2006 Md Nastran Release Guide

MD Nastran 2006 Release Guide

Corporate MSC.Software Corporation 2 MacArthur Place Santa Ana, CA 92707 USA Telephone: (800) 345-2078 Fax: (714) 784-4056

Europe MSC.Software GmbH Am Moosfeld 13 81829 Munich, Germany Telephone: (49) (89) 43 19 87 0 Fax: (49) (89) 43 61 71 6

Asia Pacific MSC.Software Japan Ltd. Shinjuku First West 8F 23-7 Nishi Shinjuku 1-Chome, Shinjyku-Ku Tokyo 160-0023, JAPAN Telephone: (03)-6911-1200 Fax: (03)-6911-1201

Worldwide Web www.mscsoftware.com

Disclaimer MSC.Software Corporation reserves the right to make changes in specifications and other information contained in this document without prior notice. The concepts, methods, and examples presented in this text are for illustrative and educational purposes only, and are not intended to be exhaustive or to apply to any particular engineering problem or design. MSC.Software Corporation assumes no liability or responsibility to any person or company for direct or indirect damages resulting from the use of any information contained herein. User Documentation: Copyright

 2006 MSC.Software Corporation. Printed in U.S.A. All Rights Reserved.

This notice shall be marked on any reproduction of this documentation, in whole or in part. Any reproduction or distribution of this document, in whole or in part, without the prior written consent of MSC.Software Corporation is prohibited. This software may contain certain third-party software that is protected by copyright and licensed from MSC.Software suppliers. MSC, MSC., MD, MSC.Dytran, MSC.Marc, MSC.Nastran, MD Nastran, MSC.Patran, the MSC.Software corporate logo, and Simulating Reality are trademarks or registered trademarks of the MSC.Software Corporation in the United States and/or other countries. NASTRAN is a registered trademark of NASA. PAMCRASH is a trademark or registered trademark of ESI Group. SAMCEF is a trademark or registered trademark of Samtech SA. LS-DYNA is a trademark or registered trademark of Livermore Software Technology Corporation. ANSYS is a registered trademark of SAS IP, Inc., a wholly owned subsidiary of ANSYS Inc. ABAQUS is a registered trademark of ABAQUS Inc. All other brand names, product names or trademarks belong to their respective owners.

MDNA:V2006:Z:Z:Z:DC-REL-PDF

Contents MD Nastran 2006 Release Guide MD Nastran 2006 Release Guide

List of Nastran Books Technical Support Internet Resources

1

xii xiii xvi

Overview of MD Nastran 2006 Overview 2 Nonlinear Analysis 2 Numerical Enhancements 2 Elements 2 Dynamics and Superelements 3 Aeroelasticity 3 Optimization 4 Summary of MD Nastran Quick Reference Guide Additions 4 List of MD Nastran Documents Released with MD Nastran 2006

2

Table of Contents

7

Nonlinear Analysis Nonlinear Transient Analysis in SOL 400 10 Introduction 10 Benefits 10 Limitations for the Current Release 11 A New Numerical Integration Method – HHT 11 Nonlinear Iteration Algorithms 12 Case Control Structure – SUBCASE, STEP, ANALYSIS, and NLIC 14 Vector Operations and Convergence Criteria 16 Nonlinear Iteration Summary Table for Nonlinear Transient Analysis in SOL 400 17 Output Data Grouping: NLPACK 18 Restarts 19 Initial Conditions 21 Transient Temperature Loads 23 Boundary Condition (SPC and MPC) Changes 24 Direct Matrix Input Changes 24 Outputs 25

iv MD Nastran 2006 Release Guide

Error Handling 25 User Interfaces 26 Examples 27 MD Nastran Implicit Nonlinear - SOL 600 Non-Supported Items 58

44

MD Nastran Explicit Nonlinear - SOL 700 60 Introduction 60 Linear and Nonlinear Analysis 60 Latest Capabilities of MD Nastran Explicit Nonlinear - SOL 700 Example: Projectile Hitting a Plate with Failure 65 Example: Pickup Truck Crash Test 69 Example – 3 Car Crash Simulation 70 Where Can I Find More Information: 71

3

Numerical Enhancements New Iterative Solver Option 74 Introduction 74 Benefits 74 Method and Theory 74 Inputs 75 Outputs 75 Guidelines and Limitations 76 Demonstration Example 76 Example Input Data 76 Example Output 81 MDACMS Enhancements 83 Background 83 Summary 83 New FMS Command: MEMLIST New Module: RESMOD 84 Option P1 = ‘ATBC’ 86 Option P1 = ‘MPART’ 86 Option P1 = ‘LININD’ 87 Option P1 = ‘LDSWEEP’ 88 Option P1 = ‘USWEEP’ 89 MPYAD Method 1 Enhancement Example 90 Problem Definition: 90 Machine Resources 90

83

90

61

Contents v

Improved Robustness in the Lanczos Method MLDMP in Solution 111 (Pre-Release) User Interface 92 Case Study 92

4

91

92

Elements Three-Node Beam Element 96 Introduction 96 Benefits 96 Input 96 Guidelines and Limitations 97 Formulation 99 Output 101 Example 103 CWSEAM Connector Elements 105 Introduction 105 Inputs 105 Error Conditions for the CWELD and CWSEAM Elements 110 Check the Angle and Find Next Candidate Element for CWELD and PARTPAT Format 111 Check the CWSEAM Across a Cutout or Over a Corner with Elements in Plane 111 Check the CWSEAM Over a Corner with Elements Out of Plane 114 Example – A Symmetric Hat Profile (cwseam_hut.dat) 114 Line Interface Element 117 Introduction 117 User Interface 118 Example and Results 123 Arbitrary Beam Cross-Section Introduction 126 Benefits 126 Inputs 126 Output 128 Guidelines 130 Limitations 130 Example 130

126

vi MD Nastran 2006 Release Guide

5

Dynamics and Superelements Efficiency Enhancements to MTRXIN Module for Handling DMIG Data 142 Enhancements to BSETi/BNDFIXi and CSETi/BNDFREEi Bulk Data Entry Processing 143 Enhancements to MATMOD Module Option 16 Introduction 144 Usage 145 Example 145 Enhancements to MATMOD Module 145

144

Enhancements to External Superelement Usage Via EXTSEOUT Case Control Command 149 Introduction 149 Addition of Options to ASMBULK Keyword 149 Addition of New FSCOUP Keyword 150 Addition of New DMIGSFIX Keyword 150 Automatic Numbering Scheme for Q-set DOFs Via AUTOQSET Usage 151 Automatic Availability of Output for Boundary Points and PLOTEL Points of External Superelements in Assembly Run 152 New MATDB Option As Equivalent to Current MATRIXDB Option 152 Changes to Rotordynamic for MD Nastran 2006 153 Additional Damping Options for Rotors 153 Squeeze Film Damper as Nonlinear Force 158 Squeeze Film Damper as Nonlinear Element 159 Gyroscopic Terms Added to Aero Solution Sequences 161 Campbell Diagrams 161 Rotor Forward and Backward Mode Identification 162 Rotor Mode Tracking 165 Comments 165 Modified Basic Equations Used in Rotordynamics 166 Frequency Response 167 Complex Modes 169 Nonlinear Transient Response 171 Exterior Acoustics 172 Introduction 172 Benefits 172 Input 172 Definition of Infinite Elements 172 Definition of Field Point Meshes 175 Example 175

Contents vii

Case Control Commands 176 Output 179 Guidelines 179 Limitations 180 Example 180 Input File 182 Excerpt of fluid1.bdf 183 Results 184

6

Aeroelasticity Monitor Points 188 Introduction 188 Benefits 189 Input 189 Output 190 Examples 193 Guidelines and Limitations

193

Spline6/7 195 Introduction 195 Benefits 196 Input 196 Combination of Controllers/User Input Loads Enhancements 197 Introduction 197 Benefits 197 Input/Output 198 Guidelines and Limitations 198 Examples (aelinka.dat, aelinkb.dat,i3fusa.dat,aepload4.dat,fusae.dat) 198 Separate Rigid and Flexible Aero Meshes Introduction 199 Benefits 199 Input 199 Output 199

199

Miscellaneous Aeroelastic Enhancements 201 Revision in the Aerodynamic Splining to the Structure Flutter Analysis with Singular Mass Matrices 201

7

201

Optimization Topology Optimization with Manufacturability Constraints

204

viii MD Nastran 2006 Release Guide

Introduction 204 Benefits 204 Input 205 Guidelines and Limitations

207

Example 1 – MBB Beam Baseline (topex3.dat)

209

Example 2 - MBB Beam with Minimum Member Size (topex3a.dat)

211

Example 3 - MBB Beam with Symmetric Constraints (topex3b.dat)

212

Example 4 - A Torsion Beam with Extrusion Constraints (topex5.dat) 214 Example 5 - A Torsion Beam with One Die Casting Constraints (topex5a.dat) 216 Example 6 - A Torsion Beam with Two Die Casting Constraints (topex5b.dat) 218 Revised Optimizer Options 220 Introduction 220 Benefits 220 Input 220 Output 222 Guidelines and Limitations 222 Supporting Trust Region in SOL 200 for Adaptive Move Limits Introduction 223 Benefits 223 Theory 223 Input 225 Outputs 226 Guidelines and Limitations 227 Examples 227 Support of Analysis Model Value Overriding Design Model Value Introduction 230 Benefits 230 Input 230 Output 230 Example 230 Guidelines and Limitations 231

223

230

Contents ix

8

Miscellaneous Enhancements Export of Static Loads 234 Introduction 234 Benefits 234 Input 234 Output 235 Examples (TPL: exptld/imptld, sysmod/fbody, sfsw/ffsw) Guidelines and Limitations 236 Enhanced Participation Factor Results Introduction 237 Theory 238 Input 240 Examples 240 Example 241 Example 241 Output 242 Example 243 Guidelines 243 Limitations 244 Example 244 Input Data 244

235

237

Total Strain Energy Output for Defined SETs Introduction 249 Inputs 249 Formats 249 Examples 249 Example 250 Output Example 251

249

Model Checkout Procedures - Method to Vary Material Properties Introduction 252 Benefits 252 Method and Theory 252 Inputs 252 Outputs 253 Guidelines and Limitations 253 Demonstration Example 253 Example Input Data 253 Example Output 258

252

x MD Nastran 2006 Release Guide

MD Nastran 2006 Release Guide

Preface

■ List of Nastran Books ■ Technical Support ■ Internet Resources

xii MD Nastran 2006 Release Guide

List of Nastran Books Below is a list of some of the Nastran documents. You may order any of these documents from the MSC.Software BooksMart site at www.engineering-e.com. Installation and Release Guides ❏ Installation and Operations Guide ❏ Release Guide

Reference Books ❏ Quick Reference Guide ❏ DMAP Programmer’s Guide ❏ Reference Manual

User’s Guides ❏ Getting Started ❏ Linear Static Analysis ❏ Basic Dynamic Analysis ❏ Advanced Dynamic Analysis ❏ Design Sensitivity and Optimization ❏ Thermal Analysis ❏ Numerical Methods ❏ Aeroelastic Analysis ❏ Superelement ❏ User Modifiable ❏ Toolkit ❏ Implicit Nonlinear (SOL 600) ❏ Explicit Nonlinear (SOL 700)

Preface xiii

Technical Support For help with installing or using an MSC.Software product, contact your local technical support services. Our technical support provides the following services:

• Resolution of installation problems • Advice on specific analysis capabilities • Advice on modeling techniques • Resolution of specific analysis problems (e.g., fatal messages) • Verification of code error. If you have concerns about an analysis, we suggest that you contact us at an early stage. You can reach technical support services on the web, by telephone, or e-mail: Web

Go to the MSC.Software website at www.mscsoftware.com, and click on Support. Here, you can find a wide variety of support resources including application examples, technical application notes, available training courses, and documentation updates at the MSC.Software Training, Technical Support, and Documentation web page.

xiv MD Nastran 2006 Release Guide

Phone and Fax

United States Telephone: (800) 732-7284 Fax: (714) 784-4343

Frimley, Camberley Surrey, United Kingdom Telephone: (44) (1276) 60 19 00 Fax: (44) (1276) 69 11 11

Munich, Germany Telephone: (49) (89) 43 19 87 0 Fax: (49) (89) 43 61 71 6

Tokyo, Japan Telephone: (81) (03) 6911 1200 Fax: (81) (03) 6911 1201

Rome, Italy Telephone: (390) (6) 5 91 64 50 Fax: (390) (6) 5 91 25 05

Paris, France Telephone: (33) (1) 69 36 69 36 Fax: (33) (1) 69 36 45 17

Moscow, Russia Telephone: (7) (095) 236 6177 Fax: (7) (095) 236 9762

Gouda, The Netherlands Telephone: (31) (18) 2543700 Fax: (31) (18) 2543707 Madrid, Spain Telephone: (34) (91) 5560919 Fax: (34) (91) 5567280

Email

Send a detailed description of the problem to the email address below that corresponds to the product you are using. You should receive an acknowledgement that your message was received, followed by an email from one of our Technical Support Engineers. MSC.Patran Support MSC.Nastran Support MSC.Nastran for Windows Support MSC.visualNastran Desktop 2D Support MSC.visualNastran Desktop 4D Support MSC.Dytran Support MSC.Fatigue Support MSC.Interactive Physics Support MSC.Marc Support MSC.Mvision Support MSC.SuperForge Support MSC Institute Course Information

[email protected] [email protected] [email protected] [email protected] [email protected] [email protected] [email protected] [email protected] [email protected] [email protected] [email protected] [email protected]

Preface xv

Training The MSC Institute of Technology is the world's largest global supplier of CAD/CAM/CAE/PDM training products and services for the product design, analysis and manufacturing market. We offer over 100 courses through a global network of education centers. The Institute is uniquely positioned to optimize your investment in design and simulation software tools. Our industry experienced expert staff is available to customize our course offerings to meet your unique training requirements. For the most effective training, The Institute also offers many of our courses at our customer's facilities. The MSC Institute of Technology is located at: 2 MacArthur Place Santa Ana, CA 92707 Phone: (800) 732-7211 Fax: (714) 784-4028 The Institute maintains state-of-the-art classroom facilities and individual computer graphics laboratories at training centers throughout the world. All of our courses emphasize hands-on computer laboratory work to facility skills development. We specialize in customized training based on our evaluation of your design and simulation processes, which yields courses that are geared to your business. In addition to traditional instructor-led classes, we also offer video and DVD courses, interactive multimedia training, web-based training, and a specialized instructor's program. Course Information and Registration. For detailed course descriptions, schedule information, and registration call the Training Specialist at (800) 732-7211 or visit www.mscsoftware.com.

xvi MD Nastran 2006 Release Guide

Internet Resources MSC.Software (www.mscsoftware.com) MSC.Software corporate site with information on the latest events, products and services for the CAD/CAE/CAM marketplace. Simulation Center (simulate.engineering-e.com) Simulate Online. The Simulation Center provides all your simulation, FEA, and other engineering tools over the Internet. Engineering-e.com (www.engineering-e.com) Engineering-e.com is the first virtual marketplace where clients can find engineering expertise, and engineers can find the goods and services they need to do their job CATIASOURCE (plm.mscsoftware.com) Your SOURCE for Total Product Lifecycle Management Solutions.

MD Nastran Release Guide Ch. 1: Overview of MD Nastran 2006 Ch. 1: Overview of MD Nastran 2006Key Highlights for MD

1

Overview of MD Nastran 2006

J

Nastran 2006

Overview

2 MD Nastran 2006 Release Guide

Overview The MD Nastran 2006 release brings major new features for enterprise computing in the areas of high performance computing, nonlinear analysis, assembly modeling, optimization, rotor dynamics and aeroelasticity.

Nonlinear Analysis • Nonlinear Transient Analysis in SOL 400 - Nonlinear transient (SOL 400) extends the nonlinear

analysis capabilities of SOL 129. It features a new transient analysis solution (HHT method), adaptive time step control, SPC and MPC changes between Subcase/Step, improved nonlinear iteration performance, the new nonlinear squeeze film damper element for rotor dynamics, and expanded nonlinear iteration controls. • MD Nastran Implicit Nonlinear - SOL 600 – The performance and capabilities of MD Nastran’s

implicit nonlinear solution have been greatly improved over MSC.Nastran. These include more robust data exchange, faster contact (three to six-fold CPU time improvements), auto SPC and MSET, inertia relief, an improved out-of-core solver, expanded results support, automated brake squeal computations, improved fixed time stepping, and improved user subroutine support. • MD Nastran Explicit Nonlinear - SOL 700 – With this new release capability you can perform

crash and drop test analysis using existing Nastran models.

Numerical Enhancements • Iterative Solvers – There is now a new iterative solution for static analysis. Also, significant

performance improvements along with reduction in I/O requirements have been achieved in the ACMS solution.

Elements • Arbitrary Beam Cross-Section – The interface for describing arbitrary cross-section shapes for

bar and beam elements has been enhanced to include a cross-section outline display, stress data recovery and design optimization. The profiles can now be optimized using SOL 200. Stress recovery includes both torsion and shear terms. • Line Interface Element – You can now connect dissimilar meshes along edges. A set of MPC

(multipoint constraint) equations are internally generated to enforce the compatibility of displacements and rotations across the interface. This feature is particularly useful for globallocal modeling, where a local fine mesh is required in a particular region due to high stress gradients. • CWSEAM Connector Elements

CWSEAM Element - A seam element to connect surface patches is now available. This element extends the existing CWELD and CFAST connector elements. The seam weld is defined by selecting two surface patches by their property IDs and specifying the width and the thickness of

CHAPTER 1 3 Overview of MD Nastran 2006

the seam. Extensive error checking and user diagnostics include detection of missing connections for CWSEAMs, defined across corners and cutouts. RBE2GS Element – This element generates internal RBE2 element connecting a grid point pair closest to a user-defined search grid point. You can exclude optional grids within search radius. • Three-Node Beam Element – A general spatial three-node beam element has been developed for

linear static, modal, dynamic, and buckling analyses. The element is implemented as a curved one-dimensional Timoshenko beam element with initial curvatures and pre-twist. The crosssectional warping effect is also included.

Dynamics and Superelements • Rotor Dynamics – In the MD Nastran release we introduce a new general displacement and

speed dependent nonlinear element for rotor bearings and a nonlinear squeeze film damper element. Also, we support the gyroscopic terms in aero solution sequences, non-linear harmonic response, and an easier Campbell diagram to identify rotor modes and track across subcases. • Enhancements to External Superelement Usage Via EXTSEOUT Case Control Command –

Several improvements have been made to external superelement (SE) usage employing the EXTSEOUT feature with a view to enhancing user convenience and flexibility. These include, the ability to: (a) specify suffixes for DMIG matrices resulting from the use of the DMIGPCH option, (b) get output for the boundary points and PLOTEL points of an external SE in the assembly run regardless of the output requests in the external SE creation run, and (c) have control over the Q-set or generalized degrees of freedom (DOFs) of an external SE in the assembly run.

Aeroelasticity • Monitor Points - We have added support for monitor points, including a MONPNT2 that selects

a specific element response for output, a MONPNT3 that outputs an integrated load on a structural subcomponent, and a MONDSP1 that provides averaged displacement components. All of these are available in SOLs 101 and 144, while SOL 146 supports MONPNT1 and MONDSP1. • Export and Import of Loads -Two methods have been provided to extract loads from an analysis

for import into another analysis. The EXPORTLD Case Control command supports the creation of a datablock that contains the external load of a user specified set of grids. Alternatively, one can export a “free-body” load based on the grid point forces of a user specified subcomponent. Both of these loads can be imported into a subsequent analysis via dblocate commands, and included in the external load specification.

4 MD Nastran 2006 Release Guide

Optimization • Topology Optimization with Manufacturability Constraints – This release supports

manufacturing constraints including casting (draw direction), extruding, and symmetry to ensure that the optimal size and shape determined for the given set of loads and boundary conditions conforms to manufacturing.

Summary of MD Nastran Quick Reference Guide Additions Additions to the MD Nastran Quick Reference Guide to accommodate developments, improvements, and added functionality for MD Nastran 2006 are substantial. The following tables categorize these changes according to the section of the QRG affected.

Input Changes Section

New

Executive Control

Modified NASTRAN

nastran Statement MODEL_CHECK

SOL 600,ID SOL 700,ID

CHAPTER 1 5 Overview of MD Nastran 2006

Input Changes Section

New

Modified

Case Control

AERCONFIG EXPORTLD FBODYLD MONITOR

PFGRID PFMODE PFPANEL SETP BCONTACT DEFAULT * ENDTIME *

ADAMSMNF BCONTACT EXTSEOUT DRSPAN

Bulk Data

ACC ACCMETR BCBODY BCBOX BCGRID * BCMATL BCPARA BCPROP BCSEG * BCTABLE BJOIN BRKSQL# BSURF CBEAM3 CBELT * CBUTT * CCRSFIL * CDAMP1D * CDAMP2D * CELAS1D * CELAS2D * CFILLET * CINTC COMBWLD * CORD1RX CORD2RX CORD3RX CORD3R * CSPOT * CSPR CWSEAM D2R0000* D2RAUTO* D2RINER* DAMPGBL * DYCHANG* DYDELEM* DYPARAM * DYRELAX* DYRIGSW * DYTERMT* DYTIMHS * ENDDYNA*

EOSPOL * FBODYLD FBODYSBE GBAG MATD001 * MATD2AN * MATD2OR * MATD003 * MATD005 MATD006 * MATD007 * MATD009 MATD010 * MATD012 * MATD013 * MATD014 * MATD015 * MATD018 * MATD019 * MATD020 * MATD20M * MATD022 * MATD024 * MATD026 * MATD027 * MATD028 * MATD030 * MATD031 * MATD032 * MATD054 * MATD057 * MATD058 * MATD059 * MATD062 * MATD063 * MATD064 * MATD066 * MATD067 * MATD068 * MATD069 * MATD070 * MATD071 * MATD073 *

AEFORCE AELINK BCPROP#* BCTABLE#* BNDFIX BNDFIX1 BNDFREE BNDFREE1 BSET BSET1 BSURF#* CELAS2D DESVAR DRESP1 IPSTRAIN# ISTRESS# ITER MATD126 MATHED# MATORT# MBOLTUS# NLSTRAT# PBARL PCONV RESTART#* TSTEPNL

6 MD Nastran 2006 Release Guide

Input Changes Section Bulk Data

New MATD074 * MATD076 * MATD077 * MATD080 * MATD081 * MATD083 * MATD087 * MATD093 * MATD094 * MATD095 * MATD097 * MATD100 * MATD119 * MATD121 * MATD126 * MATD127 * MATD181 * MATDB01 * MATDS01 MATDS02 MATDS03 * MATDS04 * MATDS05 * MATDS06 * MATDS07 * MATDS08 * MATDS13 * MATDS14 * MATDS15 * MATF MATRIG MONDSP1 MONPNT1 MONPNT2 MONPNT3 PBEAM3 PBEAM71 * + PBEAMD PBELTD * PCOMPA * PELAS1*

PLOADB3 PSHELL1 * PSHELLD PSOLIDD * PSPRMAT PWSEAM RBE2A RBE2D RBE2F * RBE3D * RBJOINT * RCONN * RESTART SBPRET * SBRETR * SBSENSR * SBSLPR * SPCD2 * SPLINE6 SPLINE7 SUPORT6# SWLDPRM TABLEDR * TEMPB3 TICD * TIC3 * TMPSET TODYNA* TTEMP USRSUB6# WALL * WALLGEO

Modified

CHAPTER 1 7 Overview of MD Nastran 2006

Input Changes Section Parameters

New CWLDIGNR* DYDTOUT,DT* DYDYLOAD* DYELAS1C,* DYELAS1F,* DYELAS1R,* DYELPLET,* DYELPLFL,* DYELPLSY,* DYSTEPFCT,,# HEATCMD# MARCBATCH# MARCBUSH# MARCITER#

MARCCBAR#* MARCRCID# MARGPFOR# MEXTRNOD# MLSTRAIN# MRBEPARM,# MRCOMPOS# MRCONVER# MRPSHELL# MSPEEDOU# SCALEMAS,* STEPFCT*

Modified MARCAUTO# MARCOTIM# MARCPINN# MARCPOST# MARCRBE3# MARCSAME# MARCSLHT#

MARCSOLV# MARCUSUB# MRESTALL# MRMAXMEM# MRSPAWN2# MRSPEEDSE# MRTABLS2# MRTABLS1#

Items with a pound sign (#) next to them are only available for MD Nastran Implicit Nonlinear (SOL 600). Items with an asterisk (*) sign next to them are only available for MD Nastran Explicit Nonlinear (SOL 700). See the individual parameter for further details. + PBEAM71 has three alternates, please see the MD Nastran Quick Reference Guide for more information.

List of MD Nastran Documents Released with MD Nastran 2006 Along with this Guide, the following documents are updated for the MD Nastran 2006 release. MD Nastran 2006 Quick Reference Guide MD Nastran 2006 Installation and Operation’s Guide MD Nastran 2006 Implicit Nonlinear (SOL 600) User’s Guide MD Nastran 2006 Explicit Nonlinear (SOL 700) User’s Guide

8 MD Nastran 2006 Release Guide

MD Nastran 2006 Release Guide + Ch. : h0title Ch. 2: Nonlinear Analysis Ch. 2: Nonlinear Analysis

2

Nonlinear Analysis

J

Nonlinear Transient Analysis in SOL 400, 10

J

MD Nastran Implicit Nonlinear - SOL 600, 44

J

MD Nastran Explicit Nonlinear - SOL 700, 60

10 MD Nastran 2006 Release Guide

Nonlinear Transient Analysis in SOL 400 Introduction Nonlinear transient analysis in SOL 400 improves the general nonlinear solution procedure in MD Nastran. It allows most linear files to be run in a nonlinear analysis environment, and includes the nonlinear solution types: • SOL 106, nonlinear static analysis (Prerelease) • SOL 129, nonlinear transient analysis • Rotor Dynamics

It will eventually include: • SOL 153, steady heat transfer • SOL 159, nonlinear heat transfer • Nonlinear normal modes analysis • Nonlinear buckling analysis

Different types of nonlinear analysis can now talk to each other in a meaningful physical sequence. For the MD Nastran 2006 release, nonlinear transient analysis is now considered a product release for SOL 400. However, the nonlinear static analysis still remains a pre-release. In this release guide, all items pertaining to the nonlinear transient analysis are discussed. For nonlinear static analysis, only items pertaining to the transient analysis are discussed. These include the SUBCASE and STEP Case Control command and the static pre-loads.

Benefits The benefits of the nonlinear transient analysis in SOL 400 are discussed in this section. Some of the benefits may be subject to the limitation discussed in next section. The benefits are: • A new transient solution integration method, the HHT (Hilbert-Hughes-Taylor) method, to give

stable transient solution. • Improved nonlinear iteration algorithms to make the solution easier and faster to converge.

These includes ADAPT, AUTO, ITER, and SEMI methods. • A new SUBCASE and STEP case control structure allows flexible loading and solution

sequences. Different nonlinear analysis types can now communicate with each other in a meaningful physical sequence in a SUBCASE. • A new comprehensive nonlinear summary table for the transient analysis. • Support of the initial conditions (IC). • A new control command NLIC allows any previous converged nonlinear static solution as the

preload for the first nonlinear transient step.

CHAPTER 2 11 Nonlinear Analysis

• The boundary conditions SPC and MPC can change between load steps. • Direct matrix input, such as K2PP, M2PP, B2PP, and TFL, can change between load steps. • Support for “grid based reordering” for a faster version of decomposition for time step size

change and stiffness update in the nonlinear iterations. • Support the nonlinear thermal loads in the transient analysis. Two new Bulk Data entries,

TTEMP and TMPSET, have been added for this new feature in the nonlinear transient analysis. • Support for rotor dynamics in the nonlinear transient analysis. • A user-friendly restart procedure introduced earlier is available to nonlinear transient analysis. • A more flexible output method for the nonlinear transient analysis. You can use a new

parameter NLPACK to control the output and restart time steps. • Solution output at requested time points. Also, allows the simulation of the same output logic

and format of SOL 129 by specifying a negative NO on the TSTEPNL Bulk Data entry. • Supports linear superelements. • Supports the XDB database for communicating with a post processor, such as MSC.Patran. • The OTIME output request is supported (except NLSTRESS).

Limitations for the Current Release The following are limitations for the current release of the nonlinear transient analysis. • RFORCE – RFORCE was supported in old SOL 99. In SOL 129, the RFORCE must be used in

conjunction with an old SOL 99 iteration method. In this release of SOL 400, RFORCE is not supported. • Omitted degrees-of-freedom (o-set). • Slide line contacts. • The XDB database is not supported for restarts. XDB can be used only for non-restart cases in

SOL 400 to communicate with post-processors such as MSC.Patran. For restart cases, use OP2 instead. • For SOL 400 nonlinear transient analysis, the Case Control command RIGID=LINEAR is set

automatically by MD Nastran. These limitations will be addressed in a future release.

A New Numerical Integration Method – HHT To solve the equation of motion for a nonlinear transient analysis, two aspects must be resolved. The first is how to integrate the equation of motion for the transient analysis and second is how to obtain an equilibrium solution for the nonlinear analysis. This section discusses the numerical integration of the equation of motion and the next section will discuss the nonlinear iteration methods for obtaining the balanced solution.

12 MD Nastran 2006 Release Guide

For numerical integration, the second order HHT (Hilbert-Hughes-Taylor) method is used in nonlinear transient analysis in SOL 400. It provides a user-definable parameter α, which defines a numerical damping associated with higher frequency modes, but also maintains the accuracy in the essential lower frequency modes. Since it is a key feature of the HHT method, it is sometimes called the HHT-α method. When α < 0 , numerical damping is introduced into the system. This leads to an unconditionally stable integration time scheme when it is in the following range 1 – --- ≤ α ≤ 0 3 When comparing with other numerical damping methods even at α = – 1 ⁄ 3 (the maximum numerical damping value), the HHT method still introduces less damping. Therefore, the solution is more accurate theoretically. Note that when α = 0 , this method is equivalent to the central finite difference method. The numerical damping, α , can be specified using parameter NDAMP (default is -0.05 in SOL 400). Parameter NDAMP is used in Example 1 and Example 7.

Nonlinear Iteration Algorithms This section discusses the nonlinear iteration algorithm used in SOL 400 to obtain an equilibrium solution for the nonlinear transient analysis. In SOL 400, the equilibrium solution is achieved by a combination of the following methods: • Time step size adjustment – At the beginning of a SUBCASE or at the convergence of a time

step, the time step size is adjusted based on the estimated current natural frequency of the structural model or the input loads. • Load iteration – At each time step, the quasi Newton method and line search technique are

employed repeatedly to obtain the balance of internal forces and external loads. This is called the load iteration or simply the iteration. The time step is converged when the balance of internal forces and external loads is obtained. You can deselect the quasi Newton method or the line search by using parameter in the TSTEPNL Bulk Data entry. When the quasi Newton method is deselected, the solution scheme becomes the modified Newton method. • Stiffness update – In many situations, the load iteration will not be able to achieve equilibrium at

a time step. In this situation, the stiffness matrix can be recomputed using the current geometric and material state of the structure model to facilitate convergence. This is called the stiffness update. Consecutive stiffness updates without load iteration is called the full Newton method. • Bisection – When the program reads that it is impossible for the solution to converge, a

procedure called divergence processing is employed. One technique used in this procedure is bisection. Bisection means cutting the time step size or load increment size by half. Divergence processing uses a combination of stiffness updates and bisections to facilitate convergence. Externally, bisection and time step adjustment are similar. However, they are initiated due to different reasons. Time step adjustment is based on the requirement of the natural frequency of the structure, which may or may not be nonlinear. Bisection is, on the other hand, due to large nonlinearity in the solution.

CHAPTER 2 13 Nonlinear Analysis

Another difference is that the time step adjustment is performed at the beginning of a SUBCASE or at a converged time step. Bisection is performed during a time step when the program determines that the solution is diverging. When the program determines that the large nonlinearity is gone and the solution is stabilized toward convergence, reversal of the bisection is performed in order to maintain the time step size required by the time step adjustment method given above. The METHOD field on the TSTEPNL Bulk Data entry selects the nonlinear iteration method. There are four options available. • ADAPT – The convergence of a time step is obtained chiefly by the time step adjustment and

the load iteration. No stiffness update is performed during the normal iteration. Stiffness updates are performed only for divergent processing and at solution convergence of a time step with number of iterations greater than 3*MAXITR. MAXITR is the maximum number of iterations given on the TSTEPNL Bulk Data entry. Even for divergence processing, the main method to correct the divergence is bisection. • AUTO – The convergence of a time step is achieved by automatically selecting the load

iterations and the stiffness updates, in combination with the ADAPT method. The ADAPT method can be deselected by setting ADJUST=0 on the TSTEPNL Bulk Data entry. This is the default method. For divergence processing, the divergence is corrected by a combination of stiffness updates and bisections. The AUTO method always tries to maintain the time step size required by the time step adjustment method. • ITER – The convergence of a time step is achieved by performing a stiffness update at every

KSTEP load iterations, in combination with the ADAPT method. Again, the ADAPT method can be deselected by setting ADJUST=0. When KSTEP=1, this is the full Newton method. The divergence processing is the same as that of the AUTO method. • SEMI – Same as the AUTO method, except that a stiffness update is performed at first iteration

of a new time step. A stiffness update is always performed at convergence of a STEP, irrespective of the option selected. AUTO and ADAPT are two major methods in SOL 400. The AUTO method tries to maintain the time step size required by the time adjustment method or the user time step. The ADAPT method usually converges with a time step size smaller than the time step required by the time step adjustment method or the user time step. For most problems, AUTO method gives better solutions; therefore, it is selected as the default method. However, if the time step estimated by the time step adjustment method or the user time step is too large, the ADAPT method gives a better solution. A better solution here means that the solution converges faster or does not diverge. The DT and NO fields on the TSTEPNL Bulk Data entry need more explanation here. The DT field defines the user time step size. NO, which may be positive or negative, defines that, at every |NO| time steps, the results are saved for output. Since both time step size adjustment and bisection may modify the time step size, options are given to select whether to output at user time step size DT or at internally computed time step size, as shown in the following:

14 MD Nastran 2006 Release Guide

If NO > 0, the output will be at the user time step size or multiples of the user time step size. Also, the time step size computed by the time step adjustment will never be greater than the user time step size DT. For default, NO = 1. If NO < 0, the output will be at the internally computed time step size, which may or may not be at the user time point determined by DT. Also, the time step size computed by the time step adjustment can be either greater or less than the use time step size DT.

Case Control Structure – SUBCASE, STEP, ANALYSIS, and NLIC The STEP command has been expanded to support nonlinear transient analysis for SOL 400 only. You can specify the type of analysis for each SUBCASE and STEP by using the Case Control command ANALYSIS. ANALYSIS supports three keywords for SOL 400. LNSTATIC, NLSTATIC (the default), and NLTRAN. A new Case Control command, NLIC is also introduced in this version. It selects the initial condition from a previous static analysis. The combination of SUBCASE, STEP, ANALYSIS, and NLIC commands provide a mechanism for defining the multiple load steps, running multiple independent cases, and specifying multiple (and mixed) types of analyses in one job. The following examples illustrate the manner in which the SUBCASE, STEP, and ANALYSIS commands are used. • With one SUBCASE and multiple steps, each step defines the total new external load and other

characteristics for the step, which will be applied by the completion of the step. The solution of any STEP is a continuation of the solution of its previous STEP. The following is a typical example. SUBCASE 1 ANALYSIS = NLTRAN TSTEPNL = 200 STEP 10 DLOAD = 10 STEP 20 DLOAD = 20 STEP 30 DLOAD = 30

$ This line can be omitted

• Multiple SUBCASEs may be executed in one job where the types of analysis, loads and

boundary conditions can be changed. All SUBCASEs are independent of each other, i.e., no load history information is transmitted from one SUBCASE to the next. At the start of each SUBCASE, the deflections, stresses and strains throughout the model are zero. For example: SUBCASE 1 ANALYSIS = NLSTAT NLPARM = 100 STEP 110 LOAD = 110 STEP 120 LOAD = 120

$ This line can be omitted

CHAPTER 2 15 Nonlinear Analysis

SUBCASE 2 ANALYSIS = NLTRAN TSTEPNL = 200 STEP 210 DLOAD = 210 STEP 220 DLOAD = 220 • In the above example, the solutions of SUBCASE 1 and SUBCASE 2 are independent of each other. If solution divergence is detected in a step, MD Nastran will terminate the solution of the current subcase and jump to the next subcase if it exits. • A case control command placed below the step level allows that command to vary from one step

to another. If it is placed above the step level, the command remains constant for all steps in the subcase. Most of the case control commands, which can be placed below the subcase level, can also placed below the step level. For example, all steps in above examples use the same Case Control command NLPARM = 100 in SUBCASE 1 and TSTEPNL = 200 in SUBCASE 2. • The SOL 400 uses an enhanced dynamic solution algorithm that makes the linear static solution

and the nonlinear static solution special cases of the general nonlinear solution procedure. For example: SUBCASE 10 STEP 1 ANALYSIS = LNSTATIC LOAD = 10 STEP 2 ANALYSIS = NLSTATIC LOAD = 20 NLPARM = 20 In above example, SUBCASE 10 has two steps. The first step requests a linear static analysis and the second step requests a nonlinear static analysis. • In the MD Nastran release, NLSTATIC and NLTRAN analyses can be mixed in a single

SUBCASE. For example: SUBCASE 10 STEP 1 ANALYSIS = NLSTAT LOAD = 10 NLAPRM = 110 STEP 2 ANALYSIS = NLSTAT LOAD = 20 NLPARM = 120 STEP 3 ANALYSIS = NLTRAN DLOAD = 30 TSTEPNL = 130

16 MD Nastran 2006 Release Guide

In the above example, SUBCASE 10 has three steps. The first two request a nonlinear static analysis and the third requests a nonlinear transient analysis. Since there is no NLIC request in the third step, the final result of the second step automatically becomes the initial condition of the third step. Note that in one SUBCASE, all steps of NLSTAT must come before the STEPs of NLTRAN. • The meaning of multiple SUBCASEs without STEP is dependent on the system cell NASTRAN

SYSTEM (366), as follows: • 0 - The solutions of all SUBCASE are independent of each other. This is consistent with the

new SOL 400 procedure. MD Nastran will keep all SUBCASE commands in the Case Control file and insert internally a “STEP 1” for each SUBCASE. • 1 - The solution of each SUBCASE is a continuation of the previous SUBCASE. This is

similar to the solution sequence SOL 129 procedure. MD Nastran will convert internally all the SUBCASE identification number to STEP identification number and insert a “SUBCASE 1” before the first STEP. The default is 0. Both SUBCASE and STEP are used in Examples 1, 2, 3, 4, 5, 7, and 8. SUBCASE only is used in Example 9. No SUBCASE and no STEP are used in Example 6.

Vector Operations and Convergence Criteria The convergence criteria are specified using the Bulk Data entry TSTEPNL in the nonlinear transient analysis. In performing the convergence tests, three error factors are computed: the displacement, the load, and the work (energy) error factors, which are printed in the Nonlinear Iteration Summary Table. These three error factors must satisfy the error tolerance rules specified by CONV, EPSU, EPSP, and EPSW on the Bulk Date entry TSTEPNL. In computing the error factors, SOL 129 used the d-set vectors for displacements and forces. By using this method, the effect of SPC loads and MPC constraints are accounted for only indirectly. Also, there are difficulties to account for the effect of Lagrange multipliers for the Lagrange rigid elements. For these reasons, in SOL 400, whenever possible, the matrix and vector operations, which include the computations of error factors, are performed in p-set (the physical set). For MD Nastran set definition, refer to the Degree-of-Freedom Set Definitions (p. 940) in the MD Nastran Quick Reference Guide. Another major modification is the computation of the work error. In SOL 129, the work error is based on the multiplication of the residual force and the displacement change. During iteration, both the residual force and the displacement change become smaller; therefore, the convergence rate of this value is proportional to the square of the convergence rate of the solution. Thus it becomes very small near convergence. Also, it does not have a counter part in the physical world. In SOL 400, the total work done to the structure model is computed at each iteration and the work error is estimated based on the total work. In this way, the work error gives an estimation of the error in the actual work done to the structural model. The total work for each iteration is printed on the Nonlinear Iteration Summary Table. Please note that this total work is only an approximation.

CHAPTER 2 17 Nonlinear Analysis

Nonlinear Iteration Summary Table for Nonlinear Transient Analysis in SOL 400 In order to track the solution sequence during the nonlinear iteration, a detailed Nonlinear Iteration Summary Table is output. A line for each iteration is output on the F06 file. Printing of the average and the maximum displacements allows you to know the solution status before the end of the job. This is useful for large nonlinear problems. Even for small problems, you will be able to know approximately how the analysis of a structural model is performing by examining this table. An example of this table is given below.

0

N O N - L I N E A R STIFFNESS UPDATE TIME ITERATION TIME TIME

1.10800E-02 1.10900E-02 1.11000E-02 1.11100E-02 1.11200E-02

I T E R A T I O N

0 0 0 0 0

1.0000 1.0000 1.0000 1.0000 1.0000

O U T P U T SUBCASE

- TIME STEP - - ERROR FACTORS - NO. BIS ADJUST ITR DISP LOAD WORK 1108 1109 1110 1111 1112

M O D U L E

0.01 SECONDS 0.00 SECONDS

2 2 2 2 2

8.58E-07 8.81E-07 9.02E-07 9.21E-07 9.40E-07

Table 2-1

3.52E-03 3.65E-03 3.77E-03 3.89E-03 4.01E-03

2.40E-08 2.25E-08 2.07E-08 1.88E-08 1.66E-08

CONV ITR MAT AVG RATE DIV DIV R_FORCE 0.01 0.01 0.01 0.01 0.01

0 0 0 0 0

1 1 1 1 1

6.6E+01 6.8E+01 7.0E+01 7.2E+01 7.4E+01

TOTL WORK 3.451E+00 3.462E+00 3.473E+00 3.484E+00 3.495E+00

1

STEP

1

- - - - - DISP - - - - - - NO. TOT TOT AVG MAX AT GRID C QNV KUD ITR 1.61E-03 1.61E-03 1.61E-03 1.61E-03 1.62E-03

-8.120E-03 -8.134E-03 -8.147E-03 -8.160E-03 -8.173E-03

103 103 103 103 103

3 3 3 3 3

7 7 7 7 7

0 0 0 0 0

2202 2204 2206 2208 2210

Information in Nonlinear Iteration Summary Table

TIME

The Current Time. Starts from 0.0 at the beginning of the 1st STEP and accumulate the value until at the end of the last STEP. For each STEP, the total time is determined by NDT and DT on TSTEPNL Bulk Data entry.

TIME STEP NO

Number of time step, including bisection. Initialized to 0 in the beginning of each STEP.

TIME STEP BIS

Number of bisections performed.

TIME STEP ADJUST

The ratio of the current time increment to the original DT on TSTEPNL Bulk Data entry.

ITR

Number of iteration at each time increment.

ERROR FACTORS: DISP LOAD WORK

There are three error factors: displacement, load, and works. In order for an increment to converge, these factors must satisfy the error tolerance rules specified by CONV, EPSU, EPSP, and EPSP on the TSTEPNL Bulk Data entry.

CONV RATE

Converge rate, which denote how fast the solution converges for the current increment. A value of 0.0 means fast converges and a value > 1.0 means that the solution will never converge.

ITR DIV

Number of iteration divergences. Action to correction solution divergence will be taken if ITRDIV > MAXDIV.

18 MD Nastran 2006 Release Guide

Table 2-1

Information in Nonlinear Iteration Summary Table

MAT DIV

Number of material divergence + 1, i.e., it will be 1 if there is no material divergence. Material divergence is due to bad creep strain or excessive subincrements in plasticity.

AVG R_FORCE

Average residual force. In order for a time step to converge, this value must become very small.

TOTAL WORK

Accumulated total work done to the structure model. This value is only an approximation.

DISP AVG MAX AT GRID C

The average displacement, the maximum displacement and its grid point identification number and component number.

NO. QNV

Number Quasi Newton vectors stored and used.

TOT KUD

Total number of stiffness updates performed.

TOT ITER

Total number of iterations performed, including the number of stiffness updates and time steps.

For a large problem, TIME STEP NO,l TOT KUD, and TOT ITR in this table may be too large to be printed in the allocated fields, resulting in print overflow. If any of these values overflows, an additional line is printed to show the offsets of these values. In the table below, TOT ITR of the first line is 111764. The offset of TOT ITR is shown as TOT ITR= 110000+XXX, where XXX is the number shown under the TOT ITR column.

0

N O N - L I N E A R STIFFNESS UPDATE TIME ITERATION TIME TIME STEP NO.= 20000 TIME

2.99820E-01 2.99830E-01 2.99840E-01 2.99850E-01 2.99860E-01

- TIME STEP NO. BIS ADJUST ITR

9982 9983 9984 9985 9986

0 0 0 0 0

1.0000 1.0000 1.0000 1.0000 1.0000

I T E R A T I O N

0.01 SECONDS 0.00 SECONDS TOT KUD= 0 TOT ITR=

4 4 4 4 4

- - ERROR FACTORS - DISP LOAD WORK

3.99E-08 4.04E-08 4.10E-08 4.15E-08 4.20E-08

5.61E-04 5.77E-04 5.93E-04 6.09E-04 6.26E-04

M O D U L E

O U T P U T SUBCASE

1

STEP

1

110000 CONV ITR MAT AVG RATE DIV DIV R_FORCE

2.24E-09 2.25E-09 2.26E-09 2.27E-09 2.27E-09

0.03 0.03 0.03 0.03 0.03

0 0 0 0 0

1 1 1 1 1

TOTL WORK

6.0E2.386E 6.1E2.386E 6.3E2.385E 6.4E2.385E 6.6E2.385E

- - - - - DISP - - - - - - NO. TOT TOT AVG MAX AT GRID C QNV KUD ITR

7.32E-02 7.32E-02 7.32E-02 7.32E-02 7.32E-02

-1.860E-01 -1.861E-01 -1.862E-01 -1.863E-01 -1.865E-01

101 101 101 101 101

3 3 3 3 3

10 10 10 10 10

0 0 0 0 0

1764 1768 1772 1776 1780

Output Data Grouping: NLPACK For the nonlinear transient analysis of a large problem with short time steps, the amount of data to be stored in the database will be huge if we do not devise some schemes to group the output data. Data grouping will save CPU time, IO time, and disk space to store the database. Another advantage is that, for a large problem, if an accident happens in the middle of a run, you can salvage the data for later restart. There are two types of data required to be saved - output and restart data • Output data – these are displacements, stresses, and strains, etc. at each output time step to be

printed on the f06 file or plotted by the post processors. They are controlled by the NO field on the TSTEPNL Bulk Data entry. For this type of data, we output them as requested by the user.

CHAPTER 2 19 Nonlinear Analysis

• Restart data – these are used to described the material and geometric state of the structure model.

We use them to reconstruct the stiffness, the mass, the damping matrices and other tables required in later usage. Restart data are usually much larger than the output data if the structural model is large. This type of data can be saved selectively without degrading the effectiveness of the transient analysis. For this purpose, in the current release, a user modifiable parameter: ‘PARAM, NLPACK,N’ is available. N means that SOL 400 will pack output data for N output time steps and restart data for the last time step as a single data package. For example, if N = 100 (the default), then one data package has output data for 100 output time steps and restart data for the last time step. Later usage, such as restart or initial condition for later step, can be performed only at NLPACK data group boundaries. Some N’s have special meaning • N = -1, all output data for a STEP and restart data for the end of the STEP are grouped into a

single package. This is the SOL 129 grouping method. In this case, the restart can be performed only at STEP boundaries. • N = 0, this is illegal. • N = 1, each package of data on the database includes the output data for one output time step and

restart data. This is the NLSTATIC grouping method. Therefore, for the nonlinear static analysis, the restart can be performed at each user output load increment, which is controlled by INTOUT on the NLPARM Bulk Data entry. NLPACK is used in Example 1.

Restarts A nonlinear restart allows you to use the material or the geometrical properties of a previously converged solution as a new starting point to continue the analysis. This is useful when you want to change your loading sequence, the solution criteria, or to extend the analysis. For SOL 400, a user-friendly restart procedure for the nonlinear static pre-release is available. For nonlinear transient analysis, the following principles are noted. • The restart must be continued at a previous converged solution point in a nonlinear transient

analysis or a static analysis by specifying a SUBCASE, STEP, and/or TIME (LOADFAC). This is accomplished by using the Case Control command NLRESTART. Refer to the Case Control Command Descriptions (p. 196) in the MD Nastran Quick Reference Guide. • When the cold start is ANALYSIS=NLSTAT, it can be restarted at any user-specified output

load increment (controlled by NOUT in NLPARM Bulk Data entry). • When the cold start is ANALYSIS=NLTRAN, it must be restarted from a saved or check-

pointed time step. The checkpoint times are dependent on DT and NO values on the TESTEPNL Bulk Data entry, and PARAM, NLPACK of the cold start run. The checkpoint times are integer multiples of (DT x NO) x NLPACK. For example, if DT=0.001 second, NO=10, and NLPACK=100, the possible times that can be used for restart are at 1.0, 2.0, etc... If a requested restart time does not match a checkpoint time, the closest checkpoint time will be used

20 MD Nastran 2006 Release Guide

• The geometry and the initial material properties of the structural model cannot be modified. This

is obvious because any modification to the geometry or the initial material properties would invalidate the previous analysis and require the nonlinear solution to start from the very beginning. In such cases, it is simpler to initiate another cold start. Performing a restart is described in the following sub-sections. File Management Commands For a restart, the data of the cold start must be made available by using the File Management commands. For nonlinear restart, two commands are needed: ASSIGN and RESTART. These two commands are existing commands and no special requirements are needed for SOL 400. There are many methods to retrieve data for a restart. One method is given in the example below. For other methods, refer to the File Management Statement Descriptions (p. 37) in the MD Nastran Quick Reference Guide or Chapter 12 of the MD Nastran Reference Manual. Case Control Modifications The presence of a Case Control command NLRESTART indicates that the current run is a restart execution. The Case Control file contains both subcases and steps, which have been executed in the cold start, and those that are to be executed in the restart. The first subcase, step and/or load factor to be executed in the restart is indicated by the options on the NLRESTART command. This is shown in the following example. NLRESTART SUBCASE 1, STEP 2, TIME 0.3 SUBCASE 1 STEP 1 LOAD = 10 STEP 2 LOAD = 20 STEP 3 LOAD = 30 In the above example, the first STEP through time 0.3 of the second STEP has been previously executed. The restart execution begins with time 0.3 of the second STEP, and continues through the end of the third STEP. If time 0.3 is not a restart point saved by NLPACK on the cold start, SOL 400 will search for the nearest restart point on the data base and use that point to begin the restart. For restart, the Case Control file structure for SUBCASE and STEP commands must be the same as the cold start up to the restart point. After the restart point, you may modify the Case Control file structure for SUBCASE and STEP commands. For example, in above example, STEPs 1 and 2 must exist in the cold start. However, STEP 3 may or may not exist in the cold start. The following Case Control commands may be modified in a nonlinear restart: • Boundary conditions such as MPC and SPC. • Nonlinear solution control, NLPARM. • The LOAD requests. • Output request such as DISP and NLSTRESS.

CHAPTER 2 21 Nonlinear Analysis

• The analysis type ANALYSIS.

Depending on the option selected with the NLRESTART command, the nonlinear restart may be logically divided into three types: a case restart, a step restart, or a time restart: The case restart begins the execution with a SUBCASE. All five types of modification described above are legal for a case restart. The step restart begins the execution with a STEP, which may be a new step or a previously executed step. Although boundary condition and analysis type modifications are allowed, you have the responsibility to determine whether they are meaningful. Special attention should be given to the analysis type modification; it may not be meaningful in many situations and could lead to erroneous results. The time restart begins execution with a user-specified TIME. For a time restart, you should not modify the analysis type, boundary conditions, or load requests. You need to exercise discretion when attempting other types of modification at this level. Also, in order to perform this type of restart, the specified TIME must be at the NLPACK data group boundary. If it is not, SOL 400 will search for the nearest data boundary and use this boundary as the restart point. Bulk Data Modifications The Bulk Data file for a nonlinear restart contains only those entries that are to be added to the cold start. The deletion Bulk Data entry “/” cannot be used. This is to serve as a reminder that the geometry and the initial properties cannot be modified. You may make modifications to the Bulk Data file by introducing new entries, which may be copies of the original entries with appropriate changes and new identification numbers. The following list of entries can be added in a restart. • Load entries such as LOAD, FORCE, PLOAD4, and SPCD. • NLPARM entries. • Boundary condition entries such as SPC, SPC1, and MPC.

Examples for cold start and restart are given in Example 4 and Example 5.

Initial Conditions In SOL 400, the traditional way of requesting initial conditions by using the Case Control command, IC, and its associated Bulk Data entry, TIC, to assign initial displacements and velocities is supported. In the current release, a user-friendly interface to define initial condition is implemented. This is the new Case Control command NLIC. It allows users to assign the result of any previous STEP of NLSTAT analysis as the initial condition for the first STEP of NLTRAN analysis in a SUBCASE. The following is an example: SUBCASE 10 STEP 1 ANALYSIS = NLSTAT LOAD = 10 NLAPRM = 110

22 MD Nastran 2006 Release Guide

STEP 2 ANALYSIS = NLSTAT LOAD = 20 NLPARM = 120 STEP 3 ANALYSIS = NLTRAN NLIC STEP 1 LOADFAC 0.5 DLOAD = 30 TSTEPNL = 130 Now, the 3rd STEP will use the result of the 1st STEP at 50% load increment as the initial condition. Please note that the NLIC can only be defined at a load increment whose output flag is on - an available restart point in static analysis. Otherwise, a fatal error message will be issued and job will be terminated. Here, SOL 400 will not search for the nearest available restart point, because we want you to know the precise restart point. In above example, if ‘LOADFAC 0.5’ is left out, then STEP 3 will take last state of STEP 1 as its initial condition. In this case, the job will always run because the last state of a step is always a restart point. For NLIC, there are some rules and limitations: • SOL 400 requires that all STEPs’ of NLSTAT must be located before all STEPs’ of NLTRAN.

In other words, analysis change can only occur once between NLSTAT and NLTRAN in one SUBCASE. • In one SUBCASE, the beginning time of a transient STEP will be reset to 0.0 when the analysis

type is changed from a static STEP to transient STEP (or NLIC Case Control command is detected). • If you do not specify a NLIC entry when the analysis type changes from NLSTAT to NLTRAN,

the final result of the last STEP of NLSTAT will be picked up as the initial condition. • The NLIC (or IC) can only appear in the first transient analysis STEP (ANALYSIS=NLTRAN)

in a SUBCASE. Otherwise, it will be ignored. • The new Case Control command NLIC can only specify restart-able NLSTAT location as the

initial condition. (Please read the Restart section for the definition of “Restart-able”.) • It is not allowed to use NLIC to select the initial condition from any previous STEP of

NLTRAN, SOL 400 will issue a fatal error message and you should run a restart job instead. • In the same STEP, the NLIC cannot appear together with an IC. A fatal error message will be

issue when NLIC and IC appear in the same STEP. • The NLIC can only be used in SOL 400 (NONLIN).

Parameter ICOPT is used with the NLIC and IC Case Control commands. At the beginning of a NLTRAN step, the user input loads may or may not be in equilibrium with the results of the previous preload step. When ICOPT = 0, SOL 400 will compute the initial acceleration based on your’s inputs. Otherwise, it will be assumed that the initial acceleration is null. In other words, when ICOPT = 1 (the default), it is assumed that the whole structure is in equilibrium automatically. Theoretically, ICOPT = 0 gives better performance in the iteration algorithm since it guarantees the equilibrium in the beginning to avoid a suddenly jump of loads or displacements. The drawback of ICOPT = 0 comes from the

CHAPTER 2 23 Nonlinear Analysis

characteristics of the mass matrix itself, whose inverse matrix is required when computing the initial acceleration. The mass matrix is usually highly singular for a ‘lumped’ mass matrix or for a model with only solid 3D elements, a large amount of CPU times may be required and the accuracy of the result may be in doubt. An alternative way to resolve the problem of ICOPT = 1 with a suddenly large jump of loads or displacements is to insert a NLTRAN step in between the analysis step and its previous preload step. This step will have very short time duration in comparison with the analysis step and will provide a transition between the preload step and the analysis step. NLIC is used in Example 4 and Example 5. ICOPT is also used in these two examples.

Transient Temperature Loads A new capability, which has never been supported in the original nonlinear transient analysis (SOL 129), is added into SOL 400 when ANALYSIS=NLTRAN. It is the time-dependent dynamic thermal effect, which is applied to all the nonlinear elements in the residual. The time-dependent thermal-elastic equation can be written as follows ε T ( t ) = α ( T ( t ) ) ⋅ ( T ( t ) – T re f ) – α ( T 0 ) ⋅ ( T 0 – T re f )

(2-1)

where εT ( t )

= The thermal strain,

T(t)

= The current temperature is defined in the following equation T ( t ) = { T p }f ( t ) { T p } is the temperature

field and f ( t ) is the time function,

Tref

= The reference temperature,

T0

= The stress free temperature (initial temperature), and

α ( T ) = The coefficient of thermal expansion. For all nonlinear elements, the temperature effect, in both static and transient, is directly handled as thermal strain in SOL 400 when computing the element forces. To support the thermal effect in nonlinear transient analysis, two new bulk data entries have been created in the MD Nastran release. They are TTEMP and TMPSET. Basically, TTEMP is to define a timedependent dynamic thermal field, T ( t ) , which includes a spatial temperature distribution (TMPSET) and a time function (TABLEDi), in the same form as TLOAD1. TMPSET defines the spatial distribution by referencing a set of grid points. The temperatures ( Tp ) of these grid points are defined by TEMPD, TEMP, TEMPP1, or TEMPRB in the normal way. Please see the Bulk Data Entry Descriptions (Ch. 8) in the MD Nastran Quick Reference Guide, for the details of these two new bulk data entries. By using TTEMP and TMPSET, the whole model can be separated into finite sub-regions and each sub-region can have its own temperature distribution pattern. If it is necessary, you can also make every grid point as an independent sub-region or make the whole model as a single sub-region.

24 MD Nastran 2006 Release Guide

As in nonlinear static analysis, TEMP(INIT) and TEMP(LOAD) commands are used in the Case Control file to define the temperature input in nonlinear transient analysis. The SID of TEMP(LOAD) can refer to TTEMP to define the transient temperature load for a STEP. The spatial temperature distribution defined by TEMP, TEMPD, etc., must have the same SID as that of the associated TTEMP. If TEMP(INIT) refers to TTEMP entry, only the spatial temperature distribution of the entry is used and the time function is ignored. The Case Control command TEMP(LOAD) can also refers to a spatial distribution (TEMP, etc.) directly without TTEMP. In this case, the temperature time functions are linearly interpolated for the current step by using the last values of the previous step and the values of the spatial distribution referenced by the TEMP(LOAD) command. For the first step of a subcase, the interpolation is performed between the TEMP(INIT) temperature and the current temperature. The thermal effects computed by the above method depend on the current material state and geometric shape of the structural model. Therefore, they are called the ‘nonlinear’ transient temperature loads. For all upper stream superelements and all linear elements in the residual, the thermal effects are computed using the conventional method – you can use the DLOAD Bulk Data entry to combine multiple TLOAD1 and TLAOD2’s, whose EXCITE_ID reference thermal loads. The DLOAD Bulk Data entry must be referenced by a DLOAD Case Control command to be selected for analysis. The transient temperature loads computed by this method depend on the initial stiffness matrix only and are called the ‘linear’ transient temperature load. The TEMP(LOAD) and all its corresponding temperature related bulk data entries introduced above can only describe the thermal effect for the nonlinear elements in the residual. If there is no DLAOD Case Control command to select the temperature load for the linear temperature load, the temperature effect for the linear part of the structure will be lost. An example for the temperature load is given in Example 3.

Boundary Condition (SPC and MPC) Changes In SOL 400, the SPC and MPC are allowed to change from one step to next. This is accomplished by placing the SPC or MPC case control command below step level. However, it should be noted that SPC or MPC change requested below step level affect only the delta (incremental) displacements for the specific step. For example, if we add a SPC request on a grid point in STEP 2 of a subcase, the displacements of this grid will be kept constant in STEP 2 and equal to the final displacements of STEP 1. This means that the delta displacements of the grid for STEP 2 are zero because the SPC request in STEP 2, and the total displacements of STEP 2 is equal to the final displacements of STEP 1. The same principle is also applied to MPC requests below step level. An example for boundary condition changes is given in Example 8.

Direct Matrix Input Changes In SOL 400, the direct input matrices, K2PP, M2PP, B2PP and TFL, are allowed to change between steps. This is accomplished by the placing these case control commands below step level.

CHAPTER 2 25 Nonlinear Analysis

An example for the direct matrix changes is given in Example 7.

Outputs The outputs are requested by using the Case Control commands. All existing output Case Control commands such DISPLACEMENT, VELOCITY, ACCELERATION, STRESS, NLSTRESS, OLOAD, SPCFORCE, etc., are also allowed in the nonlinear transient analysis in SOL 400. Two special outputs, “Nonlinear Iteration Summary Table” and “PARAM, PH2OUT”, are available for nonlinear transient analysis in SOL 400. In addition, a new output control, “PARAM, NLPACK”, is added for the current release for nonlinear transient analysis only. This new parameter, NLPACK (=100 is the default), is used to control the packed output in SOL 400. The value of NLPACK represents the total number of output time steps in one output package. SOL 400 will process the output procedure only after collecting all "NLPACK" output time steps or at the end of each STEP. For details, please see Output Data Grouping: NLPACK, 18. Because the matrix and table trailers output volume may be extremely high, the diagnostic output requests of DIAG 8 and DIAG 15 have been turned off automatically when preparing the output data in the solver of SOL 400 if NLPACK ≠ 1. This action can reduce the .F04 file output size tremendously, especially, when there is a large output time steps requested. You can force them on by setting DIAG 56 but it is not recommended.

Error Handling In SOL 400, there are three types of fatal errors: • User or system fatal errors. • Fatal errors due to solution divergence • Fatal errors due to lack of CPU time.

For user or system fatal errors, if error occurs before the solution iteration phase, the run will terminate immediately without output the stored data. If the error occurs during the solution iteration phase, SOL will try to output all stored data for the current subcase and terminate the run. The solution will not continue into next subcase if there are multiple subcases. For fatal error due to solution divergence, SOL 400 will try to output all stored data for the current subcase and terminate the subcase. The solution sequence will jump to perform the next subcase if there are multiple subcases. For fatal error due to not enough CPU time, SOL 400 will try to output all stored data and terminate the run.

26 MD Nastran 2006 Release Guide

User Interfaces The user interfaces, which are important or new to the nonlinear transient analyses in SOL 400, are summarized in this section. For detail, please refer to the MD Nastran Quick Reference Guide. Nastran System Cells • STPFLG (SYSTEM (366)) – Selects the SUBCASE or STEP layout when there are a number of SUBCASE commands and no STEP command in a Case Control file. • TZEROMAX(SYSTEM (373)) – Controls initial time step adjustment in nonlinear transient

analysis. File Management Commands The following File Management commands are required for restarts. Please refer to the File Management Statement Descriptions (Ch. 2) in the MD Nastran Quick Reference Guide or Chapter 12 of the MD Nastran Reference Manual for details. • ASSIGN – Assigns physical file names to database files that are used by a Nastran data file to

run a job. • RESTART – Requests that data stored in a previous run be used in the current run.

Executive Control Command • SOL 400 or SOL NONLIN – Requests the SOL 400 general nonlinear solution sequence Parameters • PARAM, LGDISP – Requests a geometric nonlinear analysis. The default is 0, no geometric nonlinear effect. • PARAM, FOLLOWK – Requests whether the follower force stiffness will be used in a

geometric nonlinear analysis. The default is YES. • PARMA, FKSYMFAC – Controls whether the symmetrical follower force stiffness will be used

in a geometric nonlinear analysis. Default = 0.24. • PARAM, MAXLP – Specifies maximum number of iterations for element relaxation and

material point sub-increment process. Default = 10. • PARAM, NLAYERS – Specifies the number of layer for through thickness integration in the

material nonlinear analysis. Default = 5. • PARAM, NLTOL – Selects defaults for CONV, EPSU, EPSP, and EPSW for the Bulk Data

entries NLPARM and TSTEPNL. Default = 2. • PARAM, PH2OUT – Requests phase II outputs for a nonlinear analysis. Default = 0, phase III

output only. • PARAM, NLPACK – Control the total output time step in one output package; see section

Output Data Grouping above. Default = 100.

CHAPTER 2 27 Nonlinear Analysis

• PARAM, NDAMP – Specifies the α values when the HHT-α method using in SOL 400, see

section A New Numerical Integration Method above. Default = -0.05. • PARAM, ICOPT – Select how to handle the equilibrium when dealing with the initial condition,

see section Initial Conditions above. Case Control Commands • ANALYSIS – Selects solution method for an analysis step, see section Case Control Structure above. • NLRESTART – Requests a restart execution at a specific solution point for SOL 400, see

section Restarts above. • NLSTRESS – Requests the form and type of the nonlinear element stress output. • STEP – Delimits and identifies an analysis step, see section Case Control Structure above. • NLIC – Select the initial condition from any static analysis for the nonlinear transient analysis

Bulk Data Entries • MATHP- Specifies the hyperelastic material properties for an element. • MATS1 – Specifies the stress-dependent material properties for an element. • TSTEPNL – Defines a set of parameters for the nonlinear transient analysis iteration strategy. • TTEMP – Defines a time-dependent temperature distribution for use in the nonlinear transient

response. • TMPSET – Defines a spatial temperature distribution for use in the TTEMP Bulk Data entry.

Examples The following nine examples show the inputs and capabilities of the nonlinear transient analysis. The intention of these examples is to show the input structure for SOL 400. The model itself and the detailed entries in the Bulk Data file are not important. Example 1 Example one, EX01, is a simplified version of the standard QA file, NLTSUB02. This model only has QUAD4 elements. It has both material nonlinearity (MATS1) and geometrical nonlinearity (PARAM, LGDISP, 1). The 1st STEP will process the output data at every 5 output time steps and the 2nd STEP do it only once because of the settings of the parameter NLPACK. All bold-font statements are entries pertaining to the nonlinear analysis. ID MSC, EX01 $ TIME 150 $ SOL 400 $ CEND TITLE=ISOTROPIC MATERIAL & MATS1, ELLIPTIC CYLINDER UNDER EX01 SUBTITLE =SPC CHANGE IN EACH STEP, NLPACK’s SET 10 = 10000,11200

28 MD Nastran 2006 Release Guide

SET 20 = 101 SEALL = ALL DISPL = ALL STRESS = 20 $ SUBCASE 100 ANALYSIS=NLTRAN STEP 10 PARAM,NLPACK,5 DLOAD = 100 SPC = 200 TSTEPNL = 310 STEP 20 PARAM,NLPACK,-1 DLOAD = 100 SPC = 400 TSTEPNL = 320 $ BEGIN BULK PARAM NDMAP -0.05 PARAM LGDISP 1 TSTEPNL 310 100 TSTEPNL 320 100 $ PLOAD4 510 101 $ TLOAD1 100 510 TABLED1 120 +TBD1 0. 0. MAT1 100 3.+7 MAT1 101 3.+7 MATS1 100 $ GRID 10000 GRID 10001 GRID 10100 GRID 10101 GRID 10200 GRID 10201 GRID 10300 GRID 10301 GRID 10400 GRID 10401 GRID 10500 GRID 10501 GRID 10600 GRID 10601 GRID 10700 GRID 10701 GRID 10800 GRID 10801 GRID 10900 GRID 10901 GRID 11000 GRID 11001 GRID 11100 GRID 11101 GRID 11200 GRID 11201 $

0.01 0.01

10 10

AUTO AUTO

5. 0

THRU 0

112

120 +TBD1

5.

1. 0.3 0.3 PLASTIC 3.+5

16. .283-2 .283-2

100. 100. 99.3625 99.3625 96.8149 96.8149 92.5105 92.5105 86.6025 86.6025 79.2443 79.2443 70.5889 70.5889 60.7898 60.7898 50. 50. 38.3729 38.3729 26.0617 26.0617 13.2197 13.2197 0.0 0.0

10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0

0.0 0.0 3.30491 3.30491 6.51543 6.51543 9.59323 9.59323 12.5 12.5 15.1974 15.1974 17.6472 17.6472 19.8111 19.8111 21.6506 21.6506 23.1276 23.1276 24.2037 24.2037 24.8406 24.8406 25. 25.

1.

ENDT 500000. 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345

CHAPTER 2 29 Nonlinear Analysis

CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 $ PSHELL $ SPC1 SPC1 $ SPC1 SPC1 SPC1 SPC1 $ ENDDATA

101 102 103 104 105 106 107 108 109 110 111 112

100 100 100 100 100 100 100 100 100 100 100 100

10000 10100 10200 10300 10400 10500 10600 10700 10800 10900 11000 11100

10001 10101 10201 10301 10401 10501 10601 10701 10801 10901 11001 11101

100

100

0.10

100

200 200

16 26

11200 10000

11201 10001

400 400 400 400

16 26 1 2

11200 10000 10700 10701

11201 10001

10101 10201 10301 10401 10501 10601 10701 10801 10901 11001 11101 11201

10100 10200 10300 10400 10500 10600 10700 10800 10900 11000 11100 11200 101

Example 2 Example two, EX02, is modified version of the standard QA file, NLTSUB02. It shows two different types of analyses in the same job. This model is similar to the Example one except for adding some static loads and the required NLPARM’s. All bold-font statements are entries that show the difference in the two different analysis types. ID MSC, EX02 $ TIME 150 $ SOL 400 $ CEND TITLE=TEST MIXED ANALYSES - NLSTAT AND NLTRAN SUBTITLE =SPC CHANGE IN THE STEPS IN EACH SUBCASE SET 10 = 10000,11200 SET 20 = 101 SEALL = ALL DISPL = ALL STRESS = 20 $ SUBCASE 100 ANALYSIS=NLSTAT STEP 10 LOAD = 800 SPC = 200 NLPARM = 110 STEP 20 LOAD = 900 SPC = 400 NLPARM = 120 $ SUBCASE 200 ANALYSIS=NLTRAN STEP 10

EX02

30 MD Nastran 2006 Release Guide

DLOAD = 100 SPC = 200 TSTEPNL = 310 STEP 20 DLOAD = 100 SPC = 400 TSTEPNL = 320 $ BEGIN BULK NLPARM 110 NLPARM 120 $ LOAD 800 LOAD 900 (.. The rest is example....) ENDDATA

10 10

AUTO AUTO

YES YES

0.01 1.0 510 0.05 1.0 510 the same as what is in the Bulk Data file in the first

Example 3 Example three, EX03, is modified form of the standard QA file, NLTTL002. This model only has 1 QUAD4 element and 2 TRAI3 elements. Its major purpose is to show the various combinations of TTEMP and TMPSET inputs in nonlinear transient analysis for the thermal effect. All the bold-font statements are entries related to the temperature related inputs. ID MSC, EX03 $ SOL 400 DIAG 8,15 TIME 60 CEND SEALL = ALL SUPER = ALL TITLE = THERMAL LOAD TEST FOR NONLINEAR TRANSIENT ANALYSIS SUBTITLE = Q4/T3 MODEL, TTEMP AND TMPSET $ECHO = NONE MAXLINES = 999999999 $ TEMPERATURE(INITIAL) = 1 SUBCASE 1 analysis=NLTRAN step 1 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD) = 3 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all step 2 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD) = 4 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all SUBCASE 2 analysis=NLTRAN step 3 TSTEPNL= 1 SPC = 2

EX03

CHAPTER 2 31 Nonlinear Analysis

TEMPERATURE(LOAD) = 5 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all step 4 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD) = 6 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all SUBCASE 3 analysis=NLTRAN step 5 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD) = 7 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all step 6 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD) = 8 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all SUBCASE 4 analysis=NLTRAN step 7 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD) = 9 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all step 8 TSTEPNL= 1 SPC = 2 TEMPERATURE(LOAD) = 10 DISPLACEMENT(SORT1,REAL)=ALL nlstress = all stress = all $ BEGIN BULK PARAM POST -1 PARAM COUPMASS 1 PARAM LGDISP 1 PARAM K6ROT 100. PARAM,NOCOMPS,-1 PARAM PRTMAXIM YES PARAM,COMPMATT,YES PARAM,EPSILONT,INTEGRAL PARAM NLTOL 0 TSTEPNL,1,4,0.25,1,AUTO $ PCOMP 1 * 1 .04875 $ MAT8 1 7.15+6 2.9+6

79. 0. .29

1.4+6

0. YES 1.9-4

32 MD Nastran 2006 Release Guide

MATT8

2.9-6 1 1

6.-6 3 2

79. 5

4

6

$ TABLEM1 1 + CR 60. 2.9-6 70. 2.9-6 80. 3.24-6 100. + CS 120. 4.01-6 140. 3.89-6 150. 3.78-6 160. + CT 180. 3.52-6 200. 3.47-6 220. 3.55-6 240. + CU 250. 3.87-6 260. 3.99-6 280. 4.12-6 300. + CV 320. 4.24-6 ENDT $ TABLEM1 2 + CW 60. 6.-6 70. 6.-6 80. 7.67-6 100. + CX 120. 1.341-5 140. 1.37-5 150. 1.349-5 160. CY + CY 180. 1.266-5 200. 1.222-5 220. 1.218-5 240. CZ + CZ 250. 1.296-5 260. 1.334-5 280. 1.415-5 300. DA + DA 320. 1.46-5 ENDT $ TABLEM1 3 + BX 60. 7.15+6 70. 7.15+6 80. 7.15+6 100. + BY 120. 7.11+6 140. 7.08+6 150. 7.07+6 160. + BZ 180. 7.06+6 200. 7.05+6 220. 7.05+6 240. + CA 250. 7.04+6 260. 7.05+6 280. 7.06+6 300. + CB 320. 7.08+6 ENDT $ TABLEM1 4 + CM 60. .29 70. .29 80. .29 100. + CN 120. .29 140. .29 150. .29 160. + CO 180. .29 200. .29 220. .29 240. + CP 250. .29 260. .29 280. .29 300. + CQ 320. .29 ENDT $ TABLEM1 5 + CC 60. 2.9+6 70. 2.9+6 80. 2.9+6 100. + CD 120. 2.75+6 140. 2.68+6 150. 2.64+6 160. + CE 180. 2.47+6 200. 2.35+6 220. 2.22+6 240. + CF 250. 2.03+6 260. 1.95+6 280. 1.8+6 300. + CG 320. 1.65+6 ENDT $ TABLEM1 6 + CH 60. 1.4+6 70. 1.4+6 80. 1.4+6 100. + CI 120. 1.29+6 140. 1.24+6 150. 1.22+6 160. + CJ 180. 1.15+6 200. 1.1+6 220. 980000. 240. + CK 250. 810000. 260. 750000. 280. 620000. 300. CL + CL 320. 500000. ENDT $ cquad4,1,1,1,2,5,4 ctria3,2,1,1,2,4 ctria3,3,1,2,5,4 $ GRID 1 0.00000 0.00000 0.00000 GRID 2 1.00000 0.00000 0.00000 GRID 4 0.00000 1.00000 0.00000 GRID 5 1.00000 1.00000 0.10000 $ SPCADD 2 1

3.86-6 3.68-6 3.76-6 4.24-6

+ + + + +

+ 1.168-5+ 1.328-5+

CR CS CT CU CV CW CX

1.259-5+ 1.46-5 +

7.13+6 7.07+6 7.04+6 7.08+6

+ + + + +

BX BY BZ CA CB

.29 .29 .29 .29

+ + + + +

CM CN CO CP CQ

2.82+6 2.58+6 2.09+6 1.65+6

+ + + + +

CC CD CE CF CG

+ 1.34+6 + 1.2+6 + 870000.+ 500000.+

CH CI CJ CK

CHAPTER 2 33 Nonlinear Analysis

SPC1 1 123456 spc1 1 123456 $ TTEMP,3,111,300 TMPSET,111,4,5 TTEMP,3,101,310 TMPSET,101,1,2 $ TTEMP,4,102,400 TMPSET,102,1,2,4,5 $ TTEMP,5,201,500 TMPSET,201,1,2,4,5 $ TTEMP,6,-1,400 $ TTEMP,7,202,700 TMPSET,202,1,2 $ TTEMP,8,204,800 TMPSET,204,1,2 $ TTEMP,9,402,900 TMPSET,402,1,2,4,5 $ TEMP 1 1 TEMP 1 2 TEMP 1 4 TEMP 1 5 $ TEMP 3 1 TEMP 3 2 TEMP 3 4 TEMP 3 5 TABLED1 300 0.0 .9875 TABLED1 310 0.0 .9875 $ TEMP 4 1 TEMP 4 2 TEMP 4 4 TEMP 4 5 TABLED1 400 1.0 .9876542 $ TEMP 5 1 TEMP 5 2 TEMP 5 4 TEMP 5 5 TABLED1 500 0.0 .9875 $ TEMP 6 1 TEMP 6 2 TEMP 6 4 TEMP 6 5 $ $ TEMP 7 1

1 4

2

79. 79. 79. 79. 80. 80. 80. 80. 1.0

1.0

ENDT

1.0

1.0

ENDT

1.0

ENDT

1.0

ENDT

81. 81. 81. 81. 2.0 80. 80. 80. 80. 1.0 81. 81. 81. 81. 80.

34 MD Nastran 2006 Release Guide

TEMP 7 TEMP 7 TEMP 7 TABLED1 700 0.0 $ TEMP 8 TEMP 8 TEMP 8 TEMP 8 TABLED1 800 1.0 $ TEMP 9 TEMP 9 TEMP 9 TEMP 9 TABLED1 900 0.0 $ TEMP 10 TEMP 10 TEMP 10 TEMP 10 ENDDATA

2 4 5 .9875 1 2 4 5

80. 80. 80. 1.0

.9875 1 2 4 5

ENDT

1.0

ENDT

1.0

ENDT

81. 81. 81. 81.

.9876542 2.0 1 2 4 5

1.0

80. 80. 80. 80. 1.0 81. 81. 81. 81.

Example 4 Example four, EX04, is modified from the standard QA file, NLTIC19. This model only has 1 HEXA element. Its purpose is to shows two different types of analyses in the same SUBCASE, the model itself is not important. All the bold-font statements are entries that show the difference between those analyses and how to set the initial condition for the nonlinear transient analysis after static analysis. Note that the nonlinear transient analysis does not use the final results of the closest static analysis as the initial condition; instead, it asks the results of the 50% load increment in the 1st STEP to be the initial condition. Also, parameter ICPOT=0 is selected, which will compute the initial acceleration at the beginning (t=0.0) of the transient analysis when it is not in balance. ID MSC, EX04 $ DIAG 8,15 TIME 60 SOL 400 $ CEND TITLE= ELASTIC-PLASTIC STATIC & TRANSIENT RESPONSE, SUBTI= INITIAL ACCELERATION COMPUTED - PARAM,ICOPT,0 SET 1 = 1111 SET 2 = 100 DISP = 1 VELO = 1 ACCE = 1 OLOAD = 1 $ STRESS(PLOT) = 2 SUBCASE 1130 step 1 LABEL=UNIAXIAL TENSION (LOADING) ANALYSIS=NLSTAT SPC=100 LOAD=1130

EX04

CHAPTER 2 35 Nonlinear Analysis

NLPARM = 1 step 2 LABEL=UNIAXIAL TENSION (UNLOADING) ANALYSIS=NLSTAT SPC=100 NLPARM = 1 step 10 LABEL=I.C. FROM THE FIRST NLSTAT STEP(50%) - UNBALANCED CASE (NLIC) ANALYSIS=NLTRAN NLIC STEP 1 LOADFAC 0.5 SPC=100 DLOAD=2130 TSTEPNL=10 param,icopt,0 BEGIN BULK PARAM,LANGLE,3 PARAm,LGDISP,1 PARAM,W4,1.0 $ NLPARM 1 4 AUTO ALL 1.-6 TSTEPNL 10 2000 0.001 AUTO $ MAT1 1 30.0+6 11.5+6 0.3 7.332-2 0.01 PSOLID 1 1 $ SPC1 100 123456 1000 SPC1 100 1 1010 SPC1 100 2 1001 SPC1 100 3 1100 GRDSET 456 $ TLOAD1 2130 2130 0 500 TABLED1 500 +TAB1 +TAB1 0. 0. 1. -1. 1.2 0. 10. 0. +TAB2 +TAB2 ENDT $ LOAD 1130 -1.6 2. 121 LOAD 2130 -1.6 1. 121 $ GRID 1000 0. 0. 0. GRID 1100 1. 0. 0. GRID 1110 1. 1. 0. GRID 1010 0. 1. 0. GRID 1001 0. 0. 1. GRID 1101 1. 0. 1. GRID 1111 1. 1. 1. GRID 1011 0. 1. 1. $ CHEXA 100 1 1000 1100 1110 1010 1001 1101 +HX100 +HX100 1111 1011 $ PLOAD4 121 100 36.+3 1100 1111 PLOAD4 121 100 36.+3 1000 1011 ENDDATA

36 MD Nastran 2006 Release Guide

Example 5 Example five, EX05, is a modified version of the standard QA file, NLTIC19R. This model is a restart run of the Example four, EX04. Since there is no structure change in the SUBCASE 1130 and there is no parameter in NLRESTART command, this restart job will start from the 2nd SUBCASE. Its purpose is to shows how the Case Control commands NLRESTART and NLIC can work together. All bold-font statements are entries that show the key Case Control commands in this example. Note that the nonlinear transient analysis in the 2nd SUBCASE asks the final results in the 1st STEP of the 1st SUBCASE to be the initial condition. Also, parameter ICPOT=1 (the default) is selected, which will NOT compute the initial acceleration but loads in the beginning (t=0.0) of the transient analysis, that assumes the whole model is in equilibrium automatically when initial conditions are applied. ASSIGN RSFILE=’DBSDIR:ex04.MASTER’ $ RESTART LOGICAL=RSFILE $ $ ID MSC, EX05 $ DIAG 8,15 TIME 60 SOL 400 $ CEND TITLE= ELASTIC-PLASTIC STATIC & TRANSIENT RESPONSE, EX05 SUBTI= NO INITIAL ACCELERATION COMPUTED - PARAM,ICOPT1 SET 1 = 1111 SET 2 = 100 DISP = 1 VELO = 1 ACCE = 1 OLOAD = 1 $ STRESS = 2 NLRESTART SUBCASE 1130 step 1 LABEL=UNIAXIAL TENSION (LOADING) ANALYSIS=NLSTAT SPC=100 LOAD=1130 NLPARM = 1 step 2 LABEL=UNIAXIAL TENSION (UNLOADING) ANALYSIS=NLSTAT SPC=100 NLPARM = 1 step 10 LABEL=I.C. FROM THE FIRST NLSTAT STEP - UNBALANCED CASE (NLIC) ANALYSIS=NLTRAN NLIC STEP 1 LOADFAC 0.5 SPC=100 DLOAD=2130 TSTEPNL=10 param,icopt,0 SUBCASE 1131 LABEL=I.C. FROM THE 1st NLSTAT STEP OF PREVIOUS SUBCASE (NLIC) ANALYSIS=NLTRAN NLIC SUBCASE 1130 STEP 1 SPC=100 DLOAD=2130 TSTEPNL=10

CHAPTER 2 37 Nonlinear Analysis

param,icopt,1 BEGIN BULK ENDDATA

Example 6 Example six, EX06, is modified from the standard QA file, NLTROT01. This model simply shows how to run Rotor Dynamics in SOL 400. All bold-font statements are the basic entries that may be required in rotor dynamic analysis. ID MSC, EX06 $ SOL 400 DIAG 8, 15 CEND $ ANALYSIS=NLTRAN RIGID=LINEAR $ RGYRO= 100 TSTEP= 100 SET 99= 101 disp= 99 $ BEGIN BULK $ UNBALNC, 100, 2.0, 101, 0., 1., 0., , 1.0, 0.0, 0.0, 0.0, 1000., none $ TSTEPNL, 100, 5000, 3.0E-4, 10 $ ROTORG 10 101 THRU 103 $ RSPINT 10 101 102 FREQ 0.01 TABLED1, 100, , 0.0, 22.5, 100.0, 22.5, endt $ $ ROTOR 1 $ GRID, 101, , 0., 0., 0. GRID, 102, , 1., 0., 0., , 14 GRID, 103, , 2., 0., 0. GRID, 104, , 0., 0., 0. GRID, 105, , 2., 0., 0. $ RBE2, 1001, 102, 123456, 101, 103 RBE2, 1002, 101, 123456, 104 RBE2, 1003, 103, 123456, 105 $ CONM2, 1004, 102, , 50., , 5.0, , 15.0, , , 15.0 $ CELAS1, 1005, 1000, 104, 2 CELAS1, 1006, 1000, 104, 3 CELAS1, 1007, 1000, 105, 2 CELAS1, 1008, 1000, 105, 3 PELAS, 1000, 1.0E+5, 0.0 $ param, g, 0.05

100

38 MD Nastran 2006 Release Guide

param, w3, 141.3 $ enddata

Example 7 Example seven, EX07, is modified from the standard QA file, NLTK2PP1. This model shows how to apply K2PP in SOL 400, such as using different sets of K2PP in different STEP. For example, the 1st STEP requests the K2MAT matrix as a K2PP input and the 2nd STEP requests the combination of K2MAT and K3MAT matrices as a K2PP input. All the bold-font statements are the entries that are required in this kind of analysis. ID MSC, EX07 $ SOL 400 $ DIAG 8,15 TIME 50 CEND $ SEALL=ALL MPC = 20 SPC = 10 analysis=NLTRAN TITLE = LINEAR TRANSIENT RESP. (DIRECT METHOD) TEST SUBTITLE = COULOMB FRICTION LESS F3(0),F4(0) $ ECHO = NONE SET 10= 1,7 DISP=10 $ SUBCASE 1 STEP 1 DLOAD = 12 K2PP = K2MAT TSTEPNL = 10 STEP 2 DLOAD = 12 K2PP = K2MAT, K3MAT TSTEPNL = 10 $ BEGIN BULK param,ndamp,-0.055 $ CORD2R 1 0 0. 0. 0. 0. +CORD 1. 0. 0. $ GRDSET 1 1 GRID 1 -460. 0. 0. GRID 3 -460. 0. 100. GRID 5 -460. 0. 200. GRID 2 290. 0. 0. GRID 4 290. 0. 100. GRID 6 290. 0. 200. GRID 7 0. 0. 200. $ CONM2 3 3 1 0.6867 CONM2 4 4 1 1.2735 CONM2 7 7 1 15.445 +CONM 3.0E5 $

EX07

0.

1.

+CORD

1246

+CONM

CHAPTER 2 39 Nonlinear Analysis

CELAS2 CDAMP2 CELAS2 CDAMP2 CELAS2 CDAMP2 CELAS2 CDAMP2 $ MPC +MPC10 MPC +MPC11 MPCADD $ SPC1 $ TABLED1 +TBLD11 +TBLD12 $ EPOINT $ DMIG DMIG DMIG $ DMIG DMIG DMIG $ DAREA DELAY $ EPOINT $ DMIG DMIG $ DMIG DMIG $ DAREA DELAY $ TLOAD1 $ TSTEPNL ENDDATA

1 1 2 2 3 3 4 4

2200. 3.2 4200. 6.2 550. 13.3 2000. 0.

1 1 2 2 3 3 4 4

10

3 3 5 3 11

750. -460. 750. 1.

20

7 6 7 6 10

10

5

1

THRU

12 -100. ENDT

0.

0.

0.

0.005

1

1 101 1

3

2. -2.

1 101 1

3

3. -3.

202 2

3

2. -2.

202 2

3

3. -3.

11

3 3 3 3 3 3 3 3

3 3 4 4 5 5 6 6

3 3 3 3 3 3 3 3

5

3

-290.

+MPC10

5

3

-1.

+MPC11

3.

100.

6 3.

+TBLD11 +TBLD12

101 K2MAT K2MAT K2MAT

0 1 101

1 3

K3MAT K3MAT K3MAT

0 1 101

1 3

12 12

101 101

1

1. 0.

202 K2MAT K2MAT

2 202

3

K3MAT K3MAT

2 202

3

12 12

202 202

12

12

12

10

1000

0.002

1. 0.54 12 1

AUTO

10000

Example 8 Example eight, EX08, is modified from the standard QA file, NLTSTP06. This model shows the example of the SPC-Set change between STEP’s. All the bold-font statements are the entries that are required. ID MSC, EX08 $ TIME 150 SOL 400

$ $

40 MD Nastran 2006 Release Guide

DIAG 8,15 $ CEND TITLE=ANISOTROPIC MATERIAL & MATS1, ELLIPTIC CYLINDER UNDER EX08 SUBTITLE = TWO STEP’S TEST, SPC SET CHANGE AND SAME DT SET 10 = 10000,11200 SET 20 = 101 SEALL = ALL DISPL = ALL STRESS = 20 SPCF = ALL OLOAD = ALL $ SUBCASE 100 ANALYSIS=NLTRAN STEP 10 DLOAD = 100 SPC = 200 TSTEPNL = 310 STEP 20 DLOAD = 100 SPC = 400 TSTEPNL = 320 $ BEGIN BULK PARAM LGDISP 1 TSTEPNL 310 100 0.01 10 AUTO +TS11 TSTEPNL 320 100 0.01 10 AUTO +TS21 $ PLOAD4 510 101 5. THRU 112 $ TLOAD1 100 510 0 0 120 TABLED1 120 +TBD1 +TBD1 0. 0. 5. 1. 16. 1. ENDT MAT2 100 3.2967+79.8901+60. 3.2967+70. 1.1538+70.283-2 MAT2 101 3.2967+79.8901+60. 3.2967+70. 0.283-2 MATS1 100 PLASTIC 3.+5 500000. $ GRID 10000 100. 0.0 10. 345 GRID 10001 100. 0.0 0.0 345 GRID 10100 99.3625 3.30491 10. 345 GRID 10101 99.3625 3.30491 0.0 345 GRID 10200 96.8149 6.51543 10. 345 GRID 10201 96.8149 6.51543 0.0 345 GRID 10300 92.5105 9.59323 10. 345 GRID 10301 92.5105 9.59323 0.0 345 GRID 10400 86.6025 12.5 10. 345 GRID 10401 86.6025 12.5 0.0 345 GRID 10500 79.2443 15.1974 10. 345 GRID 10501 79.2443 15.1974 0.0 345 GRID 10600 70.5889 17.6472 10. 345 GRID 10601 70.5889 17.6472 0.0 345 GRID 10700 60.7898 19.8111 10. 345 GRID 10701 60.7898 19.8111 0.0 345 GRID 10800 50. 21.6506 10. 345 GRID 10801 50. 21.6506 0.0 345 GRID 10900 38.3729 23.1276 10. 345 GRID 10901 38.3729 23.1276 0.0 345 GRID 11000 26.0617 24.2037 10. 345 GRID 11001 26.0617 24.2037 0.0 345 GRID 11100 13.2197 24.8406 10. 345

CHAPTER 2 41 Nonlinear Analysis

GRID GRID GRID $GRID $GRID $GRID $ CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 $ PSHELL $ SPC1 SPC1 $ SPC1 SPC1 SPC1 SPC1 $ ENDDATA

11101 11200 11201 20000 20001 20100

13.2197 24.8406 0.0 0.0 25. 10. 0.0 25. 0.0 0. 0. 0. 100. 0. 0. 0. 100. 0.

101 102 103 104 105 106 107 108 109 110 111 112

100 100 100 100 100 100 100 100 100 100 100 100

10000 10100 10200 10300 10400 10500 10600 10700 10800 10900 11000 11100

10001 10101 10201 10301 10401 10501 10601 10701 10801 10901 11001 11101

100

100

0.10

100

200 200

16 26

11200 10000

11201 10001

400 400 400 400

16 26 1 2

11200 10000 10700 10701

11201 10001

10101 10201 10301 10401 10501 10601 10701 10801 10901 11001 11101 11201

345 345 345 123456 123456 123456 10100 10200 10300 10400 10500 10600 10700 10800 10900 11000 11100 11200 101

Example 9 Example nine, EX09, is modified from the standard QA file, NLTSTP07. This model shows that the upper stream superelement can have output requests that are different from the residual. Also, a case control command OTIME is used here to select a subset of all output time steps, which is selected by the TSTEPNL Bulk Data entry. It can reduce the output data dramatically. For example, in the following file, TSTEPNL asks output at time=0.0, 0.1,…, 1.0 second but OTIME overwrites this request and only makes output at time=0.5 second. All the bold-font statements are the entries that are required to complete all above requests in this example. ID MSC, EX09 $ TIME 150 $ SOL 400 $ DIAG 8,15 $ CEND TITLE=Test For Upperstream Superelement Output Request SUBTITLE = OTIME Output Request SET 1 = 0.5 SET 10 = 11200 SET 20 = 101 LOADSET = 500 DISPL = 10 OTIME = 1 $ SUBCASE 10

EX09

42 MD Nastran 2006 Release Guide

SUPER=10 METHOD=10 SET 10001 = 10001 DISP =10001 SUBCASE 100 ANALYSIS=NLTRAN DLOAD = 100 SPC = 200 TSTEPNL = 310 $ BEGIN BULK PARAM LGDISP 1 $ SESET,10,10000,thru,10301 SEQSET1 10 0 10500 THRU EIGRL 10 $ TSTEPNL 310 100 0.01 10 $+TS11 1.E-2 LSEQ 500 110 510 PLOAD4 510 101 5. $ TLOAD1 100 110 0 0 TABLED1 120 +TBD1 0. 0. 5. 1. $MAT1 100 3.+7 0.3 MAT2 100 3.2967+79.8901+60. MAT2 101 3.2967+79.8901+60. MATS1 100 PLASTIC 3.+5 $ GRID 10000 100. 0.0 GRID 10001 100. 0.0 GRID 10100 99.3625 3.30491 GRID 10101 99.3625 3.30491 GRID 10200 96.8149 6.51543 GRID 10201 96.8149 6.51543 GRID 10300 92.5105 9.59323 GRID 10301 92.5105 9.59323 GRID 10400 86.6025 12.5 GRID 10401 86.6025 12.5 GRID 10500 79.2443 15.1974 GRID 10501 79.2443 15.1974 GRID 10600 70.5889 17.6472 GRID 10601 70.5889 17.6472 GRID 10700 60.7898 19.8111 GRID 10701 60.7898 19.8111 GRID 10800 50. 21.6506 GRID 10801 50. 21.6506 GRID 10900 38.3729 23.1276 GRID 10901 38.3729 23.1276 GRID 11000 26.0617 24.2037 GRID 11001 26.0617 24.2037 GRID 11100 13.2197 24.8406 GRID 11101 13.2197 24.8406 GRID 11200 0.0 25. GRID 11201 0.0 25. $ CQUAD4 101 100 10000 10001 CQUAD4 102 100 10100 10101 CQUAD4 103 100 10200 10201

11001 AUTO

+TS11 THRU

112

120 +TBD1 16. 1. .283-2 3.2967+70. 3.2967+70.

ENDT

10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0 10. 0.0

345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345 345

10101 10201 10301

10100 10200 10300

1.1538+70.283-2 0.283-2 500000.

CHAPTER 2 43 Nonlinear Analysis

CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 CQUAD4 $ PSHELL $ SPC1 SPC1 $ SPC1 SPC1 SPC1 SPC1 $ ENDDATA

104 105 106 107 108 109 110 111 112

100 100 100 100 100 100 100 100 100

10300 10400 10500 10600 10700 10800 10900 11000 11100

10301 10401 10501 10601 10701 10801 10901 11001 11101

100

100

0.10

100

200 200

16 26

11200 10000

11201 10001

400 400 400 400

16 26 1 2

11200 10000 10700 10701

11201 10001

10401 10501 10601 10701 10801 10901 11001 11101 11201

10400 10500 10600 10700 10800 10900 11000 11100 11200 101

44 MD Nastran 2006 Release Guide

MD Nastran Implicit Nonlinear - SOL 600 This section documents the additions to SOL 600 for MD Nastran 2006. The following new capabilities have been added: • Reduced memory for many SOL 600 analyses is triggered by PARAM,MARCOOCC. There are

two effects when selecting this parameter: • The memory used for decomposition is used for other purposes as well, which reduces

memory required, but may result in an increase in I/O time. • When using SOLVER type 8, the minimal amount of memory will be used. • Reduced memory for analyses when composites or multiple element types are used.

The storage of element data quantities like stresses and strains has been modified. Previously, the amount of memory allocated per element was the maximum required for any element type. Thus there was a memory overhead in cases with different element types, or shells with different number of layers. In this release, the element data is dynamically allocated based upon element groups, where an element group contains one unique element type and material type. The amount of memory saved with the new element data storage is model dependent. There is no savings in memory if a homogeneous model with one element type is used. Extreme cases would be when there are only a few elements that require a large amount of memory, for example a model with a few 20-grid point CHEXA with the remainder of the mesh being 4-grid point CTETRA. In one example with a combination of 10,000 composite CHEXA and 80,000 CTETRA, which had several composite groups, with a maximum of 30 layers, the memory required for element storage was reduced from 11.9 Gbytes to 0.75 Gbytes. An engine model that had a total of 310,000 elements containing a combination of 20-node CEXA, 8-node CHEXA, 10-node CTETRA, 4-node CTETRA and CQUAD4 has achieved a memory reduction from the prior 3.76 GBytes to 0.86 Gbytes. No new input is required. • The amount of memory has been reduced when a large number of MPC, RBE2, and RBE3 are in

the model. The memory usage was especially acute when some RBEs have a large number of grid points. Furthermore the computational time associated with the application of the MPCs has been reduced. • Improvements have been made to reduce the amount of memory used by SOL 600 when

spawned from MSC.Nastran and in the Nastran translator. For advanced users, parameters were added to override the automatic memory variables and control each memory request. These are all documented in the MD Nastran 2006 Quick Reference Guide. • The value on the memory given on the PARAM,MARCMEM,value is no longer used in the

same way as in previous versions. Instead of setting the 2nd field of the SIZING entry, it now sets –ml value on the command line where the integer value entered is in Mbytes. For most analyses, the value entered can be smaller than what was needed for previous versions.

CHAPTER 2 45 Nonlinear Analysis

• There are two new parameters for allocating the memory use, the first

PARAM,MRALLOCG,value; allocates the initial amount of General memory. The value specified is in megabytes. In this release General memory is used for material property data, boundary condition data, overhead, and the assembly of the global stiffness matrix (except CASI solver). The General memory is also used for Solver 0 and Solver 4 (NLSTRAT,ISOLVER). The second parameter PARAM,MRALLOCS,value’ allocates the initial memory for the decomposition of the global stiffness matrix for Solver 8 (multifrontal direct solver). This is often useful to avoid reallocation of memory which occurs in deformable-deformable contact. For parallel processing the amount specified is the total for the job. It is divided by the number of domains used for each domain. • The CASI iterative solver was added; which can be activated by the NLSTRAT ISOLVER

entry. Currently, two preconditioner are available, a primal and standard preconditioned, types 0 and 1, respectively. The primal preconditioner is the default and is recommended for illconditioned problems. If a non-positive definite matrix is encountered (such as in a buckling analysis), the solver automatically switches to a direct solver. In this release this solver may not be used for Herrmann elements, where the Lagrange multiplier is at the corner node, such as the higher order elements or the triangular and tetrahedral elements. This solver should also not be used with the gap element. As an example of the improved performance with this solver an engine block with 2.2 million degrees of freedom was analyzed with the following normalized results.

Solver Type

Normalized Solution Time

2

0.785

8

1.0

9

0.174

• The computational times associated with running jobs in parallel has been reduced. This

reduction is both in the time associated with creating the domains in during the solution process. For poorly conditioned models, the improvements have been as large as a factor of two. • MD Nastran 2006 PC versions are released using the Intel version of MSC.Marc as the default.

The Digital Visual Fortran (DVF) version is available on the MD Nastran CD, but is no longer fully supported by SOL 600. If you prefer to use the DVF version, the OUTR options (op2, punch, xdb, f06) are no longer available and if attempted will generate an error. Memory has been reduced for analyses run in parallel. • The number of contact bodies has been increased from 99 to 999 • We have made improvements to MD Nastran so more problems with MPC's, RBE2, RBAR, and

RTRPLT will run to completion. For the 2006 release, AUTOMSET (param,automset,yes) has been added. Most analyses will not require AUTOMSET and since it takes additional computing time, MPC-CHECK,3 (param,marmpchk,3) should usually be used instead for models with complex rigid systems.

46 MD Nastran 2006 Release Guide

• MPC's and rigid elements combined with contact and/or the same node in more than one contact

body can sometimes cause the solver portion of SOL 600 to fail. There is a new feature in MSC.Marc known as optimized contact that can frequently help these types of models to run correctly. For version MSC.Marc 2005 r3, optimized contact is not the default either in MSC.Marc (stand-alone) or MD Nastran SOL 600. If MSC.Marc exit 2011 or convergence problems are encountered with such models, you should try optimized contact. To invoke optimized contact from MD Nastran, set field 6 of each BCBODY entry with flexible contact to 2. In addition, set field 3 of each "SLAVE" continuation line (the next line after all lines with SLAVE) to 2. In turn, this sets MSC.Marc's CONTACT entry 4th datablock, 3rd field to 2 and each CONTACT TABLE 3rd datablock 8th entry to 2 respectively. Detailed discussions and an example of optimized are provided in Chapter 8 of the MSC.Marc Theory and Information Manual (Volume A of the MSC.Marc documentation) - see text before and after figure 8-4. • For most bulk data entries, SOL 600 does not make the distinction between zero and a blank.

Thus, if a zero is entered and the default is some other value, the default will normally be used. If you wish to use zero, enter a small number such as 1.0E-12 instead. • Not all MD Nastran Case Control or Bulk Data entries are supported in SOL 600. Please

consult the MD Nastran Version 2006 QRG (SOL 600 Executive Control entry) for a list of items that are not supported. • Inertia Relief has been added. The SOL 600 capability exceeds that available in other MD

Nastran solution sequences using new Bulk Data entry, SUPORT6. • The “support” method may be used to specify which degrees of freedom should be

“supported” for each body. This is an extension of the PARAM,INREL,1 method and may use fewer computer resources than the eigenvalue method for some models. Inertia Relief may be employed on a subcase-by-subcase basis and can be removed if all previously unsupported bodies merge into the main body (which is supported) either all at once or gradually. • PSHELL with the same bending-membrane coupling as in other solution sequences has been

added into the 2006 release. This will allow you to analyze composite structures using the smeared approach (such as done in other MD Nastran solution sequences) or through-thethickness integration (which is more accurate and presently the only way to analyze composite structures) will be offered. If material nonlinearity occurs in the element, then the PSHELL smeared approach should not be used. The choice is activated by using PARAM,MRPSHELL,1. • Post-buckling responses using the single-file parallel option sometimes do not agree with the

responses using a single processor for the 2006 version. It is recommended that post-buckling analyses use a single processor. • A new option named DMIG-OUT is available in the 2006 release. This capability will allow the

stiffness, differential stiffness and mass matrices (assembled or element-by-element) to be output for selected output times or at the end of each nonlinear subcase for use in other analyses. This is a less expensive procedure, than using the Bulk Data entry, MDMIOUT (which creates a superelement), but results in a much larger matrix. • We have made the following improvements to the OP2 file produced by SOL 600 for MD

Nastran 2006:

CHAPTER 2 47 Nonlinear Analysis

• Contact forces are now included on the OP2 file in the “slide line” block. • GPFORCE is available starting with the 2006 release • MPC forces are now included on the OP2 file. • In the 2006 release, Case Control MUST be used to create an OP2 file. This is consistent with

other Nastran solution sequences, but is a change in behavior from previous releases. • For the 2006 release, you must include Case Control requests such as DISP=ALL in order to

obtain output in op2, xdb, punch or f06 files. In addition, OUTR requests on the SOL 600 entry must be made (for example OUTR=OP2,F06). The applicable Case Control requests for SOL 600 are DISP, STRESS, STRAIN, SPCFORCE, MPCFORCE, GPFORCE and BOUTPUT. BOUTPUT maps 3D contact to the older 2D Slideline Contact datablock (see item codes for contact in section 6 of the 2006 Quick Reference Guide). At present, MSC.Patran cannot process 2D slideline or 3D contact from the op2 or xdb. • The output interval for the t16 file (and thus the OP2 file) is controlled by either the NLPARAM

bulk data or PARAM,MARCOTIM, which is documented in the MD Nastran 2006 Quick Reference Guide. • A preliminary version of Grid Force Balance is available. The output is available in the op2,

xdb, f06 and punch files and is triggered by Case Control GPFORCE( )=ALL as well as PARAM,MARGPFOR • A simplified procedure is available for activating large displacement – large strain analysis, by

using the PARAM,MLSTRAIN. This option will automatically select the best formulation based upon the individual element type and material model. It effectively replaces the use of PARAM,LGDISP; PARAM, MRUPDATE; PARAM, MRFINITE and PARAM,MARCDILT for most simulations. Internally the following formulations are used. Large Strain Option element type / material model

1-d

plane stress or membranes or shell elements

plane strain or axisymmetric, or 3-d, displacement form.

plane strain or axisymmetric, or 3-d, Herrmann form

conventional elastic-plastic

Updated Lagrange Additive Plasticity No Finite Strain

Updated Lagrange Additive Plasticity Includes Finite Strain

Updated Lagrange Additive Plasticity Includes Finite Strain Utilized Constant Strain

Updated Lagrange Multiplicative Plasticity Includes Finite Strain

Mooney, Ogden, Gent or ArrudaBoyce

Total Lagrange

Total Lagrange

Updated Lagrange

Updated Lagrange

Foam

Total Lagrange

Total Lagrange

Updated Lagrange

Updated Lagrange, Incompressibility Neglected

• The Gent and Arruda Boyce models may now be used with plane stress, shell and membrane

elements

48 MD Nastran 2006 Release Guide

• The NLELAST option on the MATS1 is now supported in SOL 600 as in the other solution

sequences (106, 129, and 400). It is more general in that it may be used will all structural element types (except the shear panel). • A new higher order tetrahedral element is available which has improved behavior in bending. To

activate this element, use the PARAM,MRALIAS,127184 to switch the element formulation from SOL 600 element type 127 to 184. • The method for updating the thickness of shells and plane stress elements has changed if the

PARAM,MRFINITE or PARAM,MLSTRAIN. This is activated using: PARAM,MRV09V11,1 • The in-plane shear behavior of the CQUAD 4 element using reduced integration has been

improved. This element technology is invoked by using PARAM,075140. This is activated using: PARAM,MRV09V11,1 • Dissimilar meshes of shell elements may now be “glued” together using fully moment carrying

capability of the contact glue option. This is activated using the BCTABLE option. • A new parameter has been added when using SOL 600 analysis. When relevant, this generally

results in improved behavior, but will lead to some differences in results with the previous release. This is activated using PARAM,MRV09V11,value, where -1

Do not add the features

1

Add the following features (default): feature,4703 to speed up DDM jobs (for 1-processor jobs, it has no effect). feature,5701 to disable old rigid rotation checking which was too stringent feature,601 to improve contact feature,5301 to improve deformable-deformable contact feature,3201 to improve contact friction types 6 and 7 feature,5601 to improve thickness updating when the updated Lagrange method is used feature,5801 to improve in-plane bending of SOL 600 element type 140 feature,6001 to improve concrete cracking analysis Note that the above features are only used for certain problems. Even though all are included with the default option, they have no effect for problems that do not use them. For example, feature,5801 has no effect on models that do not use SOL 600 element type 140, feature 601 has no effect on models that do not have contact. • The speed of the t16op2 results translator has been increased by a factor of 4 or more for large

models. The speed increase is triggered using PARAM,MSPEEDOU,1 • Translation speed has increased for beam and shell type elements (in addition to the previous

speed enhancements for solid elements) by using PARAM,MSPEEDSE,2 (or 3). The speed increase varies from model to model but can be as great as a factor of 4-10 for some models.

CHAPTER 2 49 Nonlinear Analysis

• A new Bulk Data entry for brake squeal named BRKSQL is available which replaces several

parameters and MARCIN entries previously used. With the entry, new capabilities are also introduced. It is now possible to determine the unstable brake squeal roots using MD Nastran’s complex eigenvalue solver and unsymmetric friction stiffness matrices for an undeformed structure or after a nonlinear subcase. Brake squeal analysis for SOL 600 is accomplished by starting a primary MD Nastran job (as usual) which spawns SOL 600 to calculate the unsymmetric friction stiffness matrices either at the beginning or end of a nonlinear subcase, then spawning a second MD Nastran job to calculate the complex eigenvalues. Unstable roots indicate potential brake squeal. They are designated by positive real roots and negative damping in the f06 output file. See the BRQSQL entry from more details and the attached example. • A new fixed-time stepping approach has been added which avoids some convergence problems

with AUTO LOAD particularly for multiple subcases. AUTO LOAD is still available but the new approach is recommended particularly for multiple subcases. The available methods are selected using PARAM,MARCITER,N where N is the number of fixed time steps desired. • MD Nastran SOL 600 now uses the same compilers on all systems. This allows user

subroutines to be employed on all systems. For Windows and Linux, the Intel compiler is now used. Previously, the Digital Visual Fortran and PFG Fortran compilers, respectively, were used. Only the Intel versions are delivered with MD Nastran. • User subroutine support has been added through Bulk Data entry, USRSUB6 • The SOL 600,ID executive control statement has been revised to add some clarifying remarks • TEMP(INIT) does not work properly using Updated Lagrange (param,mvarupdat,1). If

TEMP(INIT) is required in the model, please use the Total Lagrange formulation (param,marupdat,-1). If all initial temperatures are zero, TEMP(INIT) may be omitted and Updated Lagrange may be used. • The Case Control BCTABLE text has been clarified • The NDDL description for some SOL 600 bulk data entries is not up to date. These entries are

intercepted and placed on a special database used by the SOL 600 translators. Another aspect of the NDDL not being up to date is that the 3D contact Bulk Data entries are only valid for SOL 600. They must be removed from the input deck for other solution sequences for MD Nastran 2006. It is anticipated that this will be corrected in the next MD Nastran release. • The following new Bulk Data entries have been added for SOL 600 (see next section for a

description of each new entry): • BRKSQL (Brake Squeal) • SUPORT6 (Inertia Relief for SOL 600) • USRSUB6 (User subroutines for SOL 600) • The following Bulk Data entries have been revised or additional capabilities added: • RESTART (Shared with SOL 700, items for SOL 700 were added) • NLSTRAT (CASI solver, rigid rotation control added) • IPSTRAIN (text clarified) • IPSTRESS (text clarified)

50 MD Nastran 2006 Release Guide

• BCPROP (text clarified) • MBOLTUS (Extraneous variables removed) • MATHED (text clarified) • MATORT (defaults change to zero) • The following parameters have been added • MARCITER • HEATCMD • MSPEEDOU • MRCONVER • MEXTRNOD • MARCBUSH • MRCOMPOS • MRBEPARM • MARBATCH • MARCCBAR • MARCRACC • MARCRCID • MRPSHELL • MARGPFOR • MLSTRAIN • MARCRADD • MRV09V11 • The following parameters have been revised to add options, clarify text or change defaults • MARCSOLV • MARCRBE3 • MARCOTIM • MARCSLHT • MARCPOST • MARCAUTO • MARCGAUS • MRMAXMEM • MRTABLS1 • MRTABLS2 • MARCUSUB

CHAPTER 2 51 Nonlinear Analysis

• MRSPAWN2 • MARCPINN • MRESTALL • MARCOPP2 • MSPEEDSE • MARCSAME • The following parameter has been removed: • MARNOT16 • Detailed Descriptions of each new Bulk Data entry:

52 MD Nastran 2006 Release Guide

BRKSQL

Specifies data for Brake Squeal Calculations using SOL 600

Specifies data for brake squeal calculations using SOL 600. Format: 1 BRKSQL

2

3

4

METH

AVSTIF

FACT1

R1

R2

R3

5

6

7 GLUE

X

Y

Z

3.0

4.0

8

9

10

ICORD

NASCMD

RCFILE

Example: BRKSQL

1

5.34E6

1.0

1.0

0.0

0.0

1.0

2.0

tran nastb

Field METH

Contents Method flag corresponding to the type of brake squeal calculations to be performed. (Integer, Default = 1) 0 = Perform brake squeal calculations before any nonlinear analysis has taken place. 1 = Perform brake squeal calculations after all nonlinear load cases.

AVSTIF

Approximate average stiffness per unit area between the pads and disk. This value is also known as the initial friction stiffness in the MSC.Marc Volume C documentation. AVSTIF can be obtained by either experiment or numerical simulation. A larger value of AVSTIF corresponds to a higher contact pressure, which usually results in more unstable modes. (Real; no Default; required field)

FACT1

Factor to scale friction stiffness values; see Remark 3. (Real; Default = 1.0)

GLUE

Flag specifying whether MPC for non-pad/disk surfaces with glued contact are used or ignored (Integer, Default = 0). A value of 0 means ignore the MPC; a value of 1 means include the MPCs (see Remark 6).

ICORD

Flag indicating whether coordinates are updated or not. A value of 0 means coordinates are not updated. A value of 1 means coordinates are updated using the formula Cnew=Corig+Defl, where Cnew are unpdated coordinates, Corig are original coordinates, and Defl are the final displacements. (Integer; Default = 0)

CHAPTER 2 53 Nonlinear Analysis

Field

Contents

R1

X direction cosine (basic coord system) of axis of rotation; corresponds to ROTATION A second datablock. (Real; no Default. Required field)

R2

Y direction cosine (basic coord system) of axis of rotation; corresponds to ROTATION A second datablock.

R3

Z direction cosine (basic coord system); corresponds to ROTATION A second datablock. (Real; no Default. Required field)

X

X coordinate in basic coord system of a point on the axis of rotation; corresponds to ROTATION A third datablock. (Real; no Default. Required field)

Y

Y coordinate in basic coord system of a point on the axis of rotation; corresponds to ROTATION A third datablock. (Real; no Default. Required field)

Z

Z coordinate in basic coord system of a point on the axis of rotation; corresponds to ROTATION A third datablock. (Real; no Default. Required field)

NASCMD

Name of a command to run MD Nastran (limited to 64 characters) -- used in conjunction with the CONTINUE options on the SOL 600 entry. The full path of the command to execute MD Nastran should be entered. The string will be converted to lower case. See Remark 2. (Character; Default = nastran)

RCFILE

Name of an RC file to be used with a secondary MD Nastran job (limited to 8 characters) -- used in conjunction with the CONTINUE options on the SOL 600 entry. An extension of “.rc” will automatically be added. See Remark 2. (Character; Default = nastb.rc)

Remarks: 1. This entry is used to calculate complex eigenvalues for brake squeal using unsymmetric stiffness friction matrice. Options exist to obtain the unsymmetric stiffness matrices using the undeformed geometry (initial contact) or after all specified nonlinear subcases. 2. SOL 600 performs brake squeal calculations. The main (original) MD Nastran job with input file jid.dat or jid.bdf spawns the SOL 600 job. MD Nastran SOL 600 calculates unsymmetric friction stiffness matrices that1 are saved on a file (jid.marc.bde with associated file jid.marc.ccc). The primary MD Nastran job then creates input data for a second MD Nastran job (jid.nast.dat) to use the unsymmetric stiffness matrices in an complex eigenvalue extraction. The primary MD Nastran job spawns a second MD Nastran job to calculate the complex eigenvalues. The complex eigenvalues and eigenvectors are found in jid.nast.f06, jid.nast.op2, etc. NASCMD is the name of the command used to execute the secondary MD Nastran job. NASCMD can be up to 64 characters long and must be left justified in field 2. The sting as entered will be used as is -- except that it will be converted to lower case regardless of whether it is entered in upper or lower case.

54 MD Nastran 2006 Release Guide

RCFILE is the name of an RC file to be used for the secondary MD Nastran job. It should be similar to the RC file used for the primary run except that additional memory will usually be necessary to calculate the complex eigenvalues and batch=no should also be specified. RCFILE is limited to 8 characters and an extension of “.rc” will be added automatically. This entry will be converted to upper case in MD Nastran but will be converted to lower case before spawning the complex eigenvalue run. This RC file must be located in the same directory as the MD Nastran input file. This entry is the same as specifying PARAM,MRRCFILE. One or the other should be used. 3. MPC are produced for contact surfaces with glued contact. DMIGs are produced for contact surfaces without glued contact. The brakes and drums should not use glued contact; other regions of the structure can used glued contact. 4. The continuation lines may be omitted if defaults are appropriate. 5. When a BRKSQL entry is used, PARAM,MRMTXNAM and PARAM,MARCFIL1 should not be entered. 6. When brake squeal matrices are output, unsymmetric friction stiffness matrices are output for non-glued contact surfaces. For surfaces with glued contact, MPCs are output. The GLUE flag signals SOL 600 to look for these MPCs and combine them with other MPCs that might be in the model using MPCADD, or if no MPCs were originally used, to add the MCPs due to glued contact. Glued contact surfaces may not be used for the disk-rotor interface. If GLUE is zero or blank, the MPC for glued contact in the brake squeal bde file, if present, will be ignored. Sometimes MD Nastran puts out MPCs with only one degree-of-freedom defined. Such MPCs will be ignored; otherwise, MD Nastran will generate a fatal error. 7. If ICORD=1, an MD Nastran t19 file will be automatic.

CHAPTER 2 55 Nonlinear Analysis

SUPORT6

Inertia Relief for SOL 600 - Used in MD Nastran Implicit Nonlinear SOL 600 only

Defines inertia relief for SOL 600. Format: 1 SUPORT6

2

3

4

SID

METH

IREMOV

MODES

FMAX

FSHIFT

5

6

7

GID

CDOF

CID

3000

123456

0

8 IDS1

Examples: SUPORT6

2

1

SUPORT6

3

2

6

0.6

-10.0

SUPORT6

0

3

1

SUPORT6

4

3

-2

101

9

10

56 MD Nastran 2006 Release Guide

Field

Contents

SID

Set ID corresponding to a Case Control SUPORT1 command or zero (Integer, Default = 0) 0 = if this is the only SUPORT6 entry, use this SUPORT6 entry for all subcases. If there are multiple SUPORT6 entries, use the one with SID=0 for increment zero. N = Use this SUPORT6 entry for the subcase specified by Case Control SUPORT1=N Different SUPORT6 entries can be used for each subcase if desired and different subcases can use different methods. If there is only one SUPORT6 entry (with SID=0) no Case Control SUPORT1 commands are necessary.

METH

Method to use (Integer, Default = 0) 0 = Inertia relief is not active for this subcase 1 = Use the “Kinematic” method – do not enter continuation line. Input will come from fields 5-7 of this entry 2 = Use the “Eigenvalue” method – Input data from the 2nd line must is used and fields 5-7 of the primary line must be blank (any SUPORT/SUPORT1 Bulk Data entries are ignored). 3 = Use the “Support Method”, usually specified using param,inrel,-1 for other solution sequences (see Remark 3). Do not enter the continuation line. Input will come from all SUPORT entries and those SUPORT1 entries with ID=SID.

IREMOV

Method to retain or remove inertia relief from a previous subcase (Integer, Default = 1) 1 = Retain inertia relief conditions from previous subcase 1 = Remove inertia relief loads immediately 2 = Remove inertia relief loads gradually IREMOV should be blank or 1 unless METH is 0

GID

Reference Grid ID for kinematic method (Integer, Default = 0) =0 Use the origin =N Use grid ID N (Used for METH=1 ONLY)

CDOF

Degrees of freedom for which inertia relief loads will be applied (Integer, no Default). Enter a string of values identifying the degrees of freedom for the model. For 3D models, usually 123456 is entered. For 2D models two or three degrees of freedom as applicable may be entered. The limit is 6 degrees of freedom for 3D models (see Remark 2). (Used for METH=1 ONLY)

CID

Coordinate system flag designating how to apply inertia relief loads (Integer, Default = 0) 0= Basic coordinate system N=Apply loads in coordinate system designated by field 7 of the GRID entry for grid id N. (Used for METH=1 ONLY)

CHAPTER 2 57 Nonlinear Analysis

Field

Contents

IDS1

ID of SUPORT1 entries to be used if METH=3 and SID=0 (Integer, no Default) For METH=3, only SUPORT1 entries with ID=IDS1 will be used in increment zero. All SUPORT entries will be used (Used for METH=3 when SID=0 ONLY)

MODES

Number of modes to use in the Eigenvalue method (Integer, no Default) (Used for METH=2 ONLY)

FMAX

Rigid body modes frequency cutoff (Hz) (Real, Default =1.0 Hz) (Used for METH=2 ONLY)

FSHIFT

Shift frequency used in Lanczos eigenvalue extraction (Hz) (Real, Default = -1.0 Hz) (Used for METH=2 ONLY)

Remarks: 1. The continuation entry is required only if the eigenvalue method (METH=2) is used. Fields 5-7 must be blank if the eigenvalue method is to be used. The continuation option must be omitted if the kinematic method is to be used. The kinematic method is similar to param,inrel,-2 for other solution sequences except that the inertia relief loads are updated at each iteration. 2. For the kinematic method, a maximum of 6 degrees of freedom are allowed for 3D structures (2 or 3 dof for 2D structures). You are responsible for knowing how many rigid body modes need to be “constrained” with inertia relief. For multiple contact bodies which are unsupported at the beginning of an analysis but eventually contact, there are usually 6 dof per flexible body. This situation requires the use of the eigenvalue method with MODES set to 6 times the number of unsupported flexible bodies. If some flexible bodies are supported in some directions but not in others, the number will be less than 6 per body. It is suggested that a preliminary SOL 103 eigenvalue extraction be performed to assess the number of rigid body modes. 3. The parameter INREL is ignored by SOL 600.

58 MD Nastran 2006 Release Guide

USRSUB6

Defines User Subroutines for SOL 600 - Used in MD Nastran Implicit Nonlinear - SOL 600 only

Defines user subroutines for SOL 600 Format: 1 USRSUB6

2

3

U1

U2

U9

U10

4 U3

5 U4

6 U5

7 U6

8 U7

9

10

U8

Examples: USRSUB6

UDAMAG

USRSUB6*

SEPFORBBC

UVOID

TENSOF

Field Ui

Contents Name of user subroutine to be included (Character, no Default) See MSC.Marc Volume D for list of available User subroutines

Remarks: 1. All user subroutines must reside in the directory where the MD Nastran input file resides. 2. All names must be in lower case and have the extension .f 3. SOL 600 combines all user subroutines into one large subroutine named u600.f and u600.f is passed to the command line when spawned from MD Nastran.\

Non-Supported Items Of the remaining non-supported items, the most important are listed below. If your model requires the use of these items, you should use SOL 106 or 129 instead. • CGAP is only partially supported and its use with SOL 600 is discouraged • Most MD Nastran superelements types are not available yet except for external

superelements. SOL 600 may be used to create a superelement and write out a DMIG that may be used in a subsequent MD Nastran analysis. • Certain Case Control entries such as STATSUB are not available

CHAPTER 2 59 Nonlinear Analysis

• MSC.Marc 2005 r3 is installed with MD Nastran 2006. Appropriate licenses are needed to use

SOL 600. For most computer systems, installation is automatic. However, for some systems, particularly IBM AIX systems, the MSC.Marc Installation Manual found in the MSC Combined Documentation CD should be consulted. For certain IBM AIX systems, the include file in the tools directory must be changed and the ~/marc2005/lib/lib_extra directory might need to be renamed to ~/marc2005/lib/lib_shared if a compiler is not available. MSC technical support personnel can assist with these issues. • For MD Nastran 2006 it is still recommended that postprocessing be accomplished using the t16

file particularly if contact output or multiple type of stress or strain tensor information is desired. MSC.Patran and certain other programs can postprocess all t16 data.

60 MD Nastran 2006 Release Guide

MD Nastran Explicit Nonlinear - SOL 700 Introduction SOL 700 is the first release of powerful Explicit Nonlinear Solution available in MD Nastran 2006 and offers unprecedented new technology to analyze transient dynamic events of short duration with severe geometric and material nonlinearities. MD Nastran SOL 700 allows users to work within one common modeling environment using the same Bulk Data interface. The NVH, linear and nonlinear models can be used for explicit applications such as crash, crush, and drop test, blade out and bird strike simulations. This dramatically reduces the time spent to build different models for implicit and explicit analysis and prevents the users from making mistakes because of unfamiliarity between different programs. MD Nastran SOL 700 is being developed in phases. The first phase, available in MD Nastran 2006 r1 is intended to solve highly nonlinear transient structural applications such as crash simulations, drop test, crush and impact problems. Although Phase 1 primarily addresses crash and impact loading, usually described by initial velocity input, other types of dynamic loading are also supported. Special crash features such as seat belts and occupant dummies are also supported. Future releases of MD Nastran will also support fluid structure interaction (FSI) capability and allows users to simulate applications such as airbags, sloshing and blast problems. SOL 700 is based on the well-known LS-DYNA solver, which is well integrated inside MD Nastran. The MD Nastran style of input data is processed within the IFP (Input File Processor) for user input errors and then filtered and mapped directly to the LS-DYNA memory by means of LS-DYNA style structured file. There are no translations between Nastran “.bdf” input file to LS-DYNA “.key” input file format. LS-DYNA then continues with computations to produce output results for highly nonlinear problems. Native LS-DYNA results files such as d3plot and d3thdt are available for post processing. In the MD Nastran 2006 r1 release, standard Nastran output such as op2, xdb and punch are not available but may be supported in future releases. The MD Nastran input can contain as many subcases as desired; however only one may be selected for use in any particular SOL 700 analysis. This is done using the Case Control commands, SKIP ON or OFF, to pick the desired subcase.

Linear and Nonlinear Analysis SOL 700 is an explicit dynamic analysis program that can perform linear transient analyses (such as SOL 109) as well as nonlinear transient analyses (such as SOL 129). It is also set up to perform linear or nonlinear static analyses (such as SOL 101 and SOL 106). Because of the numerical integration approach used within LS-DYNA, very small time steps are required to maintain accuracy and solution stability. The penalty for taking small time steps is partially offset by not having to decompose a stiffness matrix. See the MD Nastran Explicit Nonlinear User’s Guide for further theoretical details. The small time step requirements do not create a large problem when simulating events that occur quickly, such as impact or crash. However, for longer events such as low frequency

CHAPTER 2 61 Nonlinear Analysis

dynamics or static analysis, the run time sometimes becomes too large for explicit methods and implicit analyses need to be employed. New entries have been added to MD Nastran to make it easier to describe crash and impact. Examples are the new TICD entry that adds a from-thru-by grid ID description so that initial velocity input can be described by one line rather than a TIC entry for each grid. This allows an existing input file to be edited and quickly changed to a crash analysis. For those familiar with the LS-DYNA material descriptions, about 70 of the most commonly used LSDYNA material models are supported in SOL 700. Contact is described using the same style as MD Nastran Implicit Nonlinear Solution (SOL 600); however, a new entry called “WALL” is added to facilitate the modeling of rigid and flat barriers commonly used during crash and impact simulations. During explicit simulations, the structure will usually undergo very large deformations. As elements are distorted severely, the smallest element dimension will control the simulation timestep and therefore the runtime. When the time step for explicit analysis decreases to very small values or reaches zero, the job will hung. To alleviate the small time step problem, an initial and minimum time step using PARAM*,DYINISTEP and PARAM*DYMINSTEP should be defined. Default values of 1.0E-6 and 1.0E-9 have been defined respectively if these parameters are not entered. If different values are desired, you can enter them (both) in the Bulk Data or in an RC file. RC files do not allow wide-field parameters, therefore if they are to be entered in an RC file, they must be truncated to 8 characters. For example, param,dyinistep,1.0E-4 and param,dyminstep,1.0E-8 are both valid entries.

Latest Capabilities of MD Nastran Explicit Nonlinear - SOL 700 MD Nastran 2006 is the first official release of Explicit Nonlinear SOL 700 and it has been dramatically enhanced. The following additions including thirty NEW material models have been added: • MATD032 – Auto glass • MATD058 – Composites and fabrics • MATD067 – Nonlinear Elastic Discrete Beam • MATD068 – Nonlinear Plastic Discrete Beam • MATD069 – SID Damper Discrete Beam • MATD070 – Hydraulic Gas Damper Discrete Beam • MATD071 – Cable Discrete Beam • MATD073 – Urethane foam • MATD074 – Elastic Spring Discrete Beam • MATD076 – Viscoelastic • MATD083 – Low and medium density foams • MATD087 – Cellular Rubber • MATD093 – Elastic 6DOF Spring Discrete Beam

62 MD Nastran 2006 Release Guide

• MATD094 – Inelastic Spring Discrete Beam • MATD095 – Inelastic 6DOF Spring Discrete Beam • MATD097 – General Joint Discrete Beam • MATD119 – General Nonlinear 6DOF Discrete Beam • MATD121 – General Nonlinear 1DOF Discrete Beam • MATD126 – Modified Honeycomb • MATDB01 – Seatbelt Material • MATDHP – Hyperelastic - Mooney Rivlin • MATDS03 – Elastoplastic Spring Material • MATDS04 – Nonlinear Elastic Spring Material • MATDS05 – Nonlinear Viscous Damper Material • MATDS06 – General Nonlinear Spring Material • MATDS07 – Maxwell Viscoelastic Spring Material • MATDS08 – Inelastic Spring Material • MATDS13 – Tri-Linear Degrading Material • MATDS14 – Squat Shear wall Material • MATDS15 – Muscle Material

The scripts used to execute the explicit solution were improved for parallel runs when different computers are involved. It is recommended that only the same type of computers running the same O/S be used with the exception that different O/S’s may be used in certain cases for Linux systems and different versions of Windows may be used with PC’s. For such systems, a hostlist needs to be setup with the format: Hostname1 #cpus1 workdir1 exe1 Hostname2 #cpus2 workdir2 exe2 Hostname3 #cpus3 workdir3 exe3 etc. • If exe3 is blank, it is assumed that the exe on node 3 is at the same location as node 1 • workdir(i) is not used but is added for compatibility with SOL 600 and other MSC products. A

dummy entry needs to be made if exe(i) is required • Multiple CPU runs using a machine with several cpu’s in the same box do not require a hostlist • See the SOL 700,ID (p. 175) in the MD Nastran Quick Reference Guide for more details • Two ways of specifying dynamic loads are available using PARAM,DYDYLOAD. The first

method is to translate the loads in MD Nastran. The second method is to pass the loads directly to the explicit solution which has improved capabilities to handle these loads. A description of this parameter follows: PARAM,DYDYLOAD,IFLAG (Integer, Default = 1)

CHAPTER 2 63 Nonlinear Analysis

Determines if MD Nastran dynamic loads are passed directly to the explicit solution or translated by the internal translator in MD Nastran. 1. Dynamic loads are translated by the internal translator in MD Nastran. 2. Dynamic loads are passed directly to the explicit solution. For this option to work properly, if loads other than what is listed below are used, the job may fail or obtain the wrong results. Case Control DLOAD LOADSET LOAD (dynamic relaxation only) Bulk Data LSEQ DLOAD DELAY LOAD (dynamic relaxation only) DAREA TLOAD1 TABLED1, TABLED2, TABLED3 FORCE FORCE2 MOMENT MOMENT2 GRAV PLOAD PLOAD4 RFORCE (CID, METHOD, RACC, MB fields are not available) SPCD Note: 1. This parameter may be placed in rc files. Error diagnostics have been improved. You should examine files jid.dytr_prep.d3hsp, jid.dytr_prep.out and jid.dytr.d3hsp for the string “Error” as well as the standard files jid.f06 (search for FATAL and Severe Warning”) and jid.log (look for anything unusual) should a job not run to completion. The following new Bulk Data entries have been added: • ACCMETR – Define seat belt an accelerometer • BCGRID – Define grid points to be included as slave body contact entity

64 MD Nastran 2006 Release Guide

• BCSEG – Define grid points which are part of an element to be used in contact analyses • CBELT – Define a Seatbelt Element • DYDELEM – Delete failed elements and continue analysis • DYTERMT – Terminate the job depending on user-specified conditions (such as failed

elements) • DYRELAX – Dynamic relaxation specifications for restart runs • DYCHANG – Boundary changes for restart runs • D2R0000 – Switch standard materials to rigid materials • D2RINER – Define inertial properties for materials switch to rigid materials • PBELTD - Define section properties for the seat belt elements • R2RAUTO – Switch parts to rigid materials • RBE2F – Define nodal constraint sets for translational motion in global coordinates • RCONN – Defines a rigid connection between the different parts of Lagrangian meshes • SBPRET – Defines a seat belt pretensioner • SBRETR – Defines a seat belt retractorBSENSR – Defines a seat belt sensor • SBSLPR – Define seat belt slip ring • SPCD2 – Define an imposed nodal motion on a node or a set of nodes.

The following Bulk Data entries have been changed or additions have been made • CELAS2D • PBARL (now available for SOL 700) • RESTART (new options added) • DYPST1, DYPST2, DYPST3, DYPST4, DYPST5 (Bulk Data entries for d3plot to op2). • WALLGEO – Defines a geometric rigid wall

The following SOL 700 parameters have been added or revised: • CWLDIGNR • SCALEMASS • STEPFCT • DYELPLSY • DYELPLET • DYELPLFL • DYELAS1C • DYELAS1F • DYELAS1R • DYDTOUT

CHAPTER 2 65 Nonlinear Analysis

• DYDYLOAD • DYPARAM,ELDLTH • DYPARAM,LSDYNA,BINARY • DYPARAM,LSDYNA,DB-EXTENT • DYPARAM,LSDYNA,HOURGLASS • DYPARAM,LSDYNA,OUTPUT • DYPARAM,LSDYNA,RELAX

Example: Projectile Hitting a Plate with Failure One typical example of SOL 700 Phase 1 is a projectile hitting a plate at an oblique angle. The initial velocity of the projectile is large enough that over time various elements in the plate fail. Depending on the postprocessor used, if it can account for failed elements, the failed elements are removed from the model. This model involves contact between the projectile and the plate. SOL 600-style contact is used. It also involves the use of LS-DYNA material MATD024 (elastoplastic material with arbitrary stress- strain curves and strain-rate dependency). This model with close to 8000 grid points requires about 20 minutes to run on a 2.4 GHz PC. The following plots show the evolution of the effective stress and damage with time:

66 MD Nastran 2006 Release Guide

CHAPTER 2 67 Nonlinear Analysis

Portions the MD Nastran input file named projtl.dat are shown and discussed below: SOL 700,NLTRAN path=1 stop=1 TIME 10000 CEND ECHO = NONE DISPLACEMENT(SORT1,print,PLOT) = ALL Stress(SORT1,PLOT) = ALL Strain(SORT1,PLOT) = ALL accel(print,plot)= ALL velocity(print,plot)= ALL echo=both SPC = 2 IC=1 TSTEPNL = 20 BCONTACT = 1 weightcheck=yes page BEGIN BULK TSTEPNL 20 10 11 1 5 10 + + +

68 MD Nastran 2006 Release Guide

+ 0 PARAM,DYDTOUT,5 PARAM*,DYCONSLSFAC,1.0 PARAM,OGEOM,NO PARAM,AUTOSPC,YES PARAM,GRDPNT,0 param,dyendtim,1 param,dymats1,1 param,dyldknd,0 $ BCTABLE 1 4 SLAVE 3 + YES MASTER 4 $ BCBODY 3 3 DEFORM 3 0 BCBODY 4 3 DEFORM 4 0 $ BCPROP 3 2 BCPROP 4 1 $ $ $ ========== PROPERTY SETS ========== $ $ * projectile * $ PSOLID 1 1 $ $ * plate * $ PSOLID 2 2 $ $ $ ========= MATERIAL DEFINITIONS ========== $ $ $ $ -------- Material MAT_PLASTIC_KINE.2 id =2 MATD024 1 18.62 1.17 .22 0.0179 0.8 $ -------- Material MAT_PLASTIC_KINE.1 id =1 MATD024 2 7.896 2.1 .284 0.01 0.8 $ $ $ $ ======== Load Cases ======================== $ $ $ ------- Initial Velocity BC ini ----$ TICD 1 1 1 0.1246 2586 1 TICD 1 1 3 -0.03339 2586 1 . . . ENDDATA

All of the previous input data are described in the MD Nastran Quick Reference Guide and summarized above. Note that it was only necessary to add BCONTACT=1 to the Case Control, a few new Bulk Data

CHAPTER 2 69 Nonlinear Analysis

parameters and a few contact entries to the Bulk Data to an existing file that would be used in MD Nastran SOL 101, 106, 109 or 129 analyses.

Example: Pickup Truck Crash Test Another example involves crash testing of a pickup truck against a rigid wall. The input data file for this example is quite large and can be provided on request. It is a typical example of what can be done using a full car or truck model, developed originally for NVH analysis and subsequently used for SOL 700 for crash simulation.

70 MD Nastran 2006 Release Guide

Example – 3 Car Crash Simulation This is an example of a large model simulating the 3 car crash scenario. The model was taken from topcrunch.org –site (http://www.topcrunch.org/benchmark_results.sfe). The original model was in LS-DYNA key-file which was translated to MD Nastran format to be run by SOL 700. The original model was corrected to include the contact definition between the front and rear cars and the road. The model size information and results are shown below:

CHAPTER 2 71 Nonlinear Analysis

Where Can I Find More Information: MD Nastran Explicit Nonlinear Analysis, SOL 700, is documented in the following manuals and guides: • MD Nastran Quick Reference Guide • MD Nastran Explicit Nonlinear User’s Guide • MSC.Patran User’s Guide • MSC.Patran – MD Nastran and MSC.Dytran Preference Guides • LS-DYNA Keyword User’s Manual, Version 970 (available from LSTC) • LS-DYNA Theoretical Manual (available from LSTC)

72 MD Nastran 2006 Release Guide

MD Nastran 2006 Release Guide Ch. :

3

Numerical Enhancements

J

New Iterative Solver Option, 74

J

MDACMS Enhancements, 83

J

MPYAD Method 1 Enhancement, 90

J

Improved Robustness in the Lanczos Method, 91

J

MLDMP in Solution 111 (Pre-Release), 92

74 MD Nastran 2006 Release Guide

New Iterative Solver Option Introduction Static structural analyses of very large solid element models pose difficult computational challenges for the solvers available in MD Nastran. For most modeling situations, the sparse direct solver is the solver of choice because it is usually the most efficient. However, as the number of degrees of freedom grows ever larger, iterative solution methods become more attractive since they tend to produce results faster than the direct method. For this reason, both solution techniques are available in MD Nastran. In order to increase performance even more in the iterative method, the solver offered by Computational Applications and System Integration, Inc. (CASI) is being introduced into MD Nastran.

Benefits The introduction of the element-based iterative solver option allows users to run larger jobs faster and with fewer resources (memory and disk) than could be done before. It is anticipated that most jobs will run at least twice as fast when the element-based solver option is specified compared to jobs run with any of the existing MD Nastran iterative solver pre-conditioner choices. For very large jobs, the performance could be up to ten times better.

Method and Theory Until now, the iterative solution technique in MD Nastran has been matrix-based, meaning that the process does not use any element topology information to assist in the solution. The iterative solver operates on the same matrices that are processed by the direct solver. The element-based iterative solver on the other hand, uses finite element topology and element stiffness matrices directly to obtain the solution. Using this information generally results in smaller pre-conditioners that take less time to factor and that have more model – specific “information”, as a result, fewer conjugate gradient iterations are required to arrive at a converged solution compared to matrix-based techniques. Convergence for the element-based iterative solver is achieved when the value of one of four norms falls below the specified convergence tolerance (the default value is 1.0e-04) and the values of all four norms have fallen below a slightly looser tolerance. To define the norms, let • b be the original right-hand-side • A be the global system matrix • M be the pre-conditioner • x be the solution at the current step • r be the current residual • || || denote 2-norm • | | denote infinity norm • ∆x denote the change in current solution x at a particular step.

CHAPTER 3 75 Numerical Enhancements

Then, the four norms are defined as follows: 1. Reduction in 2-norm of residual r N1 = -------b 2. Reduction in infinity norm of residual r N2 = -----b 3. Reduction in preconditioned norm of residual N3 =

T

–1

T

–1

r M r ⁄ b M b

4. Estimate of normalized energy norm of error in solution N4 =

T

T

( ∆x A∆x ) ⁄ ( x Ax )

Inputs The SMETHOD Case Control command must be used to select the iterative solver. The SMETHOD command has been enhanced to allow selection of either the existing matrix-based technique or the new element-based technique directly, accepting all default options. This is accomplished by specifying SMETHOD=MATRIX to invoke the existing matrix-based iterative solution technique and SMETHOD=ELEMENT to invoke the new element-based iterative solution technique. The SMETHOD command also accepts the specification of an integer value representing the ID of an ITER Bulk Data entry. In this way, default options can be changed. The PRECOND field of the ITER Bulk Data entry accepts the keyword “CASI” to indicate that the element-based solver is to be used.

Outputs There is no new MD Nastran output produced by the element-based iterative solver. The intermediate convergence parameter output produced by the MSGFLG=YES option of the ITER Bulk Data entry contains the values of the four convergence norms at each iteration. A summary file is produced by the element-based iterative solver that contains various statistics about the solution process. The file name uses the Job ID (jid.PCS), where jid is the name of the input data file.

76 MD Nastran 2006 Release Guide

Guidelines and Limitations The element-based iterative solver is intended for very large static structural analysis models composed mainly of 10 node CTETRA elements. It generally out-performs the direct solver when the problem size exceeds one million degrees of freedom and will out-perform the matrix-based iterative solver when the problem size reaches approximately three million degrees of freedom. The element-based solver is intended for a very specific set of model characteristics. As such, the following limitations apply: • Available in linear static structural analysis (SOL 101) only • No GENEL elements allowed • No K2GG direct input matrix selection allowed • No ASET/OMIT reduction allowed • No SUPORTi allowed • No SCALAR points (explicitly or implicitly defined) allowed • No heat transfer allowed • No p-elements allowed • Only BAR, BEAM, BUSH, ROD, CONROD, ELAS1, ELAS2, SHEAR, QUAD4, QUAD8,

QUADR, TRIA3, TRIA6, TRIAR, TETRA, PENTA and HEXA elements are allowed

Demonstration Example A simple example is presented that demonstrates the use of the element-based iterative solver. The ITER Case Control command is used to specify the element-based iterative solver. The example problem is used for demonstration purposes only and is not representative of anything in particular. The model data consists of a simple solid brick structure subject to an end load.

Example Input Data ID CASI,DEMO SOL 101 TIME 10000 CEND ECHO = NONE DISPLACEMENT = ALL smethod = element SUBCASE = 1 SPC = 1 LOAD = 1 BEGIN BULK iter,1000,,,,,,,,+it1 +it1 precond=casi PARAM,AUTOSPC,YES GRID, 1,, 0.00,0.00,0.00 GRID, 2,, 0.00,1.00,0.00 GRID, 3,, 0.00,0.00,0.50 GRID, 4,, 0.00,1.00,0.50 GRID, 5,, 1.25,0.00,0.00

CHAPTER 3 77 Numerical Enhancements

GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID, GRID,

6,, 1.25,1.00,0.00 7,, 1.25,0.00,0.50 8,, 1.25,1.00,0.50 9,, 2.50,0.00,0.00 10,, 2.50,1.00,0.00 11,, 2.50,0.00,0.50 12,, 2.50,1.00,0.50 13,, 3.75,0.00,0.00 14,, 3.75,1.00,0.00 15,, 3.75,0.00,0.50 16,, 3.75,1.00,0.50 17,, 5.00,0.00,0.00 18,, 5.00,1.00,0.00 19,, 5.00,0.00,0.50 20,, 5.00,1.00,0.50 21,, 6.25,0.00,0.00 22,, 6.25,1.00,0.00 23,, 6.25,0.00,0.50 24,, 6.25,1.00,0.50 25,, 7.50,0.00,0.00 26,, 7.50,1.00,0.00 27,, 7.50,0.00,0.50 28,, 7.50,1.00,0.50 29,, 8.75,0.00,0.00 30,, 8.75,1.00,0.00 31,, 8.75,0.00,0.50 32,, 8.75,1.00,0.50 33,,10.00,0.00,0.00 34,,10.00,1.00,0.00 35,,10.00,0.00,0.50 36,,10.00,1.00,0.50 37,, 0.00,0.50,0.00 38,, 0.00,0.50,0.50 39,, 1.25,0.50,0.00 40,, 1.25,0.50,0.50 41,, 2.50,0.50,0.00 42,, 2.50,0.50,0.50 43,, 3.75,0.50,0.00 44,, 3.75,0.50,0.50 45,, 5.00,0.50,0.00 46,, 5.00,0.50,0.50 47,, 6.25,0.50,0.00 48,, 6.25,0.50,0.50 49,, 7.50,0.50,0.00 50,, 7.50,0.50,0.50 51,, 8.75,0.50,0.00 52,, 8.75,0.50,0.50 53,,10.00,0.50,0.00 54,,10.00,0.50,0.50 55,, 0.00,0.00,0.25 56,, 0.00,1.00,0.25 57,, 1.25,0.00,0.25 58,, 1.25,1.00,0.25 59,, 2.50,0.00,0.25 60,, 2.50,1.00,0.25 61,, 3.75,0.00,0.25 62,, 3.75,1.00,0.25 63,, 5.00,0.00,0.25 64,, 5.00,1.00,0.25 65,, 6.25,0.00,0.25

78 MD Nastran 2006 Release Guide

GRID, 66,, 6.25,1.00,0.25 GRID, 67,, 7.50,0.00,0.25 GRID, 68,, 7.50,1.00,0.25 GRID, 69,, 8.75,0.00,0.25 GRID, 70,, 8.75,1.00,0.25 GRID, 71,,10.00,0.00,0.25 GRID, 72,,10.00,1.00,0.25 GRID, 73,, 0.625,0.00,0.00 GRID, 74,, 0.625,1.00,0.00 GRID, 75,, 0.625,0.00,0.50 GRID, 76,, 0.625,1.00,0.50 GRID, 77,, 1.875,0.00,0.00 GRID, 78,, 1.875,1.00,0.00 GRID, 79,, 1.875,0.00,0.50 GRID, 80,, 1.875,1.00,0.50 GRID, 81,, 3.125,0.00,0.00 GRID, 82,, 3.125,1.00,0.00 GRID, 83,, 3.125,0.00,0.50 GRID, 84,, 3.125,1.00,0.50 GRID, 85,, 4.375,0.00,0.00 GRID, 86,, 4.375,1.00,0.00 GRID, 87,, 4.375,0.00,0.50 GRID, 88,, 4.375,1.00,0.50 GRID, 89,, 5.625,0.00,0.00 GRID, 90,, 5.625,1.00,0.00 GRID, 91,, 5.625,0.00,0.50 GRID, 92,, 5.625,1.00,0.50 GRID, 93,, 6.875,0.00,0.00 GRID, 94,, 6.875,1.00,0.00 GRID, 95,, 6.875,0.00,0.50 GRID, 96,, 6.875,1.00,0.50 GRID, 97,, 8.125,0.00,0.00 GRID, 98,, 8.125,1.00,0.00 GRID, 99,, 8.125,0.00,0.50 GRID,100,, 8.125,1.00,0.50 GRID,101,, 9.375,0.00,0.00 GRID,102,, 9.375,1.00,0.00 GRID,103,, 9.375,0.00,0.50 GRID,104,, 9.375,1.00,0.50 GRID,105,, 0.625,0.00,0.25 GRID,106,, 0.625,1.00,0.25 GRID,107,, 1.875,0.00,0.25 GRID,108,, 1.875,1.00,0.25 GRID,109,, 3.125,0.00,0.25 GRID,110,, 3.125,1.00,0.25 GRID,111,, 4.375,0.00,0.25 GRID,112,, 4.375,1.00,0.25 GRID,113,, 5.625,0.00,0.25 GRID,114,, 5.625,1.00,0.25 GRID,115,, 6.875,0.00,0.25 GRID,116,, 6.875,1.00,0.25 GRID,117,, 8.125,0.00,0.25 GRID,118,, 8.125,1.00,0.25 GRID,119,, 9.375,0.00,0.25 GRID,120,, 9.375,1.00,0.25 GRID,121,, 0.625,0.50,0.00 GRID,122,, 0.625,0.50,0.50 GRID,123,, 1.875,0.50,0.00 GRID,124,, 1.875,0.50,0.50 GRID,125,, 3.125,0.50,0.00

CHAPTER 3 79 Numerical Enhancements

GRID,126,, 3.125,0.50,0.50 GRID,127,, 4.375,0.50,0.00 GRID,128,, 4.375,0.50,0.50 GRID,129,, 5.625,0.50,0.00 GRID,130,, 5.625,0.50,0.50 GRID,131,, 6.875,0.50,0.00 GRID,132,, 6.875,0.50,0.50 GRID,133,, 8.125,0.50,0.00 GRID,134,, 8.125,0.50,0.50 GRID,135,, 9.375,0.50,0.00 GRID,136,, 9.375,0.50,0.50 GRID,137,, 0.000,0.50,0.25 GRID,138,, 1.250,0.50,0.25 GRID,139,, 2.500,0.50,0.25 GRID,140,, 3.750,0.50,0.25 GRID,141,, 5.000,0.50,0.25 GRID,142,, 6.250,0.50,0.25 GRID,143,, 7.500,0.50,0.25 GRID,144,, 8.750,0.50,0.25 GRID,145,,10.000,0.50,0.25 GRID,146,, 0.625,0.50,0.25 GRID,147,, 1.875,0.50,0.25 GRID,148,, 3.125,0.50,0.25 GRID,149,, 4.375,0.50,0.25 GRID,150,, 5.625,0.50,0.25 GRID,151,, 6.875,0.50,0.25 GRID,152,, 8.125,0.50,0.25 GRID,153,, 9.375,0.50,0.25 CTETRA 1 1 55 105 CTETRA 2 1 105 73 CTETRA 3 1 146 76 CTETRA 4 1 137 73 CTETRA 5 1 121 106 CTETRA 6 1 121 74 CTETRA 7 1 57 107 CTETRA 8 1 107 77 CTETRA 9 1 147 80 CTETRA 10 1 138 77 CTETRA 11 1 123 108 CTETRA 12 1 123 78 CTETRA 13 1 59 109 CTETRA 14 1 109 81 CTETRA 15 1 148 84 CTETRA 16 1 139 81

1 122 1 146 4 40 1 121 2 76 2 58 5 124 5 147 8 42 5 123 6 80 6 60 9 126 9 148 12 44 9 125

4 75 4 57 7 138 2 146 4 138 8 39 8 79 8 59 11 139 6 147 8 139 12 41 12 83 12 61 15 140 10 148

3

7

137

38

7

5

137

122

5

8

122

57

4

5

37

56

5

8

56

146

5

6

106

138

7

11

138

40

11

9

138

124

9

12

124

59

8

9

39

58

9

12

58

147

9

10

108

139

11

15

139

42

15

13

139

126

13

16

126

61

12

13

41

60

80 MD Nastran 2006 Release Guide

CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA CTETRA

17 125 18 125 19 61 20 111 21 149 22 140 23 127 24 127 25 63 26 113 27 150 28 141 29 129 30 129 31 65 32 115 33 151 34 142 35 131 36 131 37 67 38 117 39 152 40 143 41 133 42 133 43 69 44 119 45 153 46 144

1 110 1 82 1 111 1 85 1 88 1 85 1 112 1 86 1 113 1 89 1 92 1 89 1 114 1 90 1 115 1 93 1 96 1 93 1 116 1 94 1 117 1 97 1 100 1 97 1 118 1 98 1 119 1 101 1 104 1 101

10 84 10 62 13 128 13 149 16 46 13 127 14 88 14 64 17 130 17 150 20 48 17 129 18 92 18 66 21 132 21 151 24 50 21 131 22 96 22 68 25 134 25 152 28 52 25 133 26 100 26 70 29 136 29 153 32 54 29 135

12 140 16 43 16 87 16 63 19 141 14 149 16 141 20 45 20 91 20 65 23 142 18 150 20 142 24 47 24 95 24 67 27 143 22 151 24 143 28 49 28 99 28 69 31 144 26 152 28 144 32 51 32 103 32 71 35 145 30 153

13

16

60

148

13

14

110

140

15

19

140

44

19

17

140

128

17

20

128

63

16

17

43

62

17

20

62

149

17

18

112

141

19

23

141

46

23

21

141

130

21

24

130

65

20

21

45

64

21

24

64

150

21

22

114

142

23

27

142

48

27

25

142

132

25

28

132

67

24

25

47

66

25

28

66

151

25

26

116

143

27

31

143

50

31

29

143

134

29

32

134

69

28

29

49

68

29

32

68

152

29

30

118

144

31

35

144

52

35

33

144

136

33

36

136

71

32

33

51

70

CHAPTER 3 81 Numerical Enhancements

CTETRA CTETRA

47 135 48 135 1

1 120 1 102 1

PSOLID MAT1,1,1.0 SPC1,1,456,1,THRU,153 SPC 1 1 SPC 1 2 SPC 1 3 SPC 1 4 SPC 1 55 SPC 1 56 SPC 1 37 SPC 1 38 SPC 1 137 PLOAD4* 1 * 1.000000000E+00 * 0 * PLOAD4* 1 * 1.000000000E+00 * 0 * ENDDATA

30 104 30 72 0 123 123 123 123 123 123 123 123 123

32 145 36 53

33

36

70

153

33

34

120

145

0. 0. 0. 0. 0. 0. 0. 0. 0.

48 1.000000000E+00 1.000000000E+00* 1.000000000E+00 33 30* 1.000000000E+00 0.000000000E+00 0.000000000E+00* 45 1.000000000E+00 1.000000000E+00* 1.000000000E+00 33 32* 1.000000000E+00 0.000000000E+00 0.000000000E+00*

Example Output The output generated consists of the usual MD Nastran output as well as an output file generated by the element-based iterative solver. The contents of this file summarize various statistics about the solution process. Some of the statistics include the number of terms in the various matrices, number of degrees of freedom, number of iterations taken and convergence parameter values. The file will have a suffix of .PCS and appear in the same location as other output files produced by the job. The contents of the .PCS file for the example problem are shown here for reference. **************************************************************************** ** (C) Copyright 1992-2004 Computational Applications and System Integration Inc. All rights Reserved. **************************************************************************** ** Job:./v2006rgat:Wed Oct 12 10:30:35 2005 **************************************************************************** ** ESTIMATED MEMORY (MB): 0.094738 Preallocated Virtual Memory : 27.3828 MB Virtual Memory Used : 1.96344 MB **************************************************************************** ** **************************************************************************** **

82 MD Nastran 2006 Release Guide

(C) Copyright 1992-2004 Computational Applications and System Integration Inc. All rights Reserved. **************************************************************************** ** Job:./v2006rgat:Wed Oct 12 10:30:36 2005 Degrees of Freedom: 459 DOF Constraints: 27 Elements: 48 Assembled: 0 Implicit: 48 Nodes: 153 Number of Load Cases: 1 Nonzeros in Upper Triangular part of Global Stiffness Matrix : 0 Nonzeros in Preconditioner: 8298 *** Precond Reorder: MLD *** Nonzeros in V: 2160 Nonzeros in factor: 5220 *** Primal Preconditioner Activated *** VTAeV:uTime:0 Sec:sTime:0 Sec Total Operation Count: 851878 Total Iterations In PCG: 8 Average Iterations Per Load Case: 8.000000 Input PCG Error Tolerance: 1e-04 Achieved PCG Error Tolerance: 5.81869e-05 DETAILS OF SOLVER CP TIME(secs)User System Assembly0 0 Preconditioner Construction0 0 Preconditioner Factoring0 0 Preconditioned CG0 0 **************************************************************************** ** Total PCG Solver CP Time: User: 0 secs: System: 0 secs **************************************************************************** ** Available Physical Memory (RAM) : 0 MB Estimate of Memory Usage In CG : 0.080898 MB Estimate of Disk Usage : 0.09228 MB Preallocated Virtual Memory : 27.3828 MB Virtual Memory Used : 4.16164 MB *** Implicit Matrix Multiplication Activated : Mode 3 *** **************************************************************************** ** Multiply with A time in decisecs 0 Precond solve time in decisecs 0 **************************************************************************** ** Total Elapsed Time (Secs): 1 **************************************************************************** **

CHAPTER 3 83 Numerical Enhancements

MDACMS Enhancements Background Matrix Domain Automated Component Modal Synthesis (MDACMS) is now the default ACMS method. The older Geometric Domain approach (GDACMS) remains available but is not the recommended ACMS method. The PARTOPT keyword on the DOMAINSOLVER Executive System command is used to choose between the Geometric and Matrix (or DOF) domains: PARTOPT=DOF is now the default for ACMS.

Summary The primary goal of development of MD Nastran 2006 MDACMS is to improve performance by reducing disk I/O and Executive System overhead. Generally, this is achieved by allowing Nastran to utilize memory more effectively than in the past. In addition, several subDMAPs have been consolidated into a single new DMAP module. Specific enhancements to the MDACMS capability include the following: • The ability to specify key scratch datablocks for Scratch Memory (SMEM) residence via a new

FMS command: MEMLIST. • Introduction of a new module to perform functions in support of residual vector calculations:

the RESMOD module. • Enhancements to matrix multiply-and-add (MPYAD module) Method 1.

New FMS Command: MEMLIST The File Management Section (FMS) has been enhanced to include a new MEMLIST command, described below. The purpose of the MEMLIST command is to limit the use of Scratch Memory (SMEM) to a subset of Nastran scratch datablocks. In this way, the effectiveness of SMEM increases to the extent that the user knows which scratch datablocks are likely to be accessed most often. A pre-defined MEMLIST command has been created and is available in the form of an INCLUDE file. This file is delivered in the SSSALTERDIR directory, which is available when a full Nastran installation has been performed. In order to access this file, specify the following INCLUDE command in the FMS Section of the input file: INCLUDE

‘SSSALTERDIR:memlist.acms’

This file lists scratch datablocks that will reduce the disk I/O by a significant amount, provided that enough Scratch Memory has been specified. The following is the MD Nastran Quick Reference Guide description of the MEMLIST command.

84 MD Nastran 2006 Release Guide

MEMLIST

Specify Datablocks Eligible for SMEM

Specify a list of scratch datablocks that may reside in scratch memory (SMEM). Format: MEMLIST DATABLK = (DBname1, DBname2, ..., DBnamei) Describer

Meaning

DBnamei

Name of a MD Nastran datablock.

Remarks: 1. Only NDDL and local scratch datablocks may be included in MEMLIST specification. 2. Datablocks specified will reside in SMEM on a first come, first served basis. 3. Datablocks not specified by this command will not reside in SMEM. 4. Database directories for the SCRATCH DBset reside in SMEM and are not affected by any MEMLIST specification. 5. Continuation lines are allowed. 6. Multiple MEMLIST commands are honored. 7. Scratch I/O activity is reported in the F04 file by including DIAG 42 in the Executive Section. Example: MEMLIST DATABLK = (KOO, MOO, KQQ, MQQ) If generated, datablocks KOO, MOO, KQQ, and MQQ will reside in scratch memory. All other datablocks will be excluded from scratch memory.

New Module: RESMOD The ACMS process entails computing residual vectors at each automatically generated component. Each step taken during residual vector calculations is carried out by a particular subDMAP call. In order to streamline the DMAP and reduce Executive System overhead, the RESMOD module has been developed for MD Nastran 2006. The RESMOD module is only invoked during MDACMS operations, when the size of the vectors is relatively small, which is a characteristic of MDACMS computations. The module syntax is similar to the MATMOD module, since the first parameter (P1) defines the operation to be performed. However, unlike MATMOD, P1 is a character pneumonic instead of an integer code value. The complete DMAP description is below.

CHAPTER 3 85 Numerical Enhancements

RESMOD

RESVEC Calculations

Perform linear algebra functions to support residual vector calculations. Format: RESMOD

I1,I2,I3,I4,I5/O1,O2,O2,O3,O4,O5/P1/P2/P3/P4/P5/P6 $

Input Data Blocks: Ii:

Input data blocks. I1 is required. I2 through I5 may not be necessary depending on the value of P1.

Output Data Blocks: Oi

Output data blocks.

Parameters: P1

Input-character-no default. Option selection described in the table below.

P2,P3,P4

Input-integer-default=0. Integer parametric data depending on P1.

P5,P6

Input-real-default=0.0. Real parametric data depending on P1.

Remark: Each option corresponds to a different value of the first parameter, P1, as follows.

P1 Value

Brief Description

‘ATBC’

Performs [A] [B][C] if [C] present; [A]T[B][A] otherwise

‘MPART’

Partitions stiffness, mass, and eigenvector matrices based on mass content

‘LININD’

Find linearly independent and dependent vectors of a matrix

‘LDSWEEP’

Sweeps “modal” loads for load vectors

‘USWEEP’

Sweeps a matrix for small vectors

T

Details for each option are given in the following sections.

86 MD Nastran 2006 Release Guide

Option P1 = ‘ATBC’ Performs the matrix multiplication [I1]T[I2][I3] if [I3] is present; [I1]T[I2][I1] otherwise. Format: RESMOD

I1,I2,I3,,/O1,,,,/’ATBC’ $

Input Data Blocks: I1,I2,I3

Any matrix data blocks.

Output Data Blocks: O1

Matrix product.

Remark: [I2] is assumed to be symmetric. Example: Compute the product [D] = [A] T [B] [C]

RESMOD

A,B,C,,/D,,,,/’ATBC’ $

Option P1 = ‘MPART’ Partitions stiffness, mass, and eigenvector matrices based on mass content. Format: RESMOD

PHI,K,M,,/PHI0,K0,PHI1,M1,K1/’MPART’////ZROSTIFF/ZROMASS $

Input Data Blocks: PHI

A set of eigenvectors.

K

Stiffness matrix associated with [PHI].

M

Mass matrix associated with [PHI].

CHAPTER 3 87 Numerical Enhancements

Output Data Blocks: PHI0

Massless eigenvectors.

K0

Stiffness associated with [PHI0].

PHI1

Eigenvectors which contain mass.

M1

Mass associated with [PHI1].

K1

Stiffness associated with [PHI1].

Parameters: ZROSTIFF

Input-real-default=1.0E-8. Null stiffness filter criteria.

ZROMASS

Input-real-default=1.0E-16. Null mass filter criteria.

Remark: Only real matrices are supported.

Option P1 = ‘LININD’ Partitions a matrix into linearly independent and dependent sets. Format: RESMOD

U,M,,,/U0,U1,,,/’LININD’////ZROVEC $

Input Data Blocks: U

Any real matrix.

M

Mass matrix associated with [U].

Output Data Blocks: U0

Linearly dependent vector set from [U].

U1

Linearly independent vector set from [U].

Parameters: ZROVEC

Input-real-default=1.0E-6. Null filter criteria.

88 MD Nastran 2006 Release Guide

Remarks: 1. M may be purged, in which case the identity matrix is assumed. 2. Output matrices [U0] and [U1] should satisfy the following conditions: T

[ U0 ] [ M ] [ U0 ] = computational zeros T

[ U1 ] [ M ] [ U0 ] > 0.0 3. Only real matrices are supported.

Option P1 = ‘LDSWEEP’ Sweeps “modal” loads for load vectors. Format: RESMOD

LD,PHI,MXX,MQQ,/LDIND,,,,/’LDSWEEP’/NORMFLG $

Input Data Blocks: LD

A set of load vectors.

PHI

Modal vectors.

MXX

Mass matrix, physical degrees of freedom.

MQQ

Mass matrix, modal degrees of freedom.

Output Data Blocks: LDIND

Filtered load vectors.

Parameters: NORMFLG

Input-integer-default=0. Normalization flag. Set to –1 to unit normalize load vectors.

Remarks: 1. The filtered load vectors are: T

T

[ LDIND ] = [ LD ] – [ M ] [ PHI ] ⋅ INV ( [ PHI ] [ M ] [ PHI ] ) ⋅ [ PHI ] [ LD ] 2. Only real matrices are supported.

CHAPTER 3 89 Numerical Enhancements

Option P1 = ‘USWEEP’ Sweeps a matrix for small vectors. Format: RESMOD

U,PHI,MXX,MQQ,/UIND,,,,/’USWEEP’/NORMFLG $

Input Data Blocks: U

A set of vectors.

PHI

Modal vectors.

MXX

Mass matrix, physical degrees of freedom.

MQQ

Mass matrix, modal degrees of freedom.

Output Data Blocks: UIND

Filtered vectors.

Parameters: NORMFLG

Input-integer-default=0. Normalization flag. Set to –1 to unit normalize input vectors.

Remarks: 1. The filtered vectors are: T

[ UIND ] = [ U ] – INV ( [ PHI ] [ MQQ ] [ PHI ] ) ⋅ [ MXX ] ⋅ [ U ] 2. Only real matrices are supported.

90 MD Nastran 2006 Release Guide

MPYAD Method 1 Enhancement The Storage 3 option of matrix multiply and add (MPYAD) module Method 1 has been enhanced remove null rows of the [B] matrix, where [B] is the second matrix in the matrix product [ D ] = ±[ A ] [ B ] ±[ C ] This results in a reduction of the number of operations necessary to complete the matrix multiply. MPYAD Method 1 Storage 3 is frequently invoked during MDACMS reduction operations.

Example This example demonstrates the potential impact of these enhancements.

Problem Definition: • Acoustic Analysis (modal frequency response, SOL 111) • Over 600,000 grid points; 3.5 million degrees of freedom • Over 4,000 structure modes up to 600 Hertz; 200 fluid modes • 12 load cases; over 700 forcing frequencies

Machine Resources • Linux IA64 with 12Gb main memory • HP DS2100 3-way striped scratch disk

Version

Elap (sec)

CPU (sec)

Total I/O (gb)

HiWater Disk (gb)

MSC.Nastran 2005 r2

12472

10734.3

37.303

1501.81

MD Nastran 2006

9369

8239.3

31.873

684.402

Speedup

24.88%

23.24%

14.56%

54.43%

The MSC.Nastran 2005 r2 run was made with one gigabyte of memory (“mem=1gb”). The MD Nastran 2006 run was made using “mem=8gb smem=7gb”. This resulted in the same Open Core size (1gb) but with 7gb memory devoted to SMEM. The standard MEMLIST specification found in SSSALTER:memlist.acms was used for MD Nastran 2006. Finally, both runs utilized serial processing.

CHAPTER 3 91 Numerical Enhancements

Improved Robustness in the Lanczos Method A new feature in the READ module is used to scale some intermediate quantities computed during the Lanczos procedure. The effect is a more stable factorization, with a lower MAT RATIO, particularly when Lagrange multipliers are used. In practical examples, this feature has reduced max ratios by six orders of magnitude. This feature may be disabled by setting system cell 166 to 48.

92 MD Nastran 2006 Release Guide

MLDMP in Solution 111 (Pre-Release) The Multi-Level Distributed Memory Parallel (MLDMP) option is available for solution 111 in prerelease status. This option generates eigenvectors using the Lanczos method in a hierarchic parallel fashion. That is, the frequency range is divided into a user-specified number of segments, and each segment is assigned to a logical group or cluster of processors. The modes in each segment are computed in parallel, and in turn, each cluster uses a matrix-based domain decomposition to compute the modes for its segment in parallel. The new option provides improved scaling across a larger number of processors.

User Interface The MLDMP option may be selected by specifying DOMAINSOLVER MODES (PARTOPT=DOF) in the Executive Control Section of the input file, and then using the DMP and NCLUST command line keywords to specify the number of processors and the number of logical clusters, respectively. Remember that the number of logical clusters is the same as the number of frequency segments. The value of DMP should be a multiple of NCLUST. The number of matrix domains will be the quotient DMP/NCLUST, so it is recommended that values of DMP and NCLUST be chosen so that DMP/NCLUST is a power of 2. The upper frequency limit must be specified on the EIGRL bulk data entry, and it is recommended that a lower frequency limit be specified as well.

Case Study A 1.3 Mdof body-in-white model was run, computing modes up to 300 Hz (1397 eigenvalues), using a cluster of 8 IBM P655 servers, each with 8 1.5-GHz POWER4+ processors and 16 GB of physical memory. Each node had two local, 73GB disks for scratch. The parallel performance scaled well, achieving nearly a 6-fold improvement when using 16 processors. DMP Performance (Elapsed Time) 6 5 4 Speedup 3 2 1 0 2

4

8

16

Number of Processors

CHAPTER 3 93 Numerical Enhancements

The MLDMP option also reduces the per-processor resource requirements in terms of both memory required and I/O performed: I/O Reduction

Memory Hiwater

Megawords

I/O per processor (GB)

2000 1500 1000 500 0 1

2

4

8

16

Number of Processors

250 200 150 100 50 0 1

2

4

8

16

Number of Processors

94 MD Nastran 2006 Release Guide

MD Nastran 2006 Release Guide Ch. :

4

Elements

J

Three-Node Beam Element, 96

J

CWSEAM Connector Elements, 105

J

Line Interface Element, 117

J

Arbitrary Beam Cross-Section, 126

96 MD Nastran 2006 Release Guide

Three-Node Beam Element Introduction A general three-node beam element has been developed for linear static, modal, dynamic and buckling analyses. The element has been implemented as a curved one-dimensional Timoshenko beam element so that both the initial curvatures of beam reference axis and the cross-section shears are included in the formulation of linear strain-displacement relations. The geometry of beam axis is specified by the offset vectors from the grid points to the shear centers of the beam cross-sections. The quadratic interpolation is used for both beam axis and the shape functions. When a three-node beam element degenerates to a two-node straight beam element, the linear interpolation is adopted. Variable cross-sectional properties are interpolated quadratically for a three-node and linearly for a degenerate two-node beam element. Unlike MD Nastran two-node straight beam element (CBEAM), the three-node beam element is developed based on the displacement method, in which the displacements at nodal points are taken as primary variables and the variational principle is applied to minimize the total element energy in formulating element stiffness, consistent mass and differential stiffness matrices. At each beam element nodal point, there are three translative and three rotational degrees of freedom, respectively. When the beam cross-section torsional warping effect is considered, another degree of freedom, which represents the warping variable, is added to the six nodal degrees of freedom at each grid point. The warping degrees of freedom are represented by either scalar or grid points. Element-related loads, such as distributed forces and moments, as well as thermal loads, can be applied on this element. The solution output includes element stresses, strains, forces and moments, element strain energy and grid point forces.

Benefits Perhaps the most suitable situation of the application of three-node beam elements is that the element is used in conjunction with higher-order shell elements, such as TRIA6 and QUAD8 that are used to model stiffeners. It can also be applied as an alternative to the existing straight two-node beam element in modeling favorably a structural geometry with initial curvatures. In addition to normal stresses and strains at beam cross-sections, both shear stresses and strains are also recovered at cross-sectional stress output points. When warping effect is considered, normal stresses caused by cross-sectional bi-moments are computed and output accordingly.

Input Several new Bulk Data entries have been created for three-node beam element connection, property, distributed thermal and mechanical loads. They are CBEAM3, PBEAM3, TEMPB3 and PLOADB3. For a detailed description of each entry, please refer to MD Nastran Quick Reference Guide included in this release.

CHAPTER 4 97 Elements

Guidelines and Limitations Geometry and Coordinate Systems The geometry of a three-node beam element is specified by element connection Bulk Data entry CBEAM3. The offset vectors W a , W b , and W c , are measured from grid points GA, GB and GC to the corresponding shear centers, A, B and C, respectively, at the beam cross-sections, as shown in Figure 4-1. Shear centers, A, B and C, are coplanar points. They define a plane in space if they are non-collinear. A quadratic approximation of the locus of beam shear center is uniquely defined by the spatial locations of these three shear centers. In what follows, we will refer the locus of beam shear center as the beam reference axis, or simply, beam axis. Taking the locus of shear center as the beam primary reference axis is consistent with the CBEAM element. Theoretically, the beam reference axis can be chosen arbitrarily. We also assume that the beam reference axis is a smooth spatial curve. The beam cross-section is perpendicular to the beam axis. Locus of Shear Locus of Shear Center

Center

Y e le m Yelem

ZZeelem l em

νν

AA

e beb

C C

wW c

eet

c

en e n

X e l em X elem

wa

BB

Wa GA

GC GC

Wb w b

GA

GB GB Figure 4-1

Locus of Shear Center of Three-node Beam Element

The element coordinate system ( X ele m , Yele m , Zele m ) is established by the orientation vector ν in the same way as what is defined for CBEAM element, as shown in Figure 4-1. For a spatial curve, such as the beam reference axis, the natural coordinate system is its Frenet-Serret frame ( e t, e n, e b ) , as shown in Figure 4-1. Here e t , e n and e b are the unit tangential, normal and bi-normal vectors, respectively. Tangent vector e t points to the direction from A to B along the beam axis. Vector en

is in the plane defined by these three non-collinear shear centers and points inwardly with respect to

the bending of beam axis. Bi-normal vector is perpendicular to both e t and e n by following the right-

98 MD Nastran 2006 Release Guide

hand rule of e b = e t ⋅ e n . When the beam axis is a straight line, i.e., three sectional shear centers are collinear, the Frenet-Serret frame is undefined. Then it will be replaced by the element coordinate system. To formulate finite element equations and define the beam element properties, a local convected coordinate system ( e x, e y, e z ) is created. The x-axis is always along the beam axis and its convected x coordinate is measured by the arc-length, s. Its base vector, e x , is taken as same as vector e t . The base vectors of the local coordinate system, e y and e z , are defined in such a way that they rotate an angle φ (pre-twist angle), from e n and e b , respectively, in the plane of beam cross-section, as shown in Figure 4-2. The orthogonal curvilinear coordinate system ( e x, e y, e z ) is introduced here as the local

convected coordinate system, instead of the Frenet-Serret frame, to model the pre-twist of the beam cross-section. When φ = 0 , the Frenet-Serret frame (or the element coordinate system if the beam axis is straight) becomes the local convected coordinate system. The angle, φ , may vary along the beam axis. The pre-twist angles at three beam cross-sections are given in Bulk Data entry, CBEAM3.

eb

eb

e z ez

ey

ey

φ Shear Sh ear Center C enter

Figure 4-2

en

en

Local Coordinate System on a Beam Cross-Section

The properties of a three-node beam element listed in Bulk Data entry, PBEAM3, are referred to the local coordinate system. The output of element stresses, strains and forces is also presented in the local coordinate system. Element Properties, Materials and Loads There are some similarities between PBEAM and PBEAM3 entries in terms of both format and content. Attention, however, should be paid to their differences. The local coordinate system is primarily referred

CHAPTER 4 99 Elements

in defining cross-sectional properties, such as area moments and product of inertia, and locations of neutral axis and nonstructural mass center of gravity. Four stress output points on a beam cross-section are also specified in the local coordinate system. Unlike PBEAM, in which you can specify the properties at as many as nine intermediate stations, PBEAM3 requires their definitions at only three grid locations. For a degenerate two-node beam element, those fields related to the mid-grid are ignored. Values of warping function and its gradients at stress output points are required if torsional warping stresses are to be recovered. Shear effectiveness factors may not be zero. Since the element is formulated on the Timoshenko beam theory and quadratic shape functions are used for interpolation, zero shear effectiveness factors will not automatically lead to a three-node Euler-Bernoulli beam element. Both MAT1 and MAT2 entries can be referred by PBEAM3. The loads related to the three-node beam element are element thermal and distributed mechanical loads, given by TEMPB3 and PLOADB3, respectively. The distributed forces and moments can be specified in any one of local, element, basic and any user-specified coordinate systems. The load must be applied over entire length of the element along the beam axis. Limitations There are some limitations in the current implementation with the three-node beam element. First of all, it is limited to linear analysis solution sequences only. Heat transfer analysis with the three-node beam element is not supported. Other limitations are identified as follows. • X-Y PLOT output • Random analysis • PBEAML and PBCOMP related features • CBEAM related features, such as pin-flags and shear relief

Formulation Strain-Displacement Relations The formulation of a three-node beam element is based on Timoshenko beam theory. The kinematical assumption hereafter is that the displacement vector at an arbitrary point of the beam cross-section is uniquely defined by the displacement vector at the beam reference axis and the rotations of the crosssection, superposed by a longitudinal warping displacement. For small deformation theory, the rotation of the cross-section is a vector. The displacement vector at point (s, y, z) of a beam cross-section is u ( s, y, z ) = U x e x + U y e y + U z e z where:

100 MD Nastran 2006 Release Guide

U x ( s, y, z ) = u ( s ) + zθ y ( s ) – yθ z ( s ) + ω ( s )ψ ( y, z ) U y ( s, y, z ) = ν ( s ) – zθ x ( s ) U z ( s, y, z ) = w ( s ) + yθ x ( s ) in which u ( s ) , v ( s ) and w ( s ) are three translative displacement components at the beam axis; θ x ( s ) , θy ( s )

and θ z ( s ) are three rotational degrees of freedom of the beam cross-section; and ψ ( y, z ) is a given

warping function and ω ( s ) the warping degree of freedom. The assumption of the warping displacement is based on the Saint-Venant torsion theory of straight bars. The Green-Lagrangian normal and shear strains, { ε, γ y, γ z } , are ε = ε 0 + zχ y – yχ z + ψω s γ y = γ y 0 – zχ x + ψ y ω γ z = γ z 0 + yχ x + ψ z ω where: ε0 = u , s + κy w – κz v γ y0 = ν , s – θ z + κ z u – κ x w γ z0 = w , s + θ y – κ y u + κ x ν χ x = θ x, s – κ z θ y + κ y θ z χ y = θ y, s + κ z θ x χ z = θ z, s – κ y θ x ∂ψ ψ y = ------- + κ z ψ ∂y ∂ψ ψ z = ------- – κ y ψ ∂z in which ( ) , s = ∂ ( ) ⁄ ( ∂s ) , the derivative with regard to the arc-length of beam axis. Constitutive Relation The general stress-strain relations are given, including thermal loads, at an arbitrary point of a beam cross-section, as σ    { σ } =  τy  =    τz 

C 11 C 12 C 13   ε   α∆T      C 22 C 23   γ y  –  0      Sym C 33   γ z   0 

CHAPTER 4 101 Elements

where C ij are material elastic constants, α the thermal expansion coefficient and ∆T the variation of temperature. Element Forces and Moments The axial and shear forces as well as torsion and bending moments of the cross-section in the local coordinate system are Nx =

∫ σdA A

Vy =

∫ τ y dA A

Vz =

∫ τ z dA A

Mx =

∫ ( yτ z – zτ y ) dA A

My =

∫ σz dA A

Mz =

∫ ( – yσ ) dA

and the bi-shear force and bi-moment, which are associated with the warping degree of freedom and its derivative, are Vb =

∫ ( τ y ψ y + τ z ψ z ) dA A

Mb =

∫ σψ dA A

Output Element forces, moments, stresses and strains, are computed at three beam cross-sections, in the local coordinate system. These three cross-section locations are related to either three grid points or two Gauss integration points and the parametrized origin. Both normal and shear stresses and strains are output at four cross-sectional stress recovery points in the local coordinate system. The output examples of element forces, stresses and strains are shown in Listing 4-1, Listing 4-2, and Listing 4-3.

102 MD Nastran 2006 Release Guide

Listing 4-1

F O R C E S

0

0

0

I N

B E A M 3

E L E M E N T S ( C B E A M 3 ) - FORCES IN LOCAL COORDINATE SYSTEM - BENDING MOMENTS - SHEAR FORCES MY MZ QY QZ

GRID/ GAUSS

ELEMENT-ID 2901

Output of Element Forces and Moments

0.0 0.0 0.0

1.087807E+02 1.902465E+01 6.390266E+01

0.0 0.0 0.0

0.0 0.0 0.0

0.0 0.0 0.0

3901 3903 3904

0.0 0.0 0.0

-1.048109E+03 -3.558532E+00 -7.528904E+02 -7.162810E+01 -9.004999E+02 -3.759332E+01

0.0 0.0 0.0

1.042715E+02 7.585925E+01 9.006535E+01

0.0 0.0 0.0

0.0 0.0 0.0

0.0 0.0 0.0

3903 3902 3905

0.0 0.0 0.0

-7.267761E+02 -7.611831E+01 -1.843143E+01 -1.042837E+02 -3.726037E+02 -9.020099E+01

0.0 0.0 0.0

7.135274E+01 3.180659E+00 3.726670E+01

0.0 0.0 0.0

0.0 0.0 0.0

0.0 0.0

3901

3902

I N

ELEMENT-ID 2901

2903

Output of Element Stresses

B E A M 3

GRID/ STRESS GAUSS COMPONENT

2902

E L E M E N T S

( C B E A M 3 )

- STRESSES IN LOCAL COORDINATE SYSTEM SXD SXE SXF S-MAX

SXC

S-MIN

M.S.-T

M.S.-C

SX SY SZ SX SY SZ SX SY SZ

5.889157E+04 1.087807E+03 -5.671596E+04 1.087807E+03 5.889157E+04 -2.348231E+02 -2.348231E+02 -2.348231E+02 -2.348231E+02 -2.348231E+02 0.0 0.0 0.0 0.0 0.0 5.818494E+03 1.902465E+02 -5.438001E+03 1.902465E+02 5.818494E+03 -1.096482E+03 -1.096482E+03 -1.096482E+03 -1.096482E+03 -1.096482E+03 0.0 0.0 0.0 0.0 0.0 3.235503E+04 6.390266E+02 -3.107698E+04 6.390266E+02 3.235503E+04 -6.656523E+02 -6.656523E+02 -6.656523E+02 -6.656523E+02 -6.656523E+02 0.0 0.0 0.0 0.0 0.0

-5.671596E+04 -9.8E-01 -9.6E-01 -2.348231E+02 0.0 -5.438001E+03 -1.096482E+03 0.0 -3.107698E+04 -6.656523E+02 0.0

SX SY SZ SX SY SZ SX SY SZ

5.344819E+04 1.042714E+03 -5.136276E+04 1.042714E+03 5.344819E+04 -3.558532E+01 -3.558532E+01 -3.558532E+01 -3.558532E+01 -3.558532E+01 0.0 0.0 0.0 0.0 0.0 3.840311E+04 7.585925E+02 -3.688593E+04 7.585925E+02 3.840311E+04 -7.162810E+02 -7.162810E+02 -7.162810E+02 -7.162810E+02 -7.162810E+02 0.0 0.0 0.0 0.0 0.0 4.592565E+04 9.006535E+02 -4.412434E+04 9.006535E+02 4.592565E+04 -3.759331E+02 -3.759331E+02 -3.759331E+02 -3.759331E+02 -3.759331E+02 0.0 0.0 0.0 0.0 0.0

-5.136276E+04 -9.8E-01 -9.6E-01 -3.558532E+01 0.0 -3.688593E+04 -7.162810E+02 0.0 -4.412434E+04 -3.759331E+02 0.0

3901 3901 3903 3904

Listing 4-3

S T R A I N S ELEMENT-ID 2901

I N

2902 2903

Output of Element Strains

B E A M 3

GRID/ STRAIN GAUSS COMPONENT 2901

0

BI-MOMENT

-1.156075E+03 -2.348231E+01 -1.125649E+02 -1.096482E+02 -6.343201E+02 -6.656523E+01

2901

0

BI-SHEAR FORCE

0.0 0.0 0.0

S T R E S S E S

0

TOTAL TORQUE

2901 2902 2903

Listing 4-2

0

AXIAL FORCE

SX SY SZ SX SY SZ SX SY SZ

E L E M E N T S

SXC 1.000000E-01 8.765757E-17 0.0 1.000000E-01 5.160202E-17 0.0 1.000000E-01 6.962979E-17 0.0

( C B E A M 3 )

- STRAINS IN LOCAL COORDINATE SYSTEM – SXD SXE SXF S-MAX 1.000000E-01 8.765757E-17 0.0 1.000000E-01 5.160202E-17 0.0 1.000000E-01 6.962979E-17 0.0

1.000000E-01 8.765757E-17 0.0 1.000000E-01 5.160202E-17 0.0 1.000000E-01 6.962979E-17 0.0

1.000000E-01 8.765757E-17 0.0 1.000000E-01 5.160202E-17 0.0 1.000000E-01 6.962979E-17 0.0

1.000000E-01 8.765757E-17 0.0 1.000000E-01 5.160202E-17 0.0 1.000000E-01 6.962979E-17 0.0

S-MIN

M.S.-T

1.000000E-01 -1.0E+00 8.765757E-17 0.0 1.000000E-01 5.160202E-17 0.0 1.000000E-01 6.962979E-17 0.0

3901 3901 3903 3904

SX SY SZ SX SY SZ SX SY SZ

1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 -1.0E+00 -7.548301E-16 -7.548301E-16 -7.548301E-16 -7.548301E-16 -7.548301E-16 -7.548301E-16 0.0 0.0 0.0 0.0 0.0 0.0 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 -4.543672E-16 -4.543672E-16 -4.543672E-16 -4.543672E-16 -4.543672E-16 -4.543672E-16 0.0 0.0 0.0 0.0 0.0 0.0 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 1.000000E-01 -6.045987E-16 -6.045987E-16 -6.045987E-16 -6.045987E-16 -6.045987E-16 -6.045987E-16 0.0 0.0 0.0 0.0 0.0 0.0

M.S.-C

CHAPTER 4 103 Elements

Example ID MSC, b3arcbck $ ARCH BUCKLING SOL 105 TIME 10 CEND $ TITLE = BUCKLING OF AN ARCH WITH CBEAM3 ELEMENTS SUBTI = HALF CIRCLE, PRESSURE LOAD SPC = 10 DISP = ALL FORCE = ALL SPCFORCE = ALL $ SUBCASE 1 LABEL= LOAD CASE LOAD = 10 SUBCASE 2 LABEL= BUCKLING CASE METHOD = 10 $ BEGIN BULK $-------2-------3-------4-------5-------6-------7-------8-------9-------0-----EIGRL 10 5 $ PLOADB3 10 1 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 2 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 3 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 4 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 5 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 6 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 7 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 8 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 9 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 10 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 11 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 PLOADB3 10 12 LOCAL 0.0 1.0 0.0 FORCE 1.0 + + 100. 100. 100.0 $ CBEAM3 1 1 1 2 21 100 CBEAM3 2 1 2 3 22 100 CBEAM3 3 1 3 4 23 100 CBEAM3 4 1 4 5 24 100 CBEAM3 5 1 5 6 25 100 CBEAM3 6 1 6 7 26 100 CBEAM3 7 1 1 8 31 100 CBEAM3 8 1 8 9 32 100 CBEAM3 9 1 9 10 33 100

104 MD Nastran 2006 Release Guide

CBEAM3 10 1 10 11 34 100 CBEAM3 11 1 11 12 35 100 CBEAM3 12 1 12 13 36 100 $ PBEAM3 1 2 .1 .01 .01 0.0 .02 + + 0.5 0.0 0.0 0.5 -0.5 0.0 0.0 -0.5 $ MAT1 2 1.0E+7 0.3 .05 .001 0.0 .01 +MAT1-2 +MAT1-2 1000. 2000. 3000. $ GRID 2 2.58819 9.659258 0.0 GRID 3 5.0 8.660254 0.0 GRID 4 7.07107 7.07107 0. GRID 5 8.66025 5.0 0. GRID 6 9.65926 2.58819 0. GRID 7 10. 0. 0. $-------2-------3-------4-------5-------6-------7-------8-------9-------0-----GRID 8 -2.588199.659258 0.0 GRID 9 -5.0 8.660254 0.0 GRID 10 -7.071077.07107 0. GRID 11 -8.660255.0 0. GRID 12 -9.65926 2.58819 0. GRID 13 -10. 0.0 0.0 $-------2-------3-------4-------5-------6-------7-------8-------9-------0-----GRID* 21 1.30526 9.91445 * * 0.0 GRID* 22 3.82683 9.2388 * * 0.0 GRID* 23 6.08761 7.93353 * * 0.0 GRID* 24 7.93353 6.08761 * * 0.0 GRID* 25 9.2388 3.82683 * * 0.0 GRID* 26 9.91445 1.30526 * * 0.0 GRID* 31 -1.30526 9.91445 * * 0.0 GRID* 32 -3.82683 9.2388 * * 0.0 GRID* 33 -6.08761 7.93353 * * 0.0 GRID* 34 -7.93353 6.08761 * * 0.0 GRID* 35 -9.2388 3.82683 * * 0.0 GRID* 36 -9.91445 1.30526 * * 0.0 $GRID 100 0.0 0.0 0.0 $-------2-------3-------4-------5-------6-------7-------8-------9-------0-----SPC1 10 12345 7 13 SPC1 10 123456 100 $ ENDDATA

CHAPTER 4 105 Elements

CWSEAM Connector Elements Introduction The functionality of connector elements is enhanced by supporting a seam element to connect two surface patches. To define the seam weld, you must select two surface patches by their property IDs and specify the width and the thickness of the seam. You also have to specify start point “GS” and end point “GE” of the seam segment. These two points do not have to lie on or in between the shell planes. The program will project these two points onto the selected surface patches to find the connecting shell grids.

Inputs The seam connection is modeled by the new CWSEAM and PWSEAM Bulk Data entries and the modified SWLDPRM Bulk Data entry. CWSEAM

A Shell Patch Seam Connection

Defines a seam element connecting two surface patches. Format: 1 CWSEAM

2

3

EID

PID

GS

GE

4

5

6

7 PIDA

“GRIDID”

8

9

10

9

10

PIDB

Alternate Format: 1 CWSEAM

2

3

EID

PID

XS

YS

4

5

6

“XYZ” ZS

XE

7 PIDA

YE

8 PIDB

ZE

Example: CWSEAM 3 30024

17 65467

GRIDID

2305

7116

106 MD Nastran 2006 Release Guide

Field EID

Contents Element identification number. (0 < Integer < 100,000,000)

PID

Property identification number of a PWSEAM entry. (Integer > 0)

LTYPE

Connectivity search type. (Character) If LTYPE=”GRIDID”, location is defined by GS and GE. If LTYPE=”XYZ”, location is defined by two XYZ locations.

PIDA,PIDB

Property identification numbers of PSHELL entries defining surface A and B respectively. (Integer > 0)

GS, GE

Grid ID’s of piercing points on patches A and B of the Start and End of the seam. (Integer > 0)

XS,YS,ZS

Location of the start of the seam in basic coordinate system. (Real or blank)

XE,YE,ZE

Location of the end of the seam in basic coordinate system. (Real or blank)

Remarks: 1. Element ID numbers must be unique with respect to all other element ID numbers. 2. GS and GE define the start and end points of the seam element. At these points and using the value W specified on the PWSEAM entry, surface patches A and B are determined. Points projected onto the surface patches A and B from GS and GE are used to determine the auxiliary points that form faces of a CHEXA element. These auxiliary points are then connected to the physical grids of the patches. The total number of unique physical grids ranges from a possibility of 6 to 32 grids. The auxiliary points must have a projection on patches A and B, but they do not have to lie on patch A or B. 3. A maximum of three shell elements of patch A and three shell elements of patch B can be connected with one CWSEAM element, see Figure 4-3.

E

S Figure 4-3

Connected Shell Elements for a CWSEAM Element

CHAPTER 4 107 Elements

PWSEAM

Seam Connector Element Property

Defines the property of seam connector (CWSEAM) elements. Format: 1

2

3

PWSEAM PID

MID

4 W

5

6

7

8

9

10

T

Example: PWSEAM 7

1

16.

Field

Contents

PID

Property identification number. (Integer > 0)

MID

Material identification number. (Integer > 0)

W

Width of the seam. See Remark 1. (Real > 0.)

T

Thickness of the seam. See Remark 2. (Real > 0. or blank)

Remarks: 1. The length of the seam is the distance between GS and GE. The width of the seam is measured perpendicular to the length and lies in the plane of the patches A and B (see Figure 4-4). The width is also used to find the projection of the seam on the two patches A and B. GE GS T W

Figure 4-4

Dimensions of a CWSEAM Element

2. If left blank, the thickness will be computed as T = ( T A + T B ) ⁄ 2 where T A is the thickness of patch A and TB is the thickness of patch B.

108 MD Nastran 2006 Release Guide

SWLDPRM

Parameters for CFAST, CWELD, and CWSEAM Connectors

Overrides default values of parameters for CFAST, CWELD, and CWSEAM connectivity search. Format: 1

2

3

4

SWLDPRM PARAM1

VAL1

PARAM2

PARAM5

VAL5

-etc.-

5 VAL2

6

7

PARAM3

VAL3

PRTSW

1

8 PARAM4

9 VAL4

Example: SWLDPRM GSPROJ

15.0

Field

GSMOVE 2

Contents

PARAMi

Name of the spot weld parameter. Allowable names are listed in Table 4-1. (Character)

VALi

Value of the parameter. (Real or Integer; see Table 4-1.)

10

CHAPTER 4 109 Elements

Table 4-1

PARAMi Names and Descriptions

Name

Type

Default

Description

CHKRUN

Integer 0, 1, 2

0

Stop the program after the connectivity of connector CWELD elements are generated. 0=abort on first error or run to completion; 1=stop after weld connectivity has been checked; 2=continue run if no errors are found or stop run after all weld connectivity errors have been found.

GMCHK

Integer 0, 1, 2

0

For CWELD with PARTPAT format and CWSEAM only. 0=no geometry error checks; 1=check errors of CWELD elements with patch A and patch B tilting toward each other or check errors of the CWSEAM across a cutout or over a corner with patch elements in plane or out of plane; 2=check errors and output all candidate shell elements if an error is encountered. If GMCHK=1 or 2 and an error is detected, the program will loop back to search for next candidate element until a good pair of connection is found or all adjacent elements have been checked. In the latter case, a user fatal message 7595, 7638, or 7667 will be issued. A UFM 7595 is issued if the angle between the normal vectors of the patches at end GS or between the normal vectors of the patches at end GE exceeds the value of GSPROJ; a UFM 7638 is issued if either the length of the seam spans more than three elements or the seam spans a cutout; a UFM 7667 is issued if the angle between the normal vectors of the top patches at GS and GE or between the normal vectors of the bottom patches at GS and GE exceeds GSPROJ or if the angle between the free edges of the shell elements onto which GS and GE are projected is less than 160o (if GSPROJ < 20.0) or (180o-GSPROJ) (if GSPROJ > 20.0).

GSMOVE

Integer > 0

0

Maximum number of times GS for the CFAST or CWELD (PARTPAT or ELPAT options only) or GS/GE for the CWSEAM is moved in case a complete projection of all auxiliary points has not been found.

GSPROJ

Real

20.0

Maximum angle allowed between the normal vectors of shell A and shell B. The spot weld element will not be generated if the angle between these two normal vectors is greater than the value of GSPROJ. If GSPROJ is set to -1.0, the program will skip the checking of GSPROJ.

110 MD Nastran 2006 Release Guide

Table 4-1 Name

PARAMi Names and Descriptions Type

Default

Description

GSTOL

Real > 0.0

0.0

For CFAST or CWELD (PARTPAT and ELPAT only), if GSTOL > 0.0 and the distance between GS and the projected point GA or GB is greater the GSTOL, a UFM 7549 is issued and the CFAST or CWELD is rejected. For CWSEAM, if GSTOL > 0.0 and the distance between GS and the projected point GSA or GSB or the distance between GE and the projected point GEA or GEB is greater than the GSTOL, a UFM 7549 is issued and the CWSEAM is rejected.

NREDIA

0 < Integer < 4

0

CFAST or CWELD (PARTPAT and ELPAT) only. Maximum number of times the diameter D is reduced in half in case a complete projection of all points has not been found.

PROJTOL

0.0 < Real < 0.2

0.02

For CFAST or CWELD, tolerance to accept the projected point GA or GB if the computed coordinates of the projection point lie outside the shell element but is located within PROJTOL*(dimension of the shell element forming the patch). For the PARTPAT option for the CWELD or the PROP option for the CFAST it is recommended that PROJTOL=0.0. For the CWSEAM, a projection from GS/GE will always be attempted as if PROJTOL=0.0 and if one cannot be found then the non-zero value of PROJTOL will be used.

PRTSW

Integer 0, 1, 2

0

Print diagnostic output. 0=no diagnostic output; 1=print diagnostic output to f06 file; 2=punch diagnostic output.

Remarks: 1. This entry changes the default settings of control variables for the CFAST, CWELD, and CWSEAM connector elements. None of the parameters of this entry are required. Only one SWLDPRM entry is allowed in the Bulk Data Section. 2. Connectivity information is generated for the CFAST and CWSEAM elements. For the CWELD, connectivity information is only generated for the PARTPAT, ELPAT, ELEMID, and GRIDID options.

Error Conditions for the CWELD and CWSEAM Elements The GMCHK parameter specified in the SWLDPRM Bulk Data entry checks the errors of CWSEAM elements across cutouts or over corners. There are three allowable values of GMCHK. This parameter is also used by CWELD elements with PARTPAT format to check the angle between patches A and B and to find the next candidate element if the angle check fails. • GMCHK = 0 (Default) Do not check errors

CHAPTER 4 111 Elements

• GMCHK = 1 Check errors • GMCHK = 2 Check errors and output all candidate shell elements if there is an error

encountered If GMCHK is turned on, MD Nastran will perform the following checking while searching for the projected shell elements. Note that SHSA is the shell element that gets projection from GS on shell A; SHEA is the shell element that gets projection from GE on shell A. Same algorithms are applied to SHSB and SHEB for shell B.

Check the Angle and Find Next Candidate Element for CWELD and PARTPAT Format If GSPROJ is greater than zero, MD Nastran will check the angle between SHSA and SHSB while searching for the projected shell elements. If the angle is greater than GSPROJ, the program will loop back to find next possible projection pair and check the angle between them again, until the angle of the new pair is less than GSPROJ or all candidate elements have been checked.

Check the CWSEAM Across a Cutout or Over a Corner with Elements in Plane 1. If SHSA is equal to SHEA, the seam lies within one element. No checks are required. 2. If SHSA and SHEA share two corner grids, these elements are adjacent. No checks are required. 3. If SHSA and SHEA share only one corner grid, the seam is over a corner. There are two exceptions: • There exists a shell element (SHMA) that shares two corner grids with SHSA and SHEA.

Also, either the angle between vector S 1 S 2 and vector E 1 E 4 is greater than theta degrees (where theta=160o if GSPROJ < 20.0; theta=180 o -GSPROJ if GSPROJ > 20.0) or the middle point (M) of line segment S 2 E 4 projects to SHSA, SHMA, or SHEA. S1 ⁄ E1

S2

E4 M

SHSA

S3

SHMA S4 E2

SHEA

E3 This model is acceptable.

112 MD Nastran 2006 Release Guide

S2

E4 M S1 ⁄ E1 SHSA

SHEA

S3

E3

SHMA S4 E2 This model fails.

• This shared grid is a shell grid of another two different shell elements.

S2

S3

S4

E4

S1 ⁄ E1 E2

E3

4. If SHSA and SHEA do not share any corner grid, MD Nastran will check if there is an element (SHMA) lying between SHSA and SHEA. SHMA must share two corner grids with SHSA and another different one corner grid with SHEA, or vice versa. The following five examples demonstrate the acceptable and failed cases. • SHMA shares one edge with SHSA and shares one corner grid with SHEA. This case is

acceptable. S1

S4

S2

S3

E1 E2

E4

E3

• SHMA shares one edge with SHEA and shares one corner grid with SHSA. This case is

acceptable.

CHAPTER 4 113 Elements

E1

S1

S4

E2

E4

E3

S3

S2

• SHMA shares one corner grid with SHSA and shares another corner grid with SHEA. An

error is detected because the seam spans a cutout.

S1

S4

E1

E4

S3

E2

E3

S2

• SHMA shares one edge with SHSA and shares another edge with SHEA. This case is

acceptable. S1

S4

E1

E4

S2

S3

E2

E3

• There does not exist a single element that shares an edge or corner grid with SHSA or SHEA.

An error is detected because the length of the seam spans more than three elements.

114 MD Nastran 2006 Release Guide

S1

S4

E1

E4

S2

S3

E2

E3

Check the CWSEAM Over a Corner with Elements Out of Plane The GSPROJ parameter is used to check the error of a seam over a corner with SHSA and SHEA not lying on a same plane. If the angle between the shell normal vectors of SHSA and SHEA is greater than GSPROJ, an error is detected. The default value of GSPROJ is 20o. No angles will be checked if GSPROJ=-1.

Example – A Symmetric Hat Profile (cwseam_hut.dat) This example demonstrates the application of CWSEAM elements to analyze a symmetric hat profile model, see Figure 4-5. Each edge of the hat is connected by 27 CWSEAM elements. The grids with identification numbers 6000 to 6028 and 8000 to 8028 are used as the piercing points to define the seams, see Figure 4-6. A rigid body element (RBE2) is specified to constrain one end of the hat.

Figure 4-5

Hat Profile

CHAPTER 4 115 Elements

Figure 4-6

Piercing Points and Seams

The input for the seam welds is listed as follows. CWSEAM CWSEAM : CWSEAM CWSEAM $ CWSEAM CWSEAM : CWSEAM CWSEAM $ PWSEAM

7000 6000 7001 6001

500 6001 500 6002

GRIDID

100

200

GRIDID

100

200

7026 6026 7027 6027

500 6027 500 6028

GRIDID

100

200

GRIDID

100

200

9000 8000 9001 8001

500 8001 500 8002

GRIDID

100

200

GRIDID

100

200

9026 8026 9027 8027

500 8027 500 8028

GRIDID

100

200

GRIDID

100

200

500

1

1.0

116 MD Nastran 2006 Release Guide

The normal mode analysis results are shown below.

R E A L E I G E N V A L U E S MODE EXTRACTION EIGENVALUE NO. ORDER 1 1 -3.607717E-05 2 2 2.210966E-05 3 3 4.523934E-05 4 4 4.937511E-05 5 5 1.087932E-04 6 6 1.537703E-04 7 7 1.154947E+07 8 8 1.585229E+07 9 9 2.653947E+07 10 10 2.959784E+07 11 11 3.002028E+07 12 12 3.041736E+07 13 13 3.328896E+07 14 14 3.757468E+07 15 15 4.259932E+07 16 16 4.738684E+07

RADIANS 6.006427E-03 4.702091E-03 6.726020E-03 7.026743E-03 1.043040E-02 1.240041E-02 3.398451E+03 3.981493E+03 5.151647E+03 5.440389E+03 5.479077E+03 5.515193E+03 5.769658E+03 6.129819E+03 6.526814E+03 6.883810E+03

CYCLES 9.559526E-04 7.483609E-04 1.070479E-03 1.118341E-03 1.660049E-03 1.973587E-03 5.408803E+02 6.336742E+02 8.199102E+02 8.658648E+02 8.720222E+02 8.777703E+02 9.182696E+02 9.755909E+02 1.038775E+03 1.095592E+03

GENERALIZED MASS 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00 1.000000E+00

GENERALIZED STIFFNESS -3.607717E-05 2.210966E-05 4.523934E-05 4.937511E-05 1.087932E-04 1.537703E-04 1.154947E+07 1.585229E+07 2.653947E+0 2.959784E+07 3.002028E+07 3.041736E+07 3.328896E+07 3.757468E+07 4.259932E+07 4.738684E+07

CHAPTER 4 117 Elements

Line Interface Element Introduction Line interface element is used to connect dissimilar meshes along the edges of finite element mesh subdomains. These subdomains have boundaries usually associated with either two-dimensional shell elements or one dimensional beam elements. A set of MPC (Multipoint Constraint) equations are internally generated with the interface boundary grids to enforce the compatibility of displacements and rotations across the interface. There are perhaps three situations in which finite element analysts want to use the interface element technique to connect two or more independently meshed regions. They are: • Different groups of engineers work almost independently in building finite element models. • Global-local modeling is used in the analysis, where a fine mesh is required in a particular area

due to high stress gradients while the rest of area only needs a coarse mesh, in consideration of the balance of computing resources and the solution accuracy. • Some regions of a structural model need constant changes or modifications, while the rest of

structure needs little or no change. The purpose of interface element technology is to provide engineers a simple and useful tool in building a more flexible finite element model. The interface element technology is not intended to raise the overall solution accuracy with the existing mesh resolutions of individual subdomains. It is rather how to preserve the solution accuracy in the regions where the finite element results are more interesting to an analyst than in others. The method that we have developed for the line interface element is to achieve primarily the continuity of displacements and rotations across the interface in a way that a measure of their discontinuity is minimized. Since the smoothness (continuity of derivatives) of displacement components across the interface is not enforced by this method, some fluctuation of stresses in the vicinity of the interface could be expected. This stress unevenness or interface effect, however, diminishes quickly in the area away from the interface. This is a phenomenon that can be explained by Saint-Venant’s Principle. When applying an interface element, you are asked to specify a boundary on which all the degrees of freedom at the grids are taken as the independent. The degrees of freedom associated with the grids on other boundary or boundaries referenced by the interface element are taken as the dependent and put into the m-set. In the terminology of contact mechanics, the interface boundaries are categorized as the master and slave ones. The nodal points on the master boundary are the independent grids and the nodes on the slave boundary are the dependent grids. An interface element is equivalent to a glued or tied contact that connects the dissimilar meshes. The conventional way to specify the dependency or master-slave relationship of the interface boundaries is that the boundary with a fine mesh is tied to the one with a coarse mesh. In other words, the boundary with a fine mesh is chosen as a dependent or slave boundary and the one with a coarse mesh as an independent or master boundary. This practice, however, sometimes introduces a seemingly stiff connection along the interface. In this case, it may yield better solutions by switching the dependency relation between the interface boundaries.

118 MD Nastran 2006 Release Guide

The line interface element is intended for linear and non-superelement analyses. It should not be used for heat transfer analyses at this moment.

User Interface There are two Bulk Data entries used to define a line interface element. CINTC is the element connection entry which specifies the connectivity of line interface boundaries, represented by Bulk Data entry, GMBNDC. Bulk Data Entry: CINTC

CINTC

Line Interface Element Connection

Defines a line interface element with specified boundaries. Format: 1 CINTC

2 EID

3

4

5

6

7

8

9

10

TYPE

LIST=(BID1(INTP1), BID2(INTP2),…, BIDn(INTPn) )

Example: CINTC

1001

GRDLIST

LIST=(101,102(Q),-103(Q),104(L))

Field EID TYPE

Contents Element identification number. (0
METHOD

Optimization Method: (Integer > 0; Default = 1) = 1 Modified Method of Feasible Directions for both MSCADS and DOT = 2 Sequential Linear Programming for both MSCADS and DOT = 3 Sequential Quadratic Programming for both MSCADS and DOT = 4 SUMT method for MSCADS = IJK for user's specified MSCADS optimization strategy.

222 MD Nastran 2006 Release Guide

Output There are no outputs that are affected by optimizer selection with the exception that the optimizer output produced using the IPRINT parameter on the DOPTPRM entry is dependent on the method selected. In particular, the banner for the MSCADS code appears as: M S C . A D S E N H A N C E D

A D S

P R O G R A M

F O R A U T O M A T E D

D E S I G N

S Y N T H E S I S

Guidelines and Limitations The optimization results from MSCADS are expected to be comparable to those from DOT. If this is not the case, the OPTCOD parameter can be used to invoke the DOT optimizer. It is recommended that the Topology Optimization option be utilized for topology optimization and for sizing and shape optimization problems with thousands of design variables. Sizing and shape cannot be combined with topology optimization in a single run.

CHAPTER 7 223 Optimization

Supporting Trust Region in SOL 200 for Adaptive Move Limits Introduction Formal approximate optimization is used in SOL 200 to find a new design without performing expensive and exact finite element analyses (Ref. 1, Chapter 2.7). However, move limits must be applied to define a restricted region on which an adequate approximate model can be created. Convergence checks are made following each approximate optimization task. Currently, if the approximate optimization comes up with a design that an exact analysis shows is actually worse, it is assumed that the region defined by move limits are too generous and they are reduced. Using Trust Region Concepts, this simple update strategy can be improved in three fundamental ways: 1. A merit function is applied to provide a more quantitative measure of the quality of the approximation. 2. A provision is made to increase the move limits when the approximate optimization results are shown to be of high quality. 3. If the new design is judged to actually be worse, it is discarded and the approximate optimization task is performed again with tighter move limits.

Benefits Since the move limits can be either reduced or increased in an adaptive fashion, it is expected that the quality of the approximate model will be enhanced. This should lead to more robust optimization result and faster convergence. In addition, rejecting a bad design should also smooth the design optimization process.

Theory Concept of Trust Region The main idea behind the Trust Region is to first compute a merit function that is a combination of the objective function and the maximum violated constraint value and then form a ratio of the exact reduction in a merit function to the predicted reduction in the merit function. The ratio can be written as follows, assuming a design task is a constrained minimization optimization task: MF p – MF c Ratio = -----------------------------MF p – MF a

224 MD Nastran 2006 Release Guide

where: MF c = Φ c + PW ⋅ maxg c

The current exact merit function

MF p = Φ p + PW ⋅ maxg p MF a = Φ a + PW ⋅ maxg c

The previous exact merit function The approximate merit function.

Notice that a merit function is the sum of objective ( Φ ) and the product of penalty weight and the maximum violated constraint ( g ) . Subscripts c, p and a, indicate that the function is evaluated exactly at the current design cycle, evaluated exactly at the previous design cycle and evaluated approximately, respectively. The penalty weight plays an important role in a successful optimization task with Trust Region Method. The magnitude of Ratio varies in the real interval of ( – ∞, ∞ ) . The denominator is the predicted reduction in merit function while the numerator is the exact reduction in merit function. Since we consider the case of minimizing the objective, the denominator should always produce a positive number to indicate that the optimizer has done a good job. Different Ratio values can measure the quality of the approximate model. For example, a negative Ratio (likely due to negative numerator) indicates that the approximate model is so bad that the exact merit function is greater than the previous exact. Thus reducing move limits is necessary. On the other hand, Ratio = 1 indicates the approximate model is very good that the predicted reduction is identical to the exact reduction and the move limits can be increased. In general, the following strategies are used to update move limits if: 1. Ratio < η 1 (say 0.01), reject the design, cut the move limits in half and repeat the approximate optimization task. For a minimization task, the reduction in the merit function must be greater than zero. A too small or negative Ratio indicates that the new design proposed by the approximate model either does not reduce the merit function, or the quality of the approximate model is very poor. 2. η 1 < Ratio < η2 (say 0.25), accept the design, but cut the move limits in half for the next approximate design task. The ratio in this range indicates that quality of the approximate model is not good enough, or the current move limit is still too large. 3. η 2 < RATIO < η 3 (say 0.75), accept the design and do not adjust the move limits. 4. Ratio > η 3 , accept the design, but increase the move limits by 50%, up to a pre-specified upper value. The ratio approaching to 1 indicates that the approximate model I is accurately predicting the actual behavior. Therefore, the current move limits can be increased. In addition, although Ratio > 1 indicates that the approximate model is not particularly accurate, but it predicts in the right direction so that larger move limits can also be used. Creating the Constrained Merit Function For the unconstrained minimization tasks, the merit function is simply the objective. For constrained minimization tasks, the second term on the right hand side of the merit function accounts for violated constraints. Since Ratio is computed using three merit functions, according to Ref. 2, the approximate

CHAPTER 7 225 Optimization

optimization problem should also be solved in the same fashion to minimize the merit function that is formed by the objective and the corresponding 2nd term. A capability to transform an approximate optimization task to a feasible design was implemented and can be readily used here to satisfy this consistency requirement. Notice that the algorithm of Ref. 3 computes the penalty weight, PW = Pena l ⋅ Φ o , where Φ o is the starting objective at the beginning of the approximate optimization job, while here PW is obtained with a single number (See Penalty Weight Section). Penalty Weight Penalty Weight (PW) is used to form the merit function. The penalty weight plays an important role in a successful optimization task with Trust Region Method. It is problem dependent. The larger it becomes, the more the maximum violated constraint is penalized. There are two ways to define PW: automatic and user specified. For the automatic way, PW = 10 * the initial objective from the initial design cycle. This is the default option. Alternatively, the user can provide his own through a Bulk Data Parameter, MXLAGM1 (See Input Section). Then, PW = 10.* MXLAGM1. Rejecting a Design If Ratio < η 1 , the current design will be rejected. When the flag is set, the subsequent design sensitivity phase will be skipped and the approximate optimization job will be performed based on the previous good design with reduced move limits.

Input New Parameters added to the DOPTPRM entry TREGION

Flag to invoke Trust Region method. = 0 (Default) Don’t employ trust regions = 1 turn Trust Region on

ETA1 ( η 1 )

the cutting ratio 1 (Default = 0.01), used by Trust Region Method.

ETA2 ( η 2 )

the cutting ratio 2 (Default = 0.25), used by Trust Region Method.

ETA3 ( η 3 )

the cutting ratio 3 (Default = 0.7), used by Trust Region Method.

UPDFAC1

Updating Factor 1 (Default = 2.0), used by Trust Region Method.

UPDFAC2

Updating factor 2 (Default = 0.5), used by Trust Region Method.

DPMAX

Maximum fraction of change on designed property (Default = 0.5) , used by Trust Region Method.

DXMAX

Maximum fraction of change on design variable (Default = 1.0), used by Trust Region Method.

226 MD Nastran 2006 Release Guide

Bulk Data Parameter PARAM,MXLAGM1,VALUE - Control parameter for Penalty Weight (Real, Default = 0.0).

Outputs Special Printout from DOM12 If Trust Region method is invoked, DOM12 prints out additional information message as shown below. This message is printed out once every design cycle. The left column is design cycle number. It prints out Objective, Maximum violated constraint and merit function for exact current, exact previous and approximate. It further prints out Ratio together with numerator, denominator. It also prints out the final Update factor for move limits plus the rejecting status. Finally, it prints out current move limits for property and design variable ply penalty weight.

DCYCL OBJECTIVE 2 PREV 6.893711E+00 CURR 9.935308E+00 APPX 9.935904E+00 MOVEP,MOVP-MIN = MOVEX,MOVX-MIN = NDOFs(NDV-NACS)= PENAL WEIGHT =

MAX-CONS 2.133793E+01 1.392006E+01 1.391907E+01 5.000000E-01 1.000000E+00 0 0.6894E+02

MERIT-FUN 1.477869E+03 9.695438E+02 9.694761E+02 1.000000E-02 5.000000E-02

NUMER 5.0832E+02

DENOM 5.0839E+02

RATIO 9.9987E-01

UPFAC REJ-FLAG TTTT 2.0000E+00 0 TTTT TTTT TTTT TTTT TTTT TTTT TTTT

Marker Indicating a Rejected Design in Design History A rejected design will be marked by adding symbol ‘R’ to the design cycle number shown in the Summary of Design Cycle History at the end of f06 file. Below is an example that shows design cycle 2 has been marked with ‘R’. This is because although this design produces a smaller objective but with the violated constraint. So the design is rejected. Design cycle 1 is used as the next starting design point.

*************************************************************** S U M M A R Y O F D E S I G N C Y C L E H I S T O R Y *************************************************************** (HARD CONVERGENCE ACHIEVED) NUMBER OF FINITE ELEMENT ANALYSES COMPLETED NUMBER OF OPTIMIZATIONS W.R.T. APPROXIMATE MODELS

16 15

OBJECTIVE AND MAXIMUM CONSTRAINT HISTORY --------------------------------------------------------------------------------------------------------------OBJECTIVE FROM OBJECTIVE FROM FRACTIONAL ERROR MAXIMUM VALUE CYCLE APPROXIMATE EXACT OF OF NUMBER OPTIMIZATION ANALYSIS APPROXIMATION CONSTRAINT --------------------------------------------------------------------------------------------------------------INITIAL 1

6.614414E+02 5.987441E+02

5.987546E+02

1.102773E-01 -1.743120E-05

-4.438843E-04

2R

5.475672E+02

5.475823E+02

-2.764282E-05

2.106060E+00

3

5.626934E+02

5.627052E+02

-2.104267E-05

-3.308058E-04

CHAPTER 7 227 Optimization

Guidelines and Limitations 1. All new parameters introduced in the DOPTPRM have their own defaults and are usually adequate. If you want the optimization job to have more aggressive move limit, you may do so by reduce ETA3 and/or increase DPMAX and DXMAX or increase UPDFAC1. Conversely, you may increase ETA3 and/or reduce DPMAX, DXMAX and/or decrease UPDFAC1. 2. A non-zero MXLAGM1 is used to override the default Penalty Weight (PW). This parameter is problem dependent and may require some iteration to come up a good number. When the need arises to specify one, a general rule is to specify a bigger number (say 100. and larger) for the maximum constraint is grossly violated. 3. In some cases, it is possible that activating Trust Region in SOL 200 may produce less

desirable result than a non-Trust Region job.

Examples The example (dtrustr2.dat) is a Stiffened Panel constrained optimization job taken from the testing problem library (d200x7.dat). It tries to minimize a weight response while satisfies stress and displacement constraints. The same job was run with and without Trust Region (TR). The Trust Region is invoked by specifying TREGION=1 on the DOPTPRM entry. In addition, the parameter MXLAGM1 is set to 10. Figure 7-9 plots the objective history and DELX history with and without TR. The TR job converges at

design cycle 15 (notice that plots count initial design cycle as 1 that is actually zero if counted in the f06) while the non-TR job converges at design cycle 27. Both has same final objective function with maximum feasible constraint at the tolerance of GMAX=0.5%. The fast convergence achieved by the TR job may be explained by the DELX history shown at the bottom of Figure 7-9. The non-trust region job uses a constant move limit (e.g., DELX=0.5) while the DELX in the trust region job is adaptively updated: between design cycles 2 and 6, DELX=1.0 and then reduced below 0.5 between design cycles 8 and 14. Finally, Figure 7-10 plots the maximum constraint values with and without TR. Listing 7-7 lists the summary of the design history.

16.0

6.0 5.5 5.0 4.5 4.0 3.5 3.0 2.5 2.0 1.5 1.0 0.5 0.0

14.0

Objective

12.0 10.0 8.0 6.0 4.0 2.0 0.0 0

5

10

15

20

25

Fraction of Move Limit

228 MD Nastran 2006 Release Guide

30

Design Cycle OBJ-TR

Figure 7-9

OBJ-NTR

DELX-TR

DELX-NTR

Objective History of Example 2: Trust Region vs. Non-Trust Region

1.4

Maximum Constraint

1.2 1.0 0.8 0.6 0.4 0.2 0.0 -0.2

0

5

10

15

20

25

30

Design Cycle MaxC-TR

Figure 7-10

MaxC-NTR

Max. Constraint History of Example 2: Trust Region vs. Non-Trust Region

CHAPTER 7 229 Optimization

Listing 7-7

Table Summary of Objective and Maximum Constraints

INITIAL

5.784520E+00 1 2 3 4 5 6 7R 8R 9 10R 11 12 13 14 15

8.610938E+00 6.194046E+00 7.550942E+00 7.982732E+00 7.912356E+00 7.772725E+00 7.562489E+00 7.575960E+00 7.943342E+00 7.829101E+00 7.925030E+00 7.889203E+00 7.907179E+00 7.924466E+00 7.924493E+00

1.291873E+00 8.610291E+00 6.193711E+00 7.550880E+00 7.982616E+00 7.912348E+00 7.772723E+00 7.562516E+00 7.575985E+00 7.943305E+00 7.829069E+00 7.925027E+00 7.889194E+00 7.907176E+00 7.924470E+00 7.924493E+00

7.509516E-05 5.412208E-05 8.146334E-06 1.451547E-05 1.084769E-06 1.840425E-07 -3.657057E-06 -3.398793E-06 4.622315E-06 4.019795E-06 4.211797E-07 1.148394E-06 3.015218E-07 -5.415548E-07 0.000000E+00

6.616151E-01 5.258847E-01 2.141915E-01 9.803727E-02 6.846836E-02 5.525844E-02 6.685141E-02 6.633586E-02 1.302273E-02 1.883844E-02 9.176641E-03 8.753594E-03 3.031719E-03 3.125000E-06 -1.562500E-07

References 1. MSC.Nastran 2004 Design Sensitivity and Optimization User’s Guide, MSC.Software Corporation, Santa Ana, CA., 2003 2. MSC.Nastran 2005 Release Guide, MSC.Software Corporation, Santa Ana, CA., 2004 3. Prof. L. Lasdon, private communication, Dec. 13, 2004.

230 MD Nastran 2006 Release Guide

Support of Analysis Model Value Overriding Design Model Value Introduction In SOL 200, when the value of an analysis model property is different from a design model value obtained by the relation defined on a DVxREL1 entry, the design model value overrides the analysis model value. The new PVAL option provides an alternate to allow the analysis model value to take the precedence over the design model value.

Benefits Provides a flexible way for a sizing optimization job to start with either design model values or analysis model values.

Input The PVAL option is applicable to three linear design property entries: DVPREL1, DVCREL1 and DVMREL1. To activate this option, specify the character input of “PVAL” on the COEF1 field on a DVPREL1 (DVCREL1, DVMREL1) entry.

Output None.

Example The example shows designing a plate thickness. The plate thickness, 2.5, is defined on PSHELL 1 entry. First, the design entries without the PVAL option are given below. In this case, the design model value, 2.0 (the product of the initial design variable value, 1.0 and the coefficient, 2.0 on the DVPREL1 entry) will override the analysis model value. The comparison of analysis model value and design model value printed in the f06 file is shown here: PSHELL DESVAR DVPREL1

1 1 1 1

2 THICK PSHELL 2.0

2.5 1. 1

0.1 T

10.

CHAPTER 7 231 Optimization

----- COMPARISON BETWEEN INPUT PROPERTY VALUES FROM ANALYSIS AND DESIGN MODELS ---------------------------------------------------------------------------------------------------------------------------------------------------------------PROPERTY PROPERTY PROPERTY ANALYSIS DESIGN LOWER UPPER DIFFERENCE SPAWNING TYPE ID NAME VALUE VALUE BOUND BOUND FLAG FLAG -----------------------------------------------------------------------------------------------------------------------------------------------------------PSHELL

1

T

2.500000E+00 2.000000E+00 N/A

N/A

WARNING

Then, the DVPREL1 entry with the PVAL option is shown here with other two entries being kept the same. In this case, the design model value equals the analysis model property value, 2.5 obtained directly from the 4th field of PSHELL 1 entry. The similar comparison of analysis model value and design model value is printed in the f06 file. DVPREL1

1 1

PSHELL PVAL

1

T

----- COMPARISON BETWEEN INPUT PROPERTY VALUES FROM ANALYSIS AND DESIGN MODELS ---------------------------------------------------------------------------------------------------------------------------------------------------------------PROPERTY PROPERTY PROPERTY ANALYSIS DESIGN LOWER UPPER DIFFERENCE SPAWNING TYPE ID NAME VALUE VALUE BOUND BOUND FLAG FLAG -----------------------------------------------------------------------------------------------------------------------------------------------------------PSHELL

1

T

2.500000E+00 2.500000E+00 N/A

N/A

NONE

Guidelines and Limitations 1. The PVAL option only applies to the linear design property entries and is not applicable to DVxREL2 entries. 2. When the PVAL option is used, only a single design variable can be referenced on a DVxREL1 entry and PVAL is applied to the COEF1 field. If a DVxREL1 entry references more than one design variable with the PVAL option, a user fatal error message will be issued.

232 MD Nastran 2006 Release Guide

MD Nastran 2006 Release Guide Ch. :

8

Miscellaneous Enhancements

J

Export of Static Loads, 234

J

Enhanced Participation Factor Results, 237

J

Total Strain Energy Output for Defined SETs, 249

J

Model Checkout Procedures - Method to Vary Material Properties, 252

234 MD Nastran 2006 Release Guide

Export of Static Loads Introduction Functionality was added to MD Nastran to facilitate load transfer from one run to the next in three important ways: 1. MD Nastran can use Grid Point Force methodology to extract the load on a user defined free body. This load is output on a PG-like matrix that has an associated NAME, ID and optional label. A BGPDT data block is also produced that contains information on the grids associated with the free-body. 2. MD Nastran can export static loads from a load case defined in the current subcase. 3. MD Nastran can now import a load from a pre-defined database (including, but not limited to, loads produced using the previous steps) to be used in the formation of the load on a structure.

Benefits The design of complex structures frequently involves joint development with a system integrator and a number of subcontractors. The development of design loads is typically the task of the system integrator based on an analysis of the entire vehicle. It is then necessary to communicate the loads on the pieces of the structure to various subcontractors. The ability to extract the load on a free body is particularly useful in aeroelasticity, where the load can be a combination of applied, rigid aerodynamic and inertial loadings. The ability to export the statically applied load, or some portion of the load, is felt to be of benefit when it is desired to apply the same loading to different representations of the same structure.

Input The ability to export a statically applied load is enabled by the new EXPORTLD Case Control command as described in the MD Nastran 2006 Quick Reference Guide. Typically, this is applied at the subcase level, but can be applied above the subcase level as well. In any case, the command results in a unique load vector (qualified by LOADID and LOADNAME) for each subcase. If a subset of grids is provided by identifying a SET Case Control command as part of the EXPORTLD command, only the loads on the grids associated with this grid are exported. A BGPDT (Basic Grid Point Data Table) is output with the load vector to identify the degrees of freedom associated with each of the rows in the vector. The ability to export a free body load is done through the combination of the new FBODYLD Case Control command and the FBODYLD and FBODYSB Bulk Data entries. The FBODYLD Case Control command is used to point to the FBODYLD Bulk Data (via the NAMEi called out on the case control command) that defines the submodel for which the freebody load will be calculated and stored. The case control command also provides an optional load ID that can be associated with the load. The FBODYLD Bulk Data entry, in turn, points to a FBODYSB Bulk Data entry. The FBODYLD entry provides a label that is intended to identify the loading condition while the FBODYSB entry has a second label that is intended to identify the component. Both labels are optional. The FBODYSB entry identifies the grids

CHAPTER 8 235 Miscellaneous Enhancements

and elements that make up the free body and provides the ability to exclude certain types of grid point forces in creating the free body load. The remarks for the EXPORTLD Case Control command indicate how the loads created with an EXPORTLD request can be used in a subsequent run using FMS statements such as: ASSIGN loads1=’run1.MASTER’ DBLOCATE datablk=(EXTLD,EXTBGP) WHERE(LOADNAME=’ALLCASES’), CONVERT(LOADID=LOADID+1000) LOGICAL=loads1 … CEND LOADS=1001 $ Select external load with LOADID=1001, imported from previous run. The EXTLD datablock contains the loads whereas the EXTBGP contains the grid point information that is used to match up the imported loads with the grid points. Clearly, it is necessary that the Grid ID’s have the same meaning in the two runs. The import of a load created using the FBODYLD Case Control command is similar except it is now necessary to rename the datablocks created in the previous run to match those required for the import of these loads: ASSIGN loads1=’fbrun1.MASTER’ DBLOCATE datablk=(FBLPG/EXTLD,FBLBGPDT/EXTBGP) WHERE(LOADNAME=’fblcase’), CONVERT(LOADID=LOADID+1000) LOGICAL=loads1 … CEND LOADS=1001 $ Select external load with LOADID=1001, imported from previous run.

Output The new commands produce limited output. The FBODYLD request does produce informational messages from a DBDICT statement that requests output on the presence of all FBLPG and FBLBGPDT data blocks along with qualifiers as to loadid, namei (from case control and the FBODYLD Bulk Data entry), submodel name from the FBODYSB entry and the labels from the two bulk data entries.

Examples (TPL: exptld/imptld, sysmod/fbody, sfsw/ffsw) There are three simple sets of test cases in the text problem library that demonstrate these new features, each with an export import pair. Exptld.dat exports the load applied to the center section of a flat plate while imptld.dat applies this load to a model of only the center section of the plate. In this case, it is not necessary to dblocate the EXBGP datablock because the exported load is perfectly aligned with the reduced model. However, this is not a good practice in general. Sysmod.dat is a SOL 101 run that creates a free body load on center section of the same small plate model used in the previous example. Note that the applied loads are excluded using an input of “A” on the XFLAG field of the FBODYSB Bulk Data entry. Only the element forces are used to create the load,

236 MD Nastran 2006 Release Guide

which is in equilibrium across the cutout. The fbody.dat file imports this load onto a model that is only the center section of the original model. It is necessary to constrain a corner of this “free body” to remove the rigid body motion. An examination of the .f06 results for this run shows that the SPC forces are negligible while the stresses agree well for the elements that are shared between the two models. The displacements do not agree, but this is to be expected because they displacements for the small model are relative to the artificially constrained model. Sfsw.dat is a SOL 144 run that demonstrates the ability to ask for different free body loads is separate subcases and has multiple FBODYLD/FBODYSB pairs for different components of the familiar forward swept wing. The fuselage subsystem is selected for further analysis in the subsequent run and it is seen the FBODYSB entry with FUSELAGE in the NAMES field has the applied loads excluded using an ‘A’ in the XFLAG field. Ffsw.dat imports this load into a SOL 101 that only has a model of the fuselage and comparison of the results shows that the stresses in the bars that represent the fuselage agree well between the two runs.

Guidelines and Limitations The EXPORTLD command has utility in SOL 101. In SOL 144, only the applied loads are output with this command and these are typically zero. The applied loads are typically excluded when using the FBODYSB Bulk Data entry so that only element forces remain at the grid points. Import of loads has the following rules • If a set of imported loads share a common LOADID value, then those loads will implicitly be

added. The same holds true for imported loads and bulk data load sets that share a common ID. • To explicitly combine load sets, the load IDs should be made unique. The LOAD Bulk Data

entry can then be used to explicitly define the linear combination. • Both standard exported loads (EXPORTLD) and free body loads (FBODYLD) can be imported

and used together in a single run. It is up to the user to keep the load IDs unique between them. • The BGPDT is used to link the exported loads to the grids points of the model to which they are

applied. This means that the grid id’s for the loaded grids must be the same in the two models.

CHAPTER 8 237 Miscellaneous Enhancements

Enhanced Participation Factor Results Introduction New Case Control commands PFMODE, PFPANEL and PFGRID have been implemented to request modal, panel and grid participation factors. These commands will replace the existing FLSPOUT and MCFRACTION Case Control commands. A new, consistent output format is used for all types of modal and panel participation factors. This format is similar to the output format obtained with the MCFRACTION command. The output format of grid participation factors is similar to the output format of displacements. In addition, the new implementation supports • panel definition by referencing a set of grids, a set of elements or a set of properties. • panel and grid participation factors in direct frequency response analysis (SOL 108).

Finally, an adjoint method is used to compute acoustic structural modal participation factors, acoustic panel participation factors and acoustic grid participation factors, resulting in significant performance improvements.

Benefits • The new case control commands and the new output formats provide a consistent user interface

to all kinds of participation factors that is easy to use. • The following example shows significant reductions of computation times and IO when

computing panel participation factors: Problem Data 3.3 mio. 25000 1022 45 85

Structural Degrees of Freedom Fluid Degrees of Freedom Structural Modes Fluid Modes Subcases

Panel participation factors have been computed for 2 fluid grid points and 9 panels.

Performance Data WO/Panel Part. Elapsed Time (s) CPU Time (s) IO (GB)

22020 9027 24426

W/Panel Part. 3960 1332 6415

These data refer to the computation of the participation factors only.

238 MD Nastran 2006 Release Guide

Theory In a linear structural dynamic analysis, the results at a degree of freedom considered are the sum of the contributions of the different modes, e.g., the accelerations at a degree of freedom considered are the sum of the accelerations due to the responses of the different structural modes. These contributions are called structural modal participation factors or modal contribution fractions. The degrees of freedom considered are called response degrees of freedom. Structural modal participation factors allow to identify the structural modes that have the largest influence on the response. Likewise, in an acoustic analysis, the pressure at a grid point considered is the sum of the pressures due to the responses of the different fluid modes. These contributions are called acoustic fluid modal participation factors. Acoustic fluid modal participation factors allow to identify the fluid modes that have the largest influence on the response. In a coupled analysis, the pressure at a response degree of freedom is the sum of the pressure due to the acoustic sources in a rigid cavity, and the pressure due to the acceleration of the fluid-structure interface, the so-called wetted surface. The pressure due to the acoustic sources in a rigid cavity is called the load participation factor. The acceleration of the fluid-structure interface is the sum of the accelerations due to the responses of the different structural modes, obtained from a coupled analysis. These contributions are called acoustic structural modal participation factors. One acoustic structural modal participation factor equals the

CHAPTER 8 239 Miscellaneous Enhancements

pressure at the response degree of freedom if there are no acoustic sources, and if the acceleration of the wetted surface consists of the response of one mode only. Thus, the acoustic structural modal participation factors allow to identify the structural modes that have the largest influence on the pressure at the grid point considered. In the absence of acoustic sources within the cavity, the acoustic structural modal participation factors sum up to the total pressure at the response degree of freedom. Modal participation factors, by their nature, are useful only in the low-frequency range where the resonance frequencies are well separated, and the response is dominated by a small number of modes. On the contrary, geometric participation factors are useful also at higher frequencies where the response has contributions from a large number of modes. There are two types of geometric participation factors, namely panel participation factors and grid participation factors. A panel is a set of grid points of the wetted surface. The panel participation factor is that pressure at the grid point considered that results from the accelerations of the grid points of the panel only, with all other grid points of the wetted surface kept fixed. Thus, panel participation factors allow to identify the regions of the wetted surface that have the largest influence on the acoustic pressure at the grid point considered. Panel participation factors usually do not sum up to the total acoustic pressure. This is only the case if the panels do not overlap, and if their union equals the complete wetted surface. The accelerations of the grid points of the panel are the sum of the accelerations due to the different structural modes. The pressure due to the accelerations at the grid points of the panel that are due to one mode only is called the acoustic panel modal participation factor. Acoustic panel modal participation factors sum up to the panel participation factors. Finally, if the panels consist of one grid point only, acoustic grid participation factors are obtained. For each structural grid point of the wetted surface, there are six acoustic grid participation factors, i.e. the pressures at the response degree of freedom due to the accelerations of the six degrees of freedom of this grid point. The acoustic grid participation factors depend on the mesh size. Thus, their absolute value has no physical meaning. However, if the mesh of the wetted surface is of comparable size everywhere, the acoustic grid participation factors allow to quickly identify the regions that make the largest contribution to the acoustic pressure at the grid point considered, and thus help to define the panels. Participation factors are complex quantities, summing up to the complex response. Thus, if they are divided by the response, they sum up to one. The participation factors divided by the response are called normalized participation factors. Normalized participation factors are complex quantities, too. The real parts of the normalized participation factors sum up to one whereas the imaginary parts sum up to zero. Thus, the real part of a normalized participation factor is that part of the participation factor that is in phase with the total response, divided by the magnitude of the total response. It is called the modal fraction. The phase of a normalized participation factor is the phase of the participation factor relative to the total response. If the modal fraction is multiplied by the magnitude of the total response, the projected participation factor is obtained. It is that part of the participation factor that is in phase with the total response. The projected participation factors sum up to the total magnitude.

240 MD Nastran 2006 Release Guide

Input Computation and output of modal participation factors is controlled by the PFMODE Case Control command:  PFMODE  STRUCTURE , PRINT, PUNCH , REAL or IMAG ,  FLUID PLOT PHASE  ALL  [ SORT = sorttype ], [ KEY = sortitem ], ITEMS =   ,  ( itemlist )   ALL   ALL      FLUIDMP =  m f  , STRUCTMP =  m s  ,      NONE   NONE   ALL   ALL      PANELMP =  setp  , SOLUTION =  setf  , [ FILTER = fratio ]      NONE   NONE  ,  setdof  [ NULL = ipower ] ) =    NONE 

Examples SET 20 = 25/T3, 33/T3 PFMODE(STRUCTURE, STRUCTMP=ALL) = 20 Compute structural modal participation factors for z-translations at grid points 25 and 33 SET 20 = 11217 SET 90 = 25., 30., 35. PFMODE(FLUID, STRUCTMP=ALL, FLUIDMP=ALL, SOLUTION = 90) = 20 Compute acoustic structural and fluid modal participation factors for pressure at grid point 11217 at excitation frequencies 25Hz, 30Hz and 35Hz. Computation and output of panel participation factors is controlled by the PFPANEL Case Control command:

CHAPTER 8 241 Miscellaneous Enhancements

  ALL  PFPANEL  PRINT, PUNCH , REAL or IMAG , PANEL =  -----------  ,  PLOT PHASE  setp    ALL [ SORT = sorttype ], [ KEY = sortitem ], ITEMS =   ,  ( itemlist )   ALL    SOLUTION =  setf  , [ FILTER = fratio ], [ NULL = ipower ]    NONE    =  setdof   NONE 

Example SET 100 = 10., 12. SET 200 = 1222, 1223 PFPANEL(SOLUTION=100, SORT=ABSD) = 200 Compute acoustic panel participation factors for pressure at grid points 1222 and 1223 at excitation frequencies 10Hz and 12Hz. Output is sorted according to descending modal fractions. Computation and output of grid participation factors is controlled by the PFGRID Case Control command:   ALL  PFGRID  PRINT, PUNCH , REAL or IMAG , GRIDS =    PLOT PHASE  setg   ALL    SOLUTION =  setf     NONE 

   setdof   =     NONE  

Example SET 20 = 11217 SET 90 = 25., 30., 35. PFGRID(SOLUTION = 90) = 20 Compute acoustic grid participation factors for the pressure at grid point 11217 at excitation frequencies 25Hz, 30Hz and 35Hz. Detailed descriptions of the PFMODE, PFPANEL and PFGRID Case Control Commands can be found in the Quick Reference Guide.

242 MD Nastran 2006 Release Guide

Panels are defined in the Bulk Data Section using PANEL Bulk Data entries which reference SET1 or SET3 Bulk Data entries. • SET1 Bulk Data entries list the grid points of the panels. • SET3 Bulk Data entries with option ELEM list the elements of the panels. The panels consist of

all grid points associated to these elements. • SET3 Bulk Data entries with option PROP list the property identifiers of the elements of the

panels. The panels consist of all grid points associated to the elements with the property identifiers defined.

Output Output can be printed to the .f06 file, written to the .pch file or the .op2 file or stored in the database for later access by SimOffice. Three different formats are used for printed output to the .f06 files. The format for modal participation factors is similar to the format obtained with the MCFRACTION command. The header contains the type of the participation factor, information on the grid point and degree of freedom considered, the total response, information on excitation frequency, subcase and load and information on the maximum modal response, the sort method and the filter. In case of acoustic panel modal participation factors, the header contains the name of the panel considered and the panel response instead of the total response. The data are presented in ten columns:

Column 1

Label Mode Id

Description Mode number

2

Natural Freq (Hz)

Resonance frequency

3-4

Modal Response: Real / Imaginary

Real and imaginary part of participation factor

5-6

Modal Response: Magnitude / Phase

Magnitude and phase of participation factor

7

Projection Magnitude

Projected participation factor: That part of the participation factor that is in phase with the total response

8

Relative Phase

Phase of participation factor relative to total response

9

Modal Fraction

Real part of normalized participation factor

10

Scaled Response Magnitude

Projected participation factor divided by largest magnitude of all participation factors

The format for acoustic panel participation factors is the same as for modal participation factors, except that the first two columns contain the panel names.

CHAPTER 8 243 Miscellaneous Enhancements

Load participation factors are included in the acoustic structural modal participation factors and the acoustic panel participation factors, with a mode number of 0 and a panel name –LOAD-. Acoustic structural modal participation factors, together with the load participation factor, sum up to the total response. Acoustic grid participation factors use the output format of complex displacements. Both real and imaginary part or magnitude and phase format are available. There is one output per excitation frequency and fluid grid point.

Example

The numbers printed indicate the normalized acoustic pressure at the selected grid point due to the accelerations at the corresponding degrees of freedom.

Guidelines The amount of output produced may be very large. This is especially true for acoustic panel mode participation factors and for acoustic grid participation factor (e.g., the number of data produced for acoustic panel modal participation factors equals the number of subcases times the number of excitation frequencies times the number of response degrees of freedom times the number of panels times the number of structural modes). Consequently, output should be limited to a small number of excitation frequencies and to a small number of response degrees of freedom.

244 MD Nastran 2006 Release Guide

Limitations In the current version, acoustic participation factors are not computed correctly in case of direct enforced motion.

Example The example shows the acoustic analysis of a cabin. The cabin is excited by four forces at the corners of the seat. The result of interest is the pressure at the driver’s ear. The frequency response of the pressure shows a peak at 37Hz. To investigate this peak, acoustic fluid and structure modal participation factors and panel participation factors are requested at a frequency of 37Hz. Panels are defined for the front window, the rear wall, the left and the right side, the top and the bottom.

Input Data $ Participation Factor Test Problem: Cabin $ $ Coupled Modal Frequency Response Analysis $ $ Participation Factor Example - Cabin

CHAPTER 8 245 Miscellaneous Enhancements

$ $ Illustrates use of $ o Acoustic Fluid Modal Participation Factors $ o Acoustic Struct. Modal Part. Factors $ o Acoustic Panel Part. Factors $ o Acoustic Grid Part. Factors $ $ ======================================================= $ SOL 111 DIAG 8 CEND $ ECHO=SORT(EXCEPT,CBEAM,CQUAD4,CHEXA,CPENTA,GRID) AUTOSPC(NOZERO) = YES $ METHOD(STRUCTURE)=1 METHOD(FLUID) =2 $ FREQ = 100 DLOAD = 200 $ SET 1 = 11217 SET 20 = 11217 SET 90 = 37. $

246 MD Nastran 2006 Release Guide

DISP(PHAS) = 1 $ PFMODE(FLUID, STRUCTMP=ALL, FLUIDMP=ALL, SOLUTION=90, SORT=ABSD) = 20 PFPANEL(SOLUTION=90, SORT=ABSD) = 20 $ OUTPUT(XYPLOT) XPAPER=29. YPAPER=21. XGRID=YES YGRID=YES XTITLE = Frequency YTITLE = Pressure XYPLOT DISP RESPONSE / 11217(T1) $ BEGIN BULK $ $ Request OP2 for PATRAN PARAM, POST, -1 $ $ Define Structural Damping PARAM, G, 0.02 $ $ Define Fluid Damping PARAM, GFL, 0.002 $ $ Define Reference Pressure for dB (in Pa) PARAM, PREFDB, 2.8284-5 $ PARAM, GRDPNT, 0 $ Request Weight Output $ $ Structural and Acoustic Modes up to 300Hz EIGRL, 1,,300. EIGRL, 2,,300. $ $ Frequency Range: 25Hz to 100Hz by Steps of 5Hz FREQ1, 100, 25., 5., 15 $ Additional Frequencies around Resonance Frequencies FREQ4, 100, 25., 100., 0.01, 5 $ $ Excitation Forces RLOAD1, 200, 210,,, 220 DAREA, 210, 1, 3, 1., 7, 3, 1. DAREA, 210, 29, 3, 1., 35, 3, 1. TABLED1, 220 , 0., 1., 1000., 1., ENDT $ $ Nonmatching Fluid-Structure Interface ACMODL, DIFF $ $ Include Structural and Acoustic Model INCLUDE 'cabin_structure.bdf' INCLUDE 'cabin_fluid.bdf' $

CHAPTER 8 247 Miscellaneous Enhancements

$ Panels $ SET3, 101, ELEM, 127, THRU, 162, 667, THRU, 738 SET3, 201, ELEM, 37, THRU, 72, 739, THRU, 810 SET3, 301, ELEM, 331, THRU, 384 SET3, 401, ELEM, 25, THRU, 36, 73, THRU, 126 SET3, 501, ELEM, 271, THRU, 294, 601, THRU, 612 SET3, 601, ELEM, 1, THRU, 24, 455, THRU, 478, , 497, THRU, 562 $ PANEL, LEFT, 101, RIGHT , 201, FRONT, 301, REAR, 401 PANEL, TOP , 501, BOTTOM, 601 $ ENDDATA Acoustic Structural Mode Participation Factors:

248 MD Nastran 2006 Release Guide

Acoustic Panel Participation Factors:

The acoustic structural mode participation factors show that the largest contribution comes from the 7th structural mode which has a resonance at 37.2Hz. The acoustic panel participation factors show that the rear wall and the bottom make the largest positive contribution whereas all remaining panels make negative contributions.

CHAPTER 8 249 Miscellaneous Enhancements

Total Strain Energy Output for Defined SETs Introduction Total Strain Energy output can now be requested for user defined element SETs.

Inputs A new Case Control command, SETP described below is introduced for defining the list of element SETs, which are referenced by the ESE – Element Strain Energy Output request.

SETP

Process Set Definition

Process Sets are used to define lists of SET identifications to be processed individually for data recovery:

Formats SETP n = {i1[,i2,i3 THRU i4 EXCEPT i5,i6,i7,i8 THRU i9]}

Examples SET 77=5 SET 88=5, 6, 7, 8, 9, 10 THRU 55

Describer n

Meaning SETP identification number. Any SETP may be redefined by reassigning its identification number. SETPs specified under a SUBCASE command are recognized for that SUBCASE only. (Integer > 0) SET Identification numbers. If no such identification number exists, the request is ignored. (Integer > 0)

EXCEPT

Set identification numbers following EXCEPT will be deleted from output list as long as they are in the range of the set defined by the immediately preceding THRU. An EXCEPT list may not include a THRU list or ALL.

Remarks: 1. A SETP command may be more than one physical command. A comma at the end of a physical command signifies a continuation command. Commas may not end a set. THRU may not be used for continuation. Place a number after the THRU. 2. Set identification numbers following EXCEPT within the range of the THRU must be in ascending order.

250 MD Nastran 2006 Release Guide

In SET 88 above, the numbers 77, 78, etc., are included in the set because they are outside the prior THRU range. 3. SETP usage is limited to the EDE, EKE, and ESE Case Control Commands.

Example A small example (see setp01.dat in the examples folder) is shown below to show usage of the SETP command. Note only essential entries are shown. id msc, setp $ TIME 6 SOL 101 CEND SPC=1 setp 100 = 1 thru 43 set 1 = 1 set 2 = 2 set 3 = 3 set 4 = 4 set 5 = 5 set 6 = 6 set 7 = 7 set 8 = 8 set 9 = 9 . . SUBCASE 1001 LOAD=101 ese = 100 SUBCASE 1002 LOAD=102 ese = 100 BEGIN BULK CQUAD4 1 1 CQUAD4 2 1 CQUAD4 3 1 CQUAD4 4 1 CQUAD4 5 1 CQUAD4 6 1 CQUAD4 7 1 CQUAD4 8 1 CQUAD4 9 1 . . ENDDATA

1 2 3 4 5 6 8 9 10

2 3 4 5 6 7 9 10 11

9 10 11 12 13 14 16 17 18

8 9 10 11 12 13 15 16 17

CHAPTER 8 251 Miscellaneous Enhancements

Output Example An excerpt of the element strain energy output for the example is shown below: 0 E L E M E N T ELEMENT-TYPE = QUAD4 SUBCASE 1001

S T R A I N

SUBCASE 1001

E N E R G I E S

* TOTAL ENERGY OF ALL ELEMENTS IN PROBLEM * TOTAL ENERGY OF ALL ELEMENTS IN SET

= 1 =

4.593646E+00 2.973878E-03

0 ELEMENT-ID 1 TYPE = QUAD4

STRAIN-ENERGY 2.973878E-03

SUBTOTAL

2.973878E-03

PERCENT OF TOTAL 0.0647

STRAIN-ENERGY-DENSITY 1.631036E+00

0.0647

0

SUBCASE 1001 E L E M E N T ELEMENT-TYPE = QUAD4 SUBCASE 1001

S T R A I N

E N E R G I E S

* TOTAL ENERGY OF ALL ELEMENTS IN PROBLEM * TOTAL ENERGY OF ALL ELEMENTS IN SET

= 2 =

4.593646E+00 1.778719E-03

0 ELEMENT-ID 2 TYPE = QUAD4

SUBTOTAL

STRAIN-ENERGY 1.778719E-03 1.778719E-03

PERCENT OF TOTAL 0.0387 0.0387

STRAIN-ENERGY-DENSITY 5.811762E-01

252 MD Nastran 2006 Release Guide

Model Checkout Procedures - Method to Vary Material Properties Introduction A new feature has been introduced that provides users with a simple means to evaluate the mass and thermal load characteristics of a structure. The feature is intended primarily for linear static analysis runs that are being used to validate aspects of the finite element model prior to embarking on more expensive production static and dynamics analyses. It allows the user to temporarily modify the material density and thermal expansion coefficient fields of material property bulk data entries. To implement the feature, the new MODEL_CHECK Executive Control statement and several NASTRAN Statement keywords have been introduced. Use of the feature causes the affected material property fields to be temporarily modified during the run. All results will be based on the temporary values of the material properties. The material property data stored on the Material Property Table data block is not modified and retains the original values supplied on the bulk data entries.

Benefits The introduction of this new feature simplifies the procedure typically used to evaluate the mass and thermal load characteristics of a finite element model. This procedure usually involves preparation, usage and storage of a duplicate set of bulk data material property entries that have the material density and thermal expansion coefficient values set to the values desired for model checkout purposes. When the model is undergoing checkout procedures, the production set of bulk data material property entries is replaced by the alternate set of bulk data material property entries. Creating and switching between the two sets of data for production and checkout runs is tedious and prone to errors. The material property update options of the MODEL_CHECK statement improve user productivity by reducing the need to create, maintain and substitute different sets of material properties needed for model check purposes.

Method and Theory There is no additional theory introduced by this feature. Finite element matrix generation and stress recovery operations use material properties in exactly the same manner as without this feature. The only difference is the actual value of the material property itself. The method is equally simple. As material property data is referenced, a check is made to see whether MODEL_CHECK is active for temporary material property updates. If it is, the appropriate entry of the material property data (mass density and/or thermal expansion coefficient(s)) is set to the user-specified value. All subsequent computations use the updated value.

Inputs This feature is activated using the new MODEL_CHECK Executive Control statement. The MODEL_CHECK statement features keywords that allow a value to be temporarily assigned to the

CHAPTER 8 253 Miscellaneous Enhancements

material density and thermal expansion coefficients. The general format of the statement used to change material properties to a specified value is: MODEL_CHECK [ MAT_DENSITY=value, ]

[ MAT_TECO=value, ] [ MAT_TEIJ=value ]

The complete description of the MODEL_CHECK statement can be found in Executive Control Statement Descriptions (p. 108) in the MD Nastran Quick Reference Guide.

Outputs The MODEL_CHECK material property update feature produces no printed output other than an informational message summarizing the updates that will take place.

Guidelines and Limitations • MODEL_CHECK is ignored in RESTARTs • Material property updates will take effect for all MAT1, MAT2, MAT3, MAT8 and MAT9 Bulk

Data entries present in the input. • Material properties stored on the Material Property Table (MPT) data block are those present on

the bulk data material property entries. • Post-processing of results could reference in-consistent data since the results are based upon

different material property data than is present in the bulk data.

Demonstration Example A simple example is presented that demonstrates the material property update feature. The example consists of several disjoint models and is not intended to be representative of any production model. The MODEL_CHECK statement is used to temporarily set all material densities and thermal expansion coefficients to 0.0. This results in model mass contributions from only the CONM2 element and the nonstructural mass as well as results for the temperature load case (subcase 3) being null.

Example Input Data $ $*********************************************************************** $ $VERSION: 2004+ $TEST DECK NAME: varmat01a.dat (Baseline Model w/MODEL_CHECK) $ Density is not temperature dependent. $ Thermal expansion coefficient is not temp. dependent $ MODEL_CHECK command present. $ $PURPOSE: $ Demonstrate usage of the new MODEL_CHECK Executive Control Statement $ Note that non-structural mass cannot be modified using this command. $ $DESCRIPTION:

254 MD Nastran 2006 Release Guide

$ The model consists of $ 1) CONM2 eid 3001 contributing mass. $ 2) ROD eid 101 referencing MAT1 materials $ 3) QUAD4 eid 3301 w/ PSHELL referencing MAT1 materials $ 4) QUAD4 eid 3313 w/ PSHELL referencing MAT1 and MAT2 materials $ 5) QUAD4 eid 3321 w/ PCOMP referencing MAT8 materials $ 6) HEXA eid 6701 w/ PSOLID referencing MAT9 materials $ 7) TRIAX6 id 5301 referencing MAT3 materials $ $ A MODEL_CHECK executive command is used to modify material property $ data temporarily during the run. The command demonstrates $ 1) setting the material density to 0.0 via the OFF option $ 2) setting the material thermal expansion coefficients to 0.0 via $ the OFF option $ 3) continuation of MODEL_CHECK command $ $EXPECTED RESULTS: $ 1) There should be an informational message indicating which of the $ material property data is being modified. $ 2) The grid point weight generator and element summary outputs should $ indicate mass for only the conm2 element and the non-structural $ masses of the rods and plates $ 3) results output for subcase 3 (temperature loading) should be 0.0 $ since MODEL_CHECK is setting the alphas=0.0 $ ID MSC, varmat TIME 30 $ SOL 101 $ $======================================================================== $ temporarily set the density and thermal expansion coefficients for all $ materials to 0.0 $ model_check mat_density=off, mat_tecoeff=off,mat_teij=off $ $======================================================================== $ CEND TITLE= VARIABLE MATERIAL TEST CASE SUBTITLE = MSC V2005 ECHO = SORT SPC = 12 TEMP(MATE) = 1 SET 10002= 1 THRU 13999, 14399 THRU 16900 DISP=ALL ELFORCE=ALL OLOAD = ALL $ SPCF=ALL ESE=10002 SEFINAL=1 GPFO=10002 $ ELSUM(EID,PRINT) = ALL $ SUBCASE 1 LABEL = STATIC LOAD LOAD = 1 P2G=MATLOAD K2GG=MATK

CHAPTER 8 255 Miscellaneous Enhancements

SUBCASE 3 LABEL = TURN ON TEMP LOADS TEMP(LOAD) = 2 $ BEGIN BULK $ $ C O M M O N D A T A PARAM, SNORM, 0. $ CORD2C 1 0 3.0 -1.0 +CORD2C 9.0 0.0 -1.0 $ CORD2R 2 0 0.0 -2.0 +CORD2R 0.0 0.0 0.0 $ CORD2S 3 1 3.0 225.0 +CORD2S 3.0 -45.0 3.0 $ GRAV 3 1.0 1.0 TEMPD 1 100.0 TEMPD 2 200.0 $ MAT1 1 1. .8 .1 +MAT11 2.0 3.0 4.0 MATT1 1 2 +MATT1 4 5 6 $ MAT1 2 1.0E+7 0.3 +MAT1-2 1000. 2000. 3000. MATT1 2 +MATT1-2 2 2 $ MAT2 22 1.0E+7 0.5E+6 0.5E+6 +MAT221 .01 .02 .025 100.0 MATT2 22 +MATT221 $ MAT3 33 1.0E+7 1.0E+7 1.0E+7 +MAT331 2.4E+6 .001 MATT3 33 +MATT331 $ MAT8 3 1.E+7 1.E+7 .25 +MAT81 1.-6 2.-6 1.E-4 +MAT82 1.0 $ MAT9 9 1.E+7 +MAT91 +MAT92 5.1+3 5.1+3 +MAT93 .002 .003 .004 .005 MATT9 9 +MATT91 +MATT92 +MATT93 $ TABLEM1 2 +TABLE-2 0.0 1.0 150.0 1.0 +TABL-2 ENDT ENDT TABLEM2 3 100.0 +TABLE-3 0.0 0.1 50.0 0.1

T O

A L L

P R O B L E M S

0.0

9.0

-1.0

0.0

+CORD2C

0.0

1.011234-2.0

0.0

+CORD2R

0.0

3.0

1.234567+CORD2S

1.0

.05

225.0

1.0

.001

100.

.01

+MAT11 +MATT1

.05

.001

100.0

.01

+MAT1-2 +MATT1-2

1.0E+7 0.5E+6 0.035

1.0E+7

.022

+MAT221 +MATT221

.33 .001

.33 .001

.33 100.

4.E+6

4.E+6 1.E-3

4.E+6

.00259 +MAT331 .025 +MATT331 1.0 1.E-4

+MAT81 +MAT82

1.E+7

+MAT91 +MAT92 +MAT93

1.E+7 .006

5.1+3 100.0

.05 .008

.001

+MATT91 +MATT92 +MATT93

150.

0.5

300.

0.5

+TABLE-2 +TABL-2

50.0

0.5

150.0

0.5

+TABLE-3 +TABL-3

256 MD Nastran 2006 Release Guide

+TABL-3 200.0 10.0 ENDT TABLEM3 4 100.0 2.0 +TABLE-4 +TABLE-4 0.0 0.1 25.0 .1 25.0 2.0 75.0 2.0 +TABL-4 +TABL-4 300.0 .00001 ENDT TABLEM4 5 100.0 100. 2.0 10.00 +TABLE-5 +TABLE-5 2.0 ENDT TABLEM4 6 0.0 100. 0.0 100.00 +TABLE-6 +TABLE-6 1.0 .25 ENDT TABLEM1 91 +TAB912 +TAB911 0.0 0.01 150.0 0.05 150. 0.1 300. 0.2 +TAB912 +TAB912 ENDT TABLEM1 92 +TAB921 +TAB921 0.0 0.001 150.0 0.002 150. 0.003 300. 0.006 +TAB922 +TAB922 ENDT TABLEM1 93 +TAB931 +TAB931 0.0 1.0 150.0 1.0 150. 0.08 300. 0.1 +TAB932 +TAB932 ENDT $ PARAM, GRDPNT 0 PARAM, NT 1 PARAM, TINY 0. PARAM, AUTOSPC,YES PARAM, COMPARE,1 $ PROCESS SELECTED S.E., THEN ENTIRE MODEL, DMAP0 PARAM, PNCHDB, 1 $ PUNCH FROM DATA BASE, DMAP0 PARAM, NOELOP, 1 $ SUM OF FORCES. MG 21 OCT 1980 $PARAM, NOGPF, -1 $ SUPPRESS GPFO OUTPUT. LOOK AT ELOP INSTEAD. MG $ $ SPCS TO BE SELECTED FOR RF 1 THRU 12 SPCADD 12 1 2 $ SPCS TO BE SELECTED FOR RF 51,53 AND 59 SPCADD 13 1 3 $ FREQ1 10 0.0 1.0 1 RLOAD2 11 12 14 TABLED1 14 +TABD4.1 +TABD4.1-1.0 1.0001 2.0 1.0001 ENDT $ $ ++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++ ++ $ $ ROD ELEMENT NO. 1 $ CROD 101 101 101 102 GRID 101 0 0.0 0.0 0.0 GRID 102 0 1.0 0.0 0.0 SPC1 1 123456 101 SPC1 1 2356 102 FORCE1 1 102 1.0 101 102 MOMENT1 1 102 1.0 101 102 DAREA 12 102 1 1.0 102 4 1.0 PROD 101 1 1.0 2.0 0.1 0.5 $ $ $+++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++ ++++ $ $ QUAD4 ELEMENT NO. 33 $ CQUAD4 3301 3301 3301 3302 3303 3304 0.

CHAPTER 8 257 Miscellaneous Enhancements

GRID 3301 0 0.0 0.0 0.0 GRID 3302 0 1.0 0.0 0.0 GRID 3303 0 1.0 1.0 0.0 GRID 3304 0 0.0 1.0 0.0 SPC1 1 1256 3302 3303 SPC1 1 123456 3301 3304 FORCE 1 3302 0 1.0 0.0 0.0 1.0 FORCE 1 3303 0 1.0 0.0 0.0 1.0 DAREA 12 3302 3 1.0 3303 3 1.0 PSHELL 3301 1 1.0 1 120.0 1 1.0 0.5 +QUAD41 +QUAD41 0.2 -0.3 $ CQUAD4 3313 3313 3313 3314 3315 3316 382.5 +QUAD42 +QUAD42 .63 .67 .53 GRID 3313 3 3.0 90. 0. 3 123456 GRID 3314 3 3.0 90. 60. 2 123456 GRID 3315 3 3.0 40. 60. 1 4 GRID 3316 3 3.0 30. 0. 0 5 FORCE 1 3315 2 3.14159 0. 2.71828 0. DAREA 12 3315 3 1.73205 PSHELL 3313 22 .618034 2 1 .30103 +QUAD43 +QUAD43 0. $ $ COMPOSITE TESTING , WITH STRAIN THEORY, ADDED 17JUN87, LNA CQUAD4 3321 3321 3321 3322 3323 3324 0. GRID 3321 0 0.0 0.0 0.0 13456 GRID 3322 0 10.0 0.0 6 GRID 3323 0 10.0 10.0 0.0 6 GRID 3324 0 0.0 10.0 0.0 123456 FORCE 1 3322 0 1.+3 1.0 0.0 1.0 FORCE 1 3323 0 1.+3 1.0 0.0 1.0 DAREA 12 3322 3 1.0 3323 3 1.0 PCOMP 3321 1. STRN +QUAD4C +QUAD4C 3 0.5 0. YES 3 0.5 0. YES $ $+++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++ ++++ $ $ HEXA ELEMENT NO.67 $ $ CHEXA 6701 6701 6701 6702 6703 6704 6705 6706 +C6701 +C6701 6707 6708 GRID 6701 0 0.0 0.0 0. 0 456 GRID 6702 0 0.0 .08 0. 0 456 GRID 6703 0 0.0 .08 .1 0 456 GRID 6704 0 0.0 0. .1 0 456 GRID 6705 0 1.0 0. 0. 0 456 GRID 6706 0 1.0 .08 0. 0 456 GRID 6707 0 1.0 .08 .1 0 456 GRID 6708 0 1.0 0. .1 0 456 PSOLID 6701 9 0 2 SPC1 1 123 6701 THRU 6704 FORCE 1 6705 0 .25 0. 0. -1. FORCE 1 6706 0 .25 0. 0. -1. FORCE 1 6707 0 .25 0. 0. -1. FORCE 1 6708 0 .25 0. 0. -1. PLOAD4 1 6701 -125. 6701 6703 $

258 MD Nastran 2006 Release Guide

$+++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++ ++++ $ $ DUM1 ELEMENT NO. 53 $ $ADUM1,6,3,0,3,CTRIAX6 $ CTRIAX6 5301 33 5301 5302 5303 5304 5305 5306 +TRIAX61 +TRIAX6130.0 GRID 5301 0 6.0 0.0 0.0 0 2456 GRID 5302 0 6.0 0.0 2.0 0 2456 GRID 5303 0 6.0 0.0 4.0 0 2456 GRID 5304 0 4.238 0.0 3.0 0 2456 GRID 5305 0 2.536 0.0 2.0 0 2456 GRID 5306 0 4.238 0.0 1.0 0 2456 SPC1 1 3 5302 PLOADX 1 .0222139.03332095301 5302 5303 $ $+++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++ ++++ $ $ CONM2 ELEMENT NO. 30 $ CONM2 3001 3001 0 1.0 1.0 1.0 1.0 +CONM21 +CONM21 1.0 1.0 1.0 1.0 1.0 1.0 GRID 3001 0 0.0 0.0 0.0 SPC 1 3001 123456 0.0 $ $======================================================================== $ $ DMIG ELEMENT NO. 100 $ NOTE:P.S. 3 ADDED 14-JAN-82 GRID 10000 GRID 10001 3 DMIG MATK 0 6 2 0 DMIG MATK 10000 3 10000 3 1.D6 + 10001 3 -1.D6 DMIG MATK 10001 3 10001 3 1.D6 DMIG MATLOAD 0 9 1 0 DMIG* MATLOAD 1 +DMIG *DMIG 10000 3 1. DMIG* MATLOAD 2 +DMIG2 *DMIG2 10000 3 0. $ enddata

Example Output The printed output for the example problem consists of all of the output typically generated by a static analysis for the requests present in the case control section of the input and is not reproduced here. There is a small section of additional printed output generated in the Executive Control Echo region when the MODEL_CHECK material property options are used. The output summarizes the requested material property updates and is shown on the next several lines.

CHAPTER 8 259 Miscellaneous Enhancements

$ MODEL_CHECK MAT_DENSITY=OFF, MAT_TECOEFF=OFF,MAT_TEIJ=OFF ******************************************************************************************************* ******************************************************************************************************* * * * THE PRESENCE OF THE MODEL_CHECK EXECUTIVE STATEMENT CAUSES THE FOLLOWING MATERIAL * * PROPERTY VALUES TO BE MODIFIED FOR EVERY MAT1, MAT2, MAT3, MAT8 AND MAT9 MATERIAL * * PROPERTY ENTRY PRESENT IN THE INPUT BULK DATA SECTION: * * MATERIAL DENSITY REVISED VALUE = 0.00000E+00 * * THERMAL EXP. DIRECT COEFF. REVISED VALUE = 0.00000E+00 * * THERMAL EXP. SHEAR COEFF. REVISED VALUE = 0.00000E+00 * * * ******************************************************************************************************* *******************************************************************************************************

There is no other printed output generated that is peculiar to the material property update feature. All other output is typical printed output that is generated by the case control requests. For this example, the Grid Point Weight Generator output was requested via param,grdpnt,0 in the bulk data so that the mass of the structure could be verified as being produced by only the CONM2 element and the element nonstructural mass.

260 MD Nastran 2006 Release Guide