MSC.Nastran 2005 - MSC Software Corporation

MSC.Nastran 2005 - MSC Software Corporation
MSC.Nastran 2005
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  2004 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.
MSC, MSC., MSC.Dytran, MSC.Marc, MSC.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.
NA*V2005*Z*Z*Z*DC-REL
C O N T E N T S
MSC.Nastran 2005 Release Guide
MSC.Nastran 2005
Release Guide
Table of Contents
Table of Contents
Preface
■
List of MSC.Nastran Books, x
■
Technical Support, xi
■
Internet Resources, xiii
■
Release Guide Introduction, 2
❑ Nonlinear, 2
❑ Numeric Enhancements, 2
❑ Elements, 3
❑ Dynamics, 3
❑ Optimization, 3
❑ Rotor Dynamics, 4
❑ DDAM, 4
❑ Further Enhancements, 4
■
MSC.Nastran Explicit Nonlinear -- SOL 700 - Beta Capability, 6
❑ Introduction, 6
❑ Linear and Nonlinear Analysis, 7
❑ Description of the SOL 700 Executive Control Statement, 8
❑ Executive Control Parameters:, 9
■
MSC.Nastran Implicit Nonlinear - SOL 600, 33
❑ Additions to the SOL 600 Executive Control Statement:, 33
❑ Temperature-Dependent Stress Strain Curves, 37
❑ Improved Parallel Processing for SOL 600, 39
■
Pre-release of the Nonlinear Transient Analysis in SOL 400, 43
❑ Introduction, 43
❑ Benefits, 43
❑ Limitations for the Current Release, 44
❑ Case Control Commands – SUBCASE, STEP and ANALYSIS, 45
❑ Vector Operations and Convergence Criteria, 47
❑ Solution Algorithm and Simulation of SOL 129, 47
1
MSC.Nastran 2005
Release Guide
2
Nonlinear Analysis
❑
❑
❑
❑
❑
❑
Nonlinear Iteration Summary Table for Nonlinear Transient
Analysis in SOL 400, 48
Restart, 50
Temperature Excitation, 51
Outputs, 52
User Interfaces, 53
Examples, 55
■
Correction in the Solution Algorithm for Elasto-Plastic Material, 67
❑ Example, 68
■
Correction for the Nonlinear Element Strain Energy, 70
❑ Example, 70
■
ACMS Now Available in the Matrix (DOF) Domain, 74
■
Improvements for Geometric Domain Based ACMS, 76
■
Improved Matrix Diagonal Diagnostics for 2x2 Pivots
(MAXRATIO), 77
■
Performance Improvement in Modal Frequency Response for Large
Frequency Ranges, 78
■
Temperature-Dependent Composites Support Extended to
Unsymmetric Laminates, 80
■
Global Ply Results Tracking, 83
■
GPFORCE and ESE Output for DMIG and GENEL, 87
■
Bar Element Torsional Mass Moment of Inertia, 88
■
PARAM,COUPMASS Lumped Mass Option, 89
❑ Inputs, 89
❑ Outputs, 89
■
QUADR Convergence Behavior, 92
❑ Introduction, 92
❑ Benefits, 92
❑ Inputs, 92
❑ Example, 92
■
Arbitrary Beam Cross Section (Pre-Release), 96
❑ Introduction, 96
❑ Benefits, 96
3
Numeric
Enhancements
4
Elements
❑
❑
Inputs and Outputs, 96
Guidelines, 97
5
Dynamic Analysis
■
C-Set Improvements, 102
■
Enhancements to the MODESELECT Case Control Command, 103
■
Automatic Q-Set (AUTOQSET), 105
❑ Example, 106
■
Enhancements to Dynamic Excitation Processing in DPD
Module, 109
■
Enhancements to Transient Response Analysis, 110
❑ Increased Accuracy from TRLG Module, 110
❑ Improved Calculations for Enforced Motion in TRLG and TRD1
Modules, 110
❑ Initial Condition Specification for Enforced Motion Usage via
SPC/SPCD, 110
■
Composite Ply Strength Ratio Response Type for the DRESP1
Entry, 114
❑ Introduction, 114
❑ Benefits, 114
❑ Input, 114
❑ Outputs, 114
❑ Guidelines and Limitations, 115
❑ Example (TPL: csrsens.dat), 115
■
New FUNC(tions) for the DRESP2 Entry, 117
❑ Introduction, 117
❑ Benefits, 117
❑ Theory, 117
❑ Input, 119
❑ Outputs, 120
❑ Guidelines and Limitations, 120
■
Transformation of Approximate Optimization Task to a Feasible
Design, 122
❑ Introduction, 122
❑ Benefits, 122
❑ Theory, 122
❑ Input, 123
❑ Outputs, 123
6
Optimization
❑
❑
Guidelines and Limitations, 123
Example (TPL: mmfdpen.dat), 123
■
Residual Vectors Based on Adjoint Loads, 125
❑ Introduction, 125
❑ Benefits, 125
❑ Input, 125
❑ Outputs, 125
❑ Guidelines and Limitations, 125
❑ Example (rvadjsens.dat), 126
■
Multiple Boundary Conditions for DFREQ/MFREQ in SOL 200, 128
❑ Theory, 128
❑ Input/Output, 128
❑ Guidelines and Limitations, 129
■
Benefits of Matrix Domain ACMS in SOL 200, 130
■
ADS Optimizer, 131
❑ Introduction, 131
❑ Benefits, 131
❑ Input, 131
❑ Remarks:, 133
❑ Output, 134
❑ Guidelines and Limitations, 134
■
Topology Optimization - Beta Capability, 135
❑ Introduction, 135
❑ Benefits, 136
❑ Input, 136
❑ TOPVAR – Topological Design Variables, 136
❑ New Responses - Compliance and Fractional Mass, 137
❑ New and Modified Design Optimization Parameters
(DOPTPRM), 138
❑ Outputs, 139
❑ Guidelines and Limitations, 141
❑ Example 1 (topex1.dat), 144
■
BIGDOT Optimizer, 147
❑ Introduction, 147
❑ Benefits, 147
❑ Input, 147
❑ Output, 148
❑ Guidelines and Limitations, 148
❑ Example, 148
7
Rotor Dynamics
■
Squeeze Film Damper Nonlinear Force, 150
❑ Introduction, 150
❑ Squeeze Film Damper Model Imbedded in MSC.Nastran
Transient Solution, 150
❑ Theory for General Squeeze Film Damper Model, 151
❑ Squeeze Film Damper Input Data Format, 152
❑ Squeeze-Film Damper Example, 154
❑ References, 156
■
A DDAM Processor for MSC.Nastran Including an MSC.Patran
Interface, 158
❑ Introduction, 158
❑ DDAM with SOL 187, 158
■
Guidelines for Effective DDAM Analysis, 169
❑ A Note on Symmetry, 170
■
Theoretical Background, 172
■
Worked Two Mass Problem, 178
■
Format of Coefficient File, 185
■
Control File Format, 187
■
User defined Shock Spectra, 190
■
MSC.Patran Interface, 192
❑ Program Operation:, 192
■
MSC.Nastran ADAMS Integration, 198
❑ Overview, 198
❑ Limitations, 198
■
Alternative Solution Algorithms for Flutter Analysis, 199
❑ Introduction, 199
❑ Benefits, 200
❑ Input, 200
❑ Guidelines and Limitations, 201
❑ Example (pkswep.dat), 202
■
Little - Big Endian, 203
❑ Variable Endian OUTPUT2 and OUTPUT4 Files, 203
8
DDAM Processor
9
Miscellaneous
❑
❑
❑
❑
❑
Introduction, 203
Benefits, 203
Theory, 204
Inputs and Outputs, 204
Examples, 204
■
Reduced OP2 File SET Consistency Check, 206
❑ Introduction, 206
❑ Benefits, 206
❑ Method and Theory, 207
❑ Inputs, 207
❑ Outputs, 208
❑ Guidelines and Limitations, 208
❑ Demonstration Example, 209
❑ Example Input Data (TPL: rop2s*.dat), 209
❑ Example Output, 211
■
SPC and SPCD Entries in Machine Precision, 213
❑ Limitation, 213
■
Reading of PUNCHed Long Field Format Bulk Data, 214
■
New Complex Conjugate Option for Matrix Multiplication, 215
❑ Examples:, 215
■
Acceleration Loads (ACCEL and ACCEL1 Bulk Data Entries), 216
■
A Caution Concerning MSC.Access Application Development, 218
■
Divergent Thermal Results Error Correction (Q1-0768221), 223
■
Displacement Output Filters, 224
■
Write Results Recovery for Subcases into Separate F06 Files, 226
❑ Example, 239
■
DMAP Modules in MSC.Nastran 2005, 242
❑ DMAP Module Changes, 242
■
Summary of Data Block Changes from MSC.Nastran 2004 to
MSC.Nastran 2005, 251
■
More Stringent Case Control Check, 253
10
Upward
Compatibility
INDEX
MSC.Nastran Release Guide , 255
MSC.Nastran 2005 Release Guide
Preface
■ List of MSC.Nastran Books
■ Technical Support
■ Internet Resources
x
List of MSC.Nastran Books
Below is a list of some of the MSC.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
Preface
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.
Phone
and
Fax
United States
Telephone: (800) 732-7284
Fax:
(714) 784-4343
Frimley, Camberley
Surrey, United Kingdom
Telephone: (44) (1276) 67 10 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
xi
xii
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]
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.
Preface
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.
xiii
xiv
MSC.Nastran 2004 r3 Release Guidex
CHAPTER
1
MSC.Nastran 2005 Release Guide
■ Release Guide Introduction
2
1.1
Release Guide Introduction
MSC.Nastran 2005 introduces new capabilities and enhancements to existing
capabilities while improving solution accuracy and performance. This guide covers
all new functionality that has been added to the MSC.Nastran program since the
MSC.Nastran 2004 r1 release in September 2003, and includes 2004 r2, 2004 r3, and
2005 r1. In addition, some of the new capabilities discussed in this guide are initial
implementations, considered to be in beta form and offered for trial purposes.
Nonlinear
The horizons of MSC.Nastran continue to broaden as development pushes the
program forward to take on more advanced and complex types of analysis. The
release of MSC.Nastran 2004 brought a new dimension to the analysis capabilities of
MSC.Nastran, with a new implicit nonlinear solution sequence (SOL 600) that
embodies MSC.Marc, taking the product into the realm of complex highly nonlinear
calculations, with contact and advanced materials. The trend continues this year with
the preliminary release of the explicit nonlinear solution sequence (SOL 700),
comprising MSC.Dytran and LS-Dyna, to the MSC.Nastran family of solvers.
This new capability, offered in beta form with MSC.Nastran 2005, allows complex
explicit nonlinear calculations, including crash and impact analysis in this initial
phase of implementation. Also, many known issues have been addressed concerning
implicit nonlinear SOL 600, increasing overall robustness of the solution sequence.
Also available in MSC.Nastran 2005 is another new nonlinear solution sequence,
SOL 400. Offered initially as a beta release, SOL 400 will embody the current
MSC.Nastran nonlinear capabilities of solution sequences 106 and 129 into a single
solution sequence.
Numeric Enhancements
A new domain decomposition method is now available in beta form for the
Automated Component Mode Synthesis capability, which improves performance of
NVH types of analysis, particularly for models with complex geometry. You can
experience further performance improvements with a new technique used in the
calculation of frequency response quantities for large problems solved across a wide
frequency range.
Matrix to factor diagonal reporting has also been improved for analyses that use the
Lagrange Multiplier Technique.
CHAPTER 1
MSC.Nastran 2005 Release Guide
Elements
Analysis of composite structures now extend to include temperature dependency for
unsymmetric laminates. Also, post processing composite structures is now much
easier with global ply results tracking, particularly for areas where ply drop off is
apparent.
For bar elements, it is now possible to specify a torsional mass moment of inertia
value, and for both bar and beam elements a new option to specify lumped mass with
no off diagonal terms has been added. This version of MSC.Nastran also introduces
an arbitrary beam cross section beta capability, allowing the specification of cross
section shapes using points, and further allowing these profiles to be optimized in
SOL 200.
Improvements to the QUADR element are evident with improved convergence
behavior, particularly for coarsely meshed models. You can now obtain grid point
force output for DMIG and GENEL type definitions.
Dynamics
Improvements to the dynamic analysis capabilities of MSC.Nastran include:
• The support of multiple boundary conditions for frequency response
analysis in SOL 200
• Better handling of c-set masses during the calculation of component modes
• Enhancements to dynamic excitation processing
• Enforced motion calculations
In addition, the MODESELECT Case Control command has been extended to include
easier mode selection for all selection criteria, essentially replacing many of the
existing mode selection bulk data parameters, as well as adding a new criteria based
on modal effective mass.
Optimization
As well as the new nonlinear solution sequences, MSC.Nastran 2005 offers a beta
topology optimization capability. This addition to the existing SOL 200 optimization
solution sequence allows optimization analyses to be performed that require many
design variables, a typical requirement of topology optimization.
Other optimization enhancements include:
• New functions for DRESP2
3
4
• A new response type for DRESP1
• The ability to transform an approximate optimization task to a feasible
design
• Increased accuracy with dynamic response optimization analyses through
the use of residual vectors
Rotor Dynamics
The rotor dynamics capability introduced in MSC.Nastran 2004 has been further
enhanced to include the modeling of squeeze film dampers.
DDAM
We have introduced a new dynamic design analysis method (DDAM) solution
sequence (SOL 187). Widely used in the ship building industry, DDAM is a form of
shock spectrum analysis used to determine the dynamic response of a component to
shock loading.
Further Enhancements
We have added many other enhancements to MSC.Nastran 2005. Some are
mentioned in the following list.
• Furthering the integration of MSC.Nastran with MSC.ADAMS are new
capabilities that aid model checkout and the determination of component
attachment points
• The new variable endian capability allows easier transfer of OP2 results data
between machines with differing binary file formats
• New ACCEL Bulk Data entries allow easier specification of acceleration
loads across the model
• A new complex conjugate option for matrix multiplication (MPYAD) has
been added, facilitating matrix manipulation
• SPC and SPCD entries are now stored in machine precision
• New PKS and PKNLS flutter options in aeroelastic analysis
MSC.Nastran 2005 Release Guide+
CHAPTER
2
Nonlinear Analysis
■ MSC.Nastran Explicit Nonlinear -- SOL 700 - Beta Capability
■ MSC.Nastran Implicit Nonlinear - SOL 600
■ Pre-release of the Nonlinear Transient Analysis in SOL 400
■ Correction in the Solution Algorithm for Elasto-Plastic Material
■ Correction for the Nonlinear Element Strain Energy
6
2.1
MSC.Nastran Explicit Nonlinear -- SOL 700 - Beta
Capability
Introduction
MSC.Nastran Explicit Nonlinear, also known as SOL 700, is a new capability
introduced as a preliminary capability in MSC.Nastran 2005. This is the first phase of
adding explicit nonlinear dynamics to MSC.Nastran.
The Phase 1 effort primarily is intended to solve highly nonlinear structural crash and
impact problems. Fluids, air bags, seat belts, and passengers are not a part of Phase 1
and will be added in subsequent phases. Although Phase 1 primarily addresses crash
and impact loading, usually described by initial velocity input, other types of dynamic
loading are also supported.
SOL 700 works in a manner similar to SOL 600, but instead of spawning MSC.Marc, a
special version of the well-known LS-Dyna program is spawned. Like SOL 600,
SOL 700 contains an internal translator. MSC.Nastran input data is translated to
MSC.Dytran input data during the IFP portion of MSC.Nastran. Later in IFP, LS-Dyna
is spawned. Special subroutines have been added to LS-Dyna to accept MSC.Dytran
format input data similar to LSTC’s keyword input data in the standard version of LSDyna. Inside LS-Dyna, the MSC.Dytran input data is stored directly in memory and
converted to a structured LS-Dyna style input file (which is the old style type of input
without headers). LS-Dyna then continues with computations to produce output
results for highly nonlinear problems.
SOL 700 is primarily intended for engineers and analysts who have constructed an
MSC.Nastran finite element model for a purpose other than crash, but who wish to
use the model for crash. This avoids having to read the MSC.Nastran model into a
GUI, translate it to LS-Dyna or MSC.Dytran, and thus risk losing or not properly
translating some MSC.Nastran input data.
Once you have completed the LS-Dyna portion of the execution, standard LS-Dyna
results files such as d3plot, as well as standard MSC.Nastran files such as op2, xdb,
punch and f06, are available for postprocessing. The capability will be delivered with
the MSC.Nastran 2005 r2 release.
SOL 700 contains an internal translator that creates an MSC.Dytran file. If the original
MSC.Nastran input file is named jid.dat (or jid.bdf), the MSC.Dytran file that is
created is named jid.dytr.dat. The translator examines and converts Executive
Control statements, Case Control commands and Bulk Data entries to MSC.Dytran.
CHAPTER 2
Nonlinear Analysis
The MSC.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 a 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 upcoming MSC.Nastran Explicit Nonlinear User’s Guide for further theoretical
details. The small time step requirements are not a great problem when simulating
events that occur quickly, such as impact or crash. However, for longer events such
as low frequency dynamics or static analysis, the run time sometimes is too great for
explicit methods and implicit analyses need to be employed.
SOL 700 has three ways of solving static problems:
• Dynamic relaxation -- The input is applied as a step function and large
damping is added. The solution is run until approximate steady-state values
are obtained.
• Slow buildup -- The static load is ramped slowly from zero to full value over
a period of time long enough that no important natural frequencies are
excited. No extra damping is added.
• Slow buildup with extra damping -- This method is like the previous method
except that some extra damping is added; thus, the final run time can often
be reduced.
Which method to use depends on the problem being solved and whether extra
damping affects the solution or not. The second method produces the “exact” results
but may take excessive computer time in some cases. The first method is the “classic”
method of solving static problems using explicit analysis techniques.
New entries have been added to MSC.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
numerous Grid point lines. This allows an input file setup for something else to be
edited and quickly changed to a crash analysis.
For those familiar with the LS-Dyna material descriptions, about 25 of the most
important and commonly used LS-Dyna materials may be input to SOL 700 directly.
7
8
Contact is described using the same entries as SOL 600; however there is a new entry
to easily describe a rigid wall used for car crash simulation. That entry is the
MSC.Dytran WALL entry (see new entry section below).
In addition, for those familiar with MSC.Dytran, several important MSC.Dytran
Parameters have been added.
Description of the SOL 700 Executive Control Statement
Format:
SOL 700,ID PATH= COPYR= OUTR= STOP= NP= NOERROR
Example:
SOL 700,129 PATH=3 OUTR=OP2 NP=4
(700,129 request nonlinear transient dynamics, path=3 requests use of the dytranlsdyna script, outr=op2 requests that an op2 file, np=4 requests that 4 processors be
used)
Summary:
SOL 700 is a new Executive Control statement like SOL. It normally activates an
explicit nonlinear transient analysis integration scheme using dytran-lsdyna. It may
also be used for implicit static analyses using LS-Dyna’s Dynamic Relaxation or slow
buildup options. The calculations will not be performed directly within MSC.Nastran.
Instead, SOL 700 will use a separate solver based on LS-Dyna, which is spawned from
MSC.Nastran. This client-server approach is similar to SOL 600, using MSC.Marc. For
linear analyses such as normal modes, frequency response, or linear direct transient
response, MSC.Nastran should be used.
For the first phase of this project, the SOL 700 statement will spawn dytran-lsdyna,
which uses an MSC.Dytran text input interface to LS-Dyna. dytran-lsdyna is a 3D,
explicit nonlinear analyses code with DMP (parallel processing domain
decomposition) capabilities.
For Phase 2 of the project and beyond, fluid coupling, airbags, seat belts, and dummy
passengers will be added. Then the user will be able to select the standard
MSC.Dytran program or an enhanced dytran-lsdyna program.
Inputs and outputs will be the same as, or similar to, the familiar MSC.Nastran inputs
and outputs or, at the user’s request, LS-Dyna type outputs will be available. The LSDyna style outputs are the default for SOL 700.
CHAPTER 2
Nonlinear Analysis
For ID=129 or NLTRAN, SOL 700 will generate a dytran-lsdyna input data file
“jid.dytran.dat”, where “jid” is the name of the MSC.Nastran input file without the
extension). For example, if the MSC.Nastran input file is named abcd.dat, (or
abcd.bdf) then “jid”=abcd).
Unless explicitly specified using the STOP= option, dytran-lsdyna will be executed
from MSC.Nastran on any computer system capable of doing so (which includes most
UNIX systems and Windows systems). For dytran-lsdyna to run, it must be installed,
properly licensed, and accessible from the directory where the MSC.Nastran input
data resides, MSC_BASE must be provided in the environment.
Executive Control Parameters:
The required ID may be one of several valid solution sequence integers or names
shown in “Solution Sequences” on page 144 of the MSC.Nastran Quick Reference Guide
for the SOL statement. Examples are 129 and NLTRAN.
The following solutions are available for Phase I of this project: 101, 106, 109, 129 (and
their equivalent names).
All items on the SOL 700,ID after ID itself, may be specified in environmental
variables. This may be done in any manner environmental variables can be set. They
may be set by the MSC.Nastran user at run time or by the system administrator when
MSC.Nastran is installed. Any values specified on the SOL statement override those
in the environment. Environmental variables are fully described in the MSC.Nastran
2005 Installation and Operations Guide. A keyword file is available to describe the
format of each variable. The variable is normally set in the system-wide rc file, a user’s
rc file, a local rc file or in a script used to submit MSC.Nastran. Any string or value
listed on the SOL 700,ID statement is also valid as an environmental variable. If the
environmental variables are placed in the system-wide rc file, they may be used by a
company for all MSC.Nastran users and even hide the fact that dytran-lsdyna is being
spawned if so desired.
The following describes the various options for PATH. We suggest the use of
PATH=3 for Linux and UNIX and path=1 for Windows.
PATH=1 (May be used with Windows and Linux only)
If PATH=1 is specified, MSC.Nastran will determine the proper command to execute
a serial dytran-lsdyna run. To aid MSC.Nastran in determining where dytran-lsdyna
is located, the dynrun.pth file must be located in the same directory where the
9
10
MSC.Nastran input file resides. The dynrun.pth file must contain one line providing
the location (complete path) of the dytran-ls-dyna run script. A typical example of the
line in the file dynrun.pth follows.
Windows
c:\sol700\
Linux:
/msc/users/sol700
A string is appended to this path to form the complete command used to execute
dytran-lsdyna:
“dytran-lsdyna jid=name.dytr.dat
O=name.dytr,d3hsp G=name.dytr.d3plot D=name.dytr.d3dump
F=name.dytr.d3thdt
A=name.dytr.runrsf B=name.dytr.d3drfl
For Windows, MSC.Nastran will spawn dytrna-lsdyna using the following command
assuming the MSC.Nastran input data is named enf2e.dat. (Although the example
appears as if it is on multiple lines, it is actually on a single line.)
c:\sol700/dytran-lsdyna i=enf2e.dytr.dat O=enf2e.dytr.d3hsp G=enf2e.dytr.d3plot
D=enf2e.dytr.d3dump F=enf2e.dytr.d3thdt A=enf2e.dytr.runrsf B=enf2e.dytr.d3drfl
PATH=2 (May be used with Windows and Linux only)
If PATH=2 is specified, it is expected that the directory with the dytran-lsdyna run
script is on the PATH. If PATH=2 is specified, dytran-lsdyna will be executed from
inside MSCNastran using the commands for the PATH=1 option except that
dynrun.pth is not required.
PATH=3 (Applicable to all computer systems)
If PATH=3 is specified, a script or batch file to execute dytran-lsdyna, located in the
same directory as the dytran-lsdyna executable, will be executed. The name of the
script or batch files is run_dytran (or run_dytran.bat). This directory and name of the
script is determined by the first line in a file named sol700.pth. Options are specified
on subsequent lines of the sol700.pth file.
CHAPTER 2
Nonlinear Analysis
Available PATH=3 options for Windows PC systems are as follows:
exe
The full path to the executable for dytran-lsdyna that is to be used.
Optional -- If exe= is omitted, the directory where the script or batch
file resides (first line of sol700.pth) will be used and dytran-lsdyna for
UNIX/Linux and dytran-lsdyna.exe for windows will be appended.
If exe= is used, it must be the second line in the sol700.pth file.
nproc
Number of processors.
(Default is to used NP on the SOL 700 line. If NP and nproc are
omitted, the default is 1). For parallel execution, the directory where
the MSC.Nastran input file exists must be shared with read/write
privileges. If wdir is used, it must also be shared (see below). The
directory where the dytran-lsdyna executable resides must also be
shared for parallel execution. In addition, all rules for MPICH must be
followed properly, (see your system administrator to be sure all
computers are properly configured for parallel execution using
MPICH). The version of MPICH to use is 1.2.5 as of the initial SOL 700
release. It can be obtained from ftp.mcs.anl.gov if necessary.
bat
Run in background or forground (default).
debug
Output many messages from the script or batch file.
memory
Amount of memory. Example: memory=20m.
steps
Number of steps (1 or 2; default is 2).
Two steps means that lsdyna is executed twice: once to form the
“structured input file” and again to analyze it. Although steps=1 is
faster, there are some models that fail using the steps=2 option.
wdir
Working directory. For parallel execution, this directory must be
shared with read/write privileges. Default is directory where
MSC.Nastran input resides.
copy
Yes or no. Input and output files are copied from wdir to the input
directory. Default is yes.
delete
Yes or no. LS-Dyna scratch files are deleted or not. Default is yes.
11
12
machine
Machines and number of processors to use in the form:
machine1#2+machine2#4 (use 2 processors on machine 1 and
4 processors on machine 2)
host
file name. Name of a hostfile containing the same information as
“machine”
The format of hostfile is as follows for the example for machine:
machine1 2
machine2 4
A Windows example of the file sol700.pth for the PATH=3 case follows.
e:\sol700\dytran-lsdyna\run_dytran
exe=f:\latest_dytran-lsdyna\dytran-lsdyna.exe
nproc=4
memory=20m
steps=2
wdir=f:\temp
delete=yes
machine=pc01#2+pc02#2
For the above example, MSC.Nastran will create the following command to spawn
dytran-lsdyna assuming your input file is named abcd.dat. (Although the example
appears like it is on multiple lines, it is actually on a single line.)
e:\sol700\dytran-lsdyna\run_dytran exe=f: \latest_dytran-lsdyna\dytranlsdyna.exe jid=abcd.dytr nproc=4 memory=20m wdir=f:\temp delete=yes
machine=pc01#2+pc02#2
Available PATH=3 options for UNIX/Linux systems follows.
exe
The full path to the executable for dytran-lsdyna that is to be used.
(Optional -- If exe= is omitted, the directory where the script or batch
file resides (first line of sol700.pth) will be used and dytran-lsdyna for
UNIX/Linux and dytran-lsdyna.exe for windows will be appended.)
If exe= is used, it must be the second line in the sol700.pth file.
nproc
Number of processors. (Default is to use NP on the SOL 700 line. If
NP and nproc are omitted, the default is 1.)
bat
Yes or no. Run in background or forground (default). Leave out for
steps=2
debug
Yes or no. Outputs many messages from the script or batch file.
CHAPTER 2
Nonlinear Analysis
memory
Amount of memory; example: memory=20m (20 MB).
steps
Number of steps (1 or 2; default is 2). Two steps means that lsdyna is
executed twice: once to form the “structured input file” and again to
analyze it.
Although steps=1 is faster, there are some models that fail using the
steps=2 option.
wdir
Working directory. Default is directory where MSC.Nastran input
resides.
copy
Yes or no. Input and output files are copied from wdir to the input
directory. Default is yes.
delete
Yes or no. LS-Dyna scratch files are deleted or not. Default is yes.
cluster
Yes or no. If yes is specified, the job will be initiated on the machine
that the user is logged on to, but the analysis is performed on the
cluster nodes that are specified in machinefile. If the default of off is
used, the job will run on the local machine and the machines listed in
the machine file depending on the number of processors specified.
This option is not available for early SOL 700 releases. Default is no.
mpipath
The MPI install directory if you wish to used a non-default MPI
directory.
mpirun
The MPI run command you want to use. If entered, it overrides the
default MPI run command on your machine as well as the command
in mpipath.
A UNIX/Linux example of the file sol700.pth for the PATH=3 case follows.
/users/joe/sol700/run_dytran
nproc=4
memory=20m
steps=2
wdir=/tmp/dyna
For the above example, MSC.Nastran will create the a command similar to the
following to spawn dytran-lsdyna assuming your input file is named abcd.dat
/users/joe/sol700/run_dytran \
exe=/users/joe/sol700/dytran-lsdyna \
jid=abcd.dytr nproc=4 memory=20m steps=2 wdir=/tmp/dyna
13
14
If PATH is not specified, a special version of dytran-lsdyna will normally be used.
This version will be located in a subdirectory named dyna/machine below the
MSC.Nastran base directory (MSC_BASE). The machine directory will be aix, alpha,
hpux, etc. If MSC_BASE is not available for a particular computer system, PATH=1,
2 or 3 must be specified.
STOP
STOP is an optional item. STOP is used to prevent execution of dytran-lsdyna or
prevent execution of MSC.Nastran after IFP if so desired. DO NOT ENTER any of the
STOP options if any of the OUTR options are entered as the DMAP generated
automatically by MSC.Nastran will put an EXIT in the proper place. The various
options are as follows.
STOP=1
If STOP=1, MSC.Nastran will be gracefully stopped after IFP. This option is used to
prevent MSC.Nastran from performing its own solution (normally used when the
solution is performed by dytran-lsdyna with ID=129).
STOP=3
If STOP=3, MSC.Nastran is stopped after IFP and dytran-lsdyna is not executed. This
would be the normal STOP option if the user wants to examine a dytran-lsdyna input
file, make some changes and then execute dytran-lsdyna manually.
The following dytran-lsdyna files are potentially affected by the OUTR option.
OUTR=OP2,XDB,F06,PCH (Not available in Version 2005 r1)
Choose one or more or omit -- translate dytran-lsdyna jid.dytr.d3plot output to
MSC.Nastran. This option requires the use of the MSC.Nastran Toolkit. A license is
not needed for the Toolkit as it is imbedded in standard SOL 700 licensing. The
conversion between LS-Dyna’s d3plot and op2.xdb.f06,punch is made using
MSC.Patran’s DRA/DAC together with a special version of the toolkit. The special
toolkit executable is spawned from the original MSC.Nastran job after dytran-lsdyna
completes and if any of the OUTR options are specified.
NP
NP=the number of processors (domains) for parallel processing. The default is one.
In order to use more than one domain, MPI, Lam, POE, or whatever parallel program
is needed must be properly installed on all computers involved and a hostfile
CHAPTER 2
Nonlinear Analysis
designating which computers are to be used for each domain must have been setup
prior to running the job. It is required that if NP>1, PATH=3 be used and a file named
sol700.pth be located in the same directory as the MSC.Nastran input data. The
sol700.pth file should contain all commands necessary to run dytran-lsdyna in
parallel. This file must have execute permissions.
NOERROR
NOERROR is an optional item. If NOERROR is specified, errors due to features that
are available in MSC.Nastran but not available in dytran-lsdyna, and/or features not
yet supported by the translator will be ignored. If NOERROR is entered and STOP=2
(or 3) is not specified, dytran-lsdyna will be executed even though the complete
MSC.Nastran model may not have been completely translated.
NOERROR only be used by experienced analysts and then only with extreme caution.
Table 2-1 Case Control Commands Available in SOL 700
Item
Case Contol Commands Available in SOL 700
$
Y
ACCELERATION
Y
BCONTACT
Y
BEGIN BULK
Y (Other BEGIN forms are not allowed)
DISPLACEMENT
Y
DLOAD
Y
ECHO
Y
ELFORCE see FORCE
Y
ENDTIME
Y (new)
FORCE & ELFORCE
Y (automatically produced in d3plot files no user control)
GROUNDCHECK
Y (MSC.Nastran f06 only)
IC
Y
INCLUDE
Y
LABEL
Y (MSC.Nastran f06 only)
LINE
Y (MSC.Nastran f06 only)
LOAD
Y (for dynamic pseudo-statics only)
15
16
Table 2-1 Case Control Commands Available in SOL 700
Item
Case Contol Commands Available in SOL 700
LOADSET
Y
MAXLINES
Y (MSC.Nastran f06 only)
MPC
Y
NLPARM
Y (Psuedo static analysis only)
NLSTRESS
Y (Changed to STRESS)
PAGE
Y (In MSC.Nastran only)
PARAM
Y (Only applicable parms are used)
PRESSURE
Y
SET
Y
SET –
OUTPUT(PLOT)
N
SKIP
Y (Required if multiple subcases are present)
SPC
Y
STRAIN
Y
STRESS
Y
SUBCASE
Y (See note)
Note: Only one subcase can be selected for a particular SOL 700 analysis. Many
subcases may be entered in the input file, but the one to be used must be
selected using the SKIP ON and SKIP OFF Case Control commands. If the
SKIP ON/OFF commands are not found or are in the wrong place, the first
subcase encountered will be used and the others ignored.
SUBTITLE
Y
TITLE
Y
TSTEP
Y (Same as TSTEPNL)
TSTEPNL
Y
VELOCITY
Y
WEIGHTCHECK
Y (In MSC.Nastran only)
CHAPTER 2
Nonlinear Analysis
Table 2-2 Bulk Data Entries Available in SOL 700
Item
Bulk Data Entries Available in SOL 700
Fatal Error
AXIC
N
Y
AXIF
N
Y
AXSLOT
N
Y
BAROR
Y
BCBPDY
Y
BCHANGE
N
BSURF
Y
BCBOX
Y
BCPROP
Y
BCMATL
Y
BCONP
N
BCTABLE
Y
Y (Revised)
BLSEG
N
Y
CBAR
Y
CBEAM
Y
CBEND
N
Y
CBUSH
N
Y
CCONEAX
N
Y
CDAMP1D
Y (New)
CDAMP2D
Y (New)
CELAS1D
Y (New)
CELAS2D
Y (New)
CFLUID
N
Y
CGAP
N
Y
CHACAB
N
Y
CHEXA
Y (8 Nodes only)
CONM2
Y
17
18
Table 2-2 Bulk Data Entries Available in SOL 700
Item
Bulk Data Entries Available in SOL 700
Fatal Error
CONROD
Y
CORD1C
Y
CORD1R
Y
CORD1S
Y
CORD2C
Y
CORD2R
Y
CORD2S
Y
CORD3G
N
CPENTA
Y (5 Nodes only)
CQUAD4
Y
CQUAD8
Y (4 Nodes only)
CQUADR
Y
CQUADX
N
Y
CREEP
N
Y
CROD
Y
CSHEAR
N
CTETRA
Y (4 Nodes only)
CTRIA3
Y
CTRIA6
Y (3 Nodes only)
Y
Y
CTRIA3R
Y
CTRIAX
N
Y
CTRIAX6
N
Y
CTUBE
Y
CVISC
Y
CWELD
N
CSPOT
Y (New – LS-Dyna Weld)
CFILLET
Y (New – LS-Dyna Weld)
Y
CHAPTER 2
Nonlinear Analysis
Table 2-2 Bulk Data Entries Available in SOL 700
Item
Bulk Data Entries Available in SOL 700
CBUTT
Y (New – LS-Dyna Weld)
CCRSFIL
Y (New – LS-Dyna Weld)
COMBWLD
Y (New – LS-Dyna Weld)
DAMPGBL
Y (New for Dynamic Relaxiation)
Fatal Error
DAREA
Y
DEFORM
N
Y
DELAY
N
Y
DMI
N
Y
DMIAX
N
Y
DMIG
N
Y
DPHASE
N
Y
DTI
N
Y
ECHOOFF
Y
ECHOON
Y
ENDDATA
Y
EOSPOL
Y (New – Equation of state)
FORCE
Y
FORCE1
N
FORCE2
Y
FORCEAX
N
Y
GENEL
N
Y
GRAV
Y
GRDSET
Y
GRID
Y
INCLUDE
Y
IPSTRAIN
N
Y
ISTRESS
N
Y
Y
19
20
Table 2-2 Bulk Data Entries Available in SOL 700
Item
Bulk Data Entries Available in SOL 700
LOAD
Y
LSEQ
Y
MAT1
Y
MAT2
Y
MAT3
Y
MAT8
Y
MATDxxx
Y (New LS-Dyna materials)
MATD20M
Y (New Rigid Material Merge)
Fatal Error
MATEP
N
Y
MATHE
N
Y
MATHED
N
Y
MATF
N
Y
MATHP
Y
MATS1
Y
MATVE
N
Y
MATORT
N
Y
MATVORT
N
Y
MATVP
N
Y
MATG
N
Y
MFLUID
N
Y
MOMAX
N
Y
MPC
Y
MPCAX
N
Y
NLPARM
Y (For pseudo statics)
NLRGAP
N
Y
NOLINi
N
Y
NTHICK
N
Y
CHAPTER 2
Nonlinear Analysis
Table 2-2 Bulk Data Entries Available in SOL 700
Item
Bulk Data Entries Available in SOL 700
Fatal Error
PANEL
N
Y
PBAR
Y
PBARL
N
Y
PBCOMP
N
Y
PBEAM
Y
PBEAML
N
Y
PBEND
N
Y
PBUSH
N
Y
PCOMP
Y
PDAMP
Y
PDAMP5
N
PELAS
Y
PELAST
N
Y
PGAP
N
Y
PHBDY
N
Y
PINTC
N
Y
PINTS
N
Y
PLOAD
Y
PLOAD1
N
PLOAD2
Y
PLOAD4
Y (Continuation supported)
Y
Y
PLOADX1
N
Y
PLPLANE
N
Y
PLSOLID
N
Y
PMASS
N
Y
PRESPT
N
Y
PROD
Y
21
22
Table 2-2 Bulk Data Entries Available in SOL 700
Item
Bulk Data Entries Available in SOL 700
PSHEAR
N
PSHELL
Y
PSOLID
Y
PTUBE
Y
PVISC
Y
RBAR
Y
RBE1
N
RBE2
Y
RBE3
Y (Changed to RBE3D)
Fatal Error
Y
RESTART
Y
Y
RFORCE
Y (CID, METHOD, continuation line not
supported)
RLOADi
N
Y
RROD
N
Y
RSPLINE
N
Y
RTRPLT
N
Y
SLOAD
N
Y
SPC
Y
SPC1
Y
SPCADD
Y
SPCAX
N
SPCD
Y
SUPAX
N
TABLED1
Y
TABLED2
Y
TABLED3
Y
TABLES1
Y
Y
Y
CHAPTER 2
Nonlinear Analysis
Table 2-2 Bulk Data Entries Available in SOL 700
Item
Bulk Data Entries Available in SOL 700
Fatal Error
TEMP
N
Y
TEMPD
N
Y
TIC
Y
TICD
Y (New with increment options)
TIC3
Y (New MSC.Dytran type entry)
TLOAD1
Y
TLOAD2
Y
TSTEP
Y (Changed to TSTEPNL)
TSTEPNL
WALL
Y
Y (New rigid wall entry)
Summary of New or Changed Bulk Data Entries for SOL 700
BCTABLE
Contact table – many new fields have been added for “slaves”
CDAMP1D Scalar damper connection
CDAMP2D Scalar damper connection
CELAS1D
Scalar spring connection
CELAS2D
Scalar spring connection
CSPOT
Spot weld in the LS-Dyna style (replaces CWELD for SOL 700)
CFILLET
Fillet weld in the LS-Dyna style (replaces CWELD for SOL 700)
CBUTT
Butt weld in the LS-Dyna style (replaces CWELD for SOL 700)
CCRSFIL
Cross-fillet weld in the LS-Dyna style (replaces CWELD for SOL 700)
COMBWLD Complex combined weld in the LS-Dyna style (replaces CWELD for
SOL 700)
DAMPGBL Defines values to use for dynamic relaxation
EOSPOL
Defines equation of state to use for solids in combination with certain
materials.
MATD001
LS-Dyna material 1 – isotropic elastic
MATD2OR
LS-Dyna material 2 – orthotropic
23
24
MATD2AN LS-Dyna material 2 – Anisotropic
MATD003
LS-Dyna material 3 – isotropic with kinematic hardening
MATD005
LS-Dyna material 5 – soil and foam
MATD006
LS-Dyna material 6 – viscoelastic
MATD007
LS-Dyna material 7 – nearly incompressible rubber
MATD012
LS-Dyna material 12 – low cost isotropic plasticity model for solids
MATD013
LS-Dyna material 13 – non-iterative plasticity model with failure
MATD014
LS-Dyna material 14 – soil and foam with failure
MATD015
LS-Dyna material 15 – Johnson-Cook strain and temperature sensitive
plasticity
MATD018
LS-Dyna material 18 – isotropic plasticity with rate effects
MATD019
LS-Dyna material 19 – strain-rate dependent material model
MATD020
LS-Dyna material 20 – rigid material
MATD20M
merges several rigid materials defined using MATD020
MATD022
LS-Dyna material 22 – orthetropic material with brittle failure
(composites)
MATD024
LS-Dyna material 24 – elasto-plastic material with arbitrary stress-strain
curves and strain-rate dependency
MATD026
LS-Dyna material 26 – Anisotropic honeycomb and foam
MATD027
LS-Dyna material 27 – Two-variable rubber model
MATD028
LS-Dyna material 28 – Elasto-plastic resultant formulation
MATD030
LS-Dyna material 30 – Shape-memory superelastic material
MATD031
LS-Dyna material 31 – Frazer-Nash rubber
MATD054
LS-Dyna material 54 – Enhanced composite material model
MATD057
LS-Dyna material 57 – Highly compressible low density foams
MATD059
LS-Dyna material 59 – Shell or solid composite models
MATD062
LS-Dyna material 62 – Confor viscous foam model
MATD063
LS-Dyna material 63 – Crushable foam with damping
MATD064
LS-Dyna material 64 – Strain-rate dependent plasticity with power law
hardening
CHAPTER 2
Nonlinear Analysis
MATD077
LS-Dyna material 77 – General Christensen rubber model
MATD080
LS-Dyna material 80 – Ramberg-Osgood plasticity
MATD081
LS-Dyna material 81 – Elasto-visco-plastic with arbitrary stress-strain
curve
MATD100
LS-Dyna material 100 – Material for spot welds
MATD127
LS-Dyna material 127 – Arruda-Boyce rubber
MATD181
LS-Dyna material 181 – Simplified rubber and foam model
RBE3D
MSC.Dytran-style RBE3
TICD
Initial conditions like TIC with from-thru-by incrementing
WALL
Rigid wall
Summary of New Bulk Data Parameters for SOL 700
DYENDTIM
Determines how to translate TSTEPNL to MSC.Dytran
DYMATS1
Determines how to translate MATS1 to MSC.Dytran
DYLDKND
Designates type of stress-strain curve
DYCOWPRD
ID of Cowper Symonds strain rate equation
DYCOWPRP
P in Cowper Symonds strain rate equation
DYNAMES
Control of output file names - d3plot or jid.dytr.d3plot
DYSTATIC
Method to simulate static analysis (see above three methods)
DYBLDTIM
Number of seconds a static load is built up
DYBULKL
Value of the linear coefficient in the bulk viscosity equation
DYINISTEP
Initial time step
DYCONSLSFAC
Default scale factor for contact forces
DYCONRWPNAL
Scale Factor for rigid wall penalty value
DYCONPENOPT
Penalty stiffens option
DYCONTHKCHG
Whether or not shell thickness change is considered in contact
DYCONENMASS
Treatment of mass of eroded grids
DYCONECDT
Time step size for eroding contact
DYCONIGNORE
Flag to ignore initial penetration or not
25
26
DYCONSKIPRWG
Controls whether or not to generate a few extra nodes to
visualize a rigid wall
DYHRGIHQ
Default hourglass viscosity type
DYHRGQH
Default hourglass viscosity coefficient
DYENERGYHGEN
Hourglass energy calculation option
DYTERMNENDMAS Percent change in mass to end calculation
DYTSTEPERODE
Flag which determines whether elements will be eliminated at
time TSMIN
DYTSTEPDT2MS
Time step size for mass scaling
DYMAXSTEP
Maximum allowable time step
DYMINSTEP
Minimum time step that terminates the analysis
DYSHELLFORM
Default shell formulation
DYSHTHICK
Specifies whether or not shell thickness changes with
membrane straining
DYSTEPFCTL
Scale factor for internally calculated time step
DYRBE3
Control of RBE3 translation to MSC.Dytran RBE3 or RBE3D
DYSHNIP
Number of integration points for SOL 700 shells
DYNEIPH
Control of integration point data output for solids
DYNEIPS
Control of integration point data output for shells
DYMAXINT
Another control of integration point data output for shells
DYSTRFLG
Control of strain tensor output
DYSIGFLG
Flag to include stress tensor in binary output file
DYEPSFLG
Flag to include effective plastic strain in binary output file
DYRLTFLG
Flag to include stress resultants in binary output file
DYENGFLG
Flag to include internal energy and thickness in binary output
file
DYCMPFLG
Flag determining coordinate of output stress and strain
tensors
DYIEVERP
Flag determining if more than one output state can be written
to d3plot files
DYBEAMIP
Number of beam integration points for output
CHAPTER 2
Nonlinear Analysis
DYDCOMP
Flag controlling elimination of rigid body output
DYSHGE
Flag controlling output hourglass energy density
DYSTSSZ
Flag controlling output of shell element time step and mass
DYN3THDT
Flag controlling output of material energy
DYNINTSL
Number of solid element integration points for output
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 (elasto-plastic
material with arbitrary stress- strain curves and strain-rate dependency). This
problem takes about 20 minutes to run on a 2.4 GHz PC.
The following plots show various time slices for the analysis:
27
28
CHAPTER 2
Nonlinear Analysis
Portions the MSC.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
+
+
29
30
+
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
SLAVE
3
+
4
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
$ -------- Material MAT_PLASTIC_KINE.1 id =1
MATD024
2
7.896
2.1
.284
0.01
$
$
$
$ ======== Load Cases ========================
$
$
$ ------- Initial Velocity BC ini ----$
TICD
1
1
1
0.1246
TICD
1
1
3
-0.03339
.
.
.
ENDDATA
0.8
0.8
2586
2586
1
1
CHAPTER 2
Nonlinear Analysis
All of the previous input data are described in the compatible MSC.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 parameters and a few
contact entries to the Bulk Data to an existing file that would be used in MSC.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, in SOL 700 for crash simulation.
31
32
Where Can I Find More Information:
MSC.Nastran Explicit Nonlinear Analysis, SOL 700, is documented in the following
manuals and guides:
• MSC.Nastran Quick Reference Guide
• MSC.Nastran Explicit Nonlinear User’s Guide
• MSC.Patran User’s Guide
• MSC.Patran – MSC.Nastran and MSC.Dytran Preference Guides
• LS-Dyna Keyword User’s Manual, Version 970 (available from LSTC)
• LS-Dyna Theoretical Manual (available from LSTC)
• MSC.Dytran Reference Manual
• MSC.Dytran Theory Manual
CHAPTER 2
Nonlinear Analysis
2.2
MSC.Nastran Implicit Nonlinear - SOL 600
Between the release of MSC.Nastran 2004 and MSC.Nastran 2005, there have been
many improvements, a few new capabilities have been added and several errors have
been corrected. This section summarizes the most important of these items.
Additions to the SOL 600 Executive Control Statement:
The new executive control statement is as follows:
SOL 600, ID PATH= COPYR= NOERROR OUTR=op2,xdb,pch,f06,eig,dmap,beam
NOEXIT STOP= CONTINUE=
New items are dmap, beam and CONTINUE. An explanation of these items follows:
dmap
The user will enter his own DMAP to create whatever type of
output that is desired, such as op2, xdb, punch, f06. For all
other options, DMAP is generated as needed internally by
MSC.Nastran.
beam
The beam option must be specified if op2,xdb,pch. or f06
options are specified and beam internal loads are to be
placed in any of these files. The beam and eig options are
mutually exclusive (you cannot specify both).
CONTINUE= is an option that specifies how MSC.Nastran will continue its analysis
after MSC.Marc finishes. To continue the analysis, do not enter any STOP or OUTR
options. It is possible to perform more than one of these operations if necessary.
0
MSC.Nastran will continue the current solution sequence as
normal. For example, if SOL 600,106 is entered, SOL 106 will
continue as normal after MSC.Marc finishes. Only 3D
contact or materials supported by SOL 106 may be used.
1
MSC.Nastran will switch to SOL 107 to compute complex
eigenvalues. MSC.Marc will generate DMIG matrices for
friction stiffness (and possibly damping) on a file specified
by pram,marcfil1,name and time specified by
param,marcstif,time. This is accomplished by making a
complete copy of the original MSC.Nastran input file and
spawning off a new job with the SOL statement changed and
an INCUDE statement for the DMIG file.
33
34
2
MSC.Nastran will switch to SOL 107 to compute complex
eigenvalues. MSC.Marc will generate OUTPUT4 matrices
for friction stiffness (and possibly damping) on a file
specified by pram,marcfil2,name and time specified by
param,marcstif,time, This is accomplished by making a
complete copy of the original MSC.Nastran input file and
spawning off a new job with the SOL statement changed and
an INCLUDE statement for the DMIG file.
3
MSC.Nastran will switch to SOL 111 to compute modal
frequency response. MSC.Marc will generate natural
frequencies and mode shapes that are read into MSC.Nastran
from a file specified by param,marcfil3,name
4
Same as option 3, except that SOL 112 for linear transient
response will be used.
5
MSC.Nastran will switch to the solution sequence given in
field 9 of the MDMIOUT entry. In addition, the DMIG entries
specified by MDMIOUT will be included in a separate
MSC.Nastran execution spawned from the original
execution. Case Control and Bulk Data will be added to the
original input to properly handle these matrices in the
spawned MSC.Nastran execution.
CHAPTER 2
Nonlinear Analysis
An example of input using the continue=1 option is as follows:
SOL 600,106 path=1 stop=1 continue=1
TIME 10000
CEND
param,marcbug,0
ECHO = sort
DISP(print,plot) = ALL
STRESS(CORNER,plot) = ALL
STRAIN(plot) = ALL
SPC = 1
LOAD = 1
NLPARM = 1
CMETHOD=101
BEGIN BULK
param,marcfil1,dmig002
param,mrmtxnam,kaax
param,mrspawn2,tran
param,mrrcfile,nast2.rc
PARAM,OGEOM,NO
PARAM,AUTOSPC,YES
PARAM,GRDPNT,0
EIGC, 101, HESS, , , , ,50
NLPARM
1
10
AUTO
PLOAD4
1
121
-800.
PLOAD4
1
122
-800.
1
P
YES
(rest of deck is the same as any other SOL 600 input file)
CQUAD4
CQUAD4
ENDDATA
239
240
2
2
271
272
272
273
293
294
292
293
The full input for this example can be obtained from MSC.Nastran development. The
name of the input file continu2.dat
Support of Complex Eigenvalue Analysis
SOL 600 now supports complex eigenvalue analysis via the CMETHOD Case Control
command and the EIGC Bulk Data entry. In addition, four new Bulk Data parameters
have been introduced:
param,marcfil1,dmig002
This means that a file named dmig002 will be used. It
contains stiffness matrix terms (possibly from a set of
unsymmetric friction stiffness matrices)
param,mrmtxnam,kaax
This means that in the dmig002 file, use DMIG matrix
terms labeled kaax (or KAAX – case does not matter).
35
36
param,mrspawn2,tran
This means that the primary MSC.Nastran run will
spawn another MSC.Nastran run to compute the
complex eigenvalues. The name of the command is
nastran (nas is always used and the characters specified
by this parameter are added to the end of nas. Thus, we
get nas+tran=nastran).
param,mrrcfile,nast2.rc
This is the name of the rc file to be used for the second
(spawned) MSC.Nastran run.
The flow of the run is as follows:
• Create a primary MSC.Nastran SOL 600 input file (we will name it jid.dat for
this example)
• Submit MSC.Nastran in the standard fashion. For this example, the
following command is used:
nastran jid rc=nast1.rc
The nast1.rc file contains items such as scratch=yes, memory=16mw, etc.
• The primary MSC.Nastran run creates an MSC.Marc input file named
jid.marc.dat
• The primary MSC.Nastran run spawns MSC.Marc to perform nonlinear
analysis. MSC.Marc generates the required DMIG matrices for this example.
• The nonlinear MSC.Marc analyses completes and generates standard files.
• Control of the process returns to MSC.Nastran. A new MSC.Nastran input
file named jid.nast.dat will be created from the original input file. This file
will contain the CMETHOD Case Control command and EIGC Bulk Data
entry, all of the original geometry and additional entries to read the dmig002
file.
• A second MSC.Nastran job will be spawned from the primary MC.Nastran
run using the command
nastran jid.nast rc=nast2.rc
The nast2.rc file can be the same as nast1.rc or can contain different items.
Usually memory will need to be larger in nast2.rc than in nast1.rc.
• The second MSC.Nastran run computes the complex eigenvalues and
finishes.
• Control of the process returns to the primary MSC.Nastran run and it
finishes.
CHAPTER 2
Nonlinear Analysis
The first portion of the dmig002 file is as follows:
$2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678 234567812345
DMIG
KAAX
0
1
2
0
324
DMIG*
KAAX
6
1
*
6
1 3.014712042D+05
*
6
2 4.204709763D+08
*
DMIG*
KAAX
6
2
*
6
1 1.204709763D+05
*
6
2 3.014712042D+05
*
DMIG*
KAAX
6
3
*
6
1-4.616527206D+04
*
6
2-4.616527206D+04
*
6
3 1.308497299D+05
DMIG*
KAAX
17
1
*
6
1 6.239021038D+04
*
6
2-2.528344607D+03
*
6
3-6.239758760D+03
*
17
1 5.939989945D+05
*
Temperature-Dependent Stress Strain Curves
MSC.Nastran 2005 offers the capability of stress-strain curve dependence as a function
of temperature. The user specifies these stress strain curves at different temperatures
and then specifies the temperature to use for each subcase. Linear interpolation
between the supplied curves is used to determine the appropriate curve at the
temperature specified for a particular subcase. MSC.Marc’s AF-Flowmat capability is
used for this capability; therefore, user subroutines do not have to be supplied. This
capability is best explained with an example (this example can be obtained from
MSC.Nastran development. The name of the file is mattep20.dat).
SOL 600,NLSTATIC path=1 stop=1
TIME 10000
CEND
ECHO = NONE
DISPLACEMENT(plot) = ALL
SPCFORCE(PLOT) = ALL
Stress(PLOT) = ALL
Strain(PLOT) = ALL
SPC = 1
NLPARM = 2
temp(init)=10
subcase 1
temp(load)=11
LOAD = 100
subcase 2
temp(load)=12
LOAD = 200
subcase 3
temp(load)=13
LOAD = 300
37
38
BEGIN BULK
param,mrafflow,mymat0
param,mrtabls1,4
param,mrtabls2,1
NLPARM
2
10
AUTO
1
20
P
PARAM,LGDISP,1
tempd, 10, 70.
tempd, 11, 110.
tempd, 12, 700.
tempd, 13, 1100.
$LOAD, 20, 1.0, 2.0, 1, 1.0, 2
load, 100, 1., 1., 1
load, 200, 1., -.5, 1
load, 300, 1., 1.1, 1
PLOAD4
1
1
-15.
.
.
.
$ Constraint Set 1 : Untitled
SPC
1
1 123456
0.
SPC
1
8 123456
0.
SPC
1
15 123456
0.
SPC
1
22 123456
0.
SPC
1
29 123456
0.
$ Property 1 : Untitled
PSHELL
1
1
0.125
1
1
0.
$ Material 1 : AISI 4340 Steel
MATEP, 1,TABLE, 35000., 2,CAUCHY,ISOTROP,ADDMEAN
MAT1
1 2.9E+7
0.327.331E-4 6.6E-6
70.
+MT
+MT
1 215000. 240000. 156000.
MAT4
14.861E-4
38.647.331E-4
$
1
2
3
4
5
6
7
8
9
$2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678
MATTEP
1
21
MATT1
1
7
TABLEM1
7
+
70.0
6.6E-6
1000. 6.5E-6
1200. 6.4E-6 1500.
6.3E-6
+
2000.
6.2E-6
ENDT
$2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678
TABLEST
21
+
70.0
31
1000.
32
1200.
33
1500.
34
+
2000.
35
ENDT
TABLES1, 31
, 0., 15000., 1.0, 16000., 10., 25000., 100., 30000.,
, 99999., 40000., ENDT
TABLES1, 32
, 0., 13000., 1.0, 14000., 10., 23000., 100., 28000.,
, 99999., 28000., ENDT
TABLES1, 33
, 0., 11000., 1.0, 12000., 10., 21000., 100., 26000.,
, 99999., 25000., ENDT
TABLES1, 34
, 0., 9000., 1.0, 10000., 10., 19000., 100., 22000.,
, 99999., 24000., ENDT
TABLES1, 35
, 0., 5000., 1.0, 7000., 10., 9000., 100., 13000.,
, 99999., 15000., ENDT
GRID
1
0
0.
0.
0.
0
.
1
CHAPTER 2
Nonlinear Analysis
.
.
CQUAD4
.
.
.
ENDDATA
In this input, the stress strain curves are specified by TABLES1 entries. The collection
of stress-strain curves to be used is specified in the TABLEST entry and the
corresponding temperatures at which they apply is specified in the TABLEM1 entry.
The TABLEM1 ID is called out in field 7 of the MATT1 entry and the TABLEST ID is
called out in field 5 of the MATTEP entry. TABLEST must list the stress strain
TABLES1 IDs in order of increasing temperature and the first ID must be at the lowest
temperature specified anywhere in the analysis. In this example, it is a temperature of
70 corresponding to temp(init)=10 in the Case Control. Similarly, the temperatures in
the TABLEM1 entry must be in increasing order. The stress-strain curves should
cover the entire range of temperatures for the analysis so that no extrapolation is
needed. The actual temperatures for each subcase are given by the temp(load)
specifications for each subcase.
There is one parameter that is critical to this analysis:
param,mrafflow,mymat0
Name of the file containing temperature dependent
stress versus plastic strain curves in MSC.Marc’s
AF_flowmat format. This file can be generated from the
current MSC.Nastran run using TABLEST and
TABLES1 entries or a pre-existing file can be used
depending on the value of PARAM,MRAFFLOR. The
extension “.mat” will be added to Name. If this is a new
file, it will be saved in the directory from which the
MSC.Nastran execution is submitted. If a pre-existing
file is to be used, it can either be located in the directory
where the MSC.Nastran execution is submitted or in the
MSC.Marc AF_flowmat directory.
Improved Parallel Processing for SOL 600
In previous versions of SOL 600, the basic MSC.Marc input file had to be split up into
as many MSC.Marc input files as processors to be used. MSC.Nastran 2005
incorporates the capability to use a new MSC.Marc feature called the Single File
Parallel file. For this to work properly, the user must obtain MSC.Marc 2003 beta 2 or
39
40
later to run in combination with MSC.Nastran. The interface to use this capability
specifies KIND=0 or blank on the PARAMARC entry as shown below (the other
options are still available but should be considered obsolete).
Format:
1
2
3
4
PARAMARC
ID
KIND
NPROC
5
6
7
8
9
10
Example: To create 4 parallel processes using MSC.Marc’s single file input
PARAMARC
51
4
Field
Contents
ID
Identification number of the PARAMARC entry -- Not presently used.
(Integer)
KIND
Designates how parallel domains are created. (Integer > 0, Default = 0)
0=Parallel processing is accomplished using MSC.Marc’s single file
input. MSC.Marc Version 2005 and subsequent versions must be used.
The command line to execute MSC.Marc is changed from -np N (or nprocd N) to -nps N where N is the number of processors. The
maximum number of processors for MSC.Marc is 256. Continuation
lines may not be entered for KIND=0.
A similar option to create a single-file MSC.Marc t16 file is available starting with
MSC.Marc 2005. This option is picked using Bulk Data PARAM,MARCOUTR,1. Be
sure to have MSC.Marc 2005 or later before using this option since it does not work
properly with earlier versions.
Support for Intel and Digital Visual Fortran PC Version of MSC.Marc
Starting with MSC.Marc 2005, an Intel version as well as a Digital Visual Fortran (also
known as Comopaqa Visual Fortran) is available. MSC.Nastran 2004 r3 and
MSC.Nastran 2005 support both versions. Distinctions between the two versions are
only necessary for specifying the PATH to MSC.Marc and for OUTR results
processing. The PATH can be handled as normal by using one of the path options on
the SOL 600 Executive statement. The OUTR options will be processed internally by
MSC.Nastran if the MSC.Marc Intel version is used and will require an external
t16op2.exe program if the Digital Visual Fortran version is used. Beam/Bar loads,
CHAPTER 2
Nonlinear Analysis
stresses and strains are available using the Intel version and are not available using the
Digital Visual Fortran version. The PC version for OUTR processing can be selected
by the new MSC.Nastran Bulk Data parameter:
MARCWIND
Integer, Default=0 Determines which Windows version of
MSC.Marc (Digital Visual Fortran or Intel) is to be used for those
versions of MSC.Marc that support both versions. This option is
only necessary if any OUTR option is used. If the Intel version is
used, all t16op2 work is accomplished inside MSC.Nastran. If the
DF version is used, a separate t16op2.exe program is required and
must be on the PATH. This parameter applies only to SOL 600 used
in combination with MSC.Marc 2005 or later versions. The
MSC.Marc PC version prior to 2005 always used the Digital Visual
Fortran version.
0
The Digital Visual Fortran version of MSC.Marc is used.
1
The Intel version of MSC.Marc is used.
Other SOL 600 Items:
• PBUSHT support has been added for nonlinear springs. TABLED1 can be
used to specify the load-deflection curve. The PBUSHT/TBLED1 data is
mapped to MSC.Marc’s SPRINGS option with table-driven force-deflection
curves. This capability will work with MSC.Marc 2003 or 2005.
• Buckling: In prior SOL 600 versions, only one nonlinear load case could be
run prior to a buckling eigenvalue extraction. Now, multiple nonlinear load
cases can be run before requesting buckling eigenvalue extraction.
• Improved beam offsets: MSC.Nastran 2005 supports beam and shell/plate
offsets - they were not supported in some earlier versions and only partially
supported in recent versions. The offsets are handled by adding extra nodes
at the offset coordinates and connecting RBE2 between original and offset
coordinates. Beam type 98 must be used rather than beam type 14 for offsets
since beam type 14 does not have the fully 6 DOFs required for RBE2. That
means beam plasticity cannot be combined with the beam offset. The
numbering of the extra modes starts at the highest node ID, and increments
by one above that.
• CBEAM and CBAR internal loads, stresses and strains were added for op2,
xdb, punch and f06 results. This addition is applicable to UNIX/Linux
systems and to Windows systems if an Intel Marc 2005 (or beyond) version
is used.
41
42
• Bolt elements were added to support MSC.Marc both outside the USA and
within the USA. MSC.Nastran Bulk Data entries, MBOLT and MBOLTUS
reflect these new additions.
• The stacking direction for 3D composites were added with a new entry,
MSTACK.
• Licensing for SOL 600 was changed to eliminate an extra license to spawn
MSC.Marc. The MSC.Marc license is adequate for that purpose. In addition,
a standard MSC.Nastran Nonlinear (SOL 160, 129) license was sometimes
required -- this has now been eliminated.
• Improved support for element material coordinate systems
• Improved non-constant pressure loading, which means that P1, P2, P3, P4 on
the PLOAD4 entry will be used. Before, P1 was applied as a constant
pressure n the element face.
• The following errors have been corrected:
• Work hardening slope specified by MATEP was ignored.
• Gasket materials could not be defined with other solid element
materials.
• Eigenvalue analysis after a nonlinear analysis sometimes gave wrong
results.
• FTYPE variable of the BCPARA entry was not translated.
• More than one NLSTRAT entry could not be provided.
• RFORCE did not translate properly.
• MSC.Marc’s ORIENTATION option was not employed correctly.
• CPENTA pressures were sometimes applied to the wrong face.
• BEGINBULK caused an abort.
CHAPTER 2
Nonlinear Analysis
2.3
Pre-release of the Nonlinear Transient Analysis in
SOL 400
Introduction
In order to improve the nonlinear solution procedure in MSC.Nastran, a general
nonlinear solution sequence, SOL 400, has been introduced since MSC.Nastran 2004
to support nonlinear static analysis. In MSC.Nastran 2005, a new capability, the
nonlinear transient analysis, has been added to SOL 400. Since some capabilities are
still under development and the V&V test has not been completed, this is only a prerelease and its intention is to get user feedback. Eventually, this solution sequence will
include all nonlinear analyses, such as the nonlinear static analysis, the nonlinear
transient analysis, the nonlinear buckling analysis, the nonlinear normal modes
analysis, and other related solution procedure such as the linear static and transient
analysis into one general solution procedure. In the final run, SOL 400 is going to
replace the current nonlinear static solution sequence SOL 106 and the nonlinear
transient solution sequence SOL 129. In addition, the nonlinear heat transfer solution
sequence, SOL 153 and SOL 159 will also be included in SOL 400 in the future. Up
until now, SOL 400 does not replace SOL 106 and 129.
Benefits
The new benefits of SOL 400 are discussed this section. Some of the benefits may be
subject to the limitation discussed in next section. The benefits are:
• The Case Control command STEP, which was first introduced in
MSC.Nastran 2004 to allow user to input a flexible loading and solution
sequence at an independent loading SUBCASE in the nonlinear static run, is
also supported by nonlinear transient analysis.
• User can specify different type of ANALYSIS, such as NLSTAT and
NLTRAN, at different SUBCASE’s in a single run.
• The different STEP’s can specify different types of ANALYSIS only when
they belong to the same kind of analyses, such as static or transient analysis.
For example, both NLSTAT and LNSTAT are static analyses; therefore, they
can be mixed in a SUBCASE. However, NLSTAT and NLTRAN cannot be
mixed in a SUBCASE.
• An improved nonlinear iteration procedure to make solution easier and
faster to converge. All AUTO, TSTEP (or ITER), ADAPT and SEMI, which is
the method for controlling stiffness updates, are supported in the nonlinear
transient analysis.
43
44
• AUTOSPC can be executed when every time updating the matrices if user
requests.
• Direct matrix input, such as K2PP, and EPOINT are supported in nonlinear
transient analysis.
• Support “grid based reordering” for a faster decomposition to both
nonlinear static and transient analyses.
• Support thermal excitation in the nonlinear transient analysis. Two new Bulk
Data entries, TTEMP and TMPSET, have been added for this new feature in
nonlinear transient analysis.
• The GPFORCE and ESE output are supported in the nonlinear static
analysis.
• The same restart capability, which had been introduced in MSC.Nastran
2004, is also available to the nonlinear transient analysis now.
• A more flexible output method for the nonlinear transient analysis. User can
use a new parameter NLPACK to control the output and restart time steps.
• Allow simulation of the same output logic and format of SOL 129 by
specifying a negative NO on the TSTEPNL Bulk Data entry.
Limitations for the Current Release
In this pre-release, the following capabilities are not supported:
• Initial Condition in the nonlinear transient analysis.
• The nonlinear normal modes and the nonlinear buckling analysis.
• RFORCE and Creep.
• The arc-length method (input by NLPCI Bulk Data entry).
• The stress data recovery of the layer composite elements.
• Only the left-rotation-vector method, LANGLE=3, is allowed to process
large rotation in nonlinear transient analysis.
• The nonlinear static analysis (ANALYSIS=NLSTAT) and the nonlinear
transient analysis (ANALYSIS=NLTRAN) cannot be mixed in one
SUBCASE.
• The line contact.
The first 5 items will be supported in a future release. However, the last item
‘line contact’ will not be support in SOL 400. It will be replaced by the general
contact capability in SOL 600.
CHAPTER 2
Nonlinear Analysis
In the following sections, how the new capabilities work in the current
release is discussed.
Case Control Commands – SUBCASE, STEP and
ANALYSIS
The STEP command was first introduced in MSC.Nastran 2004 for the nonlinear static
analysis of SOL 400. In this release, it has been expanded to support the nonlinear
transient analysis and again for SOL 400 only. User can specify different type of
analysis at different SUBCASE and/or STEP by using the Case Control command
ANALYSIS. Until now, ANALYSIS Case Control command supports the following 3
keywords. They are LNSTATIC, NLSTATIC (the default) and NLTRAN. The
combination of SUBCASE, STEP and ANALYSIS commands will provide a
mechanism for defining the multiple load steps, running multiple independent cases
and, at same time, allowing the user to specify multiple 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. Note that it is not legal to assign two different
keywords, NLSTATIC and NLTRAN, of ANALYSIS in one SUBCASE. 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 SUBCASE’s may be executed in one job where the types of analysis,
loads and boundary conditions can be changed. All SUBCASEs are
independent from 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. In each
SUBCASE, there can have different type of ANALYSIS. For example
45
46
SUBCASE 1
ANALYSIS = NLSTAT
$ This line can be omitted
NLPARM = 100
STEP 110
LOAD = 110
STEP 120
LOAD = 120
SUBCASE 2
ANALYSIS = NLTRAN
TSTEPNL = 200
STEP 210
DLOAD = 210
STEP 220
DLOAD = 220
In above example, the solutions of SUBCASE 1 and SUBCASE 2 are
independent of each other. In case that the solution divergence is detected in
a step, MSC.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 on 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, which makes
the linear static solution and the nonlinear static solution become special
cases of the general nonlinear solution procedure. For this release, only the
linear static analysis and the nonlinear static analysis can be mixed in one
SUBCASE. 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. The
default ANALYSIS method, i.e., there is no ANALYSIS command in the Case
Control file, is NLSTATIC.
CHAPTER 2
Nonlinear Analysis
Vector Operations and Convergence Criteria
The convergence criteria are specified by using the Bulk Data entry TSTEPNL in the
nonlinear transient analysis. In performing the convergence tests, we compute three
error factors: 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 MSC.Nastran set
definition, please refer to the Quick Reference Guide, section (7.1).
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 are
become smaller; therefore, the convergence rate of this value is proportional to the
squire 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 structure model is computed during iterations and the work
error is estimated based on the total work. In this way, the work error gives an
estimation of error in 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.
Solution Algorithm and Simulation of SOL 129
In SOL 400, the solution algorithm is modified in the following areas:
• Three new nonlinear iterations and stiffness update algorithm, AUTO,
TSTEP (or ITER) and SEMI, are added on the Bulk Data entry TSTEPNL.
(Please see the “TSTEPNL Additions” on page 63 for the details of
TSTEPNL Bulk Data entry.) The old method, ADAPT, is still supported.
• The algorithm for load bi-sections.
• The algorithm for automatic time adjustment after converging at each time
step.
• The solution divergence processing.
47
48
The stiffness update strategy as well as the direct time integration method is selected
in the METHOD field of TSTEPNL Bulk Data entry. As mentioned above, there are
four options:
• If the AUTO option is selected, the program automatically selects the most
efficient strategy to adjust the incremental time step, perform the iterations,
update the matrix, and use bisection. Please note the incremental time step
adjustment is performed before the start of a time step. And bisection will be
performed after solution iterations and stiffness updates when convergence
cannot be achieved.
• If the TSTEP option is selected, the program updates the stiffness matrix
every KSTEP iterations. The bisection will be applied only when the
convergence cannot be reach by updating matrix. In this option, no
automatic time step adjustment will be performed.
• If the ADAPT option is selected, the program automatically adjusts the
incremental time step. If convergence cannot be achieved, then bisection will
be performed. This method only updates matrix at every KSTEP convergent
bisection solutions.
• If the SEMI option is selected, the program will update the stiffness matrix
after the first iteration at each time step and then assume the normal AUTO
option.
The stiffness matrix is always updated for a new STEP or Restart, irrespective of the
option selected. The AUTO method has replace ADAPT to become the new default in
the current release for ANALYSIS=NLTRAN in SOL 400.
For most of the problems we tested, SOL 400 gives equal or better performance than
that of SOL 129. However, SOL 400 only output at user specified time steps in default.
In order to give output similar to that of SOL 129, user can assign a negative NO on
TSTEPNL to retrieve the output logic from SOL 129.
Nonlinear Iteration Summary Table for Nonlinear Transient
Analysis in SOL 400
In order to allow the user 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 during the nonlinear iteration. Due to printing of the average
and the maximum displacements, the user will able to know the solution status before
the end of the job. This is useful for large nonlinear problems. Even for small
CHAPTER 2
Nonlinear Analysis
problems, the user will be able to know approximately how the analysis of a structural
model performs by examining this table. An example of this table is given below and
the descriptions of information given in this table are shown in Table 2-3.
Table 2-3 Nonlinear Iteration Summary Table
0
N O N - L I N E A R
STIFFNESS UPDATE TIME
ITERATION TIME
TIME
5.00000E-02
5.00000E-02
1.00000E-01
1.00000E-01
- TIME STEP NO. BIS ADJUST ITR
1
1
2
2
0
0
0
0
1.0000
1.0000
1.0000
1.0000
I T E R A T I O N
M O D U L E
0.02 SECONDS
0.00 SECONDS
1
2
1
2
SUBCASE
- - ERROR FACTORS - DISP
LOAD
WORK
1.00E+00
5.59E-07
8.15E-01
3.90E-07
3.30E-03
1.83E-09
4.92E-03
3.31E-09
O U T P U T
3.30E-03
1.10E-06
3.94E-03
8.20E-07
CONV ITR MAT
AVG
RATE DIV DIV R_FORCE
1.00
0.00
1.00
0.00
0
0
0
0
1
1
1
1
1.1E-04
1.0E-08
4.3E-04
2.8E-09
TOTL
WORK
1.331E-05
1.331E-05
3.098E-04
3.098E-04
1130
STEP
1
- - - - - DISP - - - - - - NO. TOT TOT
AVG
MAX
AT GRID C QNV KUD ITR
2.63E-07
2.63E-07
1.42E-06
1.42E-06
1.644E-06
1.644E-06
9.204E-06
9.204E-06
1001
1001
1011
1011
1
1
1
1
0
1
1
2
0
0
0
0
1
2
3
4
Table 2-4 Explanation of Information in Nonlinear Iteration Summary Table
TIME
The Current Time. It starts from 0.0 in the beginning of the 1st
STEP and accumulates the value until at the end of the last
STEP. To each STEP, the total time is determined by NDT and
DT on the TSTEPNL Bulk Data entry.
TIME STEP NO
Number of time increment, including bisection. Initialize 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
the TSTEPNL Bulk Data entry.
ITR
Number of iterations 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 denotes 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 divergence. Action to correction solution
divergence will be taken if ITRDIV > MAXDIV.
MATDIV
Number of material divergence + 1, i.e.,it will be 1 if there is
no material divergence. The material divergence is due to bad
creep strain or excessive sub-increments in plasticity.
49
50
Table 2-4 Explanation of Information in Nonlinear Iteration Summary Table
AVG R_FORCE
Average residual force. In order for an increment 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.
TOT KUD
Total number stiffness updates performed.
TOT ITER
Total number iterations performed, including the number of
stiffness updates.
Restart
The purpose of a nonlinear restart is to allow the user 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 the user want to change the loading
sequence, the solution criteria, or to extend the analysis.
For SOL 400, a user-friendly restart procedure has been implemented. For the
nonlinear transient analysis, only the following principles are listed in this release
note:
• The restart must be continued at previous converged solution point in a
nonlinear transient analysis by specifying a SUBCASE, STEP, and/or TIME.
This is accomplished by using the Case Control command NLRESTART;
please refer to “Case Control Commands” in Chapter 4 of the MSC.Nastran
Quick Reference Guide.
• When a job has ANALYSIS=NLSTAT in SOL 400, it can restart at any user
specified load steps (controlled by NOUT in NLPARM Bulk Data entry). The
tremendous size of database should be required when
ANALYSIS=NLTRAN in SOL 400 if the same logic mention above is used.
To reduce the size of database and save the CPU time of I/O, a new
parameter, NLPACK, is introduced in nonlinear transient analysis in SOL
400; please also see “Outputs” on page 52 e for the details of this new
parameter. The nonlinear transient job can only restart at the closest output
time step (controlled by NO on TSTEPNL Bulk Data entry), which is also the
last time step of each output package (controlled by NLPACK parameter).
CHAPTER 2
Nonlinear Analysis
• 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.
The procedure to perform the restart for the nonlinear transient analysis is similar to
the nonlinear static analysis in SOL 400; therefore, no further discussion here.
Temperature Excitation
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 timedependent 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 ref ) – α ( T 0 ) ⋅ ( T 0 – T ref )
where:
ε T ( t ) = the thermal strain
T ( t ) = the current temperature is defined in T ( t ) = { T p }f ( t )
{ T p } is the temperature field and f ( t ) is the time function,
T ref = the reference temperature,
T 0 = the stress free temperature (initial temperature), and
( T ) = the coefficient of thermal expansion
To 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.
Unlike all the other linear and nonlinear analyses, the thermal load is not created to
the nonlinear elements anymore in SOL 400.
In MSC.Nastran 2004, the thermal effect has been added into nonlinear static analysis
in SOL 400. To support it in nonlinear transient analysis, two new bulk data entries
are created in the current release. They are TTEMP and TMPSET. Basically, TTEMP
is to define a time-dependent dynamic thermal field, T(t), in the same form as
TLOAD1. At the same time, TMPSET is to define a group of grid points, which refers
to the same TTEMP Bulk Data entry. Please see “New Bulk Data Entries, TTEMP and
51
52
TMPSET” on page 64 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,
user can also make every grid point as a independent sub-region or make the whole
model as a single sub-region.
Same as 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 (and TMPSET) but not the
TEMP(INIT). The temperature of any grid point, whose ID is not listed in the
TMPSET, will be interpolated linearly in the same way as nonlinear static analysis. In
other words, when there is no TTEMP (and TMPSET) in the Bulk Data file, the
TEMP(LOAD) will refer to the TEMP (or TEMPD, TEMPP1,...,etc.) directly and a
linear interpolation scheme will be used to determine the temperature filed in any
specified time.
User should only set one temperature set (SID) in each STEP but this rule is only
forced in the nonlinear elements. To all the linear elements, user can still use DLOAD
bulk data entry to combine multiple TLOAD1 and TLOAD2’s, whose EXCITE_ID
reference thermal load, to support multiple sets of temperature loads – this is also
known as “static load for dynamics” to the temperature loads. However, it is user’s
responsibility to explain the physical meanings.
Note that all the upper stream superelements and all linear elements in the residual
are still used the original concept, “static load for dynamics” to input the thermal
effect when ANALYSIS=NLTRAN in SOL 400. The TEMP(LOAD) and all its
corresponding temperature related bulk data entries introduced above can only
describe the thermal effect to the nonlinear elements in the residual. If there is no
DLAOD Case Control command to define the temperature load in the “static load for
dynamics” way, the temperature effect to the linear part of the structure will be lost.
Outputs
The outputs are requested by using the Case Control commands. All existing output
requesting 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”, which have been introduced in MSC.Nastran 2004, are also available on
the nonlinear transient analysis in SOL 400. In addition, a new output control,
PARAM, NLPACK, is added in this release for nonlinear transient analysis only.
CHAPTER 2
Nonlinear Analysis
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 case. Note that
NLPACK=-1 means to collect all output times steps in a STEP case and then output
them all together, which is the same as SOL 129 output method. This parameter only
used in ANALYSIS=NLTRAN and restart is only possible at the end of each
"NLPACK" output time step. To nonlinear static analysis (ANALYSIS=NLSTAT),
NLPACK is always equal to 1.
User Interfaces
The user interfaces, which are important or new to the nonlinear transient analyses in
SOL 400, are summarized in this section. For details, please refer to the MSC.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.
• ITRFMT (SYSTEM (401)) – Selects the convergence parameter computation
method and the divergence solution checking method to simulate the
SOL 129. If ITRFMT = -1, use method similar to SOL 129.
• TZEROMAX (SYSTEM (373)) – Controls initial time step adjustment in
nonlinear transient analysis.
File Management Statements
The following File Management statements are required for restarts. Please refer to the
“File Management Statements” in Chapter 2 of the MSC.Nastran Quick Reference
Guide or Chapter 12 of the MSC.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 Statement
• SOL 400 or SOL NONLIN – Requests the SOL 400 general nonlinear solution
sequence
53
54
Parameters
• PARAM, LANGLE – Selects the method to represent large rotations in a
geometric nonlinear analysis, 1 for the Gimbals angle method, 2 for the left
rotation method, and 3 for the right rotation method. The default value is 3
for the nonlinear transient analysis.
• PARAM, LGDISP – Requests a geometric nonlinear analysis.
• PARAM, FOLLOWK – Requests whether the follower force stiffness will be
used in a geometric nonlinear analysis.
• PARMA, FKSYMFAC – Controls whether the symmetrical follower force
stiffness will be used in a geometric nonlinear analysis.
• PARAM, MAXLP – Specifies maximum number of iterations for element
relaxation and material point sub-increment process.
• PARAM, NLAYERS – Specifies the number of layer for through thickness
integration in the material nonlinear analysis.
• PARAM, NLTOL – Selects defaults for CONV, EPSU, EPSP, and EPSW for
the Bulk Data entry NLPARM.
• PARAM, PH2OUT – Requests phase II outputs for a nonlinear analysis.
• PARAM, NLPACK – Control the total output time step in one output
package, see “Outputs” on page 52.
• PARAM, NDAMP – Specifies the α value (a numerical damping) of the
HHT-α method in SOL 400.
Case Control Commands
• ANALYSIS – Selects solution method for an analysis step, see “Case Control
Commands” on page 54.
• NLRESTART – Requests a restart execution at a specific solution point for
SOL 400, see “Restart” on page 50.
• NLSTRESS – Requests the form and type of the nonlinear element stress
output.
• STEP – Delimits and identifies an analysis step, see “Case Control
Commands” on page 54.
Bulk Data Entries
• MATHP- Specifies the hyperelastic material properties for an element.
CHAPTER 2
Nonlinear Analysis
• MATS1 – Specifies the stress-dependent material properties for an element.
• TSTEPNL – Defines a set of parameters for nonlinear transient analysis
iteration strategy.
• TTEMP – Defines a time-dependent dynamic temperature distribution in
nonlinear transient response.
• TMPSET – Defines a time-dependent dynamic thermal load group for use in
TTEMP Bulk Data entry.
Examples
The following three examples show the inputs 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 simplified from 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 the 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
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
55
56
$
BEGIN BULK
PARAM
NDMAP
PARAM
LGDISP
TSTEPNL 310
TSTEPNL 320
$
PLOAD4 510
$
TLOAD1 100
TABLED1 120
+TBD1
0.
MAT1
100
MAT1
101
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
$
CQUAD4 101
CQUAD4 102
CQUAD4 103
CQUAD4 104
CQUAD4 105
CQUAD4 106
CQUAD4 107
CQUAD4 108
CQUAD4 109
CQUAD4 110
CQUAD4 111
0.0
1
100
100
0.01
0.01
101
5.
510
0
0.
3.+7
3.+7
5.
10
10
AUTO
AUTO
THRU
0
112
120
+TBD1
100
100
100
100
100
100
100
100
100
100
100
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
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.
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
10000
10100
10200
10300
10400
10500
10600
10700
10800
10900
11000
10001
10101
10201
10301
10401
10501
10601
10701
10801
10901
11001
10101
10201
10301
10401
10501
10601
10701
10801
10901
11001
11101
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
10100
10200
10300
10400
10500
10600
10700
10800
10900
11000
11100
CHAPTER 2
Nonlinear Analysis
CQUAD4
$
PSHELL
$
SPC1
SPC1
$
SPC1
SPC1
SPC1
SPC1
$
ENDDATA
112
100
11100
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
11201
11200
101
Example 2
Example two, EX02, is modified from 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 adding some static loads and NLPARM’s. All the bold-font statements are
entries that show difference in two different types of analyses.
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
DLOAD
= 100
SPC
= 200
TSTEPNL = 310
STEP
20
DLOAD
= 100
EX02
57
58
SPC
= 400
TSTEPNL = 320
$
BEGIN BULK
NLPARM 110
10
AUTO
YES
NLPARM 120
10
AUTO
YES
$
LOAD
800
0.01
1.0
510
LOAD
900
0.05
1.0
510
(… The rest is same as what in the Bulk Data Deck in the 1st Example…)
ENDDATA
Example 3
Example three, EX03, is modified from 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
EX03
CHAPTER 2
Nonlinear Analysis
TSTEPNL= 1
SPC = 2
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
59
60
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
2.9-6
6.-6
79.
MATT8
1
3
5
1
2
$
TABLEM1 1
+
CR 60.
+
CS 120.
+
CT 180.
+
CU 250.
+
CV 320.
$
TABLEM1 2
+
CW 60.
+
CX 120.
+
CY 180.
+
CZ 250.
+
DA 320.
$
TABLEM1 3
+
BX 60.
+
BY 120.
+
BZ 180.
+
CA 250.
+
CB 320.
$
TABLEM1 4
+
CM 60.
+
CN 120.
+
CO 180.
+
CP 250.
+
CQ 320.
$
TABLEM1 5
+
CC 60.
+
CD 120.
+
CE 180.
+
CF 250.
+
CG 320.
$
TABLEM1 6
+
CH 60.
+
CI 120.
+
CJ 180.
+
CK 250.
+
CL 320.
79.
0.
.29
1.4+6
4
6
0.
YES
1.9-4
2.9-6
70.
4.01-6 140.
3.52-6 200.
3.87-6 260.
4.24-6 ENDT
2.9-6
3.89-6
3.47-6
3.99-6
80.
150.
220.
280.
3.24-6
3.78-6
3.55-6
4.12-6
100.
160.
240.
300.
3.86-6
3.68-6
3.76-6
4.24-6
+
+
+
+
+
CR
CS
CT
CU
CV
6.-6
70.
1.341-5 140.
1.266-5 200.
1.296-5 260.
1.46-5 ENDT
6.-6
1.37-5
1.222-5
1.334-5
80.
150.
220.
280.
7.67-6
1.349-5
1.218-5
1.415-5
100.
160.
240.
300.
+
1.168-5+
1.328-5+
1.259-5+
1.46-5 +
CW
CX
CY
CZ
DA
7.15+6 70.
7.11+6 140.
7.06+6 200.
7.04+6 260.
7.08+6 ENDT
7.15+6
7.08+6
7.05+6
7.05+6
80.
150.
220.
280.
7.15+6
7.07+6
7.05+6
7.06+6
100.
160.
240.
300.
7.13+6
7.07+6
7.04+6
7.08+6
+
+
+
+
+
BX
BY
BZ
CA
CB
.29
.29
.29
.29
.29
.29
.29
.29
.29
80.
150.
220.
280.
.29
.29
.29
.29
100.
160.
240.
300.
.29
.29
.29
.29
+
+
+
+
+
CM
CN
CO
CP
CQ
2.9+6
70.
2.75+6 140.
2.47+6 200.
2.03+6 260.
1.65+6 ENDT
2.9+6
2.68+6
2.35+6
1.95+6
80.
150.
220.
280.
2.9+6
2.64+6
2.22+6
1.8+6
100.
160.
240.
300.
2.82+6
2.58+6
2.09+6
1.65+6
+
+
+
+
+
CC
CD
CE
CF
CG
1.4+6
70.
1.29+6 140.
1.15+6 200.
810000. 260.
500000. ENDT
1.4+6
1.24+6
1.1+6
750000.
80.
150.
220.
280.
1.4+6
1.22+6
980000.
620000.
100.
160.
240.
300.
+
1.34+6 +
1.2+6 +
870000.+
500000.+
CH
CI
CJ
CK
CL
$
cquad4,1,1,1,2,5,4
ctria3,2,1,1,2,4
ctria3,3,1,2,5,4
70.
140.
200.
260.
ENDT
CHAPTER 2
Nonlinear Analysis
$
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
SPC1
1
123456 1
2
spc1
1
123456 4
$
TTEMP,3,111,300
TMPSET,111,4,5
TTEMP,3,101,310
TMPSET,101,1,2
$
TTEMP,4,102,400
TMPSET,102,1,2,4,5,7,8,9,
,10,11,12
$
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
79.
TEMP
1
2
79.
TEMP
1
4
79.
TEMP
1
5
79.
$
TEMP
3
1
80.
TEMP
3
2
80.
TEMP
3
4
80.
TEMP
3
5
80.
TABLED1 300
0.0
.9875
1.0
1.0
ENDT
TABLED1 310
0.0
.9875
1.0
1.0
ENDT
$
TEMP
4
1
81.
TEMP
4
2
81.
TEMP
4
4
81.
TEMP
4
5
81.
TABLED1 400
1.0
.9876542 2.0
1.0
ENDT
$
61
62
TEMP
5
TEMP
5
TEMP
5
TEMP
5
TABLED1 500
0.0
$
TEMP
6
TEMP
6
TEMP
6
TEMP
6
$
$
TEMP
7
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
1
2
4
5
.9875
80.
80.
80.
80.
1.0
1
2
4
5
81.
81.
81.
81.
1
2
4
5
80.
80.
80.
80.
.9875
1
2
4
5
1.0
.9875
1
2
4
5
ENDT
1.0
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.
CHAPTER 2
Nonlinear Analysis
TSTEPNL Additions
TSTEPNL
Parameters for Nonlinear Transient Analysis
Field
Contents
METHOD
Method for controlling stiffness updates and direct-time-integration
strategy. See Remark 4. (Character=“AUTO”,”TSTEP”,“ADAPT” or
“SEMI”; Default=”AUTO”)
KSTEP
The criteria for the stiffness matrix update. See Remark 5. (Integer>0;
Default=2)
Remarks:
4. The stiffness update strategy as well as the direct time integration method is
selected in the METHOD field.
• If the AUTO option is selected, the program automatically selects the
most efficient strategy to update matrix, adjust the incremental time
step and use bisection.
• If the TSTEP option is selected, the program updates the stiffness
matrix every KSTEP increments of time step. The bisection will be
applied only when the convergence cannot be reach by updating
matrix and no automatic time step adjustment.
• If the ADAPT option is selected, the program automatically adjusts
the incremental time step and bisection. This method only updates
matrix at every KSTEP convergent bisection solutions.
• If the SEMI option is selected, the program will update the stiffness
matrix after the first iteration at each time step and then assume the
normal AUTO option.
The stiffness matrix is always updated for a new STEP or Restart,
irrespective of the option selected.
5. For AUTO and SEMI options, the stiffness matrix is updated on convergence
if KSTEP is less than the number of iterations that were required for
convergence with the current stiffness. For ADAPT option, stiffness is
updated every KSTEP converged bisection solutions. For TSTEP, stiffness is
updated at every KSTEP iteration at a time step interval.
63
64
New Bulk Data Entries, TTEMP and TMPSET
Temperature Distribution of Transient Response for Dynamic
Thermal Excitation
TTEMP
Define a time-dependent dynamic thermal distribution in the same form as TLOAD1
{T(t)} = {A(T) ⋅ F(t) }
where A ( T ) defines the temperature field and T ( t ) is the temperature distribution for
use in the nonlinear elements in nonlinear transient analysis.
Format:
1
TTEMP
2
3
4
SID
GROUP_ID
TID
2
3
4
11
101
31
5
6
7
8
9
10
5
6
7
8
9
10
Example:
1
TTEMP
Field
Contents
SID
Temperature set identification number. (Integer >0)
GROUP_ID
Temperature group identification number (Integer >0 or =-1)
TID
Identification number of TABLEDi entry that gives F(t). (Integer >0)
Remarks:
1. SID is defined in Case Control file by TEMP(LOAD)=SID.
2. This entry is used in SOL 400 only when ANALYSIS=NLTRAN (nonlinear
transient analysis) and the temperature load is applied. It only applies to the
nonlinear elements in the Residual (SEID=0). There should be only one
temperature set for each STEP.
3. GROUP_ID determines the time-dependent distribution of temperatures. It
references to TMPSET Bulk Data entry to define all grid points, which
reference the same TABLEDi entry. Each grid point can have its own
GROUP_ID if it is necessary. GROUP_ID=-1 means all grid points are in one
group and reference to the same TTEMP Bulk Data entry.
4. TEMP(INIT) should not reference TTEMP and TMPSET.
CHAPTER 2
Nonlinear Analysis
TMPSET
Temperature Group Set Definition
Define a time-dependent dynamic thermal load group for use in TTEMP Bulk Data
entry.
Format:
1
TMPSET
2
3
4
5
6
7
8
9
ID
G1
G2
G3
G4
G5
G6
G7
G1
“THRU”
G2
“BY”
INC
10
Alternate Format:
TMPSET
ID
Example:
The Continuation Entry formats may be used more than once and in any order. They
may also be used with either format above.
Continuation Entry Format 1:
G8
G9
G10
G11
-etc.-
Continuation Entry Format 2:
G8
“THRU”
G9
“BY”
INC
15
5
THRU
21
BY
4
27
30
32
33
35
THRU
44
67
68
72
84
93
Example:
TMPSET
75
Field
Contents
ID
Temperature group identification number (Integer >0)
Gi
Grid point Identification numbers in the group (Integer >0)
65
66
Remarks:
1. This entry is used in SOL 400 only when ANALYSIS=NLTRAN (nonlinear
transient analysis) and the temperature load is applied. It only applies to the
nonlinear elements in the Residual (SEID=0).
2. GROUP_ID determines the group to a specified the time-dependent
distribution of temperatures. It is used by TTEMP Bulk Data entry to define
the corresponding TABLEDi entry. GROUP_ID must be unique for all the
other TMPSET entries.
3. TEMP(INIT) should not reference to TTEMP and TMPSET.
CHAPTER 2
Nonlinear Analysis
2.4
Correction in the Solution Algorithm for ElastoPlastic Material
The solution algorithm for Elasto-Plastic material in nonlinear analyses works best for
single-hardening-slope in MSC.Nastran 2004 and earlier versions. When there are
multiple-hardening-slopes, which defined on the TABLES1 Bulk Data entry as stressstrain curve, MSC.Nastran may produce some numerical error after loading
procedure processes into the 2nd and higher hardening slopes.
This numerical error is derived from the calculation of the scalar multiplier (a
Lagrange multiplier) dλ .
T
 ∂f 
-  [ D e ] { dε }
 ----- ∂σ 
dλ = -----------------------------------------------------------T
 ∂f 
 ∂f 
∗
H +  -------  [ D e ]  ------- 
∂σ


 ∂σ 
Eq. 2-1
where the gradient vector { ∂f ⁄ ∂σ } , is computed by differentiating the stress
function f ( σ ) representing effective stress. [ D e ] is the elasticity matrix, { dε } is the
strain increment and H∗ is the slope of hardening.
In Plasticity analysis, when a sub-increment along the stress-strain curve crossing two
hardening-slopes, for example H 1 and H 2 , the old solution algorithm will picks up one
of them, depending on the estimate stress increment, to be the value of H∗ . H∗ is
always equal to either H 1 or H 2 ; however, none of them can represent the “true”
hardening slope in this condition - that’s how the numerical error building-up. In
other word, the “true” value of H∗ must be the function of both H 1 and H 2 when it
goes through two hardening-slopes.
A new iterative algorithm is added in this release to compute the “true” value of H∗
based on the two hardening-slopes ( H 1 and H 2 ) it passed. Simply to say, we must find
H∗ based on the Eq. 2-1 and the following two equations:
H∗ dε
P
P
P
= H 1 dε 1 + H 2 dε 2
Eq. 2-2
and
dε
P
P
P
= dε 1 + dε 2
Eq. 2-3
where dεP is the total plastic strain increment in one sub-increment and dε P1 and dεP2
are the plastic strain increments corresponding to hardening-slope H 1 and H 2 .
67
68
An iterative method has been added to MSC.Nastran when computing Eq. 2-1 ,
Eq. 2-2 and Eq. 2-3 to obtain the best (or say converged) H∗ .
Note that even though MSC.Nastran 2005 can handle multiple-hardening-slope case
in Plasticity, it is still not recommended to loading too fast in nonlinear analyses. That
because if a sub-increment crossing three or more hardening slopes, the converged H∗
may be very hard to obtain.
Example
The following example shows the difference between Theoretical results,
MSC.Nastran 2004 results and MSC.Nastran 2005 results.
ID
PLASTICITY
SOL
400
DIAG
8
CEND
NLPAR
SET 1
SET 2
DISPL
STEP
1
LOAD
STEP
2
LOAD
STEP
3
LOAD
STEP
4
LOAD
STEP
5
LOAD
STEP
6
LOAD
STEP
7
LOAD
STEP
100
BEGIN BULK
GRID
11
GRID
12
CROD
1
PROD
101
MAT1
100
MATS1
100
TABLES1
+T
0.
+U
4.-5
$TABLES1
$+V
0.
FORCE
100
FORCE
200
FORCE
300
=
=
=
=
400
12 23 34
11 22 31
1
= 100
= 200
= 300
= 400
= 500
= 600
= 700
101
100
1.+7
101
101
0.
370.
102
0.
12
12
12
0.
0.
11
1.
0.
10.
12
123456
13456
.3
PLASTIC
100.
+T
1.-5
ENDT
100.
2.-5
195.
3.-5
1.-5
100.
100.
150.
195.
4.-5
370.
1.
1.
1.
ENDT
285.
+U
+V
CHAPTER 2
Nonlinear Analysis
FORCE
FORCE
FORCE
FORCE
NLPARM
+E
+B
0
ENDDATA
400
500
600
700
1.-6
12
12
12
12
400
1
1.-12
250.
285.
330.
370.
ITER
1.
1.
1.
1.
1
+E
+B
The displacement results at the tip of the ROD element are listed here
STEP
Theoretical
MSC.Nastran 2004
MSC.Nastran 2005
1
1.000000E-04
1.000000E-04
1.000000E-04
2
1.526316E-04
1.526316E-04
1.526316E-04
3
2.000000E-04
2.000000E-04
2.000000E-04
4
2.611111E-04
2.611111E-04
2.611111E-04
5
3.000000E-04
3.000000E-04
3.000000E-04
6
3.529412E-04
3.635294E-04
3.529412E-04
7
4.000000E-04
4.105882E-04
4.000000E-04
100
3.000000E-05
4.058823E-05
2.999997E-05
Note that in the loading procedure, from STEP1 to STEP 7, MSC.Nastran 2004 built
numerical error gradually but not in MSC.Nastran 2005 when comparing with the
theoretical results. The last STEP, STEP 100, is an unloading procedure,
MSC.Nastran 2005 can obtain the very close result as the theoretical one but
MSC.Nastran 2004 has about 35% error in the residual displacement.
69
70
2.5
Correction for the Nonlinear Element Strain Energy
By using the Case Control command, ESE, the user can ask NASTRAN job to compute
and output the element strain energy in all linear analyses for a long time. This
capability has been expanded to nonlinear elements in SOL 106 since
MSC.Nastran 2001 and to all nonlinear elements. The element strain energy of each
element was computed in the following way.
SE
i+1
i
= SE
0
i
i
0
i+1
0
1 i+1
+ ---  u
– u  F
+F 




2
Eq. 2-4
where SE represents the element strain energy of each element, u represents the
displacement vector, F represents the element force vector and i represents the load
increment. Note that i 0 represents the most recent output load increment, which
controlled by INTOUT in NLPARM Bulk Data entry and i 0 ≤ i . This formulation made
a limitation - the correct result can only be obtained when INTOUT=ALL, in other
words, i0 = i . Otherwise, the result is approximate when INTOUT=YES or NO and
i 0 ≤ i . Specially, it is very difficult to obtain a correct result when INTOUT=NO.
In order to remove the above limitation, the formulation of element strain energy has
been modified in MSC.Nastran 2005. It becomes
SE
i+1
i
i
i+1
i
1 i+1
= SE + --- ( u
– u )( F
+F )
2
Eq. 2-5
On the other hand, the element strain energy is not output-request-dependent
anymore in this release. No matter if INTOUT is set to ALL, YES or NO, the correct
element strain energy is calculated at the end of each loading case. By the way, the
capability of ESE, together with GPFORCE, has also been added into SOL 400 when
ANALYSIS=NLSTAT in MSC.Nastran 2005.
Example
The following example shows the difference of the element strain energy in
MSC.Nastran 2004 and MSC.Nastran 2005 when INTOUT=ALL or NO.
IN MSC, gpf001a $
SOL 106
TIME 10
DIAG 8, 15 $
CEND
TITLE=GPF001A - NONLINEAR GPFORCE TEST PROBLEM
SUBTI-HEXA ELEMENTS + AXIAL FORCES = NLM
LABEL=NONLINEARITY ANALYSIS - ITER
SPCF=ALL
CHAPTER 2
Nonlinear Analysis
DISPL=ALL
$STRESS(PRINT,PUNCH)=10
GPFORCE=ALL
ESE=ALL
SPC=100
NLPARM=1
SUBCASE 10
LOAD=100
SKIPON
SUBCASE 20
LOAD=200
SUBCASE 30
LOAD=300
SUBCASE 40
LOAD=400
SUBCASE 50
LOAD=500
BEGIN BULK
PARAM,GRDEQ,0
PARAM,LGDISP,-1
NLPARM,1,4,,ITER,1,10,,ALL
$NLPARM,1,4,,ITER,1,10,,NO
$
$ 8 NODE CHEXA MODEL
$
FORCE,100,5,,100000.0,1.0
FORCE,100,6,,100000.0,1.0
FORCE,100,7,,100000.0,1.0
FORCE,100,8,,100000.0,1.0
$
FORCE,200,5,,50000.0,1.0
FORCE,200,6,,50000.0,1.0
FORCE,200,7,,50000.0,1.0
FORCE,200,8,,50000.0,1.0
$
FORCE,300,5,,10000.0,1.0
FORCE,300,6,,10000.0,1.0
FORCE,300,7,,10000,1.0
FORCE,300,8,,10000.0,1.0
$
FORCE,400,5,,-10000.0,1.0
FORCE,400,6,,-10000.0,1.0
FORCE,400,7,,-10000.0,1.0
FORCE,400,8,,-10000.0,1.0
$
FORCE,500,5,,-100000.0,1.0
FORCE,500,6,,-100000.0,1.0
FORCE,500,7,,-100000.0,1.0
FORCE,500,8,,-100000.0,1.0
$
GRID 1
GRID 2
GRID 3
0.
0.
1.
1.
0.
1.
71
72
GRID 4
GRID 5
10.
GRID 6
10.
GRID 7
10.
GRID 8
10.
SPC1 100
123
1
CHEXA 1
8
1
+CHEX1
+CHEX1 7
8
$
$ COMMON DATA FOR EACH PROBLEM
$
PSOLID8
1
0
MAT1 1
3.+7
MATS1 1
PLASTIC
GRDSET
ENDDATA
1.
1.
1.
2
2
1.
1.
3
3
4
4
0.3
1.+7
1
1
56
3.+4
456
The results of element strain energy of the CHEXA element in the SUBCASE 100 are
listed here
MSC.Nastran 2004
INTOUT
MSC.Nastran 2005
ALL
NO
ALL
NO
8.583713E+04
2.175758E+04
8.583713E+04
8.583713E+04
MSC.Nastran 2005 Release Guide
CHAPTER
3
Numeric Enhancements
■ ACMS Now Available in the Matrix (DOF) Domain
■ Improvements for Geometric Domain Based ACMS
■ Improved Matrix Diagonal Diagnostics for 2x2 Pivots
(MAXRATIO)
■ Performance Improvement in Modal Frequency Response for
Large Frequency Ranges
74
ACMS Now Available in the Matrix (DOF) Domain
Previously, ACMS was available in the Geometric Domain. The initial domain
decomposition, which divides the model into smaller sub-models, took place on the
model geometry, on the set of grid points and their element connections. Now, ACMS
is also available in the DOF domain, which postpones the domain decomposition until
after all constraints have been eliminated, at the matrix level.
DOF Domain ACMS is invoked with the Executive level command
DOMAINSOLVER “PARTOPT” option:
DOMAINSOLVER
ACMS (PARTOPT=DOF)
The primary advantage of DOF Domain ACMS is performance, especially for models
whose complicated geometry presents problems to Geometric Domain ACMS.
Examples of such modeling include the following:
• Spot welds via manual modeling technique
• Spot welds via CWELD elements
• Acoustic coupling via rigid elements and MPCs
• Large numbers of rigid elements and/or MPCs for any purpose
The following chart shows an example of the performance gain for a model that uses
manual spot welding techniques.
Large model with manual spot welds
100
80
Elapsed Hours
3.1
96.7
60
40
17
20
9.9
7.3
DOF/2
DOF/4
0
Geometric/4
DOF/1
Domain/Processors
CHAPTER 3
Numeric Enhancements
DOF Domain ACMS performs at least as well as Geometric Domain ACMS for models
that do not feature these special characteristics, as shown in the following chart.
Large Typical NVH Model
12
Geometric Domain
10
Elapsed Hours
DOF Domain
8
6
4
2
0
1
2
4
No. of Processors
Other important features of DOF Domain ACMS include:
• A Component Modal Synthesis theory identical to that used in ACMS and in
all other MSC.Nastran CMS techniques.
• Residual vectors that are employed at every component at every level in
order to maximize the accuracy of the CMS.
• DMP (Distributed Memory Parallel) available up to eight processors,
providing excellent parallel speedup.
• Full compatibility with MSC.Nastran superelement techniques, including
External Superelements.
• Fully integrated with the SPCD method of enforced motion in SOL 111.
• Fully integrated with Acoustic Panel Participation in SOL 111 fluid-structure
interaction.
• Available in SOLs 103, 111, and 200.
• Available with external superelements
75
76
3.2
Improvements for Geometric Domain Based ACMS
Error corrections include the following:
• Improved robustness by correcting error related to free-floating (i.e.,
unconnected) scalar points.
• Fixed key errors in the ACMS interface with transient analysis and
MAXMIN data recovery.
• Fixed errors related to CWELD elements.
• Fixed key error related to parallel execution for acoustic models.
In addition, enhancements were made to make grid-based ACMS work with the new
External Superelement capability.
CHAPTER 3
Numeric Enhancements
3.3
Improved Matrix Diagonal Diagnostics for 2x2 Pivots
(MAXRATIO)
Matrix-to-factor diagonal ratios are a long-standing tool that help determine model
integrity in MSC.Nastran. With the increased use of Lagrange Multiplier Technique
(LMT) variables, 2-by-2 pivoting employed by the sparse direct solver in
MSC.Nastran has become more common. In the event of 2-by-2 pivoting, the matrixto-factor diagonal ratio was computed incorrectly prior to MSC.Nastran 2004 r3, with
the value of 1.0 used as the factor diagonal value for that DOF. If the stiffness value
was greater than maxratio, the DOF would fail the maxratio test. In these cases,
MAXRATIO calculations can produce misleading or erroneous output and the
analysis may terminate.
The MAXRATIO calculations have now been modified to take 2-by-2 pivoting into
account. Thus, when 2-by-2 pivoting occurs, maxratio calculations are not made on
the DOFs in the 2-by-2 pivot. If the maxratio vector is printed for this region it has an
artificial value of 1.0 for these DOFs, meaning that they will never be listed for
reasonable values of the MAXRATIO parameter. This produces MAXRATIO output,
which is more a true measure of the solution that has actually taken place inside the
sparse direct factorization.
For analyses such as inertia relief using the SUPORT entry selected by
PARAM,INREL,-2, or the new large displacement rigid elements, or for solid elements
using the interface spline elements, it should no longer be necessary to specify the
BAILOUT parameter. The BAILOUT parameter is not recommended for production
analysis, only for model debugging activities. It can mask models likely to produce
low quality results.
When comparing results with those from a prior version, you may see fewer high ratio
DOFs in the regions where 2-by-2 pivots are used. This is because the ratio messages
were invalid for these DOFs on prior versions.
77
78
3.4
Performance Improvement in Modal Frequency
Response for Large Frequency Ranges
Modal frequency response is a relatively inexpensive method for calculating response
quantities. For large problems with large frequency ranges and thousand of modes, it
may become very time consuming. A new technique for calculating frequency
response quantities is activated by the Bulk Data parameter, PARAM,FASTFR.
When PARAM,FASTFR,YES is specified, the alternative technique is used. For large
models with thousands of modes and a judicious use of structural damping, speedup
compared to the conventional FRRD1 module is of the order 10-to-1.
MSC.Nastran 2005 Release Guide+%ion
CHAPTER
4
Elements
■ Temperature-Dependent Composites Support Extended to
Unsymmetric Laminates
■ Global Ply Results Tracking
■ GPFORCE and ESE Output for DMIG and GENEL
■ Bar Element Torsional Mass Moment of Inertia
■ PARAM,COUPMASS Lumped Mass Option
■ QUADR Convergence Behavior
■ Arbitrary Beam Cross Section (Pre-Release)
80
4.1
Temperature-Dependent Composites Support
Extended to Unsymmetric Laminates
In MSC.Nastran 2004, laminated composites analysis was extended to include
temperature-dependent ply materials in SOL 106 Nonlinear Analysis. This approach
is based on updating the smeared laminate properties of symmetric laminates for the
nonlinear QUAD4 and TRIA3 elements. The temperature-dependency of the ply
materials was extended to include both orthotropic and anisotropic materials.
Furthermore, the more accurate integral strain method was added to complement the
default secant thermal strain method.
The symmetric laminate limitation in SOL 106 is now removed and
membrane-bending coupling effects due to unsymmetric laminates are included in
the nonlinear analysis.
Also, in this version, the temperature-dependent composites capability has been
extended to the nonlinear QUADR and TRIAR composite elements. A nonsmeared
approach is also available for the QUADR and TRIAR element types. This approach
is a more general approach in that the laminate properties are not smeared as in the
classical lamination theory, but evaluated during the element matrices calculation
using an integration by layer. The benefit of the nonsmeared approach is that it will
allow for future implementation of material nonlinear capabilities. Both the smeared
and nonsmeared approaches are valid for symmetric and unsymmetric laminates.
Non-uniform element grid point temperature and temperature gradient support by
the QUADR/TRIAR is another difference compared to the constant element
temperature QUAD4/TRIA3 element types.
Temperature-dependent QUAD4/TRIA3 composite models can be easily converted
to equivalent QUADR/TRIAR models by adding the NASTRAN QRMETH=5
command to the input file.
Note that the nonlinear QUADR/TRIAR element types are limited to
temperature-dependent composites. Additional nonlinear analysis capability for
these element types is planned for in future releases.
CHAPTER 4
Elements
The following table summarizes the user interfaces for invoking the
temperature-dependent composite capabilities for the composite element types:
Parameter
Value
QUAD4/TRIA3
QUADR/TRIAR
COMPMATT - Enable
update of
temperature-dependent
composite properties.
Yes/Smear
Supported
Supported
Nonsmear
Not Supported
Supported
No (default)
Supported
Supported
Secant (default)
Supported
Supported
Integral
Supported
Supported
EPSILONT - Select
Integral or Secant
thermal strain
calculation method
Example:
ASSIGN PUNCH=OUTDIR:'shcntr2p.n',NEW,UNIT=7
$ id msc, shcntrl2.dat $ v2005 9-Jun-2004 hdp
SOL 106
TIME 600
$ Direct Text Input for Executive Control
CEND
SEALL = ALL
SUPER = ALL
TITLE = shape control demo (n2)
ECHO = NONE
MAXLINES = 999999999
$ Direct Text Input for Global Case Control Data
TEMPERATURE(INITIAL) = 1
SUBCASE 1
$ Subcase name : Default
SUBTITLE=Default
NLPARM = 1
SPC = 2
TEMPERATURE(LOAD) = 3
DISPLACEMENT(SORT1,REAL,plot)=ALL
$ Direct Text Input for this Subcase
OUTPUT(XYOUT)
XYPUNCH DISP / 333(T3), 370(T3)
BEGIN BULK
PARAM
POST
-1
PARAM
COUPMASS 1
PARAM
LGDISP 1
PARAM
K6ROT
100.
PARAM,NOCOMPS,-1
PARAM
PRTMAXIM YES
PARAM,COMPMATT,YES
PARAM
NLTOL
0
NLPARM
1
10
ITER
1
100
YES
81
82
$ Direct Text Input for Bulk Data
$ Elements and Element Properties for region : smahcelem
$ Composite Property Record created from P3/PATRAN composite material
$ record : smahclam
$ Composite Material Description :
PCOMP
1
70.
0.
1
.0045
45.
YES
2
.0045
0.
YES
1
.0045 -45.
YES
1
.0045
90.
YES
1
.0045
90.
YES
1
.0045
45.
YES
2
.0045
0.
YES
1
.0045 -45.
YES
1
.0045
90.
YES
1
.0045
0.
YES
1
.0045
0.
YES
1
.0045
90.
YES
1
.0045 -45.
YES
1
.0045
45.
YES
1
.0045
90.
YES
1
.0045
90.
YES
1
.0045 -45.
YES
1
.0045
45.
YES
$ Pset: "smahcelem" will be imported as: "pcomp.1"
CQUAD4
73
1
75
76
113
112
CQUAD4
74
1
76
77
114
113
CQUAD4
75
1
77
78
115
114
CQUAD4
76
1
78
79
116
115
CQUAD4
77
1
79
80
117
116
CQUAD4
78
1
80
81
118
117
…
…
GRID
662
8.
3.
0.
GRID
663
8.25
3.
0.
GRID
664
8.5
3.
0.
GRID
665
8.75
3.
0.
GRID
666
9.
3.
0.
$ Loads for Load Case : Default
SPCADD
2
1
$ Displacement Constraints of Load Set : cfff
SPC1
1
123456 1
38
75
223
260
297
334
371
519
556
593
630
$ Default Initial Temperature
TEMPD
1
70.
3
250.
$ Referenced Coordinate Frames
ENDDATA
112
408
149
445
186
482
PARAM,COMPMATT,YES invokes the temperature dependent composite
capabilities for the composite QUAD4 elements in the model.
Absence of the EPSILONT parameter means that the default integral strain method of
updating the smeared laminate properties is selected for this analysis.
This example, with the associated bulk data include files, can be found in the Test
Problem Library – shcntrl2.dat, glepnast.dat, and nitnast.dat.
CHAPTER 4
Elements
4.2
Global Ply Results Tracking
Idealization of large composite panels requires that each ply within a panel be
accurately modeled with regard to stacking location and shape. When idealized in
MSC.Nastran, this creates situations where adjacent elements may not contain the
same number of plies, nor will these plies necessarily be continuous in terms of the
internal ply numbering scheme. Therefore, the interpretation of results is a laborious
task of manually identifying the consistent ply results when post-processing the
output.
To address this limitation, user specification of global ply IDs has been introduced for
easy reference of individual ply results across panels or sets of elements. A new
composite property entry called PCOMPG is available for the specification of global
ply IDs. The PCOMPG entry is an alternate property definition to the PCOMP entry.
The global ID for each ply is included in all ply result tables.
Optionally ply-layer results can be sorted by global ply ID for a given element SET for
easier results interpretation. A new Case Control command called GPRSORT is
introduced to reference an element SET. Results are sorted by element ID or by global
ply ID for a given element set.
This capability is available in all solution sequences that support composites except
Design Optimization (SOL 200).
The following example illustrates the use of the PCOMPG Bulk Data entry to define
global ply IDs.
The input file of this example, and others, can be found in the Test Problem Library –
pcompg*.dat.
Shown in Figure 4-1 is a laminated composite strip model with ply drop-off. A
complete listing of this model (TPL testdeck: pcompg1e.dat) shown in Listing 4-1,
illustrates specification of global ply IDs for each laminate on the PCOMPG entry.
Also ply results sorted by global ply IDs are requested using the new GPRSORT Case
Control command for element SET 100 (includes elements 100 and 200).
The standard ply results output is shown in Listing 4-2 with the global ply IDs
reported under the PLY ID label. Listing 4-3 shows the ply results sorted by global ply
IDs for the defined element SET 100.
83
84
8
7
6
5
4
1
8
5
4
3
2
1
Element 100
Element 200
Element 300
Figure 4-1 Laminated Composite Strip model with ply drop-offs
Listing 4-1 TPL testdeck pcompg1.dat
nastran system(361)=1
id msc, pcompg1e.dat $
time 60
sol 101
cend
title = Composite Strip with Global Ply IDs
disp =all
stress=all
set 100 = 100, 200
gprsort = 100
force=all
spcforces=all
spc=1
load=1000
begin bulk
param,k6rot,0.0
pcompg,1,,,5000.,hill,0.0,,,
,
1, 1, .0054, 45., yes
,
4, 1, .0054, 90., yes
,
5, 1, .0054, 90., yes
,
6, 1, .0054, 0.0, yes
,
7, 1, .0054,-45., yes
,
8, 1, .0054, 45., yes
pcompg,2,,,5000.,hill,0.0,,,
,
1, 1, .0054, 45., yes
,
3, 1, .0054, 0.0, yes
,
4, 1, .0054, 90., yes
,
5, 1, .0054, 90., yes
,
6, 1, .0054, 0.0, yes
,
8, 1, .0054, 45., yes
pcompg,3,,,5000.,hill,0.0,,,
CHAPTER 4
Elements
,
1, 1, .0054, 45., yes
,
2, 1, .0054,-45., yes
,
3, 1, .0054, 0.0, yes
,
4, 1, .0054, 90., yes
,
5, 1, .0054, 90., yes
,
8, 1, .0054, 45., yes
$
mat8,1,2.0e7,2.0e6,.35,1.0e6,1.0e6,1.0e6,0.0,+
+,0.0,0.0,0.0,2.3e5, 1.95e5, 13000., 32000., 12000.
cquad4,100,1,1,2,6,5
cquad4,200,2,2,3,7,6
cquad4,300,3,3,4,8,7
force,1, 4,,1.,0.0,0.0,-1.0
force,1, 8,,1.,0.0,0.0,-1.0
spc1,1,12345,1,5
load,1000,0.1,1.0,1
grid, 1,, 0.0,0.0,0.0,,6
grid, 2,, 1.0,0.0,0.0,,6
grid, 3,, 2.0,0.0,0.0,,6
grid, 4,, 3.0,0.0,0.0,,6
grid, 5,, 0.0,1.0,0.0,,6
grid, 6,, 1.0,1.0,0.0,,6
grid, 7,, 2.0,1.0,0.0,,6
grid, 8,, 3.0,1.0,0.0,,6
param,autospc,yes
param,post,-1
enddata
Listing 4-2 Ply Results Output for Each Element in the Model
S T R E S S E S
I N
L A Y E R E D
C O M P O S I T E
E L E M E N T S
( Q U A D
ELEMENT
PLY STRESSES IN FIBER AND MATRIX DIRECTIONS
INTER-LAMINAR STRESSES
ID
ID
NORMAL-1
NORMAL-2
SHEAR-12
SHEAR XZ-MAT SHEAR YZ-MAT
100
1 -2.84204E+03 -1.02828E+03 7.92127E+02
-6.67973E+00 -3.12898E-01
100
4 7.48335E+02 -8.80371E+02 -2.54907E+02
-7.95162E+00 -7.79520E-01
100
5 -7.55171E+01 -4.35131E+02 -1.69516E+02
-8.54160E+00 -7.97555E-01
100
6 3.89044E+02 -7.66743E+01 8.41258E+01
-7.62246E+00 -7.54499E-01
100
7 1.72768E+03 2.22906E+02 3.51962E+02
-4.97689E+00 -4.53933E-01
100
8 2.83923E+03 5.37783E+02 -6.37984E+02
-9.22442E-08 1.90999E-08
200
1 2.81691E+02 -2.90048E+02 3.28924E+02
-3.49256E+00 -3.51245E-01
200
3 -2.73870E+03 1.10669E+01 1.04747E+02
-9.62188E+00 -4.12887E-01
200
4 1.27601E+02 -8.43308E+01 -4.03806E+01
-9.82619E+00 -6.18361E-01
200
5 -7.30090E+02 7.11099E+01 2.39860E+01
-9.62188E+00 -4.12887E-01
200
6 2.79715E+03 -6.88072E+01 -8.83526E+01
-3.49256E+00 -3.51245E-01
200
8 -3.93539E+02 2.43778E+02 -3.62750E+02
3.93396E-16 -3.95636E-17
300
1 -4.06549E+02 -1.07470E+02 1.66640E+02
-4.97689E+00 -5.17350E-02
300
2 -3.15888E+02 -3.21002E+01 -9.81308E+01
-7.62246E+00 -8.59908E-02
300
3 -1.47324E+02 3.80228E+01 -1.87526E+01
-8.54160E+00 -9.08978E-02
300
4 1.74069E+02 9.78514E+01 4.22159E+01
-7.95162E+00 -8.88424E-02
300
5 -8.33154E+01 1.96665E+02 6.56791E+01
-6.67973E+00 -3.56612E-02
300
8 5.06968E+02 2.38382E+02 -1.75908E+02
9.22442E-08 -2.17683E-09
4 )
PRINCIPAL STRESSES (ZERO SHEAR)
ANGLE
MAJOR
MINOR
69.43 -7.31044E+02 -3.13928E+03
-8.69 7.87298E+02 -9.19334E+02
-21.66 -8.20804E+00 -5.02440E+02
9.93 4.03775E+02 -9.14045E+01
12.53 1.80594E+03 1.44653E+02
-14.50 3.00425E+03 3.72761E+02
24.50 4.31611E+02 -4.39967E+02
87.82 1.50513E+01 -2.74268E+03
-10.43 1.35034E+02 -9.17641E+01
88.29 7.18274E+01 -7.30808E+02
-1.76 2.79987E+03 -7.15284E+01
-65.65 4.07956E+02 -5.57717E+02
65.95 -3.31102E+01 -4.80909E+02
-72.67 -1.47298E+00 -3.46515E+02
-84.28 3.99010E+01 -1.49203E+02
23.96 1.92833E+02 7.90880E+01
77.43 2.11307E+02 -9.79570E+01
-26.32 5.93985E+02 1.51365E+02
MAX
SHEAR
1.20412E+03
8.53316E+02
2.47116E+02
2.47590E+02
8.30642E+02
1.31574E+03
4.35789E+02
1.37887E+03
1.13399E+02
4.01318E+02
1.43570E+03
4.82836E+02
2.23900E+02
1.72521E+02
9.45518E+01
5.68725E+01
1.54632E+02
2.21310E+02
85
86
Listing 4-3 Ply Results Sorted by Global Ply IDs
S T R E S S E S
I N
L A Y E
ELEMENT STRESSES IN FIBER AND MATRIX DIRECTIONS
ID
NORMAL-1
NORMAL-2
SHEAR-12
100 -2.84204E+03 -1.02828E+03 7.92127E+02
200 2.81691E+02 -2.90048E+02 3.28924E+02
3
200 -2.73870E+03 1.10669E+01 1.04747E+02
4
100 7.48335E+02 -8.80371E+02 -2.54907E+02
200 1.27601E+02 -8.43308E+01 -4.03806E+01
5
100 -7.55171E+01 -4.35131E+02 -1.69516E+02
200 -7.30090E+02 7.11099E+01 2.39860E+01
6
100 3.89044E+02 -7.66743E+01 8.41258E+01
200 2.79715E+03 -6.88072E+01 -8.83526E+01
7
100 1.72768E+03 2.22906E+02 3.51962E+02
8
100 2.83923E+03 5.37783E+02 -6.37984E+02
200 -3.93539E+02 2.43778E+02 -3.62750E+02
COMPOSITE STRIP WITH GLOBAL PLY IDS
TEST GPRSORT PROCESSING
GLOBAL
PLY ID
1
1
R E D
C O M P O S I T E
E L E M E N T S
INTER-LAMINAR STRESSES PRINCIPAL STRESSES (ZERO SHEAR)
MAX
SHEAR XZ-MAT SHEAR YZ-MAT ANGLE
MAJOR
MINOR
SHEAR
-6.67973E+00 -3.12898E-01
69.43 -7.31044E+02 -3.13928E+03 1.20412E+03
-3.49256E+00 -3.51245E-01
24.50 4.31611E+02 -4.39967E+02 4.35789E+02
-9.62188E+00 -4.12887E-01
87.82 1.50513E+01 -2.74268E+03 1.37887E+03
-7.95162E+00 -7.79520E-01
-8.69 7.87298E+02 -9.19334E+02 8.53316E+02
-9.82619E+00 -6.18361E-01 -10.43 1.35034E+02 -9.17641E+01 1.13399E+02
-8.54160E+00 -7.97555E-01 -21.66 -8.20804E+00 -5.02440E+02 2.47116E+02
-9.62188E+00 -4.12887E-01
88.29 7.18274E+01 -7.30808E+02 4.01318E+02
-7.62246E+00 -7.54499E-01
9.93 4.03775E+02 -9.14045E+01 2.47590E+02
-3.49256E+00 -3.51245E-01
-1.76 2.79987E+03 -7.15284E+01 1.43570E+03
-4.97689E+00 -4.53933E-01
12.53 1.80594E+03 1.44653E+02 8.30642E+02
-9.22442E-08 1.90999E-08 -14.50 3.00425E+03 3.72761E+02 1.31574E+03
3.93396E-16 -3.95636E-17 -65.65 4.07956E+02 -5.57717E+02 4.82836E+02
JULY 29, 2004 MSC.NASTRAN 7/23/04
PAGE
19
0
GLOBAL
PLY ID
1
F A I L U R E
FAILURE
ELEMENT
THEORY
ID
HILL
100
HILL
200
3
HILL
200
4
HILL
100
HILL
200
HILL
100
HILL
200
HILL
100
5
6
HILL
200
7
HILL
100
8
HILL
100
HILL
200
I N D I C E S
F O R
L A Y E R E D
C O M P O S I T E
FP=FAILURE INDEX FOR PLY
FB=FAILURE INDEX FOR BONDING
(DIRECT STRESSES/STRAINS)
(INTER-LAMINAR STRESSES)
0.0055
0.0013
0.0008
0.0007
0.0003
0.0019
0.0012
0.0016
0.0000
0.0020
0.0004
0.0017
0.0000
0.0019
0.0001
0.0015
0.0002
0.0007
0.0012
0.0010
0.0047
0.0013
E L E M E N T S
MAX OF FP,FB FOR ALL ELEMENTS
REFERENCED BY GLOBAL PLY
0.0055
0.0019
0.0020
0.0019
0.0015
0.0012
FLAG
CHAPTER 4
Elements
4.3
GPFORCE and ESE Output for DMIG and GENEL
The effects of the GENEL element and user-supplied DMIG matrices in linear statics
solution sequence (SOL 101) are now included in the Grid Point Force summations.
The GPFORCE output includes individual GENEL element identifications and DMIG
matrix names. Element strain energy for GENEL elements and DMIG matrices is also
calculated.
The existing Case Control commands, ESE for element strain energy and GPFORCE
for Grid Point Force, are used to request the output. Below is a sample F06 output
illustrating the inclusion of the DMIG contribution to the grid point force summation.
G R I D
0
0
0
POINT-ID
11
11
11
12
12
12
13
13
13
14
14
P O I N T
F O R C E
ELEMENT-ID
12
12
13
13
14
B A L A N C E
SOURCE
F-OF-SPC
K11X
*TOTALS*
QUAD4
K11X
*TOTALS*
QUAD4
QUAD4
*TOTALS*
QUAD4
QUAD4
T1
3.128563E+06
-3.128563E+06
0.0
-2.193838E+06
2.193838E+06
-9.313226E-10
9.914453E+05
-9.914453E+05
3.143214E-09
1.665495E+06
-1.665495E+06
T2
-9.800248E+05
9.800248E+05
-2.328306E-10
1.597768E+05
-1.597768E+05
4.074536E-10
-3.166309E+05
3.166309E+05
5.820766E-11
1.313788E+06
-1.313788E+06
T3
1.989233E+01
-1.989233E+01
-1.421085E-13
-1.398442E+01
1.398442E+01
-2.772893E-12
-5.283162E+00
5.283162E+00
2.898037E-11
-2.721329E+01
2.721329E+01
R1
4.673181E+03
-4.673181E+03
-3.637979E-12
-1.416497E+03
1.416497E+03
7.776180E-11
-6.762946E+02
6.762946E+02
-3.363994E-10
-1.409337E+03
1.409337E+03
R2
5.798827E+03
-5.798827E+03
-7.275958E-12
-9.718338E+03
9.718338E+03
3.037712E-10
6.893261E+03
-6.893261E+03
-1.509761E-10
4.590343E+03
-4.590343E+03
R3
-8.957655E+01
8.957655E+01
0.0
-1.905801E+00
1.905801E+00
-6.550316E-14
-6.008299E+01
6.008299E+01
-3.552714E-14
-2.426860E+01
2.426860E+01
Since the DMIG matrix names are defined by character names rather than by
enumerated values such as element identification, they currently cannot be
individually selected by SET selection of the ESE Case Control command. The
parameter, DMIGNRG is used to include the DMIG matrix energy to the Total Energy
calculation and provide individual matrix contribution information. The default of
DMIGNRG is NO. To include the DMIG contribution, the Bulk Data parameter,
DMIGNRG should be set to YES.
Example files ab1/2/3/4.dat can be found in the TPL.
87
88
4.4
Bar Element Torsional Mass Moment of Inertia
In prior versions of MSC.Nastran, the BAR element did not include the torsional mass
moment of inertia in the mass matrix. This led to different results when compared to
the BEAM element for an equivalent structure. This limitation is documented as
CSR7832.
The torsional mass moment of inertia can now be included in the BAR mass matrix by
using ‘NASTRAN SYSTEM(398)=1 or NASTRAN BARMASS=1’. Note that, by
default, this term will not be included. For both values of PARAM COUPMASS, this
term is added. If desired, the system cell default value can be changed via the
NASTRAN rc file.
The BAR torsional mass moment of inertia term for the component of rotation about
the element axis is calculated similar to the BEAM element using the following
equation:
I xx = ρL ( I 1 + I 2 )
where:
I xx = Torsional Mass Moment of Inertia
ρ = Density
L = Element of Length
I 1 and I 2 = Area Moments of Inertia
For COUPMASS=1, the axial mass will be consistent rather than coupled.
An example test file can be found in the TPL - brbm.dat.
CHAPTER 4
Elements
4.5
PARAM,COUPMASS Lumped Mass Option
The MSC.Nastran Quick Reference Guide documentation for PARAM,COUPMASS
suggests that its default value of –1 causes the generation of lumped mass matrices
that contain only translational components for the elements listed therein. Notable
exceptions to this are the CBAR and CBEAM elements, both of which will yield
rotational and coupling terms in order to preserve the mass center when element
offsets are defined. This offset mass is ‘lumped’ in the sense that it has low matrix
rank, and is ‘coupled’ in the sense that there are non-zero off diagonal terms in the
mass matrix. The CBEAM element will also yield a mass moment of inertia about the
local X axis of the element, and if system cell 398>0, then this is also true of the CBAR
element.
In order to yield a lumped mass matrix containing translational components only for
the CBAR and CBEAM elements, system cell 414 has been introduced. The default
value of this system cell (0) leaves the current behavior unchanged whereas a positive
integer value for system cell 414, along with the default value for
PARAM,COUPMASS (-1), will yield lumped mass matrices containing only
translational components for both CBAR and CBEAM elements.
Inputs
FMS SECTION
NASTRAN SYSTEM(414) = 1
BULK DATA
PARAM,COUPMASS,–1
Note: This parameter may optionally be specified in the Case Control Section.
Outputs
The resulting mass matrix for the BAR and BEAM element will only contain
translation terms. All off-diagonal and rotation terms will be zero.
Example:
The example file mass_bs.dat can be found in the Test Problem Library.
NASTRAN NLINES=99999
NASTRAN system(414) = 1
id msc, mass_bs.dat $ v2005 hdp 15-Jan-2004
$
89
90
SOL
101
DIAG 8
COMPILE SEMG $
ALTER 'ENDIF $ NOMGG>=0' $
MESSAGE//' MASS MATRIX' $
MATGPRBGPDTS,USET0,,MJJX//'G' $ MGG
EXIT $
CEND
TITLE = MASS MATRIX FOR BAR/BEAM ELEMENTS, COUPMASS = -1
BEGIN BULK
PBAR 101
100
.1
.01
.01
.02
10.
PBEAM 102
100
.1
.01
.01
.02
10.
MAT1 100
1.+7
.3
10.
PARAM COUPMASS-1
$
GRID 11
-1.
-.1
+.1
GRID 12
+1.
+.1
-.1
CBAR 1
101
11
12
1.
+A
+A
.1
.1
$
GRID 21
-1.
-.1
+.1
GRID 22
+1.
+.1
-.1
CBAR 2
101
21
22
1.
+B
+B
2356
$
GRID 31
-1.
-.1
+.1
GRID 32
+1.
+.1
-.1
CBEAM 3
102
31
32
1.
+C
+C
.1
.1
$
GRID 41
-1.
-.1
+.1
GRID 42
+1.
+.1
-.1
CBEAM 4
102
41
42
1.
+D
+D
2356
$
GRID 51
-1.
-.1
+.1
GRID 52
+1.
+.1
-.1
SPOINT53
54
CBEAM 5
102
51
52
1.
+E
+E
2356
+F
+F
53
54
ENDDATA
CHAPTER 4
Elements
The default mass matrix is shown:
0
POINT
MJJX
VALUE
POINT
COLUMN
11 T1
COLUMN
11 T2
COLUMN
11 T3
COLUMN
11 T3
COLUMNS
COLUMN
11 T1
COLUMN
12 T1
COLUMN
12 T2
COLUMN
12 T3
COLUMN
12 T3
1 (
1.11095E+01
2 (
1.11095E+01
3 (
1.11095E+01
4 (
1.11095E+00
5 (
6 (
-1.11095E+00
7 (
1.11095E+01
8 (
1.11095E+01
9 (
1.11095E+01
10 (
1.11095E+00
VALUE
POINT
VALUE
POINT
11-T1).
11 R3 -1.11095E+00
11-T2).
11-T3).
11 R1
11-R1).
11 R1
1.11095E+00
1.11095E-01
11-R2) THRU
5 (
11-R3).
11 R3 1.11095E-01
12-T1).
12 R3 -1.11095E+00
12-T2).
12-T3).
12 R1
12-R1).
12 R1
11-R2) ARE NULL.
1.11095E+00
1.11095E-01
With System Cell 414 set to 1, the mass matrix contains only diagonal terms:
0
POINT
MJJX
VALUE
POINT
COLUMN
11 T1
COLUMN
11 T2
COLUMN
11 T3
COLUMNS
COLUMN
12 T1
COLUMN
12 T2
COLUMN
12 T3
COLUMNS
VALUE
POINT
1 (
1.11095E+01
2 (
1.11095E+01
3 (
1.11095E+01
11-T1).
4 (
7 (
1.11095E+01
8 (
1.11095E+01
9 (
1.11095E+01
10 (
11-R1) THRU
12-T1).
VALUE
POINT
11-T2).
11-T3).
6 (
11-R3) ARE NULL.
12 (
12-R3) ARE NULL.
12-T2).
12-T3).
12-R1) THRU
91
92
4.6
QUADR Convergence Behavior
Introduction
A new QUADR element has been introduced in MSC.Nastran 2005 to provide more
accurate results for coarsely meshed regions where accuracy would tend to degrade.
In recent tests, the new QUADR element was compared to the QUAD4 element. The
results of the testing showed that the new QUADR element produced more accurate
results, even in regions that were coarsely meshed.
Benefits
Overall, an increase in accuracy can be expected when using the enhanced QUADR
element, and improvements in accuracy carry over to areas of the model that are more
coarsely meshed.
Existing QUAD4 element models can easily be converted to QUADR elements by
setting a single System Cell (QRMETH) in the NASTRAN Statement.
Inputs
System cell QRMETH=5 will convert all QUAD4/TRIA3 elements in the model to
QUADR/TRIAR.
Example
To demonstrate the difference in accuracy between the QUADR and QUAD4
elements, various mesh densities for a simple “T-Section” test model were run using
MSC.Nastran 2004 r3, comparing von Mises stress results taken in the central position
at Element 6, as shown.
CHAPTER 4
Elements
Four analysis runs were made using for element edge lengths (0.1, 0.05, 0.025, and
0.0125) to vary the number of elements (increasing the mesh density).
The four element stress contour plots, below, show a very similar stress distribution
for all four mesh densities; however, the actual stress values do vary slightly between
the plots.
93
94
The results for each of the four MSC.Nastran runs were tabulated and plotted to
compare the QUAD4 and QUADR elements.
CHAPTER 4
Elements
Quadr/Quad4 Comparison
450000
400000
350000
Von Mises Stress
300000
250000
MSC Q4
200000
MSC QR
150000
100000
50000
0
0
0.02
0.04
0.06
0.08
0.1
0.12
Mesh Density
It is evident that the MSC.Nastran QUADR element performs more consistently and
accurately for each of the four element mesh densities (coarse to fine) analyzed,
compared to the QUAD4 element that is less accurate for the models with larger
element edge lengths and fewer elements.
95
96
4.7
Arbitrary Beam Cross Section (Pre-Release)
Introduction
Beam elements have long been a staple in MSC.Nastran. Over the years, the capability
of beam element has grown steadily from constant cross section of PBAR to variable
cross section of PBEAM. However, users are required to compute the sectional
properties in order to utilize BAR and/or BEAM elements in the analysis. To alleviate
the amount of effort from engineers, PBARL and PBEAML were added for popular
cross sectional profiles. Nevertheless, engineers are still left to search for modeling
alternatives for 1-D structural components with arbitrary cross sectional shapes. A
new user interface for describing cross section shapes for CBAR and CBEAM element
types has been developed, and will be provided in the release of MSC.Nastran 2005 r2,
and is currently available for beta testing.
Development of this new capability in MSC.Nastran has been driven by the
automotive industry, keen to be able to easily represent the nonstandard beam
profiles commonly used in automotive design, and to use analysis tools to optimize
the profile designs themselves.
Subsequent development phases are planned, which will add more advanced features
to the Arbitrary Beam Section capability.
Benefits
The new user interface for describing cross section shapes of CBAR and CBEAM
element types will provide users with the ability to:
• More easily model 1-D structural components with arbitrary cross sectional
profiles using the MSC.Nastran BAR and/or BEAM element types for
analysis in linear solution sequences
• Design an optimal cross section profile in the Design Optimization solution
sequence, SOL 200 to optimize the overall model performance
This new capability, the Arbitrary Beam Section, will be delivered in the
MSC.Nastran 2005 r2, but is available for beta testing in MSC.Nastran 2005 r1.
Inputs and Outputs
Essentially, the shape of the beam cross section is defined using sets of POINTs as
defined on the SET1, or new SET3 Bulk Data entry (subsequent development phases
will allow section definition using geometric entities - GMCURV). These sets are then
referenced by new Bulk Data entries - PBRSECT for the BAR, PBMSECT for the BEAM
CHAPTER 4
Elements
- used to define the cross section form parameters, and reference material properties.
The types of section that can be defined include a General Section, Open Profile, and
Closed Profile, with various parameters required on the PBRSECT or PBMSECT
entries to define outer perimeter, inner perimeter, and branch segments where
applicable.
Currently for the BEAM element, only a constant cross section beam is supported.
Once all of the bulk data has been read in, equivalent BAR and BEAM elements are
created from the data supplied by the PBRSECT and PBMSECT entries. These
equivalent element definitions are printed out to the .f06 output file.
Guidelines
1. BRP for CP and OP must start or end branching from OUTP. BRP must not
start or end from another BRP.
2. BRP must not branch out from the end of OUTP. This rule covers both CP
and OP.
3. For CP and OP, a T = rs , where rs denotes a positive real single precision
number, must be present even if the thickness for every segment is
separately defined. This thickness will be used for all segments which do not
have specific thickness defined for them.
4. When PT=(id1,id2) is utilized to define the thickness of a segment, the id1
and id2 must be next to each other on the SET1 or SET3. A warning message
will be issued if this guideline is not observed.
For a design optimization analysis, the PBRSECT and PBMSECT entries are
referenced by the design variable property relation entries, DVPREL1. Dimensions
that can be taken into the design optimization analysis include:
• Overall Width - input W for PNAME field of DVPREL1. This is available for
GS, CP and OP. Overall width is computed as X1 max – X1 min . Both X1 max and
X1 min are collected by examining X1 of all POINT entries involved.
• Overall Height - input H for PNAME field of DVPREL1. Also available for
GS, CP and OP. Overall height is computed as X2 max – X2 min . Both X2 max and
X2 min are collected by examining X2 of all POINT entries involved.
• Segment Thickness - input T or T(id) for PNAME field of DVPREL1. This is
available only for CP and OP.
New PBRSECT, PBMSECT, and POINT entries are generated after each design cycle.
97
98
The stress recovery points, C, D, E, and F, are automatically selected by internal logic
that will pick POINTs with extreme coordinates, that is, closest to the four corners of
the rectangle defined by the overall width and height that encloses the cross section.
If a POINT is on a section defined as a design variable in a design optimization
analysis, then the POINT will move as the design variable changes. However, the
location of the POINT itself cannot be defined as a design variable.
Example: Z-Section Beam
2.0
4.0
2.0
Figure 4-2 Z-Section - Uniform Thickness of 0.1
The required bulk data entries to define the above section for linear analysis is as
follows:
1
2
3
4
5
POINT
1
0.0
0.0
POINT
2
2.0
0.0
POINT
3
2.0
3.9
POINT
4
3.9
3.9
POINT
5
3.9
4.0
POINT
6
1.9
4.0
POINT
7
1.9
0.1
6
7
8
9
10
CHAPTER 4
Elements
1
2
3
4
5
0.0
0.1
6
POINT
8
$SET3
SID
DES
ID1
ID2
ID3
SET3
10
POINT
1
THRU
8
7
8
9
10
where DES (description) can be POINT, GRID, or ELEMENT.
$PBRSECT
PID
MID
FORM
PBRSECT
1
1
GS
OUTP=10
where FORM can be: GS - General Section
OP - Open Profile
CP - Closed Profile
$PBMSECT
PID
MID
FORM
PBMSECT
2
1
GS
OUTP=10
PBMSECT,2 defines a constant section beam.
The z-section example showing the OP option with thickness definition is as follows:
1
2
3
4
5
POINT
11
0.0
0.05
POINT
12
1.95
0.05
POINT
13
1.95
3.95
POINT
14
3.9
3.95
SET3
20
POINT
11
THRU
PBRSECT
11
1
OP
OUTP=20, T=0.1, T(2)=[0.1, PT=(12,13)]
PBMSECT
12
1
OUTP=20, T=0.1
OP
6
14
7
8
9
10
99
100
Further examples are available in the Test Problem Library - zbr3.dat, zbr4.dat
zbr5.dat, zbm3.dat, zbm4.dat, zbm5.dat.
MSC.Nastran 2005 Release Guide
CHAPTER
5
Dynamic Analysis
■ C-Set Improvements
■ Enhancements to the MODESELECT Case Control Command
■ Automatic Q-Set (AUTOQSET)
■ Enhancements to Dynamic Excitation Processing in DPD Module
■ Enhancements to Transient Response Analysis
102
5.1
C-Set Improvements
When performing modal synthesis with free or mixed boundary conditions, the c-set
mass is usually included in the calculation of the component modes. A new
parameter, ZROCMAS, has been introduced to allow the c-set masses to be set to zero
when computing component modes. For the case where the component has large
masses on the c-set degrees of freedom, or when the user requests too many modes for
the component, the c-set residual flexibility will become singular, causing the
component reduction to fail. Setting the parameter ZROCMAS to YES will avoid this
condition by excluding the c-set masses when calculating the component modes.
CHAPTER 5
Dynamic Analysis
5.2
Enhancements to the MODESELECT Case Control
Command
The MODESELECT Case Control command, which was first made available in
MSC.Nastran 2004, has been greatly enhanced with the addition of several new
options. The enhanced command permits the user to specify ALL data related to
mode selection without the need for any parameters. The command, which can be
employed for selecting either structure modes or fluid modes, offers five different and
distinct options.
The details and usage of the enhanced command are clearly described in the
MSC.Nastran Quick Reference Guide. A short description of the various options
available with this command is listed below.
1. Mode selection based on arbitrary mode numbers
This option is the same as the one (and only one) that was available in
MSC.Nastran 2004.
2. Mode selection based on the number of lowest modes
This option is similar to the usage of the LMODES/LMODESFL parameter.
3. Mode selection based on range of mode numbers
This option can be regarded as a variation of options (1) and (2) above.
4. Mode selection based on frequency range
This option is similar to the usage of the LFREQ/LFREQFL and
HFREQ/HFREQFL parameters. However, this option is more general since
it also allows for the UNCONDITIONAL inclusion or exclusion of selected
modes regardless of their frequencies.
5. Mode selection based on modal effective mass fraction (MEFFMFRA) criteria
This powerful option is the highlight of the enhancement. It allows the user
to select modes based on different MEFFMFRA criteria. Further, like Option
(4) above, it also allows for the UNCONDITIONAL inclusion or exclusion of
selected modes regardless of their MEFFMFRA values.
There are several example problems included in the Test Problem Library that
illustrate the use of MODESELECT.
For SOL 111: kmfmodea/b/c/d/s.dat
For SOL 112: kmtmodea/b/c/d/s.dat
103
104
id msc, kmtmoded.dat
$ID TEST,MODESELECT $ TEST PROBLEM KMTMODED
$
SOL 112
TIME 30
CEND
TITLE = TEST PROBLEM KMTMODED - MODESELECT IN MODAL TRAN. RESP. ANALYSIS
SUBTITLE = TEST OF MODESELECT WITH THE MODAL EFF. MASS FRACTION OPTION
$
MODESELECT(T1FR T2FR=0.9 T3FR=0.8)
MODALSE(SORT1, PRINT, ESORT=ASCEND, THRESH=0.0, FREQ=ALL)= all
MODALKE(SORT2, PRINT, ESORT=DESCEND, THRESH=0.0, FREQ=ALL)= all
$
SUBCASE 1
disp(plot) = all
TSTEP= 100
DLOAD = 10
METHOD = 10
$
BEGIN BULK
$
$ DYNAMIC LOADING
$
freq1,5,1.,1.,20
tload2, 10, 10, , load, 0.0, 100.0, 10.0
$
tstep, 100, 200, .005, 20
$
DAREA,10,13,3,-1.
EIGRL,10,,1000.
$
$ BASIC MODEL DEFINITION
$
GRDSET,,,,,,,6
GRID,1,,-.4,0.,0.,,123456
GRID,3,,-.4,0.9,0.
=,*2,=,=,*.9,==
=1
...
...
$
$ ELEMENTS
$
CQUAD4,1,1,1,2,4,3
=,*1,=,*2,*2,*2,*2
=1
CQUAD4,4,1,7,8,14,13
CQUAD4,6,1,9,10,20,19
=,*1,=,*1,*1,*1,*1
=2
...
...
MAT1,1,30.+6,,.3,.283
PARAM,WTMASS,.00259
PSHELL,1,1,.05,1,,1
$
ENDDATA
CHAPTER 5
Dynamic Analysis
5.3
Automatic Q-Set (AUTOQSET)
Component modes (or dynamic reduction) are computed if the following items are
defined in the input file:
1. Mass is present
2. EIGR or EIGRL Bulk Data entry is requested by METHOD command (or
PARAM,METHCMRS)
3. Generalized coordinates (q-set degrees-of-freedom) are defined
The q-set DOFs are defined on QSETi entries (SEQSETi for superelements) and
associated SPOINT or GRID entries. It is the user’s responsibility to define a sufficient
number of q-set DOFs to capture all of the eigenvectors in the desired frequency range
defined on the EIGR or EIGRL entry and residual vectors. If too few q-set DOFs are
defined then modal truncation occurs and accuracy may suffer. If too many then the
dynamically reduced matrices will have null columns for the unused q-set DOFs and
may result in a performance degradation.
In MSC.Nastran 2005, the user may replace all q-set related Bulk Data entries with the
user parameter PARAM,AUTOQSET,YES. The number of component modes
computed is determined by the frequency range and/or number of desired
engenvectors specified on the selected EIGR or EIGRL Bulk Data entry.
Since the generalized coordinates are automatically defined, the following entries
may not be specified: QSETi, SEQSETi, SENQSET, or PARAM,NQSET. Also, those
GRID and/or SPOINT entries used to define the q-set may be left in the Bulk Data
section but it is recommended that they be removed.
In superelement analysis, the calculation of component modes is attempted on all
superelements including the residual structure. Also, all generalized coordinates for
all superelements will become interior to the residual structure and also assigned to
the q-set in the residual structure. In other words, component modes may not be
assigned interior to a superelement and they may not be removed (constrained).
This feature is currently not supported with:
1. Multiple boundary conditions
2. Design optimization (SOL 200)
3. Aerodynamic analyses (SOLs 144, 145, 146)
4. Cyclic symmetry analyses (SOLs 114, 115, 116, 118)
5. Restarts
105
106
Example
In the following example the user defines six q-set DOFs for natural frequencies up to
1200 cycles per unit time.
SOL 103
DIAG 8,15
CEND
TITLE= AUTOQSET DEMONSTRATION PROBLEM
SUBTITLE= TWENTY CELL BEAM
SPC=1002
METHOD=1
BEGIN BULK
EIGRL 1
1200.
QSET1
0
101
THRU
106
SPOINT 101
THRU
106
GRID
10000
0.0
0.0
=
*(1)
=
*(5.)
== $
=(19)
CBAR
101
100
10000
10001
=
*(1)
=
*(1)
*(1)
=(18)
PBAR
100
1000
0.31416 0.15708
MAT1
1000
3.+7
.3
SPC
1002
10020
3
ENDDATA
0.0
0.0
== $
1246
0.0
1.
1
7.764-4
10000
3
The results of the f06 show that six q-set are insufficient to capture the residual vectors
as shown by the messages below:
R E A L
MODE
NO.
1
2
3
4
5
6
7
E I G E N V A L U E S
EXTRACTION
ORDER
1
2
3
4
5
6
7
EIGENVALUE
1.881936E+04
3.011058E+05
1.524259E+06
4.816616E+06
1.175494E+07
2.435711E+07
4.506449E+07
(BEFORE AUGMENTATION OF RESIDUAL VECTORS)
RADIANS
CYCLES
1.371837E+02
5.487311E+02
1.234609E+03
2.194679E+03
3.428547E+03
4.935292E+03
6.713009E+03
2.183346E+01
8.733327E+01
1.964941E+02
3.492940E+02
5.456702E+02
7.854762E+02
1.068409E+03
GENERALIZED
MASS
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
GENERALIZED
STIFFNESS
1.881936E+04
3.011058E+05
1.524259E+06
4.816616E+06
1.175494E+07
2.435711E+07
4.506449E+07
^^^
^^^ USER
WARNING MESSAGE 9144 (SEMR4)
^^^ THERE ARE NO Q-SET DEGREES-OF-FREEDOM LEFT TO ACCOMMODATE ANY
RESIDUAL VECTORS.
^^^ USER INFORMATION:
NO RESIDUAL VECTORS WILL BE COMPUTED.
^^^ USER ACTION:
SPECIFY AT LEAST
6 MORE Q-SET DEGREES-OF-FREEDOM.
^^^
^^^
^^^ USER
WARNING MESSAGE 9145 ( RESLOAD )
^^^ THERE ARE NOT ENOUGH Q-SET DEGREES-OF-FREEDOM DEFINED TO
ACCOMMODATE ALL OF THE COMPUTED EIGENVECTORS AND/OR
RESIDUAL
VECTORS.
^^^ USER INFORMATION:
THE LAST
1 MODE(S) ABOVE WILL BE TRUNCATED.
^^^ USER ACTION:
SPECIFY AT LEAST
1 MORE Q-SET DEGREES-OF-FREEDOM.
CHAPTER 5
Dynamic Analysis
R E A L
MODE
NO.
1
2
3
4
5
6
^^^
^^^
^^^
^^^
E I G E N V A L U E S
EXTRACTION
ORDER
1
2
3
4
5
6
EIGENVALUE
1.881936E+04
3.011058E+05
1.524259E+06
4.816616E+06
1.175494E+07
2.435711E+07
(BEFORE AUGMENTATION OF RESIDUAL VECTORS)
RADIANS
CYCLES
1.371837E+02
5.487311E+02
1.234609E+03
2.194679E+03
3.428547E+03
4.935292E+03
2.183346E+01
8.733327E+01
1.964941E+02
3.492940E+02
5.456702E+02
7.854762E+02
GENERALIZED
MASS
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
GENERALIZED
STIFFNESS
1.881936E+04
3.011058E+05
1.524259E+06
4.816616E+06
1.175494E+07
2.435711E+07
USER
WARNING MESSAGE 9144 (SEMR4)
THERE ARE NO Q-SET DEGREES-OF-FREEDOM LEFT TO ACCOMMODATE ANY
RESIDUAL VECTORS.
USER INFORMATION:
NO RESIDUAL VECTORS WILL BE COMPUTED.
USER ACTION:
SPECIFY AT LEAST
6 MORE Q-SET DEGREES-OF-FREEDOM.
If we replace the QSETi and SPOINT entries with PARAM,AUTOQSET,YES:
SOL 103
DIAG 8,15
CEND
TITLE= AUTOQSET DEMONSTRATION PROBLEM
SUBTITLE= TWENTY CELL BEAM
SPC=1002
METHOD=1
BEGIN BULK
EIGRL 1
1200.
PARAM,AUTOQSET,YES
GRID
10000
0.0
0.0
=
*(1)
=
*(5.)
== $
=(19)
CBAR
101
100
10000
10001
=
*(1)
=
*(1)
*(1)
=(18)
PBAR
100
1000
0.31416 0.15708
MAT1
1000
3.+7
.3
SPC
1002
10020
3
ENDDATA
0.0
0.0
== $
1246
0.0
1.
1
7.764-4
10000
3
Then the results show that all of the eigenvectors and the residual vectors are now
computed.
R E A L
E I G E N V A L U E S
MODE
NO.
1
2
3
4
5
6
7
EXTRACTION
ORDER
1
2
3
4
5
6
7
EIGENVALUE
1.881936E+04
3.011058E+05
1.524259E+06
4.816616E+06
1.175494E+07
2.435711E+07
4.506449E+07
(BEFORE AUGMENTATION OF RESIDUAL VECTORS)
RADIANS
CYCLES
1.371837E+02
5.487311E+02
1.234609E+03
2.194679E+03
3.428547E+03
4.935292E+03
6.713009E+03
2.183346E+01
8.733327E+01
1.964941E+02
3.492940E+02
5.456702E+02
7.854762E+02
1.068409E+03
GENERALIZED
MASS
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
1.000000E+00
GENERALIZED
STIFFNESS
1.881936E+04
3.011058E+05
1.524259E+06
4.816616E+06
1.175494E+07
2.435711E+07
4.506449E+07
107
108
R E A L
MODE
NO.
1
2
3
4
5
6
7
8
9
E I G E N V A L U E S
EXTRACTION
ORDER
1
2
3
4
5
6
7
8
9
EIGENVALUE
1.881936E+04
3.011059E+05
1.524259E+06
4.816615E+06
1.175493E+07
2.435711E+07
4.506449E+07
9.003539E+07
1.442988E+08
(AFTER AUGMENTATION OF RESIDUAL VECTORS)
RADIANS
CYCLES
1.371837E+02
5.487311E+02
1.234609E+03
2.194679E+03
3.428547E+03
4.935292E+03
6.713009E+03
9.488698E+03
1.201244E+04
2.183346E+01
8.733327E+01
1.964941E+02
3.492940E+02
5.456702E+02
7.854761E+02
1.068409E+03
1.510173E+03
1.911840E+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
GENERALIZED
STIFFNESS
1.881936E+04
3.011059E+05
1.524259E+06
4.816615E+06
1.175493E+07
2.435711E+07
4.506449E+07
9.003539E+07
1.442988E+08
CHAPTER 5
Dynamic Analysis
5.4
Enhancements to Dynamic Excitation Processing in
DPD Module
The DPD module generates dynamic excitations (applied loads and enforced motion
information) for subsequent use in frequency response and transient response
calculations. Prior to MSC.Nastran 2005, these excitations were generated in single
precision and were stored in the Dynamic Loads Table (DLT). Starting with
MSC.Nastran 2005, these excitations are generated in machine precision. Further,
these excitations are no longer stored in the DLT, but are instead generated and held
as machine precision matrices.
There is another important enhancement in the DPD module. Depending upon the
time delays and phase angles specified, the columns of the excitation matrices are
segregated appropriately so that each column represents a dynamic excitation with its
own unique combination of time delay and phase angle. This scheme allows for the
residual vectors computed in modal dynamic analysis to be more meaningful and
more representative of the dynamic excitation employed in the analysis since it
accounts for the time delays and phase angles associated with the dynamic
excitations.
The enhancements mentioned above not only result in increased accuracy for
dynamic response calculations on double precision machines, but also facilitate more
efficient processing of these excitations in subsequent modules.
109
110
5.5
Enhancements to Transient Response Analysis
Increased Accuracy from TRLG Module
The TRLG module generates time dependent dynamic excitations (applied loads and
enforced motion data) for subsequent use in transient response calculations. Prior to
MSC.Nastran 2005, these excitations were generated in single precision. Starting with
MSC.Nastran 2005, these excitations are generated in machine precision, thereby
resulting in increased accuracy for transient response calculations on double precision
machines.
Improved Calculations for Enforced Motion in TRLG and
TRD1 Modules
The differentiation scheme employed in the TRLG module for enforced displacement
and enforced velocity applications in transient analysis has been improved in
MSC.Nastran 2005 by employing the same central finite difference scheme that is used
in the subsequent TRD1 module which performs the solution phase for linear
transient analysis (see Chapter 6 of the MSC.Nastran Basic Dynamic Analysis User’s
Guide). Appropriate enhancements have also been made to the TRD1 module to
account for these TRLG changes. These improvements impact enforced motion usage
in transient analysis not only for the SPC/SPCD approach, but also the large mass
approach. For the enforced displacement and enforced velocity applications in
transient analysis, this improved scheme yields much better correlation between the
results obtained from these two approaches than existed in earlier versions. It also
results in improved correlation with the corresponding results obtained from the
Lagrange multiplier technique (LMT).
Initial Condition Specification for Enforced Motion Usage
via SPC/SPCD
Enforced acceleration or enforced velocity usage in transient analysis via SPC/SPCD
specification requires integration to compute the corresponding enforced velocities
and/or displacements. This integration involves the use of initial conditions. Prior to
MSC.Nastran 2005, there was no way for the user to specify the initial conditions for
the enforced degrees of freedom (DOFs) in these cases. Starting with MSC.Nastran
2005, this facility is now available. With this feature, the user can specify initial
displacements for enforced DOFs in the case of enforced velocity usage via
SPC/SPCD and can specify initial displacements as well as initial velocities for
enforced DOFs in the case of enforced acceleration usage via SPC/SPCD. The initial
displacement and velocity values are specified via corresponding factors in two new
fields that have been added to the TLOAD1 and TLOAD2 Bulk Data entries. Details
CHAPTER 5
Dynamic Analysis
will be clear from the description of these expanded entries in the MSC.Nastran Quick
Reference Guide. This enhancement will greatly help users in performing enforced
motion studies with a variety of scenarios.
It should be noted here that the initial conditions for the enforced DOFs mentioned
here are distinct from, and may be used in conjunction with, the initial conditions for
independent DOFs that may be specified by a TIC Bulk Data entry.
111
112
MSC.Nastran 2005 Release Guide
CHAPTER
6
Optimization
■ Composite Ply Strength Ratio Response Type for the DRESP1
Entry
■ New FUNC(tions) for the DRESP2 Entry
■ Transformation of Approximate Optimization Task to a Feasible
Design
■ Residual Vectors Based on Adjoint Loads
■ Multiple Boundary Conditions for DFREQ/MFREQ in SOL 200
■ Benefits of Matrix Domain ACMS in SOL 200
■ ADS Optimizer
■ Topology Optimization - Beta Capability
■ BIGDOT Optimizer
114
6.1
Composite Ply Strength Ratio Response Type for the
DRESP1 Entry
Introduction
The CSTRAT response type has been added to the DRESP1 entry to support the
specification of composite ply strength ratios in a SOL 200 design task.
Benefits
Strength ratio output was provided as an additional available response in
MSC.Nastran 2004 (see Chapter 5.6 in the MSC.Nastran 2004 Release Guide). This is a
direct failure indicator and, as such, is an ideal response for the design of composites.
Input
The existing DRESP1 entry is used to identify the new CSTRAT response type. See the
MSC.Nastran Quick Reference Guide for a complete description of the DRESP1 entry.
The input requirements for the new CSTRAT response type are very similar to those
for the existing CFAILURE response type.
Outputs
Representative output produced for the CSTRAT response based on the P2 parameter
is shown in Figure 6-1 while Figure 6-2 shows representative formatted sensitivity
output for this response.
---------------------------------------------------------------------|
R E S P O N S E S
IN
D E S I G N
M O D E L
|
---------------------------------------------------------------------(N/A - BOUND NOT ACTIVE OR AVAILABLE)
I N I T I A L
-----
A N A L Y S I S
S U B C A S E =
COMPOSITE LAMINA STRESS RATIO RESPONSES
1
-----
------------------------------------------------------------------------------------------------------------INTERNAL
DRESP1
RESPONSE
ELEMENT COMPONENT
LAMINA
LOWER
UPPER
ID
ID
LABEL
ID
NO.
NO.
BOUND
VALUE
BOUND
------------------------------------------------------------------------------------------------------------1
3 FISUM
101
5
1
N/A
2.2166E-01
N/A
2
333 CFAILXX
101
5
2
1.0000E+00
2.2166E-01
N/A
Figure 6-1 Display of the CSTRAT Response Values
CHAPTER 6
Optimization
****************************************************************************
*
*
*
D E S I G N
S E N S I T I V I T Y
M A T R I X
O U T P U T
*
*
*
*
*
*
R E S P O N S E
S E N S I T I V I T Y
C O E F F I C I E N T S
*
*
*
****************************************************************************
-------------------------------------------------------------------------------------------------------------------------------DRESP1 ID=
3
RESPONSE TYPE= CSTRAT
ELEM ID=
101
COMP NO=
5
SEID=
0
SUBCASE RESP VALUE LAMINA NO. DESIGN VARIABLE COEFFICIENT
-------------------------------------------------------------------------------------------------------------------------------1 2.2166E-01
1
1 ORIENT
-1.7345E-02
-------------------------------------------------------------------------------------------------------------------------------DRESP1 ID=
333
RESPONSE TYPE= CSTRAT
ELEM ID=
101
COMP NO=
5
SEID=
0
SUBCASE RESP VALUE LAMINA NO. DESIGN VARIABLE COEFFICIENT
-------------------------------------------------------------------------------------------------------------------------------1 2.2166E-01
2
1 ORIENT
-1.7285E-03
Figure 6-2 Formatted Sensitivity Output for the CSTRAT Response Type
Guidelines and Limitations
• The SRCOMPS parameter, which the user must set to ‘YES’ to obtain printed
ply strength ratios, is not required for the CSTRAT response type.
• Only Item Codes 5 and 7 are available for this response.
Example (TPL: csrsens.dat)
Listing 6-1 shows a complete input file that demonstrates the new feature. Note the
first DRESP1 with the CSTRAT response type has left the ATTB field blank so that the
default first ply will be used for this response.
Listing 6-1 Input File with CSTRAT Response Type (csrsens.dat)
ID CSRSENS $
SOL 200 $
CEND
TITLE = TEST DRESP1 WITH RTYPE = CSTRAT
DSAPRT=(END=SENS)
DESOBJ = 3
DESSUB = 100
DISP=ALL
FORCE=ALL
STRESS=ALL
ANALYSIS = STATICS
LOAD=10
$
BEGIN BULK
CQUAD4 101
101
1
2
3
DESVAR 1
ORIENT 20.
-90.
90.0
$
ID
LABEL
RTYPE
PTYPE
REGION
DRESP1 3
FISUM
CSTRAT PCOMP
DRESP1 333
CFAILXX CSTRAT PCOMP
DCONSTR
100
333
1.0
1.01
4
0.
ATTA
5
5
ATTB
2
ATT1
101
101
115
116
DVPREL1 1
1
FORCE
10
FORCE
10
GRID
1
GRID
2
GRID
3
GRID
4
MAT8
1
PCOMP
-1.0
2
3
101
10.
0.
1.
1.
0.
1.
PCOMP
101
1
2.
-20.
DOPTPRM
P1
1
P2
14
-100.
70.
70.
0.
0.
1.
1.
.25
100.
1.+10
YES
1.
1.
1.25
100.
HILL
1
4.
1.
0.
2.
123456
6
6
16
20.
20.
1.
6.
-20.
YES
15
ENDDATA
The outputs of Figure 6-1 and Figure 6-2 were obtained from this example. Note that
the sensitivity indicates that the response in the second ply is a much weaker function
of this design variable than that of the response in the first ply.
CHAPTER 6
Optimization
6.2
New FUNC(tions) for the DRESP2 Entry
Introduction
The DRESP2 has been extended to provide two new functions that allow for the use
of the DRESP2 synthesis capability without invoking a DEQATN:
• The first new FUNC is BETA and it simplifies the input when the design task
is to minimize a maximum response value.
• The second FUNC is MATCH and this provides a simplified way to specify
a design task where one of the requirements is to match analysis results from
MSC.Nastran with a set of results that could come, for example, from a
structural test.
Benefits
The task of minimizing the maximum response has been found to be useful in a
number of applications, but particularly in NVH studies where the technique can be
used to minimize the peak response across a frequency range. This can be a tricky task
to implement and the new BETA function provides a convenient way of specifying
this design task.
Users frequently want to use SOL 200 of MSC.Nastran to obtain a better agreement
between analysis and test results. This can be a tedious process and benefits from
formulating the task in a way that may not be obvious to all users. The addition of the
MATCH function greatly simplifies the input preparation and could result in a better
agreement than would be obtained from the user’s input.
Theory
Minimizing the maximum response value is a technique that has proven valuable in
a number of applications and the new FUNC=BETA type on the DRESP2 entry merely
simplifies the data preparation for this case by creating the following design task:
Minimize:
F ( Xβ ) = C1 Xβ
Subject to:
r j – γX β
g = --------------------- ≤ 0
C3
117
118
where C 1 and C 3 are user input values that have default values of 100.and 10.0,
respectively. C 1 is used to scale the objective function and C 3 is used to offset the
constraint bound from 0.
The γ quantity is computed so that the maximum constraint for all the response is
equal to another user input value, C 2 :
g max = ( r jmax – γX β ) ⁄ C 3 = C 2
Where r jmax is the value of the maximum response for the initial design. The default
value for C 2 is 0.005, creating a maximum constraint that is just equal to the default
value of DOPTPRM parameter GMAX.
The matching of analysis results with user specified values is performed by
converting the user input data to one of two user specified formulations: a. Matching
Using Least Squares or b. Matching Using Minimization of the Maximum Deviation.
Matching Using Least Squares:
The least squares technique converts the user input into an objective function of the
following form:
m
φ =
∑
j = 1
 r – r T
j
j
 ---------------
T 
 rj 
2
where r j is a response from a DRESP1 and r Tj is a user defined target response.
There are no constraints spawned by this formulation but the user is permitted to
specified any other desired constraints in the standard fashion.
Matching Using Minimization of the Maximum Deviation:
The second formulation is a variation on minimization of the maximum response
technique described above. The objective is to minimize a spawned design variable:
F ( Xβ ) = C1 Xβ
Subject to:
T
( rj – rj )
– γX β ≤ ---------------------- ≤ γX β
T
rj
j = 1, 2, …m
CHAPTER 6
Optimization
Because X β can become small, it is necessary to offset the constraint in a fashion similar
to the BETA method given above:
Define:
T
rj – rj
R 2j = ----------------T
rj
And then determine R 2max and R 2min , the maximum and minimum values of R 2j .
The γ quantity can then be determined from user specified values of C 2 and C 3 using
the following equation.
Max ( R 2max, – R 2min ) – γX β
------------------------------------------------------------------------- = C 2
C3
Input
The new features use the existing DRESP2 entry with additional options provided for
the FUNC attribute. Additionally, the user can specify three constants that are used in
the two algorithms. All of these changes appear on the “parent” line of the DRESP2
entry, which now has the following form:
1
2
3
4
5
6
7
8
9
DRESP2
RID
Label
EQID/
FUNC
Region
Method
C1
C2
C3
10
The modified or added terms are in italics. There are two FUNC types:
FUNC= BETA indicates that the DRESP2 specifies a min-max problem and converts
the problem as shown in the “Theory” on page 117. This DRESP2 can only be invoked
by a DESOBJ case control entry. The continuations on the DRESP2 can only supply
DRESP1 data as shown in the examples section. The METHOD field in this case can
be MIN (default) or MAX (maximize the minimum response).
FUNC=MATCH indicates that the DRESP2 specifies a matching task as shown in the
Theory section above. The METHOD attribute can be either LS, indicating that the
least-squares method is to be utilized while METHOD = BETA indicates that the
minimization of the maximum normalized difference is to be performed. For
METHOD=BETA, the Ci coefficients can be input, again with defaults of 100., .005 and
10.0
119
120
Outputs
There are no added outputs produced by this enhancements with the exception that
the spawned design variable that is produced for FUNC=BETA or for
FUNC=MATCH with METHOD=BETA, will appear in the prints of design data. The
ID for the spawned design variable is the maximum number for the existing DESVAR
plus 1. Similarly, spawned responses will appear as normal responses. The ID for the
spawned DRESP2 starts from 100,000,001 and the response label is pre-defined as BBETA for FUNC=BETA and as LOW-BETA or UPP-BETA for FUNC=MATCH with
METHOD=BETA.
Guidelines and Limitations
• The new FUNC options on the DRESP2 can only be used on DRESP2’s that
are invoked by the DESOBJ entry.
• For FUNC=BETA, only DRESP1 data can be provided.
• For FUNC=MATCH, DTABLE data provides the target points for each of the
responses that is specified using a DRESP1. These data must be provided in
matching pairs.
• A target value of 0.0 is not recommended with FUNC=MATCH.
• Other constraints can be used in combination with the objective function
specified with the new DRESP2 functionality.
• If multiple DRESP1 responses are invoked with FUNC=BETA, each must be
a scalar quantity.
• If a single DRESP1 entry is invoked with FUNC=BETA, the assumption is
that this one DRESP1 generates multiple responses (e.g., displacements at a
series of frequencies or stresses for a number of elements).
Examples (dr2beta1, dr2mtch1 and dr2mtch2):
Three examples are provided with this delivery. The first is dr2beta1 and is similar to
the acoustic optimization task of “Acoustic Optimization” in Chapter 7 of the
MSC.Nastran Design Sensitivity and Optimization User’s Guide modified to utilize the
new BETA function on the DRESP2. The DRESP2 in this case has the form:
DRESP2
100
DRESP1
BETA
BETA
1
min
10000.
1.047
100.
CHAPTER 6
Optimization
Where C1=10000., C2=1.047 and C3=100. have been selected to produce an initial
design that is similar to that in the user’s guide. Note that the only user specified
constraint in this case is on the weight since the remaining constraints are spawned
from the DRESP2, as is the beta design variable.
The dr2mtch1 file is a simple eigenvector optimization task that seeks to minimize the
difference between three components of the first eigenvector while using a more
traditional constraint technique to force a match between measured and analytical
results for the third eigenvector. The original form of the design task was developed
as degvnt01.dat and is described in Chapter 2.1 of the MSC.Nastran 2004 Release Guide.
A fragment of the dr2mtch1 input file is provided to illustrate the use of the new
MATCH function:
DRESP2
500
DIFM1
DTABLE
DTABLE
LS
MATCH
TR1
TR2
DRESP1
511
512
513
TR1
1.432e-2
TR2
1.741e-1
TR3
TR3
6.381e-1
SOL 200 easily solves this oversimplified design task.
The dr2mtch2 file is for the same design task except that now the beta method is
applied to assist in the match.
121
122
6.3
Transformation of Approximate Optimization Task to
a Feasible Design
Introduction
A parameter has been added to the DOPTPRM entry that transforms an infeasible
optimization task to a feasible one.
Benefits
A general statement can be made that optimization algorithms perform best when the
design task does not include violated constraints. In fact, some algorithms will fail if
a feasible design does not exist (the algorithms used in MSC.Nastran search for the
best compromise infeasible design so that the transformation to a feasible design is not
a strict requirement). In order to facilitate the use of a general optimization
procedure, such as the ADS code which has been installed in MSC.Nastran 2005, a
simple transformation technique has been developed to ensure that the optimization
task always works in the feasible domain.
Theory
The standard optimization task minimizes an objective subject to satisfying a set of
constraints. The transformed problem, designated the β Method, involves creating a
β design variable that modifies the constraints so that:
gj ′ = gj – β
( j = 1, 2, …ncon )
and the transforms the objective function so that:
Φ′ = Φ + β∗ PENAL∗ Φ 0
where PENAL is the user defined penalty parameter, Φ 0 is the initial objective
function and β is initialized to the maximum initial constraint value. (If this maximum
value is less than CTMIN, the transformation is not applied.) In this way, the
maximum constraint value is never positive while the penalty on the objective acts to
force the β value to zero. If there is a feasible design, this technique should lead to it.
If there is not, this will result in a compromise design where the maximum constraint
violation is minimized.
CHAPTER 6
Optimization
Input
The only user input is the PENAL parameter that can be input on the DOPTPRM
entry. A suggested value for this parameter is 2.0, with larger values serving to move
the design more forcefully toward the feasible design space. Experience to date shows
that a value of 2.0 works well.
Outputs
This transformation is only applied during the approximate optimization and is
therefore not evident in standard reporting of the optimization results (i.e, the results
produced with DOPTPRM parameters P1 and P2, sensitivity prints and the summary
DESIGN HISTORY information). The prints produced when DOPTPRM IPRINT is
used to display the approximate optimization results do include this transformation,
so the user must be aware of this extra, final design variable, the transformed objective
and constraint values, and the effects this has on the sensitivities.
Guidelines and Limitations
• The method does not apply when the design task given the optimizer is
feasible.
• Setting PENAL=2.0 seems to work well, but users are free to experiment with
their application.
• PENAL must be a positive real number (0.0 is valid, but has no effect).
Example (TPL: mmfdpen.dat)
TPL file mmfdpen shows the use of the PENAL parameter in conjunction with the
DOT algorithm for the Modified Method of Feasible Directions. The file is the existing
mmfd.dat TPL file with the DOPTPRM entry modified to:
1
2
3
4
5
6
7
8
9
DOPTPRM
P1
1
p2
15
DELP
0.5
DESMAX
30
PENAL
10.
10
123
124
Even though the DOT algorithm that is used for mmfdpen and mmfd contains
strategies to deal with initially infeasible designs, the use of the PENAL parameter
showed a reduction in the number of design cycles and a slight (insignificant)
improvement in the final design as shown in Table 6-1.
Table 6-1
File Name
Final Objective
Number of Design
Cycles
mmfd
6.536e4
11
mmfdpen
6.529e4
8
CHAPTER 6
Optimization
6.4
Residual Vectors Based on Adjoint Loads
Introduction
A new RESVEC option has been introduced that creates residual vectors for use in a
modal frequency response analysis that are based on adjoint load vectors which are,
in turn, are created from user input DRESP1 entries that have RTYPE’s that are
associated with grid responses in a frequency response subcase (i.e, FRDISP, FRVELO
or FRACCL).
Benefits
Residual vectors became the default in MSC.Nastran 2004 and often show dramatic
improvements in dynamic response analyses. This benefits SOL 200, and the new
RESVEC option creates residual vectors that are ideal for obtaining accurate
sensitivity values in modal frequency response sensitivity analysis.
Input
No new input is required for this new feature, but optional describers have been
added to the RESVEC Case Control command:
ADJLOD/NOADJLOD – Control calculation of residual vectors based on adjoint
loads in a modal frequency response sensitivity analysis. (Default=ADJLOD)
See the MSC.Nastran Quick Reference Guide for a complete description of the
RESVEC Case Control command.
Outputs
There are no new outputs.
Guidelines and Limitations
• Residual vectors from adjoint loads are only applicable in SOL 200 when
ANALYSIS=MFREQ.
• If there are FREQ3,4 or 5 entries to specify excitation frequencies, the residual
vectors based on adjoint loads will not be computed automatically. In this
case, the user can generate these residual vectors by using the RVDOF or
RVDOF1 entry with grid and components the same as those entered on the
DRESP1 entry.
125
126
Example (rvadjsens.dat)
A structural model that represents a sensor on a missile is shown below. The objective
is to minimize the jitter at the sensor location so that accurate sensitivities are of
benefit. The example was exercised in three different runs:
1. Using ANALYSIS=DFREQ
2. Using ANALYSIS=MFREQ with 9 normal modes and 4 residual modes
available in MSC.Nastran 2004 (these modes are produced from three inertia
loads and one applied load.
3. Same as 2, except an additional residual vector is created based on the
DRESP1 at the sensor location.
Figure 6-3 Visual Sensor Model
Figure 6-4 shows the percent error in the sensitivity results across a range of
frequencies, where the error is computed as the difference in the modal frequency
response compared to the direct frequency response normalized by the direct
frequency response. It is seen that the single additional residual vector has a
pronounced effect in reducing the error.
CHAPTER 6
Optimization
SENSITIVITY ERROR
40.00%
20.00%
0.00%
Percent Error
60
65
70
75
80
85
90
95
-20.00%
-40.00%
-60.00%
No Residual from Adjoint
-80.00%
Residual from Adjoint
-100.00%
-120.00%
Frequency (Hz.)
Figure 6-4
100
127
128
6.5
Multiple Boundary Conditions for DFREQ/MFREQ in
SOL 200
SOL 200 has been capable of supporting multiple boundary conditions (MBC) for
statics, normal modes, buckling and aeroelasticity for some time. However, dynamic
frequency response analysis of structures subjected to multiple loads under different boundary
conditions (SPC,MPC and/or SUPORT) has not been supported in SOL 200 until recently.
With MSC.Nastran 2004 r3, SOL 200 is capable of performing sensitivity and
optimization calculations for DFREQ and MFREQ with multiple boundary
conditions.
Theory
The multiple boundary conditions for ANALYSIS = MFREQ or DFREQ in SOL 200 are
implemented with the addition of a boundary condition loop in the DMAP level. Each
pass of the new DMAP loop for a boundary condition has identical theoretical
background.
Input/Output
The MBC for MFREQ and DFREQ in SOL 200 is implemented with no new user
interface requirement. An input file can be prepared by merging several previous
SOL 200 DFREQ (or MFREQ) for the same structures that have different boundary
conditions or simply adding DSO related entries to a SOL 108 (or 111) file that has
multiple boundary conditions.
Examples (TPL: mbc01.dat, mbc02.dat, mbc03.dat)
All three test files have analysis type of MFREQ. Portions of mbc01 will be utilized for
this discussion. The subcase structure of mbc01 is shown.
SUBCASE =
1
ANALYSIS = MFREQ
LABEL =SPC Force
SPC =
100
DESSUB =
1
FREQUENCY =
SUBCASE =
2
DESOBJ(MIN)=1
$
ANALYSIS = MFREQ
LABEL =SPC Force
SPC =
200
FREQUENCY =
502
501
CHAPTER 6
Optimization
Note that the response for design objective is selected from the second subcase while
responses for design constraints are from SUBCASE 1. This arrangement is only for
demonstration purposes. DESOBJ with a global response, such as WEIGHT, can
appear either above the SUBCASE level or in the first SUBCASE. The output for an
MFREQ or DFREQ SOL 200 job with MBC is identical to those with a single boundary
condition. Hence, the output example is not shown here.
Guidelines and Limitations
• The SPC, MPC and SUPORT conditions are used to determine whether a
new boundary condition has been encountered.
• DFREQ and MFREQ subcases cannot be mixed
• The restriction on a single modal transient subcase remains.
129
130
Benefits of Matrix Domain ACMS in SOL 200
Matrix Domain Automated Component Mode Syntheses (MDACMS) is the latest
Lanczos solver introduced in MSC.Nastran 2005. You can find a detailed discussion in
“ACMS Now Available in the Matrix (DOF) Domain” on page 74. You can use this
new feature in a SOL 200 run by specifying the DOMAINSOLVER ACMS
(partopt=dof) command. It is available for Analysis=MODES and/or =MFREQ and
both serial and parallel processing are supported. A parallel run is activated when
DMP = n and n > 1.
This new feature has been tested with an NVH optimization task with a 4.2M dofs, for
an eigenanalysis up to 300 Hz that produced 1960 modes. Three separate runs were
performed. The following plot shows that a parallel (4 processor) MDACMS SOL 200
job achieves more than 6 times speedup relative to a Geometric Domain ACMS
(GDACMS) SOL 200 run (reduced time from 37 Hrs to 6 Hrs) while the serial
MDACMS SOL 200 run reduces to 14 Hrs for a 2.5 times speedup.
MDACMS vs. GDACMS in SOL200
40
35
Elapsed Time (Hour)
6.6
30
25
20
15
37
32
10
14
5
14
6
0
GDACMS
One Design Cycle
MDACMS(S)
5
MDACMS(P)
One FE Analysis
CHAPTER 6
Optimization
6.7
ADS Optimizer
Introduction
ADS is a public domain FORTRAN program for Automated Design Synthesis
developed by G.N. Vanderplaats in 1985 and is documented in Vanderplaats, G.N.,
ADS – A FORTRAN Program for Automated Design Synthesis – Version 1.10,
NASA Contractor Report 177985, NASA Langley Research Center, Hampton,
Virginia, 1985.
In MSC.Nastran 2005, an MSC.Software enhanced ADS version is added to support
SOL 200.
Benefits
The availability of the ADS optimizer provides an alternative to the existing optimizer
options that are provided in the DOT optimizer that has been the workhorse
optimization algorithm for many years. As indicated below, the ADS code is a suite
of optimization techniques and it may be that a particular optimization task will
achieve improved results when using one of the ADS techniques. Notably, ADS
contains SUMT (Sequential Unconstrained Minimization Techniques) methods that
are not available with DOT. Users who have had experience in the use of the public
domain ADS code should welcome having these algorithms available in
MSC.Nastran. The ADS optimizer will use your current optimization license, and
does not require any special licensing.
Input
There are two ways to use ADS code. One way is by modifying an executive system
parameter OPTCOD in the Runtime Configuration (RC) file as shown in Table 6-2
Table 6-2 System Cell Summary
System Cell
Number
System
Name
413
OPTCOD
Function and Reference
Specifies which optimization code to be used
in SOL 200. Optimization method is selected
by parameter METHOD on DOPTPRM entry
0 (default) – DOT (Design Optimization Tool)
1 – Enhanced ADS code
131
132
The second way is that MSC.Nastran allows users to select an ADS optimization
algorithm is by a new parameter ADSCOD added to DOPTPRM Bulk Data entry that
has the options shown in Table 6-3
Table 6-3 DOPTPRM Design Optimization Parameters
Name
ADSCOD
Description, Type and Default Value
Optimization Code: (Integer > 0, Default = 0, see Remark 1)
=0
DOT used
=1
ADS Modified Method of Feasible Directions
=2
ADS Sequential Linear Programming
=3
ADS Sequential Quadratic Programming
=4
SUMT Method
= IJK
where
I -ADS strategy options (Integer 0-9 Default = 0 see Remark 2)
0
None, Go directly to the optimizer
1
Sequential unconstrained minimization using the exterior
penalty function method
2
Sequential unconstrained minimization using the linear
extended interior penalty function method
3
Sequential unconstrained minimization using the quadratic
extended interior penalty function method
4
Sequential unconstrained minimization using the cubic
extended interior penalty function method
5
Augmented Lagrange multiplier method
6
Sequential linear programming
7
Method of centers
8
Sequential quadratic programming
9
Sequential convex programming
J - ADS optimizer options (Integer 1-5)
1
Fletcher-Reeves algorithm for unconstrained minimization
2
Davidon-Fletcher-Powell (DFP) variable metric method for
unconstrained minimization
CHAPTER 6
Optimization
Table 6-3 DOPTPRM Design Optimization Parameters
Name
Description, Type and Default Value
3
Broydon-Fletcher-Goldfarb-Shanno (BFGS) variable metric
method for unconstrained minimization
4
Method of feasible directions for constrained minimization
5
Modified method of feasible directions for constrained
minimization
K - ADS one-dimensional search options (integer 1-8)
1
Find the minimum of an unconstrained function using the
Golden Section method
2
Find the minimum of an unconstrained function using the
Golden Section method followed by polynomial interpolation
3
Find the minimum of an unconstrained function by first
finding bounds and then using polynomial interpolation
4
Find the minimum of an unconstrained function by
polynomial interpolation/extrapolation without first finding
bounds on the solution
5
Find the minimum of a constrained function using the Golden
Section method
6
Find the minimum of a constrained function using the Golden
Section method followed by polynomial interpolation
7
Find the minimum of a constrained function by first finding
bounds and then using polynomial interpolation
8
Find the minimum of a constrained function by polynomial
interpolation/extrapolation without first finding bounds on
the solution
Remarks:
1.
If ADSCOD>0, ADSCOD will override the METHOD.
2. A more complete description of the available options can be found in the
Reference cited in the introduction of this section.
133
134
Output
The outputs used with the ADS code are identical, in terms of format, to those using
the DOT code with the exception of the prints produced using the DOPTPRM IPRINT
parameter. The IPRINT output from ADS will differ for each option but all IPRINT
results are headed by a banner the identifies the results as coming from the
MSC.Software enhanced version of ADS.
Guidelines and Limitations
The ADS code has been provided in response to client requests for an alternative
optimization algorithm to the DOT code. MSC.Software has performed extensive
testing of using ADS on our suite of over 400 test problems. The basic conclusion from
these tests is that the ADS code performs adequately on many of these tests, but that
there is no compelling case to recommend the use of ADS on a general basis. It is
recommended that knowledgeable users apply ADS to some of their difficult
optimization tasks and see if they can obtain improved results. In particular, ADS
SUMT methods can comfortably solve problems with a few thousand design
variables. MSC.Software would be interested in hearing of any experience along these
lines.
One guideline is that while the DOT code has techniques for dealing with infeasible
designs, ADS is weak in this area. In this case, it is recommended that the new PENAL
parameter on the DOPTPRM entry be used to transform the optimization task from an
infeasible to a feasible one.
CHAPTER 6
Optimization
6.8
Topology Optimization - Beta Capability
Introduction
Unlike sizing and shape optimization, topology optimization finds an optimal
distribution of material, given the package space, loads, and boundary conditions.
These methods have grown rapidly in popularity and application in recent years and
topology optimization methods have been discussed in a large number of
publications. An overview of topology optimization can be found in a book by
Bendsoe and Sigmund [1] and a review article by Rozvany et al [2].
MSC.Software has integrated a topology optimization capability into
MSC.Nastran 2005 that is based on the increasingly popular density approach to
topology optimization. In the density method, Young’s modulus E and density ρ are
used as intermediate design variables for each designable finite element. The actual
design variable x is the normalized density that links Young’s modulus E and density
ρ for designable finite elements using the following relationships
ρ = ρ0 x
E = E0 x
p
where ρ 0 and E 0 are respectively the fully solid Young’s modulus and density. A
penalty factor p is introduced to enforce the design variable to be close to a 0-1
solution when p>1.0. The penalty factor p usually takes values between 2 and 4.
The general topology optimization problem available in MSC.Nastran can be stated as
follows:
Minimize:
f ( xi )
Subject to:
g j ( x i ) ≤ 0.0
η ≤ x i ≤ 1.0
j = 1, …, M
i = 1, 2, …, N
where g j represents the j-th constraints and M is the total number of constraints. The
constraint specification can be general in that any of the response types currently
available in SOL 200 can be used. N is the total number of designable elements. η is a
small positive number to prevent the stiffness matrix singularity.
135
136
Benefits
Topology optimization can generate more efficient design concepts in the early design
stage, especially for load paths. Topology optimization can also be to used to obtain
rib patterns and weld distribution patterns. The BIGDOT optimizer is available to
solve problems with a large number of design variables and constraints that DOT
struggles with due to computer memory requirements and efficiency.
Input
Topology optimization in MSC.Nastran borrows heavily from the user interface
developed for sizing and shape optimization. In particular, the design objective and
constraints are defined in an identical manner for topology and sizing/shape
optimization. This section discusses the additional bulk data entry that has been
provided to ease the creation of the design variables and then discusses other features
that have been adapted for topology optimization
TOPVAR – Topological Design Variables
To select a topologically designable region, the user needs to specify a group of
elements. All elements referencing a given property ID are made topologically
designable with the Bulk Data entry TOPVAR. Topology design variables are
automatically generated with one design variable per designable element.
The basic format for TOPVAR is:
1
2
3
4
5
6
7
8
9
TOPVAR
ID
LABEL
PTYPE
XINIT
XLB
DELXV
POWER
PID
10
Field
Contents
ID
Unique topology design region identification number. (Integer>0)
LABEL
User-supplied name for printing purpose. (Character)
PTYPE
Property entry name. Used with PID to identify the elements to be
designed. (Character: “PBAR”, “PSHELL”, etc.)
XINIT
Initial value. (Real, XLB<=XINIT). Typically, XINIT is defined to match
the mass target constraint, so the initial design does not have violated
constraints. For example, if the mass target is 30%, then it is suggested
XINIT=0.3.
XLB
Lower bound. (Real, Default = 0.001)
CHAPTER 6
Optimization
Field
Contents
XLB
Upper bound (real, Default = 1.0)
DELXV
Fractional change allowed for the design variable during approximate
optimization. (Real > 0.0, default = 0.2 see Remark 3).
POWER
A penalty factor used in relation between topology design variables and
element Young’s modulus. (Real > 1.0, default =3.0). 2.0<=POWER<=4.0
is suggested.
PID
Property entry identifier (Integer > 0)
Remarks:
1. The topologically designable element property includes PROD, PBAR,
PBARL, PBEND, PBEAM, PBEAML, PSHELL, PSHEAR, PSOLID, and
PWELD. Multiple TOPVARs are allowed to design different element types
in a single file.
2. All designed element properties must refer to a MAT1 entry; therefore, a
PCOMP cannot be used in topology optimization.
3. If DELXV is bank, the default is taken from the specification of DELX
parameter on the DOPTPRM entry.
New Responses - Compliance and Fractional Mass
The existing DRESP1 entry has been extended to provide two new response types that
are available exclusively for topology optimization. The format for the new responses
is shown in Table 6-4 and it is seen that both new response types require only the
specification of the response type and no other attributes.
Table 6-4 New Responses for Topology Optimization
Response Type
(RTYPE)
Response Attributes
ATTA
(Integer>0)
ATTB (Integer>0 or
Real>0.0)
ATTI (Integer>0)
COMP Remark 1
BLANK
BLANK
BLANK
FRMASS
Remark 1,2
BLANK
BLANK
BLANK
137
138
Remarks:
1. RTYPE=COMP (compliance of structures = p T u ) and FRMASS (mass fraction
of designed elements) entries are used for topology optimization only.
2. RTYPE=FRMASS is the mass divided by the mass calculated if all design
variables are 1.0. FRMASS is calculated for designed elements only. FRMASS
= 1.0 if all design variables are 1.0
The COMP and FRMASS response types are provided to facilitate the specification of
the classical topology optimization task of minimizing the compliance of a loaded
structure while limiting the mass to some percentage of the maximum allowable
amount. In MSC.Nastran’s implementation, these responses can be applied generally
so that the COMP response could lead to a constraint and the minimization of
FRMASS could be an objective.
New and Modified Design Optimization Parameters
(DOPTPRM)
Two new design optimization parameters are added for topology optimization in
SOL 200 as shown in Table 6-5. A new parameter TCHECK is used to turn on/off a
filtering algorithm to prevent the checkerboard like material distribution. Another
parameter TDMIN is introduced to achieve mesh independent solutions, control the
size of members in the topology optimized design, and therefore the degree of
simplicity in terms of manufacturing considerations.
In addition, a number of existing DOPTPRM parameters have different default values
for topology optimization as opposed to Sizing/Shape optimization, as shown in
Table 6-6. As described in “BIGDOT Optimizer” on page 147, the BIGDOT
optimization algorithm is available for topology optimization problems with many
(>2000) designed elements. This is selected by setting DOPTPRM parameter
METHOD to 4.
Table 6-5 New DOPTPRM Design Optimization Parameters
Name
TCHECK
Description, Type, and Default Value
Topology Filtering options (integer 0 or 1)
1 Filtering algorithm is on for topology optimization (default)
0
TDMIN
No filtering algorithm
Topology minimum member diameter (real > 0.0) in the basic
coordinate system. Default =0.0 (i.e., no minimum member size
control). This option is applied on 2 and 3 D elements only.
CHAPTER 6
Optimization
Table 6-6 Default Values for DOPTPRM Design Optimization Parameters
Parameter
Sizing/Shape
Topology
DESMAX
5
30
CONV1
0.001
1.0E-5
CONVDV
0.001
1.0E-4
DELX
0.5
0.2
DXMIN
0.05
1.0E-5
As a final comment on DOPTPRM parameters, it was necessary to change the
definition of the P2 parameter that controls the amount of print that occurs at design
cycles specified by P1. For sizing and shape optimization, design variables are printed
for any value of P1 = 1 (or if 1 is including in the sum of the options). Since a topology
optimization task can easily result in thousands of design variables, this would not be
a viable option for most problems. Instead, design variable prints are turned off
unless P2 value greater than 8 is specified.
Outputs
P2=1 (default) on Bulk Data entry DOPTPRM does not print topology design variables
to minimize optimization output since topology optimization involves in a large
number of design variables. P2>8 prints topology design variables.
Output in for the two new responses, compliance and fractional mass, and topology
design variables are shown if Figure 6-5. Also in this figure, the design variable
history shows the external element ID associated with the internal design variable ID.
139
140
----COMPLIANCE RESPONSES --------------------------------------------------------------------------------INTERNAL DRESP1
RESPONSE
LOWER
UPPER
ID
ID
LABEL
BOUND
VALUE
BOUND
----------------------------------------------------------------------------1
1
COMPL
N/A
1.4162E+02
N/A
----FRACTIONAL MASS RESPONSES --------------------------------------------------------------------------------INTERNAL
DRESP1
RESPONSE
LOWER
UPPER
ID
ID
LABEL
BOUND
VALUE
BOUND
----------------------------------------------------------------------------2
2
FRMASS
N/A
3.0000E-01
3.0000E-01
******************************************************************************
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
******************************************************************************
DESIGN VARIABLE HISTORY
----------------------------------------------------------------------------INTERNAL | EXTERNAL |
|
DV. ID. | ELEMENT ID |
LABEL
|
INITIAL
:
1
:
2
--------------------------------------------------------------------------------------------------------------------------------1 |
1
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
2 |
2
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
3 |
3
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
4 |
4
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
5 |
5
| TOPVAR
|
3.0000E-01 :
3.6000E-01 :
6 |
6
| TOPVAR
|
3.0000E-01 :
3.6000E-01 :
7 |
7
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
8 |
8
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
9 |
9
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
10 |
10
| TOPVAR
|
3.0000E-01 :
2.4000E-01 :
--------------------------------------------------------------------------
Figure 6-5 New Output in jobname.f06
PARAMETER, DESPCH – specifies when the optimized Bulk Data entries are written
to the PUNCH file for sizing and shape optimization. In topology optimization,
DESPCH is used to specify when the topology optimized element density values are
written to the topology element density history file jobname.des. This file can be
written in one of two formats. The first format is a MSC.Patran neutral element results
file that can be used with a custom template file (.res_tmpl) to display topology results
on MSC.Patran. This format is obtained by default. In order to support MSC.NastranOptiShape users, this file can also be written in OptiShape Patran Preference format
by setting PARAM,DESPCH1=-1. Thus, MSC.Nastran-OptiShape users can display
CHAPTER 6
Optimization
and animate SOL 200 topology optimization results using the MSC.NastranOptiShape Patran Preference. Figure 6-6 shows and element density history file using
the OptiShape Preference format.
/DENSI/
1
Flag for element density file
Design cycle ID
10
1
2
3
4
5
6
7
8
9
10
0.240
0.240
0.240
0.240
0.360
0.360
0.240
0.240
0.240
0.240
External element ID and density value
Figure 6-6 Element Density History File jobname.des
Guidelines and Limitations
The quality of the results of a topology optimization task is a strong function of how
the problem is posed in MSC.Nastran. This section contains a number of tips that have
been developed based on extensive testing of this new capability.
• A new DRESP1=COMP is introduced to define the compliance of structures
for topology optimizations. The response is usually used as an objective to
maximize structural stiffness in static design problems.
• A new DRESP1=FRMASS is introduced to define the mass fraction of
topology designed elements. The DRESP1=WEIGHT is the total weight of all
structural and non-structural mass. For topology optimization tasks
DRESP1=FRMASS response is recommended to define a mass reduction
target in a design constraint.
• The POWER field on the TOPVAR entry has a large influence on the solution
of topology optimization problems. A lower POWER often produces a
solution that contains large “grey” areas (area with intermediate densities 0.3
– 0.7). A higher value produces more distinct black and white (solid and
void) designs. However, near singularities often occur when a high POWER
is selected.
141
142
• A parameter TCHECK on DOPTPRM is used to turn on/off the
checkerboard free algorithm. The default of TCHECK=1 activates the
filtering algorithm. This default normally results in a better design for
general finite element mesh. However, if high order elements and/or a
coarser mesh is used, turning off the filtering algorithm may produce a better
result.
• The parameter TDMIN is mainly used to control the degree of simplicity in
terms of manufacturing considerations. It is common to see some members
with smaller size than TDMIN at the final design since the small members
have contributions to the objective. Minimum member size is more like
quality control than quantity control.
• XINIT on the TOPVAR entry should match the mass target constraint so that
the initial design is feasible.
• Maximum design cycle DESMAX=30 (as default) is often required to
produce a reasonable result. More design cycles may be required to achieve
a clear 0/1 material distribution, particularly when minimum member size
control used.
• There are many solutions to a topology optimization, one global and many
local minimization. It is not unusual to see different solutions to the same
problem with the same discretization by using different optimization solvers
or the same optimization solver with different starting values of design
variables.
• In a multiple subcase problem, a Case Control command DRSPAN can be
used to construct a weighting function via a DRESP2 or DRESP3. For
example, a static and normal mode combined problem, the objective can be
defined as
 c1 
 λ0 
obj = weight1 ⋅  -----  + weight2 ⋅  ------ 
 c0 
 λ1 
where weight1 and weight2 are two weighting factors. c 1 is the calculated
compliance and λ1 is the calculated eigenvalue via DRESP1 definition. c 0
and λ 0 are the initial value of these responses.
• The parameter BAILOUT =0 (default) may cause the topology optimization
run to exit if near singularities are detected. Users may increase the value of
XLB on TOPVAR to further prevent the singularity or set BAILOUT =-1 to
cause the program to continue processing with near singularities.
CHAPTER 6
Optimization
• To obtain a rib pattern by topology optimization, a core non-designable shell
element thickness must be defined together with two designable above and
below the core thicknesses. That is, add two designable elements for each
regular element.
• Elements referencing the composite property PCOMP entry cannot be
designed.
• Superelements are not supported.
• Topology design variable cannot used together with other type design
variables
• Topology design sensitivity is not supported
Numerical problems often occur when solving a topology optimization task. The
nature of the problem depends on element type, number of elements, optimization
algorithm and so on. One frequent numerical problem is the so-called checkerboard
effect. Checkerboard-like material distribution pattern is observed in the topology
optimization of continuum, especially when first order finite elements, such as
CQUAD4, are employed to analyze structural responses. It has been shown that the
Checkerboard-like phenomenon is caused by the finite element formulation. The
problem occurs because the checkerboard has an artificially high stiffness compared
with a structure with uniform material distribution [1]. The easiest way to decrease the
checkerboarding effect is to use higher order elements (such as CQUAD8). This
however increase the CPU-time considerably. Another closely related phenomenon is
mesh-dependent solutions. It is seen that a more detailed structure is found by
increasing the number of elements. The ideas of making a finer finite element mesh is
to get a better finite element solution. However, this finer meshing tends to have an
increasing number of members with decreasing size. This more detailed topology
solution creates a problem from a manufacturing point of view. An overview of the
techniques used to avoid the checkerboarding and mesh-dependent solutions can be
found in the reference [1]. In SOL 200, filtering algorithms are used to promote a
checkerboard-free and mesh independent topology optimized solution.
Topology otimization is powerful tool to generate design concepts in the early design
stage. Unfortunately, the topology optimzed designs usually turn out to be infeasible
for certain manfacturing processes, such as casting and extrusion. This issue will be
addressed in a future MSC.Nastran release.
143
144
Example 1 (topex1.dat)
This example leads to a conceptual design of a bicycle frame in a 2D situation by
maximizing the stiffness for a given amount of material (70% mass reduction) that
(shown in Figure 6-7) satisfies two boundary condition and load cases.
Figure 6-7 Bicycle Frame
Two loading and constraint conditions are assumed corresponding to two scenarios
riding the bicycle on sitting and standing positions as shown in the figures below.
There are 2442 QUAD4 elements and 2 TRIA3 elements.
CHAPTER 6
Optimization
Figure 6-8 FE Model of a Bicycle Frame
The input data for this example that is related to topology optimization is listed in
Listing 6-2. The result shown in Figure 6-9. is similar to existing bicycle frames.
Listing 6-2 Input File for Example 1
$ Topology Optimization Example 1/ XMY
$id msc, topex1 $ v2005 4-Jun-2004 xmy
SOL 200
$ OPTIMIZATION
CEND
$
SEALL = ALL
SUPER = ALL
ECHO = NONE
set 7 = 20
set 9 = 40
DESOBJ = 1
DESGLB = 1
SUBCASE 1
SUBTITLE=LOAD CASE 1
SPC = 2
LOAD = 7
DRSPAN = 7
145
146
ANALYSIS = STATICS
SUBCASE 2
SUBTITLE=LOAD CASE 2
SPC = 2
LOAD = 9
DRSPAN = 9
ANALYSIS = STATICS
BEGIN BULK
$
TOPVAR,
1 ,
TSHELL,
PSHELL, .3, , , ,
DRESP1
2
FRM
FRMASS
DRESP1, 20,
COMP1,
COMP
DRESP1, 40,
COMP2,
COMP
DRESP2
1
COMPL
SUM
DCONSTR 1
2
.3
1
Figure 6-9 Topology result of a Bicycle Frame
References
1. Bendsoe, M.P. and Sigmund, O. Topology Optimization Theory, Methods, and
Applications, Springer, 2003.
2. Rozvany, G.I.N., Bendsoe, M.P., and Kirsch U., Layout Optimization of
Structures, Appl. Mech. Rev., 48, 1995, pp.41-119
CHAPTER 6
Optimization
6.9
BIGDOT Optimizer
Introduction
BIGDOT is an optimization algorithm that has been developed by VR&D to solve
large optimization tasks. A guideline for the DOT optimizer (the workhorse
optimizer in SOL 200) is that it can comfortably address problems with several
hundred design variables and can be stretched to a few thousand design variables. By
contrast, BIGDOT has demonstrated the ability to solve problems with tens of
thousands of design variables with the maximum size approaching one million
variables. A reference for the BIGDOT algorithm is: Vanderplaats, G., 'Very Large
Scale Optimization', presented at the 8th AIAA/USAF/NASA/ISSMO Symposium
at Multidisciplinary Analysis and Optimization, Long Beach, CA September 6-8, 2000.
The BIGDOT algorithm is available in MSC.Nastran 2005 and is offered as an
additional option as a royalty product that is outside the MasterKey concept.
Potential users of this capability should contact their MSC sales representative to get
information about the “Topology Optimization” option within MSC.Nastran. The
Guidelines and Limitations section of this subchapter discusses how this new option
interacts with the standard “Design Optimization” option.
Benefits
The primary benefit of including the BIGDOT option is that it enables the ability to
perform topology optimization of real-world structures. As “Topology Optimization
- Beta Capability” on page 135 indicates, topology optimization entails creating a
design variable for each individual element so that one can very quickly exceed to the
several thousand design variable practical limitation that is mentioned above for the
DOT algorithm.
A second benefit that will be of interest to some clients is that it can be applied in sizing
applications where the number of design variables is in the thousands and above.
Input
BIGDOT is available in MSC.Nastran by specifying METHOD=4 on the DOPTPRM
entry. Table 6-7 contains the meanings of the four options for this parameter.
147
148
Table 6-7 Meaning of the METHOD Parameter on the DOPTPRM Entry
Value
Description
1
Modified Method of Feasible Directions using DOT (default for nontopology optimization problems)
2
Sequential Linear Programming using DOT
3
Sequential Quadratic Programming using DOT
4
BIGDOT (default for topology optimization problems)
The remaining DOPTPRM parameters that govern the behavior of the optimizer are
identical between DOT and BIGDOT so that no additional inputs are required.
Output
The output from BIGDOT algorithm itself is controlled by existing DOPTPRM
parameter IPRINT. There are no other outputs that are affected by BIGDOT.
Guidelines and Limitations
The BIGDOT algorithm is intended for problems with many design variables. For
problems with fewer than one thousand variables, the DOT or ADS algorithms are
recommended.
As mentioned in the Introduction to this section, the BIGDOT algorithm is available
to users that have purchased the “Topology Optimization” (TO) option for
MSC.Nastran. This complements the existing “Design Optimization” (DO) option in
the following way:
1. If the user has acquired the DO option only, this enables standard shape and
sizing optimization and topology optimization with a limited number of
design variables. The optimizer can be either DOT or ADS.
2. If the user has acquired the TO option only, this enables general topology
optimization tasks but does not enable standard shape and sizing
optimization. The optimizer is BIGDOT.
3. If the user has both DO and TO, the BIGDOT algorithm can then be applied
to topology and shape and sizing optimization tasks with a large number of
design variables. The optimizer can be BIGDOT or DOT or ADS.
Example
The “Example 1 (topex1.dat)” on page 144 (Topology Optimization) utilizes BIGDOT.
MSC.Nastran 2005 Release Guide14
CHAPTER
7
Rotor Dynamics
■ Squeeze Film Damper Nonlinear Force
150
7.1
Squeeze Film Damper Nonlinear Force
Introduction
The requirement for high power output from modern gas turbine engines has resulted
in highly flexible light weight rotor designs. Control of vibration response in these
engines is a major design problem. The use of rolling element bearings with low
inherent damping makes it difficult to reduce vibration amplitudes and dynamic
loads transmitted to the rotor supporting structure. Squeeze film dampers (SFDs) are
therefore used to provide adequate damping to maintain low amplitude vibration
levels and to reduce the dynamic loads transmitted to the bearings and rotor support
structures.
The general SFD model has been sucessfully incorporated into the MSC.Nastran timedomain analysis and this new capability provides the means to design and analyze
SFDs for general rotor orbits with multiple frequency content. The new capability
includes static loads and models the lift-off phenomenon important in the design of
free-floating dampers.
Squeeze Film Damper Model Imbedded in MSC.Nastran
Transient Solution
In a coordinated effort between GEAE and MSC, the general SFD model was
incorporated in MSC.Nastran for transient analysis. This was accomplished by
inserting the SFD forces in the right-hand (Force Vector) side of the equations of
motion – no special element was added to MSC.Nastran. GEAE provided MSC with
the SFD FORTRAN code, a description of the input/output data, the variable
definitions, and a checkout two-degree-of-freedom test model and results.
The SFD code lends itself to a form of a NOLIN type of element similar to NLRGAP.
The NOLIN approach works with the NASTRAN time domain solutions (SOL 109
and SOL 129). The new SFD element is called NLRSFD. The Bulk Data entry NLRSFD
is used to input the SFD data (journal diameter, land length, oil viscosity, etc.).
As with the NOLINS, the NLRSFD will be selected by the NONLINEAR Case Control
command.
·
·
The SFD code uses as input the relative displacements and velocities x, x, y, y at the
·
·
·
·
connecting grids and outputs the forces F x ( x, x, y, y ) and F y ( x, x, y, y ) acting on the SFD
damper journal grid point. Equal and opposite forces - F x ( x, x·, y, y· ) and - F y ( x, x·, y, y· ) are
applied to the stator (SFD housing) grid point.
CHAPTER 7
Rotor Dynamics
Referring to Figure 7-1, GRID I is on the damper journal and GRID J is on the damper
housing. The two grids should be coincident and have parallel Cartesian coordinate
systems. The forces applied to the grids are based on the relative displacements and
velocities of the grids determined from the previous time steps in the NASTRAN
implicit time integration. If a parallel centering spring is used, then this separate
spring is entered using the CELAS2 two-ended element.
Y
Housing
Journal
Z
GRIDS
I&J
Figure 7-1 Imbedding the SFD Model in MSC.Nastran: Grid I is on the Damper
Journal and Grid J is on the Damper Housing
Theory for General Squeeze Film Damper Model
The squeeze film damper model is based on work originally performed at Case
Western Reserve University (CWRU). It incorporates a numerical solution of the
Reynolds lubrication equation for incompressible laminar isoviscous films that is
described in Reference 1. The model is capable of handling the specified pressure
boundaries at the feed (supply) and discharge (drain) ports of the SFD. The SFD
pressure distribution is determined using a one-dimensional, finite difference scheme.
The scheme is a 1-D adaptation of the 2-D finite difference method of Castelli and
Shapiro, Reference 2. The one-dimensional finite-difference approach permits the
151
152
account of static as well as dynamic deflections and is thus capable of modeling
general damper orbits with broad frequency content. The model computes the oil film
forces by numerical integration of the instantaneous film pressure distribution.
Squeeze Film Damper Input Data Format
The squeeze film damper (SFD) is implemented as a nonlinear force similar to the
NLRGAP. The SFD forces are activated from the Case Control Section using the
NONLINEAR command.
NONLINEAR= n
The Bulk Data entry for the SFD has the following form:
1
NLRSFD
2
3
4
5
6
7
8
9
SID
GA
GB
PLANE
BDIA
BLEN
BCLR
SOLN
PRES1
THETA1
PRES2
THETA2
NPNT
VISCO
PVAPCO NPORT
10
OFFSET1 OFFSET2
Field
Contents
SID
Nonlinear load set identification number. (Integer > 0, Required)
GA
Inner (e.g., damper journal) grid for squeeze film damper. (Integer > 0,
Required)
GB
Outer (e.g., housing) grid for squeeze film damper. (Integer > 0,
Required)
PLANE
Radial gap orientation plane: XY, XZ, or ZX. See Remark 1. (Character,
Default = XY)
BDIA
Inner journal diameter. (Real > 0.0, Required)
BLEN
Damper length. (Real > 0.0, Required)
BCLR
Damper radial clearance. (Real > 0.0, Required)
SOLN
Solution option: LONG or SHORT bearing. (Character, Default =
LONG)
VISCO
Lubricant viscosity. (Real > 0.0, Required)
PVAPCO
Lubricant vapor pressure. (Real > 0.0, Required)
NPORT
Number of lubrication ports: 1 or 2 (Integer, no default)
PRES1
Boundary pressure for port 1. (Real > 0.0, Required if NPORT = 1 or 2)
CHAPTER 7
Rotor Dynamics
THETA1
Angular position for port 1. See Remark 2. (0.0 < Real > 360.0, Required
if NPORT = 1 or 2).
PRES2
Boundary pressure for port 2. (Real > 0.0, Required if NPORT = 2).
THETA2
Angular position for port 2. See Remark 2. (0.0 < Real < 360.0, Required
if NPORT = 2)
NPNT
Number of finite difference points for damper arc. (Odd integer < 201,
Default = 101)
OFFSET1
Offset in the SFD direction 1. (Real, Default = 0.0)
OFFSET2
Offset in the SFD direction 2. (Real, Default = 0.0)
Remarks:
1. The XY, YZ, and ZX planes are relative to the displacement coordinates of
GA and GB. The plane coordinates correspond to the NLRSFD directions 1
and 2. GA and GB should be coincident grids with parallel displacement
coordinate systems. Wrong answers will be produced if this rule is not
followed.
2. The angular measurement is counterclockwise from the displacement x-axis
for the XY plane, the y-axis for the YZ plane, and the z-axis for the ZX plane.
3. OFFSET1 = Damper housing ID center offset displacement relative to OD
center in the horizontal direction. Entered as a positive value for horizontally
to the left (negative x-direction) displacement.
4. OFFSET2 = Damper housing ID center offset displacement relative to OD
center in the vertical direction. Entered as a positive value for downward
(negative y-direction) displacement. Positive entry typically used for -1 g
compensation.
Note: The OFFSET2 value represents an eccentric damper housing in the vertical
direction and is typically used to compensate for the -1g displacement of
damper supported by a centering spring.
153
154
Squeeze-Film Damper Example
The following example demonstrates the use of the new NLRSFD nonlinear force. The
model is shown in Figure 7-2. The MSC.Nastran input file is shown in Listing 7-1.
The unbalance load of 20 Gm-cm is used to excite the structure. The resulting
nonlinear forces are shown in Figure 7-3.
Rotor - Grid 101
Support - Grid 102
NLRSFD
Spring to Ground
Figure 7-2 Model
Listing 7-1
NASTRAN
SOL 109
CEND
TITLE = Simple test model, SOL 109, No damping
$
ECHO= UNSORT
$
$------------- Results requests -------------------SET 101 = 100,101
DISP
(PRINT,PUNCH,SORT2) = 101
SET 102 = 101,102
ELFORCE (PRINT,PUNCH,SORT2) = 102
$
TSTEP = 999
NONLINEAR=1
SUBCASE 200
LABEL = 20 gm-in unbalance
CHAPTER 7
Rotor Dynamics
DLOAD = 200
$
OUTPUT(XYPLOT)
XGRID= YES
YGRID= YES
XTITLE= TIME (SEC)
YTITLE= SFD FORCE (X)
XYPLOT NONLINER/ 101(T1)
YTITLE= SFD FORCE (Y)
XYPLOT NONLINEAR/ 101(T2)
BEGIN BULK
$
$
1/386.4
PARAM
WTMASS258799-8
PARAM
GRDPNT
0
$
$1.....12......23......34......45......56......67......78
$
TSTEP
999
30001 .000010
100
$
$===============================================================================
$
DLOAD
200
1.0
20.0
301
20.0
302
$
TLOAD2
301
301
LOAD
0.0
100.0166.6667
270.0
TLOAD2
302
302
LOAD
0.0
100.0166.6667
0.0
$
$ F(f) = UNBAL * f**2 * (1/453.5924 lbm/gm) * (2*pi)**2 / 386.08858 in/sec**2
$
= UNBAL * f**2 * 2.25243e-4 (lbf)
$
(where UNBAL is given in GM-IN, 'freq' in Hertz)
$
= 1.0 * (10000.*2*pi/60)^2 /453.6/386.4
$
= 6.2619 (for 10,000 RPM)
$
DAREA
301
101
1 6.256715
DAREA
302
101
2 6.256715
$
$===============================================================================
$
Structural Model
$
CONM2
99
101
0
100.
(No Ip)
GRID
101
0
0.0
0.0
0.0
0
3456
onStat
GRID
102
0
0.0
0.0
1.0
0
3456
forSpinDir
$
$ CENTERING SPRINGS FOR SQUEEZE-FILM DAMPER
$
CELAS2
101 100000.
101
1
102
1
HorizK
CELAS2
102 100000.
101
2
102
2
VertK
$
$ Spring to ground
$
GRID
103
0
0.0
0.0
0.0
0 123456
CELAS2
111
1.+9
103
1
102
1
HorizK
CELAS2
112
1.+9
103
2
102
2
VertK
$
$ SQUEEZE-FILM DAMPER INPUT
$
$1.....12......23......34......45......56......67......78......89......910....10
NLRSFD
1
101
102
XY
6.44
.727
.003
SHORT+
+
7.-7
0.0
1
0.0
180.0
31+
155
156
+
$
ENDDATA
0.0
0.0
Figure 7-3 SFD Force, X and Y Direction
References
1. Adams, M. L., Padovan, J., Fertis, D. G., “Engine Dynamic Analysis With
General Nonlinear Finite-Element Codes, Part 1: Overall Approach and
Development of Bearing Damper Element”, ASME Journal of Engineering
for Power, Vol. 104, July 1982, pp. 586-593.
2. Castelli, V., and Shapiro, W., "Improved Method for Numerical Solutions of
the General Incompressible Fluid Film Lubrication Problem”, ASME Journal
of Lubrication Technology, Vol. 89, No. 2, 1967, pp. 211-218.
3. Adams, M. L., Padovan, J., Fertis, D. G., “Finite Elements for Rotor/Stator
Interactive Forces in General Dynamic Simulation, Part 1: Development of
Bearing Damper Element”, NASA CR-165214, EDA 201-3A, October 1980.
4. Ghaby, R., “Transient/Nonlinear Vibration of Gas Turbine Engines With
Squeeze Film Dampers Due to Blade Loss”, May 1984 Master of Science
Thesis, Case Western Reserve University.
5. Black, G., Gallardo, V., “Blade Loss Transient Dynamics Analysis Task IITETRA 2 User’s Manual”, NASA CR-179633, November 1986.
MSC.Nastran 2005 Release Guide
CHAPTER
8
DDAM Processor
■ A DDAM Processor for MSC.Nastran Including an MSC.Patran
Interface
■ Guidelines for Effective DDAM Analysis
■ Theoretical Background
■ Worked Two Mass Problem
■ Format of Coefficient File
■ Control File Format
■ User defined Shock Spectra
■ MSC.Patran Interface
158
8.1
A DDAM Processor for MSC.Nastran Including an
MSC.Patran Interface
Introduction
This chapter describes a method for the calculation of the response of a structure using
the Dynamic Design Analysis Method (DDAM) in MSC.Nastran.
The Theory Section, has been implemented in MSC.Nastran and in a FORTRAN code.
Due to the classified nature of specific DDAM shock environment calculations, it may
be necessary to run the entire analysis, or perform that portion of the analysis on a
separate computer. The DDAM package as implemented in MSC.Nastran performs
the analysis in three phases as outlined in the following steps:
1. SOL 187 is used to perform a fixed-base modal analysis. Additionally, it
calculates modal participation factors and modal effective mass.
2. Running the DDAM program, which accepts ASCII OUTPUT4 data from
MSC.Nastran, performs shock excitation calculations using the user
supplied shock coefficients and generates shock spectrum data.
Additionally, it terminates the shock excitation calculations when a specified
modal mass is reached. Options are provided in this step to use equations
based upon the modal masses of each mode, or a user-input design spectrum
to compute the shock excitations. This will be run automatically from within
MSC.Nastran using the ISHELL capability unless directed otherwise.
3. Continuation of the MSC.Nastran Sequence, using output from part 2 to
perform DDAM motion and stress recovery following the NRL modal
summation convention. Data is calculated and output for MSC.Patran postprocessing. This will automatically follow step 2 in SOL 187.
“MSC.Patran Interface” on page 192 describes the MSC.Patran interface that
automates the process, including coefficient and file selection.
The following section describes the process in detail, with notes and documentation
for all of the parameters and data required.
DDAM with SOL 187
The first step of the procedure is the calculation of the modal frequencies and
participation factors that are accomplished in MSC.Nastran by SOL 187. The model
must be in a “free-free” condition with the foundation degrees of freedom referenced
by a SUPORT entry. The DDAM processor considers the SUPORTed degrees of
freedom (and any other grids rigidly connected to them) to be a “fixed” base for the
CHAPTER 8
DDAM Processor
modal analysis. The information needed for the Fortran program is output from
MSC.Nastran to unit 11 in ASCII format. Unit 11 will be assigned to a file using the
ASSIGN statement in MSC.Nastran. The following paragraphs describe the
Executive, Case Control and Bulk Data Sections of the MSC.Nastran necessary
Executive Control Data/File Management Section
The solution sequence must be SOL 187.
For example:
SOL 187
It is necessary to include ASSIGN statements to assign the plot output and DDAM
output to physical files. For example:
ASSIGN OUTPUT2=‘d1.opw’, UNIT=34, DELETE
assigns OP2 formatted post processing data to be sent to the file d1.opw. You also
need to assign the NRL-summed plot data to separate units:
ASSIGN OUTPUT2=‘d1.opx’, UNIT=31, DELETE
ASSIGN OUTPUT2=‘d1.opy’, UNIT=32, DELETE
ASSIGN OUTPUT2=‘d1.opz’, UNIT=33, DELETE
The following:
ASSIGN OUTPUT4=‘d1.f11’, UNIT=11, FORM=FORMATTED, DELETE
assigns the file d1.f11 to be the DDAM output, which will be used as the input to the
Fortran program. The “DELETE” qualifier tells MSC.Nastran to delete any existing
versions of the file and replace them with the one generated in this submittal. The
output file from the Fortran program must be assigned as well:
ASSIGN INPUTT4=‘d1.f13’, UNIT=13, FORM=FORMATTED, DEFER
DEFER tells MSC.Nastran not to check for the existence of the file or delete an existing
one.
Finally, in SOL 187, the execution of the Fortran program is directed by a control file
that must be created and identified:
ASSIGN INPUTT4=‘d1.ddd’, UNIT=21, FORM=FORMATTED
The format of this file will be discussed later.
159
160
Case Control Data
The required Case Control is similar to that required for a SOL 103 modal run, with a
few caveats and exceptions. The “METHOD” command for the residual structure will
determine the frequency range of the dynamic response calculations used by DDAM.
Because of this, be sure to include a broad enough range to ensure that the required
modal mass will be available for processing. All procedures affecting Superelement
reduction to the residual degrees of freedom are allowed (i.e. component mode
synthesis, GDR and Guyan reduction). However, NRL-summed results can only be
generated for the residual model.
A PARAM, POST can be used with a limited number of output requests to generate
data for post-processing. Case control data controls the final NRL-summed DDAM
result data. Available data are STRESS, FORCE, DISPLACEMENT, VELOCITY and
ACCELERATION. Other data are either not calculated in SOL 187, or are meaningless
for DDAM. Mode shapes will come out by default. SOL 187 does not yet have the
ability to use the XDB file for direct results access in MSC.Patran.
Bulk Data
Note: In order for units to be totally consistent in DDAM analysis, the
MSC.Nastran model must be formulated in units of inches for lengths and
lb-sec2/in for mass. It is not necessary for the x, y or z axes to be correlated
to any specific direction. However, the system must have individual axes
that correspond to the fore/aft, athwartship and vertical directions (i.e. You
cannot have a system where the basic x axis points 45 degrees between the
fore/aft and vertical directions or output the whole model in a cylindrical
system.)
The input data file is required to have structure geometry, property and material
information (as any model should). Additionally, the following information must be
present.
A SUPORT entry is necessary to define the foundation reaction point (the “fixed
base”) in all 3 translational degrees of freedom. If the foundation is distributed, as in
most structures, rigid elements or MPCs must tie all the foundation points to a single
point. This point must be in the residual structure (for Superelements) and in the Aset (this is the default for a SUPORTed degree of freedom). The translational
directions of the SUPORT point define the directions for the shock response
calculations, so they should be in a rectangular coordinate system. An option in the
DDAM program allows you to orient the specific coordinate axes to the fore/aft,
athwartship and vertical directions. Though only translational directions are used for
the shock response, all 6 DOF may appear on the SUPORT entry. If one direction has
CHAPTER 8
DDAM Processor
no unconstrained mass (this happens a lot in test cases with few DOF), that direction
should be SPCed and not called out on the SUPORT entry. If a massless direction is
referenced, you get a humorous “MR MATRIX has NULL column” error.
The eigenvectors must be normalized to “MASS.” This is the default for the Lanczos
solver on the EIGRL entry, but not for other methods specified on the EIGR entry.
“MAX” normalization will result in incorrect modal masses and participation factors,
as the calculations use a shortcut for calculating the participation factors that relies on
mass normalization.
Several parameters are available to control the analysis, and to direct data to its
required places. There are two important and others somewhat less important
parameters used in the bulk data file:
DDAM Control File
In order for MSC.Nastran to run the Fortran program correctly, it is necessary to create
a small control file that tells the program some information about your model. The file
is ASCII, and the format is detailed in “Control File Format” on page 187.
This is the file assigned to unit 21 described above.
Output
Output from SOL 187 consists of the following:
• A small ASCII file, as defined by the ASSIGN statement, for input to the
Fortran program. This file contains a list of frequencies, participation factors,
the total mass, and the available modal mass in each direction.
• Another small ASCII file, also defined in the ASSIGN statement, for input
back into MSC.Nastran from the Fortran program.
• A verification file containing frequencies, modal masses, participation
factors, and calculated accelerations.
• The .F06 file
• A .OP2 file containing mode shapes
• Three .op2 files containing the NRL-summed results
The MSC.Nastran .F06 output file will contain echoes of several matrices constructed
in the DDAM process, including: (equation numbers refer to the numbers in
“Theoretical Background” on page 172)
• OMEGX - the vector of natural frequencies in rad/sec
161
162
• PAB - The participation factor matrix [P] defined in equation 9
• MTOT - the six diagonal terms of MTOTC
• MEFF - the six diagonal terms of MEFFC
• MFRACT - the ratio of effective to total mass for each direction
OMEGX, PAB, MTOT and MFRACT are output to unit 11 by an OUTPUT4 module
for use in Part 2. In addition, when the program calculates the rigid body vectors
about the SUPORT point, values of Epsilon and Strain Energy are printed for each
vector. These values can be used to determine if the model is over-constrained
(contains constrained DOF not connected to the SUPORT point. In general, Epsilon
terms should be less than 10-6. Strain energy is a measure of elastic energy in the
model resisting rigid body motion. Theoretically, it should be zero for DDAM, but in
practice it usually has some small value. As a rule, <1 is acceptable for translations,
and <100 is acceptable for rotations. If strain energies in the range of 104 or greater are
encountered, this is an indication that a constrained degree of freedom not connected
to the SUPORT entry probably exists in the model (such as an unintentionally
grounded CELAS). Keep in mind, however, that these values are all modeldependent.
If the strain energies are non-zero for the first three SUPORT points (which
correspond to the translational directions) it is an indication of non-singular degrees
of freedom that are constrained. While MSC.Nastran allows this to take place, it
violates the assumptions made in this DDAM processor, resulting in incorrect modal
masses and participation factors in that direction. As a result, the final NRL results
will be incorrect. To comply with the MSC.Nastran DDAM assumptions, it is
necessary to connect all non-singular degrees of freedom that are to be constrained to
the SUPORT point. What this means is that the only SPC entries in the model should
be for singular rotational DOF. SPC entries should not be used for other reasons, such
as symmetry constraints or non-moving foundation points.
Calculation of Shock Spectrum
“ddamish” (ddamish.exe on NT) is an interactive/batch program that performs shock
spectrum calculation for the structure under consideration. Structural data consisting
of natural frequencies and participation factors that were generated by MSC.Nastran
are utilized here as input data. The program queries the analyst for spectrum inputs,
loading characterization, and other details. In general, this program is run in batch
mode by MSC.Nastran, with the answers supplied by the .ddd control file.
CHAPTER 8
DDAM Processor
The following discusses the various prompts in the program if it is run interactively:
Do you have a shock spectrum or are you using
coefficients ?
... <CR> = use default coefficients
... c
= use other coefficient file
... s
= user input shock spectrum
The program has a provision to include a set of shock coefficients compiled into the
code. Hitting <CR> will use these coefficients. The default coefficients provide
capability to cover the full range of Navy coefficients in DDS 072, including surface
and submerged ships, deck, hull and shell mount, elastic, and plastic. The user has
the option to input custom coefficients for any or all of the configurations selectively.
Note that the choices are: <CR> (carriage return) for yes, “c” for coefficients stored in
an external file (the most common option) and “s” to use an externally defined shock
spectrum (not based on coefficients). These inputs are not case sensitive. The format
for the external coefficient file is described in “Format of Coefficient File” on
page 185, and the user spectrum format is described in “User defined Shock Spectra”
on page 190. The external coefficient file also contains provision for a modal mass
cutoff percentage and a minimum G value. If either “c” or “s” is chosen, another
prompt will appear asking for the name of the external file.
Are you using DDS-072 or NRL 1396 style
equations ?
... <CR> = use DDS-072 equations
... n
= use NRL 1396 equations
DDS-072 and NRL 1396 differ slightly in the format of the equations and how many
coefficients are required for different scenarios. This choice allows you to use either
format.
ENTER THE DESIRED NASTRAN INPUT FILE NAME:
Default: <CR> = ddam.f11
This is the .f11 file output by the MSC.Nastran run. It is necessary to type in the full
file name. If the program is unable to find or open the file, a secondary prompt will
inform you of that, and prompt for a new name. After successfully specifying the
name, the program will echo the filename that it opened, and the unit number
associated with it.
163
164
ENTER THE DESIRED VERIFICATION OUTPUT FILE NAME:
Default: <CR> = d1.ver
This file is the intermediate result echo. This file contains the summary of modes,
modal mass and mass percentages for each shock direction. The default name is the
name of the .f11 file you specified, but with a .ver extension. This file is useful to verify
which modes are contributing most to a model’s response.
ENTER THE DESIRED NASTRAN OUTPUT FILE NAME:
Default: <CR> = d1.f13
This is the file that will be used as input for the MSC.Nastran restart in Part 3. The
default name is constructed similarly to the verification default, but with .f13
appended to it.
What type of ship do we have ?
... Enter 1 for SURFACE (default coefficients)
... Enter 2 for SUBMERGED (default coefficients)
Where is
... Enter
... Enter
... Enter
the equipment mounted ?
1 for DECK (default coefficients)
2 for HULL (default coefficients)
3 for SHELL (default coefficients)
What type of factors do you want ?
... Enter 1 for ELASTIC (default coefficients)
... Enter 2 for EL-PL (default coefficients)
These three questions choose the appropriate shock coefficients. The notation
“(default coefficients)” after the description indicates that the coefficients for that
configuration were read from the list built into the program. If the user has specified
some or all coefficients in an external file, the notation “(user coefficients)” will appear
after the configuration for which coefficients were entered. The specific equations
implemented in this program are documented in “Format of Coefficient File” on
page 185.
ENTER F/A DIRECTION (X,Y, or Z):
ENTER VERTICAL DIRECTION (X,Y, or Z):
CHAPTER 8
DDAM Processor
These two questions establish the coordinate directions for the application of the
directional shock scaling factors. These are the AF and VF in the spectrum equations.
This specification allows models built in non-standard MIL-spec coordinate directions
(X forward, Y athwartship, Z up) to be processed by DDAM with the loads applied in
the correct directions.
Is this a multiple or single mode analysis ?
<CR> = normal, s = single mode
This option is provided if the user wishes to examine the contribution of a single mode
to the overall summed response. Choosing the “s” option will generate a prompt
asking for the mode number of interest. The program then generates a .f13 file
containing factors of zero (the UHVi) for all modes except the one chosen. This will
result in displacements, stresses, etc. for the model as if the entire response consisted
of just a single mode. Note that this single mode will be NRL summed, so the signs
will lost. For normal DDAM analysis, choose the normal option.
The PARTNVEC matrix and the BYMODE parameters provide similar capability.
They are described more fully in section the following sections on special
circumstances.
ENTER WEIGHT CUTOFF PERCENT OR <RET> FOR DEFAULT:
Default = 80.0
This number is the percentage of total mass at which modal processing ceases. The
DDAM document specifies that only a percentage of the total modal mass needs to be
included in the NRL sum. The default value is specified in the program with the
default coefficients, or in the alternate coefficient file. The value here should be
entered as a percentage (i.e. 80. or 100.) not as a decimal. Specifying “100.” will
process all the modes that were calculated by MSC.Nastran.
Special Circumstances – Selection of Specific Modes
If the user wishes to selectively choose which modes go into the NRL summation, a
capability is provided using DMI (Direct Matrix Input) entries. On the DMI entries,
the user describes a matrix called PARTNVEC, which is a partitioning vector. The
vector is used to break up the eigenvector matrix and UHV matrix in a specific
manner. PARTNVEC is a multi-row, 3-column matrix, where each row represents a
mode number, and each column represents a shock direction. If the matrix has a “1”
165
166
entry, that particular mode is retained for that particular shock direction. The
following shows a PARTNVEC description employing several options that a user
might be interested in for an analysis that generated 12 modes:
1
2
3
4
5
6
7
8
9
12
3
3
1.
$ define the matrix as a 12 row by 3 column matrix
DMI
PARTNVEC
0
2
1
$ define col 1 ( keep all modes - 1-12)(f/a shock)
DMI
PARTNVEC
1
1
1.
THRU
12
$ define col 2 ( keep modes 1, 2 and 3)(athw shock)
DMI
PARTNVEC
2
1
1.
2
1.
$ define col 3 ( keep only mode 5)(vert shock)
DMI
PARTNVEC
3
5
1.
Be sure to ask for all the modal mass (“100.”) in the DDAM program if you use this
option, since it will perform its own partitioning on the output from the DDAM
program.
Special Circumstances – Mode-by-Mode Output
It is occasionally desirable to look at DDAM output on a mode-by-mode basis. Such
occasions can be model or methodology verification, or to gain a better understanding
of which modes are contributing to particular results.
Mode-by-Mode output is controlled in MSC.Patran by the normal output requests,
and by three parameters:
In SOL 187, the parameters are XBYMODE, YBYMODE, ZBYMODE. Because modeby-mode output can generate a large volume of data, three parameters are included
to handle just mode-by-mode data in specific directions. For example:
PARAM,XBYMODE,YES
Will generate data only for the X direction. In addition to the .F06 file printed output,
each parameter generates a separate plot file with all the mode-by-mode results that
have been requested. These three files are in units 41-43, and can be designated to
specific files using an ASSIGN statement:
ASSIGN OUTPUT2=’job_mbm_x.op2’ UNIT=41, DELETE
CHAPTER 8
DDAM Processor
Output is controlled by requests in the case control file, so if you have requested
STRESS=ALL, and then request mode-by-mode data, you will get mode-by-mode
stresses for all modes. Again, if this is necessary, be wary of the volume of data that
can be easily produced.
Output in the .f06 file is labeled with section headers:
Each mode-by-mode section is preceded by a small header:
Important Note: Displacements, accelerations and velocities are all labeled as
Eigenvectors – look at the magnitudes to make sure you have the right one.
Special Circumstances – Single shock direction calculations
If you only need output for a single shock direction, you can use= PARAM entries to
skip particular directions:
PARAM
PARAM
PARAM
XSHOCK
YSHOCK
ZSHOCK
NO
NO
YES
If using DTI input to pick certain modes, you still have to define the 3 column matrix
– this is just to cut down on post-processing output
This capability is especially useful to cut down output when using the mode-by-mode
capability.
Special Circumstances – Running the Fortran part of the Analysis
Separately
There are circumstances where it may be necessary to run the Fortran program
separately from the MSC.Nastran job. Since the program runs automatically by
default, it is necessary to add some parameters to disable the automatic running of the
program. Some circumstances where you may need to run independently on
MSC.Nastran:
• The Fortran program is on a classified computer, but MSC.Nastran is not
• You have a different version of the Fortran program
• You have a metric DDAM program
You can use a PARAM entry to skip the Fortran part of the run, run the Fortran
elsewhere, then restart the MSC.Nastran run with the externally calculated .f13 file:
PARAM,MODEOUT,YES
This calculates modes, outputs the required DDAM data, then exits MSC.Nastran.
167
168
Use PARAM,UHVOLD,YES
This runs MSC.Nastran as usual, but does not run the Fortran program. Instead it will
red a .f13 file that has been prepared. This parameter can be used on a restart from a
MODEOUT run where the .f13 file was calculated externally.
It may also be desirable to replace the MSC Fortran program delivered with DDAM
with a site-developed one. If so, it is necessary to replace the ddamish.exe program in
the MSC.Nastran installation with your program. Because there are issues with
arguments using some Fortran compilers, contact MSC for instructions on what is
needed to use this approach.
CHAPTER 8
DDAM Processor
8.2
Guidelines for Effective DDAM Analysis
In addition to the usual guidelines for effective structural dynamic modeling and
analysis, several specific considerations are recommended for DDAM analysis. The
present discussion addresses the structural modeling, foundation modeling, and data
interpretation aspects of the procedure.
In the process of modeling the subject structure, a decision must be made at the outset
to either employ sophisticated distributed mass modeling (the more common
approach) or coarse lumped mass modeling. The latter choice is one that permits
adherence to the DDAM “50% modes” criterion, and is the type of analysis for which
DDAM was developed. However, fidelity of the structural model with the actual
structure may be severely compromised by using this approach. This is especially true
for plate and shell structures, which tend to have a significant number of shell-type
modes, which are lost in a lumped mass approach. In more complicated shell
structures the analysis is considered to be acceptable if enough modes are used such
that at least 80% of the effective mass is accounted for. This frequently can be
accomplished with significantly fewer than 50% of the modes, and usually less than
50 modes. This DDAM procedure allows the user to take either approach.
Redundant and geometrically distributed foundations require special consideration
for meaningful DDAM analysis. Since the shock environment is specified at one
location, distributed foundations must be referenced back to this single location. For
foundations that are not “extremely” distributed, RBE2 constraints can be employed
to effect the reference to the single point. On more distributed systems, however, the
mass and flexibility of the foundation may be required in the structural model. In
these cases, the foundation should be included in the analyzed model, and the DDAM
“foundation” points will be below the actual foundation.
Resilient mounting is not normally analyzed with DDAM. In cases where equipment
is resiliently mounted, the mounts are generally assumed to have bottomed out. In
this case, the mount points can be considered the “foundation” points. DDAM
analyses run on resiliently mounted systems are trivial exercises, since all of the modal
mass is accounted for in a single rigid body mode. Flexible modes of the structure are
not accounted for, and all of the loads on the actual structure are frequently zero or
close to zero.
For the process of load evaluation on a structure, particular attention should be given
to the mode-by-mode data provided in the verification file. For cases where forces or
stresses are found to be excessive, the verification file can provide valuable guidance.
169
170
In particular, modes that contribute significantly to the overall loading can be
identified. These modes can then be visualized via PATRAN, and the structure
modified to change particularly detrimental modal behavior.
Another area where care must be taken are in models where significant mass is
included that is not directly related to the structure of interest, and is of lower
frequency. Reduction gear models that include significant runs of shafting are
examples of this. In these cases, it is possible to get 80% of the modal mass entirely in
shafting modes. In these cases, it may be necessary to increase the modal mass
percentage to assure that you are getting 80% of the mass of the portion of model of
interest.
A Note on Symmetry
While the NAVSEA 3010 document does not exclude running a symmetric model, it
does not provide any guidelines to do so. There are some important considerations
when using symmetry. Among them:
• The modal mass must be doubled to calculate the shock coefficients properly
• Both symmetric and anti-symmetric modes must be included in the final
NRL sum
• Symmetry plane boundary points must be constrained with SPC entries
(which violates the SUPORT assumption in this DDAM) or connected to the
SUPORT entry with RBE elements (which incorrectly marks them as
“foundation” input points)
• The MSC.Nastran NRL sum module (DDRMM) cannot combine modes from
different NASTRAN runs without a modification to the DMAP alter.
• Cyclic symmetry involves calculating all of the proper harmonics,
calculating the modal masses correctly and then summing all of the different
harmonic modes in the final NRL sum.
Because of all these caveats, it is neither advisable nor easy to use this DDAM
processor for symmetric models.
However, if it is to be used, there are several modifications that must be made to the
procedure, including manually calculating modal masses and the resulting shock
factors. The user should be very careful doing this. The theoretical outline in
“Theoretical Background” on page 172 can serve as a guide. The methods should be
tested on a small model to assure that all the appropriate masses, coefficients, etc are
CHAPTER 8
DDAM Processor
modified. Also note that the NRL sum must be either performed manually (external
to MSC.Nastran) or the DMAP altered to accommodate combining results from the
symmetric and anti-symmetric runs.
References:
1. R.O.Belsheim and G.J.O’Hara, “Shock Design of Shipboard Equipment, Part
I, Dynamic Design Analysis Method,” NAVSHIPS 250-423-30, May 1962
2. “Shock Design Criteria for Surface Ships,” Naval Sea Systems Command,
NAVSEA 0908-LP-000-3010 Revision 1, September 1995.
3. M.M.Hurwitz, “A revision of the Dynamic Design Analysis Method
(DDAM) in NASTRAN,” Naval Sea Systems Command, December 1982.
4. NAVSEA Design Data Sheet DDS-072. (Confidential)
5. Scavuzzo & Pusey, “Naval Shock Analysis and Design,” Shock and
Vibration Information and Analysis Center (SAVIAC), 2000
Reference 1 outlines the original concept of DDAM as applied to Naval Shipboard
equipment. Reference 2 is the NAVSEA specification (latest version) that gives
specifics for performing this type of analysis. Reference 3 describes the procedure for
using DDAM within the framework of “modern” finite element codes. Reference 4
contains the classified NAVSEA coefficients for calculating the spectral quantities in
the response equations. Reference 5 is a text that follows the shock class taught by
Rudy Scavuzzo and Henry Pusey. It provides a lot of background on testing and
requirements, as well as many theoretical and analytical aspects of underwater shock
and DDAM.
171
172
8.3
Theoretical Background
Consider a structural system (Figure 8-1) described by a set of { U g } displacements, a
subset of which corresponds to a foundation interface { U m } . If the foundation
interface is redundant, let it be assumed that the foundation undergoes rigid body
displacements (that is, no foundation warping). Thus, the foundation interface is
related to a six degree of freedom (DOF) reference point displacement subset { U r }
through a multi-point constraint relationship
{ Um } = ( Gm ) { Ur }
Eq. 8-1
The remaining displacements in the { U g } set may be interrelated in a variety of ways,
depending on the particular structure’s configuration and approximating
assumptions, such as Guyan Reduction or Generalized Dynamic Reduction. When all
constraints and reductions are applied, the structural displacement state is described
in terms of a set, denoted here as the { U x } set which is partitioned as follows:
 Ul 
{ U x } =  ------ 
 Ur 
Eq. 8-2
The subset { U l } is comprised of discrete grid point displacements and generalized
displacements remaining after reduction, depending upon the choice of
approximating assumptions.
CHAPTER 8
DDAM Processor
{ Ul }
{ Um }
{ F r }, { U r }
Figure 8-1
In terms of the { U x } displacement set, the dynamics of an undamped linear static
structure subjected to foundation excitation is described by:


M ll M lr  U·· l 

+
M rl M rr  U·· 
r 


K ll K lr  U l

K rl K rr  U r



 0 
 = 


 Fr 

Eq. 8-3
Where M ll , M lr , M rl , and M rr are mass matrix partitions, K ll , K lr , K rl , and K rr are
stiffness matrix partitions, and Fr is the foundation interface reaction set. Since the
foundation { U r } is determinate due to Eq. 8-1, the transformation of the { U x } set into
base fixed displacement patterns and rigid body motions, respectively, is introduced.
Rigid body motions are readily defined on the basis of the stiffness matrix by
imposing the requirement that the { U l } set produces no static reactions due to applied
foundation motions { U r } , i.e.
[ K ll ] { U l }
or
RB
+ [ K lr ] { U r } = 0
Eq. 8-4
173
174
{ Ul }
RB
= – [ K ll ]
–1
[ K lr ] { U r }
Eq. 8-5
A convenient set of base fixed displacement patterns consists of a truncated set of base
fixed unit mass normalized modes that are the solutions of
2
[ K ll ] { φ li } = [ M ll ] { φ li }ω i
Eq. 8-6
Assembling the truncated set of modes into the matrix [ φ ll ] , the desired variable
transformation is defined as


 Ul 

 =
 Ur 


φ ll
0 rl
{ q1 } +
–1
K ll K rl
{ ur } =
1 lr 1 rr

–1
φ ll – K ll K lr  q 1

 Ur
0 rl
1 rr






Eq. 8-7
Upon transformation of the dynamic equation set, Eq. 8-3 with Eq. 8-7 (including premultiplication by the transpose of the transformation matrix, the modal equation set
is of the form


I ll P lr  q·· 
l
 ··  +
˜
P rl M rr  U r 




2
 0 
ω i O lr  q 1 


 = 
 F 
O rl O rr  U r 


Eq. 8-8
The matrix partitions are defined as follows:
T
[ I ll ] = φ ll M ll φ ll
2
T
[ ω l ] = φ ll K ll φ ll
T
–1
T
[ P lr ] = φ ll M lr – φ ll M ll K ll K lr
–1
T
[ O lr ] = φ ll [ K lr – K ll K ll K lr ]
–1
–1
–1
–1
˜
[ M rr ] = M rr – M rl K ll K lr – K rl K ll M lr + K rl K ll M ll K ll K lr
–1
[ O rr ] = K rr – K rl K ll K lr
[ P rl ] = [ P lr ]
T
[ O rl ] = [ O lr ]
T
Eq. 8-9
CHAPTER 8
DDAM Processor
The physical significance of the above noted matrix partitions is that [ P lr ] is the matrix
of participation factors, [ M˜ rr ] is the total rigid body mass referenced to { U r } , and [ O rr ] ,
the constraint matrix, is null due to the determinate foundation { U r } .
For the case of DDAM requirements, response of a structure to an imposed foundation
motion
··
··
{ U r } = { Γ }U s ( t )
Eq. 8-10
is sought. The array { Γ } serves as a directional vector for the applied motion history,
··
U s ( t ) for example, if it is directed in the U r1 sense (x direction) then Γ 1 = 1 , Γ 2 = 0 , ...
Γ 6 = 0 . From the upper partition of Eq. 8-8, the modal response equation is obtained
as
··
2
··
[ l ll ] { q 1 } + [ ω 1 ] { q 1 } = – [ P lr ] { Γ }U s ( t )
Eq. 8-11
The individual mode equations are
··
2
··
q i ( t ) + ω i q i ( t ) = – [ P lr ] { Γ }U s ( t )
Eq. 8-12
for mode “I” excited by a shock in the “j” direction. The foundation reaction forces are
determined by the lower partition of Eq. 8-8 as
··
··
··
{ F r } = [ P rl ] { q l } + [ M rr ] { Γ }U s ( t )
Eq. 8-13
In DDAM analysis, the second term is Eq. 8-13 is neglected, due to the assumption of
··
an extremely short duration applied shock, so that the U s ( t ) is zero by the time each
modal response reaches its peak value. Thus, the reaction force in the “j” direction is
determined by the summation of individual modal reactions F ij which are
··
F ij = P ij q i ( t )
Eq. 8-14
Consider now the response to an impulsive shock occurring over the duration 0 ≤ t ≤ t s s
which is much shorter than the period of any mode under consideration. Integrating
Eq. 8-12 over the shock duration results in
ts
·
q i ( t s ) = – P ij V ai
Eq. 8-15
where the term ∫ ωwi q i ( t ) is negligibly small since the modal displacement hasn’t had
enough time to 0 develop; and
··
V ij = P ij q i ( t )
Eq. 8-16
175
176
is the spectral velocity of the shock. The free response of mode “I” for t > t s is therefore
– P ij V ai
q i ( t ) = ------------------- sin ω i ( t – t s )
ωi
·
q i ( t ) = – P ij V ai cos ω i ( t – t s )
q i ( t ) = P ij ω i V ai sin ω i ( t – t s )
Eq. 8-17
The physical significance of the structure and foundation reactions are determined by
the modal superposition following Eq. 8-7 with Ur = 0 for t > t x and Eq. 8-14
respectively. Moreover, internal loads and stresses on the structure are determined by
stress recovery operations for the particular model described by the generic equation
σ
{σ} = [K ]{U}
Eq. 8-18
According to NAVSEA requirements (Reference (2)), a shock spectrum summation
method is adopted in which time phasing of modal responses is not considered. In
this approach the peak modal responses are utilized as
P ij V ai ⁄ ω i
q i peak =
·
q i peak =
P ij V ai
Eq. 8-19
··
q i peak = ω i P ij V ai
Individual modal peak physical responses are governed by the relationships of the
type
··
( U ki ) peak =
( F ji )
( σ ki )
peak
peak
=
=
··
φ ki q i peak
··
P ij q i peak
Eq. 8-20
σ
∑ K kj φ ji q i peak
It is interesting to note that substitution of the modal peak acceleration into the modal
reaction equation results in
( F ij )
peak
=
2
P ij ω i V ai
Eq. 8-21
where P ij 2 is the modal mass, i.e.
M ai =
P ij
2
Eq. 8-22
CHAPTER 8
DDAM Processor
The NAVSEA modal summation convention utilized in DDAM calculations follows
the generic form
N
R j = R jm +
∑
R ji
2
i = 1
(i ≠ m)
Eq. 8-23
Where R j is a generic response quantity and r jm is the largest modal response quantity
in the set r ji , I=1 to N (N = number of modes). It should be noted that the index “m”
is not necessarily the same for all physical responses. The current version of the
DDAM program performs the NRL summation following the latest specification in
Reference (2.). In this spec, the modes are added up in decreasing order of modal
mass, rather than in increasing order of frequency. The output now gives a
summation order so that the user can follow the process. Note that some modes may
be included in the sum for one shock direction but not included for another direction.
Up to this point, the value of the modal spectral velocities, V ai , have not been
discussed. Due to the flexibility and finite mass of the ship structure onto which the
structural system is mounted, the value of V ai is an empirical function of the modal
effective mass, M ai , and modal frequency, ωI . The actual formulae for the spectral
quantities are presented in Reference (4.), and the form of the equations are presented
in “Format of Coefficient File” on page 185.
An interesting property of modal effective mass is that the sum of the individual
terms, M ai , will approach the total actual mass of the system as the number of modes,
N, approaches the complete set for the mathematical model. The summation will
exactly approach the total system mass if no mass is allocated to the foundation
degrees of freedom { U˜ m } or { U r } . If mass is allocated to the foundation, the summed
effective mass will approach the total mass minus the foundation mass. For DDAM
analyses, NAVSEA allows utilization of a truncated mode set, which provides a
minimum of 50% of the total number of modes of the system. Because this
requirement is excessive for modern large-scale finite element models described by
thousands of degrees of freedom, NAVSEA accepts analyses that contain at least 80%
of the model’s effective modal mass. The number of modes required to achieve this
amount is highly model dependent, but frequently involves less than one hundred
modes, compared to thousands required by the 50% criterion.
177
178
8.4
Worked Two Mass Problem
Problem:
Consider the following arrangement:
2
m 1 = 8000lb = 20.70 lb-sec ⁄ in
2
m 2 = 6000 lb = 15.53 lb-sec ⁄ in
m2
x2
k2
k 1 = 500, 000 lb/in
k 2 = 200, 000 lb/in
m1
x1
k1
Step 1 - Calculate Natural Frequencies
Equation of motion from free body diagrams:
k2 ( x2 – x1 )
m1 x1
k1 x1
m2 x2
Summation of Forces:
∑ F1
··
= 0. = m 1 x 1 + k 1 x 1 – k 2 ( x 2 – x 1 )
= m 1 x 1 + ( k 1 + k 2 )x 1 – k 2 x 2
∑ F2
··
= 0. = m 2 x 2 + k 2 ( x 2 – x 1 )
··
= m2 x2 + k2 x2 – k2 x1
k2 ( x2 – x1 )
CHAPTER 8
DDAM Processor
or, in the more familiar matrix form:

m1 0 

0 m2 

··
x2
··
x2


 =



k1 + k2 –k2  x1

–k2
k2  x2



 0 
 = 


 0 

Step 2 - Solve the Equations
This can be done manually or using a computer, but the end result is the same.
Solution of these yields two modes with natural frequencies:
ω 1 = 89.72 rad/sec = 14.280 Hz.
ω 2 = 196.6rad/sec = 31.285Hz.
and corresponding eigenvectors. MSC/DDAM requires these to be “mass”
normalized, which can be accomplished by dividing each “max” normalized value by
the generalized mass [ M g ] = { φ } T [ m ] { φ } . Note that the generalized mass for a mass
normalized vector set will be 1 for all modes. The mass normalized eigenvectors will
be:
X1 =
.0873
.2329
X2 =
.2017
-.1008
Step 3 - Calculate the Participation Factors
They are determined from the following equations. Note that the participation factors
are normalization dependent. Also note that MSC.Nastran may have reversed the
signs on the second eigenvector. This simply changes some signs and the magnitudes
of the participation factors in the intermediate steps. The final solution is
independent of the normalization.
179
180
∑ X ia m i
P a = -----------------------------2
∑ ( X ia ) m i
X is
= eigenvectors, m i = individual masses
X 11 m 1 + X 21 m 2
( .0873 ) ( 20.70 ) + ( .2329 ) ( 15.53 )
P i = --------------------------------------------------------- = -------------------------------------------------------------------------------------- = 5.423
2
2
2
( .0873 ) ( 20.70 ) + ( .2329 ) ( 15.53 )
( X 11 ) m 1 + ( X 21 ) m 2
X 12 m 1 + X 221 m 2
( .2017 ) ( 20.70 ) + ( – .1008 ) ( 15.53 )
P 21 = --------------------------------------------------------- = --------------------------------------------------------------------------------------------- = 2.610
2
2
2
2
( .2017 ) ( 20.70 ) + ( – .1008 ) ( 15.53 )
( X 12 ) m 1 + ( X 22 ) m 2
Step 4 - Calculate the Modal Masses
Unlike the participation factors, the modal masses are not normalization dependent.
Note that the modal “masses” are really weights.
2
( ∑ X ia m i )
M a = -----------------------------2
∑ ( X ia ) m i
2
2
( X 11 m 1 + X 21 m 2 )
[ ( .0873 ) ( 20.70 ) + ( .2329 ) ( 15.53 ) ]
M 1 = --------------------------------------------------------- = -------------------------------------------------------------------------------------------- = 11,368.lb
2
2
2
2
( .0873 ) ( 20.70 ) + ( .2329 ) ( 15.53 )
( X 11 ) m 1 + ( X 21 ) m 2
2
2
( X 12 m 1 + X 221 m 2 )
[ ( .2017 ) ( 20.70 ) + ( – .1008 ) ( 15.53 ) ]
M 2 = --------------------------------------------------------- = ----------------------------------------------------------------------------------------------- = 2,631.lb
2
2
2
2
( .2017 ) ( 20.70 ) + ( – .1008 ) ( 15.53 )
( X 12 ) m 1 + ( X 22 ) m 2
Step 5 - Choose the Shock Coefficients
We will choose “surface ship,” “deck” inputs. These correspond to the coef.dat file in
the sample directory. They do not represent any real spectrum, and only serve to
demonstrate the DDAM solution methodology.
F/A factor = 1.0
Athwartship factor = 1.0
Vertical factor = 1.0
AA = 50.
VA = 120.
AB = 40.
VB = 50.
AC = 10.
VC = 10.
CHAPTER 8
DDAM Processor
Step 6 - Calculate the Spectrum Inputs
The equations found here are of the same form as some formal specifications. The
values, however, are simply for demonstration purposes. Note that the W in the
equations represents the weight (not mass) in 1000s of pounds (kips). Also note that
the equations deliver the accelerations in Gs and the velocity in in/sec. These
conventions are hard coded into the ddam.f program.
Mode 1:
AA ( AB + M 1 )
50 ( 40 + 11.368 )
A 0 = ------------------------------------- = ------------------------------------------ = 120g
M 1 + AC
11.368 + 10
VA ( VB + M 1 )
120 ( 50 + 11.368 )
V 0 = ------------------------------------- = --------------------------------------------- = 344.6 in/sec
M 1 + VC
11.368 + 10
V0 ω
344.6 ( 89.72 )
A v = ----------- = -------------------------------- = 80.0 g
g
386.4
Since A v is less than A 0 , use A v for the calculation.
Mode 2:
AA ( AB + M 1 )
50 ( 40 + 11.368 )
A 0 = ------------------------------------- = ------------------------------------------ = 120g
M 1 + AC
11.368 + 10
VA ( VB + M 1 )
120 ( 50 + 11.368 )
V 0 = ------------------------------------- = --------------------------------------------- = 344.6 in/sec
M 1 + VC
11.368 + 10
V0 ω
344.6 ( 89.72 )
A v = ----------- = -------------------------------- = 80.0 g
g
386.4
This time, A v is larger than A 0 , so we use A 0 for the calculations here.
Step 7 - Use the Accelerations, Eigenvectors, Individual Weights,
and Participation Factors to Find the Dynamic Forces on the
Masses.
The weights are the individual weights, not masses or modal masses.
F ia = W i X ia P a A ( ω a )
181
182
Mode 1:
F 11 = W 1 X 11 P 1 A ( ω 1 ) = ( 8000 ) ( .0873 ) ( 5.423 ) ( 80.0 ) = 302,994. lb
F 21 = W 2 X 21 P 1 A ( ω 1 ) = ( 6000 ) ( .2329 ) ( 5.423 ) ( 80.0 ) = 606,248. lb
Mode 2:
F 12 = W 1 X 12 P 2 A ( ω 2 ) = ( 8000 ) ( .2017 ) ( 2.610 ) ( 169. ) = 711, 743. lb
F 22 = W 2 X 22 P 2 A ( ω 2 ) = ( 6000 ) ( -.1008 ) ( 2.610 ) ( 169. ) = – 266,771. lb
Step 8 - Use the Mass Forces to Get the Forces in the Springs:
Mode 1:
Spring 1 = 303.0 + 606.2 = 909,200 lb
Spring 2 = 606.2
= 606,200 lb
Mode 2:
Spring 1 = 711.7 - 266.8 = 444,900 lb
Spring 2 = -266.8
= 266,800 lb
Step 9 - Perform the NRL Sum of the Spring Forces.
Note that the NRL sum reduces to a trivial summation for this 2-mass case.
Spring 1 = 909,200 + 444,900 = 1,354,100 lb
Spring 2 = 606,200 + 266,800 = 873,000 lb
Step 10 - Calculate the Nodal Displacements and Velocities.
Since the deflection of each mode is an orthogonal mode shape, the displacements,
velocities and accelerations are related by:
A = V ω = xω
2
The accelerations can be simply calculated from:
F ia
A ia = -------Wi
CHAPTER 8
DDAM Processor
Mass 1, Mode 1:
F 11
302994.
A 11 = --------- = ------------------- = 37.87 g
8000
W1
A 11
37.87 ( 386.4 )
in
V 11 = --------- = -------------------------------- = 163.1 -------89.72
ω1
sec
A 11
37.87 ( 386.4 )
x 11 = --------- = -------------------------------- = 1.818 in
2
2
( 89.72 )
ω1
Mass 2, Mode 1:
F 21
606248.
A 21 = --------- = ------------------- = 101.04 g
6000
W2
A 21
101.04 ( 386.4 )
in
V 21 = --------- = ----------------------------------- = 435.2 -------89.72
ω1
sec
A 21
101.04 ( 386.4 )
x 21 = --------- = ----------------------------------- = 4.850in
2
2
ω1
( 89.72 )
Mass 1, Mode 2:
F 12
711743.
A 12 = --------- = ------------------- = 88.97g
8000
W2
A 12
88.97 ( 386.4 )
in
V 12 = --------- = -------------------------------- = 174.9 -------ω2
196.6
sec
A 12
88.97 ( 386.4 )
x 12 = --------- = -------------------------------- = .8894 in
2
ω2
( 196.6 )
Mass 2, Mode 2:
F 22
– 266771
A 22 = --------- = --------------------- = 44.46g
W2
6000
A 22
44.46 ( 386.4 )
in
V 22 = --------- = -------------------------------- = 87.38 -------196.6
ω2
sec
A 22
44.46 ( 386.4 )
x 22 = --------- = -------------------------------- = .4445 in
2
2
ω2
( 196.6 )
183
184
Step 11 - NRL Sum the Velocities, Displacements and Accelerations
Like the forces, this is a trivial summation for this sample problem.
Mass 1:
x =1.818 + .8894 = 2.707 in
V =163.1 + 174.9 = 338.0 in/sec
A = 37.87 + 88.97 = 126.84 g
Mass 2:
x2 = 4.850 + .4445 = 5.295 in
V2 = 435.2 + 87.38 = 522.6 in/sec
A2 = 101.04 + 44.46 = 145.50 g
This sample problem is provided as the d1 model in the sample files. In the output
note that directions 2 and 3 are all 0, as those degrees of freedom were constrained out.
Only the X direction results and X directed shock (F/A) have any meaning.
CHAPTER 8
DDAM Processor
8.5
Format of Coefficient File
The DDAM coefficient file contains the weighting factors used for the response
calculations, the directional scaling factors, as well as the modal mass cutoff value.
The file is structured as shown below. The default equations to which these apply are:
(M is the modal weight in kips for that mode)
AA ( AB + M )
A 0 = AF ---------------------------------AC + M
VA ( VB + M )
V 0 = VF ---------------------------------VC + M
For surface ship, hull and shell mount, the equation is:
AA ( AB + M ) ( AC + M )
A 0 = AF ------------------------------------------------------------( AD + M )
There is a complete set of AA, AB, AC, and (when needed) AD weighting factors for
each of the possible analysis configurations (surface ship and submerged ship, deck
mount, shell mount and hull mount). In addition, there is a trio of AF (acceleration
factors) and VF (velocity factors) for each of these sets, one for each shock direction.
There are additional factors for Elastic-Plastic design.
The file is formatted sort of like an MSC.Nastran file. Each set of coefficients and
factors are entered on a COEF entry that describes the applicability of that set of
factors. The COEF entry is formatted like a NASTRAN statement - i.e. ten eight
character fields. The entry looks like:
1
COEF
2
3
4
5
6
7
nsurf
nstruc
nplast
VF(1)
VF(2)
VF(3)
AF(1)
AF(2)
AF(3)
VA
VB
VC
AA
AB
AC
8
9
10
AD
nsurf
ship type. Allowable values are SUB (submerged) and SURF (surface
ship)
nstruc
mounting location. Allowable values are DECK, HULL, and SHELL
nplast
elastic or elastic-plastic factors. Allowable values are ELASTIC and
ELPL.
The (i) in the VF and AF refer to the directions: (1)=fore/aft, (2)=athwartship, and
(3)=vertical
A blank entry or a * entry in any field will use the default value (from the program
source) for that value.
185
186
In addition to the COEF entry defining coefficients, there is a CUTOFF entry that
defines the modal mass cutoff percentage. That entry looks like:
CUTOFF
pref
pref is the cutoff weight percentage for the modal mass calculation. Enter as a
percentage, not a decimal fraction (i.e. 85. instead of .85). Note that you still have the
option of overriding this value when you run the program.
pref
100. Use all available modes.
nn. Make spectral values zero for all modes beyond the one that first exceeds
nn percent of the total mass.
A sample coef.dat file to analyze different surface ship equipment using the elasticplastic factors might look like:
# special elastic-plastic surface ship factors
# - deck coefficients
COEF
SURF
DECK
ELPL
.25
.50
1.0
.25
.50
10.
20.
50.
10.
37.5
# - hull coefficients
COEF
SURF
HULL
ELPL
.30
.60
1.0
.25
.50
5.
10.
40.
10.
45.5
# - shell coefficients
COEF
SURF
SHELL
ELPL
.25
.50
1.0
.25
.50
*
*
*
10.
45.5
1.0
6.
1.0
6.5
15.
1.0
6.5
15.
It is important that all fields be 8 characters (or spaces) long, as there is a bug in the
read routine (that should have been fixed for MSC.Nastran 2005) that requires this.
This is easily achieved by padding the ends of lines with blanks to achieve the full 8character length.
CHAPTER 8
DDAM Processor
8.6
Control File Format
The control file is simply a list of responses to the questions that the DDAM Fortran
program asks. The format can be any one of three, depending on which user options
are being requested.
No special user options:
F F T
nsurf nstruc nplast
pref
amin
f/a_axis vert_axis
.f11 filename
.f13 filename
.ver filename
User coefficient option:
T F T
coef.dat filename
nsurf nstruc nplast
pref
amin
f/a_axis vert_axis
.f11 filename
.f13 filename
.ver filename
User spectrum Option:
F T T
spec.dat filename
pref
amin
f/a_axis vert_axis
.f11 filename
.f13 filename
.ver filename
Specific file formats as follows:
• First Line – spectrum control – format a1,1x,a1,1x,a1
• First item – DDAM or general spectrum run flag
T = General non-DDAM spectrum run
F = DDAM
• Second item – Coefficients from File or form compiled source
T = coefficients from external file
187
188
F = use built-in coefficients
Ignored if first item is T
• Third item – Equation format
T = DDS-072 style equations
F = NRL 1396 style equations
Ignored if first item is T
• Second Line – file name (if needed) – format a80
• If 1st item on line 1 is T
Name of spectrum file
• If 2nd item on line 1 is T
Name of coefficient file
• If neither are T, line is not needed
• Third Line – location flags – format i1,1x,i1,1x,i1
• First item – Surface or Submarine
1 = Surface
2 = Submarine
• Second item – equipment location
1 = Deck
2 = Hull
3 = Shell
• Third item – coefficient class
1 = Elastic
2 = Elastic/Plastic
• 4th Line – Weight cutoff percentage – format F8.3
• Cutoff percentage (0. To 100.)
th
• 5 Line – Minimum G cutoff – format F8.3
• Minimum G level to use (in Gs)
• 6th Line – Axis Orientation – format a1,1x,a1
• First item – F/A axis
CHAPTER 8
DDAM Processor
X, Y, or Z
• Second item – Vertical Axis
X, Y, or Z
• 7th Line – Input file – format a80
• Name of file (full path if needed)
• 8th Line – Output file – format a80
• Name of file (full path if needed)
th
• 9 Line – verification file – format a80
• Name of file (full path if needed)
• These names will be ignored if they are passed as arguments when the
DDAM program is run.
Note that the spacing of the first line and the axis definition line are important, as are
the capitalization. The first line must be in the FORTRAN format (a1, 1x, a1, 1x, a1),
with the T or F capitalized. The axis line is the same format, but with X, Y, or Z for
each term. A sample file for a conventional analysis might look like:
F F T
1 1 1
100.
1.0
X Z
d1.f11
d2.f11
d1.ver
189
190
8.7
User defined Shock Spectra
This section describes the program package that allows for defining a user input shock
spectrum. Not to be confused with the user input shock coefficients, this routine
allows the user to completely define the spectrum as data pairs of frequency and some
motion quantity (displacement, velocity or acceleration). The user can define the
spectrum in selected units, as outlined in the following section. The frequency scale
and/or the disp/vel/accel scale can be either logarithmic or linear, as frequency and
value ranges often cover several orders of magnitude.
The data is entered into a user created file, which can have any arbitrary name. In
general, the file is fairly simple:
# = comments, anywhere in file
DATATYP type
data1
dir
BEGIN DATA
f1, data1
f2, data2
...
fn, datan
[BEGIN DATA]
[f1, data1]
[f2, data2]
[...]
[fn, datan]
[BEGIN DATA]
[f1, data1]
[f2, data2]
[...]
[fn, datan]
END FILE
freq
interp
The data on the DATATYP entry are as follows:
type
describes what motion quantity is described in the following data.
Type can be one of the following: DISP, VELO, or ACCE.
data
describes the units that the motion is described in. Data can be one of
the following: G (acceleration data in Gs), F (Displacement, Velocity or
Acceleration data in feet, ft/sec, or ft/sec2), I (displacement, velocity or
acceleration in inches, in/sec or in/sec2), or M (displacement, velocity
or acceleration in meters, m/sec or m/sec2)
CHAPTER 8
DDAM Processor
dir
describes how many spectra are in the file. dir can be 1 (a single
spectrum will be used for all three shock directions), or 3 (there are
three spectra in this file, one for each direction)
freq
describes the units for the frequency terms. Choices are RAD
(radians) or HERTZ (frequency in hertz).
interp
describes the axis/plot type. Data can be any one of the following:
LOGLOG (both axes are logarithmic), LINLIN (neither axis is
logarithmic), LOGLIN (the frequency axis is logarithmic, the other is
not), or LINLOG (the frequency range is linear, the other is
logarithmic).
The BEGIN DATA entry precedes each frequency/motion data section. If dir=1, there
will be only one BEGIN DATA entry, if dir=3, there will be three, one preceding each
section.
The data section is ended with the END FILE entry. This is included to remove the
machine-specific vagaries of reading to the end of a file.
FILES CONTENTS AND ENTRY NAMES ARE CASE SENSITIVE - USE CAPITAL
LETTERS!
Sample user spectrum data file:
# sample spectrum file
#
2
3
4
5
6
DATATYP ACCE
I
1
HERTZ
LOGLIN
# acceleration vs frequency file - acceleration in in/sec**2
BEGIN DATA
1. 1.
10. 10.
100. 1000.
# point added to define range
500. 800.
1000. 500.
END FILE
191
192
8.8
MSC.Patran Interface
Starting in Version 2004, MSC.Patran has an analysis option that enables you to set up
and run a DDAM analysis. The MSC.Patran interface will create the control file, write
the file assignments, and allow entry of the SUPORT card. Any type of DDAM
analysis can be run from within MSC.Patran, including the coefficient runs and userinput spectrum runs. The program performs several checks on the data that is entered
to prevent the user from accidentally entering bad data and then trying to run the
model.
Program Operation:
Choosing the “Solution Type” from the main analysis menu will bring up the
following form:
CHAPTER 8
DDAM Processor
The “Solution Parameters” button brings up the following form:
On the Subcase parameters form, most of the rest of the DDAM input is entered. That
form looks like:
193
194
The “Spectrum Source” option
menu has two choices, COEFs and
FILE.
• “COEFs” will instruct
DDAM to obtain the shock
spectrum and spectral
accelerations from a set of
coefficients.
• “FILE” allows input of a
general spectrum not
determined by
coefficients. If “FILE” is
chosen, the file can be
chosen using the “Spec
Source…” button that will
appear.
The “Coef Source” option menu
dictates where the coefficients are to
be found.
• "DEFAULT” will use the
coeffiecients that are hard
coded into the DDAM
program.
• “FILE” will pull them from
a file previously created by
the user, who must then
pick the file using the
“Coef File…” button that
will appear.
If the Spectrum Source is “FILE”, then the “Coefficient Options” items are enabled.
Each menu has several choices that will allow the user to choose which set of
coefficients is desired. If the coefficients are coming from a file, and the file does not
contain coefficients for the particular configuration that has been specified, the
default coefficients will be used. At the moment, no warning of this is given.
“Ship Type” can be “SURFACE” or “SUBMERGED”
“Mount Location” can be “DECK,” “HULL,” or “SHELL.”
CHAPTER 8
DDAM Processor
“Elastic/Plastic” can be “ELASTIC” or “PLASTIC” reflecting the use of the elastic
design coefficients, or the elastic/plastic design coefficients.
“Weight Cutoff” controls how many modes are used for the NRL sum. All modes up
to the specified modal mass percentage specified will be included in the NRL sum for
each direction. The “DEFAULT” switch will use the percentage that is hard coded
into the DDAM program. If the “ENTER VALUE” switch is chosen, the cutoff should
be entered as a percentage, not a decimal (e.g. 90. instead of .90).
“Minimum G Level” controls whether the calculated spectra values should be
replaced with a minimum if they fall below a certain threshold. The “N/A” switch
will use the value that is calculated, regardless of its magnitude. If the “ENTER
VALUE” switch is chosen, the minimum cutoff should be entered as a G value (e.g 1.0.
instead of 386.4).
The two axis toggles tell DDAM which direction of the model is oriented in the
fore/aft and vertical directions. Each button has possible choices of “X,” “Y,” and “Z.”
An error will be issued if both axes are set to be the same.
195
196
MSC.Nastran 2005 Release Guide
CHAPTER
9
Miscellaneous
■ MSC.Nastran ADAMS Integration
■ Alternative Solution Algorithms for Flutter Analysis
■ Little - Big Endian
■ Reduced OP2 File SET Consistency Check
■ SPC and SPCD Entries in Machine Precision
■ Reading of PUNCHed Long Field Format Bulk Data
■ New Complex Conjugate Option for Matrix Multiplication
■ Acceleration Loads (ACCEL and ACCEL1 Bulk Data Entries)
■ A Caution Concerning MSC.Access Application Development
■ Divergent Thermal Results Error Correction (Q1-0768221)
■ Displacement Output Filters
■ Write Results Recovery for Subcases into Separate F06 Files
198
9.1
MSC.Nastran ADAMS Integration
Overview
An additional capability has been added to allow the user to create a MSC.ADAMS
modal neutral file (MNF) that does not contain any modal data. The purpose for this
would be to aid model checkout, and to determine the location of attachment points.
A RIGID option has been added to the mass invariant MINIVAR describer on the
ADAMSMNF Case Control command:
ADAMSMNF FLEXBODY=YES, MINVAR=RIGID
Also, PARAM,AUTOQSET,YES can be used with this option that allows the required
SPOINTs and QSETs to be supplied by the program automatically. This parameter
should specified in the Case Control Section, above Subcase level.
Limitations
This option will work for a residual structure only model.
If PARAM,AUTOQSET,YES is specified to automatically generate SPOINT and QSET
entries, then there should be no SPOINTs or QSETs present in the bulk data.
In order to determine the location of attachment points, there should be no SPOINTs
or QSETs present in the bulk data, and PARAM,AUTOQSET,YES should not be
present in the Case Control Section.
CHAPTER 9
Miscellaneous
9.2
Alternative Solution Algorithms for Flutter Analysis
Introduction
Two new flutter solution algorithms are available in MSC.Nastran 2005. These two
methods complement the existing PK,K,K-E and PKNL methods, and are referred to
as PKS and PKNLS. The S signifies ‘sweep’ and is meant to indicate that these
methods use a sweep technique to determine the flutter eigenvalues. By contrast, the
PK and PKNL methods employ an iterative approach that relies on roots found at one
estimated k (reduced frequency) value to estimate the roots at the next estimated k.
This iterative process sometimes encounters a flutter analysis task that cannot be
solved completely so that only a limited set of results are obtained. When this occurs,
a message is printed:
**** (USER WARNING MESSAGE 4581 (FA1PKE)
PK FLUTTER ANALYSIS FAILED TO CONVERGE FOR LOOP xx, ROOT yy
Figure 9-1 shows a comparison of extracted and estimated reduced frequency values
and shows how the iterative scheme can break down. It is seen that most of the
estimated roots line up in straight lines that are almost invariant with respect to the
estimated frequency. However, one root starts at a kext of 3.0 and falls rapidly to kext
= 0.0, crossing the 45 degree line near kext=1.0. It is this root that gives the P-K
algorithm trouble since its order changes as kest increases, violating an assumption of
the algorithm.
199
200
vel = 200 kts, e3609
7.00
Series1
6.00
Series2
kext
5.00
Series3
4.00
Series4
3.00
Series5
Series6
2.00
Series7
1.00
Series8
Series9
0.00
0.00
1.00
2.00
3.00
4.00
Series10
5.00
kest
Figure 9-1 Reduced Frequency Sweep for A Test Deck Results in a Failure to
Converge Message with the PK Method.
The PKS method simply sweeps across the k-range with a series of complex
eigenanalyses at each of the estimated k-values. A determination is made as to when
the 45 degree line is cross and the corresponding flutter root is stored.
Benefits
The FAILURE TO CONVERGE message is no longer issued, while the other benefits
of the PK method (ability to deal with real roots, better estimate of complex roots, and
use in optimization) are retained.
Input
The existing FLUTTER Bulk Data interface has been enhanced with additional input
as given by the following table (with the modified inputs indicated in bold):
1
2
3
4
5
6
7
8
9
FLUTTER
SID
METHOD
DENS
MACH
VEL
IMETH
OMAX/N
VALUE
EPS
FLUTTER
10
PKNLS
1
2
3
L.
10
CHAPTER 9
Miscellaneous
Field
Contents
METHOD
PKS and PKNLS augment the existing K, KE, P-K and PKNL
methods. See Remark 9.
OMAX
The maximum frequency for the frequency sweep in Hertz. (Real >
0.0), See Remark 10.
EPS
The inverse of the number of equal reduced frequency steps used in
the frequency sweep. (Real > 0.0, Default = .01)
Remarks:
9. The PKS and PKNLS methods determine the flutter eigenvalues by
performing a sweep of reduced frequencies ranging from kest = 0.0 through
kest = π CREF OMAX/ Velocity.
10. OMAX specifies the maximum frequency in Hz. If this field in an integer, it
corresponds to the current NVALUE parameter that provides the number of
eigenvalues to be extracted. If the field is blank, the default is the number of
modal degrees of freedom in the flutter analysis.
Outputs
The output from the PKS and PKNLS methods are quite similar to those of the PK and
PKNL methods. The METHOD selected is printed in the flutter summary. DIAG 39
can be used display the eigenroots for each estimated k value, but this will produce a
large amount of output.
In SOL 200, formatted prints of the density value are now the actual density value
rather than the density ratio.
Guidelines and Limitations
• It is suggested that the PK and PKNL methods be the primary flutter
algorithms with PKS and PKNLS reserved for cases where the former
methods do not appear to be performing well.
• An attribute of the new methods is that they can produce more roots at a
given velocity than there are normal modes. This is deemed a valid result but
is counter to most current flutter methods, including those used in
MSC.Nastran. This can produce a difficult sorting task when more (or fewer)
roots are extracted at one velocity than were extracted at an earlier velocity.
MSC.Nastran attempts to cope with this and puts the new roots at POINTs
above those from of the previous velocities.
201
202
• The PKS and PKNLS methods can be applied in SOL 200
• DIAG 39 can be used in the PK and PKNL methods to provide insight into
the iterative root extraction process. Additional output is available with PKS
and PKNLS as well, but it can be voluminous for most problems.
Example (pkswep.dat)
This is the HA145A example of the MSC.Nastran Aeroelastic User’s Guide with a single
subcase applying the PKS method. The FLUTTER Bulk Data entry in this case is:
1
2
3
4
5
6
7
8
9
FLUTTER
3
PKS
1
2
3
L
5.
.01
10
The PKS method is selected and a maximum frequency of 5.0 Hz. is used in the sweep
and the sweep region is divided in 100 equally spaced frequencies ranging from 0.0 to
5.0 HZ.
The output flutter summary is headed by:
CONFIGURATION = AEROSG2D
ASYMMETRIC
POINT =
1
MACH NUMBER =
0.0000
FLUTTER SUMMARY
XY-SYMMETRY = ASYMMETRIC
DENSITY RATIO =
1.0000E+00
XZ-SYMMETRY =
METHOD = PKS
Where the METHOD=PKS indicates that the PKS method has been selected.
CHAPTER 9
Miscellaneous
9.3
Little - Big Endian
Variable Endian OUTPUT2 and OUTPUT4 Files
Introduction
Major MSC.Nastran customers typically use the program in batch mode, on a remote
mainframe computer, or cluster, requiring transfer of the model and results data
between the remote machine and the local workstation. The amount of results data is
often significant, so binary file formats are preferable with more efficient data storage
and access. However, different types of machines have different formats, and so
transferring data from one format to another involves a process of “transmitting”
(from the remote machine) to a neutral format, copying the neutral format results data
over to the local workstation, and “receiving” (to the local workstation) to rebuild a
compatible binary file. Such a process is cumbersome and requires large amounts of
disk space and can lead to reduced accuracy through loss of precision.
Benefits
MSC.Nastran has been enhanced to allow the user to specify the format in which
binary OP2 and OP4 (OUTPUT2 and OUTPUT4) files are generated, regardless of the
computer platform on which MSC.Nastran is running (note that this new capability
will not be available on Cray UNICOS). Therefore, a user running MSC.Nastran on a
platform such as Linux/i386 (the source machine) can request that a generated OP2/4
file be suitable for a platform such as IBM AIX or Hewlett-Packard HP-UX (the target
machine). This allows the OP2/4 file to be used by post-processing programs running
on the target machine directly, without having to go through a TRANS/RECEIVE
data transfer process. This increases ease of use, reduces disk requirements, and
overall processing time.
The target machine specification is entered through new options for the FORM
qualifier on the OUTPUT2 and OUTPUT4 ASSIGN statements in the File
Management Section of the input bulk data.
The benefits for OUTPUT4 files are even greater. MSC.Nastran on all platforms
(except Cray UNICOS) will be able to read binary OUTPUT4 files from any platform
(except Cray UNICOS) directly, and without the need for any intermediate
translation. Also, for users who read OUTPUT4 files into their own programs, a
translation program will be available that will allow binary OUTPUT4 files to be
copied and transformed from one format to another.
203
204
Theory
The term “Endian” refers to the byte ordering for numeric data used by a particular
computer architecture. “Big Endian” specifies that the most significant byte (MSB) of
a data element is stored at the lowest byte address, while “Little Endian” specifies that
the least significant byte (LSB) of a data element is stored at the lowest byte address.
Most UNIX platforms (i.e., almost all except Compaq Alpha) are big-endian machines,
while all Intel x86 and compatible platforms (e.g., Intel-Pentium and AMD Athlon,
including those running both Windows and Linux) are little-endian machines. Some
machines, like Intel Itanium, can be run in either big-endian mode (e.g., when running
HP-UX), or in little-endian mode (e.g., when running Linux or Windows).
Inputs and Outputs
The OUTPUT2, OUTPUT4, and INPUTT4 modules have been modified to allow the
user to specify the format of a binary file generated by these modules, i.e. whether the
file is to be in “big-endian” format or “little-endian” format. The ASSIGN statement
is used to assign physical files used by MSC.Nastran to FORTRAN units, and the
desired output format is specified using the FORM= option.
For FORTRAN files, the format of the ASSIGN statement is:
ASSIGN logical-key[={filename|*}] [UNIT=u] [[STATUS=]{NEW|OLD|UNKNOWN}]
[[FORM=]{FORMATTED|UNFORMATTED|BIGENDIAN|LITTLEENDIAN|LTEND|<ostype>}] [DEFER]
[{TEMP|DELZERO}] [DELETE] [SYS=’sys-spec’]
In addition, for OUTPUT4 files a new utility program (OP4UTIL) has been developed
that can test and convert OUTPUT4 files from one endian format to another.
The OP4UTIL utility may be used to validate, copy, or reformat binary files created
using the MSC.Nastran OUTPUT4 module. The basic format of the “op4util”
command is:
Msc2004 op4util <options> <file names>
These capabilities are available on all platforms except Cray Unicos.
Examples
To specify the endian format, the ASSIGN statement is used as follows:
Set the default OP2 file format to BIGENDIAN and assign two OP2 files, one to unit
12 with filename ‘test_op2.12’, and one to unit 35 with filename ‘test_op2.35’ in ASCII
mode.
ASSIGN OP2 BIGENDIAN
...
ASSIGN OP2=’test_op2.12’ UNIT=12
CHAPTER 9
Miscellaneous
ASSIGN OP2=’test_op2.35’ UNIT=35 FORM=FORMATTED
The OP4UTIL program is used as follows:
To generate a usage/help message:
msc2004 op4util
msc2004 op4util –h[elp]
msc2004 op4util -?
To convert a file from one big-endian to little-endian or vice-versa:
Msc2004 op4util [-x[change]] [-v[erbose]] [-m nnn] <from_fname> <to_fname>
To convert a file from one endian format to a specified endian format:
Msc2004 op4util <Endian-opt> [-v[erbose]] [-m nnn] <from_fname> <to_fname>
205
206
9.4
Reduced OP2 File SET Consistency Check
Introduction
A procedure to reduce the size of the op2 file produced for use by MSC.Patran in postprocessing operations has been available as a DMAP alter since the release of
MSC.Nastran 2001. With the release of MSC.Nastran 2004, this procedure has been
incorporated into the MSC.Nastran DMAP and the alter is no longer required. To
employ the procedure, MSC.Nastran Case Control SET commands and DMAP
parameters are used. The procedure achieves its purpose by modifying the contents
of two of the data blocks that are stored on the op2 file during POST output
operations. The GEOM1 data block GRID point data record is modified so that it
contains only a specified sub-set of all of the grids available in the model. Likewise,
the element connection data records in the GEOM2 data block are modified so that
they contain data for only a specified sub-set of the elements available in the model.
The particular IDs to be retained in these data blocks are specified in SET list
statements in the Case Control Section of the input data file. The user specifies the SET
ID for the grid point list by assigning its value to the OGRDSET DMAP parameter.
Similarly, the SET ID value assigned to the OELMSET DMAP parameter specifies the
SET ID for the element list.
A new feature has been added to this procedure. This new feature ensures that all of
the grid points connected to elements contained in the element list SET are also
members of the grid point SET list. This test is called the SET consistency check. It is
always performed when both the grid point set and element set are specified.
Ensuring that the sets are consistent eliminates the problem sometimes encountered
in post-processors when the op2 data is loaded. Some post-processors will refuse to
load data for an element if the grid points connected to the element are not also
present.
Benefits
The enhancement to the reduced op2 file size feature ensures that the grid point list
used to “reduce” the grid geometry data contains all of the grid points that are
connected to elements in the element set used to “reduce” the element connection
data. Having a consistent set of data virtually eliminates the possibility of a postprocessor rejecting element data due to element connection grid point data being
missing. Until now, it has been up to the user to ensure that the grid point set was
consistent with the element set. With this new release of MSC.Nastran, that burden
has been removed from the user. MSC.Nastran will perform a consistency check of
the grid point set and terminate the run if any grid points connecting the elements in
the element set are missing from it. This improves user productivity in several ways.
CHAPTER 9
Miscellaneous
Less time is spent re-running jobs to get the correct amount of reduced output for the
op2 file. Less time is spent correcting the grid point set as all of the missing grid points
are identified by MSC.Nastran, and a revised SET can be punched at user option.
Method and Theory
The theory behind this new feature is very simple. Each and every grid point
connected to the elements in the element set should be present in the grid point set.
The method is equally simple. A list containing all of the points present in the model
is created. Next, each of the elements in the model is checked to see if its ID is in the
element ID set. If it is, then each of the grid points that the element connects is flagged
in the point ID list. Once all of the elements have been processed, each point in the
point list that has been flagged as touched by an element is tested to see if it is present
in the grid point ID set. If a point touched by an element is not present in the grid
point set, then a FATAL error message is issued and the job will be terminated. The
grid point set is also checked to see that every point in it was flagged during the
element set processing that produced the element-related grid list. For each point in
the grid point set that is not in the element-related grid point list or is not in the model,
a WARNING message is issued. The element-related point ID list can be punched in
Case Control SET format.
There are two other options available when using this new feature. Both options
relate to how the content of the final point ID set list is created that controls the content
of the GEOM1 grid point data record. One option simply uses the element-related list
of point IDs as the grid point set. For this option, set consistency is guaranteed. The
other option merges the input grid point set into the element-related list of points and
uses the merged set of points as the grid point set. For this option, set consistency is
not checked.
Inputs
The new set consistency check operation is automatically performed in MSC.Nastran
when both the element set and the grid point set are specified. The reduced op2 file
size capability already available in MSC.Nastran 2004 is controlled by the OELMSET
and OGRDSET DMAP parameters and the specification of the associated Case
Control SET lists. The OELMSET parameter value identifies the ID of the SET
containing the IDs of the elements that are to be retained on the op2 file. The
OGRDSET parameter value identifies the ID of the SET containing the IDs of the grid
points that are to be retained on the op2 file. Several additional parameters have been
introduced with the new set consistency check feature. All of the parameters
associated with the reduced op2 file size and set consistency check feature are now
summarized.
207
208
OELMSET – Integer – Default=0. Identification number of a Case Control command
SET definition. The members of the specified SET represent the identification
numbers of the finite elements that are to be retained in the “reduced” op2 file element
connection data block.
OGRDSET – Integer – Default=0. Identification number of a Case Control command
SET definition. The members of the specified SET represent the identification
numbers of the grid points that are to be retained in the “reduced” op2 file grid
geometry data block.
OPCHSET – Integer – Default=0. SET punch request flag. If OPCHSET=1, then the
list of grid points used to reduce the grid point geometry data block will be punched
in Case Control SET definition format.
OMSGLVL – Integer – Default=0. Set consistency check error message severity flag.
The default causes FATAL messages to be generated if the grid set is not consistent
with the element-related grid point set and the job is terminated. If OMSGLVL=1, the
FATAL messages are reduced to WARNINGS and the job is allowed to continue.
OGRDOPT – Integer – Default=1. Selects the method used to create the set of grid
points retained in the reduced grid point geometry data block. The default simply
uses the set of grid point IDs listed in the OGRDSET Case Control SET. Set consistency
is checked. OGRDOPT=2 uses the list of grid point IDs that are connected to elements
in the OELMSET Case Control SET. OGRDOPT=3 merges the contents of the
OGRDSET Case Control SET with the contents of the grid point list connected to the
elements in the OELMSET Case Control SET. There is no consistency check for
OGRDOPT=2 or OGRDOPT=3. OGRDOPT=0 turns the SET consistency check off
altogether. For this case, the grid points retained are those specified in the OGRDSET
SET and the elements retained are those specified in the OELMSET SET.
Outputs
The SET consistency check feature of the reduced op2 file size capability produces no
printed output other than standard format MSC.Nastran FATAL and/or WARNING
messages. Punched output can be produced at the user request. The punched output
consists of a Case Control SET of the grid point IDs that are consistent with the
OELMSET Case Control SET of elements.
Guidelines and Limitations
• Large THRU ranges in the grid point Case Control SET definition can
generate large amounts of informational messages if the grid points in the
THRU range are not present in the model.
CHAPTER 9
Miscellaneous
• SPOINT IDs are treated as GRID point IDs. The SPOINT data record on the
element connection data block (GEOM2) is not modified if it exists.
• Rigid element connections are ignored. Only finite element connectivity is
examined for attached grid points.
• If duplicate element IDs across element types are encountered, no warning
message is generated. All elements with same ID will be processed if the ID
is in the OELMSET Case Control SET.
• This feature is active only when op2 postprocessing file generation is
requested for the MSC.Patran program (v3 or higher) (param,post,-1) with
geometry output.
• Case control grid point related output requests (e.g., DISP) must reference
the OGRDSET Case Control SET. Case control element stress, strain and
force requests (e.g., STRESS) must reference the OELMSET Case Control
SET.
• Not available when superelements are present.
Demonstration Example
A simple example is presented that demonstrates the set consistency check feature.
The model is composed of a series of disjoint elements and is not intended to be
representative of any actual modeling situation. Two SETs are defined in the Case
Control Section. The members of SET 100 are the IDs of elements that are to be
retained on the reduced op2 element connection geometry data block. This SET ID is
specified as the value of the OELMSET parameter and is entered in the Bulk Data
Section using a PARAM Bulk Data entry. It is also referenced by the FORCE Case
Control command. The members of SET 200 are the IDs of grid points that are to be
retained on the reduced op2 grid point geometry data block. This SET ID is specified
as the value of the OGRDSET parameter and is entered in the Bulk Data Section using
a PARAM Bulk Data entry also. It, too, is also referenced by the DISP Case Control
command.
Note: These PARAM entries could be placed in the Case Control Section instead of
the Bulk Data Section.
Example files mass.dat and mass_bs.dat can be found in the TPL.
Example Input Data (TPL: rop2s*.dat)
NASTRAN SYSTEM(361)=1
$
209
210
$=======================================================================
$
$ Particular features of this example:
$ 1) the element ID set is SET 100. It has a thru range that includes
$
non-existent elements. There is no informational output for this
$
condition. SET 100 is selected via param,oelmset,100 bulk data
$
entry.
$ 2) the point ID set is SET 200. It contains point ID 5 which does
$
not exist in the model. It also contains point 1005 which exists,
$
but is not referenced by an of the elements in SET 100. Both of
$
these conditions cause informational messages to be generated.
$
SET 200 is selected via param,ogrdset,200 bulk data entry.
$ 3) the element ID set (SET 100) produces an element-related point ID
$
set to be generated that contains several points that are not in
$
the point ID set (SET 200). This condition generates FATAL
$
messages and causes termination of the run unless the OMSGLVL
$
parameter is set to 1, which reduces the messages to WARNING level
$
only and the run continues.
$ 4) the element-related point set is punched in case control SET
$
format due to the presence of the param,OPCHSET,1 bulk data entry.
$
This set could be used to replace the existing point ID set on
$
a subsequent run and as long as the element set SET remained the
$
same, the two would produce a consistent set of data.
$
$ Example Summary:
$ 1) SETs supplied are not consistent.
$ 2) Element-related point set is punched in case control SET format.
$
$=======================================================================
$
SOL 101 $ STATIC ANALYSIS
CEND
$
DISPL = 200
FORCE = 100
LOAD = 85
MPC = 1
set 100 = 27,35,25,41234,123,thru,134,9701,9901
set 200 = 1,thru,5,1005
BEGIN BULK
param,post,-1
$
$ tested feature controls
$
param,oelmset,100 $ select reduced element SET ID from case control
param,ogrdset,200 $ select reduced point
SET ID from case control
param,opchset,1
$ punch element-related point set in SET format
$ param,omsglvl,1
$ WARNING message only
$
spoint,20001,21001
spoint,30001
celas3,9701,175,20001
celas3,9702,175,21001
celas3,9801,175,30001
celas3,9901,175,40001
$
GRID
777
10.
0.
0.
.
.
CHAPTER 9
Miscellaneous
.
ENDDATA
Example Output
The example problem contains inconsistent sets. The MSC.Nastran run terminates
with FATAL messages identifying the inconsistencies as shown in the following
excerpt from the .f06 listing.
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 21 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 22 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 111 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 121 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 171 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 181 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 20001 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER FATAL MESSAGE 7759 (MTM36A)
ELEMENT(S) IN SET 100 CONNECT(S) POINT ID 40001 NOT PRESENT IN GRID SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ALL POINTS CONNECTED TO ELEMENTS IN ELEMENT
SET.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER WARNING MESSAGE 7760 (MTM36A)
GRID SET 200 CONTAINS POINT ID 5 NOT PRESENT IN THE MODEL.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ONLY POINTS ACTUALLY IN THE MODEL.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
*** USER WARNING MESSAGE 7761 (MTM36A)
GRID SET 200 CONTAINS POINT ID 1005 NOT CONNECTED TO ANY ELEMENTS IN SET 200.
USER ACTION: MAKE SURE THAT THE GRID POINT SET CONTAINS ONLY POINTS ACTUALLY IN THE MODEL.
PROGRAMMER INFORMATION: MATMOD OPTION 36, SUB-OPTION 1
The fatal messages inform the user that grid points 21, 22, 111, 121, 171, 181, 20001 and
40001 are connected to elements in set 100 (the OELMSET) and that they are not
present in set 200 (the OGRDSET). The user is also warned that grid point ID 5 in set
200 is not a model grid point. In addition, a warning is issued for point 1005 in set 200.
This point was not connected to any of the elements in set 100.
The user has requested that the element-related set of grid points be punched. This
set of grid IDs is punched in Case Control SET format as shown.
SET 200 = 1,THRU,4,21,22,111,121,171,181,20001,40001
211
212
If the above SET 200 is used to replace the existing SET 200 definition, then the element
set and grid point set would be consistent and there would be no fatal messages
generated.
CHAPTER 9
Miscellaneous
9.5
SPC and SPCD Entries in Machine Precision
In previous versions, enforced displacement values defined on the SPC and SPCD
entries were always treated as single precision numbers. Under this enhancement the
SPC and SPCD entries have been converted to machine precision format. All real
values of these entries will be maintained in machine precision during all operations
in static analysis leading to more accurate computation of loads.
Limitation
The entry, GMSPC used for p-element analysis still remains in real single precision in
the bulk data interpretation.
213
214
9.6
Reading of PUNCHed Long Field Format Bulk Data
Large-field input format requires (at least) two lines for each Bulk Data entry. So, for
an entry with fields 5-9 blank, a continuation entry is necessary. A fatal error results if
a long-field entry does not contain at least one continuation entry. However, if
requested, the PUNCHed bulk data from this run would still be created with the bad
long-field format entry. This restriction has now been removed and a single line longfield format entry is now acceptable. Its PUNCHed bulk data would also be created
consistent with the input bulk data entry.
CHAPTER 9
Miscellaneous
9.7
New Complex Conjugate Option for Matrix
Multiplication
The MPYAD and SMPYAD modules have been enhanced to compute conjugate
matrix multiplication for complex matrices. The transpose flag DMAP parameter for
both modules has been extended as follows:
Transpose Flag
Meaning
0
No Transpose
1
Transpose
2
Conjugate and No Transpose
3
Conjugate and Transpose
Examples:
1. Compute [ D ] = [ A* ] [ B ] where [ A* ] is the complex conjugate transpose
of [ A ]
MPYAD
A,B,/D/3 $
2. Compute [ X ] = [ A ] ⋅ [ B ] [ C ] – [ F ] where [ B ] is the complex conjugate of
[B] .
SMPYAD A,B,C,,,F/X/3/1/-1/0/0/2 $
3. Compute [ X ] = [ U* ] [ K ] [ U ]
SMPYAD U,K,U,,,/X/3////3 $
215
216
9.8
Acceleration Loads (ACCEL and ACCEL1 Bulk Data
Entries)
Traditionally, MSC.Nastran users have used the GRAV Bulk Data entry to apply
acceleration loads. The GRAV load is applied on the overall structural model as a
uniform load.
Previously, MSC.Nastran was unable to apply an acceleration load that varied across
the structure. New Bulk Data entries, ACCEL and ACCEL1, have removed this
limitation. They allow the user to apply acceleration loads at individual grid points
or in a specified region. Both ACCEL and ACCEL1 loads are used in the same way as
other load entries (such as GRAV, FORCE, and MOMENT, etc.) through the
MSC.Nastran Case Control commands.
Examples showing the use of ACCEL and ACCEL1 are available in the TPL accelqr.dat and accel1qr.dat.
Example:
SOL 101
TIME 10
CEND
TITLE= UNIFORMLY VARYING ACCELERATION LOAD
SUBTITLE = ACCEL LOAD TEST DECK
AUTOSPC(NOPRINT)=YES
ECHO = SORT
SPC = 1000
DISP(PRINT)
= ALL
STRESS(PRINT) = ALL
OLOAD(PRINT ) = ALL
$
SUBCASE 1
LABEL= GRAVITY LOAD VARIES IN THE X DIRECTION FOR A SQUARE PLATE
LOAD = 1
SUBCASE 2
LABEL= GRAVITY LOAD VARIES IN THE Y DIRECTION FOR A SQUARE PLATE
LOAD = 2
$
BEGIN BULK
CQUADR 1
1
1
2
7
6
CQUADR 2
1
2
3
8
7
CQUADR 3
1
3
4
9
8
CQUADR 4
1
4
5
10
9
CQUADR 5
1
6
7
12
11
CQUADR 6
1
7
8
13
12
CQUADR 7
1
8
9
14
13
CQUADR 8
1
9
10
15
14
CQUADR 9
1
11
12
17
16
CQUADR 10
1
12
13
18
17
CQUADR 11
1
13
14
19
18
CQUADR 12
1
14
15
20
19
CQUADR 13
1
16
17
22
21
CHAPTER 9
Miscellaneous
CQUADR 14
1
17
18
23
22
CQUADR 15
1
18
19
24
23
CQUADR 16
1
19
20
25
24
$-------2-------3-------4-------5-------6-------7-------8-------9-------0------ACCEL
1
.267261 .534522 .801784 X
+
+
0.0
-32.2
4.0
-161.0
ACCEL
2
22
.267261 .534522 .801784 Y
+
+
0.0
-32.2
-4.0
-161.0
CORD2R 22
0.0
0.0
0.0
0.0
0.0
1.0
+
+
0.0
1.0
0.0
$-------2-------3-------4-------5-------6-------7-------8-------9-------0------GRID
1
0.0
GRID
2
1.00000
GRID
3
2.000000
GRID
4
3.000000
GRID
5
4.000000
GRID
6
0.0
1.0
GRID
7
1.00000 1.0
GRID
8
2.0000001.0
GRID
9
3.0000001.0
GRID
10
4.0000001.0
GRID
11
0.0
2.0
GRID
12
1.00000 2.0
GRID
13
2.0000002.0
GRID
14
3.0000002.0
GRID
15
4.0000002.0
GRID
16
0.0
3.0
GRID
17
1.00000 3.0
GRID
18
2.0000003.0
GRID
19
3.0000003.0
GRID
20
4.0000003.0
GRID
21
0.0
4.0
GRID
22
1.00000 4.0
GRID
23
2.0000004.0
GRID
24
3.0000004.0
GRID
25
4.0000004.0
MAT1
1
1.0+5
0.3
1.0
PSHELL 1
1
0.1
1
1
+
0
SPC1
1000
123456 1
6
11
16
21
ENDDATA
217
218
9.9
A Caution Concerning MSC.Access Application
Development
In anticipation of functional changes to the MSC.Access data base organization,
changes to the Application Program Interface (API) are being introduced during the
basic MSC.Nastran 2005 release. The changes occur in the user interfaces to the Open
routines for the keyed objects. These interfaces are:
OPENC – Create a Keyed Object
OPENR – Read or Update a Keyed Object
OPENSQ – Read a Keyed Object using Sequential Methods
Parameters made obsolete during the MSC.Nastran Version 66 releases are being
reused and redefined.
DBFLOC – Locate a Keyed Object within a Group of Logical Data Bases
An additional parameter has been added.
The user application should now provide a destination variable for the returned
information in the arguments to the DBFLOC, OPENR and OPENSQ interfaces.
Usage of a constant could result in premature application termination due an attempt
to modify protected storage. The definition of the KEY variable in other interfaces has
also changed, however until production release of the new functionality along with an
update MSC.Access Users Manual, the current application interface will remain
functional and provide a correct interfaces to any existing and current 2005 created
MSC.Access data bases.
Updated pages for the interfaces from the MSC.Access Users Manual are now
provided. The new access key, called BBB-Tree method, will be explained in the next
release.
Subroutine Name: DBFLOC
1. Entry Point: DBFLOC
2. Purpose: Locate and open an object among the open database(s)
3. Calling Sequence: CALL DBFLOC ( NAME, FILNUM, FLEN, FNUM,
KEYLEN,IRET )
NAME
Array-input
Dictionary entry of an object name
FILNUM
Integer-output
Logical file number assigned to the
opened object
CHAPTER 9
Miscellaneous
FLEN
Integer-output
The length of an instance for a keyed
object or the total length in words for a
sequential object
FNUM
Integer-output
The number of entries for keyed object or
"1" for sequential objects
KEYLEN
Integer-output
The key length in words for keyed
objects
Integer-output
Return code, conforming to
OPENR/OPENS error codes, or the
additional
IRET
101 - object format code is neither
RECORD or VECTOR
102 - dictionary entry could not be located
among open database(s)
4. Method: The object is first located, is possible, among the open databases by
search from low to high logical data enumeration. Once the first is located,
either OPENR or OPENS is used to depending upon its form. The OPENR
allows for application updates, while OPENS for sequential objects opens for
read-only. Statistics concerning the object size are also returned to the
application.
Subroutine Name: OPENC
1. Entry Point: OPENC
2. Purpose: Create new keyed object and return a logical file reference.
3. Calling Sequence: CALL OPENC
(DBNUM,NAME,WRDREC,FILNUM,KEYLEN,CLSTER,D3,D4,D5,D6,IRE
T)
DBNUM
Integer-input
Logical database number
NAME
Array-input
Dictionary entry and keyed object
name to create
WRDREC
Integer-input
Number of words per logical record in
object
FILNUM
Integer-output
Logical handle number assigned to
the object
219
220
KEYLEN
Integer-input
The number of words in the key
0-> Use Hierarchal Key Method
+n-> Use BBB-Tree Method
CLSTER
Integer-input
Clustering Method
0 -> Use standard Key clustering
algorithm
1-> Re-order keys for optimum entry
storage
D3
D4
D5
D6
Integer-input
Currently unused. In prior releases,
these arguments represented memory
addresses for I/O buffer work areas.
IRET
Integer-output
Return code from the routine
0 -> Normal data block creation
1 -> Requested NAME already existed
2 -> Too many logical files open
4. Method: NAME is checked to determine if it already exists.
The control area is checked to make sure that a new object can be opened and
made available for processing.
If both conditions above are satisfied, the buffer management area is cleared
and the DAT control area, as described in the DICENT routine description is
created. The primary map blocks and the first data area are reserved in the
dictionary and stored in the DAT array.
The DAT array is copied to both the control area and the primary map block
for file management.
The logical file number assigned by the OPENC is returned to the calling
application program.
Subroutine Name: OPENR
1. Entry Point: OPENR
2. Purpose: Open existing keyed objects for random access updating and
return logical file reference.
CHAPTER 9
Miscellaneous
3. Calling Sequence: CALL OPENR
(DBNUM,NAME,WRDREC,FILNUM,KEYLEN,D2,D3,D4,D5,D6,IRET)
DBNUM
Integer-input
Logical database number
NAME
Array-input
Dictionary entry and object name to
update
WRDREC
Integer-output
Number of words per record in object
FILNUM
Integer-output
Logical handle number assigned to the
object
KEYLEN
Integer-output
The number of words in the key
0-> Used Hierarchal Method
+n-> Used B-Tree Method
D2
D3
D4
D5
D6
Integer-input
Currently unused. In prior releases,
these arguments represented memory
addresses for I/O buffer work areas.
IRET
Integer-output
Return code from the routine
0 -> Normal data block open
1 -> Requested NAME does not exist
2 -> Too many logical files open
3 -> Currently unused. In prior
releases, it indicated too few buffers
allocated.
4 -> Object already open
4. Method: DICRDR is used to check the existence of the object NAME and to
retrieve its DAT control area.
When the object exists, it is checked for a conflict to another logical file.
When no conflict exists, then a check for available processing space (i.e., less
than thirty logical files currently open) is made.
When space is available, the DAT control area is copied to the available
control area. The remaining control fields are initialized for object
management.
221
222
The logical handle number and words per record are returned to the calling
application program.
Subroutine Name: OPENSQ
1. Entry Point: OPENSQ
2. Purpose: Open a keyed object for sequential processing and return logical
file reference.
3. Calling Sequence: CALL OPENSQ
(DBNUM,NAME,FILNUM,KEYLEN,IRET)
DBNUM
Integer-input
Logical database number
NAME
Array-input
Object dictionary entry and object to
open
FILNUM
Integer-output
Logical handle number assigned to
object
KEYLEN
Integer-output
The number of words in the key
0-> Used Hierarchal Method
+n-> Used B-Tree Method
IRET
Integer-output
Return code from the routine
0 -> Normal data block open
1 -> Requested object does not exist
2 -> Too many logical files open
3 -> Unused
4 -> Object already open for update
4. Method: This routine can only be used to open keyed objects for read access.
The existence of the object is determined by DICRDR, and its form (keyed) is
verified.
Control areas are created for logical file operations and initialized with file
control data.
FILNUM is returned to the calling routine.
CHAPTER 9
Miscellaneous
9.10
Divergent Thermal Results Error Correction (Q10768221)
This is an error correction for radiation boundary conditions in nonlinear heat
transfer. It can only occur when a RADBC entry is used in a nonlinear solution. For
problems where radiation heat transfer dominates conduction, strange non-physical
results have been observed. For most problems where radiation is modest, no bad
results will be observed. In the January 2004 beta release this error was correct for the
linear (QUAD4 and TRIA3) elements. This correction is now extended to the quadratic
(QUAD8 and TRIA6) elements in this release.
223
224
9.11
Displacement Output Filters
The option to filter displacement output based on user-defined threshold values is
now available. This option can be requested using the following new keywords in the
DISPLACEMENT command.
Format:



TM = f
RM = f
DISPLACEMENT (....,
,


 T 1 = f , T 2 = f , T 3 = f   R1 = 1, R 2 = f , R3 = f 
)
Examples:
DISP(T1=1.0E-3, T3=1.0E-2) = ALL
DISP(TM=1.0E-3, PRINT, PLOT) = ALL
DISP(TM=1.0E-3, PRINT, PLOT, SORT2) = 20
Describers
Meaning
TM
Translational Magnitude Filter
T1, T2, T3
Translational Component Filters
RM
Rotational Magnitude Filters
R1, R2, R3
Rotational Component Filters
F
Filter value (Real > 0.0)
Remarks:
1. Displacement components may be selected to control filtering to reduce the
amount of output produced. When magnitudes are selected, the component
values are ignored. Only a single positive value for f can be supplied and
comparisons are performed in the global reference frame. Comparisons are
performed after the SET intersection is performed against the domain.
Selection of this option does not effect the MAXMIN(GRID) operations.
Scalar comparisons are performed using the minimum of all supplied values
for the filters. Complex values filters are performed on the Magnitude when
components are selected. Complex vector magnitudes follow a derivation
using a deterministic interpretation for frequency response.
CHAPTER 9
Miscellaneous
2. When using filters the compound usage of the verbs PRINT, PLOT is
allowed. The entries in the printed output are the entries that exceed any
threshold, while the remaining entries within the SET are marked as plot to
allow for post-processing operations. When SORT2 is selected, then print,
plot must be used to allow for table transpose operations to occur. When any
entry in the SORT2 format is above the threshold, all values for time or
frequency will be printed for the grid.
225
226
9.12
Write Results Recovery for Subcases into Separate
F06 Files
Recovery results written to the F06 output file can now be redirected to separate
output files for each subcase.
Inputs
Both the ASSIGN and POST commands are modified for assigning the physical
filename and specification of the subcase specific filename suffix respectively.
The modified ASSIGN and POST command are shown below followed by a small
example illustrating the use of the above commands. In this example the results redirected for both subcases are redirected to use specified files.
CHAPTER 9
Miscellaneous
POST
Post-Processor Data Specifications
Controls selection of data to be output for post-processing functions via the OUTPUT2
module interface for selected commercial post-processor products. Another feature is
to redirect F06 output file results for a subcase to a user defined file.
Format:



furn
POST  TOFILE 
[ ppname ] [ oplist ]
 TOCASE  filename 
Examples:
POST TOFILE 51 PATRAN NOSTRESS
POST TOFILE SUBCASE8
POST TOCASE SUFNAME1
Describer
Meaning
TOFILE
Keyword to specify the destiny of output files. (No default if it
appears above all subcases.)
TOCASE
Keyword to specify the destiny of subcase results to user-defined
output files. (No default if it appears above all subcases.)
furn
Fortran file unit reference number where data will be written.
(Integer>0)
filename
Suffix filename (see Remark 8.). (Char8)
ppname
Name of the target post-processor program. (Default = PATRAN)
oplist
Names of output items to be processed.
Remarks:
1. The POST Case Control command controls the placement of output data on
external fortran files for use by commercial post-processors. Use of the POST
command generates the proper value for the POST DMAP parameter
associated with the particular post-processor. All of the other parameter
controls related to the POST DMAP parameter remain in effect and are
described in “Parameters” on page 603. The products supported are
identified in the following table. PATRAN is the default post-processor
name used for ppname. DBC output (POST=0) cannot be controlled by the
POST command.
227
228
ppname
Product
PARAM,POST,Value
PATRAN
MSC.Patran V3
-1
SDRC
SDRC IDEA-S
-2
NF
MSC/LMS NF
-4
FEMTOOLS
DDS/FemTools
-5
UNIGRAHICS
EDS/Unigraphics
-6
2. The TOFILE describer is followed by the specification of either a FORTRAN
unit reference number or a file name associated with the external file that
receives the output data. If a FORTRAN unit number is used, the file must
be associated with it via the ASSIGN File Management Statement. If POST
appears above all subcases, TOFILE must be used to specify either a
FORTRAN unit reference number or a file name. The default value of
TOFILE, which appears under a subcase, will inherit from the value given in
the POST above all subcases. If the unit reference number is associated with
a form=formatted file, changes in unit numbers across subcases are not
allowed.
3. The data that can be controlled for each post-processor product is limited
and is identified under the description of the POST and related DMAP
parameters in “Parameters” on page 603. The keywords that can be used for
the oplist options are shown in the following table. If an output item
supported by a particular post-processor is described in “Parameters” on
page 603 but is not listed here, then the POST command cannot be used to
control its output to the external file.
Output Item
oplist Keyword
Case
Command
Displacements
[NO]DISPLACE
DISP
Forces of Single Point Constraint
[NO]SPCFORCE
SPCFORCE
Element Forces
[NO]FORCES
ELFO/FORCE
Element Stresses
[NO]STRESS
ELST/STRESS
Element Strain Energy
[NO]ESE
ESE
Grid Point Force Balance
[NO]GPFORCE
GPFORCE
Stress at Grid Points
[NO]GPSIGMA
STRESS
CHAPTER 9
Miscellaneous
Output Item
oplist Keyword
Case
Command
Strain/Curvature at Grid Points
[NO]GPEPSILON
STRAIN
Composite Element Failure Indices
[NO]PLYFAILURE
STRESS
Element Kinetic Energy
[NO]EKE
EKE
Element Energy Loss
[NO]EDE
EDE
Multi-point Constraint Forces
[NO]MPCFORCE
MPCFORCE
Composite Lamina Stresses
[NO]PLYSIGMA
STRESS
Composite Lamina Strains
[NO]PLYEPSILON
STRAIN
Element Strains
[NO]STRAIN
STRAIN
Grid Point Stresses
[NO]GPSTRESS
GPSTRESS
Grid Point Strains
[NO]GPSTRAIN
GPSTRAIN
Applied Loads
[NO]LOAD
OLOAD
No items to be output
NONE
----------------
4. Output data items must have been generated via the appropriate case control
command in order for the data to be available for post-processing options.
For example, the specification of SPCF in the oplist of the POST command
will not produce forces of single point constraint on the POST output file
unless there is a SPCF Case Control command present. Refer to the tables
under the POST parameter description in “Parameters” on page 603 for a list
of the output items supported by each post-processor.
5. Any data generated by a case control output request is automatically
included in the oplist of the POST command. If output data is not wanted for
a particular case, then the characters “NO” should be the first two characters
of the keyword in the oplist. For example, NODISP specifies that
displacements are not to be posted to the output file even though they have
been requested via the DISP Case Control command. Alternatively, the
related POST parameters may be used. For example, to avoid outputting any
displacements whatsoever to the .op2 file, use a “PARAM, OUG, NO” Bulk
Data entry.
6. Certain data (e.g. geometry) is always generated and is not dependent upon
the presence of a case control command in the input data. The POST
command affects the placement of this data on the external file only insofar
as the selection of the post-processor defines the value of the POST DMAP
229
230
parameter value. The actions described in “Parameters” on page 603 under
the POST parameter description will prevail for the particular value of POST
associated with the selected post-processor. The primary purpose of the
POST command is to give the user more control over subcase-dependent
output data being stored on the external OUTPUT2 file.
7. If a POST command is present within any subcase, a POST command must
also be present above the subcase level. The placement of the POST
command above the subcase level causes a cumulative effect on POST
commands in subsequent subcases. Any options specified above the subcase
level propagate down into the POST command within a subsequent subcase.
Thus, if a POST command specifies NODISP (no displacement output
wanted) above the subcase level, then a POST command with the DISP
option would be required within a subcase to generate any output to the
OUTPUT2 file for displacements. This also implies that changing the
OUTPUT2 file unit reference number with the TOFILE option in a subcase
causes all output quantities currently scheduled for output to be switched to
the new unit number, not just those in the oplist for the current POST
command.
8. When the name of an output file is specified by keyword TOFILE, the
ASSIGN statement in the File Management Section (FMS) can be used to
specify the full path of its root name. the logical-key word for the root name
is OUTPUT2F. The default root name is the MSC.Nastran job name.
FORTRAN unit reference number 19 has been reserved by MSC.Nastran for
OUTPUT2F, although the user can assign other FORTRAN unit number to
it. The full file name is in the form of <root name>.<suffix filename>.
9.
When the name of an output file is specified by keyword TOCASE, the
ASSIGN statement in the File Management Section (FMS) can be used to
specify the full path of its root name. the logical-key word for the root name
is OPCASE. The default root name is the MSC.Nastran job name. FORTRAN
unit reference number 22 has been reserved by MSC.Nastran for OPCASE.
Although the user can assign other .FORTRAN unit numbers to it. The full
file name is in the form of <root name>.<suffix filename>. Also ppname and
oplist are not required. If ppname and oplist are specified, they will be
ignored. Suffix filename must be specified with keyword TOCASE.
CHAPTER 9
Miscellaneous
ASSIGN
Assigns Physical File
aaa
Assigns physical file names or other properties to DBset members or special
FORTRAN files that are used by other FMS statements or DMAP modules. Also,
assigns physical name and/or other properties to Modal Neutral Files (MNF) for
MSC.Nastran/ADAMS interface.
Format 1: Assign a DBset member name
ASSIGN log-name= = ′filename1′
= *
[TEMP] [ DELETE] [ SYS=’sys-spec’ ]
= ′*′
Format 2: Assign a FORTRAN file
ASSIGN logical-key = ′filename2′
[UNIT = u]
= *
= ′*′
[ STATUS = ]  NEW



 OLD



UNKNOWN


[ FORM = ]  FORMATTED
 [ RECL = 1 ] [ SIZE = s ]
 UNFORMATTED 


 BIGENDIAN



 LITTLEENDIAN 
 LTLEND



 <ostype>

[DEFER ]
TEMP
DELZERO
[ DELETE] [SYS = ‘sys-spec’]
Examples:
1. Assign the DBALL DBset:
ASSIGN DB1=’filename of member DB1’
INIT DBALL LOGI=(DB1)
231
232
2. Assign FORTRAN file 12 to the OUTPUT4 module using the ASCII option:
ASSIGN OUTPUT4=’filename of FORTRAN file’
UNIT=12, FORM=FORMATTED
3. Assign FORTRAN file to the OPCASE using the ASCII option:
ASSIGN OPCASE=’Filename of FORTRAN file’, STATUS=NEW
4. Define SYS parameters for the SCR300 DBset file using the default file name.
ASSIGN SCR300 SYS=’...’
5. Set the default OP2 file format to BIGENDIAN and assign two OP2 files, one
to unit 12 with the file name “test_op2.12’ and one to unit 35 with file name
‘test_op2.35’ in ASCII mode.
ASSIGN OP2 BIGENDIAN
...
ASSIGN OP2=’test_op2.12’ UNIT=12
ASSIGN OP2=’test_op2.35’ UNIT=35 FORM=FORMATTED
Describer
Meaning
log-name
The name of a DBset member name. log-name may also be
referenced on an INIT statement after the LOGICAL keyword.
filename1
The physical filename assigned to the DBset member. If the default
filename (if there is one) is to be used, filename1 may be omitted or
specified as * or ‘*’. See Remark 6.
logical-key
Specifies defaults for STATUS, UNIT, and FORM of FORTRAN
files for other FMS statements, DMAP modules, punching and
plotting operations.
filename2
The physical file name assigned to the FORTRAN file. If the default
filename is to be used, filename2 may be omitted or specified as * or
‘*”. See Remark 7.
UNlT=u
u is the FORTRAN unit number of the FORTRAN file. If this
describer is omitted and if filename2 is omitted, this ASSIGN
statement will update the defaults for subsequent ASSIGN
statements for the same logical-key value. See Remark 7.
TEMP
Requests that the file associated with log-name or logicalkey/UNIT be deleted at the end of the run.
DELETE
Requests that the file associated with logical-key/UNIT, if it exists
before the start of the run, be deleted.
CHAPTER 9
Miscellaneous
Describer
Meaning
DELZERO
Requests that the file associated with logical-key/UNIT be deleted
at the end of the run if it is zero-length, that is, if it does not contain
any data.
STATUS
Specifies whether the FORTRAN file is being created
(STATUS=NEW) or has been created prior to the run
(STATUS=OLD). If its status is not known, then
STATUS=UNKNOWN is specified.
FORM
Indicates whether the FORTRAN file is written in ASCII
(FORM=FORMATTED) or binary (FORM=UNFORMATTED,
BIGENDIAN, LITTLEENDIAN, LTLEND, <ostype>) format. See
Remark 11.
DEFER
Defers opening/creating the specified file. That is, the file will not
be opened/created during MSC.Nastran initialization. The file
must be explicitly opened by the module or DMAP accessing the
file, using, for example, FORTIO, before it can be used.
sys-spec
System specific or machine-dependent controls. For DBset files,
these control I/O performance. For FORTRAN files, these are
controls for IBM/MVS-type computers only. See Remark 14.
RECL = l
The size of a block of input/output information specified in words.
See Remark 15.
SIZE = s
The number of blocks allocated to the DBC database. See
Remark 16.
Remarks:
1. The ASSIGN statement and its applications are discussed further in the
“Database Concepts” on page 513 of the MSC.Nastran Reference Guide.
2. The log-name or logical-key describer must be the first describer on the
ASSIGN statement. All other describers may appear in any order. With the
exception of log-name, logical-key, filename1, filename2, and sys-spec,
describers and values longer than four characters may be abbreviated to four
characters.
3. For FORTRAN files, the logical-key names and their default attributes are
listed in Table 2-1. If a logical-key name is identified as “Assignable YES”,
then the defaults may be overridden on the ASSIGN statement.
233
234
4. Certain reserved names may not be used for log-names or logical-key names.
These names are the logical names listed in Table 2-1 that are identified as
“Assignable NO”. This list includes: SEMTRN, LNKSWH, MESHFL,
LOGFL, INPUT, PRINT, INCLD1, and CNTFL. If they are used, then a fatal
message is issued. Also unit numbers 1 through 10, 14, 16, 18, 19 and 21
should not be assigned. PUNCH and PLOT may be used but are not
recommended.
5. If one of the logical-key names indicated in the Remarks 3. and 4. is not
specified on this statement, then it is assumed to be a DBset member name
log-name as shown in Format 1.
6. If the same log-name is used on more than one DBset ASSIGN statement, the
following rules apply:
a. If there is no current entry for the specified log-name, a new entry in the
DBset tables will be created. If there is an existing entry for the specified
log-name, the ASSIGN parameters will modify that entry instead of
creating a new one.
b. If filename1 is omitted or is specified as * or ‘*’, the default file name or, if
this is a second or subsequent ASSIGN statement for the same log-name,
the previously specified file name (or default name if none was
previously specified) will be used.
7. If the same logical-key is used on more than one FORTRAN file ASSIGN
statement, the following rules apply:
a. If filename2 is omitted (or specified as * or ‘*’) and if the UNIT describer
is omitted, the ASSIGN parameters will modify the system default entry
for the logical-key, establishing the new defaults for any subsequent
ASSIGN entry for the logical-key. Note, however, that any entries
previously created with the same logical-key will not be modified by the
new parameters specified on this ASSIGN statement.
b. If the value specified by the UNIT describer matches the value for an
entry created by a previous ASSIGN statement with a UNIT describer,
then:
• if the logical-key values are different, a UFM will be generated,
• if the logical-key values are the same, the previous entry will be
updated instead of having a new entry created.
c. If the value specified by the UNIT describer does not match the value for
an entry created by a previous ASSIGN statement with a UNIT describer,
then a new entry will be created in the FORTRAN unit tables.
CHAPTER 9
Miscellaneous
d. If the file name is omitted or specified as * or ‘*’, the default file name or,
if this is a second or subsequent ASSIGN statement for the same logicalkey/UNIT combination, on previously specified file name (or default
name if none was previously specified) will be used.
8. If it is necessary to execute the INPUTT4 and OUTPUT4 modules on the
same unit, then specify ASSIGN OUTPUT4 only. The same is recommended
for the INPUTT2 and OUTPUT2 modules.
9. STATUS, UNIT, and FORM are ignored if assigning a log-name (DBset
member name).
10. FORM=FORMATTED must be specified for a unit when:
• ASCII output is desired from the OUTPUT4 DMAP modules that
processes the unit and, for Cray UNICOS, when ASCII input is
supplied to the INPUTT4 DMAP module that processes the unit. See
the MSC.Nastran 2005 DMAP Programmer’s Guide.
• FORMAT=NEUTRAL is selected on the DBUNLOAD and DBLOAD
FMS statements that process the unit. See the “Database Concepts”
on page 513 of the MSC.Nastran Reference Guide.
• The neutral file format is desired for the OUTPUT2 module and, for
Cray UNICOS, when ASCII input is supplied to the INPUTT2
module.
11. For the DBUNLOAD, OUTPUT2 and OUTPUT4 modules, binary format
may be requested using FORM=UNFORMATTED and, for all platforms
except Cray UNICOS, using FORM=BIGENDIAN,
FORM=LITTLEENDIAN, FORM=LTLEND or FORM=<ostype>. The
FORM=BIGENDIAN, FORM=LITTLEENDIAN, FORM=LTLEND and
FORM=<ostype> specifications are used when the generated output file is to
be processed on a platform other than current platform. The format
appropriate for the platform on which the file is to be processed (the target
platform) must be specified. FORM=LTLEND is equivalent to
FORM=LITTLEENDIAN. The FORM=<ostype> specification can by used as
a convenience, allowing the desired output format to be specified using the
target platform OS name or vendor (if there can be no ambiguity) instead of
its actual binary file format. <ostype> can be one of the following:
• AIX, FUJITSU, HPUX, IRIX, PRIMEPOWER, SOLARIS, SUPERUX or
UXPV. These are equivalent to BIGENDIAN.
• ALPHA, LINUX or WINDOWS. These are equivalent to
LITTLEENDIAN.
235
236
See the MSC.Nastran 2004 r3 Installation and Operations Guide for further
information on binary file formats.
12. For all platforms except Cray UNICOS, the FORM= describer is ignored for
the DBLOAD, INPUTT2 and INPUTT4 modules. MSC.Nastran determines
the actual file format when it accesses the specified file. If the FORM=
describer is specified on an ASSIGN statement for these logical-keys, the
syntax of the describer will be validated but will otherwise be ignored. Note,
however, that the DBLOAD and INPUTT2 modules cannot process input
files in other than the native binary format. That is, a binary file in
BIGENDIAN format cannot be processed on a LITTLEENDIAN platform
and vice versa. For MSC.Nastran on Cray UNICOS, the FORM= describer is
required for the DBLOAD, INPUTT2 and INPUTT4 modules if the file does
not have the default format.
13. For the DBUNLOAD and OUTPUT2 modules, if FORM is other than
UNFORMATTED (or equivalent, e.g., BIGENDIAN on an AIX or HPUX
platform and LITTLEENDIAN on a Linux or Windows platform), then only
data blocks with an NDDL description are processed. (See the MSC.Nastran
2005 DMAP Programmer’s Guide under the DATABLK statement.) An
NDDL description is required for TYPE=TABLE and none is required for
TYPE=MATRIX. The data block must be processed with
FORM=UNFORMATTED if TYPE=UNSTRUCTURED, KDICT or KELM.
14. See the MSC.Nastran 2004 r3 Installation and Operations Guide for further
information on sys-spec controls and on machine-dependent aspects of the
ASSIGN statement. Also, if there are SYS specifications on more than one
ASSIGN statement specifying the same log-name or logical-key/UNIT
combination, the second and subsequent specifications will appended to the
current SYS specification with a comma separator.
15. Currently the RECL keyword is used by the DBC module and has a default
minimum of 1024 words. The maximum allowed is 65536 words and is used
to increase the database capacity.
16. The SIZE keyword is used by the DBC module and has a default of 16777215.
The maximum allowed is 2147483647 and is used to increase the database
capacity. MSC.Patran releases before 2001 should use the defaults for RECL
and SIZE or database verification failures will occur.
17. logical-key name MNF does not utilize UNIT or FORM.
CHAPTER 9
Miscellaneous
S
Logical Key
Name
Table 2-1 FORTRAN Files and Their Default Attributes
Physical
Name
Unit
No.
SEMTRN
sdir/data.f01
1
LNKSWH
sdir/data.f02
MESHFL
Form
Description/
Application
Status
Assignable
Open
Access
FORMATTED
NEW
NO
YES
SEQ.
Input Data Copy
Unit
2
UNFORMATTED
NEW
NO
YES
SEQ.
Link Switch Unit
sdir/data.f03
3
FORMATTED
NEW
NO
YES
SEQ.
Input Data Copy
Unit
SEMTRN
sdir/data.f01
1
FORMATTED
NEW
NO
YES
SEQ.
Input Data Copy
Unit
LNKSWH
sdir/data.f02
2
UNFORMATTED
NEW
NO
YES
SEQ.
Link Switch Unit
MESHFL
sdir/data.f03
3
FORMATTED
NEW
NO
YES
SEQ.
Input Data Copy
Unit
LOGFl
out.f04
4
FORMATTED
NEW
NO
YES
SEQ.
Execution
Summary Unit
INPUT
data.dat
5
FORMATTED
OLD
NO
YES
SEQ.
Input File Unit
PRINT
out.f06
6
FORMATTED
NEW
NO
YES
SEQ.
Main Print Output
Unit
PUNCH
out.pch
7
FORMATTED
NEW
YES
YES
SEQ.
Default Punch
Output Uniit
authorize.dat
8
FORMATTED
OLD
NO
YES
SEQ.
Authorization File
INCLD1
NO
Available for Use
CNTFL
NO
Available for Use
INPUTT2
REQ
OUTPUT2+
out.op2
INPUTT4
REQ
OUTPUT4
REQ
PLOT
REQ
++
OLD
YES
NO
SEQ.
INPUTT2 Unit
UNFORMATTED*
NEW
YES
YES
SEQ.
OUTPUT2 Unit
REQ
++
OLD
YES
NO
SEQ.
INPUTT4 Unit
REQ
UNFORMATTED*
NEW
YES
NO
SEQ.
OUTPUT4 Unit
out.plt
14
UNFORMATTED
NEW
YES
YES
SEQ.
Plotter Output
Unit
BULKECHO
out.becho
18
FORMATTED
NEW
YES
YES
SEQ.
Plotter Output
Unit
OUTPUT2F
out
19
UNFORMATTED
NEW
YES
SEQ.
Named OUTPUT2
Pattern
OPCASE
REQ
22
FORMATED
NEW
YES
SEQ.
Available for Use
TOPDES
out.des
21
FORMATTED
NEW
YES
YES
SEQ.
Topology
Optimization
DBC
out.xdb
40
UNFORMATTED
NEW
YES
YES
DIRECT
DBUNLOAD
REQ
50
UNFORMATTED*
NEW
YES
NO
SEQ.
DBUNLOAD FMS
statement
DBLOAD
REQ
51
++
OLD
YES
NO
SEQ.
DBLOAD FMS
statement
12
Database
Converter Unit
237
238
Table 2-1 FORTRAN Files and Their Default Attributes (continued)
Logical Key
Name
MNF
Physical
Name
out.mnf
Unit
No.
none
Form
none
Status
Assignable
Open
Access
NEW
YES
NO
SEQ.
A502LU
Interface for
ADAMS/Flex
Available for Use
DBMIG
USER FILE
Description/
Application
Available for Use
REQ
REQ
REQ
REQ
YES
NO
SEQ.
Any User-Defined
File
where:
Logical Key Name
specifies the logical-key NAME used on the ASSIGN
statement.
Physical Name
specifies the default name used to open the file, i.e., the default
filename2 name.
“REQ” means that this parameter is required in the ASSIGN
statement from the user.
Unit No.
specifies the default FORTRAN unit number used by
MSC.Nastran. “REQ” means that this parameter is required in
the ASSIGN statement from the user.
Form
specifies the default FORM used when the file is opened.
Status
specifies the default STATUS used when the file is opened.
“REQ” means that this parameter is required in the ASSIGN
statement from the user.
Assignable
If “YES”, the user may assign a physical file to this logical
name.
If “NO”, the unit (if any) and logical name are reserved by
MSC.Nastran.
Open
If “YES”, the file is opened by default.
If “NO”, the file must be explicitly opened.
Access
If “SEQ”, the file is opened for sequential access.
If “DIRECT”, the file is opened for direct access.
sdir
The scratch directory specified using the “sdirectory”
keyword.
CHAPTER 9
Miscellaneous
data
The name of the input data file with all directory and
extensions removed.
out
The directory and file prefix specified using the “out”
keyword or taken by default.
Notes:
+
The actual logical-key name for this is “OP2”. If you use “OUTPUT2” (even
though this is still the logical-key name put out by MSC.Patran) you will get a
user fatal message from MSC.Nastran.
*
FORMATTED is required for neutral-format OUTPUT2 files and ASCII-format
OUTPUT4 files.
++
For Cray Unicos, the default Form is UNFORMATTED. For all other platforms,
the Form is ignored. See Remark 12.
Example
The following example demonstrates the form of the modified ASSIGN and POST
entries. The expected result would be that files ‘rsltsubc.subc1’ and ‘rsltsubc.sub2’
would contain the results for subcase 1 and 2 respectively.
assign opcase='rsltsubc'
ID MSC, RSLTSUBC
TIME
5
$ MINUTES
SOL
101 $
CEND
TITLE = WRITE RESULTS TO SEPARATE SUBCASE FILES
ECHO = UNSORT
DISPL = ALL
STRES = ALL
GPSTR = ALL
post tocase allcase
SUBCASE 1
TITLE = GPSTR1, QUADR ELEMENTS, MEMBRANE
subtitle = **** subcase 1 ****
LOAD = 1
post tocase subc1
SUBCASE 2
TITLE = GPSTR1, QUADR ELEMENTS, BENDING
subtitle = **** subcase 2 ****
LOAD = 2
post tocase subc2
OUTPUT(POST)
SET 1 = ALL
SURFACE 1, SET 1, FIBRE Z1, SYSTEM BASIC, NORMAL Z, TOPOLOGICAL
BEGIN BULK
GRID
1
.04
.02
239
240
GRID
GRID
GRID
GRID
GRID
GRID
GRID
CQUADR
CQUADR
CQUADR
CQUADR
CQUADR
PSHELL
MAT1
FORCE
SPCD
SPCD
SPCD
SPCD
FORCE
SPCD
SPCD
2
3
4
5
6
7
8
1
2
3
4
5
100
100
1
1
1
1
1
2
2
2
100
100
100
100
100
100
1.+6
5
5
6
7
8
5
5
5
SPCD
2
SPCD
SPCD
SPCD
SPCD
SPCD
PARAM
2
2
2
2
2
NEWSEQ
ENDDATA
.18
.16
.08
.0
.24
.24
.0
1
5
6
7
8
.001
3
4
.03
.08
.08
.0
.0
.12
.12
2
6
7
8
5
100
.25
0.
0.
2.4-4
3.-4
0.6-4
0.
0.
0.
6
3
2.88-5
6
7
7
8
8
-1
4
3
4
3
4
1.2-4
5.04-5
2.4-4
7.2-6
1.2-4
1
1
1
1
123456
123456
123456
123456
3
2
3
4
1
4
1
2
3
4
100
1.
5
6
7
8
2
2
2
2
0.
1.2-4
2.4-4
1.2-4
1.
5
5
0.
6
5
-2.4-4
7
5
-3.-4
8
5
-6.-5
MSC.Nastran 2004 Release Guide
CHAPTER
10
Upward Compatibility
■ DMAP Modules in MSC.Nastran 2005
■ Summary of Data Block Changes from MSC.Nastran 2004 to
MSC.Nastran 2005
■ More Stringent Case Control Check
242
10.1
DMAP Modules in MSC.Nastran 2005
This section summarizes DMAP module changes from MSC.Nastran 2004 to
MSC.Nastran 2005 which could affect user DMAP alters and solution sequences. This
information is intended to help convert MSC.Nastran 2004 DMAP alters and solution
sequences to run in MSC.Nastran 2005. The format of the following modules has been
modified in MSC.Nastran 2005 such that the MSC.Nastran 2004 format is not
upwardly compatible with MSC.Nastran 2005 and/or their behavior is not upwardly
compatible. The changes are described in the next section.
BDRYINFO
DOPR3
DPD
ELTPRT
FA1
FRLG
GUST
MODQSET
MPP
NLCOMB
NLTRLG
SDRHT
TRLG
WEIGHT
The following is a list of existing modules with new features or fixes which require
format changes in MSC.Nastran 2005 but are not documented here because their
MSC.Nastran 2004 formats are considered upwardly compatible in MSC.Nastran
2005. They are fully documented in the MSC.Nastran 2005 DMAP Programmer’s
Guide.
.
BCDR
DISOPT
DOM11
DOM12
DOM6
DOM9
DOPFS
DOPR1
DSAD
DSAL
DSAW
DSPRM
DSTAP2
FA2
GKAM
GP1
GP4
GPFDR
GPSP
IFP9
INPUTT2
MAKAEFS
MAKMON
MATMOD
MKRBVEC
MODGM2
MPYAD
NLITER
NLSOLV
OUTPRT
SDRCOMP
SEP1X
SEQP
SMPYAD
SSG1
TA1
The following is a list of new modules in MSC.Nastran 2005. They are not
documented here but are documented in the MSC.Nastran 2005 DMAP
Programmer’s Guide.
DSGRDM
GI2C
GUSTLDW
ILMP1
MDENZO
MODCASE
NDINTERP
SLITX
ILMP2
ILMPGPF
MASSCOMB
DMAP Module Changes
This section shows the changes for DMAP module instructions which were changed
from MSC.Nastran 2004 to 2005. The module change descriptions are presented as
differences with respect to the MSC.Nastran 2005 DMAP Programmer’s Guide which
is available on the "MSC.Software Combined Documentation 2005" CD-ROM. The
CHAPTER 10
Upward Compatibility
change descriptions below includes the MSC.Nastran 2005 format of the module with
changes in bold text. Any new or changed data blocks and parameters are also
described below the format.
BDRYINFO
The first parameter, ASMUNIT, is obsolete and has been removed.
DOPR3
The UNUSED data block has been removed and DIT and DYNAMIC are moved into
the 18th and 19th positions.
Format:
DOPR3
CASE,EDOM,DTB,ECT,EPT,DESTAB,EDT,OL,DEQIND,DEQATN,
BGPDT,DVPTAB*,VIEWTB,OINT,PELSET,XINIT,FOL,DIT,DYNAMIC/
OBJTAB,CONTAB,R1TAB,RESP12,RSP1CT,FRQRSP,CASEDS,
OINTDS,PELSETDS,DESELM,RESP3,ADRDUG,ADRDUTB,CASADJ,
MODRSP,CASEDM,RQATAB,RESP12X,RESP3X,CONTABX,OBJTABX,
ARVEC/
DMRESD/S,N,DESGLB/S,N,DESOBJ/S,N,R1CNT/S,N,R2CNT/
S,N,CNCNT/SOLAPP/SEID/S,N,EIGNFREQ/PROTYP/DSNOKD/
SHAPES/S,N,R3CNT/RGSENS/INREL/S,N,ADJFLG/S,N,TADJCOL/
AUTOADJ/SOLADJC/S,N,NORMEV $
DPD
The amplitude data in DLT has been moved into five new output matrices to support
machine precision enforced motion.
Format:
DPD
DYNAMIC,GPL,SIL,USET,UNUSED5,PG,PKYG,PBYG,PMYG,YG/
GPLD,SILD,USETD,TFPOOL,DLT,PSDL,RCROSSL,NLFT,TRL,
EED,EQDYN,APPLOD,ENFLODK,ENFLODB,ENFLODM,ENFMOTN/
LUSET/S,N,LUSETD/S,N,NOTFL/S,N,NODLT/S,N,NOPSDL/
DATAREC/S,N,NONLFT/S,N,NOTRL/S,N,NOEED/SORTNLFT/
S,N,NOUE/UNUSED12/SEID $
243
244
Output Data Blocks:
:
APPLOD
Matrix of applied load amplitudes
ENFLODK
Matrix of equivalent enforced motion load amplitudes due to stiffness
effects
ENFLODB
Matrix of equivalent enforced motion load amplitudes due to viscous
damping effects
ENFLODM
Matrix of equivalent enforced motion load amplitudes due to mass
effects
ENFMOTN
Matrix of enforced motion amplitudes
ELTPRT
ECT is always input in the 12st position and no longer input in the 4th position, which
is now occupied by the new data block NSMEST.
Format:
ELTPRT
ECT,GPECT,BGPDT,NSMEST,EST,CSTM,MPT,DIT,
CASSECC,EPT,UNUSED/
VELEM/
PROUT/S,N,ERROR/WTMASS $
Input Data Blocks:
NSMEST
NSM Bulk Data entries in EST format
UNUSED
Unused and may be purged.
FA1
VREF parameter is now required input.
Format:
FA1
KHH,BHH,MHH,QHHL,CASECC,EDT/
FSAVE,KHH1,BHH1,MHH1,FLUTABP/
S,N,FLOOP/S,N,TSTART/S,N,NOCEAD/LPRINT/XYUNIT/VREF $
CHAPTER 10
Upward Compatibility
Output Data Block:
FLUTABP
Flutter summary table for all methods except K and KE
Parameters:
XYUNIT
Input-integer-default=0. FORTRAN unit number to which extracted
khh1 values are written at each sweep point for the PKS and PKNLS
methods.
VREF
Input-real-no default. Flutter velocity divisor to obtain flutter indices.
FRLG
Format:
FRLG
CASECC,USETD,DLT,FRL,GMD,GOD,DIT,PHDH,
APPLOD,ENFLODK,ENFLODB,ENFLODM,ENFMOTN/
PPF,PSF,PDF,FOL,PHF,YPF/
SOLTYP/S,N,FOURIER/S,N,APP $
Input Data Blocks:
APPLOD
Matrix of applied load amplitudes
ENFLODK
Matrix of equivalent enforced motion load amplitudes due to stiffness
effects
ENFLODB
Matrix of equivalent enforced motion load amplitudes due to viscous
damping effects
ENFLODM
Matrix of equivalent enforced motion load amplitudes due to mass
effects
ENFMOTN
Matrix of enforced motion amplitudes
245
246
GUST
Format:
GUST
CASECC,DLT,FRL,DIT,QHJL,UNUSED6,UNUSED7,ACPT,
CSTMA,PHF,APPLOD,ENFLODK,ENFLODB,ENFLODM,ENFMOTN/
PHF1,WJ,QHJK,PFP/
S,N,NOGUST/BOV/MACH/Q $
Input Data Blocks:
APPLOD
Matrix of applied load amplitudes
ENFLODK
Matrix of equivalent enforced motion load amplitudes due to stiffness
effects
ENFLODB
Matrix of equivalent enforced motion load amplitudes due to viscous
damping effects
ENFLODM
Matrix of equivalent enforced motion load amplitudes due to mass
effects
ENFMOTN
Matrix of enforced motion amplitudes
MODQSET
Format:
MODQSET
GEOM1,GEOM2,GEOM4/
GEOM1W,GEOM2W,GEOM4W/
NOQSETT/QSETREC/QSETID $
Parameters:
QSETREC
QSETID
Input-integer-default=0. Records to use in defining the q-set degreesof-freedom:
>=0
No records are written
=-1
SENQSET record to GEOM1W
=-2
SPOINT record to GEOM2W and QSET1 record to GEOM4W
Input-integer-default=0. Starting q-set identification number for
QSETREC=-2.
CHAPTER 10
Upward Compatibility
MPP
MP2S inserted after MPSRP.
Format:
MPP
 MONITOR 
 MPSR   MPSER 
AECTRL,UXDAT, 
 ,
 , 
 ,MPEU,
AEMONPT


 MPAR   MPAER 
MPSIR,MPSRP,MP2S,MPSERP,UXV,INDX//
MACH/Q/AECONFIG/SYMXY/SYMXZ/MESH $
Input Data Block:
MP2S
Table of MONPNT2 responses at trim
NLCOMB
Format:
NLCOMB
CASECC,ESTNL,KDICTNL,BKDICT,ETT,PTELEM0,PTELEM,UNUSED8,
MPT,EQEXIN,SLT,DLT,BGPDT,APPLOD,DYNAMIC/
 SLT1 
 /
 DLT1 
ELDATA,
NSKIP/LSTEP/LINC/STATIC/LGDISP/OSTEP $
Input Data Blocks:
APPLOD
Matrix of applied load amplitudes
DYNAMIC
Table of Bulk Data entry images related to dynamics.
NLTRLG
Format:
NLTRLG
CASECC,USETD,DLT,SLT,BGPDT,SIL,CSTM,TRL,DIT,GMD,GOD,
PHDH,EST,MPT,APPLOD,ENFLODK,ENFLODB,ENFLODM,ENFMOTN/
PDT,TMLD,DLT1/TABS $
247
248
Input Data Blocks:
APPLOD
Matrix of applied load amplitudes
ENFLODK
Matrix of equivalent enforced motion load amplitudes due to stiffness
effects
ENFLODB
Matrix of equivalent enforced motion load amplitudes due to viscous
damping effects
ENFLODM
Matrix of equivalent enforced motion load amplitudes due to mass
effects
ENFMOTN
Matrix of enforced motion amplitudes
SDRHT
Format:
SDRHT
UG,OEF1,SLT,EST,DIT,RDEST,RECM,DLT,OEFNL1,MPT,BGPDT,
CSTM,SIL,USET,CASECC,OESNLH,APPLOAD/
HOEF1,HOES1/
TABS/SIGMA/NORADMAT $
Input Data Blocks:
APPLOD
Matrix of applied load amplitudes
OESNLH
Table of element heat flow in SORT1 format for nonlinear elements
Output Data Block:
HOES1
Table of element heat flow in SORT1 format combined for linear and
nonlinear elements.
TRD1
Format:
TRD1
CASECC,TRL,NLFT,DIT,KXX,BXX,MXX,PXT,SILD,USETD,
PARTVEC,PXT0,ROTORT,BGDD*,KCVDD*,RDG,PXTDV
UXT,PNL/
SOLTYP/NOUE/NONCUP/S,N,NCOL/FAC3/SETNAME/
NSOLT,NOTRLDFM/WTMASS $
CHAPTER 10
Upward Compatibility
Input Data Block:
PXTDV
Transient response load matrix in h-set (modal) or d-set combined
from two executions of TRLG: one with DVFLAG=0 and the other of
DVFLAG=1.
TRLG
Format:
TRLG
CASECC,USETD,DLT,SLT,BGPDT,SIL,CSTM,TRL,DIT,
 GMD   GOD   PHDH 

 ,
 , 
 ,EST,MPT,MGG,V01P,

 
  RPX 
APPLOD,ENFLODK,ENFLODB,ENFLODM,ENFMOTN/
 PPT   PST   PDT   PDT1   PHT 
 ,
, 
 ,TOL,DLTH,YPT,YPO,TOLR/

 ,
, 
 
 
  PXT 
 PPT  
S,N,NOSET/S,N,PDEPDO/IMETHOD/STIME/BETA/
S,N,FAC1/S,N,FAC2/S,N,FAC3/TOUT/TABS/
STIME/S,N,NCOLT/S,N,NSOLT/DVFLAG $
Input Data Blocks:
APPLOD
Matrix of applied load amplitudes
ENFLODK
Matrix of equivalent enforced motion load amplitudes due to stiffness
effects
ENFLODB
Matrix of equivalent enforced motion load amplitudes due to viscous
damping effects
ENFLODM
Matrix of equivalent enforced motion load amplitudes due to mass
effects
ENFMOTN
Matrix of enforced motion amplitudes
Parameter:
DVFLAG
Input-integer-default=0. Enforced motion processing flag for both the
large mass and direct methods of specification.
249
250
=0
Process only applied loads and excitations due to enforced
accelerations (default)
>0
Process only excitations due to enforced displacements and
velocities.
WEIGHT
The SEID parameter has been moved to the 4th position.
Format:
WEIGHT
VELEM,EST,MPT,DIT,OPTPRM,OGPWG,DESTAB,XINIT/
WMID,WGTM/
WGTVOL/S,N,VOLS/S,N,FRMS/SEID/DOFRMASS $
Input Data Blocks:
DESTAB
Table of design variable attributes.
XINIT
Matrix of initial values of the design variables.
Parameters:
FRMASS
Output-real-default=0.0. Fractional mass of designed structure.
SEID
Input-integer-default=0. Superelement identification number.
DOFRMASS
Input-integer-default=0. Fractional mass flag.
CHAPTER 10
Upward Compatibility
10.2
Summary of Data Block Changes from MSC.Nastran
2004 to MSC.Nastran 2005
The following material describes changes in table data blocks for only those records
that existed in MSC.Nastran 2005.
DYNAMIC - Table of Bulk Data entry images related to dynamics
Added the following real-valued words for initial displacement and velocity factors
after the TID item on the TLOAD1 record and after the B item on the TLOAD2 record
after.
Item
Type
Description
U0
Real
Initial displacement factor for enforced motion
V0
Real
Initial velocity factor for enforced motion
GEOM2 - Table of Bulk Data entries related to element connectivity
Changed names and header words for the following records:
MSC.Nastran 2004
MSC.Nastran 2005
Name
Header Words
Name
Header Words
BEAMAERO
(2601,26,0)
BEAMAERO
(1701,17,0)
CHEXAL
(7708,77,369)
CHEXAL
(7908,79,369)
Q4AERO
(3002,46,0)
AEROQ4
(2002,20,0)
T3AERO
(2701,27,0)
AEROT3
(1801,18,0)
GEOM4 - Table of Bulk Data entry images related to constraints
Changed the type of the enforced displacement value, D on the SPCD and SPC records
from single-precision to machine-precision. Also added a null item in front preceding
D.
251
252
RESP12 - Table of second level (synthetic) responses
Inserted four more items after word 5 (item REG):
Item
Type
Description
METH
Integer
Method flag for BETA/MATCH responses
C1
Real
Constant to scale beta responses
C2
Real
Constant to scale distance responses
C3
Real
Constant to shift lower bound
CHAPTER 10
Upward Compatibility
10.3
More Stringent Case Control Check
Previous versions of MSC.Nastran check the first 4 characters of the Case Control
command. For example, to request displacement output, any one of the following
commands is acceptable prior to MSC.Nastran 2005.
Disp = all
Displ = all
Displa = all
Displacement = all
Displcement = all
Starting in MSC.Nastran 2005, the full spelling is checked. Correctly spelled short
forms are still acceptable (e.g., disp, etc.) For the above example, the first four
commands are acceptable. The last one, due to the misspelled command, will cause
the job to terminate with the following fatal message:
*** USER FATAL MESSAGE 601 (IFP1D)
THE KEYWORD ON THE ABOVE CARD TYPE IS ILLEGAL OR MISSPELLED.
This change is necessary to alleviate problems caused by the lack of uniqueness for
checking only 4 characters for certain commands. In versions prior to
MSC.Nastran 2005, the following 2 commands
Elstress = all
Elstrain = all
are both treated as element stresses (elst). Starting in MSC.Nastran 2005, the
command, ELSTRAIN, will terminate the job with UFM 601 as elstrain is a nonexisting command.
253
254
I
N
D
E
X
MSC.Nastran Release Guide
I N D E X
MSC.Nastran
Release Guide
A
acceleration load, 216
ACMS
Geometric Domain, 74
Matrix Domain, 74
adjoint loads, 125
ADS optimizer, 131
Application Program Interface (API), 218
Arbitrary Beam Cross Section, 96
ASSIGN, 203
ASSIGN File Management statement
specification of, 231
B
beam cross section, 96
beam offsets, 41
Big Endian, 204
BIGDOT optimizer, 136
buckling, 41
Bulk Data Entries
ACCEL, 216
ACCEL1, 216
DOPTPRM, 122, 134, 138
DRESP1, 114, 125, 137
DRESP2, 117
FLUTTER, 200
MATHP, 54
MATS1, 55
NLRSFD, 152
NSTEPNL, 55
PBMSECT, 96
PBRSECT, 96
PUNCH, 214
RADBC, 223
SPC, 213
SPCD, 213
SUPORT, 158
TMPSET, 55, 64
TOPVAR, 136
TSTEPNL, 63
TTEMP, 55, 64
WALL, 8
256 INDEX
Bulk Data Parameters
AUTOQSET, 198
BAILOUT, 77
COMPMATT, 81
COUPMASS, 89
DESPCH, 140
EPSILONT, 81
FASTFR, 78
FKSYMFAC, 54
FOLLOWK, 54
LANGLE, 54
LGDISP, 54
MAXLP, 54
MODEOUT, 167
NDAMP, 54
NLAYERS, 54
NLPACK, 54
NLTOL, 54
OELMSET, 208, 209
OGRDOPT, 208
OGRDSET, 208, 209
OMSGLVL, 208
OPCHSET, 208
PH2OUT, 54
POST, 160
SRCOMP, 115
UHVOLD, 168
ZROCMAS, 102
C
Case Control, 253
Case Control Commands
ADAMSMNF, 198
ANALYSIS, 45, 54
ASSIGN, 226
MODESELECT, 103
NLRESTART, 54
NLSTRESS, 54
POST, 226, 227
STEP, 45, 54
SUBCASE, 45
compliance, 137
compute conjugate matrix multiplication,
215
convergence criteria, 47
crash simulation, 31
c-set masses, 102
D
Data Block
DYNAMIC, 251
GEOM2, 251
GEOM4, 251
RESP12, 252
DDAM, 157
DFREQ, 128
DIAG 39, 201
displacement output filters, 224
Distributed Memory Parallel (DMP), 75
DMAP modules, 242
DMIG, 87
DOT optimizer, 131
DPD module, 109
Dynamic Design Analysis Method (DDAM),
158
dynamic excitation, 109
dynamic relaxation, 7
E
Elasto-Plastic material, 67
Endian, 204
ENDTIME, 15
enforced displacement, 213
enforced motion, 110
error factors, 47
Explicit Nonlinear (SOL 700), 6
External Superelement, 75, 76
F
F06 output file, 161, 226
feasible design, 122
File Management Statements
ASSIGN, 53, 159
RESTART, 53
fluid modes, 103
INDEX
flutter analysis, 199
fractional mass, 137
G
GDACMS, 130
GENEL, 87
global ply IDs, 83
GPFORCE, 87
I
Implicit Nonlinear
SOL 600, 33
initial condition, 110
ISHELL, 158
L
large-field input, 214
Little Endian, 204
LS-Dyna, 6
lumped mass, 89
M
matrix diagonal, 77
MAXRATIO, 77
MDACMS, 130
MFREQ, 128
modal effective mass, 103
modal frequency response, 78, 125
modal mass, 170
modal masses, 180
MPYAD, 215
MSC.Access, 218
MSC.ADAMS, 197
MSC.ADAMS modal neutral file, 198
MSC.Marc, 36
MSC.Patran, 192
multiple boundary conditions, 128
multiple-hardening-slopes, 67
N
NLRSFD, 150
Nonlinear Iteration Summary Table, 48, 52
NRL summation, 177
O
OP2, 206
OP4UTIL, 204
OUTPUT2, 159, 203, 227
OUTPUT4, 158, 203
P
parallel processing, 39
participation factors, 179
PBUSHT, 41
PCOMPG, 83
PKNLS, 199
PKS, 199
ply results tracking, 83
PUNCH, 214
Q
QUADR, 92
R
reduced OP2 file, 206
residual vectors, 125
Restart, 50
results recovery, 226
S
shock coefficients, 180
shock spectra, 190
shock spectrum, 162
SMPYAD, 215
SOL 129, 47
SOL 187, 158
257
258 INDEX
SOL 200, 125, 130, 131, 201
SOL 400, 43
NLRESTART, 50
NLSTAT, 43
NLTRAN, 43
outputs, 52
PARAM,NLPACK, 52
PARAM,PH2OUT, 52
STEP, 43
TLOAD1, 51
TMPSET, 44, 51
TSTEP, 43
TSTEPNL, 44
TTEMP, 44, 51
SOL 600
beam, 33
Bulk Data Entries
PARAMARC, 40
Bulk Data Parameters
MARCFIL1, 35
MARCOUTR, 40
MARCWIND, 41
MRAFFLOW, 39
MRMTXNAM, 35
MRRCFILE, 36
MRSPAWN2, 36
CONTINUE, 33
dmap, 33
Implicit Nonlinear, 33
SOL 700, 8
Bulk Data Entries
BCTABLE, 17, 23
CBUTT, 19, 23
CCRSFIL, 19, 23
CDAMP1D, 17, 23
CDAMP2D, 17, 23
CELAS1D, 17, 23
CELAS2D, 17, 23
CFILLET, 18, 23
COMBWLD, 19, 23
CSPOT, 18, 23
DAMPGBL, 19, 23
EOSPOL, 19, 23
MATD001, 23
MATD003, 24
MATD005, 24
MATD006, 24
MATD012, 24
MATD013, 24
MATD014, 24
MATD015, 24
MATD018, 24
MATD019, 24
MATD020, 24
MATD022, 24
MATD024, 24
MATD026, 24
MATD027, 24
MATD028, 24
MATD031, 24
MATD054, 24
MATD057, 24
MATD059, 24
MATD062, 24
MATD063, 24
MATD064, 24
MATD077, 25
MATD080, 25
MATD081, 25
MATD100, 25
MATD127, 25
MATD181, 25
MATD20M, 20, 24
MATD2AN, 24
MATD2OR, 23
INDEX
MATDxxx, 20
MTD030, 24
RBE3D, 22, 25
TIC3, 23
TICD, 23, 25
WALL, 23, 25
Bulk Data Parameters
DYBEAMIP, 26
DYBLDTIM, 25
DYBULKL, 25
DYCMPFLG, 26
DYCONECDT, 25
DYCONENMASS, 25
DYCONIGNORE, 25
DYCONPENOPT, 25
DYCONRWPNAL, 25
DYCONSKIPRWG, 26
DYCONSLSFAC, 25
DYCONTHKCHG, 25
DYCOWPRD, 25
DYCOWPRP, 25
DYDCOMP, 27
DYENDTIM, 25
DYENERGYHGEN, 26
DYENGFLG, 26
DYEPSFLG, 26
DYHRGIHQ, 26
DYHRGQH, 26
DYIEVERP, 26
DYINISTEP, 25
DYLDKND, 25
DYMATS1, 25
DYMAXINT, 26
DYMAXSTEP, 26
DYMINSTEP, 26
DYN3THDT, 27
DYNAMES, 25
DYNEIPH, 26
DYNEIPS, 26
DYNINTSL, 27
DYRBE3, 26
DYRLTFLG, 26
DYSHELLFORM, 26
DYSHGE, 27
DYSHNIP, 26
DYSHTHICK, 26
DYSIGFLG, 26
DYSTATIC, 25
DYSTEPFCTL, 26
DYSTRFLG, 26
DYSTSSZ, 27
DYTERMNENDMAS, 26
DYTSTEPDT2MS, 26
DYTSTEPERODE, 26
Explicit Nonlinear, 6
ID, 9
NOERROR, 15
NP, 14
STOP, 14
SPC, 213
SPCD, 213
spot welds, 74
Squeeze Film Dampers (SFDs), 150
stiffness update strategy, 48
structure modes, 103
Subroutines
DBFLOC, 218
OPENC, 219
OPENR, 220
OPENSQ, 222
System Cell
QRMETH, 92
System Cells
414, 89
ITRFMT(401), 53
STPFLG(366), 53
TZEROMAX(373), 53
T
temperature excitation, 51
temperature-dependent composites, 80
Temperature-Dependent Stress Strain
Curves, 37
thermal results, 223
time integration method, 48
Topology optimization, 135
Torsional Mass Moment of Inertia, 88
transient response, 110
TRLG module, 110
259
260 INDEX
U
unsymmetric laminates, 80
V
Variable Endian, 203
W
work error, 47
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertisement