R

Defines the element real constants.

PREP7:RealConstants

	Mp Me St DY LP Th E3 E2 FL PP ED

Set identification number (arbitrary). If same as a previous set number, set is redefined. Set number relates to that defined with the element [REAL].

Real constant values (interpreted as area, moment of inertia, thickness, etc., as required for the particular element type using this set), or table names for tabular input of boundary conditions. Use RMORE command if more than six real constants per set are to be input.

Defines the element real constants. The real constants required for an element are shown in Table 4.n.1 of each element description in the ANSYS Elements Reference. Constants must be input in the same order as shown in that table. If more than the required number of element real constants are specified in a set, only those required are used. If fewer than the required number are specified, zero values are assumed for the unspecified constants.

If using table inputs (SURF151, SURF152, and FLUID116 only), enclose the table name in % signs (e.g., %tabname%).

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change RealConst

Main Menu >Preprocessor >Real Constants

Main Menu >Solution >Other >Change RealConst

Defines a "racetrack" current source.

PREP7:SpecialPurpose

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

Location of the mid-thickness of the vertical leg along the working plane X-axis.

Location of the mid-thickness of the horizontal leg along the working plane Y-axis.

Radius of curvature of the mid-thickness of the curves in the racetrack source. Defaults to .501 * DY

Total current, amp-turns (MKS) or abamp-turns (CGS), flowing in the source.

In-plane thickness of the racetrack source.

Out-of-plane thickness (depth) of the racetrack source.

Unused fields

An alphanumeric name assigned as a component name to the group of SOURCE36 elements created by the command macro. Cname may be up to 8 characters, beginning with a letter and containing only letters, numbers, and underscores. Component names beginning with an underscore (e.g., _LOOP) are reserved for use by ANSYS and should be avoided. If blank, no component name is assigned.

RACE invokes an ANSYS macro which defines a "racetrack" current source in the working plane coordinate system. The current source is generated from bar and arc source primitives using the SOURC36 element (which is assigned the next available element type number). The macro is valid for use in three-dimensional magnetic field analysis using a scalar potential formulation. Current flows in a counter-clockwise direction with respect to the working plane.

The diagram below shows you a racetrack current source.

Menu Paths

Main Menu >Preprocessor >Create >Racetrack Coil

Main Menu >Preprocessor >Loads >Apply >Excitation >Racetrack Coil

Main Menu >Solution >Apply >Excitation >Racetrack Coil

Calculates solver statistics and run time estimates.

RUNSTATS:RunStatisticsEstimator

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

Calculates solver statistics and estimates. The RALL command is a convenience command for obtaining all of the following: run time estimates [RTIMST], the wavefront statistics and memory requirements [RWFRNT], the file sizes estimates [RFILSZ], the memory statistics [RMEMRY], and the finite element model statistics [RSTAT].

Main Menu >Run-Time Stats >All Statistics

Appends results data from the database to the results file.

POST1:LoadCaseCalculations

	Mp Me St DY LP Th E3 E2 FL PP ED

Load step number to be assigned to the results data set. If it is the same as an existing load step number on the results file, the appended load step will be inaccessible. Defaults to 1.

Time value to be assigned to the results data set. Defaults to 0.0. A time value greater than the last load step should be used.

This command is typically used to append the results from a load case combination to the results file. See the LCWRITE command to create a separate load case file. Only summable and constant data are written to the results file by default; non-summable data are not written unless requested (LCSUM command)."

Main Menu >General Postproc >Write Results

Distorts the object geometry.

GRAPHICS:Scaling

	Mp Me St DY LP Th E3 E2 FL PP ED

Window number (or ALL) to which command applies (defaults to 1).

Distort object in the window X direction by this factor (defaults to 1.0).

Distort object in the window Y direction by this factor (defaults to 1.0).

Notes

Distorts the object geometry in a particular direction. An example of this command's use would be to allow long narrow sections to be distorted to a more square area for better display visualization.

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Size and Shape

Distributes the force/moment applied at the master node to a set of slave nodes, taking into account the geometry of the slave nodes as well as weighting factors.

PREP7:ConstraintEquations

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

Node at which the force/moment to be distributed will be applied.

Refers to the master node degrees of freedom to be used in constraint equations. Valid labels are:

UX

UY

UZ

ROTX

ROTY

ROTZ

UXYZ

RXYZ

ALL

The name of an array parameter that contains a list of slave nodes. Must specify the starting index number. ALL can be used for currently selected set of nodes.

The name of an array parameter that contains a list of weighting factors corresponding to each slave node above. Must have the starting index number. If not specified, the weighting factor for each slave node defaults to 1.

The force is distributed to the slave nodes proportional to the weighting factors. The moment is distributed as forces to the slaves; these forces are proportional to the distance from the center of gravity of the slave nodes times the weighting factors. Only the translational degrees of freedom of the slave nodes are used for constructing the constraint equations.

This command is valid in any processor.

Main Menu >Preprocessor >Coupling / Ceqn >Dist F/M at Mstr

Specifies "Real constants" 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 >Real Constants

Deletes real constant sets.

PREP7:RealConstants

	Mp Me St DY LP Th E3 E2 FL PP ED

Delete real constant sets from NSET1 to NSET2 (defaults to NSET1) in steps of NINC (defaults to 1). If NSET1 = ALL, ignore NSET2 and NINC and all real constant sets are deleted.

Deletes real constant sets defined with the R command.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change RealConst

Main Menu >Preprocessor >Real Constants

Main Menu >Solution >Other >Change RealConst

Sets the element real constant set attribute pointer.

PREP7:Meshing PREP7:Elements

	Mp Me St DY LP Th E3 E2 FL PP ED

Assign this real constant set number to subsequently defined elements (defaults to 1).

Notes

Identifies the real constant set number to be assigned to subsequently defined elements. This number refers to the real constant set number (NSET) defined with the real constant sets [R]. Real constant set numbers may be displayed [/PNUM]. If the element type requires no real constants, this entry is ignored. Elements of different type should not refer to the same real constant set.

Main Menu >Preprocessor >Create >Elements >Elem Attributes

Main Menu >Preprocessor >Define >Default Attribs

Forms a variable using only the real part of a complex variable.

POST26:Operations

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

Arbitrary reference number assigned to the resulting variable (2 to NV [NUMVAR]). If this number is the same as for a previously defined variable, the previously defined variable will be overwritten with this result.

Reference number of the variable to be operated on.

Unused fields.

Eight character name for identifying the variable on the printout and displays. Embedded blanks are compressed upon output.

Unused fields.

Scaling factor (positive or negative) applied to variable IA (defaults to 1.0).

Forms a variable using only the real part of a variable. Used only with harmonic analyses (ANTYPE=HARMIC).

Main Menu >TimeHist Postpro >Math Operations >Real Part

Creates a rectangular area anywhere on the working plane.

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

Working plane X coordinates of the rectangle.

Working plane Y coordinates of the rectangle.

The area will be defined with four keypoints and four lines. See the BLC4 and BLC5 commands for alternate ways to create rectangles.

Main Menu >Preprocessor >Create >Rectangle >By Dimensions

Defines a reducer in a piping run.

PREP7:Piping

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

Node where two straight pipes intersect at center of reducer. Defaults to previous run starting point.

Length of reducer (defaults to average pipe OD).

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

Defines a reducer (straight pipe element (PIPE16) with averaged specifications) in place of the intersection of two previously defined straight pipe elements in a piping run. See the PREP7 RUN command. Two new nodes are generated at the ends of the reducer. The two straight pipes are automatically "shortened" to meet the ends of the reducer. The reducer specifications and loadings are taken from the corresponding two straight pipes.

Main Menu >Preprocessor >Create >Piping Models >Reducer

Calculates the voltage reflection coefficient (REFLC), standing wave ratio (VSWR), and return loss (RL) in a COAX fed device; at postprocessing of an HF electromagnetic analysis.

POST1:Magnetics

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

Port number of the excited port with a COAX mode excitation. (See the PORTOPT command description for details.)

Port EMF (voltage) (magnitude) applied to the excited port.

Phase angle of the port EMF (voltage) (in degrees). Defaults to zero degrees.

Propagation distance between the excited port and the evaluation point. Defaults to zero (evaluation at the excited port).

Path name defining a path between conducting walls of the coax waveguide at the specified propagation distance (Pdist) from the excited port. (See also the PATH command description.)

You must specify a path [PATH command] at the propagation distance location between conducting walls of the COAX waveguide for calculating the EMF (voltage). REFLCOEF returns the parameters REFLC, VSWR, RL, and REFANG (phase angle of the reflection coefficient).

To calculate the reflection coefficient, REFLCOEF uses total and incident EMF (voltage). It prints the resulting parameters to an output device and to your screen.

See magnetic macros for further details.

Main Menu >General Postproc >Elec&Mag Calc >ReflCoeff

Renames a file.

SESSION:Files

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (32 characters maximum) to be renamed. Defaults to the current Jobname.

File name extension (8 characters maximum).

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

File name (32 characters maximum) to be created. Fname2 defaults to Fname1.

File name extension (8 characters maximum). Ext2 defaults to Ext1.

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

Renames a file. Ex: /RENAME,A,,,B renames file A to B in the same directory. /RENAME,A,DAT,,,,DIR2/ renames file A.DAT to the same name in DIR2 (on a system using "." as a name component separator and "/" as a directory separator). On all systems, this command will overwrite any existing file named B. See the ANSYS Operations Guide for details. Only ANSYS binary files should be renamed. Use /SYS and system renaming commands for other files. Note, renaming across system partitions may be internally done by a copy and delete operation on some systems.

This command is valid only at the Begin Level.

Utility Menu >File >File Operations >Rename

Specifies "Model reordering" 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.

Main Menu >Preprocessor >Numbering Ctrls >Element Reorder >List Wave Lists

Utility Menu >List >Status >Preprocessor >Reorder Module

Repeats the previous command.

APDL:ProcessControls

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of times the preceding command is executed (including the initial execution). Must be 2 or greater. NTOT of 2 causes one repeat (for a total of 2 executions).

Value increments applied to first through eleventh data fields of the preceding command.

*REPEAT must immediately follow the command that is to be repeated. The numeric arguments of the initial command may be incremented in the generated commands. The numeric increment values may be integer or real, positive or negative, zero or blank. Alphanumeric arguments cannot be incremented. For large values of NTOT, consider printout suppression (/NOPR command) first.

Most commands beginning with slash (/), star (*), as well as "unknown command" macros, cannot be repeated. For these commands, or if more than one command is to be repeated, include them within a do-loop. Graphics slash commands are an exception and can be repeated. Commands causing file switching (causing additional commands to be read) cannot be repeated. If a *REPEAT command immediately follows another *REPEAT command, the repeat action only applies to the last non-*REPEAT command. Also, *REPEAT should not be used in interactive mode immediately after a) a command (or its log file equivalent) that uses picking, or b) a command that requires a response from the user.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Automatically reissues the last display command for convenience.

GRAPHICS:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Controls the type of replot.

RESIZE - Issued internally when a graphics window resize occurs (Default).

FAST - Only applicable for 3-D devices that allow a fast redisplay for changes in the view characteristics only.

Reissues the last display command (NPLOT, EPLOT, KPLOT, PLNSOL, PLVAR, etc.), along with its parameters, for convenience. The current display specifications are used.

When the last display command is invalid in a particular processor, the use of the /REPLOT command is also invalid in that processor. However, if you attempt a /REPLOT and the last display command is invalid in the current processor, ANSYS produces an element display [EPLOT] instead, as long as the last display command was PLNSOL, PLESOL, or PLDISP. ANSYS performs this substitution of /REPLOT with EPLOT for your convenience.

For example, the PLNSOL command, which is used to display solution results as continuous contours, is a valid command in the general postprocessor [/POST1]. If you issue PLNSOL followed by /REPLOT while in the general postprocessor, the /REPLOT command effectively reissues your earlier PLNSOL command, along with its parameters. But if you then exit the general postprocessor, enter the preprocessor [/PREP7], and issue the /REPLOT command again, ANSYS internally issues EPLOT instead. This occurs because PLNSOL is not a valid command in the preprocessor.

Note that when you click on one of the buttons on the Pan-Zoom-Rotate dialog box to manipulate the view of a model, the /REPLOT command is issued internally. Thus, the substitution of /REPLOT with EPLOT as described above may occur not only for the PLNSOL, PLESOL, and PLDISP results display commands, but also for operations that you perform with the Pan-Zoom-Rotate dialog box.

This command is valid in any processor (except as noted above).

Utility Menu >Plot >Replot

Resets display specifications to their initial defaults.

GRAPHICS:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Resets slash display specifications (/WINDOW, /TYPE, /VIEW, etc.) back to their initial default settings (for convenience). Also resets the focus location to the geometric center of the object.

This command is valid in any processor.

Utility Menu >PlotCtrls >Reset Plot Ctrls

Resets all POST1 or POST26 specifications to initial defaults.

POST1:SetUp POST26:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Has the same effect as entering the processor the first time within the run. In POST1, resets all specifications to initial defaults, erases all element table items, path table data, fatigue table data, and load case pointers. In POST26, resets all specifications to initial defaults, erases all variables defined, and zeroes the data storage space.

Main Menu >General Postproc >Reset

Main Menu >TimeHist Postpro >Reset Postproc

Generates a response spectrum.

POST26:SpecialPurpose

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

Arbitrary reference number assigned to the response spectrum results (2 to NV [NUMVAR]). If this number is the same as for a previously defined variable, the previously defined variable will be overwritten with these results.

Reference number of variable containing frequency table (created with FILLDATA or DATA command). The frequency table defines the number and frequency of oscillating systems used to determine the response spectrum. The frequency interval need not be constant over the entire range. Frequencies must be input in ascending order.

Reference number of variable containing the displacement time-history.

Defines the type of response spectrum to be calculated:

0 or 1 - Displacement.

2 - Velocity.

3 - Acceleration response spectrum.

Ratio of viscous damping to critical damping (input as a decimal number).

Integration time step (ITS) size used in the numerical integration scheme. This value should be equal to or greater than that actually used in the initial transient analysis. With ANTYPE=TRANS data, DTIME defaults to a value of 1/((20)(FMAX)), where FMAX is the highest frequency in LFTAB. For reduced linear transient dynamic (ANTYPE=TRANS) displacement pass data, the ITS read from the file (previously input for DTIME in the first load step of the reduced linear transient dynamic (ANTYPE=TRANS) analysis) is used for the default.

Specifies a subset of the displacement-time history to be used in the response spectrum calculation. Defaults to the full time range.

Generates a response spectrum from displacement time-history and frequency data.

The ANSYS modal analysis (ANTYPE=MODAL) may be followed by a spectrum analysis (ANTYPE=SPECTR). This analysis requires a response spectrum input of up to 20 points. This input may be determined from the response spectrum printout or display of this command and input to the modal analysis (by hand). The response spectrum generator uses the displacements from either a full or reduced transient dynamic (ANTYPE=TRANS) analysis. If a response spectrum is to be calculated from a given displacement time-history, the displacement time-history may be input to a single one-element reduced linear transient dynamic (ANTYPE=TRANS) analysis, so that the calculated output (which should be the same as the input) will be properly located on the file.

The response spectrum is defined as the maximum response of single degree of freedom systems of varying frequency (or period) to a given input support excitation. The equation describing the response of the system in terms of the relative displacement (X) is:

where:

_n = natural frequency of the system,

_n = ratio of viscous damping to critical damping, c/c_cr

X_o = ground displacement

The solution of this equation for the maximum response, X_max, at various frequencies results in the spectral response curve. See the Section 19.11 of the ANSYS Theory Reference for calculation details.

Calculations are based on a numerical integration scheme with the displacement time-history data from the file as the input ground-forcing function. The integration time step (argument DTIME on the RESP command) and the damping coefficient (argument RATIO) are constant over the frequency range. The number of calculations done per displacement spectral response curve is the product of the number of input solution points (TMAX-TMIN)/DTIME and the number of oscillating systems (frequencies located in variable LFTAB). Input solution points requested (by DTIME and the frequency range) at a time not corresponding to an actual displacement solution time on the file are read from the next available time. The user has the option of calculating either a displacement, velocity, or acceleration spectral response.

Main Menu >TimeHist Postpro >Generate Spectrm

Resumes the database from the database file.

DATABASE:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

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

Parameter resume key:

0 - All data in the database, including the scalar parameters, are replaced with the data saved on File.DB (default).

1 - All data in the database, except the scalar parameters, are replaced with the data saved on File.DB. (Note: This option should not be used if array parameters are defined, since existing array parameters might be redefined with arbitrary values. See PARSAV and PARRES for a more general method of preventing the replacement of both scalar and array parameters.)

Using RESUME, you can resume a database file into the same version of ANSYS that the file was created in. As long as you are resuming the file into the ANSYS version that the file was created in, you do not need to manipulate or modify the file in any way. Also, although not guaranteed, you can usually resume a database file created in the previous version of ANSYS into the current version. For example, you can probably resume an ANSYS 5.2 database file into ANSYS 5.3 without encountering problems. However, ANSYS is not expected to resume an ANSYS 5.2 database file into ANSYS 5.4 or later.

RESUME causes the database file (File.DB) to be read, thereby resetting the database either a) as it was at the last SAVE command or b) as saved with the last /EXIT command, whichever was last. For multiple load step analyses, since only the data for one load step at a time may reside in the database, the load step data restored to the database will correspond to the load step data written when the save was done.

If the database file was saved [SAVE] in another ANSYS product, it may contain element type and KEYOPT specifications which are invalid in the "resuming" product. Immediately after the database resume is completed, you should redefine these invalid element types and KEYOPT settings to valid ones [ET, KEYOPT].

This command is valid in any processor. If used in SOLUTION, this command is valid only within the first load step.

Utility Menu >File >Resume Jobname.db

Utility Menu >File >Resume from

Exports displacements from an implicit run to ANSYS/LS-DYNA.

SOLUTION:ExplicitDynamics

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

The type of analysis run to which displacements are exported.

OFF - Ignore initial displacements.

DYNA - Get initial displacements from an earlier implicit (ANSYS) run and export to an explicit ANSYS/LS-DYNA run (Default).

Unused fields.

Load step number of data to be exported. Defaults to the last load step.

Substep number of data to be exported. Defaults to the last substep.

File name (32 characters maximum). No default; must be specified. The filename, however, CANNOT be the current jobname.

File name extension. Must be a .RST extension (default). Currently, only structural results are allowed.

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

This command exports the displacements, rotations, and temperatures calculated in an ANSYS implicit analysis into the `drelax' file, which is subsequently read in by ANSYS/LS-DYNA when a dynamic relaxation or stress initialization is conducted [EDDRELAX].

This command is not written to the Jobname.CDB file when the CDWRITE command is issued.

Main Menu >Preprocessor >Loads >Read Disp

Main Menu >Solution >Read Disp

Estimates file sizes.

RUNSTATS:RunStatisticsEstimator

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

Gives file size estimates for File.ESAV, File.EMAT, File.EROT, File.TRI, File.FULL, File.RST, File.RTH, and File.RMG. File sizes are given in megabytes (MB). These file estimates are for the solution of the model that currently resides in the database. This command will cause reordering [WAVES] if reordering was not already done on the model. See Chapter 18 of the ANSYS Basic Analysis Procedures Guide for file descriptions.

Main Menu >Run-Time Stats >Individual Stats

Specifies the total reaction force data to be stored.

POST26:SetUp

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

Arbitrary reference number assigned to this variable (2 to NV [NUMVAR]). Overwrites any existing results for this variable.

Node for which data are to be stored. If NODE = P, graphical picking is enabled (valid only in the GUI).

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.

Eight character name for identifying the item on the printout and displays. Defaults to an eight character label formed by concatenating the first four characters of the Item and Comp labels.

Defines the total reaction force data (static, damping, and inertial components) to be stored from single pass (ANTYPE=STATIC or TRANS) solutions or from an expansion pass of reduced two-pass (ANTYPE=HARMIC or TRANS) solutions.

Main Menu >TimeHist Postpro >Define Variables

Main Menu >TimeHist Postpro >Elec&Mag >Circuit >Define Variables

Specifies the RGB color values for indices and contours.

POST26:SetUp

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

Determines how RGB modifications will be applied.

INDEX - Specifies that subsequent color values apply to ANSYS color indices (0-15).

CNTR - Specifies that subsequent color values apply to contours (1-128). Applies to C-option devices only (i.e. X11C or Win32C).

Intensity of the color red, expressed as a percentage.

Intensity of the color green, expressed as a percentage.

Intensity of the color blue, expressed as a percentage.

First index (0-15), or contour (1-128) to which the designated RGB values apply.

Final index (0-15), or contour (1-128) to which the designated RGB values apply.

The step increment between the values N1 and N2 determining which contours or indices will be controlled by the specified RGB values.

The new maximum number of contours (1-128).

Issuing the /CMAP command (with no filename) will restore the default color settings.

Utility Menu >Plotctrls>Style>Colors>Banded Contour Map

Utility Menu >Plotctrls>Style>Colors>Default Color Map

Utility Menu >Plotctrls>Style>Colors>Reverse Video

Specifies known rigid body modes (if any) of the model.

SOLUTION:DynamicOptions

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

Up to six global Cartesian directions of the rigid modes. For a completely free 2-D model, use ALL or UX, UY, ROTZ. For a completely free 3-D model, use ALL or UX, UY, UZ, ROTX, ROTY, ROTZ. For a constrained model, use UX, UY, UZ, ROTX, ROTY, or ROTZ, as appropriate, to specify each and every unconstrained direction which exists in the model (not specifying every direction may cause difficulties in extracting the modes). Use NONE to force the subspace iteration calculation of all rigid body modes. If the structure has no constraints, the label ALL is assumed (unless substructures are present).

Notes

Specifies known rigid body modes (if any) of the model. Applies only to modal analyses with subspace iteration [MODOPT,SUBSP]. Rigid body modes specified to the program with this command are not calculated via subspace iteration, resulting in a faster solution. Any rigid body modes specified must be permitted by the applied displacement constraints (i.e., do not specify a rigid body mode in a constrained direction). Reissue the command to redefine the specification. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Imports initial stresses from an explicit run into ANSYS.

SOLUTION:FEBodyLoads

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

The type of analysis run from which stresses are imported.

OFF - Ignore initial stresses.

DYNA - Get initial stresses from an earlier explicit (ANSYS/LS-DYNA) run (Default).

Type of data imported. Note that this is an ANSYS-defined field; the only valid value is STRESS.

Location where the data is imported. Note that this is an ANSYS-defined field; the only valid value is ELEM (data imported at the element integration points).

Load step number of data to be imported. Defaults to the last load step.

Substep number of data to be imported. Defaults to the last substep.

File name (32 characters maximum). No default; must be specified. The filename, however, cannot be the current jobname.

File name extension. Must be a .RST extension (default).

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

This command imports initial stress information (in terms of resultant element force and moment vectors) and element thickness data into ANSYS from an earlier explicit (ANSYS/LS-DYNA) run. Stress information is imported only from SHELL163 elements in the explicit analysis, and applied only to SHELL181 elements in the implicit analysis. The stress information is from one averaged thickness per SHELL163 element, regardless of the number of layers (through-the-thickness integration points) or the number of planar integration points in the SHELL163 elements. This command is valid only after the first solve command of the analysis and is ignored if issued after subsequent solve commands (i.e., stresses will not be re-imported).

This command is not written to the Jobname.CDB file when the CDWRITE command is issued.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Apply >Other >Import Stress

Main Menu >Solution >Apply >Other >Import Stress

Supplies an estimate of the number of iterations for time estimates.

RUNSTATS:RunStatisticsEstimator

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

Estimated number of iterations (or load steps in a linear, static analysis) for the analysis (defaults to 1).

Notes

This estimate will be used by the program to calculate estimated run times [RTIMST].

Main Menu >Run-Time Stats >Iter Setting

Lists the real constant sets.

PREP7:RealConstants

	Mp Me St DY LP Th E3 E2 FL PP ED

List real constant sets from NSET1 to NSET2 (defaults to NSET1) in steps of NINC (defaults to 1). If NSET1 = ALL (default), ignore NSET2 and NINC and list all real constant sets [R].

The real constant sets listed contain only those values specifically set by the user. Default values for real constants set automatically within the various elements are not listed.

This command is valid in any processor.

Utility Menu >List >Properties >All Real Constants

Utility Menu >List >Properties >Specified Real Constants

Prints memory statistics for the current model.

RUNSTATS:RunStatisticsEstimator

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

Memory statistics include work space usage, database size, binary input/output buffers, and available ANSYS scratch space. Also the maximum available static wavefront that will fit in the available ANSYS scratch space is displayed. The memory statistics are displayed in units of kilobytes (KB) or megabytes (MB).

Main Menu >Run-Time Stats >Individual Stats

Modifies real constant sets.

PREP7:RealConstants

	Mp Me St DY LP Th E3 E2 FL PP ED

Existing set to be modified.

Starting location in table for modifying data. For example, if STLOC=1, data input in the V1 field is the first constant in the set. If STLOC=7, data input in the V1 field is the seventh constant in the set, etc. Must be greater than zero.

New value assigned to constant in location STLOC. If zero (or blank), a zero value will be assigned.

New values assigned to constants in the next five locations. If blank, the value remains unchanged.

Allows modifying (or adding) real constants to an existing set [R] at any location.

This command is also valid in SOLUTION.

This command cannot be accessed directly in the menu.

Adds real constants to a set.

PREP7:RealConstants

	Mp Me St DY LP Th E3 E2 FL PP ED

Add real constants 7 to 12 (numerical values or table names) to the most recently defined set.

Adds six more real constants to the most recently defined set. Repeat the RMORE command for constants 13 to 18, again for 19-24, etc.

If using table inputs (SURF151, SURF152, and FLUID116 only), enclose the table name in % signs (e.g., %tabname%).

This command is also valid in SOLUTION.

This command cannot be accessed directly in the menu.

Specifies a rocking response spectrum.

SOLUTION:SpectrumOptions

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

Global Cartesian X, Y, and Z location of center of rotation about which rocking occurs.

Global Cartesian angular velocity components associated with the rocking.

Specifies a rocking response spectrum effect in the spectrum (ANTYPE=SPECTR) analysis.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Spectrum >Settings

Main Menu >Solution >Spectrum >Settings

Creates a regular polygonal area centered about the working plane origin.

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of sides in the regular polygon. Must be greater than 2.

Length of each side of the regular polygon.

Radius of the major (or circumscribed) circle of the polygon. Not used if LSIDE is input.

Radius of the minor (or inscribed) circle of the polygon. Not used if LSIDE or MAJRAD is input.

Defines a regular polygonal area on the working plane. The polygon will be centered about the working plane origin, with the first keypoint defined at = 0°. The area will be defined with NSIDES keypoints and NSIDES lines. See the RPR4 and POLY commands for other ways to create polygons.

Main Menu >Preprocessor >Create >Polygon >By Circumscr Rad

Main Menu >Preprocessor >Create >Polygon >By Inscribed Rad

Main Menu >Preprocessor >Create >Polygon >By Side Length

Creates a regular polygonal area or prism volume anywhere on the working plane.

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

The number of sides in the polygon or prism face. Must be greater than 2.

Working plane X and Y coordinates of the center of the polygon or prism face.

Distance (major radius) from the center to a vertex of the polygon or prism face (where the first keypoint is defined).

Angle (in degrees) from the working plane X-axis to the vertex of the polygon or prism face where the first keypoint is defined. Used to orient the polygon or prism face. Defaults to zero.

The perpendicular distance (either positive or negative based on the working plane Z direction) from the working plane representing the depth of the prism. If DEPTH=0 (default), a polygonal area is created on the working plane.

Defines a regular polygonal area anywhere on the working plane or prism volume with one face anywhere on the working plane. The top and bottom faces of the prism are polygonal areas. See the RPOLY, POLY, RPRISM, and PRISM commands for other ways to create polygons and prisms.

Main Menu >Preprocessor >Create >Polygon >Hexagon

Main Menu >Preprocessor >Create >Polygon >Octagon

Main Menu >Preprocessor >Create >Polygon >Pentagon

Main Menu >Preprocessor >Create >Polygon >Septagon

Main Menu >Preprocessor >Create >Polygon >Square

Main Menu >Preprocessor >Create >Polygon >Triangle

Main Menu >Preprocessor >Create >Prism >Hexagonal

Main Menu >Preprocessor >Create >Prism >Octagonal

Main Menu >Preprocessor >Create >Prism >Pentagonal

Main Menu >Preprocessor >Create >Prism >Septagonal

Main Menu >Preprocessor >Create >Prism >Square

Main Menu >Preprocessor >Create >Prism >Triangular

Creates a regular prism volume centered about the working plane origin.

PREP7:Primitives

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

Working plane Z coordinates of the prism.

Number of sides in the polygon defining the top and bottom faces of the prism. Must be greater than 2.

Length of each side of the polygon defining the top and bottom faces of the prism.

Radius of the major (or circumscribed) circle of the polygon defining the top and bottom faces of the prism. Not used if LSIDE is input.

Radius of the minor (or inscribed circle) of the polygon defining the top and bottom faces of the prism. Not used if LSIDE or MAJRAD is input.

Defines a regular prism volume centered about the working plane origin. The prism must have a spatial volume greater than zero. (i.e., this volume primitive command cannot be used to create a degenerate volume as a means of creating an area.) The top and bottom faces are polygonal areas that are parallel to the working plane but neither face need be coplanar with (i.e., "on") the working plane. The first keypoint defined for each face is at = 0°. See the RPR4 and PRISM commands for other ways to create prisms.

Main Menu >Preprocessor >Create >Prism >By Circumscr Rad

Main Menu >Preprocessor >Create >Prism >By Inscribed Rad

Main Menu >Preprocessor >Create >Prism >By Side Length

Computes response power spectral density (PSD).

POST26:SpecialPurpose

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

Arbitrary reference number assigned to the resulting variable (2 to NV [NUMVAR]). If this number is the same as for a previous variable, the previous variable will be overwritten with this result.

Reference numbers of the two variables to be operated on. If only one, leave IB blank.

Defines the type of response PSD to be calculated:

0,1 - Displacement (default).

2 - Velocity.

3 - Acceleration.

Defines the reference with respect to which response PSD is to be calculated:

1 - Absolute value.

2 - Relative to base (default).

Eight character name for identifying the variable on listings and displays. Embedded blanks are compressed upon output.

This command computes response power spectral density (PSD) for the variables referenced by the reference numbers IA and IB. The variable referred by IR will contain the response PSD. File.PSD must be available for the calculations to occur. Requires the STORE,PSD command to be issued first.

Main Menu >TimeHist Postpro >Calc Resp PSD

Supplies system performance information for use in time estimates.

RUNSTATS:RunStatisticsEstimator

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

MIPS rating of computer (defaults to 4). This value is ignored if SMFLOP is specified.

Scalar MFLOPS rating of computer (defaults to MIPS/4).

Vector MFLOPS rating of computer (Defaults to MIPS/2).

Supplies system performance information to the program for its use in estimating run times [RTIMST]. Normally this command is invoked through the SETSPEED macro as executed by the ANSYS installation process.

Main Menu >Run-Time Stats >System Settings

Prints the FE model statistics of the model.

RUNSTATS:RunStatisticsEstimator

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

Prints the finite element model statistics of the model currently in the database. The maximum node and element number used are displayed, as well as the number of nodes and elements selected.

Main Menu >Run-Time Stats >Individual Stats

Activates a coordinate system for printout or display of results.

POST1:Controls

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

Coordinate system reference number. KCN may be 0,1,2 or any existing local coordinate system number. If KCN=SOLU, results are reported in whatever coordinate systems were associated with the results when calculated in the solution phase (i.e., the nodal and element coordinate systems). The exception is for layered shell and solid elements, for which data are transformed into the element coordinate system if LAYER=0 or if no LAYER command is issued.

Notes

Activates a coordinate system for the printout or display of results data. Results data will be rotated to this system during printout, display, or element table operations [PRNSOL, PRESOL, PLNSOL, ETABLE, etc.]. Coordinate systems can be defined with various commands [LOCAL, CS, CLOCAL, CSKP...]. If RSYS is issued with KCN>10 (i.e., a local coordinate system), and the specified system is subsequently redefined, you must reissue RSYS for results to be rotated into the redefined system.

Rotated nodal data are any of the items shown for the PRNSOL command having the Comp label COMP, such as U (displacements), S (stresses), etc. Nodal results can be properly rotated only if the resulting component set is consistent with the degree-of-freedom set at the node (the degree-of-freedom set at a node is determined by the elements attached to the node). For example, if a node does not have a UZ degree of freedom during solution, then any Z component resulting from a rotation will not print or display in POST1. Therefore, results at nodes with a single degree-of-freedom (UY only, for example) should not be rotated; that is, they should be viewed only in the nodal coordinate system or a system parallel to the nodal system (note that the command default is the global Cartesian system, which may not be parallel to the nodal system). Results at nodes with a 2-D degree-of-freedom set (UX and UY, for example) should not be rotated out of the 2-D plane.

Element component results in the database from the solution phase (KCN=SOLU) are in the element coordinate systems. For nearly all the solid elements, the default element coordinate systems are parallel to the global Cartesian coordinate system. For the shell elements and the remaining solid elements, the default element coordinate system can differ from element to element. For layered shell and layered solid elements, the default coordinate system can vary from layer to layer within the element. The element coordinate system is initially defined with the ESYS command.

If large deflection is active, the element component result directions are rotated by the amount of rigid body rotation. (However, the hyperelastic elements always produce stresses and strains in the specified results coordinate system; no rigid body rotation is added for HYPER56, HYPER58, HYPER74, HYPER84, HYPER86 and HYPER158.) Component results displayed in the global coordinate system include the element rigid body rotation from the initial global coordinate system. All other element result transformations are relative to the rotated global system. Nodal degree-of-freedom results are based on the initial (and not the updated) geometry.

PowerGraphics supports only RSYS,0; any other value for KCN causes ANSYS to revert to Full graphics, regardless of whether PowerGraphics is active. Be aware of this limitation when reviewing your results.

If you are using ANSYS/LS-DYNA, all stresses and strains output from LS-DYNA are in the global Cartesian coordinate system. Therefore, use only RSYS,0 for stresses and strains. However, if you are using composite materials, stresses can be in a local (element) coordinate system.

Main Menu >General Postproc >Options for Outp

Utility Menu >List >Results >Options

Prints runtime estimates.

RUNSTATS:RunStatisticsEstimator

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

Prints runtime estimates for the current model. A runtime estimate is given for the first iteration, for subsequent iterations, and for total runtime. The runtime estimates are itemized for such ANSYS solution components as element formulation, wavefront solution, back substitution, etc. The estimates will be for a computer system using performance attributes as described by the RSPEED command and an estimated number of iterations as specified on the RITER command. The RSPEED and RITER commands should be input before this command. Note, this command will cause reordering [WAVES] if reordering was not already done on the model.

Main Menu >Run-Time Stats >Individual Stats

Defines a pipe run.

PREP7:Piping

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

Increment (in terms of the active coordinate system components) to determine run end point. Increment is applied to branch starting point [BRANCH] or end point of previous run (whichever was later).

Number of divisions (elements) along branch (defaults to 1). A node is generated at the end of each division.

Number to be assigned to end node of branch (defaults to MAXNP + NDIV).

Number to be assigned to first element of branch (defaults to the previous maximum element number (MAXEL) + 1).

Element number increment (defaults to 1).

Defines a pipe run from a previous point to an incremental point. Nodes (and elements) are generated straight (in the active coordinate system). Elements are of type PIPE16 straight pipes. Material properties, real constants, and loads are derived from the previously defined piping specifications. Piping loads and specifications are defined with the PCORRO, PDRAG, PFLUID, PINSUL, POPT, PPRES, PSPEC, PTEMP, and PUNIT commands. Generated items may be listed (or displayed) with the standard commands (NLIST, ELIST, NPLOT, EPLOT, ETLIST, RLIST, etc.). Items may also be modified (NMODIF, EMODIF, RMODIF, etc.) or redefined as desired. See the ANSYS Modeling and Meshing Guide for details.

Main Menu >Preprocessor >Create >Piping Models >Pipe Run

Enters the run statistics processor.

SESSION:ProcessorEntry RUNSTATS:RunStatisticsEstimator

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

Enters the run statistics processor for estimating various solution size and speed statistics. Statistics include run time estimates, wavefront estimates, file size estimates, memory requirements and finite element model size information.

This command is valid only at the Begin Level.

Main Menu >Run-Time Stats

Generates wavefront statistics and memory requirements.

RUNSTATS:RunStatisticsEstimator

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

Generates current wavefront statistics, such as maximum wavefront and RMS wavefront, and memory requirements. This command will cause reordering if reordering was not already done on the model.

Main Menu >Run-Time Stats >Individual Stats