Response

Document Sample
Response Powered By Docstoc
					                  RESPONSE User Manual

                                       Version 12




ANSYS, Inc.
Southpointe
275 Technology Drive
Canonsburg, PA 15317
ansysinfo@ansys.com
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494



                 © Copyright 2009. Century Dynamics Limited. All Rights Reserved.
                        Century Dynamics is a subsidiary of ANSYS, Inc.
                    Unauthorised use, distribution or duplication is prohibited.

                             ANSYS, Inc. is certified to ISO 9001:2008
                                                Revision Information

 The information in this guide applies to all ANSYS, Inc. products released on or after this date, until
superseded by a newer version of this guide. This guide replaces individual product installation guides
                                        from previous releases.

                                 Copyright and Trademark Information
  © 2009 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.

    ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT and any and all ANSYS, Inc. brand,
    product, service and feature names, logos and slogans are registered trademarks or trademarks of
     ANSYS, Inc. or its subsidiaries located in the United States or other countries. ICEM CFD is a
 trademark used by ANSYS, Inc. under license. All other brand, product, service and feature names or
                         trademarks are the property of their respective owners.

                                                  Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE
SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS
   SUBSIDIARIES, OR LICENSORS. The software products and documentation are furnished by
ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement that contains provisions
    concerning non-disclosure, copying, length and nature of use, compliance with exporting laws,
   warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software
products and documentation may be used, disclosed, transferred, or copied only in accordance with the
                       terms and conditions of that software license agreement.

                                      ANSYS, Inc. is certified to ISO 9001:2008

                                             U.S. Government Rights
    For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license
agreement, the use, duplication, or disclosure by the United States Government is subject to restrictions
    stated in the ANSYS, Inc. software license agreement and FAR 12.212 (for non-DOD licenses).

                                               Third-Party Software
      The products described in this document contain the following licensed software that requires
                                  reproduction of the following notices.

Formula One is a trademark of Visual Components, Inc.
The product contains Formula One from Visual Components, Inc. Copyright 1994-1995. All rights
reserved.

     See the legal information in the product help files for the complete Legal Notice for ANSYS
   proprietary software and third-party software. If you are unable to access the Legal Notice, please
                                          contact ANSYS, Inc.


                                                  Published in the U.S.A.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
                       RESPONSE User Manual
                                Update Sheet for Version 12
                                        April 2009



Modifications:

The following modifications have been incorporated:

Section               Page(s)                 Update/Addition          Explanation

All                   All                     Update                   Conversion to Microsoft® Word format

3.5                   3-5                     Update                   Delete references to legacy program PICASO

App A.12.1            A-8                     Update                   Delete references to legacy program FRAKAS




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
 RESPONSE User Manual                                                                                                        Contents


                                                         TABLE OF CONTENTS


 1.   Introduction ..................................................................................................................... 1-1
   1.1.     General Theory........................................................................................................ 1-1
   1.2.     Steady State Response ............................................................................................. 1-2
   1.3.     Response Spectrum Analysis .................................................................................. 1-3
   1.4.     Transient Response ................................................................................................. 1-6
   1.5.     Response Syntax Diagrams ..................................................................................... 1-7
 2. Data Formats ................................................................................................................... 2-1
   2.1.     General Syntax ........................................................................................................ 2-1
      2.1.1.     Special Symbols .............................................................................................. 2-4
   2.2.     Data Generation Facilities ....................................................................................... 2-5
      2.2.1.     Repeat Facilities .............................................................................................. 2-5
      2.2.2.     Re-Repeat Facilities ........................................................................................ 2-6
   2.3.     UNITS ..................................................................................................................... 2-8
      2.3.1.     UNITS for Input Data ..................................................................................... 2-8
   2.4.     Solution Type .......................................................................................................... 2-9
   2.5.     Steady State Response Data .................................................................................. 2-10
      2.5.1.     UNITS in Steady State Data.......................................................................... 2-10
      2.5.2.     Damping Data for Steady State Response..................................................... 2-11
         2.5.2.1. DAMP Data block ..................................................................................... 2-11
         2.5.2.2. LOSS Data................................................................................................. 2-12
      2.5.3.     Loading Data ................................................................................................. 2-14
         2.5.3.1. Nodal Loads .............................................................................................. 2-16
         2.5.3.2. Distributed Loads ...................................................................................... 2-17
         2.5.3.3. Pressure Loads........................................................................................... 2-18
   2.6.     Seismic Response Data ......................................................................................... 2-23
      2.6.1.     UNITS for Seismic Data ............................................................................... 2-24
      2.6.2.     Damping Data for Seismic Response ............................................................ 2-24
         2.6.2.1. Damping Data ........................................................................................... 2-25
         2.6.2.2. LOSS Data................................................................................................. 2-26
      2.6.3.     Response Spectrum Data ............................................................................... 2-27
         2.6.3.1. Ordinate Definition ................................................................................... 2-28
         2.6.3.2. Axis Definition and Interpolation Command ............................................ 2-28
         2.6.3.3. Spectrum Damping Command .................................................................. 2-29
         2.6.3.4. Spectrum Definition .................................................................................. 2-30
      2.6.4.     Seismic Combination Data ............................................................................ 2-33
         2.6.4.1. The Output Motion Data ........................................................................... 2-35
         2.6.4.2. Loadcase Combination Data ..................................................................... 2-36
   2.7.     Transient Response Data ....................................................................................... 2-40
      2.7.1.     UNITS for Transient Data ............................................................................. 2-40
      2.7.2.     Damping Data for Transient Response ......................................................... 2-41
         2.7.2.1. Damping Data ........................................................................................... 2-41
         2.7.2.2. Loss Data ................................................................................................... 2-42
      2.7.3.     Transient Function Data ................................................................................ 2-43
         2.7.3.1. Transient Function Header ........................................................................ 2-44




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                     i
 RESPONSE User Manual                                                                                                      Contents


         2.7.3.2. Transient Function Definition ................................................................... 2-45
      2.7.4.     INITIAL Conditions ...................................................................................... 2-46
      2.7.5.     LOADING Data ............................................................................................ 2-47
         2.7.5.1. SEISMIC Load .......................................................................................... 2-48
         2.7.5.2. NODAL Load ............................................................................................ 2-50
      2.7.6.     RESULTS Output ......................................................................................... 2-52
         2.7.6.1. OUTPUT Times ........................................................................................ 2-53
         2.7.6.2. Selecting Stress Output ............................................................................. 2-53
         2.7.6.3. Selecting Nodal Output ............................................................................. 2-54
   2.8.     LOADFILE Analysis Data .................................................................................... 2-55
      2.8.1.     UNITS for LOADFILE Data ........................................................................ 2-56
      2.8.2.     Damping Data for LOADFILE Analysis ...................................................... 2-56
         2.8.2.1. Damping data block .................................................................................. 2-56
         2.8.2.2. Loss Data ................................................................................................... 2-57
      2.8.3.     Loadcase Selection ........................................................................................ 2-58
   2.9.     STRESS Analysis Data ......................................................................................... 2-59
      2.9.1.     STOP ............................................................................................................. 2-59
 3. Examples ......................................................................................................................... 3-1
   3.1.     Steady State Analysis .............................................................................................. 3-1
   3.2.     Seismic Analysis ..................................................................................................... 3-2
   3.3.     Transient Analysis ................................................................................................... 3-3
   3.4.     Loadfile Analysis .................................................................................................... 3-4
   3.5.     Stress Calculation Analysis ..................................................................................... 3-4
 Appendix A - Preliminary Data for RESPONSE .............................................................. A-1
   A.1      Preliminary Data .................................................................................................... A-1
   A.2      SYSTEM Command .............................................................................................. A-2
   A.3      PROJECT Command ............................................................................................. A-2
   A.4      JOB Command ....................................................................................................... A-3
   A.5      FILES Command.................................................................................................... A-3
   A.6      TITLE Command ................................................................................................... A-4
   A.7      TEXT Command .................................................................................................... A-4
   A.8      STRUCTURE Command ....................................................................................... A-5
   A.9      NEWSTRUCTURE Command .............................................................................. A-5
   A.10 OPTIONS Command ............................................................................................. A-6
   A.11 RESTART Command ............................................................................................ A-6
   A.12 SAVE Command .................................................................................................... A-7
      A.12.1 Files for Numerical Processing ...................................................................... A-7
      A.12.2 Interface Files for Plotting Programs ............................................................. A-8
   A.13 RESU command ..................................................................................................... A-9
   A.14 UNITS Command .................................................................................................. A-9
   A.15 END Command .................................................................................................... A-11
 Appendix B - Running Instructions for RESPONSE ........................................................ B-1
   B.1      ASAS Files Required by RESPONSE ................................................................... B-1
   B.2      Saving Files Produced by RESPONSE .................................................................. B-1
   B.3      Running Instructions for RESPONSE.................................................................... B-1
 Appendix C - Options ........................................................................................................ C-1




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                                  ii
 RESPONSE User Manual                                                                                            Contents


   C.1   Miscellaneous Options ........................................................................................... C-1
   C.2   Options which Control the Printing of the Data File Images ................................. C-1
   C.3   Options which Control the Printing of Expanded Data Lists ................................. C-2
   C.4   Options which Affect the Course of the Analysis .................................................. C-2
   C.5   Options which Control Printing During the Run ................................................... C-2
   C.6   Options which Control the Printing of Results ...................................................... C-3
   C.7   Special Analysis Options ....................................................................................... C-4
   C.8   Options to Save Data and Results on File .............................................................. C-5
 Appendix D - Restart Stages for RESPONSE ................................................................... D-1
   D.1   Restart Stages for Steady State Analysis................................................................ D-1
   D.2   Restart Stages for Seismic Analysis ....................................................................... D-1
   D.3   Restart Stages for Transient Analysis .................................................................... D-2
   D.4   Restart Stages for Loadfile Analysis ...................................................................... D-2
   D.5   Restart Stages for Solution Stress .......................................................................... D-2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                      iii
RESPONSE User Manual                                                                                    Introduction



RESPONSE
Dynamic Response Analysis


1.     Introduction

RESPONSE is a post-processor in the ASAS system and is used for structural dynamic response calculations.
Three methods of analysis are available:

(a)    response to a sinusoidally varying load (‘steady state’ response);

(b)    response to seismic excitation using the Response Spectrum method;

(c)    transient response due to time-varying loads and support accelerations (time history analysis).


RESPONSE can also be used to calculate eigenvector stresses from an ASAS natural frequency analysis.

RESPONSE can only be used following an ASAS natural frequency analysis.


1.1. General Theory

A finite element representation of problems in structural dynamics gives rise to a matrix equation of the form:

         x 
        M+ Cx+ Kx = R(t) ................................        (1)


in which M, C and K refer to mass, damping and stiffness matrices respectively. The x and R vectors define the
time varying displacements and loads. A dot denotes differentiation with respect to time.

The above equation represents a set of simultaneous differential equations. It is possible to perform a coordinate
transformation which decouples these equations so that they reduce to a set of independent ordinary differential
equations. Analysis is then simplified to operating on each equation individually rather than the problem of
solving the coupled system.

This procedure is used for dynamic response calculations in RESPONSE and is known as the normal mode
method. ASAS is the used to calculate the eigenvalues (ω) and the eigenvectors or mode shapes (φ) of the
structure. If a transformation is applied to equation (1) such that:
        x =φY

and if equation (1) is premultiplied by φΤ

then equation (1) becomes:

                       
        φT M φ Y+ φT C φ Y+ φT K φ Y = φT R(t)                                           (2)




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 1-1
RESPONSE User Manual                                                                                            Introduction


The above matrix equation represents a set of uncoupled equations and hence a separate equation for each mode
n can be written as:

                 
        M n Y + Cn Y n + K n Y n = P n (t) .................                  (3)


in which
                                                                                            φn Mφn
                                                                                                T
Mn          =            generalised mass for mode n                           =
                                                                                            φ n Cφ n = 2 ξ n ω n Mn
                                                                                               T
Cn          =            generalised damping for mode n                        =
                                                                                            φ n K φ n = ω n 2 Mn
                                                                                               T
Kn          =            generalised stiffness for mode n                      =
                                                                                            φ n R(t)
                                                                                               T
Pn(t)       =            generalised loading for mode n                        =

It should be noted that damping information is seldom in a form implied by equation (1).

Within RESPONSE the damping information may be defined by one of two methods:

(a)     Using the DAMP data block where the damping is defined for each mode and loadcase directly as a
percentage of critical damping.

(b)     Using the LOSS data block where the damping is defined on an element/group/material basis and the
damping factor Cn for mode n is calculated from


                                  1 (φ                         )
                                  NEL

                         ∑=
                          e
                                         T
                                         ne   K e φ ne Ce
                 Cn =
                                    1 (φ                   )
                                   NEL

                           ∑= e
                                           T
                                           ne   K e φ ne




With the frequencies (ω) and mode shapes (φ) obtained from ASAS by a natural frequency analysis, RESPONSE
sets up the generalised terms in equation (3) and obtains a solution to the differential equation in one of three
ways.

For a more detailed theoretical discussion on dynamic response analysis, the user is referred to the standard text
books, for example, ‘Dynamics of Structures’, R.W. Clough and J Penzien, McGraw-Hill, 1982.


1.2. Steady State Response

If the forces acting on the original structure R(t) are harmonic then so is the generalised forcing function Pn(t).
Consequently the solution to equation (3) can be obtained explicitly. In predicting dynamic response it is often
important to establish and retain phase relationships. The steady state solution employed by RESPONSE retains
this information by calculating the structural response using complex variable techniques.

Writing the generalised loading for mode n as:




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 1-2
RESPONSE User Manual                                                                                    Introduction


            Pn(t)         =            A Cos νt + B sin νt
                          =            P1 + iP2

where ν is the forcing frequency, then the response is:

                                          P1 + iP 2
                 q1 + iq 2 =                                  1
                                         2
                                             2
                                                 2ξ ν r   2
                                                          2
                                2 
                                   1 - ν 2  +         
                               ωn 
                                   ω n   ωn  
                                                       
                                  

The uncoupled solutions are then transformed back into the original coordinate system and the stresses recovered
from the displacements using the element stiffness properties.

RESPONSE outputs real and imaginary parts of the nodal displacement vector and element stress vectors to
allow the phase differences to be obtained.

If the structure concerned is assembled from components in ASAS, it is possible to determine stresses and
displacements in the components by carrying out component recovery analysis in ASAS after RESPONSE. The
backing files are saved automatically and no additional command is required. This facility is available for steady
state solution only.


1.3. Response Spectrum Analysis

In a number of instances (eg earthquakes, wave loading) dynamic loading is random in nature and statistical
methods are used to represent them. One such measure, termed the response spectrum, represent the response of
an equivalent single degree of freedom system, (characterised by its frequency), to a prescribed random dynamic
loading. The response is typically expressed as peak values of acceleration, velocity or displacement across a
range of frequencies for a particular value of damping.
            sv                                                          sa


                                                                                                        Percentage of
                                                                                                        Critical
                                                                                                        Damping




                         PERIOD (S)                                                   PERIOD (S)




                                             Spectral Response of S.D.O.F. Structure




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 1-3
RESPONSE User Manual                                                                                                Introduction



                              sd
                              or
                              sv
                              or
                              sa




                                                   F1             F2            F3            F4        FREQUENCY (HZ)




                                         RESPONSE idealisation of the spectral curves

The response spectra for RESPONSE may be displacement, velocity or acceleration spectra and may be input for
up to 6 independent damping factors. The response spectrum is defined specifying the displacements, velocities
or accelerations at given frequencies. Values for intermediate frequencies and damping values are obtained by
linear or logarithmic interpolation.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 1-4
RESPONSE User Manual                                                                                    Introduction


With the frequencies and mode shapes determined from the ASAS natural frequency analysis, RESPONSE
calculates the response for each individual mode of the structure directly from the input response spectra using
the equation:

                                 Γn Sd( , ) ........
                     xn = φ n          ξn fn                                  (4)
                                 Mn

where       xn              =          displacement vector due to response in mode n


            Sd(ξ n , f n ) =           spectral displacement corresponding to the damping ξn and
                                       frequency fn of the nth mode of vibration.
            Γn              =          φT M
                                        n       is called the modal participation factor
            φn              =          mode shape describing mode n
            Mn              =          generalised mass for mode n
            M               =          mass matrix

The maximum stresses in mode n are given by substituting the displacements given by (4) into the stress
calculation routines from ASAS.

The maximum total response cannot be obtained, in general, by merely adding the modal maxima because these
maxima usually do not occur at the same time. Therefore, although the simple addition of the modal spectral
values provides an upper limit to the total response, it generally over-estimates this maximum by a significant
amount. A number of different formulae have been proposed to obtain a more reasonable estimate of the
maximum response from the spectral values, and several are implemented in RESPONSE. The simplest of these
is to use the square root of the sum of the squares of the modal responses. Thus, if the maximum modal
displacements are given by (4), the maximum total displacement is approximated by:

        x max. =       ( x1 )2 max+ ( x 2 )2 max+ ............                           (5)


where the terms under the square root represent vectors of the modal displacements squared.

Other modal summation methods are available in RESPONSE including the Ten Percent Method and Double
Sum Method described in the USNRC Regulatory Guide 1.9., and the Complete Quadratic Combination method.
These methods attempt to account for cross-correlation between the modes, especially when they are closely
spaced or when symmetric modes occur.

For structures which are excited in more than one direction, the responses in each of the three coordinate
directions must also be combined.                Several spatial summation methods are provided, including absolute
summation, square root of the sum of the squares, and the US Naval Research Laboratory method of the
maximum response plus the SRSS summation of the other two.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 1-5
RESPONSE User Manual                                                                                                Introduction


1.4. Transient Response

The response of structures to general time-varying or blast loads are calculated using the transient analysis
technique. The method adopted by RESPONSE is the Modal Superposition Method. The equation of motion of
the body is uncoupled to n single degree of freedom systems, where n is the number of eigenvalues and
eigenvectors calculated in the ASAS natural frequency analysis. The one degree of freedom system is

              + 2ξω x+ ω2 x = f(t) .............. ................
             x                                                                           (6)

The solution to the n one degree of freedom systems are achieved using the convolution integral, or generally
known as the Duhamel integral, ie

                                       -ξω (t-τ )
                                 e
                      ∫ f(τ )                       sin ω D (t- τ ) d τ
                       t
            x(t) =                                                                        (7)
                                ωD
                       0


            where          ξ       =       percentage of critical damping
                           ω       =       angular frequency
                           ωD      =       damped angular frequency =                    ω 1- ξ 2
The individual modal responses of the n one degree of freedom systems are then recoupled by using the
following transformation

                           Y       =       φx ............ ................ ................ ................ (8)
            where          Y       =       resultant structural response
                           x       =       modal response
                           φ       =       eigenvectors

Facilities are available within the transient solution to allow the structure to have non-zero initial displacements
and/or initial velocities. These initial conditions are applied by calculating the response of the structure due to
damped free vibration i.e.

                                x + ξω x 
                                                                 
            x(t) =     e-ξω t  
                               ω
                                            sin ωD t + xcos ωD t 
                                                                                                    (9)
                                    D                          

then the final structural response is the summation of the initial conditions response plus the forcing function
response.

Transient analysis can result in a substantial amount of output, which is not only expensive to produce, but
difficult to assimilate. The RESULTS Data Input in RESPONSE enables the selection of which nodes and
elements are to be reported, and at which times. In this way, if the state of stress throughout a structure is
required at the time corresponding to the peak response of a particular freedom, it is not necessary to print the
full response at every timestep.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                  Page 1-6
RESPONSE User Manual                                                                                    Introduction


1.5. Response Syntax Diagrams

(a) Preliminary Data and Solution Type

A detailed description of these commands can be found in Section 2.4 and Appendix A.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 1-7
RESPONSE User Manual                                                                                    Introduction


b) Steady State Analysis

For a more detailed description of these commands, see Section 2.5.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 1-8
RESPONSE User Manual                                                                                    Introduction


c) Seismic Analysis
For a more detailed description of these commands, see Section 2.6.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 1-9
RESPONSE User Manual                                                                                    Introduction


d) Transient Analysis
For a more detailed description of these commands, see Section 2.7.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 1-10
RESPONSE User Manual                                                                                    Introduction


e) WAVE Steady State Analysis

For a more detailed description of these commands, see Section 2.8.
               LOADFILE          wave

               DAMP

               scase             fcase             smode             fmode             damp


               END



               LOSS

               MATP              matno              damp


               GROU              grpno              damp


               ELEM              elno               damp


               END



               SELE

                         case


               END



               STOP




f) Stress Calculation Analysis

For a more detailed description of these commands, see Section 2.9.

              SOLUTION             STRESS


              STOP




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 1-11
RESPONSE User Manual                                                                                    Introduction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 1-12
       RESPONSE User Manual                                                                               Data Formats




2.      Data Formats


2.1. General Syntax

The input data for RESPONSE are specified according to syntax diagrams similar to that shown below. The
conventions adopted are described in the following pages.

            HEADER

            KEYWORD                          alpha                integer                real

            END




Each data block commences with a compulsory header line and terminates with an END command which
delimit this information from any other data. The sequence of the input data follows the vertical line down the
left hand side of the page.

Within a data block, each horizontal branch represents a possible input instruction. Input instructions are
composed of keywords (shown in upper-case), numerical values or alphanumerics (shown in lower-case
characters), and special symbols. Each item in the list is separated from each other by a comma or one or more
blank spaces.

An input line must not be longer than 80 characters.

Numerical values have to be given in one of two forms:

(i)     If an integer is required a decimal point must not be supplied.

(ii)    If a real is required the decimal point may be omitted if the value is a whole number.


Exponent formats may be utilised when real numbers are required.

        For example                0.004        4.0E-3        4.0D-3       are equivalent

        similarly                  410.0        410           4.10E2       have the same value


Alphanumerics must begin with an alpha character (A-Z). The letters A-Z may be supplied in either upper or
lower case but no distinction is made between the upper and lower case form. Hence “A” is assumed identical
with “a”, “B” with “b” and so on.

        For example                CASE         are all permissible alphanumeric strings
                                   STR1
                                   END


  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 2-1
   RESPONSE User Manual                                                                                 Data Formats


      also                       COMB         are all identical strings
                                 Comb
                                 comb

      However                    3BMD         are examples of inadmissible alphanumeric strings
                                 5BL




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 2-2
    RESPONSE User Manual                                                                                 Data Formats


Alphanumeric strings must not include any special symbols (see below)



If certain lines are optional, these are shown by an arrow which bypasses the line(s)



                 KEYWORD                          integer




In order to build up a block of data, a line or a series of lines may need to be repeated until the complete set has
been defined. This is shown by an arrow which loops back.



                 KEYWORD                          integer




Some data lines require an integer or real list to be input whose length is variable. This is shown by a horizontal
arrow around the list variable(s).



                KEYWORD                          real                        (integer)




A parameter enclosed in brackets is optional



Where one or more possible alternative items may appear in the list, these are shown by separate branches for
each




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 2-3
       RESPONSE User Manual                                                                                            Data Formats


2.1.1.         Special Symbols


                                                  KEYWORD1
                                                                                       integer
                     integer                      KEYWORD2


                                                  KEYWORD3                             real

The following is a list of characters which have a special significance to the RESPONSE input.



*         An asterisk is used to define the beginning of a comment, whatever follows on the line will not be
          interpreted. It may appear anywhere on the line, any preceding data will be processed as normal. For
          example

                   * THIS IS A COMMENT FOR THE WHOLE LINE
                   case 4 2.7 * THIS IS A COMMENT FOR PART OF A LINE




’         single quotes are used to enclose some text strings which could contain otherwise inadmissible characters.

          The quotes are placed at each end of the string. They may also be used to provide in-line comments

          between data items on a given line.

          For example

                       STRUCTURE            ’As used for design study’                           STRU




,         A comma or one or more consecutive blanks will act as a delimiter between items in the line.

          For example                5, 10, 15                                is the same as           5    10    15



          Note that two commas together signify that an item has been omitted. This may be permissible for
          certain data blocks.

          For example                5,, 15                                  is the same as            5    0    15

          Unless otherwise stated in the section describing the data block, omitted numerical values are zero.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 2-4
       RESPONSE User Manual                                                                                  Data Formats


/ /       Variables shown in the syntax contained within single slashes correspond to data which may be generated
          using the Repeat (RP) facility. The slashes must not appear in the actual data.



// // Variables contained within double slashes may be generated using the Repeat (RP) and the Re-repeat
          (RRP) facilities. The slashes must not appear in the actual data.


2.2. Data Generation Facilities



2.2.1.         Repeat Facilities

Lists of regular data can often be shortened by use of a repeat facility. A block of one or more lines of data may
be identified by a delimiter character (/) and terminated by a repeat command (RP). The repeat command
contains information on how many times the set of lines of data is to be generated and how the data is to be
incremented for each generation. The general form is:
                 /

                 KEYWORD                              real                        /integer/

                 RP                                   nrep                         incr


/                    : is the delimiter character to identify the start of the data to be generated. It must be on a line of
                       its own.

KEYWORD              : items notenclosed within slashes will be repeatedwithout any increment for generated
                       real              data

/integer/            : an item enclosed by / characters indicates data which may be modified using the repeat facility.
                       The / characters must not appear in the actual data.

RP                   : command word to identify the end of the data to be generated.

nrep                 : number of times the set of lines is to be generated, including the original data line(s).

incr                  : the increment to be added to certain data items for the second and subsequent generated blocks.
                       (The first block corresponds to the original data)

For example, suppose the data format is specified as

               KEYWORD                               /integer/




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page 2-5
    RESPONSE User Manual                                                                                       Data Formats


It is required to generate the regular list of integers 1, 6, 11, 16, 21, 26, 31, 36, 41, 46. If the keyword is ALL the
data could be input as

             ALL        1          6         11         16         21        26         31         36    41   46

   or
             ALL        1
             ALL        6
             ALL        11
             .
             .
             .
             ALL        46

Using the repeat facility, the following example all produce identical data

   (i)       /
             ALL        1
             RP         10         5


   (ii)      /
             ALL        1          6
             RP         5          10


   (iii)     /
             ALL        1
             ALL        6
             RP         5          10




2.2.2.      Re-Repeat Facilities

The repeat facility can be extended to include a double repeat whereby data which has been generated by use of
the RP command may be repeated again using different increment values. The general form is:




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 2-6
           RESPONSE User Manual                                                                              Data Formats




                       //

                       /

                       KEYWORD                             real                        //integer//

                       RP                                  nrep                         incr1


                       RRP                                 nrrep                        incr2




//                    : identifies the start of the data to be re-repeated. It must precede a / line

/                     : identifies the start of the data to be repeated.

KEYWORD               : items not enclosed within slashes will be repeated without any increment for generated
                           real           data.

//integer//           : an item enclosed by // characters indicates data which may be modified using the re-repeat or
                           repeat facility. The // characters must not appear in the actual data.

RP                    : identifies the end of the data to be generated with the repeat facility.

nrep                  : number of times the block of data is to be generated, including the original data line(s)

incr1                 : the increment to be added to the data items for the second and subsequent generated blocks.
                           (The first block corresponds to the original data)

RRP                   : identifies the end of the data to be generated with the re-repeat facility.

nrrep                 : the number of times the expanded data from the repeat block is to be further generated,
                           including the original repeat block

incr2                 : the increment to be added to each of the expanded data items for the second and subsequent re-
                           generated blocks. (The first block corresponds to the expanded data items)

For example, taking the example in Section 2.2.1, if the data syntax was specified as

                      KEYWORD                                     //integer//




then the data could be

       //
       /

     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 2-7
    RESPONSE User Manual                                                                                 Data Formats


   ALL       1
   RP        5          10                   generates             1 11 21 31 41
   RRP       2          5                    generates             6 16 26 36 46

Note, the order of the numbers generated by this example in Section 2.2.1 using RP and in Section 2.2.2 using
RP and RRP is different. This may be important in a few cases where the order of the data supplied matters, for
example, the generation of user element numbers or the order of LINK nodes for assembly at a higher level.


2.3. UNITS

If units have been employed in the previous analysis it is possible to specify modified units for both the input
data and the results. The default units will be those utilised in the original analysis and if this is satisfactory no
additional information is required in the RESPONSE run.

If it is required to input the RESPONSE data in a different system of units, this can achieved by specifying one
or more UNITS commands within the main body of the RESPONSE data thus permitting a combination of unit
systems within the one data file.

If the results are required in different units to the default, the UNITS command can be specified in the
Preliminary data. See Appendix A, preliminary data.

It is not possible to modify the analysis units from those used in the previous analysis.

If units were not employed in the previous analysis the units of all data supplied must be consistent with that
adopted for the original data. No modification to reported results is possible under these circumstances.




2.3.1.      UNITS for Input Data

If units were employed in the previous analysis, the input data may be modified locally by the inclusion of a
UNITS command. The local units are operational for the data block concerned and will return to the default
global units when the next data block is encountered (ie after the next END command.)


         UNITS                        unitm




Parameters

UNITS        : Keyword

unitnm       : name of unit to be utilised (see below)




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page 2-8
     RESPONSE User Manual                                                                                Data Formats


Notes


1.      Force, length and angular unit may be specified. Only those terms which are required to be modified
        need to be specified, undefined terms will default to those supplied by the global analysis units unless
        previously overwritten in the current data block.

2.      A list of valid unit names can be found in Appendix A.13.

3.      The default angular unit is radians.


2.4. Solution Type

This line defines the type of response analysis to be performed and is compulsory for all analyses. The type of
solution chosen will also dictate which other data blocks are required to complete the analysis.

                                                                  STEADY STATE

                        SOLUTION                                  SEISMIC

                                                                  TRANSIENT

                                                                  STRESS


                         LOADFILE                        w av e



Parameters

SOLUTION              : compulsory keyword to select the type of response analysis to be performed. (Not required
                         for LOADFILE analysis)

STEADY STATE :                    This analysis assumes simple harmonic loading, giving rise to steady state response.

SEISMIC               : This analysis calculates the response of structures due to earthquakes, using response
                         spectrum techniques.

TRANSIENT             : This analysis calculates the response of structures to general time-varying loads producing
                         a time-varying response (Time history)

STRESS                : This analysis calculates the stresses which would occur in a structure if displacements
                         equivalent to the normalized eigenvectors were applied.

LOADFILE               : This analysis is used when WAVE has been used to generate the relevant real & imaginary
                         loadings for a steady state response analysis.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 2-9
      RESPONSE User Manual                                                                                Data Formats


wave                   : This is the 4 character structure name associated with the WAVE analysis which generated
                          the loading.

Notes


(a)      The user must use one of either SOLUTION or LOADFILE but not both.

(b)      The data blocks relevant to each of the five types of analysis are described as follows;-

                 STEADY STATE ... ................ Section 2.5
                 SEISMIC ............... ................ Section 2.6
                 TRANSIENT .......... ................ Section 2.7
                 LOADFILE.............. ................ Section 2.8
                 STRESS ................ ................ Section 2.9



2.5. Steady State Response Data

In this analysis two types of data are valid:

1.       Damping data: This may be specified by means of either a DAMP data block or a LOSS data block.

         A DAMP data block is used to define the damping for each mode and each loadcase as a percentage of
         the critical damping.

         A LOSS data block is used to define the damping on a material/group/element basis. The damping for
         each mode will then be calculated by the program as described in Section 1.1.


2.       Loading data: This is specified by means of a LOAD data block. The loading may be formed from
         nodal, distributed and pressure loads.




2.5.1.       UNITS in Steady State Data

In the Steady State Data, the UNITS command is applicable to the following data blocks

                          LOAD


In the loading data, the locally defined units are only operational for the current load type and will return to the
default global units when the next loadcase or load type is encountered.

The following data blocks do not permit the use of a UNITS command

                          DAMP
                          LOSS



  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-10
       RESPONSE User Manual                                                                                            Data Formats


Example


                                                                                 Operational Units          Notes


LOAD 2                                                                           KN,m,radians               Global Definition
HARM        1        2     3.5
NODAL LO
UNITS N                                                                          N,m,radians                Force amplitude
*                                                                                                           in Newtons
X      15000.0              0.0      5
Y      12000.0              0.0      4
UNITS           MM                                                               N,mm,radians               moments input in
*                                                                                                           Nmm
RY       250.0              0.0      5
END
DISTRIBU                                                                         KN,m,radians               Units revert to global
*
Y        BL1             10.0      5.0       5.0          5         6
UNITS N                                                                          N,m,radian                 load intensity in
Y        BL1             15000.0         12000.0              5.0       6    7                              Newtons/metre
END
HARM        2        1     1.9                                                   KN,m,radians               New load case reverts
*                                                                                                           units to global
*
DISTRIBU
Z        BL5             12.0      10.0       6       7
END
STOP




2.5.2.          Damping Data for Steady State Response

Damping data may be defined in one of two forms. Firstly the damping may be defined as a single value for
each mode or each loadcase. Secondly the damping may be defined with respect to each material type, element
group or element.


2.5.2.1. DAMP Data block

The DAMP data specifies the damping as a percentage of critical damping for each mode and for each loadcase.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 2-11
    RESPONSE User Manual                                                                                 Data Formats



             DAMP

             scase             fcase             smode            fmode             damp

             END



Parameters

DAMP          : compulsory header to define the start of the damping data. Must appear alone on the line

scase         : starting loadcase number (Integer)

fcase         : finishing loadcase number (Integer)

smode         : starting mode number (Integer)

fmode         : finishing mode number (Integer)

damp          : percentage of critical damping associated with the given modes and loadcases (Real)

END           : compulsory word to define the end of the damping data. Must appear alone on the line

Note


The user may include as many lines of data as necessary between DAMP and END to fully define the damping
conditions for the analysis.

Example


This example defines a value of damping of 5% for modes 1 to 2, for loadcase 1 and 2% for mode 1 and 30% for
mode 2 for loadcase 2

        DAMP
        1      1      1       2      5.0
        2      2      1       1      2.0
        2      2      2       2      3.0
        END


2.5.2.2. LOSS Data

The LOSS data specifies the damping as a percentage of critical damping for each material, element group or
element. The overall value of damping is then calculated as described in Section 1.1.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-12
     RESPONSE User Manual                                                                                Data Formats



               LOSS


               MATP               matno            damp


               GROU               grpno            damp


               ELEM               elno             damp


               END




Parameters

LOSS         : compulsory header to define the start of the LOSS data.

MATP         : keyword to denote that damping is defined for a material type

matno        : material number to which the damping value is to be applied (Integer)

GROU         : keyword to denote that damping is defined for an element group number

grpno        : group number to which the damping value is to be applied (Integer)

ELEM         : keyword to denote that damping is defined for an element

elno         : user element number to which the damping value is to be applied (Integer)

damp         : percentage of critical damping associated with this material, group or element (Real)

END          : compulsory keyword to define the end of the LOSS data.

Notes


1.      The data within the LOSS deck may be ordered in any arbitrary sense but the hierarchy is as follows.
                Element definition takes precedence over the group definition and group definition
                takes precedence over the material definition.

Example




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-13
    RESPONSE User Manual                                                                                 Data Formats


         LOSS
         MATP       1       4.0
         GROU       1       2.0
         ELEM       3       1.0
         ELEM       4       1.0
         END



2.5.3.      Loading Data

This data defines the loading. Each loadcase consists of a set of sinusoidally varying external loads at a given
frequency. The loading can be any combination of nodal loads, distributed loads and face pressures.

The overall form of the loading data is shown below.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-14
   RESPONSE User Manual                                                                                 Data Formats



               LOAD             ncase

                HARM             case             ntype             freq



               NODAL LO

                (skew )          dof              ampli             phase                //node//

                END




               DISTRIBU

                (dof)            type             v alue            phase                 //node//

                END



               PRESSURE

                U                press            phase             //node//

                FIN




                F                phase              //node//
                FIN
                P                press              //node//
                FIN

                END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-15
    RESPONSE User Manual                                                                                 Data Formats


The LOAD command specifies the start of the steady state loadcases and how many cases are to be analysed.

          LOAD               ncase



Parameters

LOAD         : a compulsory keyword which is used to define the start of the load data

ncase        : number of loadcases to be analysed. (Integer)




The HARM command defines the start of each individual loadcase

          HARM                case               ntype                 freq




Parameters

HARM         : compulsory keyword to define the start of each loadcase

case         : loadcase number (Integer, 1-9999)

ntype        : number of different load types (Integer, 1-3)

freq         : forcing frequency Hz (Real)

Note


The individual loads which comprise a loadcase are defined in blocks. Steady state analyses allow three types of
loading

                -        Nodal loads
                -        Distributed loads
                -        Pressure loads



2.5.3.1. Nodal Loads

This data block defines the nodal loads for a loadcase




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-16
      RESPONSE User Manual                                                                                Data Formats



            NODAL LO

            (skew )             dof           ampli             phase                 //node//

            END



Parameters

NODAL LO           : keyword to denote the start of the block of nodal loads

skew               : skew integer. Optional. This skew system must have been defined in the ASAS natural
                     frequency analysis (Integer, 1-9999)

dof                : a freedom code (Character)

ampli              : amplitude of the load (Real)

phase              : phase angle of the load in degrees (Real)

node               : list of node numbers at which the load is applied (Integer, 1-999999)

END                : keyword denoting the end of the nodal loads

Note


The load definition data may be placed in blocks and use made of the RP and RRP facilities to generate lists of
node numbers.

Example


In this example, a nodal load of 100.0 with a phase of 10.0 degrees is applied to freedom X of nodes 1, 2, 3, 4, 5,
6, 7, 8, 9, 10, 11, 12

        NODAL            LO
        /
        X     100.0           10.0      1     2    3
        X     1.0E2           1.0E1     4     5    6
        RP 2         6
        END


2.5.3.2. Distributed Loads

This data block defines the distributed loads for a loadcase.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-17
      RESPONSE User Manual                                                                               Data Formats



            DISTRIBU

             (dof)            type             v alue            phase                 //node//

             END




Parameters

DISTRIBU          : a keyword to denote the start of the block of distributed loads

dof               : a freedom code to define the direction of the loading if required (Character)

type              : a load pattern (Characters)

value             : list of values of force, force/unit length or distance, up to six values may be required depending
                     on the load pattern, (Real)

phase             : phase angle of the load in degrees (Real)

node              : node list defining the loaded element or loaded edge (Integer, 1-999999)

END               : keyword denoting the end of distributed loads

Notes


1.      See ASAS User Manual, Section 5.4.5 for full details of the load pattern types and their corresponding
        values.

2.      The load definition data may be placed in blocks and use made of the RP and RRP facilities to generate
        lists of nodes which define elements

Example


In this example a varying distributed load is applied on two curved beam elements in the local y direction with a
phase angle of 15 degrees. The elements are defined by node numbers 11, 12, 13, and 14, 15, 16.

        DISTRIBU
        /
        Y CB1 -6.6            -3.3       -9.9       15.0        11     12      13
        RP 2         3
        END


2.5.3.3. Pressure Loads

This data block defines the pressure loads for a loadcase.



 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-18
      RESPONSE User Manual                                                                               Data Formats


                PRESSURE
                 LDIR              (dir)

                 U                press           phase              //node//

                 FIN

                 F                phase               //node//

                 FIN

                 P                press                 //node//

                 FIN

                 END




Parameters

PRESSURE : keyword to denote the start of a block of pressure loads

LDIR              : keyword to defined direction of pressure load



dir               : load direction. Optional. Valid names are:
                     GX      global X direction
                     GY      global Y direction
                     GZ      global Z direction
                     X       local X direction
                     Y       local Y direction
                     Z     local Z direction
                     Default direction is assumed if dir is omitted.

END               : keyword denoting the end of the pressure loads

Notes


1.      Within RESPONSE there are two types of pressure loading

                     -            uniform pressure
                     -            varying pressure

        To define these pressures three types of data are required.

                     -            Uniform pressure data
                     -            Face data
                     -            Nodal Pressure data

 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-19
       RESPONSE User Manual                                                                                 Data Formats


          Each type of data is placed in blocks, with the keyword FIN denoting the end of the block and with END
          denoting the end of the entire PRESSURE data for the loadcase.


2.        Load pressure load direction is only permitted for shell elements.


2.5.3.3.1.                  Uniform Pressure

This block of data defines uniform pressure loading.

              U                 press           phase               //node//

              FIN




Parameters

U               : keyword defining that the data following is uniform pressure on an element face

press             : the value of the uniform face pressure. See Appendix A of the ASAS manual for the sign
                   convention for each element type (Real)

phase           : phase angle of uniform pressure, degrees (Real)

node            : list of node numbers defining a face, see note 2. below (Integer, 1-999999)

FIN             : keyword denoting the end of a block of uniform pressure data. If this is the last pressure data
                   required for the current loadcase END may be used instead of FIN

Notes


1.        The uniform pressure definitions may be grouped in blocks and use made of the RP and RRP facilities to
          generate lists of faces.

2.        The loaded face of a panel or of a brick element is defined by any 3 corner nodes on the face. For TRX6,
          THX6, QUX8 and QHX8 elements a face is defined by the 3 nodes forming the loaded edge. For TRX3,
          THX3, QUX4, and QHX4 elements a face is defined by the two nodes forming the loaded edge and any
          other node on the element. ASH2 or AHH2 elements are defined by their 2 nodes.


2.5.3.3.2.                  Non-uniform Pressure Loads

Two data types are required to define non-uniform pressure, one to define the face and one to define the values
of pressure at each node on the face.

This block defines a group of faces subjected to non-uniform pressure loading.


    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-20
       RESPONSE User Manual                                                                                 Data Formats



               F                phase                 //node//

               FIN



Parameters

F                  : keyword defining that the following data defines an element face

phase           : the phase of varying pressure, degrees (Real)

node            : list of node numbers defining a face (Integer, 1-999999)

FIN             : compulsory keyword denoting the end of a block of face data

Note


A number of faces may be defined using the RP and RRP facilities to generate sets of node numbers.


This block defines the pressure at nodes on the faces defined in the previous face data block.

               P                press                //node//

               FIN



Parameters

P               : keyword defining that the following data define nodal pressure values.

press           : the value of pressure at the defined nodes. See Appendix A of the ASAS manual for the sign
                    convention for each element type (Real)

node            : list of the node numbers to which pressure is applied (Integer, 1-999999)

FIN             : keyword denoting the end of a block of nodal pressure data. If this is the last pressure data
                    required for the current loadcase END may be used instead of FIN

Note


The pressure definitions may be placed in blocks and use made of the RP and RRP facilities to generate lists of
node numbers.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-21
    RESPONSE User Manual                                                                                                     Data Formats



Examples


1. Uniform Pressure

This example defines a uniform pressure of 10.0 and phase of 0.0 degrees on a face with three corner nodes of
10 20 30

                      PRESSURE
                      U     10.0             0.0       10        20       30
                      END

2. Non-uniform Pressure

This example has defined the element shown in the diagram as a face. A linear varying pressure at a phase of
10.0 degrees is applied to the face. The pressure varies from 20.0 on edge 1, 8, 7 to 0.0 on edge 3, 4, 5.
                                                                      7              6             5
                  PRESSURE
                      F   10.0               1     3        7
                      FIN                                                         8                                          4
                      P     20.0             1     8        7
                      P     0.0              3     4        5                                                            3
                                                                                       1                 2
                      END

3. Uniform and Non-uniform Pressure

This example shows the data required to produce the following pressure diagram on the given structure.
          p = 20                                                                      15
                                  20


                                                            10                        10
                                                                                                                                    5



                 13                      14                      15                    16                        17                    18
                      FACE 2                     FACE 4                  FACE 6             FACE 8                    FACE 10

                 7                       8                           9                 10                        11                 12


                      FACE 1                     FACE 3                  FACE 5             FACE 7                    FACE 9




             1                       2                           3                 4                         5                     6




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                           Page 2-22
     RESPONSE User Manual                                                                                             Data Formats


                    PRESSURE                                                           start of pressure loading
                    /
                    U     20.0        0.0       1       2   8                          defines uniform pressure
                    U     10.0        0.0       3       4   10                         on faces 1, 2, 5, 6, 9, 10
                    U       5.0       0.0       5       6   12
                    RP      2     6
                    FIN                                                                end of uniform pressure data
                    /
                    F       0.0       2     3       9                                  defines faces 3 and 4
                    RP      2     6
                    FIN                                                                end of face definition
                    /
                    P     20.0        2                                                defines varying pressure
                    P     10.0        3                                                on faces 3 and 4
                    RP      3     6
                    FIN                                                                end of nodal pressure data
                    F       0.0       4    5     1                                     defines faces 7 and 8
                    F       0.0 10 11 17
                    FIN                                                                end of face definition
                    P     10.0        4    10        16                                defines varying pressure
                    P     15.0        5    11       17                                 on faces 7 and 8
                    END                                                                end of pressure loading data


2.6. Seismic Response Data

For Seismic Response analysis three types of data are valid.

1.     Damping data. This may be specified by means of either a DAMP data block or a LOSS data block.

       A DAMP data block is used to define the damping for each mode and each loadcase as a percentage of
       the critical damping.

       A LOSS data block is used to define the damping on a material/group/element basis. The damping for
       each mode will then be calculated by the program as described in Section 1.1.


2.     Response spectrum data. This is specified by means of a SPEC data block.

3.     Seismic combination data. This is specified by means of a QUAK data blocks and is used to define
       which statistical combination method is to be used to combine the individual mode shapes to form a total
       loadcase.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 2-23
       RESPONSE User Manual                                                                                                 Data Formats


2.6.1.          UNITS for Seismic Data

In the Seismic Response Data, the UNITS command is applicable to the following data blocks

                            SPEC


The units of length may be modified by the user for the input of the spectral ordinates in the spectral definition.

The following data blocks do not permit the use of the UNITS command

                            DAMP
                            LOSS
                            QUAK

Example


                                                                    Operational Units                       Notes


SPEC 2                                                              KN,m,radians                            Global Definition
*                                                                                                           (default)
VELO        2
AXIS
SDAM        3     2.0       5.0      10.0
5.0         0.65          0.3        0.2
2.5         1.21          0.58       0.375
1.25        1.18          0.7        0.5
UNITS           MM                                                  mm                                      Change length
*                                                                                                           unit to mm
1.0             1150.0 740.0 530.0
0.8333 1100.0 760.0 550.0
END




2.6.2.          Damping Data for Seismic Response

Damping data may be defined in one of two forms. Firstly the damping may be defined as a single value for
each mode or each loadcase. Secondly the damping may be defined with respect to each material type, element
group or element.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                    Page 2-24
    RESPONSE User Manual                                                                                 Data Formats


2.6.2.1. Damping Data

The DAMP data specifies the damping as a percentage of critical damping for each mode and for each loadcase.


             DAMP

             scase             fcase              smode                fmode             damp

             END




Parameters

DAMP         : Compulsory header to define the start of the damping data. Must appear alone on the line

scase        : starting loadcase number (Integer 1-9999)

fcase        : finishing loadcase number (Integer 1-9999)

smode        : starting mode number (Integer)

fmode        : finishing mode number (Integer)

damp         : percentage of critical damping associated with the given modes and loadcases (Real)

END          : compulsory word to define the end of the damping data, and must appear alone on the line

Note


The user may include as many lines of data as necessary between DAMP and END to fully define the damping
conditions for the analysis

Example


This example defines a value of critical damping of 5% for modes 1 to 2, for loadcase 1 and 2% for mode 1,
30% for mode 2, for loadcase 2

        DAMP
        1      1      1       2      5.0
        2      2      1       1      2.0
        2   2         2       2      3.0
        END




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-25
     RESPONSE User Manual                                                                                Data Formats


2.6.2.2. LOSS Data

The LOSS data specifies the damping as a percentage of critical damping for each material, element group or
element. The overall value of damping is then calculated as described in Section 1.1.
              LOSS


              MATP               matno            damp


              GROU               grpno            damp


              ELEM               elno             damp

              END



Parameters

LOSS         : compulsory header to define the start of the LOSS data.

MATP         : keyword to denote that damping is defined for a material type

matno        : material number to which the damping value is to be applied (Integer)

GROU         : keyword to denote that damping is defined for an element group number

grpno        : group number to which the damping value is to be applied (Integer)

ELEM         : keyword to denote that damping is defined for an element

elno         : user element number to which the damping value is to be applied (Integer)

damp         : percentage of critical damping associated with this material, group or element (Real)

END          : compulsory keyword to define the end of the LOSS data.

Notes


1.      The data within the LOSS data block may be ordered in any arbitrary sense but the hierarchy is as
        follows.
                Element definition takes precedence over the group definition and group definition
                takes precedence over the material definition.


2.      Note that if spectral damping curves are defined they should bracket the minimum and maximum
        damping values so that a correct interpolation may be carried out.

 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-26
        RESPONSE User Manual                                                                              Data Formats


Example

         LOSS
         MATP        1       4.0
         GROU        1       2.0
         ELEM        3       1.0
         ELEM        4       1.0
         END



2.6.3.       Response Spectrum Data

This data block is used to define the response spectra for each direction for each loadcase and for up to 6 values
of critical damping. Each spectrum definition block comprises 4 types of data.




The types of data blocks are:

(i)      ordinate type definition data                                (DISP, VELO, ACCL)

(ii)     axis definition and interpolation method                     (AXIS)

(iii)    spectrum damping data                                        (SDAM)

(iv)     spectrum definition data lines as necessary



  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-27
    RESPONSE User Manual                                                                                 Data Formats


Each response spectrum definition is completed with a FIN unless it is the last spectrum set in which case END
must be used without FIN.

SPEC, FIN and END are compulsory key words and these words must appear alone on a line.


2.6.3.1. Ordinate Definition

This data line defines the type of ordinate axis used to define the spectrum. The ordinates may be defined in
terms of displacement, velocity or acceleration.

           DISP
           VELO                 nspec         (dura)
            ACCL




Parameters

DISP          : keyword to define that the ordinate axis of the spectrum is displacement

VELO         : keyword to define that the ordinate axis of the spectrum is velocity

ACCL         : keyword to define that the ordinate axis of the spectrum is acceleration

nspec        : defines the spectrum number (Integer)

dura         : defines the earthquake duration in seconds. This value is only required for the Double Sum
                method (DSUM), with a default of 15 seconds. (Real)

Example


This example specifies velocity is used for the ordinate axis for the first spectrum.

       VELO 1


2.6.3.2. Axis Definition and Interpolation Command

This data line defines the type of axes for the spectrum definition, linear or logarithmic.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-28
        RESPONSE User Manual                                                                              Data Formats


Parameters

AXIS :       compulsory key word

LIN :        defines a linear interpolation

LOG :        defines a logarithmic interpolation axis

FREQ : defines that frequency is used for the abscissa axis (Hz)

PERI :       defines that period is used for the abscissa axis (Seconds)

Note


The order of the terms on each line after the keyword is to define:

(i)      the abscissa interpolation             - default is linear

(ii)     the ordinate interpolation             - default is linear

(iii)    the abscissa type                      - default is frequency


If the user wishes to change any of the defaults, all three must be redefined.

Example


1. Default parameters

For this example the user has chosen to use the program default types.

         AXIS

2. User selected parameters

In this example the user has defined the abscissa axis as logarithmic interpolation. Since the abscissa has been
redefined, the user must also define the ordinate and the abscissa type even though they correspond to the
program default types.

         AXIS        LOG         LIN        FREQ


2.6.3.3. Spectrum Damping Command

These data lines define the number of spectral curves, and the value of the critical damping for each curve.


           SDAM                ndamp                         damp




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-29
      RESPONSE User Manual                                                                                Data Formats


Parameters

SDAM          : compulsory key word

ndamp         : defines the number of curves in the spectrum, maximum of 6 (Integer)

damp          : defines the values of damping as a percentage of critical damping for each curve. (Real)

Example


This example defines that curves for three values of critical damping will be defined, ie 2.0%, 5.0% and 10.0%.

        SDAM         3       2.0        5.0        10.0


2.6.3.4. Spectrum Definition




                     absc                      ordn



These data lines define the ordinate values of the spectrum curves


Parameters

absc          : abscissa value, frequency (Hz) or period (seconds) depending on the AXIS data. (Real)

ord           : ordinate values, one for each value of critical damping. (Real)

Notes


1.      For the natural frequencies and damping values used in the analysis, the spectral values are obtained by
        interpolation. The type of interpolation is defined by the AXIS data. The spectral curves for each value
        of damping are assumed to be composed of straight-line segments in the specified linear or logarithmic
        field.

2.      Interpolation for intermediate frequencies or periods will result in different spectral values if the abscissa
        type is PERIOD rather than FREQUENCY, since one is the reciprocal of the other.

3.      Interpolation between damping values is always linear.

Example


This data line defines three coordinates, one on each of three damping curves, these coordinates are (5.0, 0.65),
(5.0, 0.3) and (5.0, 0.2).



  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-30
   RESPONSE User Manual                                                                                 Data Formats


           5.0        0.65         0.3        0.2




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-31
    RESPONSE User Manual                                                                                                 Data Formats


EXAMPLE of a complete Response Spectrum

This example defines the first response spectrum in terms of velocity. Curves for six values of critical damping
are defined and each curve is specified by 15 values of frequency and velocity. This example is illustrated in the
diagram below.

       SPEC                                                            compulsory key word
       VELO       1                                                    defines ordinate axis type
       AXIS       LIN       LIN      FREQ                              defines interpolation method and abscissa type
       SDAM 6 0.0                   2.0           5.0           10.0          20.0          40.0         defines the values of
       5.0           0.65           0.3           0.2             0.175         0.125         0.11       critical damping
       2.5           1.21           0.58          0.375           0.28          0.2           0.18
       1.6667 1.255                 0.65          0.45            0.33          0.25          0.205
       1.25   1.18                  0.7           0.5             0.36          0.275         0.215
       1.0    1.15                  0.74          0.53            0.375  0.285                0.225
       0.8333 1.1                   0.76          0.55            0.3925 0.925                0.24         defines the
       0.7143 1.05                  0.77          0.56            0.41          0.305         0.245        coordinates of the
       0.625  1.02                  0.78          0.58            0.4275 0.315                0.25         spectra curves
       0.5556 1.0                   0.79          0.6             0.445  0.325                0.255
       0.5    1.0                   0.8           0.61            0.4625 0.335                0.26
       0.4545 1.0                   0.81          0.625           0.48   0.345                0.265
       0.4167 1.0                   0.82          0.64            0.4975 0.355                0.27
       0.3846 1.0                   0.83          0.665           0.515  0.365                0.275
       0.3571 1.0                   0.84          0.68            0.5325 0.375                0.28
       0.3333 1.0                   0.85          0.695           0.55          0.385         0.285
       END                                                                                                 compulsory keyword




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                      Page 2-32
       RESPONSE User Manual                                                                                          Data Formats


2.6.4.      Seismic Combination Data


 1.2

                                                                                                         % damping
 1.0                                                                                                                  0



 0.8                                                                                                                  2


                                                                                                                      5
 0.6

                                                                                                                      10
 0.4

                                                                                                                      20

 0.2                                                                                                                  40




                       2.0              1.0               0.67              0.5               0.4          0.33


These data lines are used to define which statistical combination method is to be used to combine a number of
modes together to give nodal displacements, velocities and accelerations and element stresses for the given
earthquake.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                Page 2-33
       RESPONSE User Manual                                                                               Data Formats




These data lines consist of 2 parts

(i)     motion definition data

(ii)    loadcase combination data


Each set is completed with a FIN command or if the last set an END command is used

QUAK and END are both compulsory key words. These words must appear alone on the line.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-34
    RESPONSE User Manual                                                                                 Data Formats


2.6.4.1. The Output Motion Data

These data lines define what types of output are required. Optional, with displacement motion as default.

                        DISP
                         VELO
                         ACCL
                         ALL




Parameters

DISP         : displacement

VELO         : velocity

ACCL         : acceleration

ALL          : all three types, ie displacement, velocity and acceleration.

Example


This line defines that velocity and acceleration are required as output.

       VELO         ACCL




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-35
    RESPONSE User Manual                                                                                 Data Formats


2.6.4.2. Loadcase Combination Data

These data define which statistical combination method is to be used to combine the modes and obtain the
seismic response.




Parameters

A number of statistical combination methods are available to combine the responses for each mode.

SRSS         : Square root of the sum of the squares

ABSS         : Absolute sum

ASRS         : Maximum absolute value plus the SRSS of the remaining

CQCM         : The complete quadratic combination method

TENP         : The ten percent method

DSUM         : The double sum method


 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-36
       RESPONSE User Manual                                                                                 Data Formats


ALGB            : Simple algebraic sum

SNGL            : Single mode combination method

CQAL            : CQCM combination for modes 1 to nmode2
                   ALGB combination for modes nmode2+1 to nmode

P               : Spatial combination prior to modal combination

A               : Spatial combination after modal combination

case            : Loadcase number (Integer, 1-9999)

nmode           : Number of modes to be combined (Integer)

major           : Defines the major mode number in the ASRS combination, omitted if any other combination. If
                   zero the maximum absolute value is chosen. (Integer)

nmode2          : For CQAL, limit of CQCM combination (ie for nmode2+1 to nmode algebraic combination is
                   used)

gxx             : Multiplying factor in x-direction due to x earthquake

gxy             : Multiplying factor in x-direction due to y earthquake
                  ...
                  ...

gzz             : Multiplying factor in z-direction due to z earthquake

sxx             : Spectrum number corresponding to gxx
                  ...
                  ...

szz             : Spectrum number corresponding to gzz


A number of statistical combination methods are available to combine the responses for the x, y, z, directions.

SRSS            : Square root of the sum of the squares

ABSS            : Absolute sum method

NRLS            : Maximum absolute value plus the root mean square of the remaining

MAXP            : Maximum plus 30% of the others

MAXF            : Maximum plus 40% of the others

SNGX            : No combination just take the x-direction (single mode only)




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-37
    RESPONSE User Manual                                                                                 Data Formats


SNGY         : No combination just take the y-direction (single mode only)

SNGZ         : No combination just take the z-direction (single mode only)

mode         : List of single mode numbers (Integer)




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-38
     RESPONSE User Manual                                                                                       Data Formats


If the user requires factors different for each mode, this is achieved by setting all the G factors in the
combination line to zero, then by using continuation lines the values for each mode or groups of modes are
defined. The continuation line has the form.

        smode                     fmode            gx          gy                            gz




The above line of data is repeated until all the modes are assigned with factors (by using the starting and
finishing numbers overlapping can be carried out).

Notes


1.      A list of single mode numbers may be generated using the RP facility.

2.      Each mode given in the single combination deck must be allocated a unique loadcase number. The
        loadcase number given on the deck is incremented by one automatically for each mode defined.

Examples


This example asks for a single combination of modes 1,2,3,4, and allocates each mode to four loadcases ie
loadcase 1,2,3,4.

        /
        SNGL          P       1        1.0    1.0       1.0   1     1           1           SNGX       1    2
        RP        2       2

This example defines different G-factors for modes 1 to 5 and modes 6 to 10.

        SRSS              P       1     10    0.0       0.0   0.0           1           1        1   SRSS
        1     5       1.0             1.0    1.0
        6     10 2.0                  2.0    2.0

This example shows the data required to carry out the two previous examples, but the first one requiring
displacement motion, and the second acceleration.

        QUAK
        DISP
        /
        SNGL P 1                       1.0    1.0       1.0    1    1           1           SNGX       1    2
        RP 2 2
        FIN
        ACCL
        SRSS          P       5        10    0.0    0.0       0.0       1           1        1       SRSS
        1     5           1.0          1.0    1.0
        6     10          2.0          2.0    2.0
        END


 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.           Page 2-39
       RESPONSE User Manual                                                                                               Data Formats


2.7. Transient Response Data

For Transient Response analysis five data blocks are valid:

1.        Damping data. This may be specified by means of either a DAMP data block or a LOSS data block.

          A DAMP data block is used to define the damping for each mode as a percentage of the critical damping.

          A LOSS data block is used to define the damping on a material/group/element bases. The damping for
          each mode will then be calculated by the program as described in Section 1.1.


2.        Transient function data This is defined by means of a TFUN data block. Transient functions are
          defined for subsequent use in loading histories and seismic histories.

3.        Initial conditions data This is defined by means of an INIT data block. The initial conditions of the
          structure are defined prior to carrying out a time history analysis.

4.        Loading data This is specified by means of a LOAD data block. The loading may be applied as transient
          nodal load or (for transient seismic) as transient applied acceleration to the support nodes.

5.        Results output data This is defined by means of a RESU data block. The type of results required and
          the times during the time history at which results are required are defined.




2.7.1.         UNITS for Transient Data

In the Transient Response Data, the UNITS command is applicable to the following data blocks

                            INIT
                            LOAD


The following data blocks do not permit the use of the UNITS command

                            DAMP
                            LOSS
                            TFUN
                            RESU

Example


                                                       Operational Units                                    Notes

LOAD 1                                                 KN,m,radians                                         Global Definition
*                                                                                                           (default)
TRAN 1
NODAL LO


    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                   Page 2-40
       RESPONSE User Manual                                                                                              Data Formats


UNITS N                                                N,m,radians                                          Force amplitude
*                                                                                                           in Newtons
X 1 15000.0               0.0      5
Y 1 12000.0               0.0      4
UNITS             MM                                   N,mm,radians                                         moments input in Nmm
*
RY 1        250.0         0.0      5
END
STOP




2.7.2.         Damping Data for Transient Response

Damping data may be defined in one of two forms. Firstly the damping may be defined as a single value for
each mode or each loadcase. Secondly the damping may be defined with respect to each material type, element
group or element.


2.7.2.1. Damping Data

The DAMP data specifies the damping as a percentage of critical damping for each mode.


                DAMP

                scase             fcase              smode                fmode             damp

                END




Parameters

DAMP            : Compulsory header to define the start of the damping data.

scase           : starting loadcase number (Integer, 1-9999)

fcase           : finishing loadcase number (Integer, 1-9999)

smode           : starting mode number (Integer)

fmode           : finishing mode number (Integer)

damp            : percentage of critical damping associated with the given modes and loadcases (Real)

END             : compulsory word to define the end of the damping data.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page 2-41
     RESPONSE User Manual                                                                                Data Formats


Notes


1.      The user may include as many lines of data as necessary between DAMP and END to fully define the
        damping conditions for the analysis

2.      At present only 1 transient loadcase is allowed per run. Therefore scase and fcase must both be set to
        1.

Example


This example defines a value of critical damping of 5% for mode 1, and 2% for mode 2, for loadcase 1

                    DAMP
                    1       1       1      1        5.0
                    1   1           2      2        2.0
                    END


2.7.2.2. Loss Data

The LOSS data specifies the damping as a percentage of critical damping for each material, element group or
element. The overall value of damping is then calculated as described in Section 1.1.
              LOSS


              MATP               matno            damp


              GROU               grpno            damp


              ELEM               elno             damp


              END




Parameters

LOSS         : compulsory header to define the start of the LOSS data

MATP         : keyword to denote that damping is defined for a material type

matno        : material number to which the damping value is to be applied (Integer)

GROU         : keyword to denote that damping is defined for an element group number

grpno        : group number to which the damping value is to be applied (Integer)


 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-42
    RESPONSE User Manual                                                                                 Data Formats


ELEM         : keyword to denote that damping is defined for an element

elno         : user element number to which the damping value is to be applied (Integer)

damp         : percentage of critical damping associated with this material, group or element (Real)

END          : compulsory keyword to define the end of the LOSS data.

Note


The data within the LOSS deck may be ordered in any arbitrary sense but the hierarchy is as follows.
                Element definition takes precedence over the group definition and group definition
                takes precedence over the material definition.

Example

         LOSS
         MATP       1       4.0
         GROU       1       2.0
         ELEM       3       1.0
         ELEM       4       1.0
         END



2.7.3.      Transient Function Data

This data block is used to define the time histories (transient functions) of the structural loading. Each transient
function definition block is comprised of 2 types of data




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-43
        RESPONSE User Manual                                                                              Data Formats


The types of data are:

(i)      a transient function header

(ii)     as many transient function definition data lines as required


Each transient function is completed with a FIN command or, if it is the last transient function, an END
command is used.

TFUN and END are compulsory keywords. These words must appear alone on a line.


2.7.3.1. Transient Function Header

This command defines the transient function number and title. It also it indicates how the function is to be
echoed back in the output file.




Parameters

tran          : transient function number (Integer, 1-9999)

PR            : keyword to define that the transient function is only to be printed (default)

PL            : keyword to define that the transient function is only to be plotted

PP            : keyword to define that the transient function is to be printed and plotted

title         : alphanumeric title for this transient function (up to 75 characters)

Notes


1.       For PR and PP the transient function will be echoed to the output file as a table of values.

2.       For PL and PP the transient function will be echoed to the output file as a simple graph of value verses
         time.

Example


This example defines the first transient function with title “EXAMPLE 1 of TRANSIENT ANALYSIS” and the
user wishes the transient function to be printed and plotted.



  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-44
       RESPONSE User Manual                                                                               Data Formats


        1     PP     EXAMPLE 1 OF TRANSIENT ANALYSIS


2.7.3.2. Transient Function Definition

This data block defines the time variation of the transient function or time history

               TIME                   time


               VALU                   v alu


               TIVA            time         v alu




Parameters

The transient function may be defined by one of two methods.

(i)     a list of times in increasing order defining the abscissae of the curve, followed by a list of corresponding
        values defining the ordinates of the curve (TIME and VALU).

(ii)    a list of coordinates pairs defining the curve (TIVA).

TIME          : denotes that a list of times is to follow

VALU          : denotes that a list of values is to follow

TIVA          : denotes that a list of pairs of time and value is to follow

time          : list of times, if continued onto the next line the key word is omitted (Real)

valu          : list of values, if continued onto the next line the key word is omitted (Real)

Notes


1.      Intermediate values are found by linear interpolation.

2.      All zero values must be defined, since there are no defaults.

3.      The list of times should cover the full range of time required by the results data (RESU, TIME) including
        any initial time offsets specified.

Examples


1.      This example defines the transient function as a straight line.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-45
     RESPONSE User Manual                                                                                Data Formats


         TIME         1.0     2.0      3.0       4.0
                      5.0     6.0      7.0       8.0
         VALU         0.1     0.2      0.3       0.4
                      0.5     0.6      0.7       0.8
         FIN

2.       This example defines the same straight line as above.

         TIVA         1.0     0.1      2.0       0.2      3.0       0.3      4.0      0.4
                      5.0     0.5      6.0       0.6      7.0       0.7      8.0      0.8
         FIN

3.       This example defines two transient functions. The first is the same as example 2 above. The second
         define a triangular pulse, starting at time=0.15 secs, reaching a peak at time=0.25 secs and decreasing to
         zero at time=0.5 secs. Before and after these times the value of the function is zero.

         TFUN
         1 PP         TRANSIENT FUNCTION ONE
         TIVA         1.0 0.1 2.0 0.2 3.0                           0.3
                      4.0     0.4      5.0       0.5      6.0       0.6
                      7.0     0.7      8.0       0.8
         FIN
         2 PP         TRANSIENT FUNCTION TWO
         TIME         0.0 0.15 0.25 0.5 8.0
         VALU         0.0     0.0        1.0        0.0       0.0
         END




2.7.4.      INITIAL Conditions

This data defines the initial motion of the structure at the start of the time history analysis. This data is optional
and, if omitted, all nodes are assumed to have zero initial displacement and velocity.
               INIT

               (skew )         dof         disp           v elo             //node//

               END



Parameters

INIT           : compulsory header to define the start of the initial condition data and must appear alone on the line

skew           : skew integer. This skew system must have been defined in the ASAS natural frequency analysis
                 (Integer, 1-9999)



 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-46
      RESPONSE User Manual                                                                               Data Formats


dof            : freedom code (Character)

disp           : an initial displacement (Real)

velo           : an initial velocity (Real)

node           : list of node numbers at which the initial condition applies. (Integer, 1-99999)

END            : compulsory word to define the end of the initial conditions. Must appear alone on the line

Note


The initial condition data lines may be placed in blocks and use made of the RP and RRP facilities to generate
lists of node numbers.

Example


This example gives the X freedom of nodes 1,2,3,4 an initial displacement of 0.0 and an initial velocity of 1.0.

         INIT
         /
         X 0.0 1.0              1    2
         RP 2 2
         END




2.7.5.       LOADING Data

This data block defines the transient response loading data. The general form of the loading data is shown
below.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-47
     RESPONSE User Manual                                                                                    Data Formats



               LOAD
               SEISMIC

               X

               Y         tran           factor           timoff

               Z

               END


               TRAN               ntype

               NODAL LO
               (nskew )        dof          tran            factor           timoff               //node//

               END




Parameters

LOAD         : compulsory keyword which is used to define the start of the transient load data.

SEISMIC : compulsory keyword denoting the start of a block of displacements

TRAN         : compulsory keyword denoting the start of a block of loads

END          : compulsory keyword denoting the end of a block

Notes


1.      At present transient analysis can only deal with one loadcase.

2.      Two types of loading are available but only one type of loading, SEISMIC or NODAL, can be present in
        any one run of the program

        Prescribed transient accelerations (SEISMIC load)

        Transient nodal loads (NODAL LOad)



2.7.5.1. SEISMIC Load

This data defines the prescribed transient accelerations to be applied at ALL the support nodes.




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page 2-48
       RESPONSE User Manual                                                                                 Data Formats



                SEISMIC

                X

                Y          tran       factor         timoff

                Z

                 END



Parameters

SEISMIC : is a compulsory word denoting the start of a block of displacements

X               : Freedom code for prescribed accelerations in the X direction

Y               : Freedom code for prescribed accelerations in the Y direction

Z               : Freedom code for prescribed accelerations in the Z direction

tran            : the transient function number (Integer)

factor          : multiplying factor for the transient function (Real)

timoff          : offset times ie the starting time of the transient function (Real)

END             : is a compulsory word denoting the end of a block

Note


If offset times are defined, remember there are no zero defaults, that is the first point defined before the offset is
applied should be zero.

Example


This example defines a prescribed acceleration at all the support nodes with a factor of 1.0 and in the X
direction. The history of the acceleration follows transient function 1.

          SEISMIC
          X     1    1.0       0.0
          END

This example defines a prescribed acceleration at all the support nodes with a factor of 1.0 in the X-direction and
0.4 in the Z-direction. The X accelerations vary according to transient function 1 and the Z accelerations
according to transient function 2.




    Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-49
      RESPONSE User Manual                                                                               Data Formats


         SEISMIC
         X   1    1.0       0.0
         Z 2      0.4       0.0
         END


2.7.5.2. NODAL Load

This data defines the nodal loads for a transient analysis.




Parameters

TRAN                  : is a compulsory word denoting the start of a block of loads

ntype                 : number of different load types (at present ntype will always equal 1)

NODAL LO              : is a compulsory word denoting that what follows is nodal loads.

skew                  : skew integer as defined in the ASAS dynamic analysis (Integer)

dof                   : a freedom code (Character)

tran                  : the transient function number (Integer)

factor                : multiplier for the transient function (Real)

timoff                : offset time ie the starting time of the transient function (Real)

node                  : list of node numbers at which the load is applied (Integer)

Notes


1.       The load definitions may be placed in blocks and use made of the RP and RRP facilities to generate a list
         of node numbers.

2.       If offset times are defined, remember there are no zero defaults, that is the first point defined before the
         offset is applied should be zero.



 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-50
    RESPONSE User Manual                                                                                 Data Formats


Example


This example defines a nodal load applied at the X freedom of nodes 1, 2, 10 with a factor of 1.0 and the history
of the force follows transient function 1.

                    TRAN        1
                    NODAL LO
                    X 1 1.0              0.0       1    2     10
                    END




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-51
    RESPONSE User Manual                                                                                 Data Formats


This example defines that the nodal loads of the previous example are applied in sequence at 2 seconds intervals

                    TRAN        1
                    NODAL           LO
                    X     1     1.0      0.0       1
                    X     1     1.0      2.0       2
                    X 1         1.0      4.0       10
                    END




2.7.6.      RESULTS Output

This data block defines the times at which the results from the time history analysis are to be output. This
selection is available for stresses on elements and groups of elements, and for nodal displacement, velocity and
accelerations. The general form of the results data block is shown below.




Parameters

RESU         : is a compulsory word denoting that what follows is the output selection. Must appear alone on a
                line

END          : is a compulsory word denoting the end of the result deck. Must appear alone on a line




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-52
    RESPONSE User Manual                                                                                 Data Formats


2.7.6.1. OUTPUT Times

This data defines the list of times at which the output of results are required.

          TIME                 time




Parameters

TIME         : denotes that a list of times follows at which results are required.

time         : list of times, if continued onto the next line the key word is omitted. (Real)

Example


        TIME      0.1       0.2       0.3      0.5      0.75       1.0
                  1.5       2.0       2.5      3.0      4.0        5.0


2.7.6.2. Selecting Stress Output

The maximum stresses on elements may be printed by defining a list of user element numbers or a list of element
group numbers
         ELEM                       elem


         GROU                      group




Parameters

ELEM         : denotes that a list of elements is to follow for which stresses are required to be printed.

elem         : list of user element numbers, if continued onto the next line the key word is omitted. (Integer, 1-
                999999)

GROU         : denotes that a list of group numbers, as defined in the ASAS analysis, is to follow for which
                stresses are required to be printed for each element in each group.

group        : list of group numbers, if continued onto the next line the key word is omitted. (Integer, 1-9999)

Note


Only the maximum value is printed of each stress or force on an element, calculated from the selected output
times. A complete stress history of stresses is not printed.

 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 2-53
      RESPONSE User Manual                                                                               Data Formats


Example


This example defines that the maximum stresses in elements 1, 2, 3 and all the elements in group 2 are to be
printed.

                    RESU
                    ELEM        1        2         3
                    GROU        2


2.7.6.3. Selecting Nodal Output

This data block defines the displacement, velocity or acceleration output required for a selected nodes and
freedoms. These results may be printed or plotted in the output file.




Parameters

NODE         : keyword to denote that selective nodal output is required

PR           : keyword to print the relevant output histories only (default)

PL           : keyword to plot the relevant output histories only

PP           : print and plot the relevant output histories

DISP         : keyword to request output of displacements (default)

VELO         : keyword to request output of velocities

ACCL         : keyword to request output of accelerations

ALL          : keyword to request output of displacements, velocities and accelerations

dof          : list of freedom codes for which results are required (Character)

ALL          : output results for all the freedoms at the given nodes (default)

node         : list of nodes at which the results are required (Integer)



 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-54
     RESPONSE User Manual                                                                                Data Formats


Note


The displacements, velocities and accelerations printed for seismic transient analysis are relative motions. If
absolute acceleration are required, the ABSO option must be used.

Examples


1.     This example defines that selective output is required in the X direction at nodes 1, 2, 3, 4. The
       displacement output is to be printed and plotted whereas the velocity output is only to be plotted.

                    RESU
                    TIME         1.0 2.0 3.0
                    NODE        PP DISP X 1                   2     3       4
                    NODE        PL      VELO       X    1     2     3       4
                    END

2.     This example defines that displacement and velocity output is required for freedoms X, Y, Z, RX, RY at
       nodes 1, 2, 3.

                    RESU
                    TIME          1.0       2.0
                    NODE          PP       DISP         VELO              X Y Z RX RY 1 2 3
                    END

3.     The following two examples show the use of defaults in the data for selective nodal output

                    NODE          1 2 3

       is equivalent to

                    NODE          PR       DISP         ALL           1        2       3

       and

                    NODE          ALL        1     2    3

       is equivalent to

                    NODE          PR       ALL         ALL        1        2       3


2.8. LOADFILE Analysis Data

In this analysis two types of data are valid:

1.     Damping data: This may be specified by means of a DAMP data block or a LOSS data block.

       A DAMP data block is used to define the damping for each mode and each loadcase as a percentage of
       the initial damping.


 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-55
     RESPONSE User Manual                                                                                Data Formats


         A LOSS data block is used to define the damping on a material/group/element basis. The damping for
         each mode will then be calculated by the program as described in Section 1.1.


2.       Loadcase selection data: This is specified by means of a SELE data block. This allows the user to
         select which loadcases are to be processed. The loadcases are selected from those in the data file created
         by WAVE for the structure defined on the LOADFILE data line.




2.8.1.      UNITS for LOADFILE Data

The UNITS command is not valid in the LOADFILE data.




2.8.2.      Damping Data for LOADFILE Analysis

Damping data may be defined in one of two forms. Firstly the damping may be defined as a single value for
each mode or each loadcase. Secondly the damping may be defined with respect to each material type, element
group or element.


2.8.2.1. Damping data block

The DAMP data specifies the damping as a percentage of critical damping for each mode and for each loadcase.
             DAMP

              scase            fcase              smode              fmode                damp

              END



Parameters

DAMP         : Compulsory header to define the start of the damping data. Must appear alone on the line

scase        : starting loadcase number (Integer, 1-9999)

fcase        : finishing loadcase number (Integer, 1-9999)

smode        : starting mode number (Integer)

fmode        : finishing mode number (Integer)

damp         : percentage of critical damping associated with the given modes and loadcases (Real)

END          : compulsory word to define the end of the damping data. Must appear alone on the line


 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-56
    RESPONSE User Manual                                                                                 Data Formats


Note


The user may include as many lines of data as necessary between DAMP and END to fully define the damping
conditions for the analysis

Example


This example defines a value of critical damping of 5% for mode 1, and 2% for mode 2, for all 25 loadcases

                    DAMP
                    1       25       1       1       5.0
                    1   25           2       2       2.0
                    END


2.8.2.2. Loss Data

The LOSS data specifies the damping as a percentage of critical damping for each material, element group or
element. The overall value of damping is then calculated as described in Section 1.1.
               LOSS


               MATP               matno            damp


               GROU               grpno            damp


               ELEM               elno             damp


               END




Parameters

LOSS         : compulsory header to define the start of the LOSS data

MATP         : keyword to denote that damping is defined for a material type

matno        : material number to which the damping value is to be applied (Integer)

GROU         : keyword to denote that damping is defined for an element group number

grpno        : group number to which the damping value damp is to be applied (Integer)

ELEM         : keyword to denote that damping is defined for an element




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-57
    RESPONSE User Manual                                                                                 Data Formats


elno         : user element number to which the damping value is to be applied (Integer)

damp         : percentage of critical damping associated with this material, group or element (Real)

END          : compulsory keyword to define the end of the LOSS data.

Note


The data within the LOSS deck may be ordered in any arbitrary sense but the hierarchy is as follows.
                Element definition takes precedence over the group definition and group definition
                takes precedence over the material definition.

Example

         LOSS
         MATP       1       4.0
         GROU       1       2.0
         ELEM       3       1.0
         ELEM       4       1.0
         END



2.8.3.      Loadcase Selection

These data define which base wave cases (real and imaginary parts) from the WAVE run are loadcases for the


                SELE

                 case

                 END

steady state analysis. The data are optional, and if not used all the WAVE cases are used.


Parameters

SELE         : compulsory keyword to define the start of the wave case selection data.

case         : list of wave loadcase numbers required for this analysis

END          : compulsory word to define the end of the selection data.

Example


This example defines that the base wavecases 1, 2, 10, 20, 30 from WAVE will be used in the steady state
analysis.


 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-58
     RESPONSE User Manual                                                                                 Data Formats


         SELE
         1     2   10
         20 30
         END


2.9. STRESS Analysis Data

In this type of analysis stresses are calculated corresponding to each normalised mode shape. No additional data
is required.

Notes


1.       If stress contour plots or bending moment diagrams are required a SAVE LOCO FILES command is
         required. POST and BEAMST may then be run to create the required files for the selected plotting
         program.

2.       The NEWSTRUCTURE command must not be specified in the Preliminary Data.

Example


         SOLUTION STRESS
         STOP




2.9.1.       STOP

This line of data is used to signify the end of the data for this RESPONSE analysis and must appear as the last
line of data.

         STOP




Parameters

STOP               : compulsory word




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-59
   RESPONSE User Manual                                                                                 Data Formats




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page 2-60
     RESPONSE User Manual                                                                                   Examples




3.      Examples
Five complete examples are given in this Section with notes describing each analysis type.


3.1. Steady State Analysis

        SYSTEM DATA AREA 90000
        PROJECT GD07
        JOB RESP
        FILES R7DF
        TITLE EXAMPLE ONE STEADY STATE ANALYSIS
        STRUCTURE GD07
        NEWSTRUCTURE R7DF
        OPTIONS GOON
        END                            Denotes the end of the preliminary data
        SOLUTION STEADY STATE          Denotes what follows is data for a steady state analysis
        DAMP
        1 1 1 24 2.0
        2 3 1 24 9.0                   Damping data
        4 4 1 24 1.0
        END
        LOAD 4                         Denotes that four loadcases, to be analysed
        HARM 1 1 1.0                   Denotes that only one load type used for this loadcase
        NODAL LOAD
        Z 20.0 15.0 13
        /                              Defines nodal loads
        Z 15.0 15.0 1
        RP 3 2
        END
        HARM 2 1 1.0                   Denotes that only one load type used for this loadcase
        PRESSURE
        /
        U -50.0 15.0 1 11 3            Defines pressure loads
        U -50.0 15.0 3 11 13
        RP 2 2
        END
        HARM 3 1 1.0                   Denotes that only one load type used for this loadcase
        PRESSURE
        /
        F 15.0 1 3 11                  Varying pressure-face definitions
        RP 2 2
        FIN
        /
        P 10.0 1
        P 20.0 11                      Varying pressure-pressure definitions
        RP 3 2
        END
        HARM 4 1 1.0                   Denotes that only one load type used for this loadcase
        DISTRIBU
        /
        Y CB1 -6.6 3.3 -9.9 15.0 11 12 13                   Defines distributed loads




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 3-1
   RESPONSE User Manual                                                                                                    Examples


       RP 2         2
       END
       STOP                                                                                Denotes the end of data


3.2. Seismic Analysis

       SYSTEM DATA AREA 30000
       PROJECT TES1
       JOB RESP
       FILES RES1
       TITLE EXAMPLE TWO SEISMIC ANALYSIS
       STRUCTURE TES1
       NEWSTRUCTURE RES1
       OPTIONS GOON NOBL
       END                                                                Denotes the end of the preliminary data
       SOLUTION SEISMIC                                                   Denotes what follows is data for a seismic analysis
       DAMP
       1 9        1       7   5.0                                         Damping data
       END
       SPEC
       VELO 1                                                             Defines the ordinate axis is velocity
       AXIS                                                           Defines the axis scales are default values
       SDAM           3             2.0           5.0            10.0                       Defines the % of critical damping
                      5.0           0.3           0.2              0.175
                      2.5           0.58          0.375            0.25
                      1.25          0.7           0.5              0.35                             Defines the spectrum data
                      0.8353        0.78          0.55             0.3925
                      0.5556        0.79          0.6              0.445
                      0.4545        0.81          0.625            0.48
                      0.3846        0.83          0.665            0.515
       END
       QUAK
       ALL
       SRSS A           1     7   1.0      1.0      1.0      1     1     1    SRSS                  Defines   4   combinations   for
       which
       SNGL A           2         1.0      1.0      1.0      1     1     1    SRSS 1 2 5 disp., velo., and                accl., are
       required
       FIN
       DISP
       SRSS A           5     7   1.0      1.0      2.0      1     1     1    ABSS                  Defines 1 combination for which
       END                                                                                     disp. is required
       STOP                                                               Denotes the end of data




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                 Page 3-2
   RESPONSE User Manual                                                                                                      Examples


3.3. Transient Analysis

       SYSTEM DATA AREA 30000
       PROJECT GD07
       JOB RESP
       FILES R20B
       TITLE EXAMPLE THREE TRANSIENT ANALYSIS
       STRUCTURE GD07
       NEWSTRUCTURE R208
       OPTIONS GOON
       END                                                                Denotes the end of the preliminary data
       SOLUTION TRANSIENT                                                 Denotes what follows is data for a transient analysis
       DAMP
       1 1 1 24 2.0                                                       Damping data
       END
       TFUN
       1 PR SINUSOIDAL FUNCTION
       VALU      0.000      0.100      0.199       0.296      0.389      0.479       0.565      0.644     0.717    0.783     Defines
                 0.841      0.891      0.932       0.964      0.985      0.997       1.000      0.992     0.974    0.946     the
                 0.909      0.863      0.808       0.746      0.675      0.598       0.516      0.427     0.335    0.239     ordinates
                 0.141      0.042     -0.058     -0.158      -0.256     -0.351     -0.443      -0.530    -0.612   -0.688     of the time
               -0.757      -0.816     -0.872     -0.916      -0.952     -0.978     -0.994      -1.000    -0.996   -0.982     history
               -0.959      -0.926     -0.883     -0.832      -0.773     -0.706     -0.631      -0.551    -0.456   -0.374     curve
               -0.279      -0.182     -0.083



       TIME      0.000      0.100      0.200       0.300      0.400      0.500       0.600      0.700     0.800   0.900      Defines
                 1.000      1.100      1.200       1.300      1.400      1.500       1.600      1.700     1.800   1.900      the
                 2.000      2.100      2.200       2.300      2.400      2.500       2.600      2.700     2.800   2.900      abscissa of
                 3.000      3.100      3.200       3.300      3.400      3.500       3.600      3.700     3.800   3.900      the time
                 4.000      4.100      4.200       4.300      4.400      4.500       4.600      4.700     4.800   4.900      history
                 5.000      5.100      5.200       5.300      5.400      5.500       5.600      5.700     5.800   5.900      curve
                 6.000      6.100      6.200
       END
       INIT
       Z 0.0 59.89 7
       Z 0.0 92.83 8                                                      Defines the initial conditions
       Z 0.0 45.49 9
       END
       LOAD 1
       TRAN 1
       NODAL LOAD
       Z 1 0.0 0.0             13
       Z 1 0.0 0.0             1 3 5                                      Defines the nodal loads
       Z 1 0.0 0.0             12 14 16          18
       END
       RESU
       TIME      0.000      0.100      0.200       0.300      0.400      0.500       0.600      0.700     0.800   0.900      Defines
                 1.000      1.100      1.200       1.300      1.400      1.500       1.600      1.700     1.800   1.900      the
                 2.000      2.100      2.200       2.300      2.400      2.500       2.600      2.700     2.800   2.900      times at
                 3.000      3.100      3.200       3.300      3.400      3.500       3.600      3.700     3.800   3.900      which
                 4.000      4.100      4.200       4.300      4.400      4.500       4.600      4.700     4.800   4.900      the results
                 5.000      5.100      5.200       5.300      5.400      5.500       5.600      5.700     5.800   5.900      are
                 6.000      6.100      6.200                                                                                 required
       NODE PP DISP Z 7                                                   Results for node 7 freedom Z are required
       END
       STOP                                                               Denotes the end of data




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                     Page 3-3
       RESPONSE User Manual                                                                                                 Examples


   3.4. Loadfile Analysis

           SYSTEM DATA AREA 50000
           PROJECT FJ5W
           JOB RESP
           FILES FJ5R
           TITLE EXAMPLE FOUR LOADFILE ANALYSIS
           STRUCTURE FJ5A
           NEWSTRUCTURE FJ5Y
           OPTIONS NOBL
           SAVE LOCO FILES
           END                                                                Denotes the end of the Preliminary Data
           LOADFILE FJ5W                                                      Denotes what follows is data for a waveload
           DAMP                                                               steady state analysis
           1     4    1     8    4.0                                          Damping data, 4 loadcases
           END
           SELE
           1 2        3     4                                                 Defines which wave loadcases are to be analysed
           END
           STOP


   3.5. Stress Calculation Analysis

(i). RESPONSE Data


           SYSTEM DATA AREA 100000
           PROJECT TS02
           JOB RESP
           TITLE STRESSES FROM NORMALISED EIGENVECTORS
           STRUCTURE TS02
           OPTION NOBL GOON
           SAVE LOCO FILES                                           Denotes save files for POST analysis
           END
           SOLUTION STRESS                                           Calculates eigenvector stresses only
           STOP


(ii). POST Data (see POST User Manual)


           SYSTEM DATA AREA 30000
           PROJECT TS02
           JOB POST
           TITLE PROCESS STRESSES FROM NORMALISED EIGENVECTORS
           STRUCTURE TS02




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.              Page 3-4
       RESPONSE User Manual                                                                                    Examples


           OPTION NOBL GOON
           END
           SHELL
           END

(iii). BEAMST Data (see BEAMST User Manual)


           SYSTEM DATA AREA 100000
           PROJECT TS02
           JOB POST
           TITLE PROCESS FORCES AND MOMENTS FROM EIGENVECTORS
           STRUCTURE TS02
           OPTION NOBL GOON
           END
           POST
           CASE ALL
           ELEM ALL
           UNIT M KN
           PRIN ALL
           END
           STOP




     Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 3-5
  RESPONSE User Manual                                                                                    Examples




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 3-6
    RESPONSE User Manual                                                                                Appendix A




                              Appendix A                     - Preliminary Data for RESPONSE


A.1         Preliminary Data
The preliminary data is the first block of the RESPONSE information. It defines the size of the job and the
structure that will be processed during the course of the analysis.

                  SYSTEM                           DATA AREA                   memory


                  PROJECT                          pname


                  JOB                              RESP


                  FILES                            fname


                  TITLE                            title

                  TEXT                             text


                  STRUCTURE                        sname


                  NEWSTRUCTURE                     nsname

                  OPTIONS                          option

                  RESTART                          first                 last

                  SAVE                             set                   FILES
                  RESU

                  UNITS                            unitm

                  END




The preliminary data must commence with the SYSTEM command and terminate with END. Within these
bounds the other commands may be given in any order. It is suggested, however, that the order given above is
adopted.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-1
     RESPONSE User Manual                                                                                   Appendix A


A.2         SYSTEM Command
To define the amount of memory used for data by this run. Optional.


         SYSTEM                  DATA AREA                   memory




Parameters

SYSTEM            : keyword

DATA AREA            :        keyword

memory            : amount of memory (in integer words) to be used by this run. Typical values are between
                     30000 and 1000000. If the SYSTEM command is omitted, a default value of 1000000 is used.

Examples


        SYSTEM DATA AREA 80000



A.3         PROJECT Command
To define the project name for the current run. Optional.


         PROJECT                        pname




Parameters

PROJECT           : keyword

pname             : project name for current run. (Alphanumeric, 4 characters, first character must be alphabetic)

Note


1.     All runs with the same project name access the same data base. A project data base consists of one
       project file (with a file name consisting of the 4 characters of pname with the number 10 appended)
       which acts as an index to other files created under this project, together with those other files.

Example


       PROJECT HIJK




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page A-2
     RESPONSE User Manual                                                                               Appendix A


A.4         JOB Command
To define the type of analysis for the current run. Compulsory



         JOB                     RESP




Parameters

JOB               : keyword

RESP              : keyword

Example


        JOB        POST         FRED         BILL



A.5         FILES Command
To define the prefix name for the backing files created in this run. Optional.


         FILES               fname




Parameters

FILES             : keyword

fname             : prefix name for any backing files created by this run. (Alphanumeric, 4 characters, first
                     character must be alphabetic)

Note


1.      fname is used as a prefix for all files created during the current run. The four characters are appended
        with two digits in the range 12 to 35 to create each individual file.

Example


        FILES          BILL




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-3
    RESPONSE User Manual                                                                                Appendix A


A.6         TITLE Command
To define a title for this run. Recommended.

         TITLE                         title




Parameters

TITLE             : keyword.

title             : this line of text will be printed out at the top of each page of ASAS output. (Alphanumeric, up
                     to 74 characters)

Example


        TITLE        THIS IS AN EXAMPLE OF A TITLE LINE



A.7         TEXT Command
To define a line of text to be printed once only near the beginning of the output. Several TEXT lines may be
defined to give a fuller description of the current analysis on the printed output.


                TEXT                 text




Parameters

TEXT              : keyword

text              : this line of text will be printed once, at the beginning of the output. (Alphanumeric, up to
                     75 characters)

Example


        TEXT       THIS EXAMPLE OF THE TEXT
        TEXT       COMMAND IS SPREAD
        TEXT       OVER THREE LINES




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-4
    RESPONSE User Manual                                                                                Appendix A


A.8         STRUCTURE Command
To define the name of an existing structure within the current project which is to be processed in this run.
Compulsory.




Parameters

STRUCTURE : keyword

sname             : structure name identifying which existing structure is to be accessed from the project defined
                    on the PROJECT command. (Alphanumeric, 4 characters, the first character must be
                     alphabetic)

Example


       STRUCTURE JOHN



A.9         NEWSTRUCTURE Command
To define a new structure name associated with the results created by the current run. Compulsory except for
Solution STRESS.




Parameters

NEWSTRUCTURE : keyword

nsname                     : structure name associated with the results being created by the current run in order to
                              identify these results from others. nsname must be unique for this project
                              (Alphanumeric, 4 characters, the first character must be alphabetic).




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-5
     RESPONSE User Manual                                                                               Appendix A


Note


1.     This command must not be used with analysis type SOLUTION STRESS. These results are written to
       files with the name defined on the STRUCTURE command.

Example


       NEWSTRUCTURE               STR2



A.10        OPTIONS Command
To define the control options for this run. Optional.




Parameters

OPTIONS           : keyword

option            : 4 character option name, or list of option names. See Appendix C for details of each option
                     available.

Examples


       OPTIONS          DATA        NODL       END



A.11        RESTART Command
To define the restart stages to be executed for this run. Optional.




Parameters

RESTART           : keyword




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-6
       RESPONSE User Manual                                                                              Appendix A


first             : number of the first restart stage to be computed by this run.

last              : number of the last restart stage to be computed by this run.
                     Optional, if omitted, defaults to the last valid stage for this run.

Note


1.      All valid restart stages between first and last for the current analysis will be executed. Only valid restart
        stage numbers must be defined for first and last. The valid stage numbers are given in Appendix D.

2.      If further post processing is to be carried out on the results of this analysis, the analysis must eventually
        run to the final restart stage.

Example


An example to request that the current run should execute all valid stages between data input and cross checks
(Stage 1) and element stress calculations (Stage 8)

        RESTART 1             8



A.12        SAVE Command
To define which files or sets of files are to be saved for subsequent runs. Two types of files may be saved, those
for further numeric processing and those for interfacing to graphical results display programs such as
FEMVIEW.


A.12.1 Files for Numerical Processing




Parameters

SAVE              : keyword

set               : keywords to define the sets of files to be saved for use in subsequent processing runs.
                    Permitted values are:

                     Name                Subsequent run/processing

                     LOCO         -      for loadcase factoring using LOCO
                     STRE         -      to postprocess element stresses and forces using POST and BEAMST


FILES             : Keyword




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-7
     RESPONSE User Manual                                                                                        Appendix A


Notes

1.      If several sets of files are to be saved they may be specified on one or several SAVE commands.

2.      The SAVE command may be used to save explicit files. See ASAS User Manual for details.

Example


To save files necessary for further loadcase factoring and combining

        SAVE       LOCO       FILES



A.12.2 Interface Files for Plotting Programs


       SAVE            FEMD                 FEMS             (FILES)            CREATE             name   FILE     filenm

                                                                                APPEND
                       PATD
                                             (FILES)
                       PATM




SAVE          : keyword

FEMD          : keyword to denote displacements to be added to FEMVIEW file

FEMS          : keyword to denote stresses to be added to FEMVIEW file

FILES         : keyword (Optional)

CREATE : keyword to indicate that model data must be added to FEMVIEW file

APPEND : keyword to indicate model data not to be added to FEMVIEW file

name          : model name for FEMVIEW (defaults to structure name)

FILE          : keyword to indicate file name follows

filenm        : name of file to contain FEMVIEW data

PATD          : keyword to denote displacements to be added to binary PATRAN file

PTDC          : keyword to denote displacements to be added to ascii PATRAN file

Example




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.            Page A-8
    RESPONSE User Manual                                                                                 Appendix A


To save files necessary for viewing results in FEMVIEW

       SAVE FEMD FEMS FILES APPEND TANKER FILE TANKER.FVI



A.13        RESU command
To specify saving of results. The displacements and stresses from response analysis will be saved.



           RESU




Parameters

RESU              : keyword

Example


            RESU



A.14        UNITS Command
Allows redefinition of units for the printed results if UNITS have been employed in the original analysis. If this
command is omitted and UNITS were employed in the original analyses, the printed results have the same units
as the original results.


                UNITS                         resultnm                                 unitm




Parameters

UNITS             : keyword

resultnm          : identifier for results units to be modified. The following keywords are available.

                                           DISP          -   Displacement printing
                                           STRE          -   Stress or force printing




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.    Page A-9
     RESPONSE User Manual                                                                                  Appendix A


unitnm            : name of unit to be utilised (See Notes below)

Notes


1.      For the results units, the angular term may be specified (default is radians). Valid names are:-

                                           RADIAN(S), RAD(S)
                                           DEGREE(S), DEG(S)


2.      Only those terms which are required to be modified need to be specified, undefined terms will default to
        those given by the global units definition. For example, if the global units are N, M, then the command

                                           UNITS STRE MM

        will provide stresses in terms of N/MM2.


3.      Valid Unit Names

        Length Unit                        METRE(S)                            M
                                           CENTIMETRES(S)                      CM
                                           MILLIMETRE(S)                       MM
                                           MICROMETRE(S)                       MICM
                                           NANOMETRE(S)                        NANM
                                           FOOT, FEET                          FT
                                           INCH, INCHES                        IN



        Force                              NEWTON(S)                           N
                                           KILONEWTON(S)                       KN
                                           MEGANEWTON(S)                       MN
                                           TONNEFORCE(S)                       TNEF
                                           POUNDAL(S)                          PDL
                                           POUNDFORCE,                         LBF
                                           KIP(S)                              KIP
                                           TONFORCE(S)                         TONF
                                           KGFORCE(S)                          KGF

Example


The global analysis units are N and M, but the displacements are to be printed in mm and the stresses in
KN/mm2.

        UNITS           DISP            MM
        UNITS           STRE            KN         MILLIMETRES

Note that the reactions printed in the displacement report will be in Newtons and millimetres.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-10
    RESPONSE User Manual                                                                                 Appendix A



A.15        END Command

To terminate the preliminary data. Compulsory.


          END




Parameters

END           : compulsory keyword




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-11
    RESPONSE User Manual                                                                                Appendix A




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page A-2
RESPONSE User Manual                                                                                          Appendix B




                            Appendix B                    - Running Instructions for RESPONSE


B.1         ASAS Files Required by RESPONSE
RESPONSE operates on the files produced by the preceding ASAS natural frequency analysis and hence these
files must physically be present on the user’s disk for the program to run successfully. In all cases the Project
File must exist which contains information about all other files in the current set of analyses. The name of this
file is derived from the four character Project Name defined on the PROJECT command. For example, if the
project name is PRDH, then the Project File will be PRDH10.

In the preceding ASAS natural frequency analysis, SAVE DYPO FILES must have been specified in the
preliminary data to save the required backing files for RESPONSE. These backing files will be identified by the
file name which is derived from the 4 character name on the ASAS FILES command. For example, if this name
had been RNDH, then the backing file containing the dynamic results would be RNDH35.

If the LOADFILE command is being used then the name of the file from the WAVE analysis is required on the
LOADFILE command line.

The preceding ASAS natural frequency analysis must have run to completion. If the preceding analysis did not
complete either because of a failure or because the user terminated the run deliberately with a RESTART
command, RESPONSE may error because some files or information may not exist.


B.2         Saving Files Produced by RESPONSE
RESPONSE uses files in a similar way to ASAS, and a new physical file of the response stresses and
displacements will be produced. This file will be name nnnn35, where nnnn is the four character name on the
FILES command in the RESPONSE preliminary data. This physical file may be saved (and hence used for
further post-processing) by including a SAVE command in the preliminary data of the RESPONSE run. If this
command is absent then the file will not be saved. In addition, the results from RESPONSE will be saved to a
file called nnnn45 by including a RESU command in the preliminary data. Note that RESPONSE does not
delete any of the ASAS files used as these may be required for other post-processing.



B.3         Running Instructions for RESPONSE
See the appendices in the ASAS User Manual for details on how to run any of the programs in the ASAS suite.




      Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page B-1
RESPONSE User Manual                                                                                       Appendix B




   Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page B-2
    RESPONSE User Manual                                                                                   Appendix C




                                                  Appendix C                    - Options




This appendix describes the user options available in RESPONSE.

User options are specified on the OPTIONS command line in the preliminary data as a series of 4 character
abbreviations. Many analyses can be performed without the user selecting any options. If the user wishes to
select what processing or printing is required, the appropriate options can be supplied as listed below.


C.1         Miscellaneous Options
      Option Name                        Description

      NOBL                               Do not print the ASAS banner pages




C.2         Options which Control the Printing of the Data File Images
If the user takes no action, ASAS will print the image of every data line. This printing can be prevented by using
the PRNO option. If selective printing is required, the user specifies PRNO together with the appropriate
printing option shown below:


      Option Name                        Description

      PRNO                               Print only selected data file images

      CLOA                               Print the load file images

      CDAM                               Print the damping data file images

      CSEI                               Print the seismic data file images

      CQAK                               Print the load combination data file images




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page C-1
   RESPONSE User Manual                                                                                     Appendix C




C.3          Options which Control the Printing of Expanded Data Lists
      Option Name                       Description

      NODL                              Print only selected expanded data lists

      LOAD                              Print the expanded load data

      DAMP                              Print the expanded damping data

      SEIS                              Print the expanded seismic data

      QUAK                              Print the expanded combinations data

      RESU                              Print the expanded result selection data




C.4          Options which Affect the Course of the Analysis
      Option Name                       Description

      DATA                              Stop after checking data. This is useful to enable careful checking of the
                                        data. If the check produces no error messages and option GOON has also
                                        been specified, then the Restart Stage 1 files will be saved. The subsequent
                                        restart run can omit Stage 1 and does not require any data except the
                                        Preliminary Deck.

      GOON                              Proceed even after printed WARNINGS. This option allows the run to
                                        continue despite doubtful data. It should only be used after a run in which
                                        the WARNINGS have been noted and rejected as acceptable. See Option
                                        DATA also.

      FIXD                              Allows the input data to be read in as fixed format ie version HO8 or
                                        previous.




C.5          Options which Control Printing During the Run
      Option Name                       Description

      PART                              Print the partitioning information

      PTMO                              Print the eigenvectors and generalised masses used in the calculations




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page C-2
    RESPONSE User Manual                                                                                         Appendix C




C.6         Options which Control the Printing of Results
ASAS prints the complete results unless told otherwise. The stresses are printed in scientific notation and related
to the axes which are standard for the element. The following options will modify the printing:-


      Option Name                        Description

      NODI                               Do not print reactions and displacements

      NOST                               Do not print the stresses

      FORF                               Print the stresses as normal numbers without scientific notation. The output
                                         defaults to scientific notation if a line of stresses has very large or very
                                         small values

      GLST                               Print global instead of local stresses

      BYEL                               Output stresses by element rather than by loadcase

      CBST                               Calculate beam stresses but do not print the stresses. Beam stresses will be
                                         written to the results database. (Note: RESU must be specified)

      PBST                               Calculate and print the beam stresses. Beam stresses will be writen to the
                                         results database. (Note: RESU must be specified). Not for transient
                                         solution.


      PSHS                               Print shell/plate surface stresses. (Note: RESU must be specified). Not for
                                         transient solution.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.          Page C-3
   RESPONSE User Manual                                                                                       Appendix C


C.7        Special Analysis Options
      Option Name                       Description

      ZERO                              Allows a steady state analysis to be carried out with zero forcing frequency,
                                        so a static improvement analysis on the dynamic model of the structure may
                                        be carried out. Note: The forcing frequency in the harmonic load data must
                                        not be set to zero.

      ABSO                              Allows the acceleration produced by transient seismic analysis to be
                                        converted from relative accelerations to absolute accelerations i.e. the
                                        effects of the base accelerations are included. This should only be used with
                                        Solution Transient and Seismic.

      WIND                              If option WIND is specified then load case titles saved by WAVE will be
                                        copied to the RESPONSE backing files for use by WINDSPEC. Only
                                        applicable if option WIND has been used in the preceding WAVE run




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page C-4
    RESPONSE User Manual                                                                                       Appendix C


C.8         Options to Save Data and Results on File
Input data and results are saved mainly using the SAVE file FILES command in the preliminary data, see
Appendix A.12. There are also options which cause results to be saved on backing files to enable further post-
processing to be carried out.


      Option Name                        Description

      ASDS                               The ASAS plot file is updated so that the displacements from a Seismic or
                                         Steady State analysis can be plotted. Note: The ASDS option is also
                                         required in the ASAS dynamic analysis in order to store the basic structural
                                         data on the plot file.

      NOTR                               Do not write the results to the User Results Storage Database.


      NOSS                               Do not calculate and save shell/plate surface stresses to the results database
                                         even if RESU specified.

      PODB                               Write the stress time history for the defined elements for all nodes, stress
                                         types and time steps to the User Results Storage Database for a transient
                                         analysis.

      PORT                               A FORTRAN sequential file is written containing the displacements,
                                         velocities and accelerations at requested nodal freedoms and stresses on
                                         requested elements from a transient response analysis.


      POTD                               A subset of the PORT file is written containing the nodal displacement
                                         velocity and acceleration histories only.


      POTS                               A subset of the PORT file is written containing the stress histories only.




  Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.        Page C-5
  RESPONSE User Manual                                                                                  Appendix C




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page C-6
    RESPONSE User Manual                                                                                  Appendix D




                                Appendix D                    - Restart Stages for RESPONSE


D.1        Restart Stages for Steady State Analysis

   No.          Process

   1            Data Checks
   2            Form Load Vectors
   3            Transform Loads to Normal Coordinates
   4            Solution Stage (Steady State, Seismic or Transient)
   5            Back Substitution
   7            Displacement Printing
   8            Stress Calculation
   10           Stress Printing




D.2        Restart Stages for Seismic Analysis
   No.          Process

   1            Data Checks
   4            Solution Stage (Steady State, Seismic or Transient)
   5            Back Substitution
   6            Displacement Combination
   7            Displacement Printing
   8            Stress Calculation
   9            Stress Combination
   10           Stress Printing




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page D-1
    RESPONSE User Manual                                                                                  Appendix D




D.3        Restart Stages for Transient Analysis
   No.          Process

   1            Data Checks
   3            Transform Loads to Normal Coordinates
   4            Solution Stage (Steady State, Seismic or Transient)
   5            Back Substitution
   7            Displacement Printing
   8            Stress Calculation
   10           Stress Printing




D.4        Restart Stages for Loadfile Analysis
   No.          Process

   1            Data Checks
   2            Form Load Vectors
   3            Transform Loads to Normal Coordinates
   4            Solution Stage (Steady State, Seismic or Transient)
   5            Back Substitution
   7            Displacement Printing
   8            Stress Calculation
   10           Stress Printing




D.5        Restart Stages for Solution Stress
   No.          Process

   8             Stress Calculation
   10            Stress Printing




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page D-2
   RESPONSE User Manual                                                                                  Appendix D




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page D-3

				
DOCUMENT INFO
Categories:
Tags:
Stats:
views:10
posted:8/22/2012
language:English
pages:107
Subrahmanian KR Subrahmanian KR
About Civil Engineer