.
ABAQUS Version 6.1 Module: ID:
Printed on:
ABAQUS Offices and Representatives
ABAQUS, Inc. 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
ABAQUS Europe BV 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.com
Sales, Support, and Services
United States ABAQUS Central, West Lafayette, IN, Tel: +1 765 497 1373, support@AbaqusCentral.com
ABAQUS East, Warwick, RI, Tel: +1 401 739 3637, support@AbaqusEast.com
ABAQUS Erie, Beachwood, OH, Tel: +1 216 378 1070, support@AbaqusErie.com
ABAQUS Great Lakes, Plymouth, MI, Tel: +1 734 451 0217, support@AbaqusGreatLakes.com
ABAQUS South, Flower Mound, TX, Tel: +1 214 513 1600, support@AbaqusSouth.com
ABAQUS West, Fremont, CA, Tel: +1 510 794 5891, support@AbaqusWest.com
Argentina KB Engineering S. R. L., Buenos Aires, Tel: +54 11 4326 9176/7542, sanchezsarmiento@arnet.com.ar
Australia ABAQUS Australia Pty. Ltd., Richmond VIC, Tel: +61 3 9421 2900, info@abaqus.com.au
Austria ABAQUS Austria GmbH, Vienna, Tel: +43 1 929 16 25-0, support@abaqus.at
Benelux ABAQUS Benelux BV, Huizen, The Netherlands, Tel: +31 35 52 58 424, support@abaqus.nl
Brazil SMARTtech Mecânica Serviços e Sistemas Ltda, São Paulo, Tel: +55 11 3168 3388, smarttech@smarttech.com.br
China ABAQUS China, Beijing, P. R. China, Tel: +86 10 84580366, abaqus@abaqus.com.cn
Czech Republic Synerma s. r. o., Skuhrov, Tel: +420 603 145 769, abaqus@synerma.cz
France ABAQUS France SAS, Versailles, Tel: +33 01 39 24 15 40, support@abaqus.fr
Germany ABAQUS Deutschland GmbH, Aachen, Tel: +49 241 474010, info@abaqus.de
ABAQUS Deutschland GmbH, München, Tel: +49 89 5999 1768, info@abaqus.de
India ABAQUS Engineering India (P) Ltd., Alwarpet, Chennai, Tel: +91 44 55651590, abaqus@abaqus.co.in
Italy ABAQUS Italia s.r.l., Milano (MI), Tel: +39 02 39211211, info@abaqus.it
Japan ABAQUS, Inc., Tokyo, Tel: +81 3 5474 5817, tokyo@abaqus.jp
ABAQUS, Inc., Osaka, Tel: +81 6 4803 5020, osaka@abaqus.jp
Korea ABAQUS Korea, Inc., Seoul, Tel: +82 2 785 6707, info@abaqus.co.kr
Malaysia WorleyParsons Advanced Analysis, Kuala Lumpur, Tel: +60 3 2161 2266, abaqus.my@worleyparsons.com
New Zealand Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, abaqus-tech@matrix.co.nz
Poland BudSoft Sp. z o.o., Sw. Marcin, Tel: +48 61 8508 466, budsoft@budsoft.com.pl
Russia, Belarus & Ukraine TESIS Ltd., Moscow, Russia, Tel: +7 095 212-44-22, info@tesis.com.ru
Singapore WorleyParsons Advanced Analysis, Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com
South Africa Finite Element Analysis Services (Pty) Ltd., Mowbray, Tel: +27 21 448 7608, feas@feas.co.za
Spain Principia Ingenieros Consultores, S.A., Madrid, Tel: +34 91 209 1482, abaqus@principia.es
Sweden ABAQUS Scandinavia, Västerås, Tel: +46 21 150870, abaqus@abaqus.se
Taiwan APIC, Taipei, Tel: +886 02 25083066, apic@apic.com.tw
Thailand WorleyParsons Advanced Analysis, Bangkok, Tel: +66 2 689 3000, abaqus.th@worleyparsons.com
Turkey A-Ztech Ltd., Istanbul, TURKIYE, Tel: +90 216 361 8850, info@a-ztech.com.tr
United Kingdom ABAQUS UK Ltd., Warrington, Cheshire, Tel: +44 1 925 810166, hotline@abaqus.co.uk
Sales Only
United States ABAQUS East, Mid-Atlantic Office, Forest Hill, MD, Tel: +1 410 420 8587, support@AbaqusEast.com
ABAQUS South, Southeast Office, Acworth, GA, Tel: +1 770 795 0960, support@AbaqusSouth.com
ABAQUS West, Southern CA and AZ Office, Tustin, CA, Tel: +1 714 731 5895, Info@AbaqusWest.com
ABAQUS West, Rocky Mountains Office, Boulder, CO, Tel: +1 303 664 5444, Info@AbaqusWest.com
China ABAQUS China, Shanghai, P. R. China, Tel: +021 58309096/58203227 18, abaqus@abaqus.com.cn
Finland ABAQUS Finland Oy, Espoo, Tel: +358 9 2517 2973, abaqus@abaqus.fi
India ABAQUS Engineering India (P) Ltd., Pune, Tel: +91 20 30913739, abaqus@abaqus.co.in
United Kingdom ABAQUS UK Ltd., Sevenoaks, Kent, Tel: +44 1 732 834930, hotline@abaqus.co.uk
Complete contact information is available at http://www.abaqus.com.
ID:
Printed on: Mon February 27 -- 15:32:43 2006
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.
ABAQUS Online Support System
The ABAQUS Online Support System (AOSS) has a knowledge database of ABAQUS Answers. The
ABAQUS Answers are solutions to questions that we have had to answer or guidelines on how to use
ABAQUS. You can also submit new requests for support in the AOSS. All support incidents are tracked in
the AOSS. If you are contacting us by means outside the AOSS to discuss an existing support problem and
you know the incident number, please mention it so that we can consult the database to see what the latest
action has been.
To use the AOSS, you need to register with the system. Visit the My ABAQUS section of the ABAQUS
Home Page for instructions on how to register.
Many questions about ABAQUS can also be answered by visiting the ABAQUS Home Page on the
World Wide Web at
http://www.abaqus.com
Anonymous ftp site
ABAQUS maintains useful documents on an anonymous ftp account on the computer ftp.abaqus.com. Login
as user anonymous, and type your e-mail address as your password.
Training
All ABAQUS offices offer regularly scheduled public training classes. We also provide training seminars at
customer sites. All training classes and seminars include workshops to provide as much practical experience
with ABAQUS as possible. For a schedule and descriptions of available classes, see the ABAQUS Home
Page or call your local ABAQUS representative.
Feedback
We welcome any suggestions for improvements to ABAQUS software, the support program, or
documentation. We will ensure that any enhancement requests you make are considered for future releases.
If you wish to make a suggestion about the service or products provided by ABAQUS, refer to the ABAQUS
Home Page. Complaints should be addressed by contacting your local office or through the ABAQUS Home
Page.
ABAQUS Version 6.1 Module: ID:
Printed on:
CONTENTS
Contents — Volume I
A
*ACOUSTIC FLOW VELOCITY 1.1
*ACOUSTIC MEDIUM 1.2
*ACOUSTIC WAVE FORMULATION 1.3
*ADAPTIVE MESH 1.4
*ADAPTIVE MESH CONSTRAINT 1.5
*ADAPTIVE MESH CONTROLS 1.6
*AMPLITUDE 1.7
*ANNEAL 1.8
*ANNEAL TEMPERATURE 1.9
*AQUA 1.10
*ASSEMBLY 1.11
*ASYMMETRIC-AXISYMMETRIC 1.12
*AXIAL 1.13
B
*BASE MOTION 2.1
*BASELINE CORRECTION 2.2
*BEAM ADDED INERTIA 2.3
*BEAM FLUID INERTIA 2.4
*BEAM GENERAL SECTION 2.5
*BEAM SECTION 2.6
*BEAM SECTION GENERATE 2.7
*BIAXIAL TEST DATA 2.8
*BLOCKAGE 2.9
*BOND 2.10
*BOUNDARY 2.11
*BRITTLE CRACKING 2.12
*BRITTLE FAILURE 2.13
*BRITTLE SHEAR 2.14
*BUCKLE 2.15
*BUCKLING ENVELOPE 2.16
*BUCKLING LENGTH 2.17
*BUCKLING REDUCTION FACTORS 2.18
*BULK VISCOSITY 2.19
v
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
C
*C ADDED MASS 3.1
*CAPACITY 3.2
*CAP CREEP 3.3
*CAP HARDENING 3.4
*CAP PLASTICITY 3.5
*CAST IRON COMPRESSION HARDENING 3.6
*CAST IRON PLASTICITY 3.7
*CAST IRON TENSION HARDENING 3.8
*CAVITY DEFINITION 3.9
*CECHARGE 3.10
*CECURRENT 3.11
*CENTROID 3.12
*CFILM 3.13
*CFLOW 3.14
*CFLUX 3.15
*CHANGE FRICTION 3.16
*CLAY HARDENING 3.17
*CLAY PLASTICITY 3.18
*CLEARANCE 3.19
*CLOAD 3.20
*COHESIVE SECTION 3.21
*COMBINED TEST DATA 3.22
*COMPLEX FREQUENCY 3.23
*CONCRETE 3.24
*CONCRETE COMPRESSION DAMAGE 3.25
*CONCRETE COMPRESSION HARDENING 3.26
*CONCRETE DAMAGED PLASTICITY 3.27
*CONCRETE TENSION DAMAGE 3.28
*CONCRETE TENSION STIFFENING 3.29
*CONDUCTIVITY 3.30
*CONNECTOR BEHAVIOR 3.31
*CONNECTOR CONSTITUTIVE REFERENCE 3.32
*CONNECTOR DAMAGE EVOLUTION 3.33
*CONNECTOR DAMAGE INITIATION 3.34
*CONNECTOR DAMPING 3.35
*CONNECTOR DERIVED COMPONENT 3.36
*CONNECTOR ELASTICITY 3.37
*CONNECTOR FAILURE 3.38
*CONNECTOR FRICTION 3.39
*CONNECTOR HARDENING 3.40
vi
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
*CONNECTOR LOAD 3.41
*CONNECTOR LOCK 3.42
*CONNECTOR MOTION 3.43
*CONNECTOR PLASTICITY 3.44
*CONNECTOR POTENTIAL 3.45
*CONNECTOR SECTION 3.46
*CONNECTOR STOP 3.47
*CONSTRAINT CONTROLS 3.48
*CONTACT 3.49
*CONTACT CLEARANCE 3.50
*CONTACT CLEARANCE ASSIGNMENT 3.51
*CONTACT CONTROLS 3.52
*CONTACT CONTROLS ASSIGNMENT 3.53
*CONTACT DAMPING 3.54
*CONTACT EXCLUSIONS 3.55
*CONTACT FILE 3.56
*CONTACT FORMULATION 3.57
*CONTACT INCLUSIONS 3.58
*CONTACT INTERFERENCE 3.59
*CONTACT OUTPUT 3.60
*CONTACT PAIR 3.61
*CONTACT PRINT 3.62
*CONTACT PROPERTY ASSIGNMENT 3.63
*CONTACT RESPONSE 3.64
*CONTOUR INTEGRAL 3.65
*CONTROLS 3.66
*CORRELATION 3.67
*CO-SIMULATION 3.68
*CO-SIMULATION REGION 3.69
*COUPLED TEMPERATURE-DISPLACEMENT 3.70
*COUPLED THERMAL-ELECTRICAL 3.71
*COUPLING 3.72
*CRADIATE 3.73
*CREEP 3.74
*CREEP STRAIN RATE CONTROL 3.75
*CRUSHABLE FOAM 3.76
*CRUSHABLE FOAM HARDENING 3.77
*CYCLED PLASTIC 3.78
*CYCLIC 3.79
*CYCLIC HARDENING 3.80
*CYCLIC SYMMETRY MODEL 3.81
vii
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
D
*D ADDED MASS 4.1
*DAMAGE EVOLUTION 4.2
*DAMAGE INITIATION 4.3
*DAMAGE STABILIZATION 4.4
*DAMPING 4.5
*DASHPOT 4.6
*DEBOND 4.7
*DECHARGE 4.8
*DECURRENT 4.9
*DEFORMATION PLASTICITY 4.10
*DENSITY 4.11
*DEPVAR 4.12
*DESIGN GRADIENT 4.13
*DESIGN PARAMETER 4.14
*DESIGN RESPONSE 4.15
*DETONATION POINT 4.16
*DFLOW 4.17
*DFLUX 4.18
*DIAGNOSTICS 4.19
*DIELECTRIC 4.20
*DIFFUSIVITY 4.21
*DIRECT CYCLIC 4.22
*DISPLAY BODY 4.23
*DISTRIBUTION 4.24
*DISTRIBUTING 4.25
*DISTRIBUTING COUPLING 4.26
*DLOAD 4.27
*DRAG CHAIN 4.28
*DRUCKER PRAGER 4.29
*DRUCKER PRAGER CREEP 4.30
*DRUCKER PRAGER HARDENING 4.31
*DSA CONTROLS 4.32
*DSECHARGE 4.33
*DSECURRENT 4.34
*DSFLOW 4.35
*DSFLUX 4.36
*DSLOAD 4.37
*DYNAMIC 4.38
*DYNAMIC TEMPERATURE-DISPLACEMENT 4.39
viii
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
E
*EL FILE 5.1
*EL PRINT 5.2
*ELASTIC 5.3
*ELCOPY 5.4
*ELECTRICAL CONDUCTIVITY 5.5
*ELEMENT 5.6
*ELEMENT MATRIX OUTPUT 5.7
*ELEMENT OUTPUT 5.8
*ELEMENT PROPERTIES 5.9
*ELEMENT RESPONSE 5.10
*ELGEN 5.11
*ELSET 5.12
*EMBEDDED ELEMENT 5.13
*EMISSIVITY 5.14
*END ASSEMBLY 5.15
*END INSTANCE 5.16
*END LOAD CASE 5.17
*END PART 5.18
*END STEP 5.19
*ENERGY FILE 5.20
*ENERGY OUTPUT 5.21
*ENERGY PRINT 5.22
*EOS 5.23
*EOS COMPACTION 5.24
*EOS SHEAR 5.25
*EPJOINT 5.26
*EQUATION 5.27
*EXPANSION 5.28
*EXTREME ELEMENT VALUE 5.29
*EXTREME NODE VALUE 5.30
*EXTREME VALUE 5.31
F
*FAIL STRAIN 6.1
*FAIL STRESS 6.2
*FAILURE RATIOS 6.3
*FASTENER 6.4
*FASTENER PROPERTY 6.5
*FIELD 6.6
*FILE FORMAT 6.7
ix
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
*FILE OUTPUT 6.8
*FILM 6.9
*FILM PROPERTY 6.10
*FILTER 6.11
*FIXED MASS SCALING 6.12
*FLOW 6.13
*FLUID BEHAVIOR 6.14
*FLUID BULK MODULUS 6.15
*FLUID CAVITY 6.16
*FLUID DENSITY 6.17
*FLUID EXCHANGE 6.18
*FLUID EXCHANGE ACTIVATION 6.19
*FLUID EXCHANGE PROPERTY 6.20
*FLUID EXPANSION 6.21
*FLUID FLUX 6.22
*FLUID INFLATOR 6.23
*FLUID INFLATOR ACTIVATION 6.24
*FLUID INFLATOR MIXTURE 6.25
*FLUID INFLATOR PROPERTY 6.26
*FLUID LEAKOFF 6.27
*FLUID LINK 6.28
*FLUID PROPERTY 6.29
*FOUNDATION 6.30
*FRACTURE CRITERION 6.31
*FRAME SECTION 6.32
*FREQUENCY 6.33
*FRICTION 6.34
G
*GAP 7.1
*GAP CONDUCTANCE 7.2
*GAP ELECTRICAL CONDUCTANCE 7.3
*GAP FLOW 7.4
*GAP HEAT GENERATION 7.5
*GAP RADIATION 7.6
*GASKET BEHAVIOR 7.7
*GASKET CONTACT AREA 7.8
*GASKET ELASTICITY 7.9
*GASKET SECTION 7.10
*GASKET THICKNESS BEHAVIOR 7.11
*GEL 7.12
*GEOSTATIC 7.13
x
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
H
*HEADING 8.1
*HEAT GENERATION 8.2
*HEAT TRANSFER 8.3
*HEATCAP 8.4
*HOURGLASS STIFFNESS 8.5
*HYPERELASTIC 8.6
*HYPERFOAM 8.7
*HYPOELASTIC 8.8
*HYSTERESIS 8.9
xi
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
Contents — Volume II
I
*IMPEDANCE 9.1
*IMPEDANCE PROPERTY 9.2
*IMPERFECTION 9.3
*IMPORT 9.4
*IMPORT CONTROLS 9.5
*IMPORT ELSET 9.6
*IMPORT NSET 9.7
*INCIDENT WAVE 9.8
*INCIDENT WAVE FLUID PROPERTY 9.9
*INCIDENT WAVE INTERACTION 9.10
*INCIDENT WAVE INTERACTION PROPERTY 9.11
*INCIDENT WAVE PROPERTY 9.12
*INCIDENT WAVE REFLECTION 9.13
*INCLUDE 9.14
*INCREMENTATION OUTPUT 9.15
*INELASTIC HEAT FRACTION 9.16
*INERTIA RELIEF 9.17
*INITIAL CONDITIONS 9.18
*INSTANCE 9.19
*INTEGRATED OUTPUT 9.20
*INTEGRATED OUTPUT SECTION 9.21
*INTERACTION OUTPUT 9.22
*INTERACTION PRINT 9.23
*INTERFACE 9.24
*ITS 9.25
J
*JOINT 10.1
*JOINT ELASTICITY 10.2
*JOINT PLASTICITY 10.3
*JOINTED MATERIAL 10.4
*JOULE HEAT FRACTION 10.5
K
*KAPPA 11.1
*KINEMATIC 11.2
*KINEMATIC COUPLING 11.3
xii
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
L
*LATENT HEAT 12.1
*LOAD CASE 12.2
M
*MAP SOLUTION 13.1
*MASS 13.2
*MASS DIFFUSION 13.3
*MASS FLOW RATE 13.4
*MATERIAL 13.5
*MATRIX 13.6
*MATRIX ASSEMBLE 13.7
*MATRIX INPUT 13.8
*MEMBRANE SECTION 13.9
*MODAL DAMPING 13.10
*MODAL DYNAMIC 13.11
*MODAL FILE 13.12
*MODAL OUTPUT 13.13
*MODAL PRINT 13.14
*MODEL CHANGE 13.15
*MOHR COULOMB 13.16
*MOHR COULOMB HARDENING 13.17
*MOISTURE SWELLING 13.18
*MOLECULAR WEIGHT 13.19
*MONITOR 13.20
*MOTION 13.21
*MPC 13.22
*MULLINS EFFECT 13.23
*M1 13.24
*M2 13.25
N
*NCOPY 14.1
*NFILL 14.2
*NGEN 14.3
*NMAP 14.4
*NO COMPRESSION 14.5
*NO TENSION 14.6
*NODAL THICKNESS 14.7
*NODE 14.8
xiii
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
*NODE FILE 14.9
*NODE OUTPUT 14.10
*NODE PRINT 14.11
*NODE RESPONSE 14.12
*NONSTRUCTURAL MASS 14.13
*NORMAL 14.14
*NSET 14.15
O
*ORIENTATION 15.1
*ORNL 15.2
*OUTPUT 15.3
P, Q
*PARAMETER 16.1
*PARAMETER DEPENDENCE 16.2
*PARAMETER SHAPE VARIATION 16.3
*PART 16.4
*PERIODIC 16.5
*PERMEABILITY 16.6
*PHYSICAL CONSTANTS 16.7
*PIEZOELECTRIC 16.8
*PIPE-SOIL INTERACTION 16.9
*PIPE-SOIL STIFFNESS 16.10
*PLANAR TEST DATA 16.11
*PLASTIC 16.12
*PLASTIC AXIAL 16.13
*PLASTIC M1 16.14
*PLASTIC M2 16.15
*PLASTIC TORQUE 16.16
*POROUS BULK MODULI 16.17
*POROUS ELASTIC 16.18
*POROUS FAILURE CRITERIA 16.19
*POROUS METAL PLASTICITY 16.20
*POST OUTPUT 16.21
*POTENTIAL 16.22
*PREPRINT 16.23
*PRESSURE PENETRATION 16.24
*PRESSURE STRESS 16.25
*PRESTRESS HOLD 16.26
*PRE-TENSION SECTION 16.27
xiv
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
*PRINT 16.28
*PSD-DEFINITION 16.29
R
*RADIATE 17.1
*RADIATION FILE 17.2
*RADIATION OUTPUT 17.3
*RADIATION PRINT 17.4
*RADIATION SYMMETRY 17.5
*RADIATION VIEWFACTOR 17.6
*RANDOM RESPONSE 17.7
*RATE DEPENDENT 17.8
*RATIOS 17.9
*REBAR 17.10
*REBAR LAYER 17.11
*REFLECTION 17.12
*RELEASE 17.13
*RESPONSE SPECTRUM 17.14
*RESTART 17.15
*RETAINED EIGENMODES 17.16
*RETAINED NODAL DOFS 17.17
*RIGID BODY 17.18
*RIGID SURFACE 17.19
*ROTARY INERTIA 17.20
S
*SECTION CONTROLS 18.1
*SECTION FILE 18.2
*SECTION ORIGIN 18.3
*SECTION POINTS 18.4
*SECTION PRINT 18.5
*SELECT CYCLIC SYMMETRY MODES 18.6
*SELECT EIGENMODES 18.7
*SFILM 18.8
*SFLOW 18.9
*SHEAR CENTER 18.10
*SHEAR FAILURE 18.11
*SHEAR RETENTION 18.12
*SHEAR TEST DATA 18.13
*SHELL GENERAL SECTION 18.14
*SHELL SECTION 18.15
*SHELL TO SOLID COUPLING 18.16
xv
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
*SIMPEDANCE 18.17
*SIMPLE SHEAR TEST DATA 18.18
*SLIDE LINE 18.19
*SLOAD 18.20
*SOILS 18.21
*SOLID SECTION 18.22
*SOLUBILITY 18.23
*SOLUTION TECHNIQUE 18.24
*SOLVER CONTROLS 18.25
*SORPTION 18.26
*SPECIFIC HEAT 18.27
*SPECTRUM 18.28
*SPRING 18.29
*SRADIATE 18.30
*STATIC 18.31
*STEADY STATE CRITERIA 18.32
*STEADY STATE DETECTION 18.33
*STEADY STATE DYNAMICS 18.34
*STEADY STATE TRANSPORT 18.35
*STEP 18.36
*SUBMODEL 18.37
*SUBSTRUCTURE COPY 18.38
*SUBSTRUCTURE DELETE 18.39
*SUBSTRUCTURE DIRECTORY 18.40
*SUBSTRUCTURE GENERATE 18.41
*SUBSTRUCTURE LOAD CASE 18.42
*SUBSTRUCTURE MATRIX OUTPUT 18.43
*SUBSTRUCTURE PATH 18.44
*SUBSTRUCTURE PROPERTY 18.45
*SURFACE 18.46
*SURFACE BEHAVIOR 18.47
*SURFACE FLAW 18.48
*SURFACE INTERACTION 18.49
*SURFACE PROPERTY 18.50
*SURFACE PROPERTY ASSIGNMENT 18.51
*SURFACE SECTION 18.52
*SWELLING 18.53
*SYMMETRIC MODEL GENERATION 18.54
*SYMMETRIC RESULTS TRANSFER 18.55
*SYSTEM 18.56
xvi
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
CONTENTS
T
*TEMPERATURE 19.1
*TENSILE FAILURE 19.2
*TENSION STIFFENING 19.3
*THERMAL EXPANSION 19.4
*TIE 19.5
*TIME POINTS 19.6
*TORQUE 19.7
*TORQUE PRINT 19.8
*TRACER PARTICLE 19.9
*TRANSFORM 19.10
*TRANSPORT VELOCITY 19.11
*TRANSVERSE SHEAR STIFFNESS 19.12
*TRIAXIAL TEST DATA 19.13
*TRS 19.14
U
*UEL PROPERTY 20.1
*UNDEX CHARGE PROPERTY 20.2
*UNIAXIAL TEST DATA 20.3
*USER DEFINED FIELD 20.4
*USER ELEMENT 20.5
*USER MATERIAL 20.6
*USER OUTPUT VARIABLES 20.7
V
*VARIABLE MASS SCALING 21.1
*VIEWFACTOR OUTPUT 21.2
*VISCO 21.3
*VISCOELASTIC 21.4
*VISCOUS 21.5
*VOID NUCLEATION 21.6
*VOLUMETRIC TEST DATA 21.7
W, X, Y, Z
*WAV E 22.1
*WIND 22.2
xvii
ABAQUS ID:key-toc
Printed on: Mon February 27 -- 17:38:39 2006
I
9. I
ABAQUS Version 6.1 Module: ID:
Printed on:
*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
Users Manual
“Acoustic loads,” Section 27.4.5 of the ABAQUS Analysis Users Manual
*IMPEDANCE PROPERTY
*SIMPEDANCE
Required, mutually exclusive parameters:
PROPERTY
Set this parameter equal to the name of the *IMPEDANCE PROPERTY option defining the table
of impedance values to be used.
NONREFLECTING
Set NONREFLECTING=PLANAR (default) to specify the impedance corresponding to that of a
normal incidence plane wave.
Set NONREFLECTING=IMPROVED to specify the impedance corresponding to that of
a plane wave at an arbitrary angle of incidence. This parameter can be used only for transient
dynamics.
Set NONREFLECTING=CIRCULAR to specify a radiation condition appropriate for a
circular boundary in two dimensions or a right circular cylinder in three dimensions.
Set NONREFLECTING=SPHERICAL to specify a radiation condition appropriate for a
spherical boundary.
Set NONREFLECTING=ELLIPTICAL to specify a radiation condition appropriate for an
elliptical boundary in two dimensions or a right elliptical cylinder in three dimensions.
Set NONREFLECTING=PROLATE SPHEROIDAL to specify a radiation condition
appropriate for a prolate spheroidal boundary.
9.1–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. Surface impedance type label, In, for impedance on face n.
Data line to define an absorbing boundary impedance for NONREFLECTING=CIRCULAR or
NONREFLECTING=SPHERICAL:
First (and only) line:
1. Element number or element set label.
2. Surface impedance type label, In, for impedance on face n.
3. , the radius of the circle or sphere defining the absorbing boundary surface.
Data line to define an absorbing boundary impedance for NONREFLECTING=ELLIPTICAL or
NONREFLECTING=PROLATE SPHEROIDAL:
First (and only) line:
1. Element number or element set label.
2. Surface impedance type label, In, for impedance on face n.
3. The semimajor axis, a, of the ellipse or prolate spheroid defining the surface. ais 1/2 of the
maximum distance between two points on the ellipse or spheroid, analogous to the radius of a
circle or sphere.
4. The eccentricity, , of the ellipse or prolate spheroid. The eccentricity is the square root of
one minus the square of the ratio of the semiminor axis, b, to the semimajor axis, a:
.
5. Global X-coordinate of the center of the ellipse or prolate spheroid defining the radiating
surface.
6. Global Y-coordinate of the center of the ellipse or prolate spheroid defining the radiating
surface.
7. Global Z-coordinate of the center of the ellipse or prolate spheroid defining the radiating
surface.
9.1–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
9.1–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*IMPEDANCE PROPERTY
9.2 *IMPEDANCE PROPERTY: Define the impedance parameters for an acoustic medium
boundary.
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 27.4.5 of the ABAQUS Analysis Users Manual
*IMPEDANCE
*SIMPEDANCE
Required parameter:
NAME
Set this parameter equal to a label that will be used to refer to the impedance property on the
*IMPEDANCE or *SIMPEDANCE option.
Optional parameters:
DATA
Set DATA=ADMITTANCE (default) to specify an impedance using a table of admittance values.
Set DATA=IMPEDANCE to specify an impedance using a table of real and imaginary parts
of the impedance.
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 Users Manual, for the
syntax of such file names. If this parameter is omitted, it is assumed that the data follow the keyword
line.
9.2–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. This quantity is the real part of the complex admittance. (Units of F−1 L3T−1 .)
3. Frequency. (Cycles/time.) Frequency dependence is active only during frequency domain
analysis in ABAQUS/Standard.
Repeat this data line as often as necessary in ABAQUS/Standard to describe the variation of the
coefficients with frequency. Only the first line entered will be used in direct-integration procedures.
Data lines to define an impedance using DATA=IMPEDANCE:
First line:
1. , the real part of the surface impedance. (Units of F L−3 T.)
2. , the imaginary part of the surface impedance. (Units of F L−3 T.)
3. Frequency. (Cycles/time.) Frequency dependence is active only during frequency domain
analysis in ABAQUS/Standard.
Repeat this data line as often as necessary in ABAQUS/Standard to describe the variation of the
coefficients with frequency. Only the first line entered will be used in direct-integration procedures.
9.2–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users
Manual
“Unstable collapse and postbuckling analysis,” Section 6.2.4 of the ABAQUS Analysis Users Manual
“Eigenvalue buckling prediction,” Section 6.2.3 of the ABAQUS Analysis Users Manual
Optional parameters (mutually exclusive-if neither parameter is specified, ABAQUS assumes
that the imperfection data will be entered directly on the data lines):
FILE
Set this parameter equal to the name of the results file from a previous ABAQUS/Standard analysis
containing either the mode shapes from a *BUCKLE or *FREQUENCY analysis or the nodal
displacements from a *STATIC analysis.
INPUT
Set this parameter equal to the name of the alternate input file containing the imperfection data, in
general, as the node number and imperfection values in the global coordinate system. See “Input
syntax rules,” Section 1.2.1 of the ABAQUS Analysis Users Manual, for the syntax of such file
names.
Required parameter if the FILE parameter is used:
STEP
Set this parameter equal to the step number (in the analysis whose results file is being used as input
to this option) from which the modal or displacement data are to be read.
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.
9.3–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. Set SYSTEM=S to specify the imperfection as perturbation values of spherical
coordinates. See Figure 9.3–1.
The SYSTEM parameter is entirely local to this option and should not be confused with the
*SYSTEM option. As the data lines are read, the imperfection values specified are transformed
to the global rectangular Cartesian coordinate system. This transformation requires that the object
be centered about the origin of the global coordinate system; i.e., the *SYSTEM option should
be off when specifying imperfections as perturbation values using either cylindrical or spherical
coordinates.
Data lines to define the imperfection as a linear superposition of mode shapes from the results
file:
First line:
1. Mode number.
2. Scaling factor for this mode.
Repeat this data line as often as necessary to define the imperfection as a linear combination of mode
shapes.
Data line to define the imperfection based on the solution of a static analysis from the results file:
First (and only) line:
1. Set to 1.
2. Scaling factor.
Data lines to define the imperfection if the FILE and INPUT parameters are omitted:
First line:
1. Node number.
2. Component of imperfection in the first coordinate direction.
3. Component of imperfection in the second coordinate direction.
4. Component of imperfection in the third coordinate direction.
Repeat this data line as often as necessary to define the imperfection.
9.3–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*IMPERFECTION
(X,Y,Z)
Rectangular Cartesian
(SYSTEM=R)
(default)
R
θ
Cylindrical
(SYSTEM=C)
(θ and φ are given in degrees)
(R,θ,φ)
θ
φ
Spherical
(SYSTEM=S)
Z
Y
X
YY
ZZ
X
X
(R,θ,Z)
Figure 9.3–1 Coordinate systems.
9.3–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. The *IMPORToptionmustbeusedin
conjunction with the *INSTANCE option when importing a part instance from a previous analysis.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Part instance
References:
“Transferring results between ABAQUS analyses: overview,” Section 9.2.1 of the ABAQUS Analysis
Users Manual
*INSTANCE
Required parameter:
UPDATE
Set UPDATE=NO to continue the analysis without resetting the reference configuration.
Set UPDATE=YES to continue the analysis by resetting the reference configuration to be the
imported configuration. In this case displacement and strain values are calculated from the new
reference configuration.
Optional, mutually exclusive parameters:
INCREMENT
When importing an analysis from ABAQUS/Standard into ABAQUS/Explicit or from one
ABAQUS/Standard analysis into another ABAQUS/Standard analysis, set this parameter equal to
the increment of the specified step on the ABAQUS/Standard restart file from which the analysis
is to be imported. If this parameter is omitted, the analysis is imported from the last available
increment of the specified step.
INTERVAL
This parameter applies only to ABAQUS/Standard analyses.
When importing an analysis from ABAQUS/Explicit into ABAQUS/Standard, set this
parameter equal to the interval of the specified step on the ABAQUS/Explicit state file from which
9.4–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
When importing an analysis from ABAQUS/Standard into ABAQUS/Explicit or from one
ABAQUS/Standard analysis into another ABAQUS/Standard analysis, set this parameter equal to
the iteration number of the specified step on the ABAQUS/Standard restart file from which the
analysis is to be imported. Since restart information can be written only at the end of an iteration in
a direct cyclic analysis, the INCREMENT parameter is irrelevant and is ignored if the ITERATION
parameter is specified. If this parameter is omitted, the analysis is imported from the last available
iteration of the specified step.
Optional parameters:
STATE
Set STATE=YES (default) to import the current material state of the elements at the specified step
and the specified interval, increment, or iteration.
Set STATE=NO if no material state is to be imported. In this case the elements will start with
no initial state or with the state as defined by the *INITIAL CONDITIONS option.
STEP
Set this parameter equal to the step on the ABAQUS/Explicit state file or on the ABAQUS/Standard
restart file from which the analysis is being imported. If this parameter is omitted, the analysis is
imported from the last available step on the state file or the restart file at the specified increment,
interval, or iteration.
Data lines to specify element sets to be imported:
First line:
1. List of element sets that are to be imported. Specify only element set names that are used
to define the section properties in the previous ABAQUS/Explicit or ABAQUS/Standard
analysis.
Repeat this data line as often as necessary to define the element sets to be imported. Up to 16 element
sets can be listed per data line.
There are no data lines for importing a part instance.
9.4–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Model
References:
“Transferring results between ABAQUS/Explicit and ABAQUS/Standard,” Section 9.2.2 of the
ABAQUS Analysis Users Manual
*IMPORT
Required parameter:
NORMAL TOL
Set this parameter equal to the tolerance required for the error checking on shell normals. The
default value is 0.1.
There are no data lines associated with this option.
9.5–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Model
References:
“Transferring results between ABAQUS/Explicit and ABAQUS/Standard,” Section 9.2.2 of the
ABAQUS Analysis Users Manual
*IMPORT
There are no parameters associated with this option.
Data lines to specify element set definitions to be imported:
First line:
1. List of element set names for which the element set definitions are to be imported.
Repeat this data line as often as necessary to specify the element set definitions to be imported. Up to
16 element sets can be listed per line.
9.6–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Model
References:
“Transferring results between ABAQUS/Explicit and ABAQUS/Standard,” Section 9.2.2 of the
ABAQUS Analysis Users Manual
*IMPORT
There are no parameters associated with this option.
Data lines to specify node set definitions to be imported:
First line:
1. List of node set names for which the node set definitions are to be imported.
Repeat this data line as often as necessary to specify the node set definitions to be imported. Up to 16
node sets can be listed per line.
9.7–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*INCIDENT WAVE
9.8 *INCIDENT WAVE: Define incident wave loading for a blast or scattering load on a
boundary.
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.
The *INCIDENT WAVE PROPERTY option must be used in conjunction with the *INCIDENT WAVE
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.
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
Users Manual
“Acoustic loads,” Section 27.4.5 of the ABAQUS Analysis Users Manual
*INCIDENT WAVE PROPERTY
*INCIDENT WAVE REFLECTION
Required parameter:
PROPERTY
Set this parameter equal to the name of the *INCIDENT WAVE PROPERTY option defining the
incident wave field.
Required, mutually exclusive parameters:
ACCELERATION AMPLITUDE
Set this parameter equal to the name of the amplitude curve defining the fluid particle acceleration
time history at the standoff point (“Amplitude curves,” Section 27.1.2 of the ABAQUS Analysis
Users Manual). This amplitude curve will be used to compute the fluid traction only: a solid surface
requiring a pressure load cannot be specified on the data line of an *INCIDENT WAVE option if
the ACCELERATION AMPLITUDE parameter is used.
This parameter is valid only for planar incident waves using the *INCIDENT WAVE
PROPERTY, TYPE=PLANE option. Reflected loads, using the *INCIDENT WAVE
REFLECTION option, are not permitted in this case.
9.8–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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
Users 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.
Repeat this data line as often as necessary to describe the loading on the surfaces due to the incident
wave. In problems involving fluid-solid boundaries, both the fluid surface and the solid surface comprising
the boundary must have an incident wave load specified, using the appropriate load type.
9.8–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*INCIDENT WAVE FLUID PROPERTY
9.9 *INCIDENT WAVE FLUID PROPERTY: Define the fluid properties associated with an
incident wave.
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. The alternative interface will be removed in a subsequent release.
The *INCIDENT WAVE FLUID PROPERTY must be used in conjunction with the *INCIDENT WAVE
PROPERTY option.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Model
References:
“Acoustic medium,” Section 20.3.1 of the ABAQUS Analysis Users Manual
“Acoustic loads,” Section 27.4.5 of the ABAQUS Analysis Users Manual
*INCIDENT WAVE PROPERTY
There are no parameters associated with this option.
Data line to define incident wave fluid properties:
First (and only) line:
1. , the fluid bulk modulus.
2. , the fluid mass density.
9.9–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*INCIDENT WAVE INTERACTION
9.10 *INCIDENT WAVE INTERACTION: Define incident wave loading for a blast or
scattering load on a surface.
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.
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
Users Manual
“Acoustic loads,” Section 27.4.5 of the ABAQUS Analysis Users Manual
*INCIDENT WAVE INTERACTION PROPERTY
*INCIDENT WAVE REFLECTION
Required parameter:
PROPERTY
Set this parameter equal to the name of the *INCIDENT WAVE INTERACTION PROPERTY
option defining the incident wave field.
Required, mutually exclusive parameters:
ACCELERATION AMPLITUDE
Set this parameter equal to the name of the amplitude curve defining the fluid particle acceleration
time history at the standoff point (“Amplitude curves,” Section 27.1.2 of the ABAQUS Analysis
Users Manual). This amplitude curve will be used to compute the fluid traction only: a solid
surface requiring a pressure load cannot be specified on the data line of an *INCIDENT WAVE
INTERACTION option if the ACCELERATION AMPLITUDE parameter is used.
This parameter is valid only for planar incident waves using the *INCIDENT WAVE
INTERACTION PROPERTY, TYPE=PLANE option. Reflected loads, using the *INCIDENT
WAVE REFLECTION option, are not permitted in this case.
9.10–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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
Users 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. This parameter is valid only for spherical incident waves using the
*INCIDENT WAVE INTERACTION PROPERTY, TYPE=SPHERE option.
Data line to define an incident wave:
First (and only) line:
1. Surface name.
2. The node number or set name of the source node.
3. The node number or set name of the standoff node.
4. Reference magnitude.
9.10–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*INCIDENT WAVE INTERACTION PROPERTY
9.11 *INCIDENT WAVE INTERACTION PROPERTY: Define the geometric data and fluid
properties describing an incident wave.
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 27.4.5 of the ABAQUS Analysis Users Manual
*INCIDENT WAVE INTERACTION
*UNDEX CHARGE PROPERTY
Required parameter:
NAME
Set this parameter equal to a label that will be used to refer to the incident wave interaction property
in the *INCIDENT WAVE INTERACTION option.
Optional parameter:
TYPE
Set TYPE=PLANE (default) to specify a planar incident wave.
Set TYPE=SPHERE to specify a spherical incident wave.
Data line to define an incident wave interaction property:
First (and only) line:
1. , the speed of sound in the fluid, defining the rate of propagation of the wave.
2. , the fluid mass density.
9.11–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*INCIDENT WAVE PROPERTY
9.12 *INCIDENT WAVE PROPERTY: Define the geometric data describing an incident
wave.
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.
Each *INCIDENT WAVE option must refer to an *INCIDENT WAVE PROPERTY definition. The
*INCIDENT WAVE PROPERTY option must be followed by the *INCIDENT WAVE FLUID PROPERTY
option, which defines the fluid properties used in the incident wave loading.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Model
References:
“Acoustic loads,” Section 27.4.5 of the ABAQUS Analysis Users Manual
*INCIDENT WAVE
*INCIDENT WAVE FLUID PROPERTY
Required parameter:
NAME
Set this parameter equal to a label that will be used to refer to the incident wave property in the
*INCIDENT WAVE option.
Optional parameter:
TYPE
Set TYPE=PLANE (default) to specify a planar incident wave.
Set TYPE=SPHERE to specify a spherical incident wave.
Data lines to define an incident wave property:
First line:
1. X-coordinate of , the position of the incident wave standoff point.
2. Y-coordinate of , the position of the incident wave standoff point.
3. Z-coordinate of , the position of the incident wave standoff point.
9.12–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. Alternatively, specify the
name of an *AMPLITUDE definition describing the time history of this coordinate.
3. Z-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.
If TYPE=PLANE, the vector from to defines the direction of the incoming wave; the distance
between the two points is unimportant. For incident wave loads using bubble amplitudes, the source
positions defined by the user with the *INCIDENT WAVE PROPERTY option are interpreted as
the initial positions of the source.
9.12–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*INCIDENT WAVE REFLECTION
9.13 *INCIDENT WAVE REFLECTION: Define the reflection load on a surface caused by
incident wave fields.
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.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: History data
Level: Step
References:
“Acoustic loads,” Section 27.4.5 of the ABAQUS Analysis Users Manual
*INCIDENT WAVE INTERACTION
*INCIDENT WAVE
There are no parameters associated with this option.
Data lines to define an incident wave reflection:
First line:
1. Distance from the source point to the first reflecting plane.
2. X-direction cosine of the normal to the reflecting plane, pointing away from the source point.
3. Y-direction cosine of the normal to the reflecting plane, pointing away from the source point.
4. Z-direction cosine of the normal to the reflecting plane, pointing away from the source point.
5. Reflection coefficient.
Repeat this data line as often as necessary to describe the planes that reflect the incident wave.
9.13–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. See “Input syntax rules,”
Section 1.2.1 of the ABAQUS Analysis Users Manual, for the syntax of such file names.
Optional parameter:
PASSW O RD
When the external file is encrypted, set this parameter equal to the file’s password. Passwords are
case-sensitive.
There are no data lines associated with this option.
9.14–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*INCREMENTATION OUTPUT
9.15 *INCREMENTATION OUTPUT: Define output database requests for time
incrementation data.
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 4.1.3 of the ABAQUS Analysis Users Manual
*OUTPUT
Optional parameter:
VA R I A B L E
Set VARIABLE=ALL to indicate that all incrementation variables applicable to this procedure type
should be written to the output database.
Set VARIABLE=PRESELECT to indicate that the default incrementation 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 incrementation variables requested for output must be specified
onthedatalines.
Data lines to request incrementation output:
First line:
1. Give the identifying keys for the 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 Users Manual.
Repeat this data line as often as necessary to define the time incrementation variables to be written to
the output database.
9.15–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. It is also relevant when a fully coupled thermal-stress analysis is conducted using the
*COUPLED TEMPERATURE-DISPLACEMENT or *DYNAMIC TEMPERATURE-DISPLACEMENT
options.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Model
References:
“Adiabatic analysis,” Section 6.5.5 of the ABAQUS Analysis Users Manual
“Fully coupled thermal-stress analysis,” Section 6.5.4 of the ABAQUS Analysis Users Manual
There are no parameters associated with this option.
Data line to define the inelastic heat fraction:
First (and only) line:
1. Fraction of inelastic dissipation rate that appears as a heat flux per unit volume. The fraction
may include a unit conversion factor if required. The default value is 0.9.
9.16–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 27.4.3 of the ABAQUS Analysis Users Manual
Optional, mutually exclusive parameters:
FIXED
Include this parameter to indicate that the inertia relief load from a previous step should remain
fixed at its value from the beginning of the current step.
ORIENTATION
Set this parameter equal to the name given to the *ORIENTATION definition (“Orientations,”
Section 2.2.5 of the ABAQUS Analysis Users Manual) that specifies the orientation of the local
system for rigid body degrees of freedom.
REMOVE
Include this parameter to indicate that the inertia relief load from a previous step should be removed
in the current step.
Optional data lines to specify global (or local, if the ORIENTATION parameter is used) degrees of
freedom that define the free directions along which inertia relief loads are applied:
First line:
1. Integer list of degrees of freedom identifying the free directions.
Second line (only needed to define a reference point for the rigid body direction vectors when the
user-chosen combination of free directions requires such a point):
1. Global X-coordinate of the reference point.
2. Global Y-coordinate of the reference point.
3. Global Z-coordinate of the reference point.
These data lines are needed only if rigid body motions are constrained in some directions.
9.17–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*INERTIA RELIEF
There are no data lines when the FIXED or REMOVE parameters are specified.
9.17–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 27.2.1 of the ABAQUS Analysis User’s Manual
Required parameters:
TYPE
Set TYPE=ACOUSTIC STATIC PRESSURE to define initial static pressure values at acoustic
nodes for use in evaluating the cavitation status of the acoustic element nodes in ABAQUS/Explicit.
Set TYPE=CONCENTRATION to give initial normalized concentrations for a mass diffusion
analysis in ABAQUS/Standard.
Set TYPE=CONTACT to specify initial bonded contact conditions on part of the slave surface
identified by a node set in an ABAQUS/Standard analysis.
Set TYPE=FIELD to specify initial values of field variables. The VARIABLE parameter can
be used with this parameter to define the field variable number. The STEP and INC parameters can
be used in conjunction with the FILE parameter to define initial values of field variables based on
the temperature record of a results file from a previous ABAQUS/Standard heat transfer analysis.
Set TYPE=FLUID PRESSURE to give initial pressures for hydrostatic fluid filled cavities.
Set TYPE=HARDENING to prescribe initial equivalent plastic strain and, if relevant, the
initial backstress tensor or to prescribe initial volumetric compacting plastic strain for the crushable
foam model. In ABAQUS/Standard the REBAR and USER parameters can be used with this
parameter. If the USER parameter is omitted, ABAQUS/Standard assumes that the initial conditions
are defined on the data lines.
Set TYPE=INITIAL GAP to identify the elements within which tangential fluid flow exists
initially.
Set TYPE=MASS FLOW RATE to specify initial values of mass flow rates in
ABAQUS/Standard heat transfer analyses involving forced convection modeled with the
forced convection/diffusion heat transfer elements.
Set TYPE=PLASTIC STRAIN to specify initial plastic strains. The SECTION POINTS
parameter can be used with this parameter. It is assumed that the plastic strain components are
defined on each data line in the order given for the element type, as defined in Part VI, “Elements,”
of the ABAQUS Analysis Users Manual.
9.18–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. The STEP and INC parameters can be used in conjunction with the
FILE parameter to define initial values of pressure stress from the results file of a previous
ABAQUS/Standard stress/displacement analysis.
Set TYPE=RATIO to give initial void ratio values for a coupled pore fluid diffusion/stress
analysis in ABAQUS/Standard. The USER parameter can be used with this parameter to define
initial void ratio values in user subroutine VOIDRI.
Set TYPE=REF COORDINATE to define the reference mesh (initial metric) for membrane
elements in ABAQUS/Explicit. If a reference mesh is specified for an element, no initial stress or
strain can be specified for the same element. The initial stress and strain are computed automatically
to account for deformation from the reference to the initial configuration.
Set TYPE=RELATIVE DENSITY to give initial relative density values for materials defined
with the *POROUS METAL PLASTICITY option.
Set TYPE=ROTATING VELOCITY to prescribe initial velocities in terms of an angular
velocity and a global translational velocity.
Set TYPE=SATURATION to give initial saturation values for the analysis of flow through a
porous medium in ABAQUS/Standard. If no initial saturation values are given on this option, the
default is fully saturated conditions (saturation of 1.0). For partial saturation the initial saturation
and the pore fluid pressure must be consistent in the sense that the pore fluid pressure must lie within
the range of absorption and exsorption values for the initial saturation value. If this is not the case,
ABAQUS/Standard will adjust the saturation value as needed to satisfy this requirement.
Set TYPE=SOLUTION to give initial values of solution-dependent state variables. The
REBAR and, in ABAQUS/Standard, USER parameters can be used with this parameter. If
TYPE=SOLUTION is used without the USER parameter, element average quantities of the
solution-dependent state variables must be defined on each data line.
Set TYPE=SPECIFIC ENERGY to give initial specific energy values for materials defined
with the *EOS option in ABAQUS/Explicit.
Set TYPE=SPUD EMBEDMENT to give the initial embedment for a spud can in an
ABAQUS/Aqua analysis.
Set TYPE=SPUD PRELOAD to give the initial preload value for a spud can in an
ABAQUS/Aqua analysis.
Set TYPE=STRESS to give initial stresses. (These stresses are effective stresses when the
analysis includes pore fluid flow.) The GEOSTATIC; the REBAR; the SECTION POINTS; and,
in ABAQUS/Standard, the USER parameters can be used with this parameter. If TYPE=STRESS
is used without the USER parameter, it is assumed that the stress components are defined on
each data line in the order given for the element type, as defined in Part VI, “Elements,” of the
ABAQUS Analysis Users Manual.
9.18–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. The parameter specifies the step in the
results file of a previous ABAQUS analysis from which prescribed fields of TYPE=FIELD,
TYPE=PRESSURE STRESS, or TYPE=TEMPERATURE are to be read. It can also specify the
step in the output database file of a previous ABAQUS analysis from which prescribed fields of
TYPE=TEMPERATURE are to be read.
INC
This parameter is used only with the FILE parameter. The parameter specifies the increment in
the results file of a previous ABAQUS analysis from which prescribed fields of TYPE=FIELD,
TYPE=PRESSURE STRESS, or TYPE=TEMPERATURE are to be read. It can also specify the
increment in the output database file of a previous ABAQUS analysis from which prescribed fields
of TYPE=TEMPERATURE are to be read.
Optional parameters:
ABSOLUTE EXTERIOR TOLERANCE
This parameter is relevant only for use with the INTERPOLATE parameter. Set this parameter equal
to the absolute value (given in the units used in the model) by which nodes of the current model may
lie outside the region of the model in the output database specified by the FILE parameter. If this
parameter is not used or has a value of 0.0, the EXTERIOR TOLERANCE parameter will apply.
EXTERIOR TOLERANCE
This parameter is relevant only for use with the INTERPOLATE parameter. Set this parameter equal
to the fraction of the average element size by which nodes of the current model may lie outside the
region of the elements of the model in the output database specified by the FILE parameter. The
default value is 0.05.
If both tolerance parameters are specified, ABAQUS uses the tighter tolerance.
FILE
Set this parameter equal to the name of the results file from which initial field variable or pressure
stress data are to be read. Set this parameter equal to the name of the results file or output database
file from which initial temperature data are to be read. This parameter must be used in conjunction
with the STEP and INC parameters.
GEOSTATIC
This parameter is used only with TYPE=STRESS to specify that a geostatic stress state, in which
stresses vary with elevation only, is being defined.
9.18–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users 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. This feature is used to read
temperatures from an output database file generated during a heat transfer analysis. This parameter
and the MIDSIDE parameter are mutually exclusive. If the heat transfer analysis uses first-order
elements and the current mesh is the same but uses second-order elements, use the MIDSIDE
parameter instead.
MIDSIDE
This parameter applies only to ABAQUS/Standard analyses.
Include this parameter in conjunction with the FILE, STEP, and INC parameters to indicate
that midside node temperatures in second-order elements are to be interpolated from corner
node temperatures. This feature is used to read temperatures from a results or output database
file generated during a heat transfer analysis using first-order elements. This parameter and the
INTERPOLATE parameter are mutually exclusive.
NORMAL
This parameter applies only to ABAQUS/Standard analyses.
This parameter can be used only with TYPE=CONTACT to specify that the nodes in the node
set (or the contact pair, if a node set is not defined) are bonded only in the normal (contact) direction
and are allowed to move freely in the tangential direction. If the nodes in the node set (or the contact
pair) are to be bonded in all directions, this parameter should be omitted.
REBAR
This parameter can be used with TYPE=HARDENING in ABAQUS/Standard,
TYPE=SOLUTION, or TYPE=STRESS.
When used with TYPE=HARDENING in ABAQUS/Standard, it specifies that rebars are in a
work hardened state, with initial equivalent plastic strain and, possibly, initial backstress.
When used with TYPE=SOLUTION, it specifies that rebars are being assigned initial solution-
dependent state variable values.
When used with TYPE=STRESS, it specifies that prestress in rebars is being defined. When
performing an ABAQUS/Standard analysis, some iteration will usually be needed in this case
to establish a self-equilibrating stress state in the rebar and concrete. The *PRESTRESS HOLD
option can be useful for post-tensioning simulations (see “Defining rebar as an element property,”
Section 2.2.4 of the ABAQUS Analysis Users Manual).
9.18–4
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Set UNBALANCED STRESS=RAMP (default) if the unbalanced stress is to be resolved
linearly over the step.
Set UNBALANCED STRESS=STEP if the unbalanced stress is to be resolved in the first
increment.
USER
This parameter applies only to ABAQUS/Standard analyses.
This parameter can be used with TYPE=HARDENING, TYPE=PORE PRESSURE,
TYPE=RATIO, TYPE=SOLUTION, or TYPE=STRESS.
When used with TYPE=HARDENING, it specifies that the initial conditions on equivalent
plastic strain and, if relevant, backstress tensor are to be given via user subroutine HARDINI.
When used with TYPE=PORE PRESSURE, it specifies that initial pore pressures are to be
given via user subroutine UPOREP.
When used with TYPE=RATIO, it specifies that initial void ratios are to be given via user
subroutine VOIDRI.
When used with TYPE=SOLUTION, it specifies that initial solution-dependent state variable
fields are to be given via user subroutine SDVINI.
When used with TYPE=STRESS, it specifies that stresses are to be given via user subroutine
SIGINI.
VA R I A B L E
ThisparameterisusedonlywithTYPE=FIELDwhenitisusedtodenethefieldvariablenumber.
The default is VARIABLE=1. Any number of separate field variables can be used: each must be
numbered consecutively (1, 2, 3, etc.)
Data line for TYPE=ACOUSTIC STATIC PRESSURE:
First (and only) line:
1. Node set or node number.
2. Hydrostatic pressure at the first reference point.
3. X-coordinate of the first reference point.
4. Y-coordinate of the first reference point.
5. Z-coordinate of the first reference point.
6. Hydrostatic pressure at the second reference point.
9.18–5
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. Name of the node set associated with the slave surface.
Repeat this data line as often as necessary to define partially bonded surfaces.
Data lines for TYPE=FIELD, VARIABLE=n:
First line:
1. Node set or node number.
2. Initial value of this field variable at the first temperature point. For shells and beams several
values (or a value and the field variable gradients across the section) can be given at each node
(see “Beam modeling: overview,” Section 23.3.1 of the ABAQUS Analysis Users Manual, as
well as “Shell elements: overview,” Section 23.6.1 of the ABAQUS Analysis Users Manual).
For heat transfer shells the field variables at each temperature point through the shell thickness
must be specified. The number of values depends on the (maximum) number of points specified
on the data lines associated with the *SHELL SECTION options.
3. Initial value of this field variable at the second temperature point.
4. Etc., up to seven values.
Subsequent lines (only needed if initial values must be specified at more than seven temperature
points at any node):
1. Eighth initial value of this field variable at this temperature point.
2. Etc., up to eight initial values per line.
It may be necessary to leave blank data lines for some nodes if any other node in the model has more
than seven field variable points because the total number of field variables that ABAQUS expects
9.18–6
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. Node set or node number of fluid cavity reference node.
2. Fluid pressure.
Repeat this data line as often as necessary to define initial fluid pressure for various fluid-filled cavities.
Data lines to prescribe initial equivalent plastic strain or backstresses using TYPE=HARDENING
if the REBAR, SECTION POINTS, and USER parameters are omitted:
First line:
1. Element number or element set label.
2. Initial equivalent plastic strain, .
3. First value of the initial backstress, . (Only relevant for the kinematic hardening models.)
4. Second value of the initial backstress, . (Only relevant for the kinematic hardening models.)
5. Etc., up to six backstress components. (Only relevant for the kinematic hardening models.)
Give the backstress components as defined for this element type in Part VI, “Elements,” of the
ABAQUS Analysis Users Manual. Values given on the data lines are applied uniformly over the
element. In any element for which an *ORIENTATION option applies, backstresses must be given
in the local system (“Orientations,” Section 2.2.5 of the ABAQUS Analysis Users Manual).
Repeat this data line as often as necessary to define the hardening parameters for various elements or
element sets.
Data lines to prescribe initial volumetric compacting plastic strain for the crushable foam model
using TYPE=HARDENING:
First line:
1. Element number or element set label.
2. Initial volumetric compacting plastic strain, .
Repeat this data line as often as necessary to define the initial volumetric compacting plastic strain for
various elements or element sets.
9.18–7
ABAQUS Version 6.1 Module: ID:
Printed on:
*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, .
4. Initial backstress, . (Only relevant for the kinematic hardening models.)
Repeat this data line as often as necessary to define the hardening parameters for rebars in various
elements or element sets.
No data lines are required for TYPE=HARDENING, USER.
Data lines for TYPE=HARDENING, SECTION POINTS:
First line:
1. Element number or element set label.
2. Section point number.
3. Initial equivalent plastic strain, .
4. First value of the initial backstress, . (Only relevant for the kinematic hardening models.)
5. Second value of the initial backstress, . (Only relevant for the kinematic hardening models.)
6. Third value of the initial backstress, . (Only relevant for the kinematic hardening models.)
Give the backstress components as defined for this element type in Part VI, “Elements,” of the
ABAQUS Analysis Users Manual. In any element for which an *ORIENTATION option applies,
the backstress components must be given in the local system (“Orientations,” Section 2.2.5 of the
ABAQUS Analysis Users Manual).
Repeat this data line as often as necessary to define the hardening parameters in various elements or
element sets. The hardening parameters must be defined at all section points within an element.
Data lines for TYPE=INITIAL GAP:
First line:
1. Element number or element set label.
Repeat this data line as often as necessary to identify various elements or element sets.
Data lines for TYPE=MASS FLOW RATE:
First line:
1. Node set or node number.
9.18–8
ABAQUS Version 6.1 Module: ID:
Printed on:
*INITIAL CONDITIONS
2. Initial mass flow rate per unit area in the x-direction or total initial mass flow rate in the cross-
section 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).
Repeat this data line as often as necessary to define mass flow rates at various nodes or node sets.
Data lines to prescribe initial plastic strains using TYPE=PLASTIC STRAIN if the REBAR and
SECTION POINTS parameters are omitted:
First line:
1. Element number or element set label.
2. Value of first plastic strain component, .
3. Value of second plastic strain component, .
4. Etc., up to six plastic strain components.
Give the plastic strain components as defined for this element type in Part VI, “Elements,” of the
ABAQUS Analysis Users Manual. Values given on the data lines are applied uniformly over the
element. In any element for which an *ORIENTATION option applies, the plastic strains must be
given in the local system (“Orientations,” Section 2.2.5 of the ABAQUS Analysis Users Manual).
Repeat this data line as often as necessary to define initial plastic strains in various elements or element
sets.
Data lines for TYPE=PLASTIC STRAIN, 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 plastic strain value.
Repeat this data line as often as necessary to define the initial plastic strain in the rebars of various
elements or element sets.
Data lines for TYPE=PLASTIC STRAIN, SECTION POINTS:
First line:
1. Element number or element set label.
2. Section point number.
3. Value of first plastic strain component, .
4. Value of second plastic strain component, .
9.18–9
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users 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 Users Manual).
Repeat this data line as often as necessary to define initial plastic strains in various elements or element
sets. Plastic strains must be defined at all section points within an element.
Data lines for TYPE=PORE PRESSURE if the USER parameter is omitted:
First line:
1. Node set or node number.
2. First value of fluid pore pressure, .
3. Vertical coordinate corresponding to the above value.
4. Second value of fluid pore pressure, .
5. Vertical coordinate corresponding to the above value.
Omit the elevation values and the second pore pressure value to define a constant pore pressure
distribution.
Repeat this data line as often as necessary to define the fluid pore pressure at various nodes or node
sets.
No data lines are required for TYPE=PORE PRESSURE, USER.
Data lines for TYPE=POROSITY:
First line:
1. Element number or element set label.
2. Initial porosity.
Repeat this data line as often as necessary to define initial porosity in various elements or element sets.
Data lines for TYPE=PRESSURE STRESS:
First line:
1. Node set or node number.
2. Equivalent pressure stress, p.
Repeat this data line as often as necessary to define the pressure stress at various nodes or node sets.
9.18–10
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Repeat this data line as often as necessary to define void ratios at various nodes or node sets.
No data lines are required for TYPE=RATIO, USER.
Data lines for TYPE=REF COORDINATE:
First line:
1. Element number.
2. X-coordinate of the first node.
3. Y-coordinate of the first node.
4. Z-coordinate of the first node.
5. X-coordinate of the second node.
6. Y-coordinate of the second node.
7. Z-coordinate of the second node.
Second line:
1. X-coordinate of the third node.
2. Y-coordinate of the third node.
3. Z-coordinate of the third node.
4. X-coordinate of the fourth node.
5. Y-coordinate of the fourth node.
6. Z-coordinate of the fourth node.
Repeat this pair of data lines as often as necessary to define the reference mesh in various elements.
The order of the nodal coordinates must be consistent with the element connectivity.
9.18–11
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 ato point b, where the coordinates of aand
bare given below.
3. Global X-component of translational velocity.
4. Global Y-component of translational velocity.
5. Global Z-component of translational velocity.
Second line:
1. Global X-component of point aon the axis of rotation.
2. Global Y-component of point aon the axis of rotation.
3. Global Z-component of point aon the axis of rotation.
4. Global X-component of point bon the axis of rotation.
5. Global Y-component of point bon the axis of rotation.
6. Global Z-component of point bon the axis of rotation.
Repeat this pair of data lines as often as necessary to define the angular and translational velocities at
various nodes or node sets.
Data lines for TYPE=SATURATION:
First line:
1. Node set or node number.
2. Saturation value, s. Default is 1.0.
Repeat this data line as often as necessary to define saturation at various nodes or node sets.
Data lines for TYPE=SOLUTION if the USER and REBAR parameters are omitted:
First line:
1. Element number or element set label.
2. Value of first solution-dependent state variable.
3. Value of second solution-dependent state variable.
4. Etc., up to seven solution-dependent state variables.
9.18–12
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
It may be necessary to leave blank data lines for some elements if any other element in the model
has more solution-dependent state variables because the total number of variables that ABAQUS
expects to read for any element is based on the maximum number of solution-dependent state
variables for all the elements in the model. These trailing initial values will be zero and will not be
used in the analysis. Values given on the data lines will be applied uniformly over the element.
Repeat this set of data lines as often as necessary to define initial values of solution-dependent state
variables for various elements or element sets.
Data lines for TYPE=SOLUTION, REBAR:
First line:
1. Element number or element set label.
2. Rebar name. If this field is left blank, the solution-dependent state variables are applied to all
rebars in these elements.
3. Value of first solution-dependent state variable.
4. Value of second solution-dependent state variable.
5. Etc., up to six solution-dependent state variables.
Subsequent lines (only needed if more than six solution-dependent state variables exist in the model):
1. Value of seventh solution-dependent state variable.
2. Etc., up to eight solution-dependent state variables per line.
It may be necessary to leave blank data lines for some elements if any other element in the model
has more solution-dependent state variables because the total number of variables that ABAQUS
expects to read for any element is based on the maximum number of solution-dependent state
variables for all the elements in the model. These trailing initial values will be zero and will not be
used in the analysis. Values given on the data lines will be applied uniformly over the element.
Repeat this set of data lines as often as necessary to define initial values of solution-dependent state
variables for various elements or element sets.
No data lines are required for TYPE=SOLUTION, USER.
Data lines for TYPE=SPECIFIC ENERGY:
First line:
1. Element number or element set label.
9.18–13
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. Spud can preload, .
Repeat this data line as often as necessary to define initial preload for various elements or element sets.
Data lines for TYPE=STRESS if the GEOSTATIC, REBAR, SECTION POINTS, and USER
parameters are omitted:
First line:
1. Element number or element set label.
2. Value of first (effective) stress component, axial force when used with the *BEAM GENERAL
SECTION or *FRAME SECTION options, or direct membrane force per unit width in the local
1-direction when used with the *SHELL GENERAL SECTION option.
3. Value of second stress component.
4. Etc., up to six stress components.
Give the stress components as defined for this element type in Part VI, “Elements,” of the
ABAQUS Analysis Users Manual. Stress values given on data lines are applied uniformly and
equally over all integration points of the element. In any element for which an *ORIENTATION
option applies, the stresses must be given in the local system (“Orientations,” Section 2.2.5 of the
ABAQUS Analysis Users Manual).
Repeat this data line as often as necessary to define initial stresses in various elements or element sets.
Data lines for TYPE=STRESS, GEOSTATIC:
First line:
1. Element number or element set label.
2. First value of vertical component of (effective) stress.
9.18–14
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. If this value is omitted, it is assumed to be the same as the first lateral
stress coefficient given in the previous field.
Repeat this data line as often as necessary to define an initial geostatic stress state in various elements
or element sets.
Data lines for TYPE=STRESS, REBAR:
First line:
1. Element number or element set label.
2. Rebar name. If this field is left blank, the stress is applied to all rebars in these elements.
3. Prestress value.
Repeat this data line as often as necessary to define initial stress in the rebars of various elements or
element sets.
Data lines for TYPE=STRESS, SECTION POINTS:
First line:
1. Element number or element set label.
2. Section point number.
3. Value of first stress component.
4. Value of second stress component.
5. Etc., up to three stress components.
Give the stress components as defined for this element type in Part VI, “Elements,” of the
ABAQUS Analysis Users Manual. Stress values given on data lines are applied uniformly over
the element. In any element for which an *ORIENTATION option applies, the stresses must be
given in the local system (“Orientations,” Section 2.2.5 of the ABAQUS Analysis Users Manual).
Repeat this data line as often as necessary to define initial stresses in various elements or element sets.
Stresses must be defined at all section points within an element.
9.18–15
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 23.3.6 of the ABAQUS Analysis Users Manual; “Using a general beam section to
define the section behavior,” Section 23.3.7 of the ABAQUS Analysis Users Manual; “Using
a shell section integrated during the analysis to define the section behavior,” Section 23.6.5
of the ABAQUS Analysis User’s Manual; and “Using a general shell section to define the
section behavior,” Section 23.6.6 of the ABAQUS Analysis Users Manual). For heat transfer
shells the temperature at each point through the shell thickness must be specified. The number
of values depends on the (maximum) number of points specified on the data lines associated
with the *SHELL SECTION options.
3. Second initial temperature value at the node or node set.
4. Etc., up to seven initial temperature values at this node or node set.
Subsequent lines (only needed if there are more than seven temperature values at any node):
1. Eighth initial temperature value at this node or node set.
2. Etc., up to eight initial temperature values per line.
If more than seven temperature values are needed at any node, continue on the next line. It may
be necessary to leave blank data lines for some nodes if any other node in the model has more than
seven temperature points because the total number of temperatures that ABAQUS expects to read
for any node is based on the maximum number of temperature values of all the nodes in the model.
These trailing initial values will be zero and will not be used in the analysis.
Repeat this data line (or set of lines) as often as necessary to define initial temperatures at various nodes
or node sets.
No data lines are required for TYPE=TEMPERATURE, FILE=file,STEP=step,INC=inc.
No data lines are required for TYPE=TEMPERATURE, MIDSIDE, FILE=file,STEP=step,INC=inc.
No data lines are required for TYPE=TEMPERATURE, INTERPOLATE, FILE=file,STEP=step,
INC=inc.
9.18–16
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
9.18–17
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Products: ABAQUS/Standard ABAQUS/Explicit
Type: Model data
Level: Assembly
References:
“Defining an assembly,” Section 2.9.1 of the ABAQUS Analysis Users Manual
“Transferring results between ABAQUS analyses: overview,” Section 9.2.1 of the ABAQUS Analysis
Users Manual
*END INSTANCE
*IMPORT
Required parameters if the instance is not imported from a previous analysis:
NAME
Set this parameter equal to a label that will be used to refer to the instance.
PART
Set this parameter equal to the name of the part being instanced.
Required parameter if the instance is to be imported from a previous analysis:
INSTANCE
Set this parameter equal to the name of the instance to be imported from the previous analysis.
Optional import parameter:
LIBRARY
Set this parameter equal to the name of the previous analysis from which the instance should
be imported. The previous analysis output database (.odb) file should reside in the current
(working) directory. If the LIBRARY parameter is omitted, the job name of the previous analysis
must be specified on the command line using the oldjob parameter (see “Execution procedure
for ABAQUS/Standard and ABAQUS/Explicit,” Section 3.2.2 of the ABAQUS Analysis Users
Manual). If both methods are used, the command line specification will take precedence over the
LIBRARY parameter.
9.19–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. 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 aon the axis of rotation (see Figure 9.19–1).
2. Y-coordinate of point aon the axis of rotation.
3. Z-coordinate of point aon the axis of rotation.
4. X-coordinate of point bon the axis of rotation.
5. Y-coordinate of point bon the axis of rotation.
6. Z-coordinate of point bon the axis of rotation.
7. Angle of rotation about the axis ab, in degrees.
If both translation and rotation are specified, translation is applied before rotation.
There are no data lines for an instance that is imported from a previous analysis.
9.19–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*INSTANCE
θ
a
b
θ
Figure 9.19–1 Rotation of an instance.
9.19–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*INTEGRATED OUTPUT
9.20 *INTEGRATED OUTPUT: Specify variables integrated over a surface to be written to
the output database.
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 4.1.3 of the ABAQUS Analysis Users Manual
“Integrated output section definition,” Section 2.5.1 of the ABAQUS Analysis Users Manual
*OUTPUT
*SURFACE
*INTEGRATED OUTPUT SECTION
Required, mutually exclusive parameters:
SECTION
Set this parameter equal to the name of the *INTEGRATED OUTPUT SECTION (see “Integrated
output section definition,” Section 2.5.1 of the ABAQUS Analysis Users Manual) over which this
output request is being made.
SURFACE
Set this parameter equal to the name of the surface (see “Defining element-based surfaces,”
Section 2.3.2 of the ABAQUS Analysis Users Manual) over which this output request is being
made.
Optional parameter:
VA R I A B L E
Set VARIABLE=ALL to indicate that all integrated output variables applicable to this procedure
should be written to the output database.
Set VARIABLE=PRESELECT to indicate that the default integrated output variables for the
current procedure type should be written to the output database. Additional output variables can be
requestedonthedatalines.
If this parameter is omitted, the integrated output variables for output must be specified on the
data line.
9.20–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual.
Repeat this data line as often as necessary to define the list of variables to be written to the output
database.
9.20–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Product: ABAQUS/Explicit
Type: Model data
Level: Part, Part instance, Assembly
References:
“Integrated output section definition,” Section 2.5.1 of the ABAQUS Analysis Users Manual
“Output to the output database,” Section 4.1.3 of the ABAQUS Analysis Users Manual
*INTEGRATED OUTPUT
*SURFACE
Required parameters:
NAME
Set this parameter equal to a label that will be used to refer to the integrated output section.
SURFACE
Set this parameter equal to the name of the surface (see “Defining element-based surfaces,”
Section 2.3.2 of the ABAQUS Analysis Users Manual) to be associated with the integrated output
section.
Optional parameters:
ORIENTATION
Set this parameter equal to the name of an orientation definition (“Orientations,” Section 2.2.5 of
the ABAQUS Analysis Users Manual) to define the initial coordinate system for the section. This
initial system can be further modified by using the PROJECT ORIENTATION parameter.
If this parameter is omitted, the global coordinate system is used.
POSITION
This parameter is relevant only if the REF NODE parameter is included.
Set POSITION=INPUT (default) if the location of the reference node is to be defined by the
user.
9.21–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. If an orientation is not
specified, the initial coordinate system matches the global coordinate system.
Set PROJECT ORIENTATION=YES if the initial coordinate system of the section should
be modified by projecting onto the section surface using the average normal to the surface. If an
orientation is not specified, the global coordinate system is projected onto the section surface.
REF NODE
Set this parameter equal to either the node number of the integrated output section reference node
or to the name of a node set containing the reference node. If the name of a node set is chosen, the
node set must contain exactly one node.
REF NODE MOTION
This parameter is relevant only if the REF NODE parameter is included.
Set REF NODE MOTION=INDEPENDENT (default) if the motion of the reference node is
not based on the average motion of the surface.
Set REF NODE MOTION=AVERAGE TRANSLATION if the reference node must translate
with the average translation of the surface. This choice is relevant only if the reference node is not
connected to the rest of the model.
Set REF NODE MOTION=AVERAGE if the reference node must both translate and rotate
with the average motion of the surface. This choice is relevant only if the reference node is not
connected to the rest of the model.
There are no data lines associated with this option.
9.21–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*INTERACTION OUTPUT
9.22 *INTERACTION OUTPUT: Specify spot weld interaction variables to be written to the
output database.
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 Users Manual
“Mesh-independent fasteners,” Section 28.3.4 of the ABAQUS Analysis User’s Manual
*OUTPUT
Required, mutually exclusive parameters:
NAME
Set this parameter equal to the name of the spot weld interaction for which this output request is
being made.
NSET
Set this parameter equal to the name of the node set for which this output request is being made.
Data lines to request spot weld interaction output to the output database:
First line:
1. Specify the identifying keys for the output 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 Users Manual, and “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.
9.22–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
“Mesh-independent fasteners,” Section 28.3.4 of the ABAQUS Analysis User’s Manual
Optional, mutually exclusive parameters:
NAME
Set this parameter equal to the name of the spot weld interaction for which this output request is
being made.
NSET
Set this parameter equal to the name of the node set for which this output request is being made.
Optional parameters:
FREQUENCY
Set this parameter equal to the output frequency, in increments. The default is FREQUENCY=1.
Set FREQUENCY=0 to suppress the output. The output will always be printed at the last increment
of each step unless FREQUENCY=0.
SUMMARY
Set SUMMARY=YES (default) to obtain a summary of the maximum and minimum values in each
column of the table and their locations. Set SUMMARY=NO to suppress this summary.
TOTALS
Set TOTALS=YES to print the total of each column in the table. The default is TOTALS=NO.
9.23–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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
Users 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.
9.23–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
“Tube-to-tube contact elements,” Section 31.3.1 of the ABAQUS Analysis User’s Manual
“Slide line contact elements,” Section 31.4.1 of the ABAQUS Analysis Users Manual
“Rigid surface contact elements,” Section 31.5.1 of the ABAQUS Analysis User’s Manual
Required parameter:
ELSET
Set this parameter equal to the name of the element set containing the ITT-, ISL-, IRS-, and ASI-type
contact elements for which properties are being defined.
Optional parameter:
NAME
Set this parameter equal to a label that will be used to refer to this interface definition. The label
given can be used to identify this particular interface definition in user subroutines such as GAPCON.
Data line for ITT-type elements:
First (and only) line:
1. Radial clearance between the pipes.
Data lines for ISL21A and ISL22A elements:
There are no data lines.
Data lines for IRS-type elements for use with axisymmetric elements:
There are no data lines.
9.24–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Data lines for ASI-type elements for use with axisymmetric elements or 3-D elements:
There are no data lines.
9.24–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 31.5.1 of the ABAQUS Analysis User’s Manual
*DASHPOT
*FRICTION
*SPRING
Required parameter:
ELSET
Set this parameter equal to the name of the element set containing the ITS-type elements for which
properties are being defined.
Data line for ITSUNI elements:
First (and only) line:
1. Tube outside diameter.
2. Distance between the parallel support plates on opposite sides of the tube.
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.
6. X-direction cosine of the normal to either one of the support plates.
7. Y-direction cosine of the normal to either one of the support plates.
8. Z-direction cosine of the normal to either one of the support plates.
Data line for ITSCYL elements:
First (and only) line:
1. Tube outside diameter.
9.25–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
9.25–2
ABAQUS Version 6.1 Module: ID:
Printed on:
J
10. J
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 26.3.1 of the ABAQUS Analysis Users Manual
*DASHPOT
*SPRING
Required parameter:
ELSET
Set this parameter equal to the name of the element set containing the JOINTC elements for which
properties are being defined.
Optional parameter:
ORIENTATION
Set this parameter equal to the name given to the *ORIENTATION definition (“Orientations,”
Section 2.2.5 of the ABAQUS Analysis Users Manual) that specifies the initial orientation of the
local system in the joint.
There are no data lines associated with this option; instead, include *SPRING and *DASHPOT
options as needed to define the joint behavior.
10.1–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
*EPJOINT
Required parameters:
MODULI
Set MODULI=SPUD CAN to define spud can moduli. Set MODULI=GENERAL to enter a general
elastic modulus.
NDIM
Set NDIM=2 to enter values for a two-dimensional problem. Set NDIM=3 to enter values for a
three-dimensional problem.
Optional parameter:
DEPENDENCIES
Set this parameter equal to the number of field variable dependencies included in the definition
of the moduli. If this parameter is omitted, it is assumed that the moduli are constant or depend
only on temperature. See “Specifying field variable dependence” in “Material data definition,”
Section 16.1.2 of the ABAQUS Analysis Users Manual, for more information.
Data lines for MODULI=SPUD CAN and NDIM=2:
First line:
1. , equivalent elastic shear modulus for vertical displacements.
2. , equivalent elastic shear modulus for horizontal displacements.
3. , equivalent elastic shear modulus for rotational displacements.
4. , Poisson’s ratio of the soil.
10.2–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*JOINT ELASTICITY
5. Temperature.
6. First field variable.
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 elastic behavior as a function of
temperature and other predefined field variables.
Data lines for MODULI=SPUD CAN and NDIM=3:
First line:
1. , equivalent elastic shear modulus for vertical displacements.
2. , equivalent elastic shear modulus for horizontal displacements.
3. , equivalent elastic shear modulus for rotational displacements.
4. , Poisson’s ratio of the soil.
5. , torsional elastic modulus.
6. Temperature.
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.
Data lines for MODULI=GENERAL and NDIM=2:
First line:
1. .
2. .
3. .
4. .
5. .
6. .
10.2–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. .
Third line:
1. .
2. .
3. .
4. .
5. .
6. Temperature.
10.2–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
10.2–4
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 26.11.1 of the ABAQUS Analysis Users Manual
*EPJOINT
Required parameter:
TYPE
Set TYPE=SAND to specify the model for interaction of spud cans and sand. Set TYPE=CLAY
to specify the model for interaction of spud cans and clay. Set TYPE=MEMBER to specify the
parabolic model for structural members.
Optional parameter:
DEPENDENCIES
Set this parameter equal to the number of field variable dependencies included in the definition of
the plasticity property values. If this parameter is omitted, it is assumed that the plasticity property
values are constant or depend only on temperature. See “Specifying field variable dependence”
in “Material data definition,” Section 16.1.2 of the ABAQUS Analysis Users Manual, for more
information.
Data lines for TYPE=SAND:
First line:
1. , yield strength in pure tension.
2. , constant for yield surface shape.
3. , constant for yield surface shape.
4. , soil friction angle, in degrees.
5. , soil unit weight.
6. Temperature.
10.3–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. , undrained shear strength of the clay.
2. a, hardening parameter.
3. b, hardening parameter.
4. c, hardening parameter.
5. Temperature.
6. First field variable.
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 plastic behavior as a function of
temperature and other predefined field variables.
Data lines for TYPE=MEMBER:
First line:
1. , compressive capacity.
2. , tensile capacity.
3. , horizontal capacity.
4. , moment capacity.
5. Temperature.
6. First field variable.
7. Second field variable.
8. Third field variable.
10.3–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
10.3–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 18.4.1 of the ABAQUS Analysis Users Manual
Optional parameters:
DEPENDENCIES
Set this parameter equal to the number of field variable dependencies included in the definition of
the parameters of the model, in addition to temperature. If this parameter is omitted, it is assumed
that the parameters depend only on temperature. See “Specifying field variable dependence” in
“Material data definition,” Section 16.1.2 of the ABAQUS Analysis Users Manual, for more
information.
JOINT DIRECTION
Set this parameter equal to the name of the *ORIENTATION used to define the direction of a joint
system. This use of the *ORIENTATION option does not affect the output of components of stress
and strain—it only defines the joint orientation in the original configuration. Omit this parameter to
give the bulk material failure parameters. The JOINT DIRECTION parameter cannot be used with
the SHEAR RETENTION parameter.
NO SEPARATION
Include this parameter to prevent the joint from opening. This parameter must be used in conjunction
with the JOINT DIRECTION parameter.
SHEAR RETENTION
Include this parameter to define shear retention in open joints. If this parameter is omitted, zero
shear retention is assumed. The SHEAR RETENTION parameter cannot be used with the JOINT
DIRECTION parameter.
10.4–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. 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 failure and surface
flow parameters on temperature and other predefined field variables.
Data lines defining the shear retention in open joints (SHEAR RETENTION included):
First line:
1. Fraction of elastic shear modulus retained when joints are open, . This value cannot be less
than zero.
2. Temperature.
3. First field variable.
4. Second field variable.
5. Etc., up to six field variables.
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 dependence of the shear retention on
temperature and other predefined field variables.
10.4–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 thermal-
electrical problems.
Product: ABAQUS/Standard
Type: Model data
Level: Model
Reference:
“Coupled thermal-electrical analysis,” Section 6.6.2 of the ABAQUS Analysis Users Manual
There are no parameters associated with this option.
Data line to define the joule heat fraction:
First (and only) line:
1. Fraction of electrical energy released as heat, including any unit conversion factor. The default
value is 1.0.
10.5–1
ABAQUS Version 6.1 Module: ID:
Printed on:
K
11. K
ABAQUS Version 6.1 Module: ID:
Printed on:
*KAPPA
11.1 *KAPPA: Specify the material parameters and for mass diffusion driven by
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.
Product: ABAQUS/Standard
Type: Model data
Level: Model
References:
“Diffusivity,” Section 20.5.1 of the ABAQUS Analysis Users Manual
*DIFFUSIVITY
Optional parameters:
DEPENDENCIES
Set this parameter equal to the number of field variables included in the definition of or .If
this parameter is omitted, or is assumed not to depend on any field variables but may still
depend on concentration and temperature. See “Specifying field variable dependence” in “Material
data definition,” Section 16.1.2 of the ABAQUS Analysis User’s Manual, for more information.
TYPE
Set TYPE=TEMP (default) to define (governing mass diffusion caused by temperature
gradients). Set TYPE=PRESS to define (governing mass diffusion caused by gradients of the
equivalent pressure stress).
Data lines to define the Soret effect factor, ks(TYPE=TEMP):
First line:
1. Soret effect factor, .(UnitsofF
1/2 L−1 .)
2. Concentration, c.
3. Temperature, .
4. First field variable.
5. Second field variable.
6. Etc.,uptofivefieldvariables.
11.1–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 as a function of concentration,
temperature, and other predefined field variables.
Data lines to define the pressure stress factor, kp(TYPE=PRESS):
First line:
1. Pressure stress factor, .(UnitsofLF
−1/2 .)
2. Concentration, c.
3. Temperature, .
4. First field variable.
5. Second field variable.
6. Etc.,uptofivefieldvariables.
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 as a function of concentration,
temperature, and other predefined field variables.
11.1–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
*COUPLING
There are no parameters associated with this option.
Data lines to specify the degrees of freedom to be constrained:
First line:
1. First degree of freedom constrained. See “Conventions,” Section 1.2.2 of the
ABAQUS Analysis Users Manual, for a definition of the numbering of degrees of freedom
in ABAQUS. If this field is left blank, all degrees of freedom will be constrained.
2. Last degree of freedom constrained. If this field is left blank, the degree of freedom specified
in the first field will be the only one constrained.
Repeat this data line as often as necessary to specify constraints for different degrees of freedom. When
the ORIENTATION parameter is specified on the associated *COUPLING option, the degrees of freedom
are in the referenced local system in the initial configuration; otherwise, they are in the global system. In
either case these directions will rotate with the reference node in large-displacement analyses (when the
NLGEOM parameter is included on the *STEP option).
11.2–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Product: ABAQUS/Standard
Type: Model data
Level: Part, Part instance, Assembly
Reference:
“Kinematic constraints: overview,” Section 28.1.1 of the ABAQUS Analysis User’s Manual
Required parameter:
REF NODE
Set this parameter equal to either the node number of the reference node or the name of a node set
containing the reference node. If the name of a node set is chosen, the node set must contain exactly
one node.
Optional parameter:
ORIENTATION
Set this parameter equal to the name given to the *ORIENTATION definition (“Orientations,”
Section 2.2.5 of the ABAQUS Analysis Users Manual) that specifies the initial orientation of the
local system in which the constrained degrees of freedom are defined.
Data lines to specify the nodes and degrees of freedom to be constrained:
First line:
1. Node number or node set label.
2. First degree of freedom constrained. See “Conventions,” Section 1.2.2 of the
ABAQUS Analysis Users Manual, for a definition of the numbering of degrees of freedom
in ABAQUS/Standard. If this field is left blank, all degrees of freedom will be constrained.
11.3–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. In either case these
directions will rotate with the reference node in large-displacement analyses (when the NLGEOM
parameter is included on the *STEP option).
11.3–2
ABAQUS Version 6.1 Module: ID:
Printed on:
L
12. L
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users 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.
Repeat this data line as often as necessary to define phase changes in the material; one line per phase
change. Latent heat values must be given in ascending order of temperature.
12.1–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users 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.
12.2–1
ABAQUS Version 6.1 Module: ID:
Printed on:
M
13. M
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
Optional parameters:
INC
Set this parameter equal to the increment number from which the old solution will be read. If this
parameter is omitted, the last increment for which a solution is available will be read.
The STEP parameter must be specified if the INC parameter is used.
STEP
Set this parameter equal to the step number from which the old solution will be read. If this
parameter is omitted, the last step and increment for which a solution is available will be read.
UNBALANCED STRESS
Set UNBALANCED STRESS=RAMP (default) if the stress unbalance is to be resolved linearly
over the step.
Set UNBALANCED STRESS=STEP if the stress unbalance is to be resolved in the first
increment.
Data line to translate an old-model mesh:
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 old-model mesh:
First line:
1. Value of the translation to be applied in the X-direction.
13.1–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 aon the axis of rotation (see Figure 13.1–1).
2. Y-coordinate of point aon the axis of rotation.
3. Z-coordinate of point aon the axis of rotation.
4. X-coordinate of point bon the axis of rotation.
5. Y-coordinate of point bon the axis of rotation.
6. Z-coordinate of point bon the axis of rotation.
7. Angle of rotation about the axis ab, in degrees.
If both translation and rotation are specified, translation is applied before rotation.
θ
a
b
θ
Figure 13.1–1 Rotation of an old-model mesh.
13.1–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 direct-
integration 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 24.1.1 of the ABAQUS Analysis Users Manual
Required parameter:
ELSET
Set this parameter equal to the name of the element set containing the MASS elements for which
the value is being given.
Optional parameters:
ALPHA
This parameter applies only to ABAQUS/Standard analyses.
Set this parameter equal to the factor to create mass proportional damping for the MASS
elements when used in direct-integration dynamics. This value is ignored in modal dynamics. The
default is 0.0.
COMPOSITE
This parameter applies only to ABAQUS/Standard analyses.
Set this parameter equal to the fraction of critical damping to be used with the MASS elements
when calculating composite damping factors for the modes when used in modal dynamics. This
value is ignored in direct-integration dynamics. The default is 0.0.
13.2–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 users choice must be consistent.
13.2–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
Optional parameters:
DCMAX
Set this parameter equal to the maximum normalized concentration change to be allowed in
an increment. ABAQUS/Standard will restrict the time step to ensure that this value will not
be exceeded at any node (except nodes with boundary conditions) during any increment of the
analysis. If the DCMAX parameter is omitted, fixed time increments will be used.
END
Set END=PERIOD (default) to analyze the entire time period specified on the data line. Set
END=SS to end the analysis when steady state is reached.
STEADY STATE
Include this parameter to choose steady-state analysis. Transient analysis is assumed if this
parameter is omitted.
Data line to define time stepping in a mass diffusion analysis:
First (and only) line:
1. Time step. If automatic stepping is used, this value should be a reasonable suggestion for the
initial step and will be adjusted as necessary.
2. Time period. If END=SS is chosen, the step ends when steady state is reached or after this
time period, whichever occurs first.
3. Minimum time increment allowed. If ABAQUS/Standard finds it needs a smaller time
increment than this value, the analysis is terminated. If no value is given, ABAQUS/Standard
sets the minimum increment to the minimum of 0.8 times the suggested initial time step (the
first data item on this line) and 10−5 times the time period (the second data item on this line).
13.3–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. When all nodal normalized concentrations are
changing at less than this rate, the solution terminates.
13.3–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 6.5.2 of the ABAQUS Analysis User’s Manual
“UMASFL,” Section 1.1.30 of the ABAQUS User Subroutines Reference Manual
Optional parameters:
AMPLITUDE
Set this parameter equal to the name of the amplitude versus time curve that defines the magnitude
of the flow rate during the step (“Amplitude curves,” Section 27.1.2 of the ABAQUS Analysis
Users Manual). If this parameter is omitted, the reference magnitude is applied immediately at the
beginning of the step or linearly over the step, depending on the value assigned to the AMPLITUDE
parameter on the *STEP option (“Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis
Users Manual).
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 Users Manual, for the
syntax of such file names. If this parameter is omitted, it is assumed that the data follow the keyword
line.
OP
Set OP=MOD (default) for existing *MASS FLOW RATE values to remain, with this option
modifying existing flow rates or defining additional flow rates.
Set OP=NEW if all existing *MASS FLOW RATE values applied to the model should be
removed.
USER
Include this parameter to indicate that user subroutine UMASFL will be used to define mass flow
rate values. UMASFL will be called for each node given on the data lines. If values are also given
on the data lines, these values will be ignored.
13.4–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 )ortotalmassflowrateinthe
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 one-
dimensional elements).
4. Mass flow rate per unit area in the z-direction (not needed for nodes associated with one-
dimensional elements).
Repeat this data line as often as necessary to define mass flow rates at different nodes.
Data lines to define mass flow rates using user subroutine UMASFL:
First line:
1. Node set or node number.
Repeat this data line as often as necessary. UMASFL will be called for each node listed.
13.4–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users 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. Furthermore, material names should
be unique from the names associated with property definitions such as *CONNECTOR BEHAVIOR
and *FLUID BEHAVIOR. Material names adhere to the naming convention for labels (see “Input
syntax rules,” Section 1.2.1 of the ABAQUS Analysis Users Manual), except that they cannot begin
with a number.
Optional parameters:
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.
SRATE FACTOR
This parameter applies only to ABAQUS/Explicit analyses.
Set this parameter equal to the factor used for filtering the equivalent plastic strain rate for the
evaluation of strain rate-dependent material data. The default value is 0.9.
STRAIN RATE REGULARIZATION
This parameter applies only to ABAQUS/Explicit analyses and is used only to regularize strain
rate-dependent material data.
Set STRAIN RATE REGULARIZATION=LOGARITHMIC (default) to use a logarithmic
regularization for strain rate-dependent material data.
13.5–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
13.5–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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
ortwicetogivebothmatrices.
Product: ABAQUS/Standard
Type: Model data
Level: Part, Part instance, Model
References:
“User-defined elements,” Section 26.15.1 of the ABAQUS Analysis Users Manual
*USER ELEMENT
Required parameter:
TYPE
Set TYPE=MASS to define the mass matrix. Set TYPE=STIFFNESS to define the stiffness matrix.
Optional parameter:
INPUT
Set this parameter equal to the name of the alternate input file from which the data lines are to
be read. See “Input syntax rules,” Section 1.2.1 of the ABAQUS Analysis Users Manual, for the
syntax of such file names. If this parameter is omitted, it is assumed that the data follow the keyword
line.
Data lines to define the matrix:
First line:
1. Matrix entries, four per line.
Repeat this data line as often as necessary.
13.6–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 2.10.1 of the ABAQUS Analysis Users Manual
*MATRIX INPUT
At least one of the following parameters is required:
MASS
Set this parameter equal to the name of the mass matrix.
STIFFNESS
Set this parameter equal to the name of the stiffness matrix.
There are no data lines associated with this option.
13.7–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
*MATRIX ASSEMBLE
Required parameter:
NAME
Set this parameter equal to a label that will be used to refer to this matrix.
Optional parameters:
INPUT
Set this parameter equal to the name of the alternate input file from which the data lines are to
be read. See “Input syntax rules,” Section 1.2.1 of the ABAQUS Analysis Users Manual, for the
syntax of such file names. If this parameter is omitted, it is assumed that the data follow the keyword
line.
SCALE FACTOR
Set this parameter equal to a nonzero real number by which all matrix entries will be multiplied.
The default value is .
Data lines to define the matrix in sparse format (only nonzero terms):
First line:
1. Row node number.
2. Degree of freedom number for row node.
3. Column node number.
13.8–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
13.8–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 23.1.1 of the ABAQUS Analysis User’s Manual
Required parameters:
ELSET
Set this parameter equal to the name of the element set containing the membrane elements for which
the section properties are being defined.
MATERIAL
Set this parameter equal to the name of the material to be used with these elements.
Optional parameters:
CONTROLS
In an ABAQUS/Explicit analysis, set this parameter equal to the name of a section controls
definition (see “Section controls,” Section 21.1.4 of the ABAQUS Analysis Users Manual) to be
used to specify a nondefault hourglass control formulation option or scale factors.
In an ABAQUS/Standard analysis, set this parameter equal to the name of a section
controls definition to be used to specify the enhanced hourglass control formulation (see “Section
controls,” Section 21.1.4 of the ABAQUS Analysis Users Manual) or to be used in a subsequent
ABAQUS/Explicit import analysis.
DENSITY
Set this parameter equal to a mass per unit surface area of the membrane.
If this parameter is used, the mass of the membrane includes a contribution from this parameter
in addition to any contribution from the material definition.
13.9–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. Set it equal to a nonzero value
to cause the thickness to change as a function of membrane strains. The value of the POISSON
parameter must be between −1.0 and 0.5. A value of 0.5 will enforce incompressible behavior of
the element. POISSON=0.0 means that the thickness will not change.
Set this parameter equal to MATERIAL in an ABAQUS/Explicit analysis to cause the thickness
to change based on the element material definition.
The default is POISSON=0.5 in ABAQUS/Standard and POISSON=MATERIAL in
ABAQUS/Explicit.
Data line for a constant thickness membrane:
First (and only) line:
1. Section thickness.
To define a continuously varying thickness membrane:
No data lines are used with this option when the NODAL THICKNESS parameter is specified; any
value input on the data line will be ignored. Instead, the *NODAL THICKNESS option is used to
define the section thickness.
13.9–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 *FREQUENCYstepwillbeused
with the damping values specified under the *MODAL DAMPING option. If the *MODAL DAMPING
option is not used, zero damping values are assumed.
Product: ABAQUS/Standard
Type: History data
Level: Step
References:
“Material damping,” Section 20.1.1 of the ABAQUS Analysis User’s Manual
“Dynamic analysis procedures: overview,” Section 6.3.1 of the ABAQUS Analysis Users Manual
Optional, mutually exclusive parameters:
MODAL
Set MODAL=DIRECT to select modal damping using the damping coefficients given in this option.
The data lines after the keyword line specify the modal damping values to be used in the analysis.
If the *MODAL DAMPING option is used without parameters, MODAL=DIRECT is assumed.
Set MODAL=COMPOSITE to select composite modal damping using the damping
coefficients that have been calculated in the *FREQUENCY step (“Natural frequency extraction,”
Section 6.3.5 of the ABAQUS Analysis Users Manual) from the material damping factors
given on the *DAMPING material definition option (“Material damping,” Section 20.1.1 of
the ABAQUS Analysis Users Manual). Composite modal damping can be used only with
DEFINITION=MODE NUMBERS.
RAYLEIGH
Include this parameter to select Rayleigh damping. The damping term for a particular mode is
defined as ,where and are factors defined on the first data line of the
option and is the modal mass and is the modal stiffness for mode M.
STRUCTURAL
Include this parameter to select structural damping, which means that the damping is proportional
to the internal forces but opposite in direction to the velocity. This option can be used only with the
*STEADY STATE DYNAMICS (“Mode-based steady-state dynamic analysis,” Section 6.3.8 of the
ABAQUS Analysis Users Manual) or *RANDOM RESPONSE procedures (“Random response
13.10–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*MODAL DAMPING
analysis,” Section 6.3.11 of the ABAQUS Analysis Users 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
thespeciedmodenumbers.
Set DEFINITION=FREQUENCY RANGE to indicate that the damping values are given for
the specified frequency ranges. Frequency ranges can be discontinuous.
If both the *MODAL DAMPING and *SELECT EIGENMODES options are used in the same
step, the DEFINITION parameter must be set equal to the same value in both options.
Data lines to define a fraction of critical damping by specifying mode numbers (MODAL=DIRECT
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. Fraction of critical damping, .
Repeat this data line as often as necessary to define modal damping for different modes.
Data lines to define Rayleigh damping by specifying mode numbers (RAYLEIGH 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. Mass proportional damping, .
4. Stiffness proportional damping, .
Repeat this data line as often as necessary to define modal damping for different modes.
Data lines to define composite modal damping (MODAL=COMPOSITE):
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.)
Repeat this data line as often as necessary to define modal damping for different modes.
13.10–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Data lines to define a fraction of critical damping by specifying frequency ranges
(MODAL=DIRECT and DEFINITION=FREQUENCY RANGE):
First line:
1. Frequency value (in cycles/time).
2. Fraction of critical damping, .
Repeat this data line as often as necessary to define modal damping for different frequencies. ABAQUS
will interpolate linearly between frequencies and keep the damping value constant and equal to the closest
specified value outside the frequency range.
Data lines to define Rayleigh damping by specifying frequency ranges (RAYLEIGH and
DEFINITION=FREQUENCY RANGE):
First line:
1. Frequency value (in cycles/time).
2. Mass proportional damping, .
3. Stiffness proportional damping, .
Repeat this data line as often as necessary to define modal damping for different frequencies. ABAQUS
will interpolate linearly between frequencies and keep the damping value constant and equal to the closest
specified value outside the frequency range.
Data lines to define structural damping by specifying frequency ranges (STRUCTURAL and
DEFINITION=FREQUENCY RANGE):
First line:
1. Frequency value (in cycles/time).
2. Damping factor, s.
Repeat this data line as often as necessary to define modal damping for different frequencies. ABAQUS
will interpolate linearly between frequencies and keep the damping value constant and equal to the closest
specified value outside the frequency range.
13.10–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 6.3.7 of the ABAQUS Analysis Users Manual
Optional parameter:
CONTINUE
Set CONTINUE=NO (default) to specify that this step is not to carry over the initial conditions
from the results of the preceding step. In this case the initial displacements are zero, and the initial
velocities are taken from the *INITIAL CONDITIONS, TYPE=VELOCITY option if it is used;
otherwise, they are zero. Step time begins at zero.
Set CONTINUE=YES to specify that this step is to carry over the initial conditions from the
end of the immediately preceding *MODAL DYNAMIC step or static perturbation step. If this
preceding step is a *MODAL DYNAMIC step, both the velocities and the displacements from
the end of this step are used as the initial conditions for the current step. If this preceding step is
a static perturbation step, the displacements from this step are used as the initial displacements
for the current step and the initial velocities are taken from the *INITIAL CONDITIONS,
TYPE=VELOCITY option if it is used; otherwise, they are zero. Step time is continued from the
immediately preceding *MODAL DYNAMIC or static perturbation step.
Data line for a transient modal dynamic analysis:
First (and only) line:
1. Time increment to be used.
2. Time period.
13.11–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Product: ABAQUS/Standard
Type: History data
Level: Step
Reference:
“Output to the data and results files,” Section 4.1.2 of the ABAQUS Analysis Users Manual
Optional parameter:
FREQUENCY
This parameter is valid only in mode-based dynamic procedures.
Set this parameter equal to the output frequency, in increments. The output will always be
written to the results file at the last increment of each step unless FREQUENCY=0. The default is
FREQUENCY=1. Set FREQUENCY=0 to suppress the output.
Data lines to request modal output in the results file during mode-based dynamic procedures:
First line:
1. Give the identifying keys for the variables to be written to the results file. The keys are
defined in the “Modal 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.
To write eigendata during an eigenvalue extraction procedure:
No data lines are required; the eigendata are written automatically.
13.12–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Product: ABAQUS/Standard
Type: History data
Level: Step
References:
“Output to the output database,” Section 4.1.3 of the ABAQUS Analysis Users Manual
*OUTPUT
Optional parameter:
VA R I A B L E
Set VARIABLE=ALL to indicate that all modal variables applicable to this procedure and material
type should be written to the output database.
If this parameter is omitted, the modal variables requested for output must be specified on the
data lines.
Data lines to request modal output:
First line:
1. Give the identifying keys for the variables to be written to the output database. The keys are
defined in the “Modal 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 to define the modal variables to be written to the output
database.
13.13–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*MODAL PRINT
13.14 *MODAL PRINT: Print generalized coordinate (modal amplitude) data during a mode-
based 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 4.1.2 of the ABAQUS Analysis Users Manual
Optional parameter:
FREQUENCY
Set this parameter equal to the output frequency, in increments. The output will always be printed
at the last increment of each step unless FREQUENCY=0. The default is FREQUENCY=1. Set
FREQUENCY=0 to suppress the output.
Data lines to request modal output in the data file:
First line:
1. Give the identifying keys for the variables to be printed. The keys are defined in the “Modal
variables” section of “ABAQUS/Standard output variable identifiers,” Section 4.2.1 of the
ABAQUS Analysis Users Manual.
Repeat this data line as often as necessary: each line defines a table.
13.14–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users
Manual
“Removing/reactivating ABAQUS/Standard contact pairs,” Section 29.2.6 of the ABAQUS Analysis
Users Manual
Required, mutually exclusive parameters:
ACTIVATE
Include this parameter in any step during an analysis to indicate that elements or contact pairs may
need to be removed or added during a subsequent restart analysis.
ADD
Include this parameter to indicate that the elements or contact pairs involved are being reactivated
during the step.
Set ADD=STRAIN FREE (or include the ADD parameter without a value) to specify strain-
free reactivation for stress/displacement elements or to reactivate other elements or contact pairs.
Set ADD=WITH STRAIN to specify that stress/displacement elements are reactivated with
strain. This option is not relevant for contact pairs.
REMOVE
Include this parameter to indicate that the elements or contact pairs involved are being removed
during the step.
Optional parameter:
TYPE
This parameter can be used only with the parameters ADD or REMOVE.
Set TYPE=ELEMENT (default) to remove or reactivate elements. Set TYPE=CONTACT
PAIR to remove or reactivate contact pairs.
13.15–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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. For self-contact
the master surface name is omitted or is the same as the slave surface name.
Repeat this data line as often as necessary.
No data lines are used with this option when the ACTIVATE parameter is included.
13.15–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 18.3.3 of the ABAQUS Analysis Users Manual
*MOHR COULOMB HARDENING
Optional parameters:
DEPENDENCIES
Set this parameter equal to the number of field variable dependencies included in the definition
of the material parameters other than temperature. If this parameter is omitted, it is assumed that
the material properties are constant or depend only on temperature. See “Specifying field variable
dependence” in “Material data definition,” Section 16.1.2 of the ABAQUS Analysis Users Manual,
for more information.
DEVIATORIC ECCENTRICITY
Set this parameter equal to the flow potential eccentricity in the deviatoric plane, e. This feature
allows the shape of flow potential in the deviatoric stress space to be controlled independently of
the angle of friction. If this parameter is omitted, the deviatoric eccentricity is calculated by default
as ,where is the Mohr-Coulomb angle of friction defined on the data
lines. The range of values ecan have is .
ECCENTRICITY
Set this parameter equal to the flow potential eccentricity in the meridional plane, . The meridional
eccentricity is a small positive number that defines the rate at which the flow potential approaches
its asymptote. The default is .
Data lines to define a Mohr-Coulomb plasticity model:
First line:
1. Friction angle, ,athighconningpressureinthepplane. Give the value in degrees.
13.16–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*MOHR COULOMB
2. Dilation angle, , at high confining pressure in the pplane. Give the value in degrees.
3. Temperature.
4. First field variable.
5. Second field variable.
6. Etc.,uptofivefieldvariables.
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 dependence of the material parameters
on temperature and other predefined field variables.
13.16–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*MOHR COULOMB HARDENING
13.17 *MOHR COULOMB HARDENING: Specify hardening for the Mohr-Coulomb plasticity
model.
This option is used to define piecewise linear hardening/softening behavior for a material defined by the Mohr-
Coulomb 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 18.3.3 of the ABAQUS Analysis Users Manual
*MOHR COULOMB
Optional parameter:
DEPENDENCIES
Set this parameter equal to the number of field variable dependencies included in the definition of
the cohesion yield stress, in addition to temperature. If this parameter is omitted, it is assumed
that the cohesion yield stress depends only on the plastic strain and, possibly, on temperature.
See “Specifying field variable dependence” in “Material data definition,” Section 16.1.2 of the
ABAQUS Analysis Users Manual, for more information.
Data lines to define Mohr-Coulomb hardening:
First line:
1. Cohesion yield stress.
2. Absolute value of the corresponding plastic strain. (The first tabular value entered must always
be zero.)
3. Temperature.
4. First field variable.
5. Second field variable.
6. Etc.,uptofivefieldvariables.
Subsequent lines (only needed if the DEPENDENCIES parameter has a value greater than five):
1. Sixth field variable.
13.17–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
13.17–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
There are no parameters associated with this option.
Data lines to define moisture-driven swelling:
First line:
1. Volumetric moisture swelling strain, .
2. Saturation, s. This value must lie in the range .
Repeat this data line as often as necessary to define the srelationship from to in
increasing values of s.
13.18–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
“Defining inflators,” Section 11.6.4 of the ABAQUS Analysis Users Manual
*FLUID BEHAVIOR
*FLUID CAVITY
There are no parameters associated with this option.
Data line to define the molecular weight:
First (and only) line:
1. Molecular weight of the ideal gas species.
13.19–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 4.1.1 of the ABAQUS Analysis Users Manual
Required parameters:
DOF
Set this parameter equal to the degree of freedom to be monitored at the node. In an
ABAQUS/Explicit analysis the degree of freedom will be in the global coordinate system. If
the *TRANSFORM option is used at the node in an ABAQUS/Standard analysis, the degree of
freedom is in the local, transformed, system.
NODE
Set this parameter equal to either the node number to be monitored or the name of a node set
containing the node to be monitored. If the name of a node set is chosen, the node set must contain
exactly one node.
Optional parameter:
FREQUENCY
This parameter applies only to ABAQUS/Standard analyses.
This parameter will only affect output to the message file. Set this parameter equal to the output
frequency in increments. The output will always be printed at the last increment of each step unless
FREQUENCY=0. The default is FREQUENCY=1. Set FREQUENCY=0 to suppress the output.
There are no data lines associated with this option.
13.20–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 32.1.1 of the ABAQUS Analysis Users Manual
“Steady-state transport analysis,” Section 6.4.1 of the ABAQUS Analysis Users Manual
“Static stress analysis,” Section 6.2.2 of the ABAQUS Analysis User’s Manual
“UMOTION,” Section 1.1.34 of the ABAQUS User Subroutines Reference Manual
Required, mutually exclusive parameters:
ROTATION
Include this parameter to define a rigid body rotation about an axis.
TRANSLATION
Include this parameter to give the x-, y-, and z-components of translation in the global coordinate
system or in the local coordinate system if *TRANSFORM was used at these nodes. Translational
motion is the default.
USER
Include this parameter to indicate that magnitudes of motion will be defined in user subroutine
UMOTION. If this parameter is used, any magnitudes defined by the data lines can be redefined in
the user subroutine. The value of the TYPE parameter is not relevant when this parameter is used.
This parameter cannot be used for steady-state transport analysis.
Optional parameters:
AMPLITUDE
Set this parameter equal to the name of the amplitude curve (defined in the *AMPLITUDE option)
that gives the time variation of the motion throughout the step (“Amplitude curves,” Section 27.1.2
of the ABAQUS Analysis Users Manual).
If this parameter is omitted and the translational or rotational motion is given with
TYPE=DISPLACEMENT, the default is a RAMP function. If the translational or rotational motion
13.21–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
Set TYPE=VELOCITY (only type available for steady-state transport and static analysis)
to give translational or rotational velocities. Velocity histories for cavity radiation problems can
be specified as illustrated in the discussion on prescribing large rotations in “Cavity radiation,”
Section 32.1.1 of the ABAQUS Analysis Users Manual.
Data lines to define translational motion (TRANSLATION):
First line:
1. Node set label or node number.
2. First translational component of motion prescribed (only degrees of freedom 1, 2, or 3 can be
entered). See “Conventions,” Section 1.2.2 of the ABAQUS Analysis Users Manual, for a
definition of the numbering of degrees of freedom in ABAQUS.
3. Last translational component of motion prescribed (only degrees of freedom 1, 2, or 3 can be
entered). This field can be left blank if motion for only one component is being prescribed.
4. Magnitude of the translational displacement or velocity. This magnitude will be modified by
the *AMPLITUDE specification if the AMPLITUDE parameter is used.
Repeat this data line as often as necessary to define translational motion for different nodes and degrees
of freedom.
Data lines to define rotational motion (ROTATION):
First line:
1. Node set label or node number.
2. Magnitude of the rotation (in radians) or rotational velocity (in radians/time). This magnitude
will be modified by the *AMPLITUDE specification if the AMPLITUDE parameter is used.
The rotation is about the axis defined from point ato point b, where the coordinates of aand
bare given next. In steady-state transport analysis the position and orientation of the rotation
axis are applied at the beginning of the step and remain fixed during the step.
3. Global x-component of point aon the axis of rotation.
4. Global y-component of point aon the axis of rotation.
13.21–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*MOTION
The following data are required only for three-dimensional cases:
5. Global z-component of point aon the axis of rotation.
6. Global x-component of point bon the axis of rotation.
7. Global y-component of point bon the axis of rotation.
8. Global z-component of point bon 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.
2. First translational component of motion prescribed (only degrees of freedom 1, 2, or 3 can be
entered). See “Conventions,” Section 1.2.2 of the ABAQUS Analysis Users Manual, for a
definition of the numbering of degrees of freedom in ABAQUS.
3. Last translational component of motion prescribed (only degrees of freedom 1, 2, or 3 can be
entered). This field can be left blank if motion for only one component is being prescribed.
4. Magnitude of the translational displacement or rotation. This magnitude can be redefined in
user subroutine UMOTION.
Repeat this data line as often as necessary to define the nodes and degrees of freedom that will have
their motion prescribed by user subroutine UMOTION.
13.21–3
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 Users Manual
“MPC,” Section 1.1.13 of the ABAQUS User Subroutines Reference 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 1.2.1 of the ABAQUS Analysis Users Manual, for the
syntax of such file names. If this parameter is omitted, it is assumed that the data follow the keyword
line.
MODE
This parameter applies only to ABAQUS/Standard analyses.
This parameter is used only if the USER parameter is included.
Set MODE=DOF (default) for user subroutine MPC to operate in a degree of freedom mode.
Set MODE=NODE for user subroutine MPC to operate in a nodal mode.
USER
This parameter applies only to ABAQUS/Standard analyses.
Include this parameter to indicate that the constraint is defined in user subroutine MPC.
Data lines to define multi-point constraints:
First line:
1. MPC type from “General multi-point constraints,” Section 28.2.2 of the ABAQUS Analysis
Users Manual, or, if the USER parameter is included, an integer key to be used in user
subroutine MPC to distinguish between different constraint types.
2. Node numbers or node sets involved in the constraint.
The first 15 nodes or node sets of an MPC must be entered on the first line. If the MPC contains more
than 15 nodes, enter 0 on the next line to indicate that it is a continuation line and then continue to enter
13.22–1
ABAQUS Version 6.1 Module: ID:
Printed on:
*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.
13.22–2
ABAQUS Version 6.1 Module: ID:
Printed on:
*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 17.5.1 of the ABAQUS Analysis User’s Manual
“Hyperelastic behavior in elastomeric foams,” Section 17.5.2 of the ABAQUS Analysis Users Manual
“Mullins effect in rubberlike materials,” Section 17.6.1 of the ABAQUS Analysis Users Manual
“Energy dissipation in elastomeric foams,” Section 17.6.2 of the ABAQUS Analysis Users Manual
“UMULLINS,” Section 1.1.35 of the ABAQUS User Subroutines Reference Manual
*BIAXIAL TEST DATA
*PLANAR TEST DATA
*UNIAXIAL TEST DATA
Optional, mutually exclusive parameters:
TEST DATA INPUT
Include this parameter if the material constants are to be computed by ABAQUS from data taken
from simple tests on a material specimen. If this parameter is omitted in ABAQUS/Standard, the
material constants may be given directly on the data lines or the damage variable may be defined
through user subroutine UMULLINS. If this parameter is omitted in ABAQUS/Explicit, the material
constants must be given directly on the data lines.
USER
This parameter applies only to ABAQUS/Standard analyses.
Include this parameter if the damage variable defining the Mullins effect is defined in user
subroutine UMULLINS.
Optional parameters:
BETA
This parameter can be used only when the TEST DATA INPUT parameter is used; it defines the
value of while the other coefficients of the Mullins effect model are fitted from the test data. It
13.23–1
ABAQUS Version 6.1 Module: ID:
Printed on: