ANSYS 
  THE DOCU SYSTEM GIVES GENERAL INFORMATION ABOUT A MODULE OR SPECIFIC  
INFORMATION ABOUT A COMMAND.  GENERAL INFO IS DEPENDENT UPON WHICH
MODULE IS CURRENT WHEN THE REQUEST IS ENTERED.  MODULES ARE MADE CURRENT
BY ENTERING THE MODULE NAME OR THE NAME OF ANY COMMAND IN THAT MODULE.  
SPECIFIC COMMAND INFO IS NOT DEPENDENT UPON THE CURRENT MODULE.   
      
GENERAL INFO:     
  ENTER  DOCU         FOR DESCRIPTION OF COMMANDS IN THE MODULE   
  ENTER  DOCU,ALL     FOR FORMAT DISPLAY OF COMMANDS IN THE MODULE
  ENTER  STAT         FOR MODULE NAME AND CURRENT SPECIFICATION VALUES  
SPECIFIC INFO:    
  ENTER  DOCU,XXXX    FOR SPECIFIC DESCRIPTION OF COMMAND XXXX (WHERE   
                       XXXX IS A COMMAND FROM DOCU OR DOCU,ALL LIST).   
                      IF NO FURTHER DOCUMENTATION, USE DOCU AND DOCU,ALL
                       DESCRIPTIONS.
      
ENTER  DOCU,ALL  FOR A LIST OF TOPICS HAVING MORE DOCUMENTATION   
ENTER  DOCU  TO REPEAT THIS DESCRIPTION   
ENTER  /EOF  TO EXIT ANSYS AND RETURN TO SYSTEM 
      
$END  
ANSYS   DOCU
  THE DOCU SYSTEM GIVES GENERAL INFORMATION ABOUT A MODULE OR SPECIFIC  
INFORMATION ABOUT A COMMAND.  GENERAL INFO IS DEPENDENT UPON WHICH
MODULE IS CURRENT WHEN THE REQUEST IS ENTERED.  MODULES ARE MADE CURRENT
BY ENTERING THE MODULE NAME OR THE NAME OF ANY COMMAND IN THAT MODULE.  
SPECIFIC COMMAND INFO IS NOT DEPENDENT UPON THE CURRENT MODULE.   
      
GENERAL INFO:     
  ENTER  DOCU         FOR DESCRIPTION OF COMMANDS IN THE MODULE   
  ENTER  DOCU,ALL     FOR FORMAT DISPLAY OF COMMANDS IN THE MODULE
  ENTER  STAT         FOR MODULE NAME AND CURRENT SPECIFICATION VALUES  
SPECIFIC INFO:    
  ENTER  DOCU,XXXX    FOR SPECIFIC DESCRIPTION OF COMMAND XXXX (WHERE   
                       XXXX IS A COMMAND FROM DOCU OR DOCU,ALL LIST).   
                      IF NO FURTHER DOCUMENTATION, USE DOCU AND DOCU,ALL
                       DESCRIPTIONS.
      
ENTER COMMAND AS DESCRIBED ABOVE FOR THAT RESPONSE    
ENTER  HELP,DOCU  TO REPEAT THIS DESCRIPTION    
ENTER  FINISH  TO EXIT ROUTINE AND RETURN TO ANSYS BEGIN LEVEL    
ENTER  /EOF  AT BEGIN LEVEL TO EXIT ANSYS AND RETURN TO SYSTEM    
      
$END  
ANSYS   ALL 
 TOPIC              RESPONSE  
      
GLOSSARY       DEFINES TERMINOLOGY  
PREP           PRINTS INFO ON ANSYS PREPROCESSING ROUTINES  
POST           PRINTS INFO ON ANSYS POSTPROCESSING ROUTINES 
PLOT           PRINTS INFO ON ANSYS PLOT SLASH COMMANDS     
/              PRINTS INFO ON SLASH (/) COMMANDS OTHER THAN 
                THOSE THAT BEGIN ROUTINES AND PLOT COMMANDS 
*              PRINTS INFO ON ANSYS STAR (*) COMMANDS AND REPEAT COMMAND
HELP           PRINTS INFO ON HELP SYSTEM OF DOCUMENTATION  
      
ENTER  DOCU,TOPIC-NAME  FOR MORE DOCUMENTATION ON ABOVE TOPIC-NAME
ENTER  DOCU,PREP  FOR PREP7 DESCRIPTION TO BEGIN DATA PREPARATION 
ENTER  DOCU,ALL   TO REPEAT THIS LIST     
ENTER  /EOF       TO EXIT ANSYS AND RETURN TO SYSTEM  
      
*END  
ANSYS   PREP
***** ANSYS PREPROCESSING ROUTINES *****  
      
YOU ARE AT ANSYS PREPROCESSING PHASE LEVEL.     
      
COMMAND  ROUTINE DESCRIPTION  
      
         DEFINES ANSYS MODEL FOR MOST GENERAL CASES.  INCLUDES MESH     
         GENERATION, GEOMETRY, MATERIAL, CONSTRAINT, LOAD, AND MODEL    
         PLOTTING DEFINITIONS.
      
ENTER  DOCU,ALL  TO RE-DISPLAY TOPIC-NAME LIST  
*END  
ANSYS   PREP    PRP7    
THIS IS ANSYS PREP7 ROUTINE   
USE INFO FOR PREP7 DOCUMENTATION    
*END  
ANSYS   PREP    PRP7    MISC  
  DETAILED DOCUMENTATION AVAILABLE BELOW THIS LEVEL   
$END  
ANSYS   PREP    PRP7    MISC    SAVE
SAVE  
      
CAUSES THE CURRENT CORE DATA TO BE WRITTEN TO BINARY FILE16.  THE 
DATA IN CORE REMAINS UNTOUCHED.  THE COMMAND MAY BE ISSUED PERIODICALLY 
TO INSURE A CURRENT FILE BACK-UP IN CASE OF A SYSTEM 'CRASH'
OR A 'LINE DROP'.  IT MAY ALSO BE ISSUED BEFORE A 'DOUBTFUL' COMMAND    
SO THAT IF THE RESULT IS NOT WHAT WAS INTENDED THE CORE MAY BE    
RESET TO THE PREVIOUS STATE.  REPEATED USE OF THIS COMMAND OVERWRITES   
THE PREVIOUS DATA ON THE FILE.  AN AUTOMATIC SAVE IS DONE AT THE  
NORMAL EXIT FROM PREP7 (I.E. AT THE FINISH COMMAND).  
$END  
ANSYS   PREP    PRP7    MISC    RESU
RESU  
      
CAUSES FILE16 TO BE READ, THEREBY RESETTING THE CORE DATA AS IT   
WAS AT THE LAST SAVE COMMAND OR FINISH COMMAND. 
$END  
ANSYS   PREP    PRP7    MISC    CHEC
CHECK 
      
CAUSES ALL CURRENT DATA IN CORE TO BE CHECKED FOR COMPLETENESS.   
AN AUTOMATIC CHECK IS DONE BEFORE   
THE SOLVE FILE (SFWRITE) IS WRITTEN.  A SOLUTION CHECK RUN IS ALSO
RECOMMENDED FOR NEW PROBLEMS. 
$END  
ANSYS   PREP    PRP7    MISC    SFWR
SFWRIT
      
CAUSES THE CURRENT CORE DATA TO BE WRITTEN TO THE BINARY SOLVE    
FILE (FILE3).  THIS FILE CONTAINS ALL MODEL DATA AND A SINGLE     
LOAD STEP DATA NEEDED FOR ENTRY TO THE SOLUTION PHASE AT THE SOLUTION   
LEVEL.  THIS COMMAND MUST BE GIVEN BEFORE 
LEAVING PREP7 IF THE ANALYSIS IS TO CONTINUE INTO THE SOLUTION PHASE.   
PREVIOUS DATA ON THE FILE, IF ANY, IS OVERWRITTEN.  IF KTEMP=-1,  
FILE17 MUST ALSO BE SUPPLIED ALONG WITH FILE3 TO THE SOLUTION PHASE     
SINCE THESE TEMPERATURES ARE NOT WRITTEN ON FILE3.    
$END  
ANSYS   PREP    PRP7    ETYP  
USED TO DEFINE AN ANALYSIS TYPE AND ELEMENT TYPES.    
      
  KAN     DEFINES AN ANALYSIS TYPE  
  ET      DEFINES AN ELEMENT TYPE   
  KEYOPT  DEFINES OPTIONS FOR AN ELEMENT TYPE   
  ETLIST  LISTS ELEMENT TYPES 
  ETDEL   DELETES ELEMENT TYPES     
*END  
ANSYS   PREP    PRP7    ETYP    ALL 
USED TO DEFINE THE ANALYSIS TYPE AND ELEMENT TYPES    
      
 RELATED MODULES ARE    
  INFO   - FOR SELECTION OF ELEMENT TYPES 
  OPTION - FOR ANALYSIS OPTIONS     
      
KAN    KEY (KEY=0,STATIC   2,MODAL) 
ET     ITYP   JSTIF KOP1 KOP2 KOP3 KOP4 KOP5 KOP6 INOPR     
KEYOPT ITYP   KNUM  KOP 
ETDEL  ITYP1  ITYP2 INC 
ETLIST ITYP1  ITYP2 INC  KEY  
USE  STIF,N  COMMANDS IN INFO MODULE
  TO SELECT ELEMENTS AND ELEMENT OPTIONS  
*END  
ANSYS   PREP    PRP7    ETYP    KAN 
KAN,KEY     
      
DEFINES AN ANALYSIS TYPE
      
KEY - 0 STATIC             (DEFAULT)
      2 MODAL     
*END  
ANSYS   PREP    PRP7    ETYP    ET  
ET,ITYPE,JSTIF,KOP1,KOP2,KOP3,KOP4,KOP5,KOP6,INOPR    
      
DEFINES AN ELEMENT TYPE 
      
ITYPE - ELEMENT TYPE NUMBER (BETWEEN 1 AND 20)  
JSTIF - STIFFNESS LIBRARY NUMBER FOR THIS ELEMENT TYPE
KOP1  - KEYOPT(1) FOR THIS ELEM. LIBRARY STIFNESS SELECTION 
KOP2  - KEYOPT(2) FOR THIS ELEM. LIBRARY STIFNESS SELECTION 
KOP3  - KEYOPT(3) FOR THIS ELEM. LIBRARY STIFNESS SELECTION 
KOP4  - KEYOPT(4) FOR THIS ELEM. LIBRARY STIFNESS SELECTION 
KOP5  - KEYOPT(5) FOR THIS ELEM. LIBRARY STIFNESS SELECTION 
KOP6  - KEYOPT(6) FOR THIS ELEM. LIBRARY STIFNESS SELECTION 
*END  
ANSYS   PREP    PRP7    ETYP    KEYOPT    
KEYOPT, ITYPE, KNUM, KEYOPT(KNUM)   
      
DEFINES OPTIONS FOR ELEMENT TYPE  ITYPE   
      
ITYPE - ELEMENT TYPE NUMBER (MUST ALREADY BE DEFINED BY ET COMMAND)     
KNUM  - KEYOPT NUMBER BEING SET BY THIS COMMAND 
KEYOPT(KNUM) - THE VALUE OF THIS KEYOPT PARAMETER     
*END  
ANSYS   PREP    PRP7    CDSY  
USED TO DEFINE LOCAL COORDINATE SYSTEMS   
      
  CS      DEFINES A LOCAL COORDINATE SYSTEM     
  LOCAL   DEFINES A LOCAL COORDINATE SYSTEM (ALTERNATE)     
  CSYS    ACTIVATES AN ALREADY DEFINED COORDINATE SYSTEM    
  DSYS    ACTIVATES AN ALREADY DEFINED COORD SYS FOR DISPLAY
  CSCIR   GENERATES ACROSS THE +180 DEGREE LINE 
  CENTER  CALCULATES THE RADIUS OF CURVATURE AND THE CENTER OF    
           CURVATURE LOCATION RELATIVE TO ANY THREE NODES   
  NROTAT  FOR AUTOMATIC NODAL COORDINATE SYSTEM ROTATION    
  CSLIST  LISTS COORDINATE SYSTEMS  
  CSDEL   DELETES COORDINATE SYSTEMS
*END  
ANSYS   PREP    PRP7    CDSY    ALL 
USED TO DEFINE LOCAL COORDINATE SYSTEMS   
      
 RELATED MODULES ARE    
  PLOT   - TO PLOT THE COORDINATE SYSTEMS 
      
CS    KCN    KCS   NORIG NXAX  NXYPL PAR1  PAR2 
LOCAL KCN    KCS    XC    YC    ZC   THXY   THYZ  THXZ  PAR1  PAR2
CSYS  KCN   
DSYS  KCN   
CSCIR KCN    KTHET KPHI 
CENT  NODE   NODE1 NODE2 NODE3 RADIUS     
NROT  NODE1  NODE2 NINC 
CSLIS KCN1   KCN2  KCINC
CSDEL KCN1   KCN2  KCINC
*END  
ANSYS   PREP    PRP7    CDSY    CS  
CS,KCN,KCS,NORIG,NXAX,NXYPL,PAR1,PAR2     
      
DEFINES A LOCAL COORDINATE SYSTEM   
      
KCN   - ARBITRARY NUMBER ASSIGNED TO THIS COORDINATE SYSTEM.  MUST BE   
         GREATER THAN 10 (40 MAX.)  
KCS   - COORDINATE SYSTEM TYPE
         0 - CARTESIAN  
         1 - CYLINDRICAL
         2 - SPHERICAL  
         3 - TOROIDAL   
NORIG - NODAL POINT DEFINING THE ORIGIN OF THIS COORDINATE SYSTEM 
NXAX  - NODAL POINT DEFINING THE X-AXIS ORIENTATION OF THIS COORDINATE  
         SYSTEM   
NXYPL - NODAL POINT DEFINING THE X-Y PLANE (WITH NORIG AND NXAX) OF     
         THIS  COORDINATE SYSTEM    
PAR1,2 - PARAMETERS FOR THIS COORDINATE SYSTEM TYPE   
         FOR KCS=1 AND 2, PAR1 = RATIO OF MINOR RAD TO MAJOR RAD  
          IN X-Y PLANE, PAR2 = SAME IN X-Z PLANE
         FOR KCS=3 (TOROIDAL), PAR1 = MAJOR RADIUS OF TORUS 
*END  
ANSYS   PREP    PRP7    CDSY    LOCA
LOCAL,KCN,KCS,XC,YC,ZC,THXY,THYZ,THXZ,PAR1,PAR2 
      
DEFINES A LOCAL COORDINATE SYSTEM (ALTERNATE)   
      
KCN   - ARBITRARY NUMBER ASSIGNED TO THIS COORDINATE SYSTEM.  MUST BE   
         GREATER THAN 10 (MAX. 40)  
KCS   - COORDINATE SYSTEM TYPE
         0 - CARTESIAN  
         1 - CYLINDRICAL
         2 - SPHERICAL  
         3 - TOROIDAL   
XC,   - GLOBAL CARTESIAN COORDINATES OF THE ORIGIN    
YC,      OF THIS COORDINATE SYSTEM  
ZC    
THXY, - ROTATION ANGLES OF THIS LOCAL     
THYZ,    COORDINATE SYSTEM RELATIVE TO THE
THXZ     GLOBAL CARTESIAN COORDINATE SYSTEM     
PAR1,2 - PARAMETERS FOR THIS COORDINATE SYSTEM TYPE   
         FOR KCS=1 AND 2, PAR1 = RATIO OF MINOR RAD TO MAJOR RAD  
          IN X-Y PLANE, PAR2 = SAME IN X-Z PLANE
         FOR KCS=3 (TOROIDAL), PAR1 = MAJOR RADIUS OF TORUS 
*END  
ANSYS   PREP    PRP7    CDSY    CSYS
CSYS,KCN    
      
ACTIVATES AN ALREADY DEFINED COORDINATE SYSTEM  
      
KCN - NUMBER OF COORDINATE SYSTEM TO BE ACTIVATED     
        0 - GLOBAL CARTESIAN  
        1 - CYLINDRICAL 
        2 - SPHERICAL   
        N - REFERENCE NUMBER OF USER DEFINED SYSTEM   
*END  
ANSYS   PREP    PRP7    CDSY    CSCI
CSCIR,KCN,KTHET,KPHI    
      
GENERATES ACROSS THE +180 DEGREE LINE     
      
KCN   - NUMBER OF COORDINATE SYSTEM IN WHICH SINGULARITY POINT IS 
         CHANGED  
KTHET - KTHET=1 DEFINES 360 DEGREES AS THE SINGULARITY POINT (ALLOWS    
         THETA IN SYSTEM KCN TO CROSS 180 DEGREE LINE)
KPHI  - KPHI=1 ALLOWS CROSSING THE 180 DEGREE LINE IN A TOROIDAL SYSTEM 
*END  
ANSYS   PREP    PRP7    CDSY    CENT
CENTER,NODE,NODE1,NODE2,NODE3,RADIUS
      
CALCULATES THE RADIUS OF CURVATURE AND THE CENTER OF CURVATURE LOCATION 
  RELATIVE TO ANY 3 NODES     
      
NODE   - NODE NUMBER TO BE ASSIGNED TO THE CALCULATED CENTER OF   
          CURVATURE POINT     
NODE1, - IF RADIUS IS EQUAL TO ZERO, NODE1, NODE2, AND NODE3 DEFINE A   
NODE2,    CIRCULAR ARC FOR WHICH THE RADIUS AND THE CENTER OF CURVATURE 
NODE3     ARE TO BE CALCULATED.  IF RADIUS IS NOT EQUAL TO ZERO, NODE1  
          AND NODE2 DEFINE THE CIRCULAR ARC     
RADIUS - IF ZERO, THE PROGRAM WILL CALCULATE THE RADIUS OF CURVATURE.   
          IF GREATER THAN ZERO, CENTER OF CURVATURE IS LOCATED ON NODE3 
          SIDE OF NODE1, NODE2 LINE.  IF LESS THAN ZERO, CENTER OF
          CURVATURE IS LOCATED ON SIDE OPPOSITE TO NODE3.   
*END  
ANSYS   PREP    PRP7    CDSY    NROT
NROTAT,NODE1,NODE2,NINC 
      
FOR AUTOMATIC NODAL COORDINATE SYSTEM ROTATION  
      
NODE1, - ROTATE NODAL COORDINATE SYSTEMS FROM NODE1   
NODE2,    TO NODE2 IN STEPS OF NINC IN CURRENTLY
NINC      ACTIVE COORDINATE SYSTEM  
*END  
ANSYS   PREP    PRP7    CDSY    DSYS
DSYS,KCN    
      
ACTIVATES AN ALREADY DEFINED COORDINATE SYSTEM FOR DISPLAY (PRINT 
 AND PLOT) OF NODAL POINT LOCATIONS 
      
KCN - NUMBER OF COORDINATE SYSTEM TO BE ACTIVATED     
         0 - GLOBAL CARTESIAN 
         1 - GLOCAL CYLINDRICAL     
         2 - SPHERICAL  
         N - REFERENCE NUMBER OF USER DEFINED SYSTEM  
$END  
ANSYS   PREP    PRP7    CDSY    CSLI
CSLIST,KCN1,KCN2,KCINC  
      
LISTS COORDINATE SYSTEMS
      
KCN1, - LIST COORDINATE SYSTEMS FROM KCN1 
KCN2,    TO KCN2  
KCINC    IN STEPS OF KCINC    
*END  
ANSYS   PREP    PRP7    NODE  
USED TO DEFINE NODAL POINTS   
      
N          DEFINES A NODE IN THE CURRENT COORDINATE SYSTEM  
FILL       GENERATES A LINE OF NODES (IN THE CURRENTLY ACTIVE     
            COORDINATE SYSTEM) BETWEEN TWO  DEFINED NODES   
QUAD       GENERATES A QUADRATIC LINE OF NODES  
NGEN       GENERATES ADDITIONAL NODES FROM A GIVEN PATTERN  
SYMM       GENERATES ADDITIONAL NODES FROM A GIVEN PATTERN  
            BY A SYMMETRY REFLECTION
TRANS      TRANSFERS A PATTERN OF NODES FROM ONE COORDINATE SYSTEM
            TO ANOTHER  
NSCALE     GENERATES NEW NODE PATTERNS WITH INDEPENDENT SCALING   
            FACTORS IN THREE DIFFERENT DIRECTIONS     
NMODIF     MODIFIES A PREVIOUSLY DEFINED NODE   
NLIST      PRINTS THE GLOBAL CARTESIAN COORDINATES OF NODES 
NDELE      DELETES NODES FROM THE MODEL   
MOVE       CALCULATES AND MOVES A NODE TO AN INTERSECTION POINT   
SOURCE     SELECTS COORDINATE LOCATION OF UNDEFINED NODES   
            IN PLOTS    
*END  
ANSYS   PREP    PRP7    NODE    ALL 
USED TO DEFINE NODAL POINTS   
      
RELATED MODULES ARE     
 CDSYS  - TO DEFINE LOCAL COORDINATE SYSTEMS    
 PLOT   - TO PLOT THE NODAL POINTS  
      
N     NODE    X     Y     Z    THXY  THYZ   THXZ
FILL  NODE1  NODE2 NFILL NSTRT NINC  ITIME  INC   SPACE     
QUAD  NODE1  NINTR NODE2 NFILL NSTRT NINC   PKFAC     
NGEN  ITIME  INC   NODE1 NODE2 NINC  DX     DY    DZ   SPACE
SYMM  NCOMP  INC   NODE1 NODE2 NINC 
TRANS KCN    INC   NODE1 NODE2 NINC 
NSCAL INC    NODE1 NODE2 NINC  RX    RY     RZ  
NMODI NODE    X     Y     Z    THXY  THYZ   THXZ
NLIST NODE1  NODE2 NINC 
NDELE NODE1  NODE2 NINC 
MOVE  NODE   KC1    X1    Y1    Z1   KC2     X2    Y2    Z2 
    (INPUT THREE LOCATIONS AND THREE 999 VALUES (UNKNOWNS)) 
SOURCE  X     Y     Z   
*END  
ANSYS   PREP    PRP7    NODE    N   
N,NODE,X,Y,Z,THXY,THYZ,THXZ   
      
DEFINES A NODE IN THE CURRENT COORDINATE SYSTEM 
      
NODE  - NODE NUMBER TO BE ASSIGNED  
X,Y,Z - NODE LOCATION IN THE CURRENTLY ACTIVE COORDINATE SYSTEM   
         (R,THETA,Z FOR CYLINDRICAL,R,THETA,PHI FOR SPHERICAL     
          OR TOROIDAL)  
THXY, - NODAL COORDINATE ROTATION ANGLES  
THYZ, 
THXZ  
*END  
ANSYS   PREP    PRP7    NODE    FILL
FILL,NODE1,NODE2,NFILL,NSTRT,NINC,ITIME,INC,SPACE     
      
GENERATES A LINE OF NODES (IN THE CURRENTLY ACTIVE COORDINATE     
 SYSTEM) BETWEEN TWO DEFINED NODES  
      
NODE1, - THE BEGINNING AND ENDING NODES FOR THE FILL-IN (NODE1    
NODE2     DEFAULTS TO NEXT TO LAST NODE SPECIFIED, NODE2 DEFAULTS 
          TO LAST NODE SPECIFIED)   
NFILL  - FILL IN NFILL NODES BETWEEN NODE1 AND NODE2  
            (DEFAULT IS ABS(NODE2 - NODE1) - 1) 
NSTRT  - NODE NUMBER ASSIGNED TO THE FIRST FILLED-IN NODE   
          (DEFAULT IS NODE1 + NINC) 
NINC   - INCREMENT TO ADD TO EACH OF THE REMAINING FILLED-IN NODES
          (DEFAULT IS ((NODE2-NODE1)/(NODE2-NODE1)),  
           LINEAR INTERPOLATION)    
ITIME  - DO FILL-IN OPERATION A TOTAL OF ITIME , INCREMENTING     
INC       NODE1,NODE2 AND NSTRT BY INC EACH TIME (ITIME AND INC BOTH    
          DEFAULT TO 1) 
SPACE  - TO CHANGE SPACING BETWEEN NODES (DEFAULT IS 1.0, I.E.  LINEAR  
          INTERPOLATION). SPACE IS THE RATIO OF THE DISTANCE BETWEEN    
          THE LAST TWO NODES AND THE FIRST TWO NODES  
*END  
ANSYS   PREP    PRP7    NODE    QUAD
QUAD,NODE1,NINTR,NODE2,NFILL,NSTRT,NINC,PKFAC   
      
GENERATES A QUADRATIC LINE OF NODES 
      
NODE1  - BEGIN FILL-IN FROM THIS NODE LOCATION  
NINTR  - INTERMEDIATE OR GUIDING NODE     
NODE2  - END QUADRATIC FILL-IN AT THIS NODE LOCATION  
NFILL  - FILL-IN NFILL NODES BETWEEN NODE1 AND NODE2 (DEFAULTS TO 
          ABS(NODE2-NODE1) - 1). NFILL MUST BE POSITIVE     
NSTRT  - NODE NUMBER ASSIGNED TO FIRST FILLED-IN NODE (DEFAULTS   
          TO NODE1 + NINC)    
NINC   - ADD THIS INCREMENT TO EACH OF THE REMAINING FILLED-IN    
          NODE NUMBERS (MAY BE POSITIVE OR NEGATIVE) DEFAULTS TO  
          (NODE2-NODE1)/(NODE2-NODE1)     
PKFAC  - PEAK LOCATION PARAMETER.  DEFAULT = 0.5 (PEAK OCCURS AT  
          THE NINTR LOCATION). ALLOWABLE RANGE IS GT 0 AND LT 10. 
*END  
ANSYS   PREP    PRP7    NODE    NGEN
NGEN,ITIME,INC,NODE1,NODE2,NINC,DX,DY,DZ,SPACE  
      
GENERATES ADDITIONAL NODES FROM A GIVEN PATTERN 
      
ITIME, - DO THIS GENERATION OPERATION A TOTAL OF ITIME,     
INC    -  INCREMENTING ALL NODES IN THE GIVEN PATTERN BY INC
          EACH TIME (INC DEFAULTS TO 0)   
NODE1, - BEGINNING AND ENDING NODE NUMBERS DEFINING THE PATTERN   
NODE2     TO BE REPEATED (NODE2 DEFAULTS TO NODE1)    
NINC   - INCLUDE ALL NODES FROM NODE1 TO NODE2 IN STEPS OF NINC   
          (DEFAULTS TO 1)     
         (IF NODE1 IS ALL, THE SET TO BE REPEATED IS ALL SLEECTED NODES)
DX,DY, - NODE LOCATION INCREMENTS IN THE CURRENTLY ACTIVE   
DZ        COORDINATE SYSTEM (DR,DTHETA,DZ FOR CYLINDRICAL,  
          DR,DTHETA,DPHI, FOR SPHERICAL OR TOROIDAL)  
SPACE  - SCALE GENERATED NODE PATTERN BY THIS VALUE BEFORE  
          APPLYING NODE LOCATION INCREMENTS (DEFAULT IS 1)  
*END  
ANSYS   PREP    PRP7    NODE    SYMM
SYMM,NCOMP,INC,NODE1,NODE1,NINC     
      
GENERATES ADDITIONAL NODES FROM A GIVEN PATTERN BY A  
 SYMMETRY REFLECTION ABOUT A COMPONENT IN THE CURRENTLY     
 ACTIVE COORDINATE SYSTEM.    
      
NCOMP  - 0,1 - X (OR R) SYMMETRY    
           2 - Y (OR THETA) SYMMETRY
           3 - Z (OR PHI) SYMMETRY  
INC    - INCREMENT ALL NODES IN THE GIVEN PATTERN BY INC TO FORM  
          THE REFLECTED NODE PATTERN
NODE1, - BEGINNING AND ENDING NODE NUMBERS DEFINING THE PATTERN   
NODE2     TO BE REFLECTED (NODE2 DEFAULTS TO NODE1).  IF ALL THEN 
          USE ALL SELECTED NODES.   
NINC   - INCLUDE ALL NODES FROM NODE1 TO NODE2 IN STEPS OF NINC   
          IN THE PATTERN (DEFAULTS TO 1)  
        (IF (NODE1 IS ALL, THE PATTERN IS ALL SELECTED NODES)     
*END  
ANSYS   PREP    PRP7    NODE    TRAN
TRANS,KCN,INC,NODE1,NODE2,NINC
      
TRANSFERS A PATTERN OF NODES FROM ONE COORDINATE SYSTEM TO ANOTHER
      
KCN    - THE PATTERN IS TO BE TRANSFERRED TO COORDINATE SYSTEM    
          NUMBER KCN FROM THE CURRENTLY ACTIVE SYSTEM 
INC    - INCREMENT ALL NODES IN THE GIVEN PATTERN BY INC TO FORM  
          THE TRANSFERRED NODE PATTERN    
NODE1, - BEGINNING AND ENDING NODE NUMBERS DEFINING THE PATTERN   
NODE2  -  TO BE TRANSFERRED (NODE2 DEFAULTS TO NODE1).  IF ALL THEN     
          USE ALL SELECTED NODES.   
NINC   - INCLUDE ALL NODES FROM NODE1 TO NODE2 IN STEPS OF NINC IN THE  
          PATTERN (DEFAULTS TO 1)   
        (IF NODE1 IS ALL, THE PATTERN IS ALL SELECTED NODES)
*END  
ANSYS   PREP    PRP7    NODE    NSCA
NSCALE,INC,NODE1,NODE2,NINC,RX,RY,RZ
      
GENERATES NEW NODE PATTERN WITH INDEPENDENT SCALING FACTORS IN    
 THREE DIFFERENT DIRECTIONS.  RX, RY, RZ ARE INTERPRETED IN THE   
 CURRENTLY ACTIVE COORDINATE SYSTEM.
      
INC    - INCREMENT THE NODE PATTERN BY INC
NODE1, - INCLUDE ALL NODES FROM NODE1 TO NODE2 IN STEPS OF NINC.  
         IF NODE1 IS ALL THEN USE ALL SELECTED NODES. 
NODE2,
NINC  
         (IF NODE1 IS ALL, THE PATTERN IS ALL SELECTED NODES)     
RX,RY, - SCALE THE NODE LOCATION BY RX IN THE X DIRECTION, RY IN  
RZ        THE Y DIRECTION, AND RZ IN THE Z DIRECTION OF THE CURRENTLY   
          ACTIVE SYSTEM.  A RATIO OF GREATER THAN 1 WILL ENLARGE THE    
          PATTERN.  IF LESS THAN 1, THE PATTERN IS REDUCED. 
          (DEFAULT RX,RY,RZ = 1) X,Y,Z SHOULD BE INTERPRETED AS R,
          THETA,Z FOR CYLINDRICAL COORDINATE AND R,THETA,PHI FOR  
          SPHERICAL AND TOROIDAL COORDINATES.   
*END  
ANSYS   PREP    PRP7    NODE    NMOD
NMODIF,NODE,X,Y,Z,THXY,THYZ,THXZ    
      
MODIFIES A PREVIOUSLY DEFINED NODE  
      
NODE   - MODIFY COORDINATES OF THIS NODE  
          (IF NODE=ALL  THEN MODIFY ALL SELECTED NODES)     
X,Y,Z* - REPLACE THE PREVIOUS COORDINATE VALUES ASSIGNED TO THIS  
THXY,     NODE WITH THESE (NON-ZERO) CORRESPONDING COORDINATE VALUES    
THYZ, 
THXZ  
 *X,Y,Z SHOULD BE INTERPRETED AS R,THETA,Z FOR CYLINDRICAL  
 COORDINATES OR R,THETA,PHI, FOR SPHERICAL AND TOROIDAL COORDINATES     
*END  
ANSYS   PREP    PRP7    NODE    MOVE
MOVE,NODE,KC1,X1,Y1,Z1,KC2,X2,Y2,Z2 
      
CALCULATES AND MOVES A NODE TO AN INTERSECTION POINT  
      
NODE   - NODE NUMBER TO BE MOVED    
KC1    - FIRST COORDINATE SYSTEM NUMBER   
X1,Y1, - INPUT ONE OR TWO VALUES DEFINING THE LOCATION OF THE     
Z1*        NODE.  INPUT 999 FOR UNKNOWN VALUE(S) TO BE CALCULATED 
KC2    - SECOND COORDINATE SYSTEM NUMBER  
X2,Y2  - INPUT ONE OR TWO VALUES DEFINING THE LOCATION OF THE     
Z2*       NODE.  INPUT 999 FOR UNKNOWN VALUE(S) TO BE CALCULATED  
          *X,Y,Z SHOULD BE INTERPRETED AS R,THETA,Z FOR CYLINDRICAL     
          COORDINATES, OR R,THETA,PHI FOR SPHERICAL OR TOROIDAL   
*END  
ANSYS   PREP    PRP7    NODE    SOUR
SOURCE,X,Y,Z
      
SELECTS COORDINATE LOCATION OF UNDEFINED NODES IN PLOTS.  X, Y, Z 
 ARE INTERPRETED IN THE CURRENTLY ACTIVE COORDINATE SYSTEM. 
      
X,Y,Z  - NODE LOCATION (DEFAULT IS UNDEFINED NODES AT GLOBAL ORIGIN)    
*END  
ANSYS   PREP    PRP7    ELEM  
USED TO DEFINE ELEMENTS 
      
E          DEFINES ELEMENT CONNECTIVITY   
EMODIF     MODIFIES A PREVIOUSLY DEFINED ELEMENT
EGEN       GENERATES ADDITIONAL ELEMENTS  
ESYM       GENERATES ADDITIONAL ELEMENTS FROM A GIVEN NODE PATTERN
            BY A SYMMETRY REFLECTION.     
ESTART     STARTING NUMBER FOR ELEMENTS   
EDELET     DELETES ELEMENTS FROM THE MODEL
ECOMPR     REMOVES DELETED ELEMENTS FROM THE MODEL AND CAUSES ALL 
            ELEMENTS FOLLOWING DELETED ELEMENTS TO BE RENUMBERED (ACTION
ELIST       PRINTS THE ELEMENTS     
MAT,        DEFINES A MATERIAL, TYPE, OR REAL CONSTANT TABLE
TYPE,        NUMBER TO BE ASSIGNED TO DEFINED ELEMENTS
REAL         ENTER DOCU,MAT FOR DOCUMENTATION ON ALL THREE COMMANDS.    
EN,          SAME AS E, EGEN, AND ESYM COMMANDS BUT ALLOW AN
ENGEN,        ELEMENT NUMBER TO BE SPECIFIED.   
ENSYM 
*END  
ANSYS   PREP    PRP7    ELEM    ALL 
USED TO DEFINE ELEMENTS 
      
 RELATED MODULES ARE    
  PLOT   - TO PLOT THE ELEMENTS     
      
E      I      J     K     L     M     N     O     P   
EMODIF IEL    STLOC I1    I2    I3    I4    I5   I6   I7   I8     
EGEN   ITIME  INC   IEL1  IEL2  IEINC MINC  TINC  RINC  CINC
ESYM   INODE  INC   IEL1  IEL2  IEINC     
ESTART ISTRT
EDELE  IEL1   IEL2  INC 
ECOMPR (ACTION)   
ELIST  IEL1   IEL2  INC 
MAT    MAT  
TYPE   ITYPE
REAL   NSET 
EN     IEL   I      J     K     L     M     N     O     P   
ENGEN  IINC  ITIME  INC   IEL1  IEL2  IEINC MINC  TINC  RINC  CINC
ENSYM  IINC  INODE  INC   IEL1  IEL2  IEINC     
*END  
ANSYS   PREP    PRP7    ELEM    E   
E,I,J,K,L,M,N,O,P 
      
DEFINES ELEMENT CONNECTIVITY  
      
I,J,K, - NUMBER ASSIGNED TO NODE I (FIRST NODE),J (SECOND NODE),ETC.    
L,M,N,
O,P   
*END  
ANSYS   PREP    PRP7    ELEM    EMOD
EMODIF,IEL,STLOC,I1,I2,I3,I4,I5,I6,I7,I8  
      
MODIFIES A PREVIOUSLY DEFINED ELEMENT     
      
IEL    - ELEMENT TO BE MODIFIED     
         (IF IEL IS ALL, ALL SELECTED ELEMENTS ARE MODIFIED)
STLOC  - LOCATION OF FIRST NODE NUMBER TO BE MODIFIED 
          (I.E.,NODE I IS LOCATION 1, NODE M IS LOCATION 5, ETC.) 
I1,I2, - REPLACE THE PREVIOUS NODE VALUES ASSIGNED TO THIS ELEMENT
I3,I4,    WITH THESE CORRESPONDING VALUES (NON-BLANK).
I5,I6,    IF FIRST NODE NUMBER IS ZERO, CHANGE NODE TO ZERO.
I7,I8 
*END  
ANSYS   PREP    PRP7    ELEM    EGEN
EGEN,ITIME,INC,IEL1,IEL2,IEINC,MINC,TINC,RINC,CINC    
      
GENERATES ADDITIONAL ELEMENTS 
      
ITIME, - DO THIS GENERATION OPERATION A TOTAL OF ITIME, INCREMENTING    
INC       ALL NODES IN THE GIVEN PATTERN BY INC.  INC DEFAULTS TO 1     
IEL1,  - BEGINNING AND ENDING ELEMENT NUMBERS DEFINING THE PATTERN TO   
IEL2,     BE REPEATED.  INCLUDE ALL ELEMENTS FROM IEL1 TO IEL2 IN 
IEINC     STEPS OF IEINC. IEL2 DEFAULTS TO IEL1. IEINC DEFAULTS TO 1.   
         IF IEL1 IS NEGATIVE, USE THE PREVIOUS (-IEL1) ELEMENTS   
          AS THE PATTERN TO BE REPEATED.  
         (IF IEL1 IS ALL, USE ALL SELECTED ELEMENTS AS THE PATTERN)     
MINC   - INCREMENT MATERIAL NUMBER OF ALL ELEMENTS IN THE GIVEN   
          PATTERN BY MINC EACH TIME AFTER THE FIRST (DEFAULTS TO 0)     
TINC   - INCREMENT TYPE NUMBER OF ALL ELEMENTS (DEFAULTS TO 0)    
RINC   - INCREMENT REAL CONSTANT TABLE NUMBER OF ALL ELEMENTS     
          (DEFAULTS TO 0)     
*END  
ANSYS   PREP    PRP7    ELEM    ESYM
ESYM,INODE,INC,IEL1,IEL2,IEINC
      
GENERATES ADDITIONAL ELEMENTS FROM A GIVEN NODE PATTERN BY A
 SYMMETRY REFLECTION.   
      
INODE  - NODE IN THE ITH POSITION ON ELEMENT IEL1 (1,2,3, OR 4)   
INC    - NODE NUMBER INCREMENT TO BE ADDED TO GIVEN PATTERN 
IEL1,  - INCLUDE ALL ELEMENTS FROM IEL1 TO IEL2 IN STEPS OF 
IEL2,  -  IEINC.  
IEINC 
         (IF IEL1 IS ALL, USE ALL SELECTED ELEMENTS AS THE PATTERN)     
*END  
ANSYS   PREP    PRP7    PLOT  
DISPLAYS (OR PLOTS) NODES, ELEMENTS, LOADS, AND COORDINATE SYSTEMS
      
CSPLT,KEY    - SHOW LOCAL COORDINATE SYSTEMS    
NDIRPL,KEY   - SHOW NODAL COORDINATE SYSTEMS    
RESET        - RESET ALL SPECIFICATONS    
NPLOT,NUMKEY - PLOT THE NODES (WITH NUMBERS)    
EPLOT        - PLOT THE ELEMENTS    
      
DOCU,BC     - FOR DOCUMENTATION ON DISPLAYING BOUNDARY CONDITIONS 
DOCU,NUM    - FOR DOCUMENTATION ON NUMBERING ITEMS ON DISPLAY     
*END  
ANSYS   PREP    PRP7    PLOT    PLOT
      
USE   PLOT $DOCU   TO GET ANSYS PREP7 PLOTTING COMMANDS.    
USE   HELP,PLOT    TO GET ANSYS DISPLAY PLOT COMMANDS.
$END  
ANSYS   PREP    PRP7    PLOT    ALL 
PLOTS NODES,ELEMENTS,COORD,SYSTEMS, AND LOADS   
      
CSPLT  KEY    (KEY)     
NDIRPL KEY    (KEY)     
RESET     (RESET ACTION)
NPLOT  KNUM    (KNUM: 0 - NO NODES, 1 - SHOW NODES)   (PLOT ACTION)     
EPLOT     (PLOT ACTION) 
      
LABEL,KEY: LABEL= TMBC,RMBC,TDBC,RDBC,FBC,MBC,PRBC,NTBC,HFBC,CVBC 
                  ALBC  
            KEY=0,1 -IF KEY=1, PLOT SHOWS BOUNDARY CONDITION OF LABEL   
LABEL,KEY:  LABEL= ENUM,NNUM,RNUM,MNUM,TNUM,LNUM  KEY = 0,1 
            KEY = 1, PLOTS ELEMENTS WITH SELECTED ITEM NUMBERED   
*END  
ANSYS   PREP    PRP7    PLOT    BC  
THESE COMMANDS CAUSE THE BOUNDARY CONDITIONS TO BE SHOWN ON THE DISPLAY 
      
ALBC,KEY    KEY=0 TURN OFF ALL BOUNDARY CONDITION PLOT KEYS 
            KEY=1 TURN ON ALL BOUNDARY CONDITION PLOT KEYS  
TDBC,KEY    TRANSLATIONAL DISPLACEMENTS   
RDBC,KEY    ROTATIONAL DISPLACEMENTS
FBC,KEY     FORCES
MBC,KEY     MOMENTS     
PRBC,KEY    NODAL PRESSURES   
TMBC,KEY    TRANSLATIONAL MASTER DOF
RMBC,KEY    ROTATIONAL MASTER DOF   
$END  
ANSYS   PREP    PRP7    PLOT    NUM 
THESE COMMANDS CAUSE ELEMENT PLOT ITEMS TO BE NUMBERED (USE ONLY ONE    
 AT A TIME) 
      
NNUM,KEY    NODE NUMBERS (MAY BE USED WITH ANY ONE OTHER)   
ENUM,KEY    ELEMENT NUMBERS   
RNUM,KEY    ELEMENT REAL CONSTANT NUMBERS 
TNUM,KEY    ELEMENT TYPE NUMBERS    
LNUM,KEY    ELEMENT LOCATION NUMBERS
$END  
ANSYS   PREP    PRP7    OPTI  
USED TO DEFINE ANALYSIS OPTIONS     
      
TO INPUT OR CHANGE VALUES     
LABEL,VALUE 
KAY,NUMBER,VALUE   (ENTER DOCU,KAY FOR DOCUMENTATION) 
      
TREF   - REFERENCE TEMPERATURE FOR THERMAL EXPANSION  
*END  
ANSYS   PREP    PRP7    OPTI    ALL 
USED TO DEFINE ANALYSIS OPTIONS     
      
 RELATED MODULES ARE    
  LOPT   - TO DEFINE LOAD STEP OPTIONS    
      
LABEL,VALUE  (TREF,BETAD ARE VALID LABELS)
KAY,NUMBER,VALUE  
*END  
ANSYS   PREP    PRP7    OPTI    TREF
TREF,VALUE  
      
DEFINES THE REFERENCE TEMPERATURE FOR THE THERMAL STRAIN CALCULATIONS   
IN STRUCTURAL ANALYSES.  THERMAL STRAINS ARE A FUNCTION OF  
ALPHA*(T-TREF) WHERE ALPHA IS THE COEFFICIENT OF THERMAL EXPANSION
PROPERTY AND T IS THE ELEMENT TEMPERATURE.  UNITS SHOULD BE 
CONSISTENT WITH ALPHA.  
      
VALUE - REFERENCE TEMPERATURE FOR THERMAL EXPANSION.  
$END  
ANSYS   PREP    PRP7    OPTI    KAY 
KAY DOCUMENTATION IS DEPENDENT ON THE ANALYSIS TYPE.  ENTER THE   
OPTIONS MODULE AND RE-ISSUE THE DOCU COMMAND.   
      
         EX:   OPTI $DOCU,KAY 
*END  
ANSYS   PREP    PRP7    OPTI    KAY     0 
***** STATIC ANALYSIS OPTIONS ***** 
NONE REQUIRED     
*END  
ANSYS   PREP    PRP7    OPTI    KAY     2 
***** MODE-FREQUENCY OPTIONS *****  
KAY,2 -  N  EXPAND FIRST N MODE SHAPES    
      - -1  EXPAND MODE SHAPES IN FREQUENCY RANGE     
KAY,3 -  0  DO NOT PRINT REDUCED MODE SHAPES    
      -  1  PRINT ALL REDUCED MODE SHAPES 
      -  N  PRINT FIRST N REDUCED MODE SHAPES   
*END  
ANSYS   PREP    PRP7    RCON  
USED TO DEFINE THE ELEMENT REAL CONSTANTS 
      
  R      DEFINES UP TO SIX REAL CONSTANTS 
  RMORE  DEFINES MORE THAN SIX REAL CONSTANTS   
  RMODIF MODIFIES A DEFINED REAL CONSTANT 
  RDELE  DELETES A DEFINED REAL CONSTANT  
  RCOMPR REMOVES DELETED SETS OF REAL CONSTANTS (DELETED SET NUMBERS    
           CAN THEN BE REUSED)                  (ACTION)    
  RLIST  LISTS THE REAL CONSTANTS   
*END  
ANSYS   PREP    PRP7    RCON    ALL 
USED TO DEFINE THE ELEMENT REAL CONSTANTS 
      
  RELATED MODULES ARE:  
  INFO -- FOR DEFINITION OF ELEMENT REAL CONSTANTS    
      
R      NSET  R1    R2    R3    R4    R5    R6   
RMORE  R7    R8    R9    R10   R11   R12  
       (RMORE COMMANDS WILL CONTINUE ADDING TO SET)   
RMODIF NSET  STLOC V1   V2   V3   V4   V5   V6  
RLIST  NSET1 NSET2 NINC 
RDELE  NSET1 NSET2 NINC 
RCOMPR  (ACTION)  
*END  
ANSYS   PREP    PRP7    RCON    R   
R,NSET,R1,R2,R3,R4,R5,R6
      
DEFINES UP TO SIX REAL CONSTANTS    
      
NSET    - SET IDENTIFICATION NUMBER 
R1...R6 - THE SPECIFIC VALUES FOR EACH REAL CONSTANT  
*END  
ANSYS   PREP    PRP7    RCON    RMOD
RMODIF,NSET,STLOC,V1,V2,V3,V4,V5,V6 
      
MODIFIES A PREVIOUSLY DEFINED SET OF REAL CONSTANTS   
      
NSET    - SET IDENTIFICATION NUMBER 
STLOC   - STARTING LOCATION WITHIN SET TO BEGIN MODIFICATION
V1...V6 - UP TO SIX NEW VALUES FOR REAL CONSTANTS SELECTED  
*END  
ANSYS   PREP    PRP7    MATE  
USED TO DEFINE LINEAR AND NON-LINEAR MATERIAL PROPERTIES    
      
  LABEL   DEFINES MAT. PROP. AS CONSTANT OR A POLYNOMIAL    
  MPTEMP  DEFINES TEMPERATURE TABLE 
  MPTGEN  GENERATES TEMPERATURE TABLE     
  MPDATA  DEFINES MAT. PROP. IN TABULAR FORM    
  MPTRES  RESETS TEMP. TABLE TO THAT OF PREVIOUS MATERIAL   
  MPDRES  RESETS MATERIAL TABLE TO THAT OF PREVIOUS MATERIAL
  MPDELE  DELETES MAT. PROP. ENTRY  
  MPLIST  LISTS PROPERTY TABLES     
*END  
ANSYS   PREP    PRP7    MATE    ALL 
USED TO DEFINE THE MATERIAL PROPERTIES    
      
 RELATED MODULES ARE    
  INFO   - FOR DEFINITION OF ELEMENT PROPERTIES 
           REQUIRED FOR EACH ELEMENT TYPE 
      
LABL*   MAT   C0    C1    C2    C3    C4  
MPTEMP  STLOC T1    T2    T3    T4    T5    T6  
MPTGEN  STLOC NUM  TSTRT TINC 
MPDATA  LAB * MAT   STLOC  C1    C2    C3    C4    C5    C6 
MPTRES  LAB * MAT 
MPDRES  LAB * MATF LAB * MATT 
MPDELE  LAB * MAT1  MAT2  INC 
     (* LAB  = EX,ALPX,DENS,KXX,GXY,ETC.) 
*END  
ANSYS   PREP    PRP7    MATE    LABE
LABEL,MAT,CO,C1,C2,C3,C4
      
DEFINES MATERIAL PROPERITIES AS A CONSTANT OR A 
        POLYNOMIAL EQUATION (MAX. ORDER OF 4)   
      
LABEL*  MATERIAL PROPERTY LABEL     
MAT     MATERIAL NUMBER 
CO      CONSTANT VALUE OR CONSTANT TERM IN POLYNOMIAL 
C1-C4   REMAINING TERMS IN POLYNOMIAL     
      
 *VALID LABELS EX   ALPX NUXY EY   ALPY EZ   ALPZ     
               NUYZ NUXZ DENS GXY  GYZ  GXZ     
*END  
ANSYS   PREP    PRP7    MATE    MPTE
MPTEMP,STLOC,T1,T2,T3,T4,T5,T6
      
DEFINES TEMPERATURE TABLE FOR RELATING MATERIAL PROPERTIES  
       (DEFAULTS TO 0-2300 DEG. IN STEPS OF 100 FOR POLYNOMIAL)   
      
STLOC   STARTING LOCATION IN TABLE FOR ENTERING TEMPERATURES
        (DEFAULTS TO LAST LOCATION FILLED PLUS ONE)   
T1-T6   TEMPERATURES    
*END  
ANSYS   PREP    PRP7    MATE    MPTG
MPTGEN,STLOC,NUM,TSTRT,TINC   
      
GENERATES TABLE OF TEMPERATURES     
      
STLOC    STARTING LOCATION IN TABLE FOR GENERATING TEMP.    
NUM      NO.OF TEMPERATURE POINTS TO BE GENERATED     
TSTRT    TEMPERATURE ASSOCIATED WITH FIRST MAT. PROP. VALUE 
TINC     CONSTANT TEMPERATURE INCREMENT   
*END  
ANSYS   PREP    PRP7    MATE    MPTR
MPTRES,LAB,MAT    
      
SETS TEMPERATURE TABLE TO THAT OF A PRIOR SET   
      
LAB     MAT. PROP. LABEL OF PRIOR SET     
MAT     MATERIAL NUMBER OF PRIOR SET
*END  
ANSYS   PREP    PRP7    MATER   MPDR
MPDRES,LABF,MATF,LABT,MATT    
      
SETS MATERIAL TABLE TO THAT OF A PREVIOUS SET   
      
MATF -  MATERIAL TABLE NUMBER COPIED FROM 
MATT -  MATERIAL TABLE NUMBER COPIED TO   
LABF -  MATERIAL PROPERTY LABEL ASSOCIATED WITH MATF  
LABT -  MATERIAL PROPERTY LABEL ASSOCIATED WITH MATT  
*END  
ANSYS   PREP    PRP7    MATE    MPDA
MPDATA,LAB,MAT,STLOC,C1,C2,C3,C4,C5,C6    
      
DEFINES MATERIAL PROPERTIES IN TABULAR FORM     
      
LAB     MAT. PROP. LABEL
MAT     MATERIAL NO.    
STLOC   STARTING LOCATION IN TABLE FOR ENTERING DATA  
        (DEFAULTS TO LAST LOCATION ENTERED PLUS ONE)  
C1-C6   MATERIAL PROPERTY TABLE VALUES    
*END  
ANSYS   PREP    PRP7    MAST  
USED TO DEFINE THE MASTER (DYNAMIC) DEGREES OF FREEDOM.     
      
  M       SPECIFY NODES AND DIRECTION OF MASTER D.O.F.
  MGEN    TO GENERATE ADDITIONAL MASTERS  
  TOTAL   DEFINE TOTAL NUMBER OF MASTER DEGREES OF FREEDOM  
  MLIST   LIST CURRENT MASTER DEGREES OF FREEDOM
  MDELE   DELETE SPECIFIED MASTER DEGREES OF FREEDOM  
*END  
ANSYS   PREP    PRP7    MAST    ALL 
USED TO DEFINE THE MASTER (DYNAMIC) DEGREES OF FREEDOM.     
      
M       NODE  LAB   NEND  NINC  LAB2  ....  LAB6
TOTAL   NTOT  NRMDF     
MLIST   NODE1 NODE2 NINC
MDELE   NODE  LAB   NEND  NINC LAB2  ....  LAB6 
*END  
ANSYS   PREP    PRP7    MAST    M   
M,NODE,LAB,NEND,NINC,LAB2,...,LAB6  
      
SPECIFY NODES AND DIRECTIONS OF MASTER DEGREES OF FREEDOM.  
      
      
NODE    - FIRST NODE OF MASTER DEGREE OF FREEDOM
LAB     - DIRECTION OF MASTER DEGREE OF FREEDOM 
NEND    - LAST NODE IN LIST OF MASTER DEGREE OF FREEDOM     
NINC    - INCREMENT OF NODE NUMBER ON ABOVE DEGREE OF FREEDOM LIST
LAB2...6- ADDITIONAL DIRECTIONS OF MASTER D.O.F.
*END  
ANSYS   PREP    PRP7    MAST    MGEN
MGEN,ITIME,INC,NODE1,NODE2,NINC     
      
GENERATES A SET OF MASTERS    
      
ITIME - TOTAL NUMBER OF SETS OF MASTERS TO BE GENERATED (MUST BE  
         GREATER THAN 1)
INC   - INCREMENT ALL NODES IN THE GIVEN PATTERN BY INC     
NODE1 - BEGINNING AND ENDING NODE NUMBERS DEFINING THE
NODE2 -  PATTERN TO BE REPEATED (NODE2 DEFAULTS TO NODE1)   
NINC  - INCLUDE ALL NODES FROM NODE1 TO NODE2 IN STEPS OF NINC (DEFAULTS
         TO 1)    
$END  
ANSYS   PREP    PRP7    MAST    TOTA
TOTAL,NTOT,NRMDF  
      
DEFINE TOTAL NUMBER OF MASTER DEGREES OF FREEDOM.     
      
NTOT - TOTAL NUMBER OF MASTER DEGREES OF FREEDOM
         ALL MASTER DEGREES OF FREEDOM (UP TO NTOT)   
         NOT SPECIFIED BY M COMMANDS WILL BE AUTOMATICALLY  
         SELECTED.
NRMDF - IF 1, EXCLUDE ROTATIONAL DEGREES OF FREEDOM   
*END  
ANSYS   PREP    PRP7    LOPT  
USED TO DEFINE LOAD OPTIONS (PRINT CONTROLS, PLOT CONTROLS, ETC.) 
      
  ENTER DOCU,1 FOR LOAD OPTIONS     
  ENTER DOCU,2 FOR CALCULATION OPTIONS    
  ENTER DOCU,3 FOR PRINT CONTROLS   
*END  
ANSYS   PREP    PRP7    LOPT    1   
USED TO DEFINE LOAD OPTIONS   
  ACEL, OMEGA, DOMEGA, CGLOC, CGOMEGA, AND DCGOMEG  DESCRIBE
          A NON-UNIFORM ACELERATION FIELD.  THE FIELD INCLUDES A  
          UNIFORM ACELERATION, AND ROTATION ABOUT TWO NON-PARALLEL AXES.
  KTEMP   SPECIFIES THE SOURCE OF TEMPERATURES FOR THIS LOAD STEP 
  TUNIF   DEFINES THE VALUE OF THE UNIFORM TEMPERATURE TO BE USED IF    
           KTEMP IS SET TO ZERO     
  KUSE    SELECTS NEW OR PREVIOUSLY CREATED STIFFNESS MATRIX
  DMPRAT  SPECIFIES MODAL DAMPING RATIO (KAN=2 ONLY)  
  SED     SPECIFIES SEISMIC EXCITATION DIRECTION (KAN=2 ONLY)     
  EXMO    EXPANDS WITHIN SPECIFIED FREQ RANGE (KAN=2 ONLY)  
  SVTYP   DEFINES TYPE OF SPECTRUM TABLE     (KAN=2 ONLY)   
  FREQ    DEFINES SPECTRUM FREQUENCY VALUES  (KAN=2 ONLY)   
  SV      DEFINES THE DAMPED SPECTRUM VALUES (KAN=2 ONLY)   
  MCOMB   DEFINES THE TYPE OF MODAL COMBINATION DIRECTIVES WRITTEN ON   
           FILE24 FOR POST27 (KAN=2 ONLY) 
*END  
ANSYS   PREP    PRP7    LOPT    ACEL
ACEL,ACELX,ACELY,ACELZ  
      
SPECIFIES THE COMPONENTS OF A UNIFORM ACCELERATION FIELD (USUALLY 
  GRAVITY)  
      
ACELX - ACCELERATION IN GLOBAL CARTESIAN X, Y, AND Z DIRECTIONS.  
ACELY    UNITS ARE LENGTH/TIME**2 (INCHES/SEC**2).  THE INERTIA FORCE   
ACELZ    ACTS OPPOSITE THE ACCELERATION DIRECTION.    
*END  
ANSYS   PREP    PRP7    LOPT    SED 
SED,SEDX,SEDY,SEDZ
      
SPECIFIES SEISMIC EXCITATION DIRECTION (KAN=2 ONLY)   
      
SEDX - X EXCITATION DIRECTION 
SEDY - Y EXCITATION DIRECTION 
SEDZ - Z EXCITATION DIRECTION 
*END  
ANSYS   PREP    PRP7    LOPT    EXMO
EXMO,FREQB,FREQE,SIGNF  
      
EXPANDS MODES WITH SPECIFIED FREQ. RANGE (KAN=2 ONLY) 
      
FREQB, - EXPAND MODES FOR ALL FREQUENCIES GE FREQB AND LE   
FREQE     FREQE   
SIGNF  - EXPAND ONLY MODES WITHIN SIGNF OF THE MOST   
          SIGNIFICANT MODE (PERCENTAGE OF MOST SIGNIFICANT  
          MODE). DEFAULT = .001     
*END  
ANSYS   PREP    PRP7    LOPT    OMEG
OMEGA,OMEGX,OMEGY,OMEGZ 
      
SPECIFIES THE COMPONENTS OF A UNIFORM ANGULAR VELOCITY VECTOR     
  ABOUT THE ORIGIN
OMEGX - ROTATION VELOCITY ABOUT GLOBAL CARTESIAN X, Y, AND Z AXES.
OMEGY    UNITS ARE RADIANS/TIME     
OMEGZ 
*END  
ANSYS   PREP    PRP7    LOPT    DOMEGA    
DOMEGA, DOMEGAX, DOMEGAY, DOMEGAZ   
      
SPECIFIES THE COMPONENTS OF THE RATE-OF-CHANGE OF THE OMEGA VECTOR
        (UNITS ARE RADIANS/TIME**2) 
*END  
ANSYS   PREP    PRP7    LOPT    CGLOC     
CGLOC, XLOC, YLOC, ZLOC 
      
SPECIFIES THE GLOBAL CARTESIAN LOCATION OF A POINT ON AN AXIS OF  
 ROTATION FOR THE ENTIRE SYSTEM.  THE ROTATION OF THE ENTIRE SYSTEM     
 CAUSES AN ACELERATION OF THE ORIGIN OF THE STRUCTURE COORDINATE SYSTEM.
  (SEE  CGOMEGA AND DCGOMEG  COMMANDS)    
*END  
ANSYS   PREP    PRP7    LOPT    CGOMEG    
CGOMEGA, CGOMX, CGOMY, CGOMZ  
      
SPECIFIES THE GLOBAL CARTESIAN COMPONENTS OF A ROTATION VECTOR PASSING  
 THROUGH THE POINT CGLOC  AND CARRYING THE ENTIRE SYSTEM.   
*END  
ANSYS   PREP    PRP7    LOPT    DCGOMEG   
DCGOMEG, DCGOMX, DCGOMY, DCGOMZ     
      
SPECIFIES THE GLOBAL CARTESIAN COMPONENTS OF THE RATE-OF-CHANGE OF THE  
 CGOMEGA ROTATION VECTOR.     
*END  
ANSYS   PREP    PRP7    LOPT    KTEM
KTEMP,LSTP,ITER,TIME    
      
SPECIFIES THE SOURCE OF TEMPERATURES FOR THIS LOAD STEP     
      
LSTP  - IF GREATER THAN ZERO, USE LOAD STEP AND ITER FROM THE THERMAL   
         ANALYSIS FILE4 
        0 - USE TUNIF AT ALL NODES.  TIME MUST BE BLANK.    
       -1 - USE SPECIFIED ELEMENT TEMPERATURES (USE NODAL TEMPERATURES  
             IF NO ELEMENT TEMPERATURES, USE TUNIF IF NO NODAL    
             TEMPERATURES).   
       -3 - USE TEMPERATURE FROM PREVIOUS LOAD STEP   
ITER  - USE THIS ITERATION FROM THERMAL ANALYSIS FILE4 (WITH LSTP>0).   
         IF ITER=0, LSTP IS ASSUMED TO BE CUMULATIVE ITERATION NUMB.    
TIME  - SELECT DATA SET OF FILE4 AT (OR NEAREST) TIME VALUE INSTEAD     
        OF LOAD STEP AND ITERATION.  LSTP AND ITER MUST BE = 0 AND
        TIME NON-BLANK FOR TIME TO BE USED.     
*END  
ANSYS   PREP    PRP7    LOPT    TUNI
TUNIF,TEMP  
      
DEFINES THE VALUE OF THE UNIFORM TEMPERATURE TO BE USED IF KTEMP IS     
  SET TO ZERO (KTEMP = 0  INDICATES NO NODAL TEMP., ELEMENT TEMP.,
  OR TEMP. COMING FROM A PREVIOUS THERMAL ANALYSIS)   
      
TEMP - VALUE OF THE UNIFORM TEMPERATURE TO BE USED    
*END  
ANSYS   PREP    PRP7    LOPT    KUSE
KUSE,KEY    
      
SELECTS NEW OR PREVIOUSLY CREATED STIFFNESS MATRIX    
      
KEY - 0 - ANSYS LOGIC WILL SELECT NEW OR OLD STIFFNESS MATRIX     
      1 - USE OLD STIFFNESS MATRIX FOR ALL ITERATIONS 
     -1 - USE NEW STIFFNESS MATRIX FOR ALL ITERATIONS 
*END  
ANSYS   PREP    PRP7    LOPT    DMPR
DMPRAT,RATIO
      
DEFINES THE DAMPING RATIO FOR MODAL DAMPING     
  USED ONLY FOR RANDOM RESPONSE TO PSD IN KAN=2 (SVTYP,4) AND     
  FOR MODAL DAMPING IN LINEAR HARMONIC RESPONSE (KAN=6)     
      
RATIO - THE FRACTION OF CRITICAL DAMPING  
          (RATIO = 0.02 IS 2 PERCENT OF CRITICAL DAMPING)   
$END  
ANSYS   PREP    PRP7    LOPT    SVTY
SVTYP,KSV,FACT    
      
DEFINES TYPE OF SPECTRUM TABLE
      
KSV - 0 - VELOCITY SPECTRUM   
      1 - FORCE SPECTRUM
      2 - ACCELERATION SPECTRUM     
      3 - DISPLACEMENT SPECTRUM     
      4 - PSD SPECTRUM FOR RANDOM VIBRATION (ACEL**2/HERTZ) 
           ***  WARNING ***  NOTICE UNITS - MANY SPECS ARE G**2/HERTZ   
FACT - SCALE FACTOR APPLIED TO SPECTRUM VALUES (DEF. TO 1.0).  VALUES   
       ARE SCALED WHEN WRITTEN TO SOLUTION INPUT FILE.  IN-CORE   
       VALUES REMAIN THE SAME.
*END  
ANSYS   PREP    PRP7    LOPT    FREQ
FREQ,FREQ1,-- TO FREQ8  
      
DEFINES THE SPECTRUM FREQUENCY VALUES     
      
FREQ1 - DEFINE UP TO EIGHT FREQUENCY VALUES (IN ASCENDING ORDER)  
 --   
FREQ8 
*END  
ANSYS   PREP    PRP7    LOPT    SV  
SV,DAMP,SV1,-- TO SV8   
      
DEFINES THE DAMPED SPECTRUM VALUES  
      
DAMP - PERCENTAGE OF DAMPING  
SV1  - DEFINE UP TO EIGHT SPECTRUM VALUES (IN ASCENDING ORDER)    
 --   
SV8   
NOTE- SPECTRUM VALUES WILL BE SCALED BY THE FACTOR INPUT ON THE SVTYP   
      COMMAND WHEN AN LWRITE OR AFWRITE COMMAND IS ISSUED.  
*END  
ANSYS   PREP    PRP7    LOPT    MCOMB     
MCOMB,MTYP  
      
 DEFINES THE TYPE OF MODAL COMBINATION DIRECTIVES WRITTEN ON FILE24     
  FOR POST27 (KAN=2 ONLY)     
      
 MTYP - 0 - NO DIRECTIVES WRITTEN ON FILE24     
        1 - WILSON CQC DIRECTIVES WRITTEN 
        2 - NRC 10 PERCENT  METHOD DIRECTIVES WRITTEN 
        3 - DOUBLE SUM DIRECTIVES WRITTEN 
        4 - SRSS DIRECTIVES WRITTEN 
$END  
ANSYS   PREP    PRP7    LOPT    2   
USED TO DEFINE CALCULATION OPTIONS  
      
NO OPTIONS SPECIFIED    
*END  
ANSYS   PREP    PRP7    LOPT    3   
USED TO DEFINE PRINT CONTROLS 
NO OP[TIONS SPECIFIED   
*END  
ANSYS   PREP    PRP7    LOAD  
USED TO DEFINE DISPL,FORCES, AND PRESSURES
      
  D       SPECIFIES DISPLACEMENTS   
  SYMBC   GENERATES SYMMETRIC DISPLACEMENT BOUNDARY CONDITIONS    
  ASYMBC  GENERATES ANTI-SYMMETRIC DISPLACEMENT BOUND. COND.
  F       SPECIFIES FORCES    
  P       SPECIFIES PRESSURES 
  PSF     GENERATES SURFACE PRESSURES     
  LSCALE  SCALES DISPLACEMENTS, FORCES AND PRESSURES  
  (I)LIST LISTS BOUNDARY CONDITIONS (I=D,F,P)   
           ENTER  DOCU,DLIST  FOR DOCUMENTATION 
  (I)DELE DELETES DISPLACEMENT AND FORCES (I=D,F)     
           ENTER  DOCU,DDELE  FOR DOCUMENTATION 
  PDELE   DELETES PRESSURES   
           ENTER  DOCU,PDELE  FOR DOCUMENTATION 
*END  
ANSYS   PREP    PRP7    LOAD    ALL 
USED TO DEFINE DISPLACEMENTS, FORCES, AND 
  PRESSURES.
 RELATED MODULES ARE     PLOT  - TO PLOT THE LOADS    
      
D       NODE  LAB   DISP  CDISP NEND  NINC  LAB2  ....  LAB6
SYMBC   KCN   NORML VALUE TOLER     
ASYMBC  KCN   NORML VALUE TOLER     
F       NODE  LAB   FORCE CFORC NEND  NINC
P       NODE1 NODE2 PRESS ----- N1END N1INC NODE3 NODE4     
PSF     KCN   NORML LOCAT PRESS ----- TOLER SLDIR SLZER SLOPE SLKCN     
LSCALE  DFACT FFACT PFACT BFACT     
DLIST   NODE1 NODE2 NINC       (ALSO FLIST,PLIST)     
DDELE   NODE  LAB   NEND  NINC  (ALSO FDELE)    
PDELE   NODE1 NODE2 N1END N1INC NODE3 NODE4     
*END  
ANSYS   PREP    PRP7    LOAD    D   
D,NODE,LAB,DISP,CDISP,NEND,NINC,LAB2,...LAB6    
      
SPECIFIES DISPLACEMENTS 
      
NODE   - NODE NUMBER AT WHICH DISPLACEMENT IS TO BE SPECIFIED     
         (IF NODE IS ALL, CONSTRAIN ALL SELECTED  NODES)    
LAB    - DISPLACEMENT DIRECTION OR DEGREE OF FREEDOM  
          (VALID LABELS ARE ALL,UX,UY,UZ,ROTX,ROTY,ROTZ.    
          LAB=ALL IS USED TO SPECIFY DISPL. AT ALL VALID    
          DEGREES OF FREEDOM FOR THE SELECTED ELEMENT TYPES.
DISP   - VALUE OF DISPLACEMENT
NEND,  - USED TO NAME ADDITIONAL NODES WHERE SAME DISPL.    
NINC      IS SPECIFIED. DISPL. SPECIFIED FROM NODE TO NEND  
          WITH NODE INCREMENTS OF NINC    
LAB2   - OTHER LABELS AT WHICH SAME DISPLACEMENT IS SPECIFIED     
 TO LAB6    
*END  
ANSYS   PREP    PRP7    LOAD    SYMB
SYMBC,KCN,NORML,VALUE,TOLER   
      
GENERATES SYMMETRIC BOUNDARY CONDITIONS   
      
KCN   - NUMBER OF COORDINATE SYSTEM IN WHICH SYMMETRIC
         DISPLACEMENTS OCCUR  
NORML - COMPONENT OF NORMAL TO SYMMETRY SURFACE 
         0,1 - YZ SYMMETRY PLANE    
         2   - XZ SYMMETRY PLANE    
         3   - XY SYMMETRY PLANE    
VALUE - VALUE OF THE COMPONENT DEFINING THE SYMMETRY SURFACE
          IF  ALL  USE ALL SELECTED NODES.
TOLER - ALL NODES WITHIN  TOLER  TOLERANCE OF SYMMETRY SURFACE    
         HAVE SYMMETRIC BOUNDARY CONDITIONS APPLIED   
*END  
ANSYS   PREP    PRP7    LOAD    ASYM
ASYMBC,KCN,NORML,VALUE,TOLER  
      
GENERATES ANTI-SYMMETRIC BOUNDARY CONDITONS     
      
KCN   - NUMBER OF COORDINATE SYSTEM IN WHICH ANTI-SYMMETRIC 
        DISPLACEMENTS OCCUR   
NORML - COMPONENT NORMAL TO SURFACE OF ANTI-SYMMETRY  
         0,1 - ANTI-SYMMETRY ABOUT X
         2 - ANTI-SYMMETRY ABOUT Y   3 - ANTI-SYMMETRY ABOUT Z    
         TRANSLATIONAL DIRECTIONS ONLY (KTDOF=1)
VALUE - VALUE OF THE COMPONENT DEFINING THE ANTI-SYMMETRY SURFACE 
          IF  ALL  USE ALL SELECTED NODES.
*END  
ANSYS   PREP    PRP7    LOAD    F   
F,NODE,LAB,FORCE,CFORC,NEND,NINC    
      
SPECIFIES FORCES  
      
NODE  - NODE NUMBER AT WHICH FORCE IS TO BE SPECIFIED 
         (IF NODE IS ALL, PUT THIS FORCE ON ALL SELECTED NODES)   
LAB   - DIRECTION OF FORCE (VALID LABELS ARE FX,FY,FZ,MX,MY,MZ)   
FORCE - VALUE OF FORCE  
NEND, - USED TO NAME ADDITIONAL NODES WHERE SAME FORCE
         IS SPECIFIED. FORCE SPECIFIED FROM NODE TO NEND    
NINC     WITH NODE INCREMENT OF NINC
*END  
ANSYS   PREP    PRP7    LOAD    P   
P,NODE1,NODE2,PRESS,,N1END,N1INC,NODE3,NODE4    
      
SPECIFIES PRESSURES     
      
NODE1  - NUMBER OF FIRST NODE ON PRESSURE FACE  
NODE2  - NUMBER OF SECOND NODE ON PRESSURE FACE 
PRESS  - VALUE OF PRESSURE    
BLANK  - A FIELD IS SKIPPED HERE    
N1END  - USED FOR GENERATION OF MORE THAN ONE PRESSURE SURFACE.   
         NUMBER OF NODE ON THE LAST PRESSURE FACE TO BE SPECIFIED 
          (POSITION ON FACE IS SAME AS NODE1 ON FIRST PRESSURE FACE)    
N1INC  - INCREMENT BETWEEN NODE NUMBERS IN SAME POSITION ON 
          PRESSURE FACES BEING SPECIFIED  
NODE3, - NUMBER OF THIRD AND FOURTH NODES ON PRESSURE FACE  
NODE4 
*END  
ANSYS   PREP    PRP7    LOAD    PSF 
PSF,KCN,NORML,LOCAT,PRESS,,TOLER,SLDIR,SLZER,SLOPE,SLKCN    
      
GENERATES PRESSURE ON A SURFACE.  PRESSURE SLOPE MAY ALSO BE GENERATED. 
      
KCN    - COORDINATE SYSTEM OF SURFACE     
         (IF KCN IS ALL, SURFACE IS DEFINED AS ALL SELECTED NODES)
NORML  - COMPONENT OF NORMAL TO SURFACE  (1,2 OR 3)   
LOCAT  - LOCATION OF CONSTANT SURFACE COORDINATE
PRESS  - PRESSURE AT SLZER    
BLANK  - A FIELD IS SKIPPED HERE    
TOLER  - TOLERANCE FOR NODE LOCATIONS WITH RESPECT TO LOCAT 
SLDIR  - COMPONENT OF SLOPE DIRECTION  (1,2, OR 3)    
SLZER  - COORDINATE LOCATION WHERE SLOPE CONTRIBUTION IS ZERO     
SLOPE  - RATE OF CHANGE OF PRESSURE WITH COORDINATE IN SLOPE DIRECTION  
SLKCN  - COORDINATE SYSTEM OF SLOPE (DEFAULTS TO KCN) 
$END  
ANSYS   PREP    PRP7    LOAD    LSCA
LSCALE,DFACT,FFACT,PFACT
      
SCALES DISPLACEMENTS, FORCES, AND PRESSURES     
      
DFACT - SCALE ALL DISPLACEMENTS BY DFACT  
FFACT - SCALE ALL FORCES BY FFACT   
PFACT - SCALE ALL PRESSURES BY PFACT
*END  
ANSYS   PREP    PRP7    LOAD    DLIS
DLIST,NODE1,NODE2,NINC  
FLIST,NODE1,NODE2,NINC  
PLIST,NODE1,NODE2,NINC  
      
LISTS BOUNDARY CONDITIONS     
      
NODE1, - LIST SELECTED BOUNDARY CONDITION FROM NODE1 TO     
NODE2,    NODE2 WITH NODE INCREMENTS OF NINC    
NINC  
         (IF NODE1 IS ALL, LIST CONDITIONS FOR ALL SELECTED NODES)
*END  
ANSYS   PREP    PRP7    LOAD    DDEL
DDELE,NODE,LAB,NEND,NINC
FDELE,NODE,LAB,NEND,NINC
      
DELETES DISPLACEMENTS AND FORCES    
      
NODE  - NODE NUMBER AT WHICH SPECIFICATION IS TO BE DELETED 
         (IF NODE IS ALL,DELETE SPEC. FOR ALL SELECTED NODES)     
LAB   - LABEL FOR DELETED SPECIFICATION   
NEND, - DELETE SPECIFICATION FROM NODE TO NEND WITH NODE    
NINC     INCREMENTS OF NINC   
*END  
ANSYS   PREP    PRP7    LOAD    PDEL
PDELE,NODE1,NODE2,N1END,N1INC,NODE3,NODE4 
      
DELETES PRESSURES 
      
NODE1  - FIRST NODE NUMBER ON PRESSURE FACE TO BE DELETED   
         (IF NODE IS ALL, DELETE ALL PRESS ON SELECTED NODES)     
NODE2  - SECOND NODE NUMBER ON PRESSURE FACE TO BE DELETED  
N1END  - NODE NUMBER ON THE LAST PRESSURE FACE TO BE DELETED
          (POSITION ON FACE IS SAME AS NODE1 ON FIRST PRESSURE FACE)    
N1INC  - INCREMENT BETWEEN NODE NUMBERS IN SAME POSITION ON 
          PRESSURE FACES BEING DELETED    
NODE3, - NUMBER OF THIRD AND FOURTH NODES ON PRESSURE FACE  
NODE4     BEING DELETED (IF ANY)    
   (IF NODE1 IS THE LABEL  ALL  THEN ALL PRESSURES ARE DELETED.)  
*END  
ANSYS   PREP    PRP7    NTEM  
USED TO DEFINE THE NODAL TEMPERATURE DISTRIBUTION FOR A STRUCTURAL
  ANALYSIS  
      
  T       SPECIFIES A NODAL TEMPERATURE   
  TGEN    GENERATES A SET OF NODAL TEMPERATURES FROM A GIVEN PATTERN    
  TLIST   LISTS NODAL TEMPERATURES  
  TDELE   DELETES SPECIFIED NODAL TEMPERATURES  
  TSIZE   CHANGES THE SIZE OF THE TEMPERATURE TABLE   
  TREAD   READS TEMPERATURE DATA FROM FILE4 PRODUCED FROM THERMAL 
          (KAN=-1) ANALYSIS   
*END  
ANSYS   PREP    PRP7    NTEM    ALL 
USED TO DEFINE THE NODAL TEMPERATURE DISTRIBUTION FOR A STRUCTURAL
  ANALYSIS. 
      
T     NODE   TEMP  FLUEN
TGEN  ITIME  INC   NODE1 NODE2 NINC DELT  
TLIST NODE1  NODE2 NINC 
TDELE NODE1  NODE2 NINC 
TREAD LSTP   ITER   TIME
*END  
ANSYS   PREP    PRP7    NTEM    T   
T,NODE,TEMP 
      
SEPECIFES A NODAL TEMPERATURE 
      
NODE  - NODE NUMBER AT WHICH TEMPERATURE IS SPECIFIED 
TEMP  - VALUE OF NODAL TEMPERATURE  
*END  
ANSYS   PREP    PRP7    NTEM    TGEN
TGEN,ITIME,INC,NODE1,NODE2,NINC,DELT,DELF 
      
GENERATES A SET OF NODAL TEMPERATURES     
      
ITIME - TOTAL NUMBER OF TEMPERATURE SETS TO BE GENERATED (MUST BE 
         GREATER THAN 1)
INC   - INCREMENT ALL NODES IN THE GIVEN PATTERN BY INC     
NODE1 - BEGINNING AND ENDING NODE NUMBERS DEFINING THE
NODE2 -  PATTERN TO BE REPEATED (NODE2 DEFAULTS TO NODE1)   
NINC  - INCLUDE ALL NODES FROM NODE1 TO NODE2 IN STEPS OF NINC (DEFAULTS
         TO 1)    
DELT  - INCREMENTAL TEMPERATURE BETWEEN SETS    
*END  
ANSYS   PREP    PRP7    NTEM    TREAD     
TREAD,LSTP,ITER,TIME    
      
READS TEMPERATURE DATA FROM THERMAL FILE4 FROM KAN=-1 ANALYSIS.   
      
LSTP  - IF >0 READ NODAL TEMPS. FROM LOAD STEP (LSTP), ITERATION  
         (ITER) ON FILE4.     
ITER  - ITERATION NUMBER ON FILE4 ASSOCIATED WITH LSTP (USED ONLY 
         IF LSTP>0).  IF ITER=0 (OR BLANK), LSTP IS ASSUMED TO BE 
         CUMULATIVE ITERATION NUMBER.     
TIME  - USED ONLY IF LSTP AND ITER ARE ZERO (OR BLANK).  SELECT DATA    
         SET ON FILE4 AT (OR NEAREST) TIME VALUE INSTEAD OF BY    
         LOAD STEP AND ITERATION NUMBER.  
$END  
ANSYS   PREP    PRP7    RSEL  
THIS MODULE IS USED TO SELECT NODES OR ELEMENTS 
AREAS AND VOLUMES FOR OTHER PROCESSING (MODEL AND B.C. GEN, LISTS,
DELETES, PLOTS, ETC.)   
 COMMAND             PURPOSE  
+RSEL  - RESELECT FROM THE CURRENT SET OF DATA  (FORM A SUBSET)   
+ASEL  - SELECT AN ADDITIONAL SET OF DATA 
+USEL  - UN-SELECT A SET OF DATA    
+INVERT- SELECT PREVIOUSLY UNSELECTED DATA, UNSELECT PREV. SELECTED DATA
+ALL   - SELECT ALL DATA  (RESET)   
NELEM  - SELECT ONLY NODES ATTACHED TO CURRENTLY SELECTED ELEMENTS
ENODE  - SELECT ONLY ELEMENTS ATTACHED TO CURRENTLY SELECTED NODES
      
WHERE + IS (N) FOR NODES,  (E) FOR ELEMENTS     
$END  
ANSYS   PREP    PRP7    RSEL    ALL 
+RSEL   LABEL  VMIN   VMAX   VINC   KABS  
+ASEL   LABEL  VMIN   VMAX   VINC   KABS  
+USEL   LABEL  VMIN   VMAX   VINC   KABS  
+INV  
+ALL  
NELEM 
ENODE   EKEY   (0=ANY, 1=ONLY)
$END  
ANSYS   PREP    PRP7    RSEL    NRSEL     
NRSEL, LABEL, VMIN, VMAX, VINC, KABS
      
THIS COMMAND RESELECTS A SET OF NODES FOR FURTHER PROCESSING.     
      
LABEL  - A LABEL CHOSEN FROM THE SET (NODE,BLANK,X,Y,Z)     
VMIN   - MINIMUM VALUE OF LABEL TO BE SELECTED  
VMAX   - MAXIMUM VALUE OF LABEL TO BE SELECTED  
VINC   - INCREMENT OF LABEL (NODE ONLY)   
KABS   - IF KABS = 1, TAKE ABSOLUTE VALUE BEFORE TEST OF RANGE    
$END  
ANSYS   PREP    PRP7    RSEL    ERSEL     
ERSEL, LABEL, VMIN, VMAX, VINC
      
THIS COMMAND RESELECTS A SET OF ELEMENTS FOR FURTHER PROCESSING.  
      
LABEL  - A LABEL CHOSEN FROM THE SET (ELEM,TYPE,STIF,MAT,REAL)    
VMIN   - MINIMUM VALUE OF LABEL TO BE SELECTED  
VMAX   - MAXIMUM VALUE OF LABEL TO BE SELECTED  
VINC   - INCREMENT OF LABEL (ELEM,TYPE,STIF,MAT ONLY) 
$END  
ANSYS   PREP    PRP7    NMER  
USED TO MERGE COINCIDENT NODES OR AFTER THE SYMMETRY REFLECTIONS  
 TO CONNECT THE SECTIONS.     
      
MERGE  - MERGES COINCIDENT NODES AND DELETES HIGHER NODE (ACTION) 
NCOMPR - COMPRESSES NODE NUMBERS ELIMINATING NUMBERS  
          NOT USED (ACTION)   
*END  
ANSYS   PREP    PRP7    NMER    ALL 
USED TO MERGE COINCIDENT NODES.  IT IS OFTEN USED AFTER THE 
  MESH MODULE TO CONNECT THE REGIONS TOGETHER OR USED 
  AFTER THE SYMMETRY REFLECTIONS TO CONNECT THE SECTIONS.   
      
MERGE  TOLER  NODE1  NODE2  INC  (ACTION) 
NCOMP        (ACTION)   
*END  
ANSYS   PREP    PRP7    NMER    MERG
MERGE,TOLER,NODE1,NODE2,INC   
      
TO MERGE SELECTED COINCIDENT NODES TOGETHER     
      
TOLER  - ZONE OF COINCIDENCE (DEFAULTS TO 0.0001)     
NODE1,  - COMPARE ONLY NODES NODE1 TO NODE2 IN STEPS OF INC, RETAINING  
NODE2,      THOSE NODES AND ELIMINATING ANY COINCIDENT NODES. DEFAULT IS
INC         TO MERGE THE ENTIRE MODEL AND RETAIN THE LOWEST NODES.
*END  
ANSYS   PREP    PRP7    EPRE  
USED TO DEFINE ELEMENT PRESSURES    
      
  EP      DEFINES ELEMENT PRESSURES 
  EPGEN   GENERATES ADDITIONAL ELEMENT PRESSURES
  EPLIST  LISTS ELEMENT PRESSURES   
  EPDELE  DELETES ELEMENT PRESSURES 
*END  
ANSYS   PREP    PRP7    EPRE    ALL 
USED TO DEFINE ELEMENT PRESSURES (DISTRIBUTED LOADS)  
      
EP     IEL    FACE   PRESS  -----  IEND  INC    
EPGEN  ITIMES INC    IEL1   IEL2   IEINC  
EPLIST IEL1   IEL2   INC
EPDELE IEL1   IEL2   INC    IFACE   
*END  
ANSYS   PREP    PRP7    EPRE    EP  
EP,IEL,IFACE,PRESS,,IEND,INC  
      
DEFINES ELEMENT PRESSURES     
      
IEL   - NUMBER OF ELEMENT     
         (IF IEL IS  ALL, APPLY PRESSURE TO ALL SELECTED ELEMENTS)
IFACE - NUMBER OF FACE ON ELEMENT   
PRESS - VALUE OF PRESSURE     
BLANK - A FIELD IS SKIPPED HERE     
IEND, - PRESSURE APPLIES FROM ELEMENT NUMBER IEL TO ELEMENT 
INC      IEND WITH ELEMENT NUMBER INCREMENTS OF INC   
*END  
ANSYS   PREP    PRP7    EPRE    EPGE
EPGEN,ITIME,INC,NEL1,NEL2,NINC,IFACE
      
GENERATES ADDITIONAL ELEMENT PRESSURES    
      
ITIME - NUMBER OF SETS TO BE GENERATED    
INC   - ELEMENT NUMBER INCREMENT BETWEEN SETS   
IEL1, - SET IS FROM ELEMENT NUMBER IEL1 TO ELEMENT    
IEL2,    NUMBER IEL2 WITH ELEMENT NUMBER INCREMENTS   
IEINC    OF IEINC.  IF IEL1 IS ALL THEN USE ALL PRESS.
IFACE    FACE NUMBER.  IF ALL THEN USE ALL FACES.     
*END  
ANSYS   PREP    PRP7    ETEM  
USED TO DEFINE ELEMENT TEMPERATURES (MAINLY FOR ELEMENTS WHICH HAVE     
  A TEMPERATURE GRADIENT THRU THE THICKNESS - BEAMS AND SHELLS)   
  USE NTEMP MODULE FOR NODAL TEMPERATURE INPUT  
      
  TE     DEFINES AN ELEMENT TEMPERATURE   
  TEGEN   GENERATES A SET OF ELEMENT TEMPERATURES     
  TELIST  LISTS ELEMENT TEMPERATURES
  TEDELE  DELETES SPECIFIED ELEMENT TEMPERATURES
*END  
ANSYS   PREP    PRP7    ETEM    ALL 
USED TO DEFINE ELEMENT TEMPERATURES (MAINLY FOR ELEMENTS WHICH HAVE     
  A TEMPERATURE GRADIENT THRU THE THICKNESS - BEAMS AND SHELLS)   
  USE NTEMP MODULE FOR NODAL TEMPERATURE INPUT  
      
TE     IEL     T1    T2 (ETC) (6 MAX)     
TEMORE T7      T8    T9    T10   T11   T12
TEGEN  ITIME   INC   IEL1   IEL2  IEINC   
TELIST IEL1    IEL2  INC
TEDELE IEL1    IEL2  INC
*END  
ANSYS   PREP    PRP7    ETEM    TE  
TE,IEL,T1,T2,T3,T4,T5,T6
      
DEFINES AN ELEMENT TEMPERATURE
      
IEL - ELEMENT AT WHICH TEMPERATURE IS SPECIFIED 
T1  - FIRST TEMPERATURE FOR THIS ELEMENT  
T2  - SECOND TEMPERATURE FOR THIS ELEMENT 
  TO  
T6  - SIXTH TEMPERATURE FOR THIS ELEMENT  
*END  
ANSYS   PREP    PRP7    ETEM    TEGE
TEGEN,ITIME,INC,IEL1,IEL2,IEINC     
      
GENERATES A SET OF ELEMENT TEMPERATURES   
      
ITIME - TOTAL NUMBER OF TEMPERATURE SETS TO BE GENERATED (MUST BE 
         GREATER THAN 1)
INC   - INCREMENT ALL ELEMENTS IN THE GIVEN PATTERN BY INC  
IEL1  - BEGINNING AND ENDING ELEMENT NUMBERS DEFINING PATTERN     
IEL2  -  TO BE REPEATED (IEL2 DEFAULTS TO IEL1) 
IEINC - INCLUDE ALL ELEMENTS FROM IEL1 TO IEL2 IN STEPS OF IEINC  
         (DEFAULTS TO 1)
*END  
ANSYS   PREP    PRP7    INFO  
 TOPIC                RESPONSE
PURPOS - PREP7 GENERAL INFORMATION  
PROCED - STEP-BY-STEP INSTRUCTIONS FOR MOST ANALYSES  
MODULE - PREP7 MODULE DESCRIPTIONS  
ANALY  - TYPES OF ANALYSIS AVAILABLE
STIF,N - DOCUMENTATION FOR LIBRARY ELEMENT N    
PSTIF,N -  POST DATA THAT WILL BE AVAILABLE FOR LIBRARY ELEMENT N 
MISC   - DESCRIPTION OF MISCELLANEOUS FILE ACTION COMMANDS  
         (CHECK,SFWRIT,AFWRIT,SAVE,RESUME COMMANDS)   
REPT   - DESCRIPTION OF REPEAT COMMAND (ENTER DOCU,REPT)    
ICSYS  - COORDINATE SYSTEMS   
      
ENTER  DOCU,TOPIC-NAME  FOR MORE INFORMATION ON THAT TOPIC  
ENTER  DOCU,PURP  FOR INFORMATION ON HOW TO BEGIN PREP7 INPUT     
ENTER  INFO  TO REPEAT THIS TABLE   
*END  
ANSYS   PREP    PRP7    INFO    PURP
PURPOSE - TO PREPARE ANSYS INPUT DATA     
ENTER  PROCED  TO OBTAIN STEP-BY-STEP INSTRUCTIONS FOR MOST ANALYSES    
ENTER  MODULE-NAME  FOLLOWED BY  STATUS  TO DISPLAY COMMAND SETTINGS    
  (ISSUE  DOCU,MODULE  FOR MODULE NAME LIST)    
  (ENTER  DOCU  OR  DOCU,ALL  FOR AVAILABLE COMMANDS IN THAT MODULE)    
      
ENTER  INFO  TO DISPLAY INITIAL PREP7 INFORMATION TABLE     
*END  
ANSYS   PREP    PRP7    INFO    MODU
ETYPE   - DEFINE ANALYSIS AND ELEMENT TYPES     
CDSYS   - DEFINE COORDINATE SYSTEMS 
NODES   - DEFINE NODAL POINTS 
ELEMENT - DEFINE ELEMENTS     
PLOT    - PLOT NODES, ELEMENTS, LOADS     
OPTION  - SET UP ANALYSIS DATA OPTIONS    
RCON    - PREPARE THE ELEMENT REAL CONSTANT DATA
MATER   - PREPARE THE MATERIAL PROPERTY DATA    
MASTER  - DEFINE MASTER DEGREES OF FREEDOM
LOPTION - DEFINE LOAD OPTIONS (PRINT,DATA FILE,ETC)   
LOADS   - DEFINE NODAL DISPLACEMENTS,FORCES,PRESSURES 
NTEMP   - DEFINE NODAL POINT TEMPERATURES 
RSELECT - DATA BASE PROCESSOR TO SELECT (OR UNSELECT) NODES AND ELEMENTS
$END  
ANSYS   PREP    PRP7    INFO    ANAL
***** ANSYS ANALYSIS TYPES *****    
      
COMMAND    ANALYSIS TYPE
      
KAN,0    STATIC              (DEFAULT)    
KAN,2    MODE-FREQUENCY 
      
ENTER  COMMAND (AS SHOWN ABOVE)  TO SELECT ANALYSIS TYPE    
ENTER  PROC,1  FOR ADDITIONAL INFORMATION 
*END  
ANSYS   PREP    PRP7    INFO    MISC
THE FOLLOWING COMMANDS ARE ACTION COMMANDS. ENTERING THE    
COMMAND CAUSES THE DESCRIBED FUNCTION TO BE PERFORMED.
      
CHECK  - CHECKS PREP7 DATA                                 (ACTION)     
SFWRIT - WRITES A BINARY FILE (FILE3) CONTAINING THE  
          CURRENT LOADS                                    (ACTION)     
CDWRIT - WRITES BCD PREP7 INPUT FILE FROM FILE16           (ACTION)     
           (ENTER  PROC,16  FOR MORE INFORMATION)     
      
SAVE   - SAVES ALL CURRENT DATA ON RESUME FILE16           (ACTION)     
RESUME - RESTORES ALL DATA FROM THE LAST SAVED FILE16     (ACTION)
           (ENTER  PROC,16  FOR MORE INFORMATION)     
*END  
ANSYS   PREP    PRP7    INFO    REPT
RPNN,V1,V2,V3,V4,V5,... 
      
RPNN REPEATS THE COMMAND THAT IMMEDIATELY PRECEDES IT.
THE REPEAT IS DONE A TOTAL OF NN TIMES (9999 MAX).    
THE ORIGINAL COMMAND IS INCLUDED IN THE COUNT OF NN.  
EACH PARAMETER FOLLOWING RPNN INCREMENTS THE    
PARAMETER IN THE SAME ORDER ON THE PREVIOUS COMMAND   
(V1 INCREMENTS THE FIRST PARAMETER,ETC.). A BLANK OR 0
PARAMETER INDICATES NO INCREMENT.   
EXAMPLE:    
     MOVE,10,1,60,-90,999,12,999,70,999   
     RP13,1,,,7.5 
      
THE RP COMMAND WILL REPEAT THE MOVE COMMAND 12 TIMES (13    
COUNTING THE MOVE ITSELF) INCREMENTING 10 (THE NODE NUMBER) 
BY 1, NOT CHANGING 1 OR 60 (THE COORDINATE SYSTEM AND THE   
RADIUS), INCREMENTING -90 (THETA) BY 7.5, AND NOT CHANGING  
ANY OTHER PARAMETERS FROM THE MOVE COMMAND.     
*END  
ANSYS   PREP    PRP7    INFO    ICSY
 ***** PREP7 COORDINATE SYSTEMS *****     
  0   - CARTESIAN     (X,Y,Z)       NO PARAMETER
  1   - CYLINDRICAL   (R,THETA,Z)   NO PARAMETER
  2   - SPHERICAL     (R,THETA,PHI) NO PARAMETER
  3   - TOROIDAL      (R,THETA,PHI) PARAMETER=MAJOR RADIUS  
 11-40  USER DEFINED SYSTEMS (USING ANY OF THE ABOVE TYPES) 
      
ENTER  CDSY  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC
TO SET UP A COMPLETE ANALYSIS THE FOLLOWING STEPS ARE USED  
 1. DEFINE THE ANALYSIS TYPE AND ELEMENT TYPES  
      (ENTER PROC,1 FOR MORE INFORMATION) 
 2. DEFINE THE ANALYSIS OPTIONS (PROC,2)  
 3. DEFINE THE MATERIAL PROPERTIES (PROC,3)     
 4. DEFINE THE ELEMENT CONSTANTS(REAL CONST.) (PROC,4)
 5. DEFINE THE GEOMETRY OF THE STRUCTURE (PROC,5)     
 6. DEFINE COUPLED DEGREES OF FREEDOM (NOT AVAILABLE) 
 7. DEFINE CONSTRAINT EQUATIONS (NOT AVAILABLE) 
 8. FOR KAN=2, DEFINE MASTER DOF (PROC,8) 
 9. DEFINE DYNAMIC GAPS (NOT REQUIRED)    
10. DEFINE LOAD SET OPTIONS (PROC,10)     
11. DEFINE DISPLACEMENTS,FORCES,AND PRESSURES (PROC,11)     
12. DEFINE TEMPERATURE (PROC,12)    
13. MERGE COINCIDENT NODES, IF NECESSARY (PROC,13)    
14. REORDER ELEMENTS, IF NECESSARY (PROC,14)    
15. WRITE THE ANALYSIS FILE (PROC,15)     
16. FOR MORE ANALYSES,ENTER /PREP7 AND RESUME (PROC,16)     
ENTER  PROC,N (WHERE N IS NO.)  OR PROC,NEXT  OR PROC,PREV  OR PROC,SAME
*END  
ANSYS   PREP    PRP7    INFO    PROC    1 
 ***STEP 1***     
ENTER  /TITLE  .......  TO DEFINE A TITLE FOR THE ANALYSIS  
ENTER  DOCU,ANALY  TO LIST ANALYSIS TYPES - CHOOSE ONE.     
USE  STIF,N  TO REVIEW ELEMENTS     
USE  ET  COMMAND OF ETYPE MODULE TO ASSOCIATE THE ELEMENT WITH A  
     TYPE NUMBER  (ISSUE  DOCU,ET  FOR MORE INFORMATION).   
      
ENTER  ETYP  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
ENTER  PROC,NEXT  FOR NEXT PROCEDURE STEP 
*END  
ANSYS   PREP    PRP7    INFO    PROC    2 
 ***STEP 2***     
THE OPTION MODULE IS USED TO SELECT THE ANALYSIS OPTIONS    
      
ENTER  OPTI  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    3 
 ***STEP 3***     
USE THE MATERIAL MODULE TO DEFINE THE MATERIAL PROPERTIES   
 FOR ALL MATERIALS USED IN THE STRUCTURE. TEMPERATURE 
 DEPENDENT MATERIAL PROPERTIES MAY BE PLOTTED.  
      
ENTER  MATE  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    4 
 ***STEP 4***     
USE THE RCON MODULE TO SPECIFY THE GEOMETRIC DATA REQUIRED  
 FOR THE ELEMENTS USED (THICKNESS,AREA,ETC)     
 DATA REQUIRED FOR EACH ELEMENT IS IDENTIFIED AS
 REAL CONSTANTS IN THE STIF,N DESCRIPTIONS
      
ENTER  RCON  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    5 
 ***STEP 5***     
USE CDSYS MODULE TO DEFINE LOCAL COORDINATE SYSTEMS   
USE NODES MODULE TO DEFINE NODAL POINTS (N)     
USE ELEMENT MODULE TO DEFINE ELEMENTS (E) 
USE PLOT MODULE OFTEN TO VERIFY GEOMETRY  
      
ENTER  DOCU,ICSYS  FOR MORE INFORMATION   
*END  
ANSYS   PREP    PRP7    INFO    PROC    6 
 ***STEP 6***     
DEFINE COUPLED DEGREES OF FREEDOM   
THIS STEP IS NOT AVAILABLE    
*END  
ANSYS   PREP    PRP7    INFO    PROC    7 
 ***STEP 7***     
DEFINE CONSTRAINT EQUATIONS   
THIS STEP IS NOT AVAILABLE    
*END  
ANSYS   PREP    PRP7    INFO    PROC    8 
 ***STEP 8***     
FOR ANALYSIS TYPE 2, MASTER DOF MUST BE IDENTIFIED    
 THEY WILL BE IGNORED IF USED IN OTHER ANALYSIS TYPES 
 THE MASTER MODULE IS USED TO DEFINE THE MASTERS(M)   
 THE PLOT MODULE MAY BE USED TO PLOT THE MASTERS
 THE USE OF THE TOTAL,N COMMAND TO ALLOW ANSYS TO SELECT    
  ITS OWN SET OF MASTERS IS RECOMMENDED.  
      
ENTER  MAST  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    9 
 ***STEP 9***     
DEFINE DYNAMIC GAP CONDITIONS 
THIS STEP IS NOT REQUIRED.    
*END  
ANSYS   PREP    PRP7    INFO    PROC    10
 ***STEP 10***    
THE LOPTION MODULE IS USED TO SELECT THE CONTROL,     
 PRINT, AND DATA FILE OPTIONS FOR A LOAD SET    
THE LOPTIONS MODULE IS ALSO USED TO DEFINE BODY 
 LOADS SUCH AS ACCELERATION AND ROTATIONAL
 VELOCITY.  
      
ENTER  LOPT  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    11
 ***STEP 11***    
STRUCTURAL (KAN NE -1)  
USE THE LOADS MODULE TO DEFINE SPECIFIED DISPLACEMENTS (D)  
 SPECIFIED NODAL FORCES (F) AND ELEMENT PRESSURES USING     
 THE NODAL FORMAT (P). IF PRESSURE FACE IS NOT UNIQUE,
 USE ALTERNATE ELEMENT PRESSURE LOADS (EPRESS MODULE  
 EP COMMAND).     
      
 THE PLOT MODULE MAY BE USED TO PLOT N,F,P
      
ENTER  LOAD  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    12
 ***STEP 12***    
SET TEMPERATURE KEY (LOPTIONS MODULE, KTEMP COMMAND). 
 IF TEMPERATURES ARE UNIFORM, DEFINE UNIFORM TEMP.    
 (LOPTION MODULE, TUNIF COMMAND). IF NODAL TEMP.
 DISTRIBUTION IS TO BE USED, DEFINE NODAL TEMP. 
 (NTEMP MODULE, T COMMAND). IF NODAL TEMP. SPECIFI-   
 CATIONS ARE NOT SUFFICIENT (E.G.,GRADIENTS ACROSS    
 BEAMS), USE THE ETEMP MODULE, TE COMMAND.
THE TEMPERATURES MAY ALSO COME FROM AN ANSYS THERMAL  
 SOLUTION AS DEFINED IN THE LOPTION MODULE, KTEMP COMMAND.  
      
ENTER  NTEM  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT NTEMP MODULE 
*END  
ANSYS   PREP    PRP7    INFO    PROC    13
 ***STEP 13***    
USE THE NMERGE MODULE, MERGE COMMAND TO MERGE   
 COINCIDENT NODES.
      
ENTER  NMER  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    14
 ***STEP 14***    
USE THE ORDER MODULE TO REORDER ELEMENTS. 
      
ENTER  ORDE  FOLLOWED BY  DOCU, DOCU,ALL, AND/OR STAT  FOR  
   STATISTICS AND MORE INFORMATION ABOUT THIS MODULE  
*END  
ANSYS   PREP    PRP7    INFO    PROC    15
 ***STEP 15***    
AFTER THE ANALYSIS HAS BEEN COMPLETELY DEFINED THE    
 COMMAND  SFWRIT  WILL WRITE A COMPLETE SET OF DATA   
  ONTO  FILE3.   A CHECK IS DONE PRIOR TO 
 THE WRITING OF THE FILE AND THE FILE IS NOT WRITTEN  
 IF ERRORS ARE FOUND.   
USE THE COMMAND  FINISH  TO LEAVE PREP7 AND WRITE THE RESUME FILE16.    
THE ANSYS PROGRAM WILL RUN THE ANALYSIS.  
      
ENTER  DOCU,MISC  FOR MORE INFORMATION.   
*END  
ANSYS   PREP    PRP7    INFO    PROC    16
 ***STEP 16***    
TO MODIFY THE ANALYSIS, ATTACH THE MODEL FILE16,
 RE-ENTER PREP7 AND GIVE THE COMMAND  RESUME  TO RESTORE    
 THE ENTIRE ANALYSIS DATA SET AS IT EXISTED AT THE PREVIOUS FINISH.     
THE COMMAND SAVE MAY BE GIVEN AT ANY TIME TO SAVE THE 
 CURRENT DATA ON THE RESUME FILE.  IN CASE OF ERROR, THE    
 COMMAND RESUME WILL RESTORE THE DATA FROM THE LAST SAVED FILE.   
      
      
TO SEND A FILE16 TO ANOTHER SITE, ENTER PREP7 AND ISSUE THE RESUME
 COMMAND.  THEN ENTER  CDWRIT,NOUT (NOUT DEFAULTS TO 28) TO GENERATE    
 A CODED FILE CONTAINING PREP7 INPUT COMMANDS OF THE DATA THAT IS IN    
 CORE FROM THE RESUME.  AFTER THE FILE IS SENT, ENTER PREP7 AND ISSUE   
 A /INPUT,NOUT (WHERE NOUT IS THE FILE NUMBER FROM THE CDWRIT COMMAND). 
 AFTER THE DATA IS READ IN, ISSUE A  SAVE OR FINISH COMMAND TO GENERATE 
 A FILE16.  
      
ENTER  DOCU,MISC  FOR MORE INFORMATION.   
*END  
ANSYS   PREP    PRP7    INFO    PSTI
PSTIF,N     
      
DISPLAYS THE AVAILABLE STRESS DATA ON THE FILE12 STRESS RECORDS.  
ONLY THE ITEMS IN GROUPS 1 THRU 3 WILL BE DISPLAYED.  
      
ENTER  PSTIF,N  FOR ITEM LIST FOR LIBRARY ELEMENT N   
ENTER  INFO  TO DISPLAY PREP7 INITIAL INFORMATION TABLE     
$END  
ANSYS   PREP    PRP7    INFO    STIF
      
ENTER  STIF,N  FOR INFORMATION ABOUT LIBRARY ELEMENT N
*END  
ANSYS   PREP    PRP7    INFO    STIF    1 
TWO-DIMENSIONAL SPAR    
      
NUMBER OF NODES= 2
DEGREES OF FREEDOM PER NODE= 2
REAL CONSTANTS (2)=  AREA, INITSTRAIN     
PROPERTIES=  EX,ALPX,DENS     
PRESSURES=   (NONE)     
TEMPERATURES    T(I),T(J)     
KEYOPT   1 = 0 - CONSISTENT MASS MATRIX   
           = 1 - LUMPED MASS MATRIX 
*END  
ANSYS   PREP    PRP7    INFO    STIF    3 
TWO-DIMENSIONAL ELASTIC BEAM  
      
NUMBER OF NODES= 2
DEGREES OF FREEDOM PER NODE= 3
REAL CONSTANTS (5)=  AREA, IZZ, HEIGHT, SHEARZ, INITSTRAIN  
PROPERTIES=  EX ALPX NUXY DENS
PRESSURES=   LOAD PER UNIT LENGTH   
TEMPERATURES=  TTOP,TBOT
KEYOPT   5 = 1 - PRINT STRESS AT INTERMEDIATE POINTS  
KEYOPT   6 = 1 - PRINT MEMBER FORCES
*END  
ANSYS   PREP    PRP7    INFO    STIF    11
AXISYMMETRIC CONICAL SHELL    
      
NUMBER OF NODES= 2
DEGREES OF FREEDOM PER NODE= 3
REAL CONSTANTS (2)=  TK(I), TK(J)   
PROPERTIES=  EX, EY, NUXY, ALPX, ALPY, DENS     
PRESSURES=   NORMAL PRESSURE (ON FACE 1)  
TEMPERATURES=  TBOT,TTOP
KEYOPT   4 = N - PRINT AT N INTERIOR POINTS + END POINTS    
KEYOPT   5 = 1 - PRINT ELEMENT STRAINS    
KEYOPT   6 = 1 - PRINT MEMBER FORCES
*END  
ANSYS   PREP    PRP7    INFO    STIF    14
SPRING-DAMPER     
      
NUMBER OF NODES= 2
DEGREES OF FREEDOM PER NODE= 3
REAL CONSTANTS (1)=  K  
PROPERTIES=  (NONE)     
PRESSURES=   (NONE)     
TEMPERATURES=  (NONE)   
KEYOPT   2 = N - USE NTH DOF  
KEYOPT   3 = 0 - 3-D LONGITUDINAL   
             1 - 3-D TORSIONAL
             2 - 2-D LONGITUDINAL   
*END  
ANSYS   PREP    PRP7    INFO    STIF    21
GENERALIZED MASS  
      
NUMBER OF NODES= 1
DEGREES OF FREEDOM PER NODE= 6
REAL CONSTANTS (6)= MASSX, MASSY, MASSZ, IXX, IYY, IZZ (0)  
REAL CONSTANTS (36)=  6 X 6 SYMMETRIC MATRIX  (1)     
REAL CONSTANTS (1)=  MASS  (2)
REAL CONSTANTS (2)=  MASS IZZ  (3)  
REAL CONSTANTS (1)=  MASS  (4)
PROPERTIES=  (NONE)     
PRESSURES=   (NONE)     
TEMPERATURES=  (NONE)   
KEYOPT   3 = 0 - 3-D MASS WITH RI.  
             1 - 3-D MASS     
             2 - 3-D MASS WITHOUT RI.     
             3 - 2-D MASS WITH RI.  
             4 - 2-D MASS WITHOUT RI.     
*END  
ANSYS   PREP    PRP7    INFO    STIF    27
STIFFNESS, MASS, OR DAMPING MATRIX  
      
NUMBER OF NODES= 2
DEGREES OF FREEDOM PER NODE= 6
REAL CONSTANTS (36)=  6X6 SYMMETRIC MATRIX
REAL CONSTANTS (72)=  KEYOPT(3) = 1 
REAL CONSTANTS (78)=  KEYOPT(3) = 2 OR 4  
PROPERTIES=  (NONE)     
PRESSURES=   (NONE)     
TEMPERATURES=  (NONE)   
KEYOPT   3 = 0,1 - 6X6 STIFFNESS MATRIX   
             2 - 12X12 MASS MATRIX  
             4 - 12X12 STIFFNESS MATRIX   
KEYOPT   6 = 0 - OFF-DIAGONAL STIFNESS SUBMATRICES DETERMINED FROM
                  ON-DIAGONAL SUBMATRICES 
             1 - OFF-DIAGONAL STIFNESS SUBMATRICES DETERMINED FROM
                  SUBMATRICES INPUT AS SECOND SET OF REAL CONSTANTS     
*END  
ANSYS   PREP    PRP7    INFO    STIF    42
TWO-DIMENSIONAL ISOPARAMETRIC SOLID 
      
NUMBER OF NODES= 4
DEGREES OF FREEDOM PER NODE= 2
REAL CONSTANTS (0)=  IF KEYOPT(3) = 0,1,2 
REAL CONSTANTS (1)=  THICKNESS (IF KEYOPT(3) = 3)     
PROPERTIES=  EX,EY,NUXY,ALPX,ALPY,DENS,GXY (IN PLANE STRESS)
             EX,EY,EZ,NUXY,NUYZ,NUXZ,ALPX,ALPY,ALPZ,DENS,GXY (AXISYM)   
PRESSURES=   IJ,JK,KL,LI
TEMPERATURES=  T(I),T(J),T(K),T(L)  
KEYOPT   1 = 1 - ELEMENT COORD. SYSTEM PARALLEL TO I-J
KEYOPT   2 = 1 - NO EXTRA SHAPE     
KEYOPT   3 = 0 - PLANE STRESS         1 - AXISYMMETRIC
             2 - PLANE STRAIN         3 - PLANE STRESS (THICKNESS INPUT)
*END  
ANSYS   PREP    PRP7    INFO    STIF    54
TWO-DIMENSIONAL TAPERED UNSYMMETRICAL BEAM
      
NUMBER OF NODES= 2
DEGREES OF FREEDOM PER NODE= 3
REAL CONSTANTS (16)=  AREA1, IZ1, HYT1, HYB1, AREA2, IZ2    
        HYT2, HYB2, DX1, DY1, DX2, DY2, SHEARZ, AREAS1, AREAS2, EFS     
PROPERTIES=  EX, ALPX, NUXY, DENS   
PRESSURES=  QY (LOAD PER UNIT LENTGTH ON FACE 1)
TEMPERATURES= TTOP,TBOT 
KEYOPT   6 = 1 - PRINT OUT MEMBER FORCES  
*END  
ANSYS   PREP    PRP7    INFO    STIF    63
QUADRILATERAL SHELL     
      
NUMBER OF NODES= 4
DEGREES OF FREEDOM PER NODE= 6
REAL CONSTANTS (5)=  TK(I), TK(J), TK(K), TK(L), EFS  
PROPERTIES=  EX, EY, ALPX, ALPY, NUXY, DENS, GXY
PRESSURES=  NORMAL PRESSURE ACTING ON FACE 1, FACE 2  
TEMPERATURES= TTOP,TBOTTOM    
KEYOPT   1 = 0 - BENDING AND MEMBRANE STIFFNESS 
             1 - MEMBRANE STIFFNESS ONLY  
             2 - BENDING STIFFNESS ONLY   
KEYOPT   2 = 0 - ZIENKIEWICZ IN-PLANE ROT. STIFF.     
             1 - NO IN-PLANE ROT. STIFF.  
KEYOPT   3 = 1 - SUPPRESS EXTRA SHAPES    
KEYOPT   6 = 0 - FLAT SHELL PRESSURE
             1 - CURVED SHELL PRESSURE    
KEYOPT   7 = 0 - FULL MASS MATRIX   
             1 - REDUCED MASS MATRIX
*END  
