Post by subrahmanian1956

VIEWS: 7 PAGES: 115

									                        POST 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superseded by a newer version of this guide.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.
                                 POST 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

1.1                   1-1                     Update                   Delete references to legacy program PICASO

4.3.2                 4-5                     Update                   Delete Section 4.3.2 (PICASO Input)

App A.12              A-12                    Update                   Delete references to legacy program PICASO




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

                                                 TABLE OF CONTENTS


1.   Introduction ........................................................................................................ 1-1
  1.1.    General Description ................................................................................... 1-1
  1.2.    Facilities Available .................................................................................... 1-2
     1.2.1.    Shell Elements ................................................................................... 1-2
     1.2.2.    Laminated Shell Elements ................................................................. 1-3
     1.2.3.    Beam Elements .................................................................................. 1-3
     1.2.4.    Axisymmetric Solid and Shell Elements ........................................... 1-3
     1.2.5.    Harmonic Solids................................................................................. 1-3
  1.3.    Program Requirements............................................................................... 1-4
  1.4.    Element Grouping ...................................................................................... 1-4
  1.5.    Loadcase Combination............................................................................... 1-5
  1.6.    Local Axes Consideration .......................................................................... 1-5
     1.6.1.    Local Axes for SHELL, LAMI and SBEAM Data ............................ 1-5
     1.6.2.    Local Axis for BRICK Data .............................................................. 1-6
     1.6.3.    Output Axes Definition ...................................................................... 1-6
     1.6.4.    Averaging Groups with Differing Output Systems ......................... 1-13
     1.6.5.    Material Axes for Laminated Shells ................................................ 1-14
  1.7.    Processing of Summed Out-of-Plane Shear Forces for the TRB3 Element 1-
  15
  1.8.    Boundary Conditions for Harmonic Runs ............................................... 1-16
  1.9.    UNITS ...................................................................................................... 1-16
2. INPUT Data ....................................................................................................... 2-1
  2.1.    General Principles ...................................................................................... 2-1
     2.1.1.    Special Symbols ................................................................................. 2-3
  2.2.    UNITS Command ...................................................................................... 2-9
  2.3.    Data Type Commands.............................................................................. 2-11
     2.3.1.    Data Type and Sub-Type Commands .............................................. 2-11
  2.4.    Output Axis Commands........................................................................... 2-13
     2.4.1.    CONS Command (SHELL or SBEAM data) .................................. 2-13
     2.4.2.    OUTP Command (SHELL data only).............................................. 2-14
     2.4.3.    OUTR Command (SHELL data only) ............................................. 2-15
     2.4.4.    OUTT Command (SHELL data only) ............................................. 2-16
     2.4.5.    OUTB Command (SBEAM data only) ............................................ 2-16
     2.4.6.    SKEW Command (SHELL data only) ............................................. 2-17
  2.5.    Group Data Commands............................................................................ 2-18
     2.5.1.    LAYE Command (LAMI data only)................................................ 2-18
     2.5.2.    RDAT Command ............................................................................. 2-20
     2.5.3.    TCRD Command ............................................................................. 2-21
  2.6.    Group/Element Selection Commands ...................................................... 2-22
     2.6.1.    GROU Command............................................................................. 2-22
     2.6.2.    EXTR Command ............................................................................. 2-23
     2.6.3.    SKIP Command ............................................................................... 2-24
     2.6.4.    NOAV Command ............................................................................ 2-25
     2.6.5.    AVGR Command............................................................................. 2-26
  2.7.    Loadcase Combination Commands ......................................................... 2-27
     2.7.1.    NEWC Command ............................................................................ 2-27
     2.7.2.    ADDC Command............................................................................. 2-28



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                             i
POST User Manual                                                                                                           Contents
     2.7.3.    ADDF Command ............................................................................. 2-29
  2.8.    Stress Type Selection Commands ............................................................ 2-31
     2.8.1.    FACT Command .............................................................................. 2-31
     2.8.2.    AVST Command ............................................................................. 2-31
     2.8.3.    FANM Command (SHELL data only) ............................................ 2-32
     2.8.4.    BANM Command (SHELL data only) ............................................ 2-33
     2.8.5.    PRST Command .............................................................................. 2-34
     2.8.6.    PRVM Command............................................................................. 2-35
     2.8.7.    SHRS Command (SHELL data only) .............................................. 2-36
     2.8.8.    WOOD Command (SHELL data only)............................................ 2-37
     2.8.9.    REIN Command (SHELL data only) ............................................... 2-38
  2.9.    Control Output Commands ...................................................................... 2-39
     2.9.1.    PRIN Command ............................................................................... 2-39
     2.9.2.    PLOT Command .............................................................................. 2-40
  2.10. Check Stresses ......................................................................................... 2-41
     2.10.1. FECS and FECM Commands (SHELL data only) .......................... 2-41
     2.10.2. VONM Command ............................................................................ 2-42
     2.10.3. TRES Command .............................................................................. 2-43
  2.11. Harmonic Combination Commands ........................................................ 2-44
     2.11.1. Data for Harmonic Analyses ............................................................ 2-44
     2.11.2. ANGL Command (HARM Data only) ............................................ 2-45
     2.11.3. COMB Command (HARM data only) ............................................. 2-45
     2.11.4. SELE Command (HARM data only) ............................................... 2-46
     2.11.5. COS and SIN Commands (HARM data only) ................................. 2-47
  2.12. Miscellaneous Commands ....................................................................... 2-49
     2.12.1. SECT Command .............................................................................. 2-49
     2.12.2. ANGL Command (SHELL data only) ............................................. 2-50
     2.12.3. END Command ................................................................................ 2-50
3. Examples ............................................................................................................ 3-1
  3.1.    Example 1: Default Data ........................................................................... 3-1
  3.2.    Example 2: Simple Shell Result Processing ............................................. 3-1
  3.3.    Example 3: Simple Axi-symmetric Result Processing ............................. 3-2
  3.4.    Example 4: Post Processing Component Results from Multi Level
  Axisymmetric Analysis .......................................................................................... 3-3
  3.5.    Example 5: Loadcase Combinations......................................................... 3-4
  3.6.    Example 6: Post Processing Harmonic Analyses ..................................... 3-5
  3.7.    Example 7: Harmonic Combinations ........................................................ 3-6
  3.8.    Example 8: Post Processing Shell Compatible Beams ............................. 3-7
  3.9.    Example 9: Post Processing Laminated Shells ......................................... 3-8
4. Output ................................................................................................................ 4-1
  4.1.    Printed Output ............................................................................................ 4-1
     4.1.1.    SHELL Data....................................................................................... 4-1
     4.1.2.    LAMI Data ......................................................................................... 4-2
     4.1.3.    Shell BEAM Data .............................................................................. 4-2
     4.1.4.    BRICK, AXIS and HARM Data........................................................ 4-2
  4.2.    Backing Files ............................................................................................. 4-2
  4.3.    Plotting Program Input ............................................................................... 4-3
     4.3.1.    FEMVIEW Input ............................................................................... 4-3
     4.3.2.    PATRAN® Input ................................................................................ 4-4
Appendix A - Preliminary Data Block for POST .................................................A-1



Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.                            ii
POST User Manual                                                                                                        Contents
  A.1    Introduction ................................................................................................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-3
  A.7    TEXT Command ........................................................................................A-4
  A.8    STRUCTURE Command...........................................................................A-4
  A.9    COMPONENT Command .........................................................................A-5
  A.10 NEWSTRUCTURE Command .................................................................A-6
  A.11 OPTIONS Command .................................................................................A-6
  A.12 SAVE Command .......................................................................................A-8
  A.13 RESU Command........................................................................................A-9
  A.14 UNITS Command (not valid for fixed format ASAS data) .......................A-9
  A.15 END Command ........................................................................................A-10
Appendix B -     - Running Instructions for POST .................................................. B-1
  B.1    ASAS Files Required by POST ................................................................. B-1
  B.2    Running Instructions for POST ................................................................. B-1
Appendix C -     - Equations used for Stress Calculations ....................................... C-1
  C.1    Notation...................................................................................................... C-1
  C.2    Stress Formulae .......................................................................................... C-2
  C.3    Wood-Armer Calculations ......................................................................... C-3
    C.3.1     Wood-Armer Moments - Orthogonal Reinforcing ............................ C-3
    C.3.2     Wood-Armer Moments - Skewed Reinforcing .................................. C-4
  C.4    Reinforcement Area Calculations .............................................................. C-4
Appendix D - - Loadcase Combination Methods ................................................D-1




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



POST
Post-processing for ASAS Stress Output


1.     Introduction


1.1. General Description

POST is a general post-processing program designed to aid the engineer using ASAS to analyse shell, solid and
three-dimensional axisymmetric structures. It performs many tedious tasks on the ASAS results such that the
engineer can concentrate on the design of his structure without the need to waste precious man time in repetitive
arithmetic calculations.

ASAS and LOCO finish by printing stresses and/or moments for each node of each element and storing these on
a backing file. POST reads these stresses from the backing file and averages the stresses given by all the
elements at each node. From these, surface, principal, von-Mises, Tresca, section stresses and Wood-Armer
moments may be calculated and printed depending on the processing requested and the element type. These and
other facilities are described fully in the next section.

Note that if POST is to be run, the command SAVE LOCO FILES must be included in the preliminary data of
the previous ASAS or LOCO run, so that the appropriate files will be retained for use by the program.

The program will also convert stress results into a suitable format ready for plotting using FEMVIEW or
PATRAN®*.

To produce an interface file for one of these plotting programs, SAVE commands must be given in the POST
preliminary data (see Appendix A-). In addition, the run results may be saved permanently on the project files
using the RESU command.

Note that the BR32 element is not available with FEMVIEW at present.

*     PATRAN®            - a corporate trademark of the MSC Software Corporation.




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




1.2. Facilities Available

POST has six different processing paths depending on which type of element is being considered. The process
required is selected by the user and causes POST to processes only those elements of the correct type in the
model. Thus an analysis having a number of differing element types will require more than one run of POST to
post-process the whole model. The processes are identified by data type as follows:


       Data Type                       Element Family                                                   Elements
       Command

         SHELL                       thick & thin shells                  QUS4 TCS6 TCS8 GCS6 GCS8 TBC3

                                            plate                         SLB8
                                         membranes                        QUM4 QUM8 TRM3 TRM6
                                         sandwiches                       SND6 SND8 SN12 SND16
                                       triangular plate                   TRB3
         LAMI                         laminated shells                    QUS4 TCS6 TCS8
         SBEAM                    shell compatible beams                  GCB3 TCBM
         BRICK                               bricks                       BRK6 BRK8 BR15 BR20 BR32 TET4 TE10
    AXIS SOLID                      axisymmetric solids                   QUX4 QUX8 TRX3 TRX6
    AXIS SHELL                      axisymmetric shells                   ASH2
   HARM SOLID                 harmonic axisymmetric solids                QHX4 QHX8 THX3 THX6
   HARM SHELL                 harmonic axisymmetric shells                AHH2



Only one data type command may be submitted in each run; other data type commands will be ignored.

Restriction: When using SAVE FEMS or SAVE PICA, only one of the shell element families may be processed
in each run. The GROU command should be used to restrict the element type(s) to those associated with one of
the SHELL families. (Note that thick and thin plates are considered as one element family).




1.2.1.      Shell Elements

For Shell elements, top, middle and bottom surface stresses are calculated for each element in turn, and a set of
average stresses is calculated for each node which is associated with two or more elements. The outshears for
plate and shell elements, with the exception of the TRB3 element, may also be averaged by using the SHRS
command.

The in-plane principal stresses (σ1 and σ2) are printed for each of the three surfaces along with the principal
stress difference (σ1 - σ2). Two ’check stresses’ can be provided by the user, against which the stresses at each
node can be compared and flagged if they exceed the check stress. As an aid to results interpretation, asterisks
are used to highlight the highest absolute values of σ1, σ2 and (σ1 - σ2) for each surface.




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


1.2.2.      Laminated Shell Elements

The nodal stresses in and normal to the fibre direction and also the inshear stress are calculated for individual
laminae from the resultant strain for the whole composite section. Where a node is associated with more than
one element in the same group the strains for the whole composite section will be averaged at the node prior to
the layer stresses being calculated.




1.2.3.      Beam Elements

Results for TCBM and GCB3 elements are processed in terms of member forces and moments. Where a node is
associated with more than one element within the same groups the averaged results will be presented. The user
may also specify a new output axes for the elements to override the default element local axes.




1.2.4.      Axisymmetric Solid and Shell Elements

The program calculates average nodal stresses for the solid elements. The user may print the averaged nodal
stresses for any or all of the loadcases, each factored by a constant if required. In addition to the average nodal
stresses the program prints the von Mises equivalent stress for each node and the factor by which this stress
exceeds a user defined allowable level.

The user may also request a printout of principal stresses and directions for any or all of the loadcases, again
factored by a constant if required. In addition to the principal stresses and directions, the program prints the sum
of the principal stresses, the von Mises equivalent stress, the Tresca stress and the factor by which the Tresca
stress exceeds a user defined allowable level.

For axisymmetric solids only, the user may request additional information for the stresses across a specified
section of the structure. This comprises the average ‘membrane’ stress components across the section and the
bending stress components at each node across the section. The principal membrane stresses are also printed
along with the corresponding stress intensities.




1.2.5.      Harmonic Solids

Additional features of POST permit the calculation of the average nodal stresses for the harmonic solid elements
THX3, QHX4, THX6 and QHX8. The user may generate a number of combined loadcases from structures with
different harmonic numbers (analogous to the manner of operation of LOCO) and produce stress output at a
number of angular stations around the structure for these combined loadcases. This allows the user to perform
Fourier series types of analysis for known harmonics of load at substantially less cost than would be involved in
a full three dimensional (brick) analysis.




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


In order to identify the combined results being created, a new structure name is required and this is defined using
the NEWSTRUCTURE command in the preliminary data. If the set of files for the combined loadcases has been
saved and additional POST runs on the same load cases are needed, a harmonic re-run with simplified data input
requirements may be performed. In the re-run, the structure name becomes the new structure name in the
original run with the NEWSTRUCTURE command omitted. All the loadcase combination data are also omitted.

Average nodal stresses at each circumferential station, von Mises equivalent stress and the factor by which it
exceeds a user defined allowable are printed.

Principal stresses may be produced in an analogous manner to the purely axisymmetric values described above.

Currently the facility to produce extra information about stresses across specific sections is not available with the
harmonic elements.


1.3. Program Requirements

The program works directly from backing files created during an ASAS or LOCO run. The files described must
be saved using the appropriate commands described in the User Manuals. All other information is provided via
the data commands described in detail in Chapter 2 Any elements other than those allowed for the data type
specified in Section 1.2 are ignored by the program; however, at least one of these elements types must be
encountered.

For an axisymmetric job all the elements are not only axisymmetric themselves but the loading is also
axisymmetric. For harmonic analyses the program checks that the user specified harmonic number on all the
harmonic elements accessed from an individual ASAS structure have the same harmonic number. Clearly, a
structure with a mixed harmonics in a loadcase is physically meaningless as discontinuities in displacements are
implied.


1.4. Element Grouping

It may not always be desirable, or even meaningful, to average the nodal stresses of adjacent elements. For
example, where there are different material properties or thicknesses between elements, the strains may be
continuous but there will be step changes in the stresses.                         If the nodal stresses are averaged at such
discontinuities, these step changes will be lost and a false average obtained.

For this reason, POST considers the elements in groups. These groups may be made up of one ASAS element
group (i.e. the groups defined in the ASAS element topology data), or of elements defined by a list of element
numbers in the POST data. In the case of the former, individual elements may be omitted from a group by using
the SKIP command in the POST data. Note that if EXTR groups are created in POST, then the CREATE
Command should be used on the SAVE FEMS line.

POST works through the groups in order, considering all loadcases for one group before moving on to the next.
Within the groups, all nodal stresses are averaged, but no averaging occurs across the group boundaries.




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


If a group contains a mixture of more than one sub-type, e.g. shells, plates and membranes, then POST will only
process elements with the same type as the first valid element found for that group (i.e. shell, membrane or
plate). If other element types are required from a group then new groups can be created using the EXTR
command (Section 2.6.2) containing only the element types required.

In SHELL data, should any thickness discontinuity be encountered between adjacent elements within a group, an
error message is printed and POST moves on to the next group. The allowable tolerance is 1% difference in
thickness at each node. It is possible to override this error by a warning if option CCGO is specified in the
preliminary data.

For SHELL and SBEAM data, a check is also provided to ensure the offset compatibility between adjacent
elements within a group. An error message is printed if this check fails and POST moves on to the next group.
As before, it is possible to change the error status to warning status by specifying option CCGO in the
preliminary data.

For LAMI data, strains rather than stresses are averaged. Nodal thickness however, is used in the calculation of
the individual lamina stresses and so once again there may not be nodal discontinuities within a group.
Additionally all the elements within the group must have a consistent ASAS material axes and composite layer
data in order that the layer stresses are calculated correctly from the averaged strains. Further consideration of
the ASAS material orientation is given in Section 1.6.5.


1.5. Loadcase Combination

The program allows the user to create new loadcases by factoring and combining any or all of the existing
loadcases, including new loadcases already created. Average nodal stresses and principal stresses may be
printed for these combinations as well as for the original loadcases. A number of combination methods are
available in addition to simple summation. These are described in detail in Appendix D-.


1.6. Local Axes Consideration



1.6.1.      Local Axes for SHELL, LAMI and SBEAM Data

ASAS nodal stresses are calculated in the element local axis system for some shell elements and the shell beam
elements. In cases where the element local axis systems of adjacent elements within an element group are not
consistent (that is, the same orientation with respect to the global axis system), it is not meaningful to average
nodal stresses across element boundaries. In such cases it is possible to reorientate the stresses into a consistent
set before averaging by specifying a new axis system, called the output axis system, which is common to all
elements within the group.            The new output axis systems are defined by the OUTP, OUTR, and OUTT
commands for shell elements and the OUTB command for the shell beam elements.

Whilst an output command must be used for any group containing elements with inconsistent axes they may also
be used whenever the user simply wants to reorientate the output axes. If an output command is not used for a




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


given group, then the CONS command should be used for that group, indicating the axes are consistent. POST
is not able to check for axes consistency, so if CONS is used it is the user’s responsibility to satisfy himself that
the axes are consistent.

For laminated shells the strains used to calculate the individual layer stresses are once again in the element’s
local axes system. In this case the output orientation of the results is already predefined by the fibre orientation
for each layer which in turn is related to the material axes of each each element. POST automatically converts
the ASAS strains into the material axes before the nodal averaging, and then further rotates the strains into the
fibre direction for each of the individual layers examined.




1.6.2.      Local Axis for BRICK Data

In the case of brick and axi/harmonic elements, the ASAS results are in the global axis system and therefore
consistent. For this reason there are no commands for reorientating stresses for these element types.




1.6.3.      Output Axes Definition

(a)      Cartesian Axes System - OUTP Command


The cartesian axes are defined in terms of a reference direction and a reference point. Firstly, the top and bottom
surfaces of the shell are defined. This is done by drawing a vector from the reference point towards the node in
question. This is called the control vector. The first surface cut by the control vector is defined as the bottom
surface, and the second as the top surface. The new Z axis at this node is normal to the shell and positive in the
direction from the bottom surface towards the top surface. See Figure 1.

The new X axis lies in the plane containing the new Z axis and the reference direction: note that the reference
direction is specified by direction cosines with respect to the global axis system. The X axis is positive on the
side of the Z axis containing the positive reference direction. The new Y axis forms a right-handed set with the
new X and Z axes. See Figure 2.

The above rules break down in two cases. The first is where the reference direction and the new Z axis are
parallel and the second where the control vector is tangential to the shell surface.

In both cases, warnings are printed when the control vector is within 5° of the shell surface tangent. Errors are
printed should the angle be less than 1°. In the case of an error the node in question is omitted.




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




                      Figure 1                                                                      Figure 2




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


Example: Cylindrical Shells

Consider a cylindrical shell of diameter 10 and length 100 orientated parallel to the Z axis with its central axis at
X=5, Y=0. A suitable output axes may be specified by a reference direction parallel to the central axis and the
reference point on the central axis halfway along the cylinder.




                                                                Figure 3

The reference point could be anywhere within the boundary of the tube, but the central location ensures the least
chance of failing the 5º check. The resulting output axes system has the outer surface of the cylinder as the top
surface, the local x’ stress in the longitudinal direction and the local y’ stress in the hoop direction.




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


Example: Flat Shells/Plates

For a flat plate the ideal position for the reference point is on the plate normal through the centre of the plate at a
distance equivalent to half the plate length below the plate. Again the exact position is not critical. The
reference direction should then be defined in the plane of the plate in the direction required for the local x’ stress.


                                       L                         y'
                                             y'   node 2
                                                                 x'
                              node 1         x'

                                                  L                              Reference direction
                                                  2
                                                           Reference Point


                                                                Figure 4

In some cases it may be desirable to use the same output axes definition for a series of plates. If the reference
point is placed between plates this will result in a reversal of the local y’ direction. This may not be significant
for stress results but will affect the definition of the skew angles for Wood-Armer moments and reinforcement
area calculations.



                               y'           x'         T                                  y'            x'     T
                                                       B                                                       B


                                                                                          y'            x'     T
                                       Reference poi nt
                                                                                                               B


                                            x'
                                           y'
                                                       B                                          Reference poi nt
                                                       T




                                                                Figure 5




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



(b)     Radial Axes System - OUTR Command


The cartesian axes definition cannot be used to give radial and hoop stresses for a flat circular disc. In order to
cover this case the radial axes definition may be used. These axes are defined by two points, the first is the
centre point for the radial axes system and the second is a reference point as for the cartesian axes system. A
reference direction is set up for each individual node within the group and is defined by the vector from the node
to the centre point. The local axes system for the node is then set up from the reference direction and the
reference point using the same conventions as for cartesian axes definition. See Figure 6.

At the centre of the disc the centre point may coincide with the central node, such that a reference direction is not
defined. In this case (and also if the reference direction defined is normal to the shell) the local X will be
defined as lying in the plane containing the local Z (or shell normal) and the global ordinate that is most normal
to the local Z. In the case of the local Z being normal to two global ordinates, the global X would be used as
first preference and the global Y as the second. The local Y is then defined normally to both local X and Z.




                                                                                 Reference                   Z1
                                     Z2                  Centre Point
                                                                                 Direction
                                                                                 for Node 1
                                                 X2                                                X1


                   Y2                     Node 2                                                              Node 1
                                                                                                        Y1




                                                             Reference Point



                                                                Figure 6




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


Example: Hemispherical Shell/Disc

For a hemispherical shell the reference point should be placed at or near the centre of the hemisphere (at zero
radius) and the centre point on the hemisphere at the centre.

In the case of a flat disc the reference point should be positioned on the axis of the disc at a distance equivalent
to the radius of the disc below the disc.




                                                                Figure 7

In both cases the local y’ stress will be in the hoop direction. For the hemispherical shell the local x’ stresses will
be in the longitudinal direction and for the flat disc in the radial direction.




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


(c)    Toroidal Axes System - OUTT Command


The toroidal axes system is used to give hoop and longitudinal stresses for torus shaped structures. These axes
are defined by the coordinates of the torus centre point, the direction cosines for the major axes and the major
radius. For each node a radial slice is made through the torus at the position of the node. The axes reference
point for the node is then defined as being on the circular minor axis at the position of the slice, and the reference
direction as tangential to the circular minor axis at the same point. The reference direction is positive in the
positive sense of the minor axes which itself follows a right hand screw rule with the direction cosines defining
the major axes. The local axes system for the node is then set up form the reference direction and reference
point using the same conventions as for the cartesian axes definition. See Figure 8.

For the toroidal axes system, the major radius may not be zero (instead the OUTP or OUTR systems should be
used). Also if the node under consideration lies on the circular minor axes, the local axes for the node cannot be
defined and the elements containing this node will be skipped.




                                                  Figure 8 OUTT Axes System

See Figure 10 for an example demonstrating the use of the OUTT output axes system.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 1-12
      POST User Manual                                                                                              Introduction



(d)      Beam Axes System - OUTB Command


The new output axes system is assumed to have the X lying tangentially along the beam element. The positive
direction is defined by specifying a reference direction for the output X-axis. The positive direction along the
beam is that which gives an angle in the range of ±90° with the reference direction.

A second reference direction (relating to the Z) is used to complete the output axes system. The new Y is
positioned such that it is mutually perpendicular to the new X and the second reference direction, the direction
forming a right handed set with the reference direction and the new X. Finally the new Z is positioned to form
an orthogonal right handed axes set with the new X and Y.

Example output systems for beam elements are shown in Figure 9.



                                                   Z

                                                                                                        Z Axis
                                                                                                        Reference
                                                                                                        Direction




                                   X                               Y

                                                                                 X Axis Reference Direction

                                                              Z




                                         X




                                             Y




                                                  Figure 9 OUTB Axes System



1.6.4.      Averaging Groups with Differing Output Systems

The AVGR command gives the user the ability to average across group boundaries with differing output axes
systems. This is admissible, but the user must ensure that where the groups meet the local axes systems are
aligned so that averaging is valid.              Figure 10 shows a typical example of where averaging across group




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 1-13
    POST User Manual                                                                                    Introduction


boundaries with differing output axes systems may be used. The structure consists of a cylinder (Group 1 with
output system OUTP), connected to a 90° section of a pipe bend or torus (Group 2 with output system OUTT).
The other end of the bend connects to a second cylinder (Group 3 with output system OUTP). Finally the
second cylinder is closed with a spherical cap (Group 4 with output system OUTR). For each section, the
longitudinal stress is σx and the hoop stress is σy. The through thickness direction for all Groups in the local Z
axis.




                                     Figure 10 Example of Averaging Across Groups



1.6.5.      Material Axes for Laminated Shells

The consistency of the material axes is a requirement for POST since the element strains are converted into the
material axes prior to combination. This is usually satisfied unless different global reference axes have been
defined to set up the material axes on adjacent elements. Figure 11 shows the relationship between global axes,
element local axes, material axes and fibre orientation. Layers are numbered from the bottom surface of the
shell element (on the negative local Z side of the element) towards the top surface.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 1-14
    POST User Manual                                                                                    Introduction




                                                               Figure 11


1.7. Processing of Summed Out-of-Plane Shear Forces for the TRB3 Element

For the TRB3 elements only, the nodal shear value obtained using the FANM command is the sum of the nodal
shear force from all elements surrounding the node. This value is of limited use as it represents the outforce
balancing any external force or reaction at that node and gives little indication of the internal shearing force in
the plate. More useful values are obtained if the nodal shears are summed either side of a line or section defined
by the element boundaries. The section may form a closed loop ie, first and last nodes identical, or may be open
ended.

If the FANM/BANM/AVST and the SECT commands are present in the data, the normal output is augmented by
an extra table. The summed nodal shears on each side of the section are reported for each nodal point on the
section, giving two shear forces at each node. The elements which contribute to each value are also reported.




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 1-15
    POST User Manual                                                                                    Introduction


These shear forces may be interpreted to give a picture of the internal shearing forces at each node on the
section.


1.8. Boundary Conditions for Harmonic Runs

If the harmonic part of the program is used then each ASAS job accessed must have the same element topology
data. Thus, if an analysis was to combine a purely axisymmetric structure (and load) this must be run as a
harmonic job with the geometry property for the harmonic number set to 0.0. To restrain rigid body motions
special suppression data are required for the harmonics 0 and 1. For harmonic 0 at least one TH (θ) degree of
freedom should be removed, to prevent the structure rotating as a rigid body about the Z axis. For harmonic 1
there must be at least one R and one θ degree of freedom suppressed as the displaced shape implied by this
harmonic corresponds to a rigid body motion of the section in the R–θ plane. All harmonics require at least one
Z suppression, but for the harmonics 2 and above there is no need to have any R or θ suppressions to remove
rigid body movements.


1.9. UNITS

If UNITS have been employed in the ASAS analysis it is possible to specify modified units for both the POST
input data and the results. The default units will be those utilised in the original analysis and if this is
satisfactory then no additional information is required in the POST data. Note, however, that the angular data
unit defaults to degrees.

If modified units for input data are required, this is achieved by specifying one or more UNITS commands
within the main body of the POST data thus permitting a combination of unit systems within the one data file
(see Section 2.2 UNITS command).

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

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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 1-16
    POST User Manual                                                                                    Introduction




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 1-17
       POST User Manual                                                                                    Input Data




2.      INPUT Data

As with most of the member programs of the ASAS suite, the input of information and data is divided into two
sections. The first is the Preliminary Data and the second is the POST Data.

The Preliminary Data defines the relationship of the run to all the other runs already completed in the project, the
backing files required, and also specifies the title of the run. If subsequent processing is required after POST, the
data to be saved from the run must also be defined in the Preliminary Data. The full details of these commands,
along with examples, are given in Appendix A- of this manual.

A summary of the POST commands available is given in Table 1. Detailed descriptions of each of the
commands will be found in the remainder of Chapter 2


2.1. General Principles

The input data for POST are specified according to syntax diagrams similar to the one shown below. The
conventions adopted are described in the following paragraphs.




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




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


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               COMB          are all identical strings
                                  Comb
                                  comb


Integer lists are terminated by supplying an END command either on the last line of the integer data, or on the
line immediately after. For example

        GROU                                    is the same as                 GROU
        1    5         6      END                                              1    5         6
                                                                               END

Note that END following immediately after the header line specifies no values. For example

        GROU
        END

In order to reduce the amount of data required, facilities exist to abbreviate the integer lists.

(i)     Where the integer list represents all items from an existing list (for example, choosing all groups for
        processing) the list may be replaced by the word ALL.

                   GROU
                   ALL

        Note that when ALL is utilised, the keyword END is omitted.

        This may not be used where the integer list is to specify new items of information, for example, new
        loadcase numbers.

(ii)    A sequence of integers may be generated by giving the first value and following this with the negative of
        the last value for example 5 -8 generates the numbers 5,6,7 and 8.


If a command is optional, this is shown by an arrow which bypasses the line(s)

            HEADER

            list             END




A data list is indicated by a horizontal arrow around the list variable




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



                     list




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

                        KEYWORD1


                        KEYWORD2




2.1.1.       Special Symbols

The following is a list of characters which have a special significance to the LOCO 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




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


       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
     POST User Manual                                                                                                  Input Data


                                            Table 1 : Summary of Commands


                                          Units Command                                                          Section 2.2
    Command                             Meaning                                   Additional Data           Valid          Note
                                                                                    Required                 For
 UNIT                  Input units definition                         Unit name(s)                         all         1


                                     Data Type Commands                                                          Section 2.3
    Command                             Meaning                                   Additional Data           Valid          Note
                                                                                    Required                 For
  SHELL                 SHELL                                          None                                S
  LAMI                  LAMI type data                                 None                                L
  SBEAM                 Shell BEAM type data                           None                                Sb
  BRICK                 BRICK type data                                None                                B
  AXIS                  AXISYMMETRIC type data                         Data sub-type (on new line)         A
  HARM                  HARMONIC type data                             Data sub-type (on new line)         H
  SOLID                 Data sub-type - SOLID elements                 None                                AH
  SHELL                 Data sub-type - SHELL elements                 None                                AH


                                   Output Axis Commands                                                          Section 2.4
    Command                             Meaning                                   Additional Data           Valid          Note
                                                                                    Required                 For
  CONS                  Consistent local axis system                   None                                Sb          2
                        throughout elements
  OUTP                  Define cartesian output axis                   6 real numbers = 3 direction        S           2
                        system                                         cosines, 3 coordinates
  OUTR                  Define radial output axis system               6 real numbers = 2 sets of 3        S           2
                                                                       coordinates
  OUTT                  Define toroidal output axis system             7 real numbers = 3 coordinates, 3   S           2
                                                                       direction cosines, 1 radius
  OUTB                  Define beam output axis system                 6 real numbers = 2 sets of          Sb
                                                                       direction cosines
  SKEW                  Defines (non orthogonal) x, y,                 2 real angles (degrees)             S
                        directions for Wood-Armer and
                        reinforcement area calculations




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



                                   Group Data Commands                                                          Section 2.5
    Command                             Meaning                                   Additional Data           Valid      Note
                                                                                    Required                 For
  LAYE                  Define laminate layers to be                   Integer list of lamina layers or     L
                        processed                                      ALL
  RDAT                  Define data required for tensile               4 real numbers = 2 design            S         3
                        reinforcement area calculations                stresses, 2 cover depths
  TCRD                  Define data required for                       5 real numbers = 3 design            S         3
                        tensile/compressive reinforcement              stresses, 2 cover depths
                        area calculations


                       Group/Element Selection Commands                                                         Section 2.6
    Command                             Meaning                                   Additional Data           Valid      Note
                                                                                    Required                 For
  GROU                  Selection of specified ASAS                    Integer list of ASAS groups or       all
                        groups                                         ALL
  EXTR                  Selects extra groups of elements               Integer list of user element         all
                                                                       numbers
  SKIP                  Selects elements not to be                     Integer list of element numbers      all
                        considered
  NOAV                  Prevents stress averaging at nodes             None                                 all
  AVGR                  Amalgamates groups for stress                  Integer list of ASAS groups or       all
                        averaging                                      ALL


                         Loadcase Combination Commands                                                          Section 2.7
    Command                             Meaning                                   Additional Data           Valid      Note
                                                                                    Required                 For
  NEWC                  Defines new loadcase numbers                   Integer list of loadcase numbers     all
  ADDC                  Defines loadcases to be used in                Integer list of ASAS loadcase        all
                        creating new loadcases                         numbers
  ADDF                  Defines loadcases with specific                Integer loadcase number followed     all
                        factors used in creating new                   by integer-real pairs for loadcase
                        loadcases                                      number and factor




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



                           Stress Type Selection Commands                                                     Section 2.8
    Command                             Meaning                                   Additional Data         Valid      Note
                                                                                    Required               For
  FACT                  Defines a factor to be applied to              One real factor                    all
                        results
  AVST                  Selects loadcases for processing               Integer list of loadcase numbers   all
                        of averaged stresses                           or ALL
  FANM                  Forces and Moments printout for                Integer list of loadcase numbers   S
                        average stresses                               or ALL
  BANM                  Bending and membrane printout                  Integer list of loadcase numbers   S
                        for average stresses                           or ALL
  PRST                  Selects loadcases for processing               Integer list of loadcase numbers   S Sb
                        of principal stresses                          or ALL                             BAH
  PRVM                  Selects loadcases for processing               Integer list of loadcase numbers   S         4
                        of von Mises stresses                          or ALL
  SHRS                  Selects loadcases for processing               Integer list of loadcase numbers   S
                        of averaged out-of-plane shear
                        forces
  WOOD                  Selects loadcases for processing               Integer list of loadcase numbers   S
                        of Wood-Armer moments                          or ALL
  REIN                  Selects loadcases for processing               Integer list of loadcase numbers   S
                        of reinforcement areas                         or ALL


                                Control Output Commands                                                       Section 2.9
    Command                             Meaning                                   Additional Data         Valid      Note
                                                                                    Required               For
  PRIN                  Selects loadcases for printing                 Integer list of loadcase numbers   all
                                                                       or ALL
  PLOT                  Selects loadcases for plotting                 Integer list of loadcase numbers   all
                                                                       or ALL


                                 Check Stresses Commands                                                   Section 2.10
    Command                             Meaning                                   Additional Data         Valid      Note
                                                                                    Required               For
  FECS                  Defines surface stress allowable               One real stress value              S
  FECM                  Defines mid-plane stress                       One real stress value              S
                        allowable
  VONM                  Defines level of allowable von                 One real stress value              BAH
                        Mises stress
  TRES                  Defines level of allowable Tresca              One real stress value              BAH
                        stress




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




                          Harmonic Combination Commands                                                          Section 2.11
     Command                                Meaning                                      Additional Data          Valid    Note
                                                                                           Required                For
  ANGL                   Defines angular position around                      List of angles                     H         5
                         structure for stress output
  COMB                   Defines number of new loadcases                      One integer value                  H         5
  SELE                   Define new loadcase numbers and titles               List of new loadcase numbers       H         5
                                                                              and titles
  COS                    Selects component loadcases and                      List of component loadcase         H         5
                         defines factors for combined cases                   numbers and factors
                         (even expansion about θ=0°)
  SIN                    Selects component loadcases and                      List of component loadcase         H         5
                         defines factors for combined cases (odd              numbers and factors
                         expansion about θ=0°)


                                   Miscellaneous Commands                                                        Section 2.12
     Command                                Meaning                                      Additional Data          Valid    Note
                                                                                           Required                For
  SECT                   Defines a section across which stresses              Integer list of ASAS group         AS
                         are to be calculated                                 numbers, section numbers and
                                                                              node numbers
  ANGL                   To print the angle of the principal axes             None for SHELL type data.          SH
                         for SHELL type data or define angular                Real list of angular locations
                         location for HARM type data                          for HARM type data
  NAME                   For PATRAN, instructs POST to create                 Name of model to be created        all
                         stress files using the first four                    in PATRAN database e.g.
                         characters of the name followed by a                 MODE
                         unique integer and extension, e.g.
                         MODE0001.NOD MODE0002.NOD
                         etc
  VMPS                   This command defines that von Mises                                                     SB
                         stress is to be calculated from principal                                               AH
                         stresses. If no VMPS command is
                         present the von Mises stress is
                         calculated from average stresses. Not
                         applicable for PATRAN.
 END                    Terminate the run                                                                        all      6


Data types:              S     -    Shell type data                            Sb -       Shell beam type data
                         L     -    Laminated shell type data                  B     -    Brick type data
                         A     -    Axisymmetric type data                     H     -    Harmonic type data




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


Notes


1.       UNIT command may only be used if units have been specified in the preceding ASAS run.

2.       Only one is applicable to a group of elements, however different groups may have different output axis
         within the same run. If none are present then CONS is assumed.

3.       RDAT and TCRD may be used in same run but must apply to different groups.

4.       For shell elements von-Mises stresses are not printed but the PRVM command will cause them to be
         added to the plot file.

5.       For HARM type jobs, these commands must follow the data sub-type command.

6.       Mandatory END command: all other decks are optional subject to note 2


2.2. UNITS Command

Specifies the units associated with subsequent data. This command is only valid if UNITS were employed in the
ASAS analysis (see Section 1.9).

           UNITS                         unit




Parameters

UNITS             : keyword

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

Note


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 of the analysis global units unless previously overwritten by
another UNITS command. The default angular unit is degrees for all data types.

Valid unit names are as follows:

Length                                 METRE(S)                       M
                                       CENTIMETRE(S)                  CM
                                       MILLIMETRE(S)                  MM
                                       FOOT,FEET                      FT
                                       INCH,INCHES                    IN

Force unit                             NEWTON(S)                      N
                                       KILONEWTON(S)                  KN




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


                                       MEGANEWTON(S)                  MN
                                       TONNEFORCE(S)                  TNEF
                                       POUNDAL(S)                     PDL
                                       POUNDFORCE                     LBF
                                       KIP(S)                         KIP
                                       TONFORCE(S)                    TONF
                                       KGFORCE(S)                     KGF

Angular unit                           RADIAN(S)                      RAD(S)
                                       DEGREES(S)                     DEG(S)

The UNITS command may be repeated throughout the data deck thus permitting the greatest flexibility in the
data input.




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



Example


Command                                             Operational Units                                   Notes

SYSTEM DATA AREA 50000
.                                                                                                       UNITS do not have to
.                                                                                                       appear in the Preliminary
.                                                                                                       data, see Section 1.9
UNITS N M                                  NEWTON, METRES, DEGREES                                      and Appendix A-.
.
.
.
END
SHELL                                      NEWTONS, METRES, DEGREES                                     Default global analysis
CONS                                                                                                    units except that angular
GROU                                                                                                    input is in degrees
ALL
AVST
ALL
UNIT MM                                    NEWTONS, MILLIMETRES, DEGREES                                Stress now input in
FECS                                                                                                    N/mm2
200.0
END


2.3. Data Type Commands



2.3.1.      Data Type and Sub-Type Commands

This command defines the type of elements to be processed in the POST run and must be the first command to
follow the preliminary data.




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



                 SHELL

                 LAMI

                 SBEAM

                 BRICK



                                          SOLID
                 AXIS
                                          SHELL
                                          SOLID
                 HARM
                                          SHELL




Parameters

SHELL             : keyword to denote that one or more of the following element types are to be processed:
                              Shell             GCS6, GCS8, TCS6, TCS8, TBC3, QUS4
                              Plate             SLB8, TRB3
                              Membrane          QUM8, QUM4, TRM6, TRM3
                              Sandwich          SND6, SND8, SND12, SND16
                     Only one element type will be processed for each group defined (see Section 1.4)

LAMI              : keyword to denote that laminated shells are to be processed:
                          QUS4, TCS6 and TCS8 elements

SBEAM             : keyword to denote that shell beam elements are to be processed:
                          TCBM or GCB3 elements

BRICK             : keyword to denote that brick elements are to be processed:
                              BRK6, BRK8, BR20, BR32, TET4, TE10 elements

AXIS              : keyword to denote that the axisymmetric elements are to be processed

                     SOLID : subcommand to AXIS to denote that axisymmetric solid elements are to be
                                       processed: TRX3, TRX6, QUX4, QUX8 elements

                     SHELL : subcommand to AXIS to denote that the axisymmetric shell element is to be
                                       processed: ASH2 elements

                  If neither subcommand is given, SOLID is assumed.

HARM              : keyword to denote that the axisymmetric harmonic elements are to be processed.




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


                     SOLID             :    subcommand to HARM to denote that harmonic solid elements are to be
                                       processed:      THX3, THX6, QHX4, QHX8 elements

                     SHELL             :    subcommand to HARM to denote that the harmonic shell element is to be
                                       processed:      AHH2 elements

                     If neither subcommand is given, SOLID is assumed.

Note


All POST runs require either SHELL, LAMI, SBEAM, BRICK, AXIS or HARM as the first command
following the preliminary data; they are mutually exclusive options.


2.4. Output Axis Commands



2.4.1.      CONS Command (SHELL or SBEAM data)

Specifies that the element local axis systems are consistent and that no stress reorientation is required
(see Section 1.6)



          CONS




Parameters

CONS          : keyword


When CONS is specified, any groups referenced by subsequent GROU and EXTR group commands will be
assumed to have consistent local element axis systems until a new output axis system is defined (OUTP, OUTR,
OUTT, OUTB). If no output command is supplied, CONS will be assumed.

Notes


1.       A group may only be assigned one axis system within the same run. Different groups however, may have
         different output axis systems.

2.       This command does not make elements within a group have consistent axes. If they do not already have
         consistent axes in the ASAS model then the CONS command must not be used otherwise invalid stress
         averaging will occur. In this instance one of the alternative output commands (OUTP, OUTR, OUTT,
         OUTB) must be used.

Example




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


         CONS
         GROU
         1    5               END
         EXTR
         10            15     16    17   END




2.4.2.        OUTP Command (SHELL data only)

Defines a cartesian/cylindrical output axis system into which all nodal stresses are to be converted prior to nodal
averaging (see Section 1.6)



             OUTP



             dx               dy              dz               x              y              z




Parameters

OUTP              : keyword

dx,dy,dz : direction cosines of the reference direction with respect to the global axis system. (Real)

x,y,z             : global coordinates of the reference point. (Real)


When OUTP is specified, any groups referenced by subsequent GROU and EXTR group commands will adopt
the output axis system defined by the direction cosines and reference point until a new output axis system is
defined (CONS, OUTR, OUTT, OUTP).

Note


A group may only be assigned one axis system within the same run. Different groups, however, may have
different output axis systems.

Example


         OUTP
         0.7071              0.7071      0.0         10.0          0.0       0.0
         GROU
         1         5        END




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


         EXTRA
         10    15         16        17       END




2.4.3.        OUTR Command (SHELL data only)

Defines a radial/spherical output axes system into which all nodal stresses are to be converted prior to nodal
averaging (see Section 1.6).



           OUTR



           xo               yo                zo               xr             yr             zr




Parameters

OUTR            : keyword

xo,yo,zo : global coordinates of the centre point. (Real)

xr,yr,zr        : global coordinates of the reference point. (Real)


When OUTR is specified, any groups referenced by subsequent GROU and EXTR group commands will adopt
the output axis system defined by the two pairs of coordinates until a new output axis system is defined (CONS,
OUTP, OUTT, OUTR).

Note


A group may only be assigned one axis system within the same run. Different groups, however, may have
different output axis systems.

Example


         OUTR
         1.0        0.0        10.0        1.0         0.0        2.0
         GROU
         1   5         END
         EXTRA
         10       15      16        17       END




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


2.4.4.      OUTT Command (SHELL data only)

Defines a toroidal output axes system into which all nodal stresses are to be converted prior to nodal averaging
(see Section 1.6).



          OUTT



          xc                yc                zc               dx             dy             dz         r




Parameters

OUTT           : keyword

xc,yc,zc : global coordinates of centre of torus (Real)

dx,dy,dz : direction cosines of major axis (Real)

r              : major radius (Real)


When OUTT is specified, any groups referenced by subsequent GROU and EXTR group commands will adopt
the output axis system defined by the specified torus until a new output axis system is defined (CONS, OUTR,
OUTT, OUTP).

Note


A group may only be assigned one axis system within the same run. Different groups, however, may have
different output axis systems.

Example


         OUTT
         100.00         0.0         100.0          0.0        1.0        0.0         25.0
         GROUP




2.4.5.      OUTB Command (SBEAM data only)

Specifies information to determine output axis system for shell beam elements (see Section 1.6)




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




          OUTB



          dxx               dxy               dxz              dzx            dzy            dzz




Parameters

OUTB              : keyword

dxx,dxy,dxz : directions cosines for x-axis reference direction with respect to the global axis system. (Real)

dzx,dzy,dzz : direction cosines for z-axis reference direction with respect to the global axis system. (Real)

When OUTB is specified, any groups referenced by subsequent GROU and EXTR group commands will adopt
the output axis system defined by these direction cosines until a new output axis system is defined (CONS,
OUTB).

Note


A group may only be assigned one axis system within the same run. Different groups, however, may have
different output axis systems.

Example


         OUTB
         0.7071         0.7071           0.0         0.0        0.0        1.0
         GROU
         7   5         END
         EXTRA
         10      15       16        17       END




2.4.6.        SKEW Command (SHELL data only)

Defines the local axes for Wood-Armer moment and reinforcement area calculations.




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




          SKEW


          angx                 angy




Parameters

SKEW          : keyword

angx          : angle that local x axis makes to the output x axis (CONS, OUTP, OUTR or OUTT) (Real)

angy          : angle between local y axis and local x axis. (Real).

Notes


1.       The WOOD/REIN commands normally assume that orthogonal axes are in use. The SKEW command
         allows non-orthogonal axes to be defined.

2.       The angles defined are measured in a conventional right-handed system. The units are degrees.

Example


         SKEW
         22.5          78.5


2.5. Group Data Commands



2.5.1.      LAYE Command (LAMI data only)

Specifies which layers of a laminated shell are to be processed.




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




           LAYE



                           ilay                         END




                            ALL




Parameters

LAYE          : keyword

ilay          : individual layers to be processed

END           : keyword to denote the end of the current block of layer data. If the list of layers continues onto
                subsequent lines, END is required on the last line only.

ALL           : keyword to denote that all layers are to be reported. END not required.

Note


When LAYE is specified, any groups referenced by subsequent GROU and EXTR group commands will have
the layers processed that are defined on this command. If no LAYE command is given then all layers of the
groups selected will be processed.

Example


        LAYE
        1 2 5 6 END
        GROU
        1 2 END
        LAYE
        ALL
        EXTR
        11 1 -20 END




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


2.5.2.      RDAT Command

Specifies details of allowable stresses and cover depths for tensile (only) reinforcement calculations.
For this case it is assumed that all compressive stress is carried by the matrix (e.g. concrete) alone and all the
tensile stress by the reinforcement (e.g. steel) alone.


           RDAT


            rdstrs                mdstrs                  cdeps




Parameters

RDAT          : keyword

rdstrs        : reinforcement design stress (Real)

mdstrs        : matrix design stress (Real)

cdeps         : cover depths (Real)

Notes


1.       If cdeps is omitted the cover depth for all reinforcing will default to 10% of the shell thickness.

2.       If only one cdeps value is specified, this is taken as the cover depth for all reinforcing.

3.       If two cdeps values are specified, these are taken as the top and bottom surface cover depths
         respectively.

4.       If four cdeps values are specified, these are taken as the top X and Y direction cover depths followed by
         the bottom X and Y direction cover depths.

5.       This data applies to any groups of elements defined on subsequent GROU or EXTR commands, until
         superceded by further RDAT or TCRD commands.

6.       RDAT and TCRD may appear in the same run but may not be for the same group of elements.




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




2.5.3.      TCRD Command

Specifies details of allowable stresses and cover depths for tensile/compressive reinforcement calculations.
For this case it is assumed that the tensile stress is carried by the reinforcement (e.g. steel) alone, but the
compressive stress is carried by both the matrix (e.g. concrete) and the reinforcement.


           TCRD


            rdtstr              rdcstr           mdstrs                  cdeps




Parameters

RDAT          : keyword

rdtstr        : tensile reinforcement design stress (Real)

rdcstr        : compressive reinforcement design stress (Real)

mdstrs        : matrix design stress (Real)

cdeps         : cover depths (Real)

Notes


1.       If cdeps is omitted the cover depth for all reinforcing will default to 10% of the shell thickness.

2.       If only one cdeps value is specified, this is taken as the cover depth for all reinforcing.

3.       If two cdeps values are specified, these are taken as the top and bottom surface cover depths
         respectively.




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


4.       If four cdeps values are specified, these are taken as the top X and Y direction cover depths followed by
         the bottom X and Y direction cover depths.

5.       This data applies to any groups of elements defined on subsequent GROU or EXTR commands, until
         superseded by further RDAT or TCRD commands.

6.       RDAT and TCRD may appear in the same run but may not be for the same group of elements.




2.6. Group/Element Selection Commands



2.6.1.      GROU Command

Specifies the ASAS group numbers to be processed by subsequent execution commands (AVST, PRST, SHRS,
WOOD and REIN)

           GROU


                           igroup                       END




                            ALL




Parameters

GROU          : keyword

igroup        : ASAS group number to be processed (Integer). All the group numbers specified must exist
                otherwise POST will stop after data checking.




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


END            : keyword to denote the end of the current block of group number data. If the list of group numbers
                 continues onto subsequent lines, END is required on last line only.

ALL            : keyword to indicate that all groups are selected. END is not required.

Note


If this command is omitted, and provided no extra groups are specified (see Section 2.6.2, EXTR groups) then
all the ASAS groups will be processed by default. If this command is omitted, but extra groups are defined, then
none of the ASAS groups will be processed.

Examples

(i)      To process ASAS groups 1 2 3 4


         GROU
         1     -4     END

(ii)     To process all ASAS groups


         GROU
         ALL

(iii)    To process ASAS groups 1,3,5,7,10,12,14


         GROU
         1      3      5        7
         10     12         14       END




2.6.2.        EXTR Command

Defines new group numbers and assigns elements to the groups for processing by subsequent execution
commands (AVST, PRST, SHRS, WOOD and REIN)



             EXTR



             igroup                  ielem                      END




Parameters




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


EXTR              : keyword

igroup            : group number for new group to be generated (Integer). This group number must be unique
                      and must not exist in the original ASAS analysis.

ielem             : user element numbers to be included in the new group (Integer).

END               : keyword to denote the end of the current block of extra group data. If the list of element
                      numbers continues onto subsequent lines, END is required on last line only.

Note


1.       One extra group is defined by each EXTR group command. Up to 50 groups may be processed at a time.

2.       This command effectively removes the elements from their original ASAS group since an element may
         only be in one group at a time.

3.       EXTR groups may be redefined with different lists of elements in separate runs of POST provided the
         Interface file is not saved from run to run.

4.       Note that if EXTR groups are created in POST, then the CREATE Command should be used on the
         SAVE FEMS line.

Examples

(i)      New group 12 contains elements 7 to 35


         EXTR
         12       7    -35        END

(ii)     New group 5 contains elements 1 to 10 and new group 7 contains elements 11 to 20


         EXTR
         5    1        -10        END
         EXTR
         7      11      12        13       14        15       -20         END




2.6.3.        SKIP Command

Specifies user element numbers which are to be excluded from the analysis.




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




             SKIP



                    ielem                    END




Parameters

SKIP          : keyword

ielem         : user element number to be skipped (Integer)

END           : keyword to denote the end of the SKIP data. If the list of element numbers continues onto
                subsequent lines, END is required on last line only.

Note


1.       This command is used to remove elements from an ASAS group. If the skipped elements need
         processing on their own, the EXTR group command should be used which will remove the elements in
         the extra group from their original ASAS groups.

2.       Up to 500 elements may be skipped.

Example


         SKIP
         1      7      9      END




2.6.4.        NOAV Command

Specifies that no averaging of adjacent element stresses is to be carried out.



             NOAV




Parameters




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


NOAV          : keyword

Notes


1.       By default, nodal stresses of adjacent elements within a group are averaged and reported. For model
         checking it may be useful to manually check the absolute variation from element to element in a
         consistent axis set using this command together with an output axis system definition. (OUTP, OUTR,
         OUTT).

2.       With the NOAV command no thickness checks are carried out to ensure that all elements at a node have
         the same thickness.

3.       This command will require a significantly larger data area (see Appendix A.2) and will produce larger
         results files than usual and thus should be used with care.




2.6.5.       AVGR Command

Specifies a set of group numbers which are to be considered as one single group for the purposes of stress
averaging.

           AVGR

                       igroup                       END



                       ALL




Parameters

AVGR          : keyword

igroup        : group number (Integer). This may be either an ASAS group or one defined in an earlier EXTR
                group command.

END           : keyword to denote the end of the current block of averaged group data. If the list of group
                numbers continues onto subsequent lines, END is required on last line only.

ALL           : keyword to indicate that all groups are selected. END is not required.

Notes

1.       By default, stress averaging only occurs between elements which are in the same group. (See Section
         1.4). There may be situations, however, where groups of elements require different axis sets but stress
         averaging across the group boundaries is both desirable and meaningful (see Figure 10). This may be




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


         achieved by use of the output axis commands (CONS, OUTP, OUTR, OUTT) and AVGR (See Section
         1.6.4).

2.       The results will be reported under the first group number appearing in the list.

Example (see Figure 10)

         OUTP
         0.0 0.0 1.0 0.0 0.0 50.0
         GROUP
         1 END
         OUTT
         50.0 0.0 100.0 0.0 1.0 0.0 50.0
         GROUP
         2 END
         OUTP
         1.0 0.0 0.0 100.0 0.0 150.0
         GROUP
         3 END
         OUTR
         200.0 0.0 150.0 150.0 0.0 200.0
         GROUP
         4 END
         AVGR
         1 2 3 4 END


2.7. Loadcase Combination Commands



2.7.1.      NEWC Command

Specifies the numbers and titles of new loadcases that are to be created using the ADDC and ADDF commands
(see Sections 2.7.2 and 2.7.3 respectively).

                          NEWC


                          new case                END



                          loadcase               `title'




Parameters

NEWC          : keyword

newcase : number of new loadcases to be created (Integer).




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


END           : keyword to denote the end of the current block of new loadcase numbers.                 If the list of new
                loadcase numbers continues onto subsequent lines, END is required on last line only.

For each loadcase defined by newcase

loadcase : loadcase number which must also appear in the newcase list above. (Integer)

title         : title associated with the new loadcase number. (Maximum 40 characters)

Note


The order of the title lines is not important.

Example


         NEWC
         5      7      9      11        END
         5                                         ’FIRST COMBINATION’
         9                                         ’THIRD COMBINATION’
         7                                         ’SECOND COMBINATION’
         11                                        ’LAST COMBINATION’




2.7.2.        ADDC Command

Specifies the constituent loadcases to be added together to form a new loadcase defined in the NEWC command
(see Section 2.7.1).

                    ADDC                         (keyw rd)


                    new case                loadcase                    END




Parameters

ADDC          : keyword

keywrd        : second keyword to define the type of summation to be carried out to the constituent loadcases
                defined on the following line(s). Valid options are:

                SSUM               simple summation (default)
                MAXE               maximum envelope
                MINE               minimum envelope




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


                MXAE              maximum absolute envelope
                ABSS              absolute sum
                SRSS              square root sum square
                REEN              reinforcement calculation envelope
                WDME              Wood-Armer moment envelope



newcase : new loadcase number which must have been defined using the NEWC command. (Integer).

loadcase : existing loadcase number to be used in the creation of the new loadcase (see notes below).
                (Integer)

END           : keyword to denote the end of the current block of constituent data. If the list of loadcase numbers
                continues onto subsequent lines, END is required on last line only.

Notes


1.       The constituent loadcases are factored by the value defined in the latest FACT command.

2.       Either ADDC and/or ADDF commands must be used for each of the new loadcases defined on the
         NEWC command.

3.       The loadcase list may include new loadcases defined on earlier ADDC or ADDF commands.

4.       Appendix D- gives details of summation types.

Example


         ADDC           SSUM
         5       2        -4          END




2.7.3.       ADDF Command

Specifies the constituent loadcases, together with their factors, to be added together to form a new loadcase
defined in the NEWC command (see Section 2.7.1).
                     ADDF                        (keyw rd)

                     new case               loadcase              factor                      END




Parameters

ADDF          : keyword




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


keywrd        : second keyword to define the type of summation to be carried out to the constituent loadcases
                defined on the following line(s). Valid options are:

                SSUM              simple summation (default)
                MAXE              maximum envelope
                MINE              minimum envelope
                MXAE              maximum absolute envelope
                ABSS              absolute sum
                SRSS              square root sum square
                MXLS              maximum limit stress
                MNLS              minimum limit stress
                WDME              Wood-Armer moment envelope
                REEN              reinforcement calculation envelope

newcase : new loadcase number which must have been defined using the NEWC command. (Integer)

loadcase : existing loadcase number to be used in the creation of the new loadcase (see notes below).
                (Integer)

factor        : factor to be applied to the loadcase. (Real) For the MXLS and MNLS two factors per loadcase are
                required.

END           : keyword to denote the end of the current block of constituent data. If the list of loadcase numbers
                continues onto subsequent lines, END is required on the last line only.

Notes

1.       Either ADDC and/or ADDF commands must be used for each of the new loadcases defined as the
         NEWC command.

2.       The use of ‘-’ to indicate a range of integers is prohibited in this command.

3.       The loadcase list may include new loadcases defined on earlier ADDC or ADDF commands.

4.       Appendix D- gives details of summation types.

Example

         ADDF      SSUM
         7 1       1.5 2          0.5        END
         ADDF MXLS
         11 1 1.5             1.0       2    0.5       0.0        END




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


2.8. Stress Type Selection Commands



2.8.1.      FACT Command

Specifies a factor to be applied to the stresses from the loadcases defined by subsequent execution commands
(AVST, PRST, SHRS, WOOD and REIN) or loadcases referred to with the ADDC command.

          FACT


          factor




Parameters

FACT          : keyword

factor        : scaling factor to be applied to subsequent loadcases. (Real)

Note


The factor remains on the selected loadcases until it is overwritten by another FACT command.

The default value is 1.0

Example


         FACT
         105.0




2.8.2.      AVST Command

Specifies the loadcases for which average stresses are to be calculated.
           AVST

                          loadcase                    END


                         ALL




Parameters




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


AVST          : keyword

loadcase : loadcase number to be processed (Integer). This must either appear in the original ASAS analysis
                or be defined in a NEWC command.

END           : keyword to denote the end of the current block of averaged stress data. If the list of loadcase
                numbers continues onto subsequent lines, END is required on last line only.

ALL           : keyword to indicate that all loadcases are selected.

Notes


1.       If AVST and PRST commands are both omitted then the averaged stresses and principal stresses (if
         applicable) will be calculated for all loadcases in the ASAS run.

2.       For BRICK, AXIS and HARM data types, the von Mises equivalent stress is calculated during printing of
         average nodal stresses. The formulae are given in Appendix C-.
         If the von-Mises equivalent stress exceeds the allowable value set by a previous VONM command (see
         Section 2.10.2) the factor by which the allowable value is exceeded is also printed.

Example

(i)             AVST
                1    4         6       END
(ii)            AVST
                ALL



2.8.3.      FANM Command (SHELL data only)

Specifies the loadcases for average stress calculation where FORCES and MOMENTS are required, as opposed
to surface stresses.



           FANM

                       loadcase                       END




                         ALL




Parameters




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


FANM          : keyword

loadcase : loadcase number to be processed. (Integer). This must either appear in the original ASAS
                analysis or be defined in a NEWC command.

END           : keyword to denote the end of the current block of force and moment data. If the list of loadcase
                numbers continues onto subsequent lines, END is required on the last line only.

ALL           : keyword to indicate that all loadcases are selected. END is not required.

Notes


1.       If FANM is specified, the nodal averaged values are output as force/unit length and moment/unit length
         instead of stresses at the top, middle and bottom surfaces.

2.       For TRB3 elements this command will produce summed through thickness shears for each node.

3.       FANM only controls the type of values output. AVST is also needed if nodal averaged values are
         required.

Example


         FANM
         1      3      END




2.8.4.       BANM Command (SHELL data only)

Specifies the loadcases for average stress calculation where BENDING and MEMBRANE stresses are required,
as opposed to surface stresses.



              BANM



                       loadcase                       END



                         ALL




Parameters

BANM          : keyword




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


loadcase : loadcase number to be processed (Integer). This must either appear in the original ASAS analysis
                or be defined in a NEWC command.

END           : keyword to denote the end of the current block of bending and membrane stress data. If the list of
                loadcase numbers continues onto subsequent lines, END is required on the last line only.

ALL           : keyword to indicate that all loadcases are selected. END is not required.

Note


1.       If BANM is specified, the nodal averaged values are output in the form of bending and membrane
         stresses instead of stresses at the top, middle and bottom surfaces.

2.       BANM only controls the type of values output. AVST is also needed if odal averaged values are
         required.

Example


         BANM
         4      -6      END




2.8.5.       PRST Command

Specifies the loadcases for which principal stresses are to be calculated.
             PRST

                     loadcase                       END



                       ALL




Parameters

PRST          : keyword

loadcase : loadcase number to be processed. (Integer). This must either appear in the original ASAS analysis
                or be defined in a NEWC command.

END           : keyword to denote the end of the current block of principal stress data. If the list of loadcase
                numbers continues onto subsequent lines, END is required on last line only.

ALL           : keyword to indicate that all loadcases are selected. END is not required.




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


Notes


1.       If AVST and PRST commands are both omitted then the averaged stresses and principal stresses will be
         calculated for all loadcases in the ASAS run.

2.       During the processing of principal stresses for solid elements (including axi-symmetric) the Tresca stress
         and von Mises equivalent stress are calculated. The formulae are given in Appendix C-.

3.       For SHELL data, P3 is the through thickness stress and is equal to zero, and hence the Tresca stress
         becomes the greater of the P1, P2 or P1 - P2 values. This value of Tresca stress is flagged with an asterisk
         in the printout but not printed separately.

4.       The von-Mises equivalent stress is not printed but if the PRVM command is specified, the value is written
         to the plot file. See Section 2.8.6 and A.12.

5.       PRST may not be used with the SBEAM data type.

Example

         PRST
         5    2        1      END
         PRST
         ALL



2.8.6.      PRVM Command

Specifies the loadcases for which von-Mises equivalent stresses are to be processed.



              PRVM



                       loadcase                       END



                           ALL




Parameters

PRVM              : keyword

loadcase          : loadcase number to be processed (Integer). This must either appear in the original ASAS
                     analysis or be defined in a NEWC command.




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


END               : keyword to denote the end of the current block of von-Mises data. If the loadcase numbers
                     continue onto subsequent lines, END is required on the last line only.

ALL               : keyword to indicate that all loadcases are selected. END is not required.

Notes


1.       This command must be used in conjunction with the PRST command, see section 2.8.5.

2.       The von-Mises stress is not printed for shell elements even when the PRVM command is used.

3.       The PRVM command causes the von-Mises stresses to be written to the plot file.

4.       The formulae used to calculate the von-Mises stress are given in Appendix C-.

Example


         PRVM
         3       7        9         END




2.8.7.       SHRS Command (SHELL data only)

Specifies the loadcases for which average out of plane shear force/unit lengths are to be calculated.



              SHRS



                       loadcase                       END



                         ALL




Parameters

SHRS              : keyword

loadcase          : loadcase number to be processed (Integer). This must either appear in the original ASAS
                     analysis or be defined in a NEWC command.

END               : keyword to denote the end of the current block of SHRS data. If the loadcase numbers
                     continue onto subsequent lines, END is required on the last line only.

ALL               : keyword to indicate that all loadcases are selected. END is not required.




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


Notes


1.       This command should not be used for TRB3 elements which are covered separately by the SECT
         command in Section 2.12.1 (see also Section 1.7)

2.       SHRS only controls the type of values output. AVST is also needed if nodal averaged values are
         required.

Example


         SHRS
         3       7        9         END




2.8.8.       WOOD Command (SHELL data only)

Specifies the loadcase numbers for which Wood-Armer moments are to be calculated. Only valid for SHELL
data and element types GCS6, GCS8, TCS6, TCS8, TBC3, QUS4, SLB8 and TRB3.



              WOOD



                       loadcase                       END



                         ALL




Parameters

WOOD          : keyword

loadcase : loadcase numbers to be processed (Integer). This must either appear in the original ASAS analysis
                or be defined in a NEWC command.

END           : keyword to denote the end of the current list of loadcases. If the list of loadcase numbers
                continues onto subsequent lines, END is required on the last line only.

ALL           : keyword to indicate that all loadcases are selected. END is not required.

Notes


1.       The formulae used for calculating Wood-Armer moments are given in Appendix C-.




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


2.       If Wood-Armer moment envelopes are required, the WDME combination type should be used on an
         ADDC/ADDF command (see Section 2.7.2/2.7.3).

3.       Specifying WOOD for a loadcase will automatically invoke the FANM command, unless BANM has
         been specified, in which case Wood-Armer stresses are produced.

Example


         WOOD
         5       3        END




2.8.9.       REIN Command (SHELL data only)

Specifies the loadcase numbers for which reinforcement areas are to be calculated. Only valid for SHELL data
and element types GCS6, GCS8, TCS6, TCS8, TBC3, QUS4, SLB8 and TRB3.



              REIN



                       loadcase                       END



                         ALL




Parameters

REIN          : keyword

loadcase : loadcase numbers to be processed (Integer). This must either appear in the original ASAS analysis
                or be defined in a NEWC command.

END           : keyword to denote the end of the current list of loadcases. If the list of loadcase numbers
                continues onto subsequent lines, END is required on the last line only.

ALL           : keyword to indicate that all loadcases are selected. END is not required.

Notes


1.       The formulae used for calculating Reinforcement Areas are given in Appendix C-.




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


2.       If reinforcement area envelopes are required, the REEN combination type should be used on an
         ADDC/ADDF command (see Section 2.7.2/2.7.3).

3.       Specifying REIN for a loadcase will automatically invoke the FANM command.

Example


         REIN
         5       3        END


2.9. Control Output Commands



2.9.1.       PRIN Command

Specifies which loadcases are to be printed. Only loadcases that are processed may be printed (AVST, PRST,
SHRS, WOOD and REIN commands).



             PRIN

                       loadcase                       END




                         ALL




Parameters

PRIN          : Keyword

loadcase : loadcase number to be printed. (Integer)

END           : keyword to denote the end of the current block of print data. If the list of loadcase numbers
                continues onto subsequent lines, END is required on the last line only.

ALL           : keyword to indicate all loadcases are selected. END is not required.

Notes


1.       By default all loadcases that are processed will be printed.




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


2.       The PRIN command must only be used with a SAVE plot FILE command (see Appendix A.12). In this
         case, all cases processed will be written to the plot file.

Example


To print loadcases 5 and 6 only

         PRIN
         5      6      END

To suppress printing of all the loadcases

         PRIN
         END




2.9.2.       PLOT Command

Used to specify which loadcases are to be saved for processing with any valid plotting program. Only loadcases
that are processed may be plotted (AVST, PRST, SHRS, WOOD and REIN commands). A SAVE plot FILE
command must be supplied in the preliminary data if plotting is required (see section A.12).



             PLOT

                       loadcase                       END




                         ALL




Parameters

PLOT           : keyword

loadcase : loadcase number to be saved for plotting. (Integer)

END            : keyword to denote the end of the PLOT data. If the list of loadcase numbers continue onto
                 subsequent lines, END is required on the last line only.

ALL            : keyword to indicate that all loadcases are selected. END is not required.




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


Notes


1.      If the PLOT command is omitted then all loadcases that are processed will be saved for plotting if a
        SAVE plot FILE command has been supplied, otherwise none is saved.

2.      If the PLOT command is used and no SAVE plot FILE command has been specified, the program will
        terminate after reading the data.

Example


Cases 1,2,3,6,7 and 8 will be added to the plot file.

        PLOT
        1     2    3    6     -8      END

All loadcases processed will be added to the plot file.

        PLOT
        ALL

No results will be added to the plot file.

        PLOT
        END


2.10. Check Stresses



2.10.1. FECS and FECM Commands (SHELL data only)

Specifies an effective surface or membrane stress to be used as the check stress to be applied to subsequent
average and principal stress calculations.
                   FECS


                   FECM

                   stress




Parameters

FECS          : keyword to denote that an effective surface stress is to be defined.

FECM          : keyword to denote that an effective membrane stress is to be defined.




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


stress        : check stress. (Real). A value of zero implies no checking.

Note


If the FANM command is in operation for any of the loadcases then no stress checking will be carried out.

Example


               Command                                                  Current Check Stress Values

          AVST                                                    FECS                                  FECM
          6 END                                                    0.0                                   0.0
          FECM
          150.0
          AVST
          1     2    END                                           0.0                                  150.0
          FECS
          200.0
          PRST
          5 END                                                  200.0                                  150.0




2.10.2. VONM Command

Specifies a user defined von Mises stress level against which the calculated von Mises stresses will be checked,
for loadcases defined by subsequent AVST and PRST commands.



          VONM


          stress




Parameters

VONM          : keyword

stress        : von Mises stress check value (Real). A value of zero implies no checking




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


Note


The stress check value remains for selected loadcases until it is overwritten by a subsequent VONM command.

Example


        VONM
        5.0




2.10.3. TRES Command

Specifies a user defined Tresca stress level against which the calculated Tresca stresses will be checked, for
loadcases defined by a subsequent PRST commands.



          TRES


          stress




Parameters

TRES          : keyword

stress        : Tresca stress check value (Real). A value of zero implis no checking.

Note


The stress check value remains for selected loadcases until it is overwritten by a subsequent TRES command.

Example


        TRES
        10.0




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


2.11. Harmonic Combination Commands



2.11.1. Data for Harmonic Analyses

If a Fourier series type of analysis is being carried out on the harmonic solid elements, THX3, QHX4, THX6 and
QHX8, data must be defined for the constituent structures and loadcases (see Section 1.2.5). The following
commands provide this additional information and must follow the HARM and BRICK / SHELL command.



                         ANGL


                         angl                   END



                         COMB                   numcomb



                         SELE                   new case                     title


                         STRUCTURE                        struct



                         COMPONENT                        struct              tree


                              COS


                              SIN

                           loadcase             factor


                          END




Parameters

See following sections for details of each command.




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


Note


The harmonic combination commands must be omitted in a harmonic re-run and the loadcase details will be
obtained from the previously saved files.




2.11.2. ANGL Command (HARM Data only)

Specifies the angular positions around the structure at which stress output is required.


                      ANGL


                       angle                 END




Parameters

ANGL          : keyword

angle         : angle at which results are required. (Real)

END           : keyword to denote the end of the angle data.

Notes


1.      A maximum of 50 angular stations are permitted.

2.      Continuation lines are permitted, the END appearing at the end of the last continuation line.

3.      The ANGL command is compulsory for all HARM data files and must be the first data after the HARM
        BRICK / SHELL data type commands.

Example


        ANGL
          20.0         33.0       42.0       57.0        30.0       END




2.11.3. COMB Command (HARM data only)

Specifies the number of harmonic combinations which are to be created by this run.




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




          COMB                 numcomb




Parameters

COMB              : keyword

numcomb           : number of harmonic combinations to be created. Must be 9 or less. (Integer)

Note


The COMB command must immediately follow the last ANGL command

Example


         COMB 3




2.11.4. SELE Command (HARM data only)

This command identifies the combination number and title to be associated with the harmonic combination
created by the subsequent commands.



          SELE                 combno                 ’title’




Parameters

SELE          : keyword

combno : user combination number for this case (Integer)
                This value must be 9 or less (see note below).

title         : combination title, up to 40 characters.




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


Notes


1.      The combination number specified on the SELE command line is used in conjunction with the specified
        angular positions to generate internal loadcase numbers for reporting results.

2.      The combination number defined on the SELE command is multiplied by 1000 and added to the integer
        angle of a station (in degrees) to arrive at a representative loadcase number. For example,

                if the SELE command defines a new combination 5 and angles of 20.0, 32.0 and
                47.0 degrees have been specified on the ANGL command, the following internal
                loadcases will be generated:- 5020, 5032 and 5047.


3.      There must be as many SELE commands supplied as the number defined on the COMB command.

Example


        SELE       2    ’CASE 7 HARMONIC 0 + CASE 5 HARMONIC 2’




2.11.5. COS and SIN Commands (HARM data only)

Specifies constituent loadcase numbers and factors to be used in the generation of a harmonic combination,
together with optional information defining the structure or component to which the loadcases are relevant.



                            STRUCTURE                        struct



                            COMPONENT                        struct               tree


                                 COS


                                 SIN

                              loadcase             factor


                           END




Parameters

STRUCTURE :                   keyword




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


struct            : 4-character ASAS structure name identifying which structure within the current project is to be
                       accessed

tree              : this is the path down the component tree from the given structure in sname to the component
                       being used for the POST combinations. If processing a global structure run from a multilevel
                       analysis, i.e. the component tree is not required, use the STRUCTURE command instead.

COS               : keyword to indicate that the loadcases selected are symmetrically expanded about the reference
                       direction (θ=0.0), i.e. the loading is maximum at θ=0.0)

SIN               : keyword to indicate that the loadcases selected are antisymmetrically expanded about the
                       reference direction (θ=0.0), i.e. the loading is maximum at an angle of θ=π/2n, where n is the
                       harmonic number

loadcase          : constituent ASAS loadcase number (Integer)

factor            : factor by which the constituent loadcase is to be multiplied (Real)

END               : keyword to denote the end of the current block of constituent loadcase information. Required
                       on the last COS or SIN command for the current SELE command.

Note


If all the constituent load information is from one ASAS run, i.e. as defined in the Preliminary data, the
COMPONENT and STRUCTURE commands are unnecessary. If the loadcase information is drawn from
more than one component or structure, the appropriate command should precede the relevant COS or SIN
command. Having specified the STRUCTURE or COMPONENT in this way, POST will continue to draw
information from the loadcase selection commands accordingly. To avoid ambiguities it is recommended that
the STRUCTURE or COMPONENT commands be defined explicitly at all times.

Example


Loadcases 1, 2 and 3 are taken from the assembled component defined in the Preliminary data. To these are
added loadcases 5 and 7 from assembled component CMP9 of structure WQH2.

         SELE      6     COMBINED LOADCASE
         COS
         1 1.3           2        2.4
         SIN
         3 -2.3
         COMPONENT WQH2 CMP9
         SIN
         5 1.0
         COS
         7 2.0
         END




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


2.12. Miscellaneous Commands



2.12.1. SECT Command

Specifies a section across which stresses are to be calculated and printed for the loadcases defined with the
AVST command. This command is only valid for AXIS type jobs or to process summed out of plane shears for
TRB3 elements (see Section 1.7).
                   SECT

                          igroup                       sectid                    END


                          sectid                      nodenm                     END




Parameters

SECT          : keyword

igroup        : the ASAS group number across which the sectional stresses are to be calculated (Integer).

sectid        : identifying number for each section defined across the ASAS group.

nodenm : node numbers defining the section. (Integer).

END           : keyword to denote the end of the current block of data. If the list of node numbers continues onto
                 subsequent lines, END is required on last line only.

Notes


1.      For each section identifier defined on the igroup line, there must be a related sectid line.

2.      Up to 17 nodes may be specified across a section. These nodes should form a ”straight” line although
        they do not necessarily have to follow the edge of an element (the section may pass diagonally across
        elements). The nodes defining a given section must be in the same order as the nodes across the ASAS
        model.

3.      Each section may be at any angle to the global axis system. A new reference plane, defined by the first
        and last nodes in the list, will be calculated for each section. All averaged nodal stresses are then
        resolved normal and parallel to this plane before the member components are evaluated.

Example

Three sections are to be numbered 22, 23 and 24, taken across ASAS group number 2.
Section 22 has nodes 1, 8, 9, 10 and 14 across it




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


Section 23 has nodes 11, 18, 19, 20 and 24 across it
Section 24 has nodes 21, 28, 30, 34 and 29 across it

        SECT
        2    22         -24        END
        22 1             8         9   10            14       END
        23 11            18        19
             20          24        END
        24 21            28       30   34            29       END



2.12.2. ANGL Command (SHELL data only)

Requests output of the direction of first principal stress instead of (P1 - P2)



          ANGL




Parameters

ANGL          : keyword

Notes


1.      If present, the angle of the first principal stress measured from the output x-axis is reported instead of the
        principal stress difference (P1 - P2).

2.      This command should not be confused with the ANGL command in a HARM run. (See Section 2.11.2)




2.12.3. END Command

Specifies the end of the data. This command must be present.



             END




Parameters

END           : compulsory keyword




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




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 2-51
     POST User Manual                                                                                     Examples




3.     Examples


3.1. Example 1: Default Data

This example shows the minimum of data necessary to run POST.

The preliminary data defines the space required (30000 words), the project name and the ASAS results to be
processed (LVW1, a single level analysis), a title and the option GOON (to prevent termination if any warnings
are issued).

Two POST commands are used: SHELL to indicate that the shell elements of LVW1 are to be processed and
END to denote the end of the post data. For this particular example it is assumed that the local axes of the shell
elements are consistent. POST will also make this assumption and print a warning which necessitates the
GOON option in the preliminary data. Similar default data may be used for each of the POST data types by
substituting the appropriate data type keyword.

POST will process all loadcases and print average and principal stresses. No files will be saved for plotting.

       SYSTEM DATA AREA 30000
       PROJ LVW1
       JOB POST
       TITLE POST PROCESSING FOR LVM MODEL
       OPTION GOON END
       END
       SHELL
       END


3.2. Example 2: Simple Shell Result Processing

This example shows the data file for running POST after a single level ASAS analysis. The structure name to be
accessed is SBSS from project SBSS. As the elements within each group are all aligned similarly with regard to
the global axes, the CONS option is selected. Elements from Groups 1, 3, 5, 6, 7 and 9 are to be processed. The
mid-plane check stress is 50.0 and the surface check stress is 75.0. The average stresses and principal stresses
are to be processed for user loadcases 1, 3, 7 8, 9, 10, 11 and 14. The average stresses and principal stresses are
to be printed for user loadcases 1 and 10. All processed stresses will be written to a FEMVIEW file with default
filename SBSSFS and default model name SBSS.

       SYSTEM DATA AREA 35000
       PROJ SBSS
       JOB POST
       TITLE EXAMPLE ILLUSTRATING SHELL DATA
       STRUCTURE SBSS
       OPTIONS END




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


       SAVE FEMS FILES
       END
       SHELL
       CONS
       GROU
       1 3 5 -7 9 END
       FECM
       50.0
       FECS
       75.0
       AVST
       1 3 7 -11 14 END
       PRST
       1 3 7 -11 14 END
       PRIN
       1 10 END
       END


3.3. Example 3: Simple Axi-symmetric Result Processing

This example shows the data deck for running POST after a single level ASAS analysis. The structure to be
accessed is named is ROTA. Elements from Groups 1, 3, 5, 6, 7 and 9 are to be processed. The von Mises
check stress is 50.0 and the Tresca check stress is 75.0. The average stresses for all loadcases are to be
processed, and principal stresses for user loadcases 1, 3, 7, 8, 9, 10, 11 and 14. The average stresses and
principal stresses are to be printed for user loadcases 1 and 10. All processed stresses will be written to a
FEMVIEW file called ROTA.FVI with a model name ROTOR.

       SYSTEM DATA AREA 35000
       PROJ ROTA
       JOB POST
       TITLE EXAMPLE ILLUSTRATING AXIS DATA
       STRUCTURE ROTA
       OPTIONS END
       SAVE FEMS FILES CREATE ROTOR FILE ROTA.FVI
       END
       AXIS
       GROU
       1 3 5 -7 9 END
       VONM
       50.0
       TRES
       75.0
       AVST




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


       ALL
       PRST
       1 3 7 -11 14 END
       PRIN
       1     10      END
       END


3.4. Example 4: Post Processing Component Results from Multi Level Axisymmetric
     Analysis

This example considers elements in component MLS1 which has been assembled into structure MLST.
Elements in groups 1, 3 and 5 are selected. One section (numbered 19) is taken from ASAS group 1 on a plane
defined by nodes 28 and 49 and passing through nodes 29, 30 and 48. Averaged stresses will be printed for
loadcases 1, 4, 5, 6 and 7.

Next an extra group, number 15, is formed of user elements numbered 31 to 36, 40 and 62 to 70. This extra
group has von Mises and Tresca check stress levels of 25.0 and 37.5 and the averaged stresses will be printed for
loadcases 2, 3, 8, 9 and 10.

       SYSTEM DATA AREA 40000
       PROJECT MLPJ
       JOB POST
       TITLE AXIS DATA WITH EXTRA GROUP
       STRUCTURE MLST
       COMPONENT MLST MLLB MLS1
       OPTIONS END
       END
       AXIS
       GROU
       1 3 5 END
       SECT
       1 19        END
       19 28 29 30 48 49 END
       AVST
       1 4 5 -7 END
       EXTRA
       15 31 -36 40 62 -70 END
       VONM
       25.0
       TRES
       37.5
       AVST
       2 3 8 -10 END
       END




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


3.5. Example 5: Loadcase Combinations

This example considers elements in component MLS1 which has been assembled into structure MLST. The
elements considered do not all have consistently oriented local axes and hence the OUTP and OUTR commands
are given to define new output axis systems. Firstly a cartesian output axis system is defined using the OUTP
command. This will then be used for elements in groups 1 3 and 5. A new radial output system is then defined
using the OUTR command. This will then be used for the elements which are defined as a new group using the
EXTR command and also for elements in groups 2 and 4. The new group will be group 16 consisting of
elements 75 to 80 and 82. In all these groups user elements numbered 37 to 39, 43 to 47 and 51 to 53 are to be
omitted from the calculations. Mid-plane and surface check stresses of 50.0 and 75.0 are set and the averaged
stresses and principal stresses will be printed for loadcases 1, 4, 5, 6 and 7.

Next the output axis system is set back to consistent axes using the CONS command, and a new extra group,
number 15, is formed of user elements numbered 31 -36, 40 and 62 -70. This extra group has mid-plane and
surface check stress levels of 25.0 and 37.5. Two new loadcases are formed, 101 by adding together cases 1 and
4 and factoring by 1.05 and 102 by adding case 4 factored by 1.25 and case 6 factored by -0.5. The averaged
stresses will be printed for loadcases 2, 3, 8, 9, 10 and 101. Note, the FACT command is used to reset the factor
to 1.0 before printing.

       SYSTEM DATA AREA 40000
       PROJECT MLPJ
       JOB POST
       TITLE         SHELL DATA WITH EXTRA GROUPS AND OUTPUT COMMANDS
       STRUCTURE MLST
       COMPONENT MLST MLLB MLS1
       OPTIONS END
       END
       SHELL
       OUTP
       0.5       0.8660           0.0        25.0         0.0         0.0
       GROU
       1 3 5 END
       OUTR
       1.0         0.0        10.0         1.0         0.0        2.0
       EXTRA
       16 75 -80              82 END
       GROU
       2    4        END
       SKIP
       37 -39 43 -47 51 -53 END
       FECM
       50.0
       FECS
       75.0




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


       AVST
       1 4 5 -7 END
       PRST
       1 4 5 -7 END
       CONS
       EXTRA
       15 31 -36 40 62 -70 END
       FECM
       25.0
       FECS
       37.5
       NEWC
       101 102 END
       101       COMBINATION OF CASE 1 AND 4
       102                 COMBINATION OF CASE 4 AND 6
       FACT
       1.05
       ADDC
       101 1           4    END
       ADDF
       102 4           1.25       6     -0.5       END
       FACT
       1.0
       AVST
       2 3 8 -10 101 END
       END


3.6. Example 6: Post Processing Harmonic Analyses

This data file runs POST for a HARMonic analysis. One new loadcase is generated which is just case 1, with an
antisymmetric expansion about θ=0, of STRUCTURE WQH1. Stress output is generated for angle θ=20° only.
Note, this will have loadcase 5020 on its printout.

       SYSTEM DATA AREA 60000
       PROJ WQX8
       JOB POST
       FILE WHHH
       TITLE                   SIMPLE HARMONIC EXAMPLE
       STRUCTURE WQH1
       NEWSTRUCTURE WHHH
       OPTIONS END
       SAVE FEMS FILES
       END




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


       HARM
       ANGL
       20.0 END
       COMB 1
       SELE 5 LOADCASE 1 of WQH1
       STRUCTURE WQH1
       SIN
       1 1.0
       END
       END


3.7. Example 7: Harmonic Combinations

This example produces two new loadcases (5, 6) from the stress results from structures WQHO, WQH1, WQH2,
WQH3, and WQH4. Output is requested at angles 20, 30, 40, 50, 60, 70, 80, 90, 100, 110 and 120 degrees. The
output will refer to loadcases 5020, 5030, 5040 ..... 5110, 5120, 6020, 6030 .... 6110, 6120. Each combined
loadcase accesses each structure and more than one loadcase from each original structure. As no PRST or
AVST command appears, the output will include both principal and average stress results.

       SYSTEM DATA AREA 60000
       PROJ WQX8
       JOB POST
       FILE WHHH
       TITLE                          FULL HARMONIC EXAMPLE
       STRUCTURE WQHO
       NEWSTRUCTURE WHHH
       OPTIONS END
       END
       HARM
       ANGL
       20.0 30.0 40.0 50.0
       60.0 70.0 80.0 90.0
       100.0 110.0 120.0 END
       COMB 2
       SELE   5 1ST COMBINED LOADCASE
       COS
       2 1.0 3 1.0
       STRUCTURE WQH1
       COS
       2 1.0         3 1.0
       STRUCTURE WQH2
       COS
       2 1.0 3 1.0




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 3-6
     POST User Manual                                                                                           Examples


          STRUCTURE WQH3
          COS
          2 1.0 3 1.0
          STRUCTURE WQH4
          COS
          2 1.0 3 1.0 END
          SELE 6 2ND COMBINED LOADCASE
          STRUCTURE WQHO
          COS
          1 1.0 2 1.0 3 3.0
          STRUCTURE WQH1
          COS
          1 1.0 2 2.0 3 3.0
          STRUCTURE WQH2
          COS
          1 1.0 2 2.0 3 3.0
          STRUCTURE WQH3
          COS 1 1.0 2 2.0 3 3.0
          STRUCTURE WQH4
          COS 1 1.0 2 2.0 3 3.0 END
          END
          END


3.8. Example 8: Post Processing Shell Compatible Beams

This example shows the data for running POST after an ASAS analysis which includes shell BEAM elements
(TCBM or GCB3). It is assumed that all the beam elements in groups 1 2 and 3 have consistent local axis and
that the user wishes to have the moments/forces reported in the element local axis.

Groups 4, 5 and 6 are to be reported in a new output axis system defined by the preceding OUTB command.

Three new loadcases have been formed. The first two have the same combination factors, one representing the
positive (or maximum) limit stress value, the second the negative (or minimum) limit stress value. The third
new loadcase takes the first two new cases and finds the absolute envelope, giving the overall worst absolute
values.

Finally the forces/moments for all loadcases are to be printed out. Since a SAVE FEMS FILES command is
present in the preliminary deck, all results will be saved for plotting in FEMVIEW. Since APPEND is specified,
no model data (coordinates and element definitions) will be added to the plot file.                     If the plot file
STIFFNER.FVI already exists the results will be appended to it. If not then the new STIFFNER.FVI file can be
read into FEMVIEW if the model data already exists for model STIFNR.

          SYSTEM DATA AREA 35000
          PROJECT STIF
          JOB POST




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.       Page 3-7
     POST User Manual                                                                                     Examples


       TITLE EXAMPLE ILLUSTRATING SBEAM DATA
       STRUCTURE STIF
       OPTIONS END
       SAVE FEMS FILES APPEND STIFNR FILE STIFFNER.FVI
       END
       SBEAM
       CONS
       GROU
       1 2 3 END
       OUTB
       0.0 1.0 0.0 0.0 0.0 1.0
       GROU
       4 5 6 END
       NEWC
       101 102 103 END
       101 MAXIMUM LIMIT STRESS CASE
       102 MAXIMUM LIMIT STRESS CASE
       103 MAXIMUM ABSOLUTE ENVELOPE OF CASES 101 & 102
       ADDF MXLS
       101 1 1.3 1.0 2 1.0 1.0 3 1.3 -1.3 END
       ADDF MNLS
       102 1 1.3 1.0 2 1.0 1.0 3 1.3 -1.3 END
       ADDC MXAE
       103 102 101 END
       AVST
       ALL
       END


3.9. Example 9: Post Processing Laminated Shells

This example shows the data deck for calculating laminate layer stresses with POST following an ASAS analysis
using laminated shells. For the ASAS groups 1 and 2 only the stresses of layers 1, 2, 5 and 6 are to be reported
(these may be the top and bottom two layers of the composite section). In addition a new group (group 11) has
been formed from elements 1 to 20 for which all the layers are to be processed. Finally a new loadcase has been
formed consisting of the summation of ASAS loadcases 1 and 2.

        SYSTEM DATA AREA 35000
        PROJECT COMP
        JOB POST
        TITLE EXAMPLE ILLUSTRATING LAMI DATA
        OPTION GOON END
        SAVE FEMS FILES
        END
        LAMI
        LAYE




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 3-8
     POST User Manual                                                                                     Examples


       1 2 5 6 END
       GROU
       1 2 END
       LAYE
       ALL
       EXTR
       11 1 TO 20 END
       NEWC
       101 END
       101 LOADCASE 1 + LOADCASE 2
       ADDF
       101 1 1.0 2 1.0 END
       END




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 3-9
     POST User Manual                                                                                      Examples




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 3-10
     POST User Manual                                                                                           Output




4.       Output

Three forms of output are available from POST, the printed stress output, a backing file that may be used for
further post-processing, and the sequential files required as input for a variety of proprietary plotting packages.


4.1. Printed Output

The printed output consists of the data check, followed by the stress output, listed group by group. Within each
group the average surface stresses and also the principal stresses are listed if requested for each loadcase in turn.
The exact form of the output will depend on the type of data being analysed, and is discussed in further detail in
the subsequent sections of this manual.




4.1.1.      SHELL Data

The average surface stresses are printed for the top, bottom and mid-surfaces of the element (as defined in
Section 2.1). These stresses are given in terms of the output axis system, as defined by the OUTP or OUTR
commands, or the local element axis system in the case of consistent axes. This set of output also includes the
number of elements contributing to the nodal average and the maximum variation in stress at the particular node.
The variation shows the user the level of the stress difference between adjacent elements at the same node and
also indicates on the accuracy of the overall stresses. In the cases of high variation compared to averaged
stresses, the accuracy of the model should be checked.

The in-plane principal stresses P1 and P2 together with the principal stress difference (P1 and P2) are printed for
each of the three surfaces. Two check stresses are also printed at the head of each page of principal stress
output. These are the mid-plane (membrane) and the surface (membrane plus bending) stress allowables FECM
and FECS respectively, and are defined by the user for the particular loadcase. At each node the ‘effective’
stress on each of the three surfaces is checked against the allowable stress - that is the top and bottom surface
effective stresses are compared with FECS and the mid-surface effective stress is compared with FECM. The
maximum of the surface stress ratios and the mid-plane stress ratio are printed only for values greater than unity
under columns headed FECS and FECM respectively.

In the above, the effective stress is the Tresca stress σT where:

                σT = max. absolute of P1, P2, (P1 - P2)


Asterisks are used throughout the printout to highlight maximum values of P1, P2, (P1, - P2) and the stress ratio.

The backing file, when saved, contains the information required to plot the stress contours for both principal
stresses and averaged nodal stresses for each loadcase of every group considered in the POST run.

If the user has specified some of the options (BANM, FANM, WOOD) which produce SHELL output with
forces and/or moments instead of the surface stresses the same procedures are followed as described above. The




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


principal and average values will, however, relate to the net section forces and moments rather than to individual
surface stresses. If the SHRS command is used, only the out-of-plane shear forces are reported.




4.1.2.      LAMI Data

The direct stresses in the fibre direction and to the normal fibre direction and the inshear stresses are presented
for each of the layers requested at each node on a group basis.




4.1.3.      Shell BEAM Data

The results for shell beams are presented as forces and moments in the output axis system defined by the OUTB
command, or the local element axis in the case of the CONS command. In addition to the forces and moments, a
variation value is printed giving an indication of the force/moment variation at a node common to two or more
elements.




4.1.4.      BRICK, AXIS and HARM Data

The average nodal stress output gives the direct stress in the three global directions and also the three shear
stresses in these directions. The von Mises stress is also calculated and listed for each node. The user defined
allowable stress is listed at the top of each page of output; where it is exceeded the ratio of the von Mises stress
to the allowable is printed in the ‘EXCESS’ column.

The principal stress output gives the three principal stresses at each node and also the sum of the principal
stresses and their direction cosines or principal angle. (For AXIS data, the hoop stress σHH is a principal stress).
The von Mises and Tresca stresses are also printed for each node. The Tresca stress is checked against the user
defined allowable which is printed at the top of the page. When the allowable is exceeded the ratio of the Tresca
stress to the allowable is printed in the ‘EXCESS’ column.


4.2. Backing Files

The backing file, or intermediate file, is used within POST to temporarily save data that will be written to a plot
file or used in loadcase combination/enveloping. It contains information on both the form of the model (nodes,
elements groups etc) and calculated stress results. For this reason it is a useful file if further processing of results
is to be undertaken. If it is required then it may be saved using SAVE INTE FILE in the preliminary deck. The
saved file will be called XXXX12 where XXXX is the 4 character structure name.

If a subsequent run of POST is made on the same structure and an intermediate file is found to exist then post
will try to append data from the current run. Before it can do this it has to check for any inconsistencies on the




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 4-2
    POST User Manual                                                                                            Output


intermediate file with the current run. Such inconsistencies include different element groupings and conflicting
loadcase numbering. In this event the current run would be terminated.

In some cases it is desirable to overwrite an existing intermediate file rather than append to it. This can only be
achieved by using SAVE NEWP FILES in the preliminary data. It is not recommended to delete the old
intermediate file, since its existence is determined from the project index file not its physical existence, hence
deleting the 12 file will require you to re-run in order to correct the project file referencing.

If the RESU command is specified in the preliminary data, the results from POST will be saved to a file called
XXXX45.


4.3. Plotting Program Input

This section describes the contents of the file(s) produced by POST for input to different plotting packages.




4.3.1.      FEMVIEW Input

FEMVIEW uses a formatted file that is created when the SAVE FEMS FILES command is present in the
preliminary data. By default the file will be saved as nnnnFS where nnnn is the four character backing file
name. This may be overridden by specifying a file name explicitly on the SAVE FEMS FILES command
(Appendix A-).

The exact format of the FEMVIEW file is described in detail in the FEMGEN/FEMVIEW user documentation
(Appendix B-). This section will only give a brief overview of the file format, sufficient for the user to be able
to understand the data within it. The data is divided into a series of ‘data decks’, each of which begins with a
header line and a terminator line (consisting of -3 only). The first number on the header line defines the type of
data that follows. The following are used in the POST created file:

                  1      -        user header defining model name (no corresponding terminator line)
                  2      -        nodal coordinates
                  3      -        element connectivity
              100        -        results data
             9999        -        end of data file


If APPEND is defined in the SAVE FEMS command then data types 2 and 3 will not be written. These may
already be in the file to which the data is being appended. The data type number is followed by either C (for
create, if model data present) or A (for append, no model data present). On the user header line this is followed
by the model name to be used by FEMVIEW. By default this is the four character backing file name, but may be
defined explicitly on the SAVE FEMS FILES command. Note that if EXTR groups are created in POST, then
the CREATE Command should be used on the SAVE FEMS line.

The nodal coordinate data and element connectivity are self explanatory except that on the elements the group
number is output in place of the material number required by FEMVIEW. The reason for this is that POST




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


averages stresses on a group basis and so a node may have different stresses for each of the groups, which can
only be accommodated by FEMVIEW by material based nodal results. This has repercussions throughout the
ASAS suite of programs, the material and group numbers being swapped over to maintain compatibility with
POST.

The results data header is followed by a loadcase name, made up of ‘L’ followed by the loadcase number, and
the loadcase title truncated to 20 characters. This is followed by further headers that give the name of the results
set, the type of results, and the names of each component of the results. Two basic results types are used,
material based nodal results and element nodal results, the latter being used only for the SBEAM results. Where
the results are in the global axes system they are written in a matrix form allowing FEMVIEW to calculate
principal stresses and present vector diagrams of principal stresses. For multi-surface results (e.g. shell/plate
stresses), the results are written from bottom surface to top surface. Thus, surface 1 is the bottom surface.




4.3.2.      PATRAN® Input

PATRAN® displays any defined stresses at each node. In POST stresses are calculated on an element group
basis and, therefore, any node lying on a boundary between two or more element groups can have more than one
set of stresses. To overcome this problem each element group is output to a separate file generated by POST.
Two files per group are generated, the first containing average stresses, the second containing principal stresses.

SBEAM result cannot be plotted in PATRAN®.


4.3.2.1. The PATRAN® Results File

Each PATRAN® Results file generated by POST is assigned a different file name. This file name is made up
from the first 4 characters given on the line following the NAME command. Appended to this is a 4 digit integer
starting at 0001 and increment by 1 for each file output. Finally, the 4 characters .NOD are added to indicate
that the values are nodal stresses.

The type of stress contained in any file, average or principal, is indicated in the title record on the file. This title
is also printed in the POST output together with the corresponding file name.

The structure of the PATRAN® input file depends upon the stress output requested. The file is written as binary
or formatted depending on the save option PATN or PTNC.

Record 1                      85       Words
for non-lamina              1-80       Title (First byte of each word only - A1 format)
stresses                      81       No. of nodes in the group (NNOG)
                           82-84       Dummy
                              85       No. of stresses on each record (NST)

Record 1              85               Words
for lamina 1-7 ‘ GROUP ’




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.      Page 4-4
    POST User Manual                                                                                        Output


stresses                    8-12       Group number
                           13-23       ‘ LOAD CASE ’
                           24-28       Loadcase number
                           29-48       ‘ LAMINA        STRESS ’
                           49-53       No. of layers
                           54-80       Dummy
                              81       No. of nodes in the group (NNOG)
                           82-84       Dummy
                              85       No. of stresses on each record (NST=3 x No. of layers)

Record 2                       80           Words. Subtitle. Contains all blanks
Record 3                       80           Words. Subtitle. Contains all blanks

Record 4               NST+1           Words
                            1          Node number
  .                 2-(NST+1)          The stresses for that node
  .
Record NNOG+3




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 4-5
     POST User Manual                                                                                                      Output


4.3.2.2. PATRAN® Results File for each Analysis Type

Each type of analysis processed by POST will write a different set of nodal stresses to the PATRAN® results file.
The correspondence between analysis type and the stress written to file is shown in Tables 4.3 and 4.4.



                             No. of                                             Stresses
    Element                                                                                                         Surface
                             Stresses              xx            yy         zz             xy            yz    xz

     AXIS                          4           σRR           σHH          σZZ          σRZ

     HARMONIC                      6           σRR           σHH          σZZ          σRZ              σZH   σRH

     BRICK                         6           σxx           σyy          σzz          σxy              σyz   σzx

     SHELL                         9           σxx           σyy                       σxy                             T

                                               σxx           σyy                       σxy                            M

                                               σxx           σyy                       σxy                            B

     PLATE                         9           σxx           σyy                       σxy                             T

                                               0             0                         0

                                               σxx           σyy                       σxy                            B

     MEMBRANE                      9           0             0                         0

                                               σxx           σyy                       σxy                            M

                                               0             0                         0

                                                                                                                      1 to
     LAMI                    3*NLAY            σxx           σyy                       σxy
                                                                                                                     NLAY


Notes


T       M       B        refer to top, middle and bottom surfaces respectively

NLAY                     number of layers in laminate

                              Table 4.3 Average Stresses Written to Patran® Results File




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.               Page 4-6
     POST User Manual                                                                                                 Output



                                                                               Stresses
                             No. of
 Element                                                                                                           Surface
                             Stresses        P1                P2               P3                L1    M1   N1
                                             L2                M2               N2                L3    M3   N3

 AXIS                             7          P1                P2               Ph                L1    M1

                                             L2                M2

 HARMONIC                        12          P1                P2              P3                 L1    M1   N1
                                             L2                M2              N2                 L3    M3   N3

 BRICK                           12          P1                P2              P3                 L1    M1   N1

                                             L2                M2              N2                 L3    M3   N3

 SHELL                           12          P1                P2              (P1-P2)                               T
                                             P1                P2              (P1-P2)                               M

                                             P1                P2              (P1-P2)                               B

                                             Tresca(T)         Tresca(M) Tresca(B)

 PLATE                           12          P1                P2              (P1-P2)                               T

                                             0                 0               0

                                             P1                P2              (P1-P2)                               B

                                             Tresca(T)         0               Tresca(B)

 MEMBRANE                        12          0                 0               0

                                             P1                P2              (P1-P2)                               M

                                             0                 0               0

                                             0                 Tresca(M) 0


                              Table 4.4 Principal Stresses Written to Patran® Results File

Note


P1     P2       P3       are principal stresses
Ph                       hoop stress
L1     M1       N1       are direction cosines for P1
L2     M2       N2       are direction cosines for P2
L3     M3       N3       are direction cosines for P3
T      M        B        refer to top, middle and bottom surfaces respectively




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.             Page 4-7
    POST User Manual                                                                                        Output




Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.   Page 4-8
     POST User Manual                                                                                   Appendix A




                     Appendix A -                    Preliminary Data Block for POST


A.1         Introduction
The preliminary data is the first block of the LOCO data. It defines the memory size to be used, the project
name, structure and component names, file names and options to be used. It also defines which files are to be
saved for further processing.

                SYSTEM                      DATA AREA                       memory

                PROJECT                      pname

                JOB                          POST

                FILES                        fname

                TITLE                        title


                TEXT                         text


                STRUCTURE                        sname

                COMPONENT                        sname                    tree

                NEWSTRUCTURE                            nsname

                OPTIONS                       option


                UNITS                    resultnm                           unitm


                SAVE                       set                (FILES)

                RESU

                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
       POST 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 4 byte 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.
                     (Integer)

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


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
       POST User Manual                                                                                 Appendix A


A.4         JOB Command
To define the type of analysis being performed. Compulsory.


           JOB                         POST




Parameters

JOB               : keyword.

POST              : keyword.

Example


        JOB        POST



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


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



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




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




           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 at 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


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




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



            STRUCTURE                      sname




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)

Note


For harmonic combinations the loadcase information to be processed may be drawn from more than one
structure and this is achieved by respecifying a STRUCTURE command within the COMBination data (see
Section 2.11.3). The structure defined in the preliminary data is adopted until a new STRUCTURE command is
supplied.

For harmonic re-run, the structure name should identify the files that contain the combined loadcase information.

See also A.9 COMPONENT command.

Example


        STRUCTURE SHIP



A.9         COMPONENT Command
For substructure analyses, this command defines the recovered component being processed in the current run.


            COMPONENT                      sname                     tree




Parameters

COMPONENT              : keyword

sname                  : structure name as defined on the previous STRUCTURE command. (Alphanumeric, 4
                         characters, the first character must be alphabetic)

tree                   : this is the path down the component tree from the given structure in sname to the
                         component which is being used for POST post-processing.




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


Notes


(i)     If the user is processing the global structure run in a substructure analysis, use only the STRUCTURE
        command (A.8).

(ii)    For harmonic combinations the loadcase information to be processed may be drawn from more than one
        structure and this is achieved by respecifying a COMPONENT command within the COMBination data
        (see Section 2.11.3). The structure defined in the preliminary data is adopted until a new COMPONENT
        command is supplied.

Example


To process the second level component, CMP2, which is part of assembled component CMP1, which is part of
structure STRU.

        COMPONENT STRU CMP1 CMP2



A.10        NEWSTRUCTURE Command
This command is only needed for HARM data type and is used to identify the results being created. However, in
this case the new structure name will not be permanently saved in the project file if no SAVE or RESU
command is specified. In this case, the same new structure name may be used repeatedly within one project.


           NEWSTRUCTURE                            nsname




Parameters

NEWSTRUCTURE : keyword

nsname                     : new structure name. This must be unique within the current project (but see note
                              above). (Alphanumeric, 4 characters, the first character must be alphabetic)

Example


                NEWSTRUCTURE               NSTR

Notes


NEWSTRUCTURE command is not needed in a harmonic re-run where the loadcase combination data are
omitted.


A.11        OPTIONS Command
To define the control options for this run. Optional.




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




           OPTIONS                       option




Parameters

OPTIONS           : keyword

option            : 4 character option name, or list of option names. See table below for details of the options
                     available

Note


The following options are available in POST:

 Option Name                         Application
 DATA                                Stop after checking the data and do not process the stresses.

 GOON                                Proceed even after printed WARNINGS. This option allows the program to
                                     continue despite doubtful data. It should be used after a run in which the
                                     WARNINGS have been noted and rejected.

 NOBL                                Do not print the POST title page.

 CCGO                                Proceed with stress averaging even after thickness and/or offset discontinuities
                                     are encountered within an element group, see Section 1.4.

 GLST                                Print shell element stresses to FEMVIEW file in global stress format. This
                                     allows the FEMVIEW stress calculation facilities to be used.
                                     Note: This does not convert the FEMVIEW stresses into the global system and
                                     so vector plots may be misleading.

 UPLT                                Write any unity stress values computed in the current run to the plot file. Unity
                                     stress values are computed when check stress values are defined, see Section
                                     2.10.

 OAIS                                The material axis definition for anisotropic shells changed with the issue of
                                     POST version H11.3. This option allows the user to continue to employ the old
                                     material axis definition if needed. It is required if and only if the structural
                                     analysis was undertaken using a version of ASAS prior to H11.3, or the
                                     complementary OAIS option has been used in the ASAS run.



Example


        OPTIONS         DATA        GOON       END




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


A.12        SAVE Command
To define the plot file which is to be saved for subsequent display by the relevant plotting program, or to save
the intermediate file

          SAVE             FEMS              (FILES)                   CREATE               (model)     (FILE)   (filename)
                                                                       APPEND
          SAVE             prog              (FILES)

           SAVE             INTE             (FILES)

           SAVE             NEWP             (FILES)




Parameters

SAVE          : keyword

FEMS          : keyword to save the FEMVIEW plot file

prog          : mnemonic to define the plotting program name. Valid names are:

                PATN          -            PATRAN nodal results file, binary
                PTNC          -            PATRAN nodal results file, formatted

(FILES)       : keyword

CREATE : keyword to signify model data is to be included (default)

APPEND : keyword to signify no model data to be included

model         : model name to be used by FEMVIEW

FILE          : keyword to indicate filename follows

filename : name of FEMVIEW file to be created

INTE          : keyword to save the intermediate file and append data to it if necessary

NEWP          : keyword to save the intermediate file and overwrite existing file if necessary

Notes


1.      The plot files are mutually exclusive and only one may be specified within any POST analysis.

2.      CREATE/APPEND and following data is only valid for prog = FEMS




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


3.      FILE may only be omitted if model is specified

4.      Note that if EXTR groups are created in POST, then the CREATE Command should be used on the
        SAVE FEMS line.

Example


        SAVE PATN FILE



A.13        RESU Command
To specify saving of results. The results processed by POST will be added to the database.


           RESU




Parameters

RESU        :            keyword

Example


            RESU


A.14        UNITS Command (not valid for fixed format ASAS data)
If UNITS have been employed in the ASAS analysis it is possible to specify modified units for the POST results.
The default units will be those utilised in the original analysis and if this is satisfactory the UNITS command
may be omitted.


            UNITS                  STRE                       unitm




Parameters

UNITS           : keyword

STRE            : keyword

unitm           : name of unit to be utilised (see Section 2.2)




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


Notes


1.      If the results from more than one structure or component are being combined in a HARM type analysis,
        the analysis units must be identical

2.      Only those terms which are required to be modified need to be specified, undefined terms will default to
        those supplied on the global units definition.

3.      For a full list of valid unit names see Section 5 of the ASAS User Manual.

Example


The global units defined in the ASAS run are N and M.
If the units are redefined in the POST runs as follows:

        UNITS          STRE         MM

the stress results will be reported in N/mm2.



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-10
     POST User Manual                                                                                    Appendix A




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




                     Appendix B -                   - Running Instructions for POST


B.1         ASAS Files Required by POST
POST operates on the files produced by the preceding ASAS or LOCO analysis. The appropriate files must
physically be present in the user’s disk space 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 all PROJECT commands in the set. For example, if the
project name is PRDH, then the Project File will be PRDH10.

The appropriate results for running POST will be saved when a ‘SAVE LOCO FILES’ or a ’SAVE STRESS
FILES’ command appears in the preliminary data of the ASAS or LOCO data. The file name will be derived
from appending 35 to the four character name on the FILES command of the ASAS or LOCO preliminary data.
This name will also appear on the STRUCTURE command of the current preliminary deck (name2 in Appendix
A-). For example, if this name had been RNDH, then the backing file containing stresses (and displacements)
would be RNDH35. For a POST run on a substructured analysis the file name for the results is derived from the
second four character name on the JOB command of the relevant stress recovery run. If this name has been
SRGP then the file would be SRGP35.

For a harmonic run accessing several structures the files required by POST are precisely analogous to those
required by LOCO.



B.2         Running Instructions for POST
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
POST User Manual                                                                                           Appendix B




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


                Appendix C -                  - Equations used for Stress Calculations

The equations used for stress calculations are based on the averaged nodal stresses. These will be orientated
according to the ASAS local element axes system unless an output axes system has been specified to reorientate
the stresses.



C.1         Notation
Stresses and Moments

    σ xx ,σ yy ,σ zz                      Direct stress in X, Y and Z directions
    σ xy ,σ yz ,σ zx                      Shear stresses in XY, YZ and ZX planes
    σ rr ,σ hh ,σ zz                      Direct stresses in R, H and Z directions
    σ rh ,σ hz ,σ zr                      Shear stresses in RH, HZ, ZR planes
     M xx , M yy , M zz                   Moments in X, Y, and Z directions
     M xy , M yz , M zx                   Torques in XY, YZ and ZX planes


Principal Stresses

    P1 , P 2 , P 3                        Principal stresses (P1 is the highest principal stress value)
    θ                                     Principal stress angle (measured from the output X axes to the absolute
                                          maximum principal stress - not necessarily P1)
Equivalent Stresses
    σV                                    von-Mises equivalent stress
    σT                                    Tresca equivalent stress


Wood -Armer Values

     M Px , M Py                          Positive Wood-Armer moment in X and Y directions
     M Nx , M Ny                          Negative Wood-Armer moment in X and Y directions
    α                                     Skew angle between reinforcement directions


Reinforcement Values

     C T ,C B                             Reinforcement cover depths (top and bottom)
     h                                    Thickness of slab
     N x , N y , N xy                     Equivalent in-plane loads in idealized layers
       *     *
     N x, N y                             Loads to be resisted by reinforcing in X and Y directions
     F RA                                 Design stress for reinforcing
     Ax , A y                             Area of reinforcement required in X and Y directions
     fc                                   Compressive force in concrete




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


C.2        Stress Formulae
Principal Stresses:
           2D Stress Field:


                           σ xx + σ yy     (σxx-σyy)2
                    P1 =               +                +σ2
                                                          xy
                                2                 4

                           σ xx + σ yy     (σxx-σyy)2
                    P2 =               -                +σ2
                                                          xy
                                2                 4

                         tan -1 2σxy 
                                        
                    θ=
                           2  σxx -σ yy 
                                        


           3D Stress Field
               P1,P2 & P3 are given by the roots of the equation :


                                              (
                  P3-(σ xx + σ yy+ σzz )P 2+ σ xx σ yy+ σ yyσzz + σzzσ xx -σ2 -σ2 -σ2 P
                                                                            xy yz zx        )
                                              (
                                             - σ xx σ yyσ zz + 2σ xyσ yzσ zx -σ xx σ 2 - σ yyσ 2 - σ zzσ 2 = 0
                                                                                     yz        zx        xy    )
Von-Mises Equivalent Stress:

        σV = P1(P1-P 2 )+ P2(P2-P3)+ P3(P3-P1)                                                                     - Solids




                    (
        σV = 1 2 (σ xx -σ yy ) +(σ yy-σzz ) +(σzz-σ xx ) +3σ2 +3σ2 +3σ2
                              2            2            2
                                                            xy ) yz   zx
                                                                                                                   - Solids




                    (
        σV = 1 2 (σrr -σhh ) +(σhh -σzz ) +(σzz-σrr ) +3σ2 +3σ2 +3σ2
                            2            2           2
                                                         rh ) hz   zr
                                                                                                                   - Axi-symmetrics




        σV = σ2 + σ2 - σxx σ yy+ 3σ2                                                                               - Shells
              xx   yy              xy




Tresca Equivalent Stress:
                  σT = maximum value of P1- P2 or P2-P3 or P3-P1                                                   - Solids

                  σT = maximum value of P1 or P2 or P1-P2                                                          - Shells (P3=0)




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


C.3       Wood-Armer Calculations
C.3.1 Wood-Armer Moments - Orthogonal Reinforcing
          Positive Moments:
                 M Px = M xx + M xy


                 M Py = M yy + M xy


                 If M Px < 0 then :                                      or             If M Py < 0 then :


                                           2                                                                         2
                                    M xy                                                                      M xy
                 M Py = M yy +                                                          M Px = M xx +
                                    M xx                                                                      M yy

                 and M Px = 0                                                           and M Py = 0


                 If M Py < 0 then M Py = 0                                              If M Px < 0 then M Px = 0




          Negative Moments:
                 M Nx = M xx - M xy


                 M Ny = M yy - M xy


                 If M Nx > 0 then :                                    or                 If M Ny > 0 then :

                                          2                                                                          2
                                   M xy                                                                       M xy
                 M Ny = M yy -                                                            M Nx = M xx -
                                   M xx                                                                        M yy
                 and M Nx = 0                                                             and M Ny = 0


                 If M Ny > 0 then M Ny = 0                                                If M Nx > 0 then = 0


Note : Wood - Armer ′Stresses ′ are given by substituting σPx for M Px etc.




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



C.3.2 Wood-Armer Moments - Skewed Reinforcing
          Positive Moments:

                                                                   M xy-M yycot 2α
                      M Px = M xx -2M xycot α + M yycot α +
                                                       2
                                                                        sin α
                                M yy M xy-M yycot α
                                                 2
                      M Py =          +
                               sin 2α     sin α

                      If M Px < 0 then :

                      M Px = 0

                                 1                 (M xy-M yycot α )2           
                                                                                  
                      M Py =            M yy +
                               sin 2α 
                                              M xx -2M xycot α + M yycot 2α      
                                                                                  
                      If M Py < 0 then :
                      M Py = 0
                                                                   (M xy-M yycot α )2
                      M Px = M xx -2M xycot α + M yycot α +  2
                                                                           M yy

          Negative Moments:

                                                                   M xy-M yycot 2α
                      M Nx = M xx -2M xycot α +M yycot α -
                                                      2
                                                                        sin α
                                M yy M xy-M yycot α
                                                 2
                      M Ny =          -
                               sin 2α     sin α

                      If M Nx > 0 then :
                      M Nx = 0

                               1               (M xy-M yycot α )2               
                                                                                  
                      M Ny =         M yy-
                            sin 2α 
                                          M xx -2M xycot α +M yycot 2α           
                                                                                  
                      If M Ny > 0 then :

                      M Ny = 0

                                                                   (M xy-M yycot α )2
                      M Nx = M xx -2M xycot α +M yycot 2α -
                                                                           M yy


Note: In the original Wood-Armer papers the equations were derived using a left handed axis system. Since
ASAS uses a right handed system the above equations have been modified by reversing the direction of the
reinforcing skew angle α.


C.4       Reinforcement Area Calculations




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


Reinforcement areas are calculated using the approach described by Clark using the equations by Nielson. The
full equations are extensive and complex and so only a brief overview of the method employed is given below.
Full details of the procedure may be found in the document ESR170490 - ASASPOST ‘Reinforcement Area
Calculations’.


The method assumes that the loading in a slab is carried as direct loading only in the layers of concrete at the top
and bottom of the slab. The thicknesses of these layers are assumed to be twice the relevant reinforcement cover
depth. The loading in the layers are calculated from the following equations:




Similar equations may be written for NyT, NyB, NxyT and NxyB equivalent forces. The actual load to be carried by
the X and Y directional reinforcing is then given by:
                  N* = N x + N xy
                   x



                  N* = N y + N xy
                   y




                  If N* < 0 then :
                      x                                                   or             If N* < 0 then :
                                                                                             y



                                        2                                                                      2
                                 N xy                                                                   N xy
                  N* = N y +
                   y                                                                     N* = N x +
                                                                                          x
                                  Nx                                                                      Ny
                  and N* = 0
                       x                                                                 and N* = 0
                                                                                              y



                  If N* < 0 then N* = 0
                      y           y                                                      If N* < 0 then N* = 0
                                                                                             x           x




It will be apparent that these are effectively the same as the Wood-Armer equations above and indeed the full set
for skew reinforcement applies. Having established the load carried by the reinforcing (N*) the area of required
area of reinforcing is given by:

                                                   N*x                          N*
                                                                                 y
                                             Ax=                         A y=
                                                   FRA                          FRA




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


In addition the principal concrete compressive force fc is also calculated:
              f c = -2 N xy


              If N* < 0 then :
                  x                                                   or              If N* < 0 then :
                                                                                          y



                            N2
                             xy                                                                    N 2xy
              f c= N x +                                                              f c= N y +
                              Nx                                                                    Ny
              and N* = 0
                   x                                                                  and N* = 0
                                                                                           y



              If N* < 0 and N* < 0 then :
                  x          y




                     Nx +Ny        (Nx-N y )2 +
              f c=          +                     N2
                                                   xy
                        2              4




The above equations do not consider any compressive load capability of the reinforcement. For details of how
this effect is included see the document ESR170490 described above.




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




 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.     Page C-7
    POST User Manual                                                                                         Appendix D




                    Appendix D -                   - Loadcase Combination Methods



The stress results for new loadcases in POST may be formed by factoring the stresses from the ASAS, or
previously formed new POST loadcases and combining them according to one of the following methods:

SSUM           -     simple summation (default)

                     The factored stresses for each of the constituent loadcases are simply added together.

ABSS           -     absolute sum.
                     The absolute values of the factored stresses for each of the constituent loadcases are added
                     together. All resulting stresses will be positive.

SRSS           -     square root of the sum of the squares
                     The factored stresses for each of the constituent loadcases are squared and then added together.
                     The resulting stresses are then square rooted. The final stresses will be positive.

MXLS           -     maximum limit stress
                     The stresses for each of the constituent loadcases are examined to see if they are positive
                     (additive) or negative (relieving). If they are additive, then they are factored by the first factor,
                     if relieving, then they are factored by the second. The resulting factored stresses are then
                     combined using the SSUM method.

MNLS           -     minimum limit stress
                     The stresses for each of the constituent loadcases are examined to see if they are negative
                     (additive) or positive (relieving). If they are additive, then they are factored by the first factor,
                     if relieving, then they are factored by the second. The resulting factored stresses are then
                     combined using the SSUM method.

MAXE           -     maximum envelope
                     The factored stresses for each of the constituent loadcases are considered in turn. The final
                     loadcase consists of the highest (positive) stress values found in the constituent loadcases for
                     each stress type.

MINE           -     minimum envelope
                     The factored stresses for each of the constituent loadcases are considered in turn. The final
                     loadcase consists of the lowest (negative) stress values found in the constituent loadcases for
                     each stress type.

MXAE           -     maximum absolute envelope
                     The absolute values of the factored stresses for each of the constituent loadcases are enveloped
                     using the MAXE method.




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


WDME           -     Wood-Armer moment envelope
                     The Wood-Armer moments are calculated from the factored stresses of each of the constituent
                     loadcases. The resulting Wood-Armer moments are then enveloped.

REEN           -     Reinforcement Calculation Envelope
                     The reinforcement requirements are calculated from the factored stresses of each of the
                     constituent loadcases. The resulting reinforcement requirements are then enveloped.

For LAMI type data the loadcase combination is conducted on the composite section strains and not the
individual layer stresses. The user should take this into account in the case of envelope and limit stress type
combinations.




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




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

								
To top