P

Deletes a defined path.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Path delete option (one of the following):

ALL - Delete all defined paths.

NAME - Delete a specific path from the list of path definitions. (Substitute the actual path name for NAME.)

Notes

Paths are identified by individual path names. To review the current list of path names, issue the command PATH,STATUS.

This command is valid in the general postprocessor.

Main Menu >General Postproc >Elec&Mag Calc >Archive Path >Path from array

Main Menu >General Postproc >Elec&Mag Calc >Delete Path >All Paths

Main Menu >General Postproc >Elec&Mag Calc >Delete Path >By Name

Main Menu >General Postproc >Path Operations >Archive Path >Path from array

Main Menu >General Postproc >Path Operations >Delete Path >All Paths

Main Menu >General Postproc >Path Operations >Delete Path >By Name

Defines the printout and screen page size.

POST1:Listing

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of lines (11 minimum) per "page" or screen. Defaults to 24. Applies to interactive non-GUI to the screen output only.

Number of characters (41 to 132) per line before wrap-around. Defaults to 80. Applies to interactive non-GUI to the screen output only.

Number of lines (11 minimum) per page. Defaults to 56. Applies to batch mode [/BATCH], diverted [/OUTPUT], or interactive GUI [/MENU] output.

Number of characters (41 to 240 (system dependent)) per line before wrap-around. Defaults to 132. Applies to batch mode [/BATCH], diverted [/OUTPUT], or interactive GUI [/MENU] output.

Notes

Defines the printout page size for batch runs and the screen page size for interactive runs. Applies to the POST1 PRNSOL, PRESOL, PRETAB, PRRSOL, and PRPATH commands. See the /HEADER command for additional controls (page ejects, headers, etc.) that affect the amount of printout. A blank (or out-of-range) value retains the previous setting. Issue /PAGE,STAT to display the current settings. Issue /PAGE,DEFA to reset the default specifications.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Writes current path information into an array variable.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

The name of the array parameter that the ANSYS program creates to store the path information. If the array parameter already exists, it will be replaced with the current path information.

Determines how data will be stored in the parameter specified with PARRAY:

POINTS - Store the path points, the nodes (if any), and coordinate system. (For information on defining paths and path points, see the descriptions of the PATH and PPATH commands.)

TABLE - Store the path data items. (See the PDEF command description for path data items.)

LABEL - Stores path data labels.

Use the PAGET command together with the PAPUT command to store and retrieve path data in array variables for archiving purposes. When retrieving path information, restore the path points (POINTS option) first, then the path data (TABLE option), and then the path labels (LABEL option).

Main Menu >General Postproc >Elec&Mag Calc >Archive Path >Path in array

Main Menu >General Postproc >Path Operations >Archive Path >Path in array

Retrieves path information from an array variable.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of the array variable containing the path information.

Specifies which path data to retrieve:

POINTS - Retrieve path point information (specified with the PPATH command and stored with the PAGET,POINTS command). The path data name will be assigned to the path points.

TABLE - Retrieve path data items (defined via the PDEF command and stored with the PAGET,,TABLE command).

LABEL - Retrieve path labels stored with the PAGET,,LABEL command.

When retrieving path information, restore path points (POINTS option) first, then the path data (TABLE option), and then the path labels (LABEL option).

Main Menu >General Postproc >Elec&Mag Calc >Archive Path >Path from array

Main Menu >General Postproc >Path Operations >Archive Path >Path from array

Restores previously saved paths from a file.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Read operation:

ALL - Read all paths from the selected file (default).

File name (32 characters maximum). Defaults to Jobname.

File name extension (8 characters maximum). Defaults to PATH if Fname is blank.

Directory name (64 characters maximum). Defaults to current directory.

This command removes all paths from virtual memory and then reads path data from a file written with the PASAVE command. All paths on the file will be restored. All paths currently in memory will be deleted.

Main Menu >General Postproc >Elec&Mag Calc >Archive Path >Paths from file

Main Menu >General Postproc >Path Operations >Archive Path >Paths from file

Reads parameters from a file.

APDL:Parameters

	Mp Me St DY LP Th E3 E2 FL PP ED

Read operation:

NEW - Replace current parameter set with these parameters (default).

CHANGE - Extend current parameter set with these parameters, replacing any that already exist.

File name (32 characters maximum). Defaults to Jobname.

File name extension (8 characters maximum). Defaults to PARM if Fname is blank.

Directory name (64 characters maximum). Defaults to current directory.

Reads parameters from a coded file. The parameter file may have been written with the PARSAV command. The parameters read may replace or change the current parameter set.

This command is valid in any processor.

Utility Menu >Parameters >Restore Parameters

Writes parameters to a file.

APDL:Parameters

	Mp Me St DY LP Th E3 E2 FL PP ED

Write operation:

SCALAR - Write only scalar parameters (default).

ALL - Write scalar and array parameters. Parameters may be numeric or alphanumeric.

File name (32 characters maximum). Defaults to Jobname.

File name extension (8 characters maximum). Defaults to PARM if Fname is blank.

Directory name (64 characters maximum). Defaults to current directory.

Writes the current parameters to a coded file. Previous parameters on this file, if any, will be overwritten. The parameter file may be read with the PARRES command.

This command is valid in any processor.

Utility Menu >Parameters >Save Parameters

Saves selected paths to an external file.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Write operation:

S - Saves only selected paths.

ALL - Saves all paths (default).

Pname - Saves the named path (from the PSEL command).

File name (32 characters maximum). Defaults to Jobname.

File name extension (8 characters maximum). Defaults to PATH if Fname is blank.

Directory name (64 characters maximum). Defaults to current directory.

Saves the paths selected with the PSEL command to an external file (jobname.path by default). Previous paths on this file, if any, will be overwritten. The path file may be read with the PARESU command.

This command is valid in /Post1.

Main Menu >General Postproc >Elec&Mag Calc >Archive Path >Paths in file

Main Menu >General Postproc >Path Operations >Archive Path >Paths in file

Defines a path name and establishes parameters for the path.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Name for this path (eight characters maximum), If nPts is blank, set the current path to the path with this name. If nPts is greater than zero, create a path of this name. If a path with this name already exists, replace it with a new path. If the NAME value is STATUS, display the status for path settings.

The number of points used to define this path. The minimum number is two, and the maximum is 1000.

The number of sets of data which you can map to this path. You must specify at least four: X, Y, Z, and S. Default is 30.

The number of divisions between adjacent points. Default is 20. There is no maximum number of divisions.

The PATH command is used to define parameters for establishing a path. The path geometry is created by the PPATH command. Multiple paths may be defined and named; however, only one path may be active for data interpolation [PDEF] and data operations [PCALC,etc.]. Path geometry points and data are stored in memory while in POST1. If you leave POST1, the path information is erased. Path geometry and data may be saved in a file by archiving the data using the PASAVE command. Path information may be restored by retrieving the data using the PARESU command.

The number of divisions defined using nDiv does NOT affect the number of divisions used by PLSECT and PRSECT.

Main Menu >General Postproc >Elec&Mag Calc >Archive Path >Path from array

Main Menu >General Postproc >Elec&Mag Calc >Archive Path >Paths from file

Main Menu >General Postproc >Elec&Mag Calc >Define Path >Defined Paths

Main Menu >General Postproc >Elec&Mag Calc >Define Path >By Location

Main Menu >General Postproc >Elec&Mag Calc >Define Path >By Nodes

Main Menu >General Postproc >Elec&Mag Calc >Define Path >On Working Plane

Main Menu >General Postproc >Elec&Mag Calc >Delete Path >All Paths

Main Menu >General Postproc >Elec&Mag Calc >Delete Path >By Name

Main Menu >General Postproc >Elec&Mag Calc >Recall Path

Main Menu >General Postproc >List Results >Path Items

Main Menu >General Postproc >Path Operations >Archive Path >Path from array

Main Menu >General Postproc >Path Operations >Archive Path >Paths from file

Main Menu >General Postproc >Path Operations >Define Path >Defined Paths

Main Menu >General Postproc >Path Operations >Define Path >By Location

Main Menu >General Postproc >Path Operations >Define Path >By Nodes

Main Menu >General Postproc >Path Operations >Define Path >On Working Plane

Main Menu >General Postproc >Path Operations >Delete Path >All Paths

Main Menu >General Postproc >Path Operations >Delete Path >By Name

Main Menu >General Postproc >Path Operations >Recall Path

Utility Menu >List >Status >General Postproc >Path Operations

Shows boundary condition symbols and values on displays.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the item:

U - Applied translational constraints (UX,UY,UZ).

ROT - Applied rotational constraints (ROTX,ROTY,ROTZ).

TEMP - Applied temperatures.

PRES - Applied fluid pressures.

V - Applied flow velocities (VX,VY,VZ).

SP0n - Mass fraction of species n, where n = 1 to 6 (FLOTRAN). If a species is given a user-defined name [MSSPEC], use that name instead of SP0n.

ENKE - Turbulent kinetic energy (FLOTRAN).

ENDS - Turbulent energy dissipation (FLOTRAN).

VOLT - Applied voltages.

MAG - Applied scalar magnetic potentials.

A - Applied vector magnetic potentials.

CHRG - Applied electric charge.

F or FORC - Applied structural forces (FX,FY,FZ).

M or MOME - Applied structural moments (MX,MY,MZ).

HEAT - Applied heat flows.

FLOW - Applied fluid flow.

AMPS - Applied current flow.

FLUX - Applied magnetic flux.

CSG - Applied magnetic current segments.

MAST - Master degrees of freedom.

CP - Coupled nodes.

CE - Nodes in constraint equations.

NFOR - POST1 nodal forces.

NMOM - POST1 nodal moments

RFOR - POST1 reaction forces.

RMOM - POST1 reaction moments (MX,MY,MZ).

PATH - Path geometry (undistorted) associated with the PATH command after a PDEFor PVECT command has been issued.

ACEL - Global acceleration (ACELX,ACELY,ACELZ vector).

OMEG - Global angular velocity (OMEGX,OMEGY,OMEGZ vector).

ALL - Represents all appropriate labels.

Unused field.

Symbol key:

0 - Do not show symbol.

1 - Show symbol.

2 - Plot value next to symbol.

Minimum value in a range of values plotted on screen.

Maximum value in a range of values plotted on screen.

Absolute number. If KEY = 2 and ABS = 0, a number falling between the MIN and MAX is displayed. If ABS is not specified, it defaults to 0. If KEY = 2 and ABS = 1, an absolute value falling between the MIN and MAX is displayed. ABS = 1 lets you eliminate the display of numbers whose absolute values are less than a desired tolerance. For example, if ABS = 1, MIN = 10 and MAX = 1e8, values such as .83646 and -5.59737 are not displayed.

Notes

Adds degree of freedom constraint, force load, and other symbols to displays. Symbols are applied to the selected nodes only. All arrow and arrowhead symbols are oriented in the nodal coordinate system and lie in two perpendicular planes. Force arrows are scaled proportional to their magnitude. (If KEY = 1, use /VSCALE to change arrow length.) For scalar quantities, the specific component direction (i.e., x, y, or z) of the symbol has no meaning, but the positive or negative sense (e.g., positive or negative x) represents a positive or negative scalar value, respectively. Use /PSTATUS or /PBC,STAT to display settings. Use /PBC,DEFA to reset all specifications back to default. See the /PSF and /PBF commands for other display symbols.

Issuing the command /PBC,PATH,1 displays all defined paths.

The /PBC command is valid in any processor.

Utility Menu >PlotCtrls >Symbols

Shows body force loads as contours on displays.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the item:

TEMP - Applied temperatures.

FLUE - Applied fluences.

HGEN - Applied heat generation rates.

JS - Applied current density magnitude.

JSX - X-component of current density.

JSY - Y-component of current density.

JSZ - Z-component of current density.

PHASE - Phase angle of applied load.

MVDI - Applied magnetic virtual displacements flag.

CHRGD - Applied electric charge density.

VLTG - Applied voltage drop.

FORC - Applied force density (FLOTRAN only).

Unused field.

Symbol key:

0 - Do not show body force load contours.

1 - Show body force load contours.

Notes

Shows body force loads as contours on displays for the selected elements. Use /PSTATUS or /PBF,STAT to display settings. Use /PBF,DEFA to reset all specifications back to default. See also the /PSF and /PBC command for other display contours.

This command is valid in any processor.

Utility Menu >PlotCtrls >Symbols

Forms additional labeled path items by operating on existing path items.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Type of operation to be performed. See notes below for specific descriptions of each operation:

ADD - Adds two existing path items.

MULT - Multiplies two existing path items.

DIV - Divides two existing path items (a divide by zero results in a value of zero).

EXP - Exponentiates and adds existing path items.

DERI - Finds a derivative.

INTG - Finds an integral.

SIN - Sine.

COS - Cosine.

ASIN - Arcsine.

ACOS - Arccosine.

LOG - Natural log.

Label assigned to the resulting path item.

First labeled path item in operation.

Second labeled path item in operation. Lab2 must not be blank for the MULT, DIV, DERI, and INTG operations.

Factor applied to Lab1 (defaults to 1.0).

Factor applied to Lab2 (defaults to 1.0).

Constant value (defaults to 0.0).

If Oper = ADD, the command format is:

This operation adds two existing path items according to the operation:

It may be used to scale the results for a single path item.

If Oper = MULT, the command format is:

Lab2 must not be blank. This operation multiplies two existing path items according to the operation:

If Oper = DIV, the command format is:

Lab2 must not be blank. This operation divides two existing path items according to the operation:

If Oper = EXP, the command format is:

This operation exponentiates and adds existing path items according to the operation:

If Oper = DERI, the command format is:

Lab2 must not be blank. This operation finds a derivative according to the operation:

If Oper = INTG, the command format is:

Lab2 must not be blank. This operation finds an integral according to the operation:

Use S for Lab2 to integrate Lab1 with respect to the path length. S, the distance along the path, is automatically calculated by the program when a path item is created with the PDEF command.

Main Menu >General Postproc >Path Operations >Add

Main Menu >General Postproc >Path Operations >ArcCosine

Main Menu >General Postproc >Path Operations >ArcSine

Main Menu >General Postproc >Path Operations >Cosine

Main Menu >General Postproc >Path Operations >Differentiate

Main Menu >General Postproc >Path Operations >Divide

Main Menu >General Postproc >Path Operations >Exponentiate

Main Menu >General Postproc >Path Operations >Integrate

Main Menu >General Postproc >Path Operations >Multiply

Main Menu >General Postproc >Path Operations >Natural Log

Main Menu >General Postproc >Path Operations >Sine

Creates a circular area centered about the working plane origin.

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

Inner and outer radii (either order) of the circle. A value of either zero or blank for either RAD1 or RAD2, or the same value for both RAD1 and RAD2, defines a solid circle.

Starting and ending angles (either order) of the circular area. Used for creating a circular sector. The sector begins at the algebraically smaller angle, extends in a positive angular direction, and ends at the larger angle. The starting angle defaults to 0.0° and the ending angle defaults to 360.0°. See the ANSYS Modeling and Meshing Guide for an illustration.

Defines a solid circular area or circular sector centered about the working plane origin. For a solid circle of 360°, the area will be defined with four keypoints and four lines. See the CYL4 and CYL5 commands for alternate ways to create circles.

Main Menu >Preprocessor >Create >Circle >By Dimensions

Creates an annotation circle (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Circle X center location (-1.0 < X < 2.0).

Circle Y center location (-1.0 < Y < 1.0).

Circle radius length.

Creates an annotation circle to be written directly onto the display at a specified location. This is a command generated by the Graphical User Interface (GUI) and will appear in the log file (Jobname.LOG) if annotation is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

All circles are shown on subsequent displays unless the annotation is turned off or deleted. Use the /LSPEC and the /PSPEC command to set the attributes of the circle.

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Sets convergence values for p-method solutions.

SOLUTION:p-MethodOptions

	Mp Me St -- LP -- -- -- -- PP ED

Tolerance (as a percentage) used for convergence checking. The analysis is considered to be converged if the values of all specified items change by less than TOLER at the end of a p-loop. Defaults to 5. If TOLER = STAT, list the currently specified p-convergence criteria. If TOLER = ERASE, erase all p-convergence specifications. If TOLER = DELE, delete only the tolerance for the specification denoted by the Item, Comp, NODE.

Convergence based on (Valid component labels are described in the table below):

SE - Strain energy (default). Does not require a component label.

S - Stress.

EPEL - Strain.

U - Translational displacement.

ROT - Structural rotation. (Valid only for SHELL150.)

Component of the Item. (Not required for Item = SE). If Item = S or EPEL, Comp defaults to EQV; if Item = U or ROT, Comp defaults to SUM. Valid component labels for each Item are described in the table below.

Node number where convergence checking is to be performed. Valid only for Item = S, EPEL, U, and ROT. For valid Item labels, a node number must be entered in this field. If NODE = P, graphical picking is enabled (valid only in the GUI). A component name may be substituted for NODE.

Surface of a p-element shell structure where the convergence checking for NODE will be performed. Valid only for Item = S or EPEL.

TOP - Top surface (default).

MID - Middle surface.

BOT - Bottom surface.

Notes

When you use the menu paths to delete p-method convergence criteria, the ANSYS program writes the command PCONV,DELE,n to its log file.

The p-level (polynomial level, i.e., the order or level n of a polynomial, where 2 n 8) is increased for each loop until the values of the specified items (Item,Comp) change less than the specified tolerance (TOLER) between loops, or until the maximum p-level has been reached [PPRANGE]. Convergence checking is performed only on included elements [PINCLUDE]. Up to 10 separate specifications may be activated at one time. Valid Item and Comp labels are shown next.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >p-Method >Convergence Crit

Main Menu >Solution >p-Method >Convergence Crit

Automatically generates hard copies for HP Unix work stations.

GRAPHICS:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Copy key:

0 - No specification setting for automatic hard copy of display.

1 - Set specification for automatic hard copy after each display.

NOW - (Action) Produce hard copy of current display (KEY is not reset to 1).

Notes

Sets automatic hard copy specification. This command is available only on HP work stations, and only during interactive runs with the /SHOW specification active (for terminals with hard copy capability).

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Specifies the allowable exterior corrosion thickness for a piping run.

PREP7:Piping

	Mp Me St -- LP -- -- -- -- PP ED

Allowable corrosion thickness.

Specifies the allowable exterior corrosion thickness for a piping run. See the PREP7 RUN command.

Main Menu >Preprocessor >Create >Piping Models >Specifications

Calculates the cross product of two path vectors along the current path.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to X-component of resultant vector.

Label assigned to Y-component of resultant vector.

Label assigned to Z-component of resultant vector.

X-component of first vector label (labeled path item).

Y-component of first vector label.

Z-component of first vector label.

X-component of second vector label (labeled path item).

Y-component of second vector label.

Z-component of second vector label.

Main Menu >General Postproc >Path Operations >Cross Product

Interpolates an item onto a path.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to the resulting path item (8 characters maximum). This item may be used as input for other path operations.

Label identifying the item for interpolation. Valid item labels are shown in the table below. Some items also require a component label.

Component of the item (if required). Valid component labels are shown in the table below.

Option to average across element boundaries:

AVG - Average element results across elements (default).

NOAV - Do not average element results across elements. If the parameter DISCON=MAT on the PMAP command, this option is automatically invoked.

Defines and interpolates a labeled path item along a predefined path [PATH]. Path item results are in the global Cartesian coordinate directions unless transformed [RSYS]. A path item must be defined before it can be used with other path operations. Additional path items may be defined from the PVECT, PCALC, PDOT, and PCROSS commands. Path items may be listed [PRPATH] or displayed [PLPATH, PLPAGM]. A maximum number of path items permitted is established by the nSets argument specified with the PATH command.

When you create the first path item [PDEFor PVECT], the program automatically interpolates four path items which are used to describe the geometry of the path. These predefined items are the position of the interpolated path points (labels XG, YG, and ZG) in global Cartesian coordinates, and the path length (label S). For alternate methods of mapping the path geometry (to include, for example, material discontinuity) see the PMAP command. These items may also be listed or displayed with the PRPATH, PLPATH and PLPAGM commands.

The number of interpolation points on the path is defined by the nDiv argument on the PATH command. See also Section 19.3 of the ANSYS Theory Reference for details. Use PDEF,STAT to list the path item labels. Use PDEF,CLEAR to erase all labeled path items, except the path geometry items (XG, YG, ZG, S).

Main Menu >General Postproc >Elec&Mag Calc >Define Path >Current Path

Main Menu >General Postproc >Elec&Mag Calc >Define Path >By Nodes

Main Menu >General Postproc >Elec&Mag Calc >Define Path >On Working Plane

Main Menu >General Postproc >Elec&Mag Calc >Recall Path

Main Menu >General Postproc >Path Operations >Clear Path Items

Main Menu >General Postproc >Path Operations >Define Path >Current Path

Main Menu >General Postproc >Path Operations >Define Path >By Nodes

Main Menu >General Postproc >Path Operations >Define Path >On Working Plane

Main Menu >General Postproc >Path Operations >Map onto Path

Main Menu >General Postproc >Path Operations >Recall Path

Calculates the dot product of two path vectors along the current path.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to dot product result.

X-component of first vector label (labeled path item).

Y-component of first vector label (labeled path item).

Z-component of first vector label (labeled path item).

X-component of second vector label (labeled path item).

Y-component of second vector label (labeled path item).

Z-component of second vector label (labeled path item).

Main Menu >General Postproc >Path Operations >Dot Product

Defines the external fluid drag loading for a piping run.

PREP7:Piping

	Mp Me St -- LP -- -- -- -- PP ED

External fluid drag pressure (global Cartesian components) at height H1.

Height (along Kcord coordinate) for first drag pressure.

External fluid drag pressure (global Cartesian components) at height H2.

Height (along Kcord coordinate) for second drag pressure.

Coordinate direction for height value (in the global Cartesian coordinate system):

X - X coordinate.

Y - Y coordinate (default).

Z - Z coordinate.

Defines the external fluid drag loading (pressure) as a function of height for a piping run. See the PREP7 RUN command. The element drag pressure is determined from the centroid height and linear interpolation. Pressures are assigned to the elements as they are generated.

Main Menu >Preprocessor >Create >Piping Models >Loads

Generates periodic constraints for 2-D planar magnetic field analyses.

PREP7:SpecialPurpose

	Mp Me St DY -- -- E3 E2 -- PP ED

Constant coordinate location of the first plane of nodes. For PLNOPT=1 or 2, the constant coordinate location is the global Cartesian coordinate system [CSYS,0] location in the X or Y direction respectively. For PLNOPT=0, the location is the angle in the global cylindrical coordinate system [CSYS,1].

Constant coordinate location of the second plane of nodes. For PLNOPT=1 or 2, the constant coordinate location is the global Cartesian coordinate system [CSYS,0] location in the X or Y direction respectively. For PLNOPT=0, the location is the angle (in degrees) in the global cylindrical coordinate system [CSYS,1].

Tolerance on the constant coordinate location for node selection. Defaults to .00001 for PLNOPT = 1 or 2 and .001 degrees for PLNOPT=0.

Minimum coordinate location along the second plane of nodes. For PLNOPT=1 or 2, the coordinate location is the global Cartesian coordinate system location in the Y or X direction respectively. For PLNOPT=0, the coordinate location is the radial coordinate value in the global cylindrical coordinate system. Periodic conditions are not applied to nodes at this location.

Maximum coordinate location along the second plane of nodes. For PLNOPT=1 or 2, the coordinate location is the global Cartesian coordinate system location in the Y or X direction respectively. For PLNOPT=0, the coordinate location is the radial coordinate value in the global cylindrical coordinate system. Periodic conditions are not applied to nodes at this location.

Tolerance dimension on node selection along the plane of nodes. Defaults to .00001.

Periodic option:

0 - Odd symmetry (default). Apply constraint equations such that AZ(i)=-AZ(j).

1 - Even symmetry. Apply node coupling such that AZ(i)=AZ(j).

Symmetry plane option:

0 - Planes of constant angle in the global cylindrical coordinate system [CSYS,1].

1 - Planes parallel to the global Cartesian X axis [CSYS,0].

2 - Planes parallel to the global Cartesian Y axis [CSYS,0].

PERBC2D invokes an ANSYS macro which generates periodic boundary condition constraints for two-dimensional planar magnetic field analysis. The macro is restricted to node pairs sharing common coordinate values along symmetry planes separated by a constant coordinate value. Planes (or lines) must lie at either constant angles (PLNOPT=0), constant X values (PLNOPT=1), or constant Y values (PLNOPT=2). PERBC2D applies constraint equations (OPT=0, odd symmetry) or node coupling (OPT=1, even symmetry) to each node pair sharing a common coordinate value along the symmetry planes. By default, periodic conditions are not applied at the first and last node pairs on the symmetry planes unless the input location values, R1 and R2, are adjusted to be less than or greater than the actual node coordinate values. Nodes are selected for application of the constraints using the NSEL command with tolerances on the constant coordinate location (LOCTOL) and the coordinate location along the plane (RTOL).

Main Menu >Preprocessor >Loads >Apply >Boundary >Periodic BCs

Main Menu >Solution >Apply >Boundary >Periodic BCs

Specifies elements to be excluded from p-level escalations.

SOLUTION:p-MethodOptions

	Mp Me St -- LP -- -- -- -- PP ED

Element number of element to be excluded. If ELEM = ALL, exclude all elements. If ELEM = STAT, give status of excluded elements. If ELEM = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for ELEM.

Notes

The elements chosen by this command will be excluded from convergence calculations. As as a result, these elements will not have their p-levels increased throughout the solution iterations.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >p-Method >Exclude Elems

Main Menu >Solution >p-Method >Exclude Elems

Calculates participation factors for the PSD or multi-point response spectrum table.

SOLUTION:SpectrumOptions

	Mp Me St -- -- -- -- -- -- PP ED

Input PSD table number for which participation factors are to be calculated.

Label defining the location of excitation:

BASE - Base excitation (default).

NODE - Nodal excitation.

Label defining excitation type (applies only to SPOPT,PSD analysis). Used only when partially correlated excitation is due to wave propagation or spatial correlation. Defaults to partially correlated excitation as defined by COVAL and QDVAL commands.

WAVE - Excitation defined by PSDWAV command.

SPAT - Excitation defined by PSDSPL command.

Calculates the participation factors for a particular PSD or multi-point response spectrum table defined with the PSDVAL command. The Jobname.DB file must contain modal solution data in order for this command to calculate the participation factor. There must be a PFACT command for each excitation spectrum.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Spectrum >Calculate PF

Main Menu >Solution >Spectrum >Calculate PF

Defines the contained fluid density for a piping run.

PREP7:Piping

	Mp Me St -- LP -- -- -- -- PP ED

Density of the contained fluid.

See the PREP7 RUN command.

Main Menu >Preprocessor >Create >Piping Models >Specifications

Defines a spring-gap constraint in a piping run.

PREP7:Piping

	Mp Me St -- LP -- -- -- -- PP ED

Node where gap is to be placed. Defaults to current run starting point.

Spring constant value (must be positive).

Increment (in terms of the active coordinate system components) to determine gap ground point. Element length must not be zero. Constraints are automatically generated at the ground point.

Gap size (defaults to the element length).

Element number to be assigned to gap (defaults to MAXEL + 1).

Defines a spring-gap constraint (gap element, CONTAC52) at a given location in a piping run. Gives spring constraint resistance after a specified gap is closed. See the RUN command.

Main Menu >Preprocessor >Create >Piping Models >Spring-Gap Supp

Writes, reads, or lists all element information

PREP7:SpecialPurpose

	Mp Me St DY LP Th E3 E2 FL PP ED

Specifies what to do with element information:

WRITE - Write all appropriate element types, key options, real constants, material properties, solution analysis options, load step options, constraint equations, coupled nodes, defined components, and GUI preference settings to the file specified with the Fname, Ext, and Dir arguments.

READ - Deletes all solution information (material properties, solution options, load step options, constraint equations, coupled nodes, results, and GUI preference settings) then reads all the information listed above into the ANSYS database from the location specified by the Fname, Ext, and Dir arguments.

LIST - Lists currently defined physics files and their titles.

DELETE - Deletes a specified physics file and its title from the database.

CLEAR - Deletes all material properties, solution options, load step options, constraint equations, coupled nodes, results, and GUI preference settings from the database.

STATUS - Displays information about all active elements and settings.

A user-defined title that quickly identifies a set of physics settings. For example, you might use "Fluid," "Structural," or "Magnetic" as titles. A title can contain up to 64 characters.

File name (32 characters maximum). Defaults to Jobname. Previous data on this file, if any, are overwritten.

File name extension (eight characters maximum). Defaults to PHn if Fname is blank, where n is a number between 1 and 9 depending on how many times you have issued the PHYSICS command. (You can have up to nine separate physics files.) If you issue the command more than nine times, the ANSYS program will require you to delete an existing file.

Directory name (64 characters maximum). Default is the current directory.

Use the PHYSICS command when you are performing a multiphysics analysis that involves two different disciplines (for example, CFD and structural analysis) and you cannot solve both analyses simultaneously. Once you have set up physics environments for both analyses, you can use the PHYSICS,READ command to change between the defined physics environments. For more information about doing multiphysics analyses, see Chapter 2 of the ANSYS Coupled-Field Analysis Guide.

The PHYSICS command outputs all solution information, including analysis options, to the Jobname.PHn file described above. Although it also outputs components, the ANSYS program does not list entities (nodes, elements, lines, etc.).

Main Menu >Preprocessor >Physics Environ >Clear

Main Menu >Preprocessor >Physics Environ >Delete

Main Menu >Preprocessor >Physics Environ >List

Main Menu >Preprocessor >Physics Environ >Read

Main Menu >Preprocessor >Physics Environ >Status

Main Menu >Preprocessor >Physics Environ >Write

Main Menu >Solution >Physics Environ >Clear

Main Menu >Solution >Physics Environ >Delete

Main Menu >Solution >Physics Environ >List

Main Menu >Solution >Physics Environ >Read

Main Menu >Solution >Physics Environ >Status

Main Menu >Solution >Physics Environ >Write

Specifies elements to be included in p-level escalations.

SOLUTION:p-MethodOptions

	Mp Me St -- LP -- -- -- -- PP ED

Element number of element to be included. If ELEM = ALL, include all elements. If ELEM = STAT, give status of included elements. If ELEM = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for ELEM.

Notes

The elements chosen by this command may have their p-levels increased throughout the solution iterations.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >p-Method >Include Elems

Main Menu >Solution >p-Method >Include Elems

Defines the external insulation constants in a piping run.

PREP7:Piping

	Mp Me St -- LP -- -- -- -- PP ED

Insulation density.

Insulation thickness.

Notes

Defines the external insulation constants in a piping run. See the RUN command.

Main Menu >Preprocessor >Create >Piping Models >Specifications

Specifies "Pipe modeling" as the subsequent status topic.

PREP7:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

This is a status [STAT] topic command. Status topic commands are generated by the GUI and will appear in the log file (Jobname.LOG) if status is requested for some items under Utility Menu>List>Status. This command will be immediately followed by a STAT command, which will report the status for the specified topic.

If entered directly into the program, the STAT command should immediately follow this command.

Utility Menu >List >Status >Preprocessor >Piping Module

Prevents a batch mode, linear static analysis from stopping when a negative or zero equation solver pivot value is encountered.

SOLUTION:AnalysisOptions

	Mp Me St -- LP Th E3 E2 -- PP ED

Determines whether to stop or continue an analysis when a negative or zero equation solver pivot value is encountered:

ON - Default value. ANSYS checks for negative or zero pivot values on linear static analyses performed with the frontal, sparse and PCG solvers. When one is encountered, an error is issued, stopping the job. A negative pivot value may be valid for some Multiphysics analyses (e.g. EMAG or Thermal); this key has no effect in these cases.

OFF - Pivots will not be checked. This key continues the analysis in spite of a zero or negative pivot value. The program will proceed until other error checking routines are encountered.

Notes

This command is valid only for linear static analyses. In a nonlinear analysis, a negative pivot may be valid. Normally, rigid body motions in a nonlinear analysis will be trapped by error routines checking infinitely large displacements (DOF limit exceeded) or non-convergence status. An under-constrained model may avoid the pivot check, but fail with a DOF limit exceeded error.

This command is applicable only to batch mode (not in the GUI). While in an ANSYS interactive session, it is generally desirable to remain in the session, even though a pivot error has occurrred. Warning messages will be displayed on the screen, allowing the user to take corrective action.

Finally, machine precision will determine if a warning or an error is issued for the small pivot case. In all cases there will be some notification that the model needs to be checked closely for an accurate solution.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Specifies a free-space time-harmonic electromagnetic wave.

SOLUTION:MiscLoads

	Mp Me St -- -- -- E3 E2 -- PP ED

Amplitude of the electric field.

Phase angle of the electric field (in degrees).

Component values of an electric field polarization vector designating the electric field polarization in the global (x,y,z) coordinate systems. The three vector components represent the end point of a vector used to position the electric field.

Component values of a plane wave propagation vector in the global (x,y,z) coordinate systems. The three vector components represent the end point of a vector used to position the electric field propagation direction. The magnitude of the resulting vector is irrelevant.

This command specifies an incident plane wave for the entire solution domain.

Main Menu >Preprocessor >Loads >Apply >Excitation >Wave Status

Main Menu >Solution >Apply >Excitation >Wave Status

Main Menu >Preprocessor >Loads >Apply >Excitation >Define wave

Main Menu >Solution >Apply >Excitation >Define wave

Plots the convergence curve for specified items from a p-method solution.

POST1:Results

	Mp Me St DY LP -- -- -- -- PP ED

Label identifying the convergence criterion to be plotted. (Valid component labels are described in the table below.)

ALL - Simultaneously plot the convergence curve for all specified Item criteria versus p-level (default). Does not require a component label.

SE - Plot strain energy curve versus p-level. Does not require a component label.

S - Plot stress curve versus p-level. Valid component labels are described in the table below.

EPEL - Plot strain curve versus p-level. Valid component labels are described in the table below.

U - Plot translational displacement curve versus p-level. Valid component labels are described in the table below.

ROT - Plot structural rotation versus p-level (valid only for SHELL150).

Component of the Item. Not required for Item = ALL and SE. Valid Comp values (and associated Item values) are shown below. (Defaults to ALL: plot the convergence curve for all Item and Comp criteria simultaneously.)

Node number where convergence checking was performed. Valid only for Item = S, EPEL, U, or ROT. Defaults to all nodes having Item and Comp previously specified as convergence criteria [PCONV].

Surface of a p-element shell structure where the convergence curve for NODE will be plotted. Valid only for Item = S or EPEL. Defaults to all surfaces.

TOP - Top surface (default).

MID - Middle surface

BOT - Bottom surface.

Notes

The previously specified convergence criterion [PCONV] is graphed versus the characteristic p-level. The characteristic p-level is the polynomial level range from the minimum defined [PPRANGE] to the maximum p-level reached by any element in the model. The Item value corresponds to the convergence criterion indicated by PCONV. All Items previously designated by the PCONV command will be plotted.

Main Menu >General Postproc >Plot Results >p-Convergence

Specifies the part of a complex variable to display.

POST26:Display

	Mp Me St DY LP -- E3 E2 -- PP ED

Complex variable part:

0 - Amplitude.

1 - Phase angle.

2 - Real part.

3 - Imaginary part.

Used only with harmonic analyses (ANTYPE=HARMIC).

Main Menu >TimeHist Postpro >Settings >Graph

Displays cracking and crushing locations in SOLID65 elements.

POST1:SpecialPurpose

	Mp Me St -- -- -- -- -- -- PP ED

Location at which symbols are to be displayed:

0 - Plot symbols at integration points (default).

1 - Plot symbol at element centroids (averaged).

Crack to be displayed:

0 - Plot all cracks (default).

1 - Plot only the first crack.

2 - Plot only the second crack.

3 - Plot only the third crack.

PLCRACK displays circles at locations of cracking or crushing in concrete elements. Cracking is shown with a circle outline in the plane of the crack, and crushing is shown with an octahedron outline. If the crack has opened and then closed, the circle outline will have an X through it. Each integration point can crack in up to three different planes. The first crack at an integration point is shown with a red circle outline, the second crack with a green outline, and the third crack with a blue outline.

Symbols shown at the element centroid (LOC=1) are based on the status of all of the element's integration points. If any integration point in the element has crushed, the crushed (octahedron) symbol is shown at the centroid. If any integration point has cracked or cracked and closed, the cracked symbol is shown at the element centroid. If at least five integration points have cracked and closed, the cracked and closed symbol is shown at the element centroid. Finally, if more than one integration point has cracked, the circle outline at the element centroid shows the average orientation of all cracked planes for that element.

Main Menu >General Postproc >Plot Results >Crack/Crush

Displays the displaced structure.

POST1:Results

	Mp Me St DY LP -- -- -- -- PP ED

Undisplaced shape key:

0 - Display only displaced structure.

1 - Overlay displaced display with similar undisplaced display (appearance is system-dependent).

2 - Same as 1 except overlay with undisplaced edge display (appearance is system-dependent).

Displays the displaced structure for the selected elements.

For information on true scale plots, refer to the description of the /DSCALEcommand [/DSCALE,,1.0].

Main Menu >General Postproc >Plot Results >Deformed Shape

Utility Menu >Plot >Results >Deformed Shape

Utility Menu >PlotCtrls >Animate >Deformed Shape

Displays the solution results as discontinuous element contours.

POST1:Results

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the item. Valid item labels are shown in the table below. Some items also require a component label.

Component of the item (if required). Valid component labels are shown in the table below.

Undisplaced shape key:

0 - Do not overlay undeformed structure display

1 - Overlay displaced contour plot with undeformed display (appearance is system-dependent)

2 - Overlay displaced contour plot with undeformed edge display (appearance is system-dependent)

Scale factor for 2-D display of contact items (defaults to 1). A negative scaling factor may be used to invert the display.

Displays the solution results as element contours discontinuous across element boundaries for the selected elements. For example, PLESOL,S,X displays the X component of stress S (i.e., the SX stress component). Various element results depend on the calculation method and the selected results location (AVPRIN, RSYS, and ESEL). Contours are determined by linear interpolation within each element, unaffected by the surrounding elements (i.e., no nodal averaging is performed). The discontinuity between contours of adjacent elements is an indication of the gradient across elements. Component results are displayed in the active results coordinate system [RSYS] (default is the global Cartesian). See the ETABLE and PLETAB commands for displaying items not available through this command (such as line element results).

For PowerGraphics displays [/GRAPHICS,POWER], results are plotted only for the model exterior surface. The items marked with * in the table below are supported by PowerGraphics.

Main Menu >General Postproc >Plot Results >Element Solu

Utility Menu >Plot >Results >Contour Plot >Elem Solution

Displays element table items.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

User-defined label, as specified with the ETABLE command, of item to be displayed.

Averaging operation:

NOAV - Do not average element items at common nodes (default).

AVG - Average the element items at common nodes.

Displays items stored in the table defined with the ETABLE command for the selected elements. For display purposes, items are assumed to be constant over the element and assigned to each of its nodes. Contour display lines (lines of constant value) are determined by linear interpolation within each element from the nodal values. These nodal values have the option of being averaged (values are averaged at a node whenever two or more elements connect to the same node) or not averaged (discontinuous). The discontinuity between contour lines of adjacent elements is an indication of the gradient across elements.

Main Menu >General Postproc >Element Table >Plot Elem Table

Main Menu >General Postproc >Plot Results >Elem Table

Utility Menu >Plot >Results >Contour Plot >Elem Table Data

Generates a contour line plot of equipotentials.

POST1:Magnetics

	Mp Me St -- -- -- E3 E2 -- PP ED

Number of contour lines to display. Issue in multiples of 9 (i.e., 9, 18, 27, etc.). Default is 27 contour lines.

Overlay:

0 - Overlay edge outlines by material number.

1 - Overlay edge outlines by real constant number.

Highest material or real constant attribute number. Command will cycle through ANUM element display overlays. Defaults to 10.

Window number to which command applies. Defaults to 1.

PLF2D invokes an ANSYS macro which plots equipotentials of the degree of freedom AZ. These equipotential lines are parallel to flux lines and thus give a good representation of flux patterns. In the axisymmetric case, the display is actually r*AZ where "r" is the node radius. The macro overlays (OLAY) edge outlines by material number or real constant number (ANUM) and allows user control over the number of contour lines to display (NCONT).

Main Menu >General Postproc >Plot Results >2D Flux Lines

Utility Menu >Plot >Results >Flux Lines

Displays element table items as contoured areas along elements.

POST1:ElementTable

	Mp Me St DY LP Th -- -- -- PP ED

Label of element table item [ETABLE] for node I magnitude.

Label of element table item for node J magnitude.

Scale factor for display (defaults to 1). A negative scaling factor may be used to invert the display.

Undisplaced shape key:

0 - Do not overlay undeformed structure display

1 - Overlay displaced contour plot with undeformed display (appearance is system-dependent)

2 - Overlay displaced contour plot with undeformed edge display (appearance is system-dependent)

Displays selected items (e.g., shears and moments) as a contoured area (trapezoid) display along line elements and 2-D axisymmetric shell elements (e.g., shear and moment diagrams). Three sides of the trapezoid are formed by the element (one side) and lines at nodes I and J of length proportional to the item magnitude and displayed normal to the element and the viewing direction (the two parallel sides).

Main Menu >General Postproc >Plot Results >Line Elem Res

Displays results as continuous contours.

POST1:Results

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the item. Valid item labels are shown in the table below. Some items also require a component label.

Component of the item (if required). Valid component labels are shown in the table below.

Undisplaced shape key:

0 - Do not overlay undeformed structure display

1 - Overlay displaced contour plot with undeformed display (appearance is system-dependent)

2 - Overlay displaced contour plot with undeformed edge display (appearance is system-dependent)

Scale factor for 2D display for contact items. Default value is 1. A negative scaling factor may be used to invert the display.

Displays the solution results as continuous contours across element boundaries for the selected nodes and elements. For example, PLNSOL,S,X displays the X component of stress S (that is, the SX stress component). Various element results depend upon the recalculation method and the selected results location [AVPRIN, RSYS, LAYER, SHELL, and NSEL]. Contours are determined by linear interpolation within each element from the nodal values, which are averaged at a node whenever two or more elements connect to the same node (except for FMAG, which is summed at the node). For PowerGraphics displays [/GRAPHICS,POWER], results are plotted only for the model exterior surface. The items marked with * are supported by PowerGraphics.

Utility Menu >PlotCtrls >Animate >Animate Over Time

Utility Menu >PlotCtrls >Animate >Dynamic Results

Utility Menu >PlotCtrls >Animate >Mode Shape

Main Menu >General Postproc >Plot Results >Nodal Solu

Utility Menu >Plot >Results >Contour Plot >Nodal Solution

Utility Menu >PlotCtrls >Animate >Deformed Results

Utility Menu >PlotCtrls >Animate >Isosurfaces

Utility Menu >PlotCtrls >Animate >Q-Slice Contours

Controls graphics options on subsequent displays.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

Apply display items as selected from the following labels:

LEG1 - Header portion of legend column (defaults to ON).

LEG2 - View portion of legend column (defaults to ON (except off with contour displays)).

INFO - Entire legend column. (defaults to AUTO).

FRAME - Frame border lines around windows (defaults to ON).

TITLE - Title (bottom left text) (defaults to ON).

MINM - Min-Max symbols on contour displays (defaults to ON).

LOGO - ANSYS logo (defaults to OFF (displayed as text at top of legend column)). If KEY=ON, the text is removed from legend column but the logo symbol is displayed in whichever active window is either in the uppermost right corner and on top, or if there is no window in that location, then in the window to the furthest right of the screen. Version information remains in the legend column.

WINS - Controls whether graphics windows automatically stretch or shrink to adjust to screen size as the legend column is turned off or on [/PLOPTS,INFO] (defaults to ON). If WINS is on and the legend column is changed from off to on, all windows are shrunk regardless of what their correct size is.

WP - Working plane (defaults to OFF). The working plane is drawn as part of the display (not just an overlaid image as in WPSTYL). This option is best used in combination with a hidden-line technique [/TYPE].

Switch:

OFF or 0 - Do not apply this display item.

ON or 1 - Apply this display item.

AUTO or 2 - (If Label = INFO) Auto-legend mode. If the display has contours, the legend is ON; if the display has no contours, the legend is OFF.

Notes

Use /PLOPTS,STAT to display settings. Use /PLOPTS,DEFA to reset all specifications back to their defaults.

When you perform multiple results displays, contours on the legend column may be truncated. To avoid this, you may wish to specify /PLOPTS,LEG1,0.

This command is valid in any processor.

Utility Menu >PlotCtrls >Window Controls >Reset Window Options

Utility Menu >PlotCtrls >Window Controls >Window Options

Forms a display.

DISPLAY:Action

	Mp Me St DY LP Th E3 E2 FL PP ED

Display plots sequentially from number NSTRT to NEND in steps of NINC. NSTRT defaults to the next plot. NEND defaults to NSTRT. NINC defaults to 1. If NSTRT=ALL, display all plots from the beginning of the file. If NEND=ALL, display to the end of the file.

Output will be to the terminal or to a file, depending on the driver [/SHOWDISP]. The INTERLEAF and DUMP drivers produce an output file for each plot named INTLnn and DUMPnn, with nn sequentially ranging from 00 to 99. A blank line after the PLOT command causes the next plot to be formed.

DISPLAY Program

Specifies "Plotting settings" as the subsequent status topic.

POST26:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

This is a status [STAT] topic command. Status topic commands are generated by the GUI and will appear in the log file (Jobname.LOG) if status is requested for some items under Utility Menu>List>Status. This command will be immediately followed by a STAT command, which will report the status for the specified topic.

If entered directly into the program, the STAT command should immediately follow this command.

Utility Menu >List >Status >TimeHist Postproc >Plot

Displays path items along the path geometry.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

The path data item to be displayed on the currently active path (defined by the PATH command). Valid path items are those defined the the PDEF command.

Scale factor for the offset from the path for the path data item displays. Defaults to 1.0.

Determines how data is displayed:

<blank> - Do not display nodes, and scale the display based on the currently selected node set (default).

NODE - Display path item data along with the currently selected set of nodes. The display geometry is scaled to the selected node set.

You can use the Gscale argument to scale the contour display offset from the path for clarity.

Main Menu >General Postproc >Path Operations >On Geometry

Main Menu >General Postproc >Plot Results >On Geometry

Displays path items on a graph.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Labels identifying the path items to be displayed. Up to six items may be drawn per frame. Predefined path geometry items XG, YG, ZG, and S [PDEF] may also be displayed.

The path must have been defined by the PATH and PPATH commands. Path items and their labels must have been defined with the PDEF, PVECT, PCALC, PDOT, and PCROSS commands. Path items may also be printed with the PRPATH command. Graph scaling may be controlled with the /XRANGE, /YRANGE, and PRANGE commands.

Main Menu >General Postproc >Path Operations >On Graph

Main Menu >General Postproc >Plot Results >On Graph

Utility Menu >Plot >Results >Path Plot

Displays membrane and membrane-plus-bending linearized stresses.

POST1:Paths

	Mp Me St DY LP -- -- -- -- PP ED

Label identifying the item to be processed. Valid item labels are shown in the table below. Items also require a component label.

Component of the item. Valid component labels are shown in the table below.

In-plane (X-Y) average radius of curvature of the inside and outside surfaces of an axisymmetric section. If zero (or blank), a plane or 3-D structure is assumed. If nonzero, an axisymmetric structure is assumed. Use a very large number (or -1) for an axisymmetric straight section.

Through-thickness bending stresses key for an axisymmetric analysis (RHO0):

0 - Include the thickness-direction bending stresses.

1 - Ignore the thickness-direction bending stresses.

Calculates and displays the membrane and membrane-plus-bending linearized stresses (as described for the PRSECT command) along a path section [PATH] as a graph. The path section is defined by two points specified with the PPATH command. For linearized stress calculations, the path must be defined with nodes. The total stress (equivalent to the PLPATH display) is also displayed. This command always uses 48 divisions along the path, regardless of the number of divisions defined by PATH.

Main Menu >General Postproc >Path Operations >Linearized Strs

Main Menu >General Postproc >Plot Results >Lineariz Strs

Defines the timerange for which data are to be displayed.

POST26:Display

	Mp Me St DY LP Th E3 E2 FL PP ED

Minimum time (defaults to the first point stored).

Maximum time (defaults to the last point stored).

Notes

Defines the time (or frequency) range (within the range stored) for which data are to be displayed. Time is always displayed in the Z-axis direction for 3-D graph displays. If XVAR=1, time is also displayed in the X-axis direction and this control also sets the abscissa scale range.

Main Menu >TimeHist Postpro >Settings >Graph

Displays a particle flow or charged particle trace on an element display.

POST1:TracePoints

	Mp Me St DY -- -- E3 E2 FL PP ED

Display option

FLUID Particle trace in fluid flow (default)

ELEC Particle trace in electric field

MAGN Particle trace in magnetic field

Label identifying the item to be contoured. Valid item labels are shown in the table below. Some items also require a component label. If Item is blank, display only the path trajectory.

Component of the item (if required). Valid component labels are shown in the table below.

Trace point number for storing trajectory data for use with PATH logic. Defaults to 0 (no trajectory path data is stored for further processing with PATH logic).

Name of prefix of array variable. Defaults to TRAC. NamePOIN stores trajectory path points for trace point number TRPNum. If Opt=ELEC or MAGN, two additional array parameters, NameDATA and NameLABL, store trajectory path data and labels for the same TRPNum.

Maximum number of loops traced by a particle. Defaults to 25 for Opt=FLUID; otherwise, defaults to 1000..

Length tolerance used for particle trajectory geometry calculation. Valid only for Opt = ELEC or MAGN. If particle trace appears to terminate inside an element, adjusting the length tolerance may be necessary. Defaults to 1.0x10^-8.

For a specified item, the variation of the item is displayed along the particle trace as a color-contoured ribbon. The TRPOIN command must be used to define a point on the trajectory path. Multiple traces may be displayed simultaneously by defining multiple trace points. Issue the TRPLIS command to list the current tracing points. Issue the TRPDEL command to delete tracing points defined earlier. Use the PAPUT command with the POIN option to retrieve the particle trajectory points as path points.

Use the PAPUT command with the TABL and LABE options to retrieve path geometry as well as the particle velocity vector components in global Cartesian coordinates (VX_TRACE, VY_TRACE, and VZ_TRACE), velocity magnitude (VS_TRACE) and time (T_TRACE). Not used if Opt = FLUID. If working in the GUI, use the "All information" option to retrieve information from all three arrays at once.

See Chapters 5 and 12 of the ANSYS Basic Analysis Procedures Guide for more information on particle flow and charged particle traces. See Chapter 15 of the ANSYS Basic Analysis Procedures Guide for information on particle trace animation.

Utility Menu >PlotCtrls >Animate >Particle Flow

Main Menu >General Postproc >Plot Results >Particle Trace

Main Menu >General Postproc >Plot Results >Plot Flow Tra

Utility Menu >Plot >Results >Flow Trace

Displays up to ten variables in the form of a graph.

POST26:Display

	Mp Me St DY LP Th E3 E2 FL PP ED

Reference numbers of the variables to be displayed.

Variables are displayed vs. variable N on the XVAR command. For complex variables, the amplitude is displayed by default [PLCPLX]. Each PLVAR command produces a new frame. See the /GRTYP command for displaying multiple variables in a single frame with separate Y-axes.

Main Menu >TimeHist Postpro >Graph Variables

Displays up to ten parameters in the form of a graph.

OPTIMIZATION:Display

	Mp Me St DY LP Th E3 E2 FL PP ED

Names of the parameters to be displayed on this frame.

Notes

Displays up to ten parameters in the form of a graph. Parameters are displayed vs. Lab on the XVAROPT command (defaults to set number) in the order corresponding to an ascending order of the XVAROPT parameter. See the /GRTYP command for displaying multiple parameters in a single frame with separate Y-axes. Each PLVAROPT command produces a new frame.

Main Menu >Design Opt >Graphs/Tables

Displays results as vectors.

POST1:Results POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Predefined vector item (from table below) or a label identifying the i-component of a user-defined vector.

Label identifying the j-component of a user-defined vector. Must be blank if Item is selected from list below.

Label identifying the k-component of a user-defined vector. Must be blank if Item is selected from list below or for 2-D user defined vector.

Label assigned to resultant vector for display labeling (defaults to Item).

Vector or raster mode overide key:

<blank> - Use the setting of KEY on the /DEVICE command.

RAST - Use raster mode for PLVECT displays.

VECT - Use vector mode for PLVECT displays.

Vector location for display of field element results:

ELEM - Display at element centroid (default).

NODE - Display at element nodes.

Edge display override key:

<blank> - Use the setting of Key on the /EDGE command.

OFF - Deactivate the edge display.

ON - Activate the edge display.

Displays various solution results as vectors (arrows) for the selected nodes and/or elements. For example, PLVECT,U displays the displacement vector for all selected nodes. For section displays [/TYPE], the vectors are shown only on the section face (i.e., cutting plane). The PLVECT display of principal strains and stresses (Item=S, EPTO, EPEL, EPPL, EPCR, or EPTH) on a "cut" of the model (/TYPE,,1 ,5,7,8, or 9) is not supported. The resulting plot displays the vectors on all selected elements, not on just the sliced surface. See the /VSCALE command to scale vector lengths. Vector magnitudes may be shown as a contour display with the PLNSOL command. Various results also depend upon the recalculation method and the selected results location [LAYER, SHELL, and NSEL].

Items may be selected from a set of recognized vector labels (Item) or a vector may be defined from up to three scalar labels (Item,Lab2,Lab3). Scalar labels may be user-defined with the ETABLE command. The vectors appear on an element display as arrows showing the relative magnitude of the vector and its direction. The vectors will be either at the node or at the element centroid depending on what item is being displayed and depending on the Loc setting. Stress vectors appear as arrows at the element centroid, with the arrowheads pointing away from each other for tension and toward each other for compression.

When vector mode is active (Mode=VECT), use the Z-buffered display type [/TYPE,,6] to maximize speed of PLVECT plots (other hidden display types may make plotting slow).

Main Menu >General Postproc >Plot Results >Predefined

Main Menu >General Postproc >Plot Results >User-defined

Utility Menu >Plot >Results >Vector Plot

Utility Menu >PlotCtrls >Animate >Q-Slice Vectors

Specifies that macro contents be written to the session log file.

APDL:MacroFiles

	Mp Me St DY LP Th E3 E2 FL PP ED

This command forces the contents of a macro or other input file to be written to Jobname.LOG. It is valid only within a macro or input file, and should be placed at the top of the file. /PMACRO should be included in any macro or input file that calls GUI functions.

This command cannot be accessed directly in the menu.

Creates mapping of the path geometry by defining path interpolation division points.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Defines the mapping method:

UNIFORM - Maps uniform divisions (specified on the nDiv argument of the PATH command) between specified points. This is the default.

ACCURATE - Map geometry using a small division at the beginning and end of each segment. This gives you accurate derivatives, integrals, tangents, and normals for curves which do not have continuous slopes at the specified points.

Sets mapping for discontinuities in the field. The divisions are modified to put a point just before and just after the discontinuity. The valid label is MAT, for a material discontinuity. No discontinuity is the default. Discontinuity mapping involves the NOAV option on the PDEF command.

Main Menu >General Postproc >Elec&Mag Calc >Define Path >Path Options

Main Menu >General Postproc >Path Operations >Define Path >Path Options

Activates the p-method solution options in the Graphical User Interface (GUI).

SOLUTION:p-MethodOptions

	Mp Me St -- LP -- -- -- -- PP ED

ON - Activates the p-method solution options.

OFF - Deactivates the p-method solution options (default).

STAT - Lists the current setting of Key.

Notes

When this option is activated, only the options applicable to a p-method solution will be displayed in the GUI. This command is not required outside of the GUI.

Main Menu >Preferences

Specifies "p-Method" as the subsequent status topic.

PREP7:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

This is a status [STAT] topic command. Status topic commands are generated by the GUI and will appear in the log file (Jobname.LOG) if status is requested for some items under Utility Menu>List>Status. This command will be immediately followed by a STAT command, which will report the status for the specified topic.

If entered directly into the program, the STAT command should immediately follow this command.

This command is also valid in SOLUTION.

Utility Menu >List >Status >p-Method

Summarizes electromagnetic results from a transient analysis.

POST26:SpecialPurpose

	Mp Me St -- -- -- E3 E2 -- PP ED

File name (8 characters maximum) to which tabular data and plot files will be written. Must be enclosed in single quotes when the command is manually typed in. Defaults to MG_TRNS. The data file extension is .OUT and the plot file extension is .PLT.

Frequency of solution output. Defaults to 1. Every FREQth solution on the results file is output.

Names of element components for force calculation. Must be enclosed in single quotes when the command is manually typed in.

Names of element components for power loss calculation. Must be enclosed in single quotes when the command is manually typed in.

Names of element components for energy, total current, and inductance calculations, respectively. Must be enclosed in single quotes when the command is manually typed in.

PMGTRAN invokes an ANSYS macro which calculates and summarizes electromagnetic results from a transient analysis. The results are summarized by element components and listed on the screen as well as written to a file (Fname.OUT). Also, graph plots of results as a function of time are created and written to a file (Fname.PLT) for use in the DISPLAY program.

Two components may be selected for the summary of electromagnetic forces (see FMAGSUM), two for power loss, and one each for stored energy (see SENERGY), total current (see CURR2D), and conductor inductance. Inductance calculation is valid only for voltage-fed or circuit-fed conductors (PLANE53 or SOLID97, KEYOPT(1)=2, or 3). See the referenced commands for other restrictions.

Main Menu >TimeHist Postpro >Elec&Mag >Magnetics

Defines percentage tolerance for a p-Method solution.

SOLUTION:p-MethodOptions

	Mp Me St -- LP -- -- -- -- PP ED

Percentage tolerance used to determine which elements to fix at the current p-level. If an element's strain energy error is less than this tolerance its p-level will be fixed at the current level. Defaults to 5.

Notes

Defines the p-level tolerance for p-method solutions (TOLER). The default value is satisfactory for most solutions.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >p-Method >Solution Options

Main Menu >Solution >p-Method >Solution Options

Creates an annotation polygon (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Unused field.

X location for vertex 5 of polygon (-1.0 < X < 2.0).

Y location for vertex 5 of polygon (-1.0 < Y < 1.0).

X location for vertex 6 of polygon (-1.0 < X < 2.0).

Y location for vertex 6 of polygon (-1.0 < Y < 1.0).

X location for vertex 7 of polygon (-1.0 < X < 2.0).

Y location for vertex 7 of polygon (-1.0 < Y < 1.0).

X location for vertex 8 of polygon (-1.0 < X < 2.0).

Y location for vertex 8 of polygon (-1.0 < Y < 1.0).

Defines the 5th through 8th vertices of an annotation polygon [/POLYGON]. This is a command generated by the Graphical User Interface (GUI) and will appear in the log file (Jobname.LOG) if annotation is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Controls entity numbering/coloring on plots.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

Type of numbering/coloring:

NODE - Node numbers on node and element plots.

ELEM - Element numbers and colors on element plots.

MAT - Material set numbers and colors on element and solid model plots (see Note).

TYPE - Element type reference numbers and colors on element and solid model plots (see Note).

REAL - Real constant set numbers and colors on element and solid model plots (see Note).

ESYS - Element coordinate system numbers on element and solid model plots (see Note).

LOC - Location numbers/colors of the element in the solution sequence (the "wavefront order," see WAVES command) on element plots. Note, LOC and ELEM numbers will be the same unless the model has been reordered.

KP - Keypoint numbers on solid model plots.

LINE - Line numbers on solid model plots (both numbers and colors on line plots).

AREA - Area numbers on solid model plots (both numbers and colors on area plots).

VOLU - Volume numbers on solid model plots (both numbers and colors on volume plots).

SVAL - Stress (or any contour) values on postprocessing plots, and surface load values and colors on model plots (when surface load symbols are on [/PSF]). For tabular boundary conditions, the table-evaluated values will be displayed on node, element, or contour displays in Post1 when load symbols (/PBF, /PSF, /PBC) are on and TABNAM is OFF.

TABNAM - Table names for tabular boundary conditions. If this label is turned on, the table name appears next to the appropriate symbol, arrow, face outline, or contour as dictated by the /PSF, /PBC, and /PBF commands.

Switch:

0 - Turns OFF numbers/colors for specified label.

1 - Turns ON numbers/colors for specified label.

This command specifies the entity numbering and coloring to be applied to subsequent plots.

The MAT, TYPE, REAL, and ESYS labels activate both the numbering and coloring of the corresponding attributes for elements on EPLOTs, keypoints on KPLOTs, lines on LPLOTs, areas on APLOTs, and volumes on VPLOTs.

The ELEM, MAT, TYPE, REAL, ESYS, and LOC labels are mutually exclusive, i.e., only one can be specified at a time. Also, turning on a LINE, AREA, or VOLU label will turn off the MAT, TYPE, and REAL labels.

Element and volume numbers are not visible for 3-D elements and volumes when Z-buffering is turned on (/TYPE,,[6,7, or 8]).

Use /PSTATUS or /PNUM,STAT to show settings. Use /PNUM,DEFA to reset all specifications back to default. Use the /NUMBER command to control whether numbers and colors are displayed together.

/PNUM,LOC and /PNUM,ESYS are not supported by PowerGraphics [/GRAPHICS,POWER].

This command is valid in any processor.

Utility Menu >PlotCtrls >Numbering

Specifies "Point flow tracing settings" as the subsequent status topic.

POST1:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

This is a status [STAT] topic command. Status topic commands are generated by the GUI and will appear in the log file (Jobname.LOG) if status is requested for some items under Utility Menu>List>Status. This command will be immediately followed by a STAT command, which will report the status for the specified topic.

If entered directly into the program, the STAT command should immediately follow this command.

Utility Menu >List >Status >General Postproc >Trace Points

Creates a polygonal area based on working plane coordinate pairs.

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

Defines a polygonal area on the working plane. The area will be defined with NPT keypoints and NPT lines, where NPT (must be at least 3) is the number of coordinate pairs defined with the PTXY command. See the RPOLY and RPR4 commands for other ways to create polygons.

This command cannot be accessed directly in the menu.

Creates annotation polygons (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of vertices of polygon (3 NVERT 8). Use /PMORE for polygons with more than 4 vertices.

X location for vertex 1 of polygon (-1.0 < X < 2.0).

Y location for vertex 1 of polygon (-1.0 < Y < 1.0).

X location for vertex 2 of polygon (-1.0 < X < 2.0).

Y location for vertex 2 of polygon (-1.0 < Y < 1.0).

X location for vertex 3 of polygon (-1.0 < X < 2.0).

Y location for vertex 3 of polygon (-1.0 < Y < 1.0).

X location for vertex 4 of polygon (-1.0 < X < 2.0).

Y location for vertex 4 of polygon (-1.0 < Y < 1.0).

Creates annotation polygons to be written directly onto the display at a specified location. This is a command generated by the Graphical User Interface (GUI) and will appear in the log file (Jobname.LOG) if annotation is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

All polygons are shown on subsequent displays unless the annotation is turned off or deleted. Use the /LSPEC and the /PSPEC command to set the attributes of the polygon. Use the /PMORE command to define the 5th through 8th vertices of the polygon.

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Selects the piping analysis standard for a piping run.

PREP7:Piping

	Mp Me St -- LP -- -- -- -- PP ED

Option label:

B31.1 - for ANSI B31.1.

NC - for ASME Section III NC, Class 2.

Notes

Selects the piping analysis standard for a piping run [RUN]. Affects only the flexibility and stress intensification factors applied to the curved pipe elements.

Main Menu >Preprocessor >Create >Piping Models >Specifications

Specifies a time-harmonic guided wave excitation for a waveguide port.

SOLUTION:SolidSurfaceLoads

	Mp Me -- -- -- -- E3 -- -- PP ED

Waveguide port number. You specify the integer number via the SF family of commands. The number must be between 1 and 6. If Status, provide status of port option settings.

Guided wave type (one of the following):

COAX - The TEM wave in a cylindrical coaxial waveguide.

TE10 - The TE10 mode in a rectangular waveguide.

TE11CIRC - The TE11 mode in a circular waveguide.

TM01CIRC - The TM01 mode in a circular waveguide.

A local coordinate system number in which the guided wave is specified. The local Z-direction must be the direction of propagation.

If Porttype = COAX:

VALUE1 - Inner radius of the coaxial waveguide.

VALUE2 - Outer radius of the coaxial waveguide.

VALUE3 - Zero-to-peak amplitude of the voltage between the inner and the outer conductors. If blank, the port will create a matching impedance.

VALUE4 - Phase angle of the applied voltage (in degrees). Defaults to 0 degrees.

VALUE5 - Input power (time-average). If power is input, it overrides the applied voltage input.

If Porttype = TE10:

VALUE1 - Width of the rectangular waveguide

VALUE2 - Height of the rectangular waveguide.

VALUE3 - Zero-to-peak amplitude of the electric field. If blank, the port will appear as a matching impedance.

VALUE4 - Phase angle of the applied E_o field (in degrees). Defaults to 0 degrees.

VALUE5 - Input power (time-average). If power is input, it overrides the E_o input.

If Porttype=TE11circ:

VALUE1 - Radius of the circular waveguide.

VALUE2 - Not used.

VALUE3 - Zero-to-peak amplitude of the H_o modal field. If blank, the port will create a matching impedance.

VALUE4 - Phase angle of the H_o field (in degrees). Defaults to 0 degrees.

VALUE5 - Input power (time-average). If power is input, it overrides the H_o field input.

If Porttype=TM01circ:

VALUE1 - Radius of the circular waveguide.

VALUE2 - Not used.

VALUE3 - Zero-to-peak amplitude of the E_o modal field. If blank, the port will create a matching impedance.

VALUE4 - Phase angle of the E_o field (in degrees). Defaults to 0 degrees.

VALUE5 - Input power (time-average). If power is input, it overrides the E_o field input.

Menu Paths

Main Menu >Preprocessor >Loads >Apply >Excitation >Port Status

Main Menu >Solution >Apply >Excitation >Port Status

Main Menu >Preprocessor >Loads >Apply >Excitation >On Areas

Main Menu >Preprocessor >Loads >Apply >Excitation >On Nodes

Main Menu >Preprocessor >Loads >Apply >Excitation >Modify Port

Main Menu >Solution >Apply >Excitation >On Areas

Main Menu >Solution >Apply >Excitation >On Nodes

Main Menu >Solution >Apply >Excitation >Modify Port

Enters the database results postprocessor.

SESSION:ProcessorEntry POST1:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Enters the general database results postprocessor (POST1). All load symbols (/PBC, /PSF, or /PBF) are automatically turned off with this command.

This command is valid only at the Begin Level.

Main Menu >General Postproc

Enters the time-history results postprocessor.

SESSION:ProcessorEntry POST26:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Enters the time-history results postprocessor (POST26).

This command is valid only at the Begin Level.

Main Menu >TimeHist Postpro

Calculates the rms power loss in a conductor or lossy dielectric.

POST1:Magnetics

	Mp Me St -- -- -- E3 E2 -- PP ED

POWERH invokes an ANSYS macro which calculates the time-averaged (rms) power loss in a conductor or lossy dielectric material from a harmonic analysis. The power loss is stored in the parameter PAVG. Conductor losses include solid conductors and surface conductors approximated by impedance or shielding boundary conditions. The power loss density for solid conductors or dielectrics is stored in the element table with the label PLOSSD and may be listed [PRETAB] or displayed [PLETAB]. PLOSSD does not include surface losses. The elements of the conducting region must be selected before this command is issued. POWERH is valid for two-dimensional and three-dimensional analyses.

Main Menu >General Postproc >Elec&Mag Calc >Power Loss

Defines a path by picking or defining nodes, or locations on the currently active working plane, or by entering specific coordinate locations.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

The point number. It must be greater than zero and less than or equal to the nPts value specified on the PATH command.

The node number defining this point. If blank, use the X, Y, Z coordinates to define the point. A valid node number will override X, Y, Z coordinate arguments.

PICK - Pick the node.

<blank> - Use X, Y, Z to define the point.

X, Y, Z arguments specify the location of the point in the global Cartesian coordinate system. Use this argument only if you omit the NODE argument.

The coordinate system for interpolation of the path between the previous point and this point. Omit this argument if you wish to use the currently active (CSYS) coordinate system. If the coordinate system of two adjacent points is different, the CS value of the latter point will be used.

For linearized stress calculations, the path must be defined with nodes.

Main Menu >General Postproc >Elec&Mag Calc >Define Path >By Location

Main Menu >General Postproc >Elec&Mag Calc >Define Path >By Nodes

Main Menu >General Postproc >Elec&Mag Calc >Define Path >Modify Path

Main Menu >General Postproc >Elec&Mag Calc >Define Path >On Working Plane

Main Menu >General Postproc >Path Operations >Define Path >By Location

Main Menu >General Postproc >Path Operations >Define Path >By Nodes

Main Menu >General Postproc >Path Operations >Define Path >Modify Path

Main Menu >General Postproc >Path Operations >Define Path >On Working Plane

Displays an element plot indicating each element's final p-level.

POST1:Results

	Mp Me St DY LP -- -- -- -- PP ED

The final polynomial level (an integer value ranging from 2 to 8) is displayed at the center of the element's facets [/EFACET] in a p-method analysis.

Main Menu >General Postproc >Plot Results >p-Levels

Specifies a range of p-level values for use in a p-method solution.

SOLUTION:p-MethodOptions

	Mp Me St -- LP -- -- -- -- PP ED

Starting p-level. Defaults to 2.

Maximum p-level. Defaults to 8.

Notes

The minimum possible p-level is 2, and the maximum possible p-level is 8. This command sets a global p-range for the entire model, where KEYOPT settings [ET] control individual element p-levels. Element KEYOPT settings override PPRANGE settings.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >p-Method >Set p range

Main Menu >Solution >p-Method >Set p range

Defines the internal pressure for a piping run.

PREP7:Piping

	Mp Me St DY LP -- -- -- -- PP ED

Pipe internal pressure.

Defines the pipe internal pressure for a piping run [RUN]. These pressures are assigned to the elements as they are generated.

Main Menu >Preprocessor >Create >Piping Models >Loads

Determines the pathrange.

POST1:Paths

	Mp Me St DY LP Th E3 E2 FL PP ED

Set the range for listing or displaying the table locations between a minimum value (VMIN) and a maximum value (VMAX) of the path distance with a location increment of LINC (defaults to 1). The first location begins at VMIN.

Path variable item to be used as the x-axis plot variable. Any valid path variable may be used (PDEF command). Default variable is the path distance, S.

Notes

Determines the path distance range for use with the PRPATH and PLPATH commands.

Main Menu >General Postproc >Path Operations >Path Range

Lists convergence values versus characteristic p-level.

POST1:Results

	Mp Me St DY LP -- -- -- -- PP ED

After a p-method solution, this command lists in tabular form all convergence values versus characteristic p-level.

This command is also valid in SOLUTION.

Main Menu >General Postproc >List Results >p-Convergence

Defines the output form for complex variables.

POST26:Listing

	Mp Me St DY LP -- E3 E2 -- PP ED

Output form key:

0 - Real and imaginary parts.

1 - Amplitude and phase angle. Stored real and imaginary data are converted to amplitude and phase angle upon output. Data remain stored as real and imaginary parts.

Defines the output form for complex variables. Used only with harmonic analyses (ANTYPE=HARMIC).

Main Menu >TimeHist Postpro >Settings >List

Specifies machine precision for solvers (currently valid only for PCG solvers).

SOLUTION:AnalysisOptions

	Mp Me St -- LP Th E3 E2 -- PP ED

Machine precision to use for solvers:

0 or double - Specifies double precision (default).

1 or single - Specifies single precision.

When the PCG or PCGOUT solvers are specified by the EQSLV command, this command can be used to specify single precision for the solver. By using single precision, about 30% less in-core memory is used by the PCG solver. However, using single precision can lead to unconvergence for the PCG solver when the problem is ill-conditioned. Double precision is the default and the recommended option for the PCG solvers

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Activates a predictor in a nonlinear analysis.

SOLUTION:NonlinearOptions

	Mp Me St -- LP Th -- -- -- PP ED

Substep predictor key:

OFF - No prediction is done (default if rotation DOF are present or element 65 is present).

ON - Use a predictor on all substeps after the first (default, unless rotation DOF are present, or SOLID65 is present).

Unused field.

Load step predictor:

OFF - No prediction across load steps is done (default).

ON - Use a predictor also on the first substep of the load step (Sskey must also be ON).

Notes

Activates a predictor in a nonlinear analysis on the degree of freedom solution for the first equilibrium iteration of each substep.

The default values given for this command assume SOLCONTROL,ON (the default). See the description of SOLCONTROL in the ANSYS Commands Reference for a complete listing of the defaults set by SOLCONTROL,ON and SOLCONTROL,OFF.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Nonlinear >Predictor

Main Menu >Solution >Nonlinear >Predictor

Enters the model creation preprocessor.

SESSION:ProcessorEntry PREP7:Database

	Mp Me St DY LP Th E3 E2 FL PP ED

Enters the general input data preprocessor (PREP7).

This command is valid only at the Begin Level.

Main Menu >Preprocessor

Prints SEPC and TEPC.

POST1:Listing

	Mp Me St DY LP Th -- -- -- PP ED

Prints the percent error in structural energy norm (SEPC) and the thermal energy norm percent error (TEPC). Approximations of mesh discretization error associated with a solution are calculated for analyses having structural or thermal degrees of freedom.

The structural approximation is based on the energy error (which is similar in concept to the strain energy) and represents the error associated with the discrepancy between the calculated stress field and the globally continuous stress field (see Section 19.7 of the ANSYS Theory Reference). This discrepancy is due to the assumption in the elements that only the displacements are continuous at the nodes. The stress field is calculated from the displacements and should also be continuous, but generally is not. Structural analyses should be linear elastic and may use solid elements having only structural degrees of freedom (excluding SOLID46, SOLID65, SOLID72 (unless KEYOPT(9)=1), HYPER56, HYPER58, HYPER74, HYPER84, HYPER86, HYPER158 VISCO88, VISCO106, VISCO107, and VISCO108) and 3-D shell elements (excluding SHELL28, SHELL41, SHELL91, and SHELL99).

Thermal analyses may use any solid and shell thermal element having only temperature degrees of freedom. The thermal approximation is based on the total heat flow dissipation and represents the error associated with the discrepancy between the calculated nodal thermal flux within an element and a continuous global thermal flux. This continuous thermal flux is calculated with the normal nodal averaging procedure.

The volume (result label VOLU) is used to calculate the energy error per element (result label SERR for the structural energy error and TERR for the thermal energy error). These energy errors, along with the appropriate energy, are then used to calculate the percent error in energy norm (SEPC for structural and TEPC for thermal). These percentages can be listed by the PRERR command, retrieved by the *GET command (with labels SEPC and TEPC) for further calculations, and shown on the displacement display [PLDISP], as applicable.

For structural analyses, the maximum absolute value of nodal stress variation of any stress component for any node of an element (result item SDSG) is also calculated. Similarly, for thermal gradient components, TDSG is calculated. Minimum and maximum result bounds considering the possible effect of discretization error will be shown on contour displays [PLNSOL]. For shell elements, the top surface location is used to produce a meaningful percentage value. SERR, TERR, SEPC, TEPC, SDSG, and TDSG will be updated whenever the nodal stresses or fluxes are recalculated.

If the energy error is a significant portion of the total energy, then the analysis should be repeated using a finer mesh to obtain a more accurate solution. The energy error is relative from problem to problem but will converge to a zero energy error as the mesh is refined. An automated adaptive meshing procedure using this energy error is described with the ADAPTmacro.

Main Menu >General Postproc >List Results >Percent Error

Utility Menu >List >Results >Percent Error

Prints the solution results for elements.

POST1:Results

	Mp Me St DY LP Th E3 E2 -- PP ED

Label identifying the item. Valid item labels are shown in the table below. Some items also require a component label.

Component of the item (if required). Valid component labels are shown in the table below.

Prints the solution results for the selected elements in the sorted sequence. For example, PRESOL,S prints the stress items SX, SY, SZ, SXY, SYZ, and SXZ for the node locations of the element. Component results are in the global Cartesian coordinate directions unless transformed [RSYS]. Shell elements print values at the top, then bottom of the element (or layer). Items are listed as columns of a table versus element number. An exception occurs for item ELEM which uses an element format (all applicable line element results are listed per element) instead of a tabular format. The FORCE command can be used to define which component of the nodal load is to be used (static, damping, inertia, or total). See the ETABLE and PRETAB commands for printing items not available through this command (such as line element results).

For PowerGraphics [/GRAPHICS,POWER], results are listed only for the element surface. The items marked with * are supported by PowerGraphics.

Main Menu >General Postproc >List Results >Element Solution

Utility Menu >List >Results >Element Solution

Prints the element table items.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Print selected items. Valid labels are <blank> or any label as specified with the ETABLE command. Convenience labels may be used for Lab1 to select groups of labels (10 labels maximum): GRP1 for first 10 stored items; GRP2 for items 11 to 20; GRP3 for items 21 to 30; GRP4 for items 31 to 40; GRP5 for items 41 to 50. Enter ETABLE,STAT command to list stored item order. If all labels are blank, print first 10 stored items (GRP1).

Prints the items stored in the table defined with the ETABLE command. Item values will be listed for the selected elements in the sorted sequence [ESORT]. The FORCE command can be used to define which component of the nodal load is to be used (static, damping, inertia, or total).

Main Menu >General Postproc >Element Table >List Elem Table

Main Menu >General Postproc >List Results >Elem Table Data

Utility Menu >List >Results >Element Table Data

Creates a polygonal area or a prism volume by vertices (GUI).

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

Creates a polygonal area or a prism volume using the vertices as input. This is a command generated by the Graphical User Interface (GUI) and will appear in the log file (Jobname.LOG) if graphical picking is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

For polygons, the PRI2 command will appear in the log file as PRI2,P51X,0.0,0.0 preceded by FITEM commands that define the vertices (in global Cartesian coordinates). For prisms, the PRI2 command will appear in the log file as PRI2,P51X preceded by FITEM commands that define the vertices and the Z-end of the prism.

See the RPOLY, POLY, RPRISM, PRISM, and RPR4 commands for other ways to create polygons and prisms.

Main Menu >Preprocessor >Create >Polygon >By Vertices

Main Menu >Preprocessor >Create >Prism >By Vertices

Specifies "Solid model primitives" as the subsequent status topic.

PREP7:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

This is a status [STAT] topic command. Status topic commands are generated by the GUI and will appear in the log file (Jobname.LOG) if status is requested for some items under Utility Menu>List>Status. This command will be immediately followed by a STAT command, which will report the status for the specified topic.

If entered directly into the program, the STAT command should immediately follow this command.

Utility Menu >List >Status >Preprocessor >Solid Model

Specifies "Print settings" as the subsequent status topic.

POST1:Status POST26:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

This is a status [STAT] topic command. Status topic commands are generated by the GUI and will appear in the log file (Jobname.LOG) if status is requested for some items under Utility Menu>List>Status. This command will be immediately followed by a STAT command, which will report the status for the specified topic.

If entered directly into the program, the STAT command should immediately follow this command.

Utility Menu >List >Status >General Postproc >List Results

Utility Menu >List >Status >TimeHist Postproc >List

Creates a prism volume based on working plane coordinate pairs.

PREP7:Primitives

	Mp Me St DY LP Th E3 -- FL PP ED

Working plane Z coordinates of the top and bottom of the prism.

Defines a prism volume based on the working plane. The top and bottom areas will each be defined with NPT keypoints and NPT lines, where NPT (must be at least 3) is the number of coordinate pairs defined with PTXY command. Also, a line will be defined between each point pair on the top and bottom face. See the RPRISM and RPR4 commands for other ways to create prisms.

This command cannot be accessed directly in the menu.

Prints solution summary data.

POST1:Listing

	Mp Me St DY LP Th E3 E2 FL PP ED

Prints solution summary data (such as time step size, number of equilibrium iterations, convergence values, etc.).

Main Menu >General Postproc >List Results >Iteration Summry

Utility Menu >List >Results >Iteration Summry

Prints the summed element nodal loads.

POST1:Results

	Mp Me St DY LP Th E3 E2 -- PP ED

Nodal reaction load type. If blank, use the first ten of all available labels. Valid labels are: Structural force labels: FX, FY or FZ (forces); F (includes FX, FY and FZ); MX, MY or MZ (moments); M (includes MX, MY and MZ). Thermal force labels: HEAT (heat flow). Fluid force labels: FLOW (fluid flow); VFX, VFY and VFZ (fluid "forces"); VF (includes VFX, VFY and VFZ). Electric force labels: AMPS (current flow); CURT (current); VLTG (voltage drop). Magnetic force labels: FLUX (magnetic flux); CSGX, CSGY, CSGZ (magnetic current segments); CSG (includes CSGX, CSGY and CSGZ).

Tolerance value about zero within which loads are not printed. Defaults to 1.0E-9 times the absolute value of the maximum load on the selected nodes. If zero, print all nodal loads.

Prints the summed element nodal loads (forces, moments, heat flows, flux, etc.) for the selected nodes in the sorted sequence. Results are in the global Cartesian coordinate directions unless transformed [RSYS]. Zero values (within a tolerance range) are not printed. Loads applied to a constrained degree of freedom are not included. The FORCE command can be used to define which component of the nodal load is to be used (static, damping, inertia, or total).

Main Menu >General Postproc >List Results >Nodal Loads

Utility Menu >List >Results >Nodal Loads

Prints the nodal solution results.

POST1:Results

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the item. Valid item labels are shown in the table below. Some items also require a component label.

Component of the item (if required). Valid component labels are shown in the table below. Defaults to COMP.

Prints the nodal solution results for the selected nodes in the sorted sequence. For example, PRNSOL,U,X prints the X component of displacement vector U (i.e., the UX degree of freedom). Component results are in the global Cartesian coordinate directions unless transformed [RSYS]. Various element results also depend upon the recalculation method and the selected results location [AVPRIN, RSYS, LAYER, SHELL, and NSEL]. If LAYER is specified, then the resulting output will be listed in Full graphics mode. The FORCE command can be used to define which component of the nodal load is to be used (static, damping, inertia, or total).

For PowerGraphics [/GRAPHICS,POWER], results are listed only for the model exterior surface. If NSORT, ESORT or /ESHAPE are specified with PowerGraphics activated, then the PRNSOL listings will be the same as in Full graphics mode. The items marked with * are supported by PowerGraphics.