S

Specifies absolute values for element table operations.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Absolute value key:

0 - Use algebraic values in operations.

1 - Use absolute values in operations.

Notes

Causes absolute values to be used in the SADD, SMULT, SMAX, SMIN, and SSUM operations.

Main Menu >General Postproc >Element Table >Abs Value Option

Forms an element table item by adding two existing items.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to results. If same as existing label, the existing values will be overwritten by these results.

First labeled result item in operation.

Second labeled result item in operation (may be blank).

Scale factor applied to Lab1 (defaults to 1.0).

Scale factor applied to Lab2 (defaults to 1.0).

Constant value.

Forms a labeled result (see ETABLE command) for the selected elements by adding two existing labeled result items according to the operation:

May also be used to scale results for a single labeled result item. If absolute values are requested [SABS,1], absolute values of Lab1 and Lab2 are used.

Main Menu >General Postproc >Element Table >Add Items

Defines the allowable stress table for safety factor calculations.

POST1:ElementTable

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

Input up to six allowable stresses corresponding to the temperature points [TALLOW].

Defines the allowable stress table for safety factor calculations [SFACT,SFCALC]. Use STAT command to list current allowable stress table. Repeat SALLOW to zero table and redefine points (6 maximum).

Main Menu >General Postproc >Safety Factor >Constant

Main Menu >General Postproc >Safety Factor >Reset Stress

Main Menu >General Postproc >Safety Factor >Temp-depend

Displays areas smaller than a specified size (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

Preference for area display. If Prefer = FACTOR, the command displays all areas whose size is smaller than the size of the average area within the model times VALUE. This is the default preference. If Prefer = AREA, the command displays all areas that are smaller than that specified by VALUE. If Prefer=NARROW, the command displays all areas that have an aspect ratio greater than VALUE (useful for finding "sliver" areas).

Numeric value used as argument for Prefer.

Use this command to locate and display disproportionately small areas when repairing the geometry of models imported from CAD files. Areas matching the criteria specified in Prefer and VALUE both display in a different color and include their IDs. This command is available only for models imported through the Default IGES option.

Main Menu >Preprocessor >Simplify >Small Areas

Saves all current database information.

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.

Saves all current database information to a file (File.DB). In interactive mode, an existing File.DB is first written to a backup file (File.DBB). In batch mode, an existing File.DB is replaced by the current database information with no backup. The command should be issued periodically to insure a current file back-up in case of a system "crash" or a "line drop." It may also be issued before a "doubtful" command so that if the result is not what was intended the database may be easily restored to the previous state. A save may be time consuming for large models. Repeated use of this command overwrites the previous data on the file (but a backup file is first written during an interactive run). When issued from within POST1, the nodal boundary conditions in the database (which were read from the results file) will overwrite the nodal boundary conditions existing on the database file.

This command is valid in any processor.

Utility Menu >File >Save as Jobname.db

Utility Menu >File >Save as

Lists solid model boundary conditions.

SOLUTION:MiscLoads

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

Lists all solid model boundary conditions for the selected solid model entities. See also DKLIST, DLLIST, DALIST, FKLIST, SFLLIST, SFALIST, BFLLIST, BFALIST, BFVLIST and BFKLIST to list items separately.

This command is valid in any processor.

Utility Menu >List >Loads >Solid Model Loads

Transfers solid model loads and boundary conditions to the FE model.

SOLUTION:MiscLoads

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

Causes a manual transfer of solid model loads and boundary conditions to the finite element model. Loads and boundary conditions on unselected keypoints, lines, areas, and volumes are not transferred. Boundary conditions and loads will not be transferred to unselected nodes or elements. The SBCTRAN operation is also automatically done upon initiation of the solution calculations [SOLVE].

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Operate >All Solid Lds

Main Menu >Solution >Operate >All Solid Lds

Deletes BEAM188 or BEAM189 cross sections from the ANSYS database.

PREP7:CrossSections

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

SFIRST

First section ID to be deleted; defaults to first available section in the database.

Last section ID to be deleted; defaults to last available section in the database.

Increment of the section ID; defaults to 1,

Deletes one or more specified sections and their associated data from ANSYS database.

Main Menu >Preprocessor >Sections >Delete Section

Defines a superelement.

PREP7:Superelements

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

Jobname (8 character maximum) of file containing superelement. Defaults to the current Jobname.

Unused fields.

Tolerance used to determine if use pass nodes are non-coincident with master nodes having the same node numbers. Defaults to 0.0001. Use pass nodes will always be replaced by master nodes of the same node number. However, if a use pass node is more than TOLER away from the corresponding master node, a warning is generated.

Defines a superelement by reading in the superelement matrices and master nodes from the superelement matrix file. The matrix file (File.SUB) must be available from the substructure generation pass. The proper element type (MATRIX50) must be active [TYPE] for this command. A scratch file called File.SORD showing the superelement names and their corresponding element numbers is also written.

Main Menu >Preprocessor >Create >Elements >From .SUB File

Describes the geometry of a BEAM188 or BEAM189 section.

PREP7:CrossSections

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

Values, such as the length of a side or the numbers of cells along the width, that describe the geometry of a beam section. See Figure 3.1 for a description of these values for the various beam sections.

Defines the data describing the geometry of a BEAM188 or BEAM189 section. The data is interpreted based on the most recently issued SECTYPE command. The data required is determined by the section subtype, and is different for each subtype. Not all SECOFFSET location values are valid for each subtype.

Subtype: RECT

Data to be supplied in the value fields:

B,H, Nb, Nh
B=Width
H=Height
Nb=Number of cells along width, default=2
Nh=Number of cells along height, default=2
Nb*Nh<25

Subtype: QUAD

Data to be supplied in the value fields:

yI,zI,yJ,zJ,yK,zK,yL,zL, Ng, Nh
yI,zI,yJ,zJ,yK,zK,yL,zL=Coordinate location of various points
Ng=Number of cells along g, default=2
Nh=Number of cells along h, default=2
Ng*Nh<25
Note-Degeneration to triangle is permitted by specifying same coordinates for cells along an edge.

Subtype: CSOLID

Data to be supplied in the value fields:

R, N
R=Radius
N=Number of cells along the circumference; default=8, N12

Subtype: CTUBE

Data to be supplied in the value fields:

Ri, Ro, N
Ri= Inner radius of the tube
Ro= Outer radius of the tube
N=Number of cells along the circumference; default=8, N12

Subtype: CHAN

Data to be supplied in the value fields:

W1,W2,W3, t1,t2 t3
W1,W2=Lengths of the flanges
W3=Overall depth
t1,t2=Flange thicknesses
t3=Web thickness

Subtype: I

Data to be supplied in the value fields:

W1,W2,W3, t1,t2 t3
W1,W2=Width of the top and bottom flanges
W3=Overall depth
t1,t2=Flange thicknesses
t3=Web thickness

Subtype: Z

Data to be supplied in the value fields:

W1, W2, W3, t1, t2, t3
W1,W2=Flange lengths
W3=Overall depth
t1,t2=Flange thicknesses
t3=Stem thickness

Subtype: L

Data to be supplied in the value fields:

W1, W2, t1, t2
W1,W2=Leg lengths
t1, t2=Leg thicknesses

Subtype: T

W1, W2, t1, t2

W1=Flange width
W2=Overall depth
t1=Flange thickness
t2=Stem thickness

Subtype: HATS

Data to be supplied in the value fields:

W1,W2,W3,W4, t1,t2 t3,t4,t5
W1,W2=Width of the brim
W3=Width of the top of the hat
W4=Overall depth
t1,t2=Thickness of the brim
t3=Thickness of the top of the hat
t4,t5=Web thicknesses

Subtype: HREC

Data to be supplied in the value fields:

W1, W2, t1, t2, t3,t4
W1=Outer width of the box
W2=Outer height of the box
t1,t2,t3,t4=Wall thicknesses

Subtype: ASEC

Arbitrary-User-supplied integrated section properties instead of basic geometry data

Data to be supplied in the value fields:

A, Iyy, Iyz, Izz, Iw, J, CGy, CGz, SHy, SHz
A - Area of section
Iyy - Moment of inertia about the y axis
Iyz - Product of inertia
Izz - Moment of inertia about the z axis
Iw - Not supported (for future use - sum of the moments of inertia)
J - Torsional constant
CGy - Y coordinate of centroid
CGz - Z coordinate of centroid
SHy - Shear deflection constant
SHz - Shear deflection constant

Subtype: MESH

User-defined mesh

Data required is created by the SECWRITE command and is read into ANSYS by the SECREAD command. See the SECREAD command for more information about this data.

When user mesh is input using SECREAD, ANSYS calculates the area, second moments of inertia, centroid and, torsion constant. However, ANSYS cannot calculate the location of shear center. SECOFFSET,USER may be used to locate the beam node.

This restriction does not apply to the common thin-walled library cross sections of subtype L, CHANNEL, I, T and HATS. The calculation of shear center and its offset with respect to centroid are supported for such cross sections.

Main Menu >Preprocessor > Sections > Common Sectns

Sets the default section library path for the SECREAD command.

PREP7:CrossSections

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

READ - Sets the read path (default)

STATUS - Reports the current section library path setting to the Jobname.log file

Defines the directory path from which to read section library files.

When the SECREAD command is given without a directory path, the command searches for a section library in the following order:

· the current working directory

· the path specified by the /SECLIB command

Menu Paths

Main Menu >Preprocessor >Sections >Section Library >Library Path

Sets the element section attribute pointer

PREP7:CrossSections

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

Defines the section ID number to be assigned to the subsequently-defined elements by the LMESH, E or EN commands. Defaults to 1. See SECTYPE for more information about the section ID number.

Main Menu >Preprocessor >Create >Elements >Elem Attributes

Main Menu >Preprocessor >Define >Default Attribs

Defines the section offset for BEAM188 and BEAM189 cross sections.

PREP7:CrossSections

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

CENT - Beam node will be offset to Centroid (Default)

SHRC - Beam node will be offset to Shear Center

ORIGIN - Beam node will be offset to origin of the cross section

USER - Beam node will be offset to user specified location input in the OFFSETY, OFFSETZ

Values that locate the node with respect to the default origin of cross section when Location field is set to USER-valid only when USER is set.

Figure 3.2 illustrates the offsets for the a channel cross section, illustrating the relative locations of SHRC and CENT.

Notes

The offsets defined by the SECOFFSET command are associated with the section most recently defined using the SECTYPE command. Not all SECOFFSET location values are valid for each subtype.

Main Menu >Preprocessor >Sections >Common Sectns

Plots the geometry of a beam section to scale.

PREP7:CrossSections

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

The section ID number as defined by the SECTYPE command.

Valid only for BEAM sections. Plots the geometry of the beam section to scale depicting the centroid, shear center and origin. SECPLOT also lists various section properties such as Iyy, Iyz, Izz.

A sample section plot for the CHAN section subtype is shown below.

SECPLOT cannot display the plots of the ASEC or MESH subtypes.

Main Menu >Preprocessor >Sections >Plot Section

Reads a customized beam section library or a user-defined beam section mesh into ANSYS.

PREP7:CrossSections

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

Section library filename, up to 32 characters in length. Defaults to Jobname if Fname is left blank.

Section library file extension, up to 8 characters in length. Defaults to SECT if Ext is blank.

Name of the directory containing the section library file, up to 64 characters in length. When the SECREAD command is given without a directory path, the command searches for a section library in the following order:

· the current working directory

· the path specified by the /SECLIB command

Option

LIBRARY - Reads in a library of sections and their associated section data values; the default. A section library may be created by editing the section-defining portions of the Jobname.log file and saving it with a .SECT suffix. AISC section libraries and other section libraries may be read by this command.

MESH - Reads in a user mesh section file containing the cell connectivity, cell flags, node boundary flags and nodal coordinates for the current beam section of subtype MESH as defined by SECTYPE. A maximum of either 25 cells or 125 nodes are allowed in the definition of the beam section. See Sample User Section Cell Mesh File for details about this file. SECWRITE builds mesh files based on 2-D models created by the user.

Here are excerpts from a sample user section mesh file for a section with 77 nodes, 15 cells and 9 nodes per cell for a two-hole box section, shown in Figure 3.4. The cell mesh for this section is shown in Figure 3.5.

The mesh file is divided into three sections: the First Line, the Cells Section and the Nodes Section. Here are brief descriptions of the contents of each section.

First Line: The First Line defines the number of nodes and the number of cells for the mesh.

Cells Section: The Cells Section contains as many lines as there are cells. In the previous sample, there are fifteen cells, so there are fifteen lines in this section. Each cell line contains the node numbers related to each cell and a cell flag (1.0 or 0.0) at the end.

When the cell flag is set to 1.0, the cell is part of the cross section where section material exists and is considered a real cell. When this flag is set to 0.0, the cell is part of the cross section where section material does not exist and is considered a pseudo cell. Real cells and pseudo cells have an associated element type number (ET) to be used with the SECWRITE command.

Note that cell nodal connectivity must be given in a counter-clockwise direction, with the center node being the ninth node. See Figure 3.5 for an illustration.

Nodes Section: The nodes section contains as many lines as there are nodes. In the previous sample, there are 77 nodes, so there are a total of 77 lines in this section. Each node line contains the nodes boundary flag, Y coordinate of the node and the Z coordinate of the node.

The nodes boundary flag is set to either 1 or 0. When this flag is set to 1, the node lies on the exterior boundary of the section; see Figure 3.4 for an illustration. When the flag is set to 0, the node lies on the interior boundary or internal part of the section. Note that there cannot be a gap in node numbering. The node number must start at one and end at the maximum node number.

Figure 3.5 Cell Mesh for the Two-hole Box Section

When user mesh is input using SECREAD, ANSYS calculates the area, second moments of inertia, centroid and, torsion constant. However, ANSYS cannot calculate the location of shear center. SECOFFSET,USER may be used to locate the beam node.

This restriction does not apply to the common thin-walled library cross sections of subtype L, CHANNEL, I, T and HATS (see the SECDATA command for details). The calculation of, and offset to shear center, is supported for such cross sections.

Main Menu >Preprocessor >Sections >Read Sect Mesh

Main Menu >Preprocessor >Sections >Section Library >Import Library

Associates section type information with a section ID number.

PREP7:CrossSections

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

Section identification number.

BEAM

Defines a beam section. This is currently the only value available for the Type argument.

When Type set to beam the various possible beam sections that can be defined on the Subtype field are:

The following figure shows the shape of each cross section subtype:

See Figure 3.1 in the SECDATA command for detailed illustrations of the BEAM section subtypes and their associated geometric data.

An 8 character string name for the section. Name could be a string such as "W36X210" or "HP13X73" for beam sections. Name must follow ANSYS naming conventions. Section names may contain letters and numbers, and cannot contain punctuation, special characters or spaces.

SECTYPE sets the section ID number, section type, and subtype for a section. If the section ID number is not specified, ANSYS increments the highest section ID number currently defined in the database by one. A previously-defined section with the same identification number will be redefined. The geometry data describing this section type is defined by subsequent SECDATA command. The offsets for beam section can be defined by a subsequent SECOFFSET command. ANSYS builds a numeric model using a nine node cell for determining the properties (Ixx, Iyy, etc.) of the section and for the solution to the Poisson's equation for torsional behavior. The SLIST command lists the section properties and the SECPLOT command displays the section to scale. The SECNUM command assigns the section ID number to a subsequently defined beam element. See Chapter 8 of the ANSYS Advanced Analysis Techniques Guide for a sample problem using section commands.

Main Menu >Preprocessor >Sections >Common Sectns

Creates an ASCII file containing user mesh section information.

PREP7:CrossSections

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

User mesh section filename, up to 32 characters in length. Defaults to Jobname if Fname is left blank.

User mesh section file extension, up to 8 characters in length. Defaults to SECT if Ext is blank.

Name of the directory containing the user mesh section file, up to 64 characters in length. Defaults to the current working directory if Dir is left blank.

Element type attribute pointer (ET) for the elements that are part of the section where material exists (real cells). See SECREAD for a detailed description.

Element type attribute pointer (ET) for the elements that are part of the section where material does not exist (pseudo cells). See SECREAD for a detailed description.

An alphanumeric name of up to eight characters in length which points to a NODE component [CM]. The NODE component contains all the nodes that lie on the exterior boundary of the section (see Figure 3.4). See SECREAD for more information.

Before creating a user mesh file, you must create a model using ANSYS 2-D meshing capabilities. Use PLANE82 to model the real cells and pseudo cells that make up the cell mesh and LESIZE to set the line division information. User mesh should be written using closed cell sections, and the number of cells is limited to no more than 25 per section. SECWRITE creates an ASCII file that containing all nodes, node boundary flags, cells and cell flags that describe a beam section. For detailed information on how to create a user mesh file, see Section 8.5 of the ANSYS Advanced Analysis Techniques Guide

When user mesh is input using SECREAD, ANSYS calculates the area, second moments of inertia, centroid and, torsion constant. However, ANSYS cannot calculate the location of shear center. SECOFFSET,USER may be used to locate the beam node.

This restriction does not apply to the common thin-walled library cross sections of subtype L, CHANNEL, I, T and HATS. The calculation of, and offset to shear center, is supported for such cross sections.

Main Menu >Preprocessor > Sections > Write Sec Mesh

Defines the excitation direction for a single-point response spectrum.

SOLUTION:SpectrumOptions

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

Global Cartesian coordinates of a point that defines a line (through the origin) corresponding to the excitation direction. For example: 0.0, 1.0, 0.0 defines global Y as the spectrum direction. Spectrum values are not scaled with this input.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Spectrum >Settings

Main Menu >Preprocessor >Loads >Spectrum >DDAM Options

Main Menu >Solution >Spectrum >Settings

Main Menu >Solution >Spectrum >DDAM Options

Lists the DOF solution of a superelement after the use pass.

PREP7:Superelements

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

Name of the superelement on File.DSUB to be listed. If a number, it is the element number of the superelement as used in the use pass. If ALL, list results for all superelements.

List key:

0 - List summary data only.

1 - List full contents. Warning, listing may be extensive.

Lists the degree of freedom solution of a superelement after the substructure use pass. Results may be listed for any superelement on File.DSUB.

This command is valid in any processor.

Main Menu >General Postproc >List Results >Superelem DOF

Utility Menu >List >Results >Superelem DOF Solu

Specifies options for the substructure expansion pass.

SOLUTION:AnalysisOptions

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

Name of the superelement matrix file created by the substructure generation pass (Sename.SUB). Defaults to the initial Jobname "File." If a number, it is the element number of the superelement as used in the use pass.

Name of the file containing the superelement degree-of-freedom (DOF) solution created by the substructure use pass (Usefil.DSUB).

Key to specify use of the imaginary component of the DOF solution. Applicable only if the use pass is a harmonic (ANTYPE=HARMIC) analysis:

OFF - Use real component of DOF solution (default).

ON - Use imaginary component of DOF solution.

Specifies options for the expansion pass of the substructure analysis (ANTYPE=SUBSTR). 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 >ExpansionPass >Expand Superelem

Main Menu >Solution >ExpansionPass >Expand Superelem

Allows graphics data to be stored in the local terminal memory.

GRAPHICS:SetUp DISPLAY:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Storage key:

SINGL - Store subsequent display in a single segment (overwrites last storage).

MULTI - Store subsequent displays in unique segments [ANIM].

DELET - Delete all currently stored segments.

OFF - Stop storing display data in segments.

STAT - Display segment status.

PC - This option only applies to PC ANSYS releases and only when animating via the AVI movie player (i.e., /DEVICE,ANIM,2). This command appends frames to the file.avi, so that the animation goes in both directions (i.e., Forward--Backward--Forward). You must have a current animation file to use this option.

Notes

Allows graphics data to be stored in the terminal local memory (device-dependent). Storage occurs concurrently with the display.

This command is valid in any processor.

Utility Menu >PlotCtrls >Redirect Plots >To Segment Memory

Utility Menu >PlotCtrls >Redirect Plots >Delete Segments

Utility Menu >PlotCtrls >Redirect Plots >Segment Status

Lists the contents of a superelement matrix file.

PREP7:Superelements

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

Name of the superelement matrix file created by the substructure generation pass (Sename.SUB). Defaults to the current Jobname. If a number, it is the element number of the superelement as used in the use pass.

List key:

0 - List summary data only.

1 - List contents, except load vectors and matrices.

2 - List contents, except matrices.

3 - List full contents. Warning; listing may be extensive.

This command is valid in any processor.

Utility Menu >List >Other >Superelem Data

Specifies "Superelements" 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 >Superelements

Determines the stored magnetic energy or co-energy.

POST1:Magnetics

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

Item to be calculated:

0 - Stored magnetic energy.

1 - Stored magnetic co-energy.

Analysis type:

0 - Static or transient.

1 - Harmonic.

SENERGY invokes an ANSYS macro which calculates the stored magnetic energy or co-energy for all selected elements. (For a harmonic analysis, the macro calculates a time-averaged (rms) stored energy.) A summary table listing the energy by material number is produced. The energy density is also calculated and stored on a per-element basis in the element table [ETABLE] with the label MG_ENG (energy density) or MG_COENG (co-energy density). The macro erases all other items in the element table [ETABLE] and only retains the energy density or co-energy density. Use the PLETAB and PRETAB commands to plot and list the energy density. The macro is valid for static and low-frequency magnetic field formulations. The macro will not calculate stored energy and co-energy for the following cases:

· Orthotropic nonlinear permanent magnets.

· Orthotropic nonlinear permeable materials.

· Temperature dependent materials.

Menu Paths

Main Menu >General Postproc >Elec&Mag Calc >Co-Energy

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

Specifies substructure analysis options.

SOLUTION:AnalysisOptions

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

Name assigned to the superelement matrix file. The matrix file will be named Sename.SUB. This field defaults to Fname on the /FILNAME command.

Matrix generation key:

1 - Generate stiffness (or conductivity) matrix (default).

2 - Generate stiffness and mass (or conductivity and specific heat) matrices.

3 - Generate stiffness, mass and damping matrices.

Print key:

0 - Do not print superelement matrices or load vectors.

1 - Print both load vectors and superelement matrices.

2 - Print load vectors but not matrices.

Stress stiffening key:

0 - Do not save space for stress stiffening in a later run.

1 - Save space for the stress stiffening matrix (calculated in a subsequent generation run after the expansion pass).

Specifies substructure analysis options (ANTYPE=SUBSTR). 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

Performs a symmetry operation on a superelement within the use pass.

PREP7:Superelements

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

Name of the superelement matrix file created by the substructure generation pass (Sename.SUB). Defaults to the current Jobname. If a number, it is the element number of a previously defined superelement in the current use pass.

Symmetry key:

X - X symmetry (default).

Y - Y symmetry.

Z - Z symmetry.

Increment all nodes in the superelement by INC.

File name (32 characters maximum) to be assigned. This field must be input.

File name extension (8 characters maximum). Defaults to SUB.

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

Performs a symmetry operation on a superelement within the substructure use pass by reversing the sign of component Ncomp in the global Cartesian coordinate system. The node numbers are incremented by INC. The new superelement is written to File.SUB in the current directory (by default). All master node nodal coordinate systems must be global Cartesian (no rotated nodes allowed).

The maximum number of transformations for a given superelement is five (including SETRAN, SESYMM, and the large rotation transformation if NLGEOM is ON in the use pass).

Main Menu >Preprocessor >Create >Elements >By Reflection

Assigns values to user-named parameters.

APDL:Parameters

	Mp Me St DY LP Th E3 E2 FL PP ED

An alphanumeric name used to identify this parameter. Par may be up to eight characters, beginning with a letter and containing only letters, numbers, and underscores. Examples: ABC A3X TOP_END ANSYS command names, function names, label names, etc. should not be used. Parameter names beginning with an underscore (e.g., _LOOP) are reserved for use by ANSYS and should be avoided. Parameter names ending in an underscore are not listed by the *STATUS command. Array parameter names must be followed by a subscript, and the entire expression must be 32 characters or less. Examples: A(1,1) NEW_VAL(3,2,5) RESULT(1000). There is no character parameter substitution for the Par field.

Numerical value or alphanumeric character string (up to 8 characters enclosed in single quotes) to be assigned to this parameter. Examples: A(1,3)=7.4 B='ABC3' May also be a parameter or a parametric expression. Examples: C=A(1,3) A(2,2)=(C+4)/2 If blank, delete this parameter. Example: A= deletes parameter A.

If Par is an array parameter, values VAL2 through VAL10 (up to the last non-blank value) are sequentially assigned to the succeeding array elements of the column. Example: *SET,A(1,4),10,11 assigns A(1,4)=10, A(2,4)=11. *SET,B(2,3),'file10','file11' assigns B(2,3)='file10', B(3,3)='file11'.

Assigns values to user-named parameters that may be substituted later in the run. The equivalent (and recommended) format is

which may be used in place of *SET,Par, ... for convenience.

This command is valid in any processor.

Parameters (numeric or character) may be scalars (single valued) or arrays (multiple valued in one, two, or three dimensions). Up to 1000 unique parameter names may be defined in any ANSYS run (fewer than 1000 are available to the user due to GUI and ANSYS macro requirements); however, a single array parameter name can represent any number of values. Parameter values may be redefined at any time. Array parameters may also be assigned values within a do-loop [*DO] for convenience. Internally programmed do-loop commands are also available with the *V-- commands (see *VFILL for an example). Parameter values (except for parameters ending in an underscore) may be listed with the *STATUS command, displayed with the *VPLOT command (numeric parameters only), and modified with the *VEDIT command (numeric parameters only). A parameter can be deleted by redefining it with a blank VALUE. If the parameter is an array, the entire array is deleted. Parameters may also be defined by a response to a query with the *ASK command or from an "ANSYS-supplied" value with the *GET command.

Array parameters must be dimensioned [*DIM] before being assigned values. Scalar parameters that are not defined are initialized to a "near" zero value. Numeric array parameters are initialized to zero when dimensioned, and character array parameters are initialized to blank. An existing array parameter must be deleted before it can be redimensioned. Array parameter names must be followed by a subscript list (enclosed in parentheses) identifying the element of the array. The subscript list may have one, two, or three values (separated by commas). Typical array parameter elements are A(1,1), NEW_VAL(3,2,5), RESULT(1000). Subscripts for defining an array element must be integers (or parameter expressions that evaluate to integers). Non-integer values are rounded to the nearest integer value. All array parameters are stored as three-dimensional arrays with the unspecified dimensions set to 1. For example, the 4th array element of a 1-dimensional array, A(4), is stored as array element A(4,1,1). Arrays are patterned after standard FORTRAN conventions.

If the parameter name Par is input in a numeric argument of a command, the numeric value of the parameter (as assigned with *SET, *GET, =, etc.) is substituted into the command at that point. Substitution occurs only if the parameter name is used between blanks, commas, parentheses, or arithmetic operators (or any combination) in a numeric argument. Substitution can be prevented by enclosing the parameter name Par within single quotes ( ' ), if the parameter is alone in the argument; if the parameter is part of an arithmetic expression, the entire expression must be enclosed within single quotes to prevent substitution. In either case the character string will be used instead of the numeric value (and the string will be taken as 0.0 if it is in a numeric argument).

A forced substitution is available in the text fields of the /TITLE,/STITLE, /TLABEL,/SYP (ARG1-ARG8), and *ABBR commands by enclosing the parameter within percent (%) signs. Also, parameter substitution may be forced within the file name, extension, or directory fields of commands having these fields by enclosing the parameter within percent (%) signs. Array parameters [*DIM] must include a subscript (within parentheses) to identify the array element whose value is to be substituted, such as A(1,3). Out-of-range subscripts result in an error message. Non-integer subscripts are allowed when identifying a TABLE array element for substitution. A proportional linear interpolation of values among the nearest array elements is performed before substitution. Interpolation is done in all three dimensions. Note, interpolation is based upon the assigned index numbers which must be defined when the table is filled [*DIM].

Most alphanumeric arguments permit the use of character parameter substitution. When the parameter name Par input, the alphanumeric value of the parameter is substituted into the command at that point. Substitution can be suppressed by enclosing the parameter name within single quotes ( ' ). Forced substitution is available in some fields by enclosing the parameter name within percent (%) signs. Valid forced substitution fields include command name fields, Dir (directory) arguments, Fname (filename) or Ext (extension) arguments, /SYP command (ARG1-ARG8 arguments), *ABBR command (Abbr arguments), /TITLE and /STITLE commands (Title argument) and /TLABEL command (Text argument). Character parameter substitution is also available in the *ASK, *CFWRITE, *IF, *ELSEIF, *MSG , *SET, *USE, *VREAD, and *VWRITE commands. Character array parameters must include a subscript (within parentheses) to identify the array element whose value is to be substituted.

If a parameter operation expression is input in a numeric argument, the numeric value of the expression is substituted into the command at that point. Allowable operation expressions are of the form

where E1, E2, etc. are expressions connected by operators (o). The allowable operations (o) are

For example, A+B**C/D*E is a valid operation expression. The * represents multiplication and the ** represents exponentiation. Note, exponentiation of a negative number (without parentheses) to an integer power follows standard FORTRAN hierarchy conventions; that is, the positive number is exponentiated and then the sign is attached. Thus, -4**2 is evaluated as -16. If parentheses are applied, such as (-4)**2, the result is 16.

A parameter is evaluated as a number within parentheses before exponentiation. Exponentiation of a negative number to a non-integer power is performed by exponentiating the positive number and prepending the minus sign, for example, -4**2.3 is -(4**2.3). The < and > operators allow conditional substitution. For example, E1<E2 substitutes the value of E1 if the comparison is true or the value of E2 if the comparison is false.

Spaces should not be used around operation symbols since " *" (a space and a star) makes the rest of the line a comment. Operation symbols (or symbols and signs) may not be immediately adjacent to each other. Parentheses may be used to separate symbols and signs, to determine a hierarchy of operations, or for clarity. For example, A**(-B) must be used instead of A**-B. Numbers ending with +0nn or -0nn are assumed to be of exponential form (as written on files by some computer systems) so that 123-002 is 123E-2 while 123-2 is 121. This form of exponential data should not be input directly by users. The default hierarchy follows the standard FORTRAN conventions, namely:

· then exponentiation (right to left)

· then multiplication or division (left to right)

· then unary association (such as +A or -A)

· then addition or subtraction (left to right)

· then logical evaluations (left to right).

Expressions (E) may be a constant, a parameter, a function, or another operation expression (of the form E1oE2oE3...oE10). Functions are of the form FTN(A) where the argument (A) may itself be of the form E1oE2oE3...oE10. Operations are recursive to a level of four deep (three levels of internally nested parentheses). Iterative floating point parameter arithmetic should not be used for high precision input because of the accumulated numerical roundoff error.

Valid functions (which are based on standard FORTRAN functions where possible) are:

SIN(X) - Sine.

COS(X) - Cosine.

TAN(X) - Tangent.

ASIN(X) - Arcsine.

ACOS(X) - Arccosine.

ATAN(X) - Arctangent.

ATAN2(Y,X) - Arctangent (Y/X) with the sign of each component considered.

SINH(X) - Hyperbolic sine.

COSH(X) - Hyperbolic cosine.

TANH(X) - Hyperbolic tangent.

SQRT(X) - Square root.

ABS(X) - absolute value.

SIGN(X,Y) - Absolute value of X with sign of Y. Y=0 results in positive sign.

NINT(X) - Nearest integer.

MOD(X,Y) - Remainder of X/Y Y=0 returns zero (0).

EXP(X) - Exponential.

LOG(X) - Natural log.

LOG10(X) - Common log.

RAND(X,Y) - Random number, where X is the lower bound, and Y is the upper bound.

GDIS(X,Y) - Random sample of Gaussian distributions, where X is the mean, and Y is the standard deviation.

LWCASE(CPARM) Lowercase equivalent of character parameter CPARM.

UPCASE(CPARM) - Uppercase equivalent of character parameter CPARM.

VALCHR(CPARM) - Numeric value of character parameter CPARM (If CPARM is a numeric parameter, returns 0.0).

CHRVAL(PARM) - Character value of numerical parameter PARM. For ABS(PARM) < 10, character value format is F8.5; for 10 ABS(PARM) < 1000, format is F8.3; for 1000 ABS(PARM) < 1000000, format is F8.0. Otherwise result is 0.0 and is not a character value.

Function arguments (X,Y,etc.) must be enclosed within parentheses and may be numeric values, parameters, or expressions. Input arguments for angular functions must evaluate to radians by default. Output from angular functions are also in radians by default. See the *AFUN command to use degrees instead of radians for the angular functions. See the *VFUN command for applying these parameter functions to a sequence of array elements. Additional functions, called "get functions" are described with the *GET command.

Main Menu >Solution >Electromagnet >Induct Matrix

Utility Menu >Parameters >Scalar Parameters

Defines the data set to be read from the results file.

POST1:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Load step number of the data set to be read (defaults to 1):

N - Read load step N.

FIRST - Read the first data set (SBSTEP and TIME are ignored).

LAST - Read the last data set (SBSTEP and TIME are ignored).

NEXT - Read the next data set (SBSTEP and TIME are ignored). If at the last data set, the first data set will be read as the next.

NEAR - Read the data set nearest to TIME (SBSTEP is ignored). If TIME is blank, read the first data set.

LIST - Scan the results file and list a summary of each load step. (FACT, KIMG, TIME and ANGLE are ignored.)

Substep number (within Lstep). For the Buckling (ANTYPE=BUCKLE) analysis or the Modal (ANTYPE=MODAL) analysis, the substep corresponds to the mode number. Defaults to last substep of load step (except for ANTYPE=BUCKLE or MODAL). If Lstep=LIST, SBSTEP=0 or 1 lists the basic step information, whereas SBSTEP=2 also lists the load step title, and labels imaginary data sets if they exist. Default maximum is 1000. When the number of substeps exceeds this limit, you need to issue SET,Lstep,LAST to bring in the 1000th load step. Use /CONFIG to increase the limit.

Scale factor applied to data read from the file. If zero (or blank), a value of 1.0 is used. A nonzero factor excludes non-summable items (see the ANSYS Basic Analysis Procedures Guide). Harmonic velocities or accelerations may be calculated from the displacement results from a Modal (ANTYPE=MODAL) or Harmonic Response (ANTYPE=HARMIC) analyses. If FACT=VELO, the harmonic velocities (v) are calculated from the displacements (d) at a particular frequency (f) according to the relationship v=2fd. Similarly, if FACT=ACEL, the harmonic accelerations (a) are calculated as a = (2f)²d.

Used only with results from complex analyses.

0 - Store real part of complex solution.

1 - Store imaginary part. (Note-For damped modal solutions, the imaginary part of the eigenvalue represents the frequency of the system.)

Time-point identifying the data set to be read. For the Harmonic response analyses, time corresponds to the frequency. For the Buckling analysis, time corresponds to the load factor. Used only in the following cases: If Lstep=NEAR, read the data set nearest to TIME. If both Lstep and SBSTEP are zero (or blank), read data set at time = TIME. Do not use TIME to identify the data set to be read if you used the arc-length method [ARCLEN] in your solution. If TIME is between two solution time points on the results file, a linear interpolation is done between the two data sets. Solution items not written to the results file [OUTRES] for either data set will result in a null item after data set interpolation. If TIME is beyond the last time point on the file, the last time point will be used.

Circumferential location (0.0 to 360°). Defines the circumferential location for the harmonic calculations used when reading from the results file. The harmonic factor (based on the circumferential angle) is applied to the harmonic elements (PLANE25, PLANE75, PLANE78, FLUID81, PLANE83, and SHELL61) of the load case. See Section 19.9 of the ANSYS Theory Reference for details. Note that factored values of applied constraints and loads will overwrite any values existing in the database. If ANGLE=NONE, all harmonic factors are set to 1 and postprocessing will yield the solution output. When using ANGLE=NONE with MODE>0, the combined stresses and strains are not valid. The default value of ANGLE is 0.0, but if the SET command is not used, the effective default is NONE.

Data set number of the data set to be read. If a positive value for NSET is entered, Lstep, SBSTEP, KIMG, and TIME are ignored. Available set numbers can be determined by SET,LIST.

Defines the data set to be read from the results file into the database. Various operations may also be performed during the read operation. The database must have the model geometry available (or use the RESUME command before the SET command to restore the geometry from File.DB). Values for applied constraints [D] and loads [F] in the database will be replaced by their corresponding values on the results file, if available (see the OUTRES command). In a single loadstep analysis, these values are usually the same, except for results from harmonic elements (see ANGLE above).

Main Menu >General Postproc >By Load Step

Main Menu >General Postproc >By Set Number

Main Menu >General Postproc >By Time/Freq

Main Menu >General Postproc >First Set

Main Menu >General Postproc >Last Set

Main Menu >General Postproc >Next Set

Main Menu >General Postproc >List Results >Results Summary

Main Menu >General Postproc >Modal Cyclic Sym

Main Menu >General Postproc >Results Summary

Utility Menu >List >Results >Load Step Summary

Creates a superelement from an existing superelement.

PREP7:Superelements

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

Name of the file containing the original superelement matrix created by the generation pass (Sename.SUB). Defaults to the current Jobname. If Sename is a number, it is the element number of a previously defined superelement in the current use pass.

Reference number of coordinate system where the superelement is to be transferred to. Defaults to the global Cartesian system. Transfer occurs from the active coordinate system.

Node offset. Defaults to zero. All new element node numbers will be offset from those on the original by INC.

Name of the file (32 characters maximum) the new superelement is to be written to. This field must be input.

File name extension (8 characters maximum). Defaults to SUB.

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

Node location increments in the global Cartesian coordinate system. Defaults to zero.

Node rotation key:

0 - The nodal coordinate systems of the transferred superelement will also be rotated into the KCNTO system (i.e., the nodal coordinate systems will rotate with the superelement). The superelement matrices are not modified.

1 - The nodal coordinate systems will not be rotated (they will remain fixed in their original global orientation). The superelement matrices and load vectors are modified if any rotations are done. Note: if this option is chosen for models with displacement degrees of freedom, and KCNTO is not the active system, the superelement Sename must have six MDOF at each node.

Creates a superelement from an existing superelement and writes the new element to a file. The new element may then be read in (during the use pass) with an SE command. Superelements may be created from the original by transferring its (the original's) geometry from the active coordinate system into another coordinate system (KCNTO), by offsetting its geometry in the global Cartesian coordinate system (DX, DY, and DZ ), or by offsetting its node numbers (INC). All three methods may be used in combination. If both the geometry transfer and the geometry offset are used, the transfer is done first.

The maximum number of transformations for a given superelement is five (including SETRAN, SESYMM, and the large rotation transformation if NLGEOM is ON in the use pass).

Main Menu >Preprocessor >Create >Elements >By CS Transfer

Main Menu >Preprocessor >Create >Elements >By Geom Offset

Forms an element table item by exponentiating and multiplying.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to results. If same as existing label, the existing values will be overwritten by these results.

First labeled result item in operation.

Second labeled result item in operation (may be blank).

Exponent applied to Lab1.

Exponent applied to Lab2.

Forms a labeled result item (see ETABLE command) for the selected elements by exponentiating and multiplying two existing labeled result items according to the operation:

Roots, reciprocals, and divides may also be done with this command.

Main Menu >General Postproc >Element Table >Exponentiate

Specifies surface loads on nodes.

SOLUTION:FESurfaceLoads

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

Nodes defining the surface upon which the load is to be applied. Use the label ALL or P, or a component name. If ALL, all selected nodes [NSEL] are used (default). If P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each element type in the ANSYS Elements Reference. Structural labels: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux). RAD (radiation). Acoustic Fluid labels: FSI (fluid-structure interaction flag); IMPD (impedance); PTOT (constant total pressure. Magnetic labels: MXWF (Maxwell force flag); MCI (magnetic circuit interface). Electric label: CHRGS (surface charge density); MXWF (Maxwell force flag). Infinite element labels: INF (Exterior surface flag for INFIN110 and INFIN111). High-frequency electromagnetic labels: PORT (number 1 through 6 for a waveguide port); SHLD (surface shielding properties). Note-VALUE and VALUE2 are not used with flag labels. Thermal labels CONV and HFLUX are mutually exclusive. If Lab=FSI, only the fluid elements must be selected for the flag to be applied.

Surface load value or table name reference for specifying tabular boundary conditions. If Lab=CONV, VALUE is typically the film coefficient and VALUE2 (below) is typically the bulk temperature. If Lab=CONV and VALUE=-N, the film coefficient may be a function of temperature and is determined from the HF property table for material N [MP]. The temperature used to evaluate the film coefficient is usually the average between the bulk and wall temperatures, but may be user-defined for some elements. To specify a table, enclose the table name in percent signs (%) (e.g., SF,NLIST,Lab,%tabnam%). Use the *DIM command to define a table. If Lab = MCI, VALUE indicates current direction (-1; current flow into the element face (IN), +1; current flow out of the element face (OUT). If Lab=RAD, VALUE is surface emissivity. If Lab = PORT, VALUE is a port number representing a waveguide port. The port number must be an integer between 1 and 6. If Lab=SHLD, VALUE1 is surface conductivity.

Second surface load value (if any). If Lab=CONV, VALUE2 is typically the bulk temperature. If Lab=RAD, VALUE2 is the ambient temperature. VALUE2 is not used for PORT. If Lab=SHLD, VALUE2 is relative permeability and defaults to 1.0. To specify a table (Lab=CONV), enclose the table name in percent signs (%) (e.g., SF,NLIST,Lab,VALUE,%tabnam%). Use the *DIM command to define a table.

Individual nodes may not be entered for this command. The node list is to identify a surface and the NLIST field must contain a sufficient number of nodes to define an element surface. The loads are internally stored on element faces defined by the specified nodes. All nodes on an element face must be specified for the face to be used, and the element must be selected. The SF command applies only to area and volume elements. For shell elements, if the specified nodes include face one (which is usually the bottom face) along with other faces (such as edges), only face one is used. If all nodes defining a face are shared by an adjacent face of another selected element, the face is not free and will not have a load applied. Where faces cannot be uniquely determined from the nodes, or where the face does not fully describe the load application, use the SFE command. A load key of 1 (which is typically the first loading condition on the first face) is used if the face determination is not unique. A uniform load value is applied over the element face.

See the SFBEAM command for applying surface loads to beam elements. See the SFGRAD command for an alternate tapered load capability. See the SFFUN command for applying loads from a node vs. value function. Also see the SFE command for applying tapered loads on individual element faces. Use the SFDELE command to delete loads applied with this command. Use the SFCUM command to accumulate (add) surface loads applied with SF.

Tabular boundary conditions (VALUE=%tabnam%) available only for structural and thermal surface load labels (Lab=PRES, CONV (film coefficient and/or bulk temperature) or HFLUX).

This command is also valid in PREP7.

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

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

Main Menu >Preprocessor >Loads >Apply >Fluid-Struct >On Nodes

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

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

Main Menu >Preprocessor >Loads >Apply >Rad Matrix >On Nodes

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

Main Menu >Solution >Apply >Excitation >On Nodes

Main Menu >Solution >Apply >Flag >On Nodes

Main Menu >Solution >Apply >Fluid-Struct >On Nodes

Main Menu >Solution >Apply >Impedance >On Nodes

Main Menu >Solution >Apply >Other >On Nodes

Main Menu >Solution >Apply >Rad Matrix >On Nodes

Main Menu >Solution >Apply >Radiation >On Nodes

Specifies surface loads on the selected areas.

SOLUTION:SolidSurfaceLoads

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

Area to which surface load applies. If ALL, apply load to all selected areas [ASEL]. If AREA = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component may be substituted for AREA.

Load key associated with surface load (defaults to 1). Load keys (1,2,3,etc.) are listed under "Surface Loads" in the input data table for each element type in the ANSYS Elements Reference. LKEY is ignored if the area is the face of a volume region meshed with volume elements.

Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each area type in the ANSYS Elements Reference. Structural label: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux); RAD (radiation). Fluid labels: FSI (fluid-structure interaction flag); IMPD (impedance). Magnetic label: MXWF (Maxwell force flag); MCI (magnetic circuit interface). Electric labels: MXWF (Maxwell force flag), CHRGS (surface charge density). Infinite element label: INF (Exterior surface flag for INFIN110 and INFIN111). High-frequency electromagnetic labels: PORT (number 1 through n for a waveguide port); SHLD (surface shielding properties). Note: VALUE and VALUE2 not used with flag labels. Thermal labels CONV and HFLUX are mutually exclusive. If Lab=FSI, only the fluid elements must be selected for the flag to be applied.

Surface load value or table name reference for specifying tabular boundary conditions. If Lab=CONV, VALUE is typically the film coefficient and VALUE2 (below) is typically the bulk temperature. If Lab=CONV and VALUE=-N, the film coefficient may be a function of temperature and is determined from the HF property table for material N [MP]. The temperature used to evaluate the film coefficient is usually the average between the bulk and wall temperatures, but may be user-defined for some elements. To specify a table, enclose the table name in percent signs (%) (e.g., SF,NLIST,Lab,%tabnam%). Use the *DIM command to define a table. If Lab = MCI, VALUE indicates current direction (-1; current flow into the element face (IN), +1; current flow out of the element face (OUT). If Lab=RAD, VALUE is the surface emissivity. If Lab=PORT, VALUE is a port number representing a waveguide port. The port number must be an integer between 1 and 6. If Lab=SHLD, VALUE is surface conductivity.

Second surface load value (if any). If Lab=CONV, VALUE2 is typically the bulk temperature. If Lab=RAD, VALUE2 is ambient temperature. VALUE2 is not used for other surface load labels. VALUE2 is not used for PORT. If Lab=SHLD, VALUE2 is relative permeability (defaults to 1.0). To specify a table (Lab=CONV), enclose the table name in percent signs (%) (e.g., SFA,NLIST,Lab,VALUE,%tabnam%). Use the *DIM command to define a table.

Surface loads may be transferred from areas to elements with the SFTRAN or SBCTRAN commands. See the SFGRAD command for an alternate tapered load capability.

Tabular boundary conditions (VALUE=%tabnam%) available only for structural and thermal surface load labels (Lab=PRES, CONV (film coefficient and/or bulk temperature) or HFLUX).

This command is also valid in PREP7.

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

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

Main Menu >Preprocessor >Loads >Apply >Fluid-Struct >On Areas

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

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

Main Menu >Preprocessor >Loads >Apply >Rad Matrix >On Areas

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

Main Menu >Solution >Apply >Excitation >On Areas

Main Menu >Solution >Apply >Flag >On Areas

Main Menu >Solution >Apply >Fluid-Struct >On Areas

Main Menu >Solution >Apply >Impedance >On Areas

Main Menu >Solution >Apply >Other >On Areas

Main Menu >Solution >Apply >Rad Matrix >On Areas

Main Menu >Solution >Apply >Radiation >On Areas

Allows safety factor or margin of safety calculations to be made.

POST1:ElementTable

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

Type of calculation:

0 - No nodal safety factor or margin of safety calculations.

1 - Calculate and store safety factors in place of nodal stresses.

2 - Calculate and store margins of safety in place of nodal stresses.

Notes

Allows safety factor (SF) or margin of safety (MS) calculations to be made for the average nodal stresses according to:

MS = (SALLOW/|Stress|) - 1.0.

Calculations are done during the display, select, or sort operation (in the active coordinate system [RSYS]) with results stored in place of the nodal stresses. Use the PRNSOL or PLNSOL command to display the results. Note that the results are meaningful only for the stress (SIG1, SIGE, etc.) upon which SALLOW is based. Nodal temperatures used are those automatically stored for the node. Related commands are SFCALC, SALLOW, TALLOW.

Main Menu >General Postproc >Safety Factor >Restore NodeStrs

Main Menu >General Postproc >Safety Factor >SF for Node Strs

Deletes surface loads from areas.

SOLUTION:SolidSurfaceLoads

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

Area to which surface load deletion applies. If ALL, delete load from all selected areas [ASEL]. If AREA = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for AREA.

Load key associated with surface load (defaults to 1). See the SFA command for details.

Valid surface load label. If ALL, use all appropriate labels. See the SFA command for labels.

Deletes surface loads (and all corresponding finite element loads) from selected areas.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Delete >Convection >On Areas

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

Main Menu >Preprocessor >Loads >Delete >Flag >On Areas

Main Menu >Preprocessor >Loads >Delete >Fluid-Struct >On Areas

Main Menu >Preprocessor >Loads >Delete >Heat Flux >On Areas

Main Menu >Preprocessor >Loads >Delete >Impedance >On Areas

Main Menu >Preprocessor >Loads >Delete >Other >On Areas

Main Menu >Preprocessor >Loads >Delete >Pressure >On Areas

Main Menu >Preprocessor >Loads >Delete >Rad Matrix >On Areas

Main Menu >Preprocessor >Loads >Delete >Radiation >On Areas

Main Menu >Preprocessor >Loads >Delete >All Load Data >On All Areas

Main Menu >Solution >Delete >Convection >On Areas

Main Menu >Solution >Delete >Excitation >On Areas

Main Menu >Solution >Delete >Flag >On Areas

Main Menu >Solution >Delete >Fluid-Struct >On Areas

Main Menu >Solution >Delete >Heat Flux >On Areas

Main Menu >Solution >Delete >Impedance >On Areas

Main Menu >Solution >Delete >Other >On Areas

Main Menu >Solution >Delete >Pressure >On Areas

Main Menu >Solution >Delete >Rad Matrix >On Areas

Main Menu >Solution >Delete >Radiation >On Areas

Main Menu >Solution >Delete >All Load Data >On All Areas

Lists the surface loads for the specified area.

SOLUTION:SolidSurfaceLoads

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

Area at which surface load is to be listed. If ALL (or blank), list for all selected areas [ASEL]. If AREA = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for AREA.

Valid surface load label. If ALL (or blank), use all appropriate labels. See the SFA command for labels.

This command is valid in any processor.

Utility Menu >List >Loads >Surface Loads >On All Areas

Utility Menu >List >Loads >Surface Loads >On Picked Areas

Specifies surface loads on beam elements.

SOLUTION:FESurfaceLoads

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

Element to which surface load is applied. If ALL, apply load to all selected beam elements [ESEL]. 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 in ELEM.

Load key associated with surface load (defaults to 1). Load keys (1,2,3,etc.) are listed under "Surface Loads" in the input table for each element type in the ANSYS Elements Reference. For beam elements, the load key defines the load orientation.

Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each element type in the ANSYS Elements Reference. Structural labels: PRES (pressure).

Surface load values or table name reference for specifying tabular boundary conditions at nodes I and J. If VALJ is blank, it defaults to VALI. If VALJ is zero, a zero is used. To specify a table, enclose the table name in percent signs (%) (e.g., SFBEAM,ELEM,LKEY,Lab,%tabnam%). Use the *DIM command to define a table.

Second surface load values at nodes I and J. Currently not used.

Offset distance from node I (toward node J) where VALI is applied.

Offset distance from node J (toward node I) where VALJ is applied. Offsets are available only for lateral surfaces of line elements having a KEYOPT(10) which is set. If no offsets are specified, the load is applied over the full element length. Values may also be input as length fractions, depending on the KEYOPT(10) setting. For example, for a line length of 5.0, an IOFFST distance of 2.0 or an IOFFST fraction of 0.4 represent the same point. If JOFFST=-1, VALI is assumed to be a point load at the location specified with IOFFST and VALJ is ignored.

Specifies surface loads on the selected beam elements. Use the SFELIST and SFEDELE commands to list and delete surface loads applied with this command.

Use the SFCUM command to accumulate (add) surface loads applied with SFBEAM. When SFBEAM follows SFCUM,ADD, the same IOFFST and JOFFST values must be used as on the previous SFBEAM command (for a given element face). Otherwise, the loads will not be accumulated. Leaving IOFFST and JOFFST blank will cause the previous offset values to be used (only when SFBEAM follows SFCUM).

Tabular boundary conditions (VALI, VALJ=%tabnam%) available only for structural surface load labels (Lab=PRES).

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Apply >Pressure >On Beams

Main Menu >Solution >Apply >Pressure >On Beams

Calculates the safety factor or margin of safety.

POST1:ElementTable

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

Label assigned to results. If same as existing label, the existing values will be overwritten by these results.

Labeled result item corresponding to the element stress.

Labeled result item corresponding to the element temperature.

Type of calculation:

0 or 1 - Use safety factor (SF) calculation.

2 - Use margin of safety (MS) calculation.

3 - Use 1/SF calculation.

Calculates safety factor (SF) or margin of safety (MS) as described for the SFACT command for any labeled result item (see ETABLE command) for the selected elements. Use the PRETAB or PLETAB command to display results. Allowable element stress is determined from the SALLOW-TALLOW table [SALLOW, TALLOW].

Main Menu >General Postproc >Safety Factor >SF for ElemTable

Specifies that surface loads are to be accumulated.

SOLUTION:FESurfaceLoads

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

Valid surface load label. If ALL, use all appropriate labels. Structural label: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux). Substructure label: SELV (Load vector number). Electric labels: CHRGS (surface charge density), MXWF (Maxwell force flag). Magnetic label: MXWF (Maxwell force flag). Infinite element: INF (Exterior surface flag for INF110 and INF111). Thermal labels CONV and HFLUX are mutually exclusive.

Accumulation key:

REPL - Subsequent values replace the previous values (default).

ADD - Subsequent values are added to the previous values.

IGNO - Subsequent values are ignored.

Scale factor for the first surface load value (defaults to 1.0).

Scale factor for the second surface load value (defaults to 1.0).

Notes

Allows repeated surface loads (pressure, convection, etc.) to be replaced, added, or ignored. Surface loads are applied with the SF, SFE, and SFBEAM commands. Issue the SFELIST command to list the surface loads. The operations occur when the next surface load specifications are defined. For example, issuing the SF command with a pressure value of 25 after a previous SF command with a pressure value of 20 causes the current value of that pressure to be 45 with the add operation, 25 with the replace operation, or 20 with the ignore operation. All new pressures applied with SF after the ignore operation will be ignored, even if no current pressure exists on that surface.

Scale factors are also available to multiply the next value before the add or replace operation. A scale factor of 2.0 with the previous "add" example results in a pressure of 70. Scale factors are applied even if no previous values exist. Issue SFCUM,STAT to show the current label, operation, and scale factors. Solid model boundary conditions are not affected by this command, but boundary conditions on the FE model are affected. (Note that FE boundary conditions may still be overwritten by existing solid model boundary conditions if a subsequent boundary condition transfer occurs.)

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Settings >Surface Loads

Main Menu >Solution >Settings >Surface Loads

Deletes surface loads.

SOLUTION:FESurfaceLoads

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

Label defining where to find the list of nodes:

ALL - Use all selected nodes [NSEL]. If=P use graphical picking in GUI. A component label may be substituted for Nlist.

Valid surface load label. If ALL, use all appropriate labels. Structural label: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux); RAD (radiation). Fluid labels: FSI (fluid-structure interaction flag); IMPD (Impedance). Magnetic label: MXWF (Maxwell force flag). Electric labels: CHRGS (Surface Charge Density); MXWF (Maxwell force flag); MCI (magnetic circuit interface). Infinite element label: INF (Exterior surface flag for INFIN110 and INFIN111). Substructure label: SELV (Load vector number). Fluid labels: FSI (Fluid-structure interaction flag); IMPD (Impedance). High-frequency electromagnetic labels: PORT (waveguide port number); SHLD (surface shielding properties. Thermal labels CONV and HFLUX are mutually exclusive. If Lab=FSI, only the fluid elements must be selected for the flag to be applied.

Deletes surface loads as applied with the SF command. Loads are deleted only for the specified nodes on external faces of selected area and volume elements. For shell elements, if the specified nodes include face one (which is usually the bottom face) along with other faces (such as edges), only the loads on face one will be deleted. The element faces are determined from the list of selected nodes as described for the SF command. See the SFEDELE command for deleting loads explicitly by element faces.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Delete >Convection >On Nodes

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

Main Menu >Preprocessor >Loads >Delete >Flag >On Nodes

Main Menu >Preprocessor >Loads >Delete >Fluid-Struct >On Nodes

Main Menu >Preprocessor >Loads >Delete >Heat Flux >On Nodes

Main Menu >Preprocessor >Loads >Delete >Impedance >On Nodes

Main Menu >Preprocessor >Loads >Delete >Other >On Nodes

Main Menu >Preprocessor >Loads >Delete >Pressure >On Nodes

Main Menu >Preprocessor >Loads >Delete >Rad Matrix >On Nodes

Main Menu >Preprocessor >Loads >Delete >Radiation >On Nodes

Main Menu >Solution >Delete >Convection >On Nodes

Main Menu >Solution >Delete >Excitation >On Nodes

Main Menu >Solution >Delete >Flag >On Nodes

Main Menu >Solution >Delete >Fluid-Struct >On Nodes

Main Menu >Solution >Delete >Heat Flux >On Nodes

Main Menu >Solution >Delete >Impedance >On Nodes

Main Menu >Solution >Delete >Other >On Nodes

Main Menu >Solution >Delete >Pressure >On Nodes

Main Menu >Solution >Delete >Rad Matrix >On Nodes

Main Menu >Solution >Delete >Radiation >On Nodes

Specifies surface loads on elements.

SOLUTION:FESurfaceLoads

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

Element to which surface load applies. If ALL, apply load to all selected elements [ESEL]. 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.

Load key associated with surface load (defaults to 1). Load keys (1,2,3,etc.) are listed under "Surface Loads" in the input data table for each element type in the ANSYS Elements Reference.

Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each element type in the ANSYS Elements Reference. Structural labels: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux); RAD (radiation). Fluid labels: FSI (fluid-structure interaction flag); IMPD (impedance). Magnetic labels: MXWF (Maxwell force flag). Infinite element labels: INF (Exterior surface flag for INFIN110 and INFIN111). Substructure label: SELV (load vector number). Electric labels: CHRGS (Surface Charge density); MXWF (Maxwell force flag). High-frequency electromagnetic labels: PORT (waveguide port number); SHLD (surface shielding properties). Note: VAL1 through VAL4 not used with flag labels. Thermal labels CONV and HFLUX are mutually exclusive. If Lab=FSI, only the fluid elements must be selected for the flag to be applied.

Value key. Used only if Lab=CONV or if Lab=RAD or if Lab = SHLD:

0 or 1 - If Lab=RAD, VAL1 through VAL4 are used as the emissivities. If Lab=CONV, VAL1 through VAL4 are used as the film coefficients. If Lab=SHLD, VAL1 through VAL4 are used as the electrical conductivities.

2 - If Lab=RAD, VAL1 through VAL4 are ambient temperatures. If Lab=CONV, VAL1 through VAL4 are the bulk temperatures. If Lab=SHLD, VAL1 through VAL4 are used as the relative permeabilities.

If only one set of data is supplied (either emissivities or temperatures when Lab=RAD; or either film coefficients or temperatures when Lab=CONV; or either conductivity or relative permeability when Lab=SHLD), the other set of data defaults to previously specified values (or zero if not previously specified).

First surface load value (typically at the first node of the face) or the name of a table for specifying tabular boundary conditions.. Face nodes are listed in the order given for "Surface Loads" in the input data table for each element type in the ANSYS Elements Reference. For example, for SOLID45, the item 1-JILK associates LKEY=1 (face 1) with nodes J,I,L, and K. Surface load value VAL1 then applies to node J of face 1. To specify a table, enclose the table name in percent signs (%), e.g., %tabname%. Use the *DIM command to define a table. VAL2 applies to node I, etc. If Lab=CONV, KVAL=0, and VAL1=-N, the film coefficient is assumed to be a function of temperature and is determined from the HF property table for material N [MP]. The temperature used to evaluate the film coefficient is usually the average between the bulk and wall temperatures, but may be user defined for some elements. If Lab=PORT, VAL1 is a port number representing a waveguide port. The port number must be an integer between 1 and 6.

Surface load value at the 2nd, 3rd, and 4th nodes (if any) of the face. Blank values default to VAL1 (for a constant load). Zero values are used as zero. To specify a table (Lab=CONV), enclose the table name in percent signs (%), e.g., %tabname%. Use the *DIM command to define a table.

Specifies surface loads on selected elements. Caution: You cannot use the SFE command with the INFIN110 or INFIN111 elements without prior knowledge of element face orientation, i.e., you must know which face is the exterior in order to flag it. Also, the surface effect elements, SURF19 and SURF22, require special usage of this command when applying pressures (see Section 4.19 and Section 4.22 of the ANSYS Elements Reference).

Tapered loads may be applied over the faces of most elements. For beam elements allowing lateral surface loads that may be offset from the nodes, use the SFBEAM command to specify the loads and offsets. See the SF command for an alternate surface load definition capability based upon node numbers. See the SFGRAD command for an alternate tapered load capability. Use the SFCUM command to accumulate (add) surface loads applied with SFE.

You can specify a table name only when using structural (PRES) and thermal (CONV (film coefficient and/or bulk temperature), HFLUX) surface load labels.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Apply >Convection >Tapered

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

Main Menu >Preprocessor >Loads >Apply >Impedance >On Elements

Main Menu >Preprocessor >Loads >Apply >Rad Matrix >On Elements

Main Menu >Preprocessor >Loads >Apply >Radiation >On Elements

Main Menu >Preprocessor >Loads >Apply >Load Vector >For Superelement

Main Menu >Solution >Apply >Convection >Tapered

Main Menu >Solution >Apply >Excitation >On Elements

Main Menu >Solution >Apply >Impedance >On Elements

Main Menu >Solution >Apply >Rad Matrix >On Elements

Main Menu >Solution >Apply >Radiation >On Elements

Main Menu >Solution >Apply >Load Vector >For Superelement

Deletes surface loads from elements.

SOLUTION:FESurfaceLoads

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

Element to which surface load deletion applies. If ALL, delete load from all selected elements [ESEL]. 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.

Load key associated with surface load (defaults to 1). If ALL, delete surface loads for all load keys.

Valid surface load label. If ALL, use all appropriate labels. Structural labels: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux); RAD (radiation). Fluid labels: FSI (fluid-structure interaction flag); IMPD (impedance). Magnetic label: MXWF (Maxwell force flag). Infinite element label: INF (Exterior surface flag for INFIN110 and INFIN111). Substructure label: SELV (Load vector number); Electric label: CHRGS (surface charge density); MXWF (Maxwell force flag). High-frequency electromagnetic labels: PORT (waveguide port number); SHLD (surface shielding properties). If Lab=FSI, only the fluid elements must be selected for the flag to be applied.

Deletes surface loads from selected elements. See the SFDELE command for an alternate surface load deletion capability based upon selected nodes.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Delete >Convection >On Elements

Main Menu >Preprocessor >Loads >Delete >Excitation >On Elements

Main Menu >Preprocessor >Loads >Delete >Flag >On Elements

Main Menu >Preprocessor >Loads >Delete >Heat Flux >On Elements

Main Menu >Preprocessor >Loads >Delete >Impedance >On Elements

Main Menu >Preprocessor >Loads >Delete >Other >On Elements

Main Menu >Preprocessor >Loads >Delete >Pressure >On Elements

Main Menu >Preprocessor >Loads >Delete >Rad Matrix >On Elements

Main Menu >Preprocessor >Loads >Delete >Radiation >On Elements

Main Menu >Preprocessor >Loads >Delete >All Load Data >On All Elems

Main Menu >Preprocessor >Loads >Delete >Load Vector >For Superelement

Main Menu >Solution >Delete >Convection >On Elements

Main Menu >Solution >Delete >Excitation >On Elements

Main Menu >Solution >Delete >Flag >On Elements

Main Menu >Solution >Delete >Heat Flux >On Elements

Main Menu >Solution >Delete >Impedance >On Elements

Main Menu >Solution >Delete >Other >On Elements

Main Menu >Solution >Delete >Pressure >On Elements

Main Menu >Solution >Delete >Rad Matrix >On Elements

Main Menu >Solution >Delete >Radiation >On Elements

Main Menu >Solution >Delete >All Load Data >On All Elems

Main Menu >Solution >Delete >Load Vector >For Superelement

Lists the surface loads for elements.

SOLUTION:FESurfaceLoads

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

Element at which surface load is to be listed. If ALL (or blank), list loads for all selected elements [ESEL]. 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.

Valid surface load label. If ALL (or blank), use all appropriate labels. Structural label: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux); RAD (radiation). Fluid labels: FSI (fluid-structure interaction flag); IMPD (impedance). Magnetic label: MXWF (Maxwell force flag). Substructure label: SELV (Load vector number). Electric labels: CHRGS (surface charge density); MXWF (Maxwell force flag). Infinite element label: INF (Exterior surface flag for INFIN110 and INFIN111). High-frequency electromagnetic labels: PORT (waveguide port number); SHLD (surface shielding properties). Thermal labels CONV and HFLUX are mutually exclusive. If Lab=SFI, only the fluid elements must be selected for the flag to be applied.

This command is valid in any processor.

Utility Menu >List >Loads >Surface Loads >On All Elements

Utility Menu >List >Loads >Surface Loads >On Picked Elems

Specifies a varying surface load.

SOLUTION:FESurfaceLoads

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

Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each element type in the ANSYS Elements Reference. Structural label: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux). Electric labels: CHRGS (Surface Charge density). Issue SFFUN,STATUS to list current command settings. Thermal labels CONV and HFLUX are mutually exclusive.

Parameter containing list of surface load values. If Lab=CONV, values are typically the film coefficients and Par2 values (below) are typically the bulk temperatures.

Parameter containing list of second surface load values (if any). If Lab=CONV, the Par2 values are typically the bulk temperatures. Par2 is not used for other surface load labels.

Specifies a surface load "function" to be used when the SF or SFE command is issued. The function is supplied through an array parameter vector which contains nodal surface load values. Node numbers are implied from the sequential location in the array parameter. For example, a value in location 11 applies to node 11. The element faces are determined from the implied list of nodes when the SF or SFE command is issued. Zero values should be supplied for nodes that have no load. A tapered load value may be applied over the element face. These loads are in addition to any loads that are also specified with the SF or SFE commands. Issue SFFUN (with blank remaining fields) to remove this specification. Issue SFFUN,STATUS to list current settings.

Starting array element numbers must be defined for each array parameter vector. For example, SFFUN,CONV,A(1,1),A(1,2) reads the first and second columns of array A (starting with the first array element of each column) and associates the values with the nodes. Operations continue on successive column array elements until the end of the column.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Settings >Node Function

Main Menu >Solution >Settings >Node Function

Specifies a gradient (slope) for surface loads.

SOLUTION:FESurfaceLoads

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

Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each element type in the ANSYS Elements Reference. Structural labels: PRES (pressure). Thermal labels: CONV (convection (bulk temperatures only)); HFLUX (heat flux). Electric labels: CHRGS (surface charge density). Thermal labels CONV and HFLUX are mutually exclusive.

Reference number of slope coordinate system (used with Sldir and SLZER to determine COORD). Defaults to 0 (the global Cartesian coordinate system).

Slope direction in coordinate system SLKCN:

X - Slope is along X direction (default). Interpreted as R direction for non-Cartesian coordinate systems.

Y - Slope is along Y direction. direction for non-Cartesian coordinate systems.

Z - Slope is along Z direction. direction for spherical or toroidal coordinate systems.

Coordinate location (degrees for angular input) where slope contribution is zero (CVALUE = VALUE). Allows the slope contribution to be shifted along the slope direction. For angular input, SLZER should be between 180° if the singularity [CSCIR] is at 180° and should be between 0° and 360° if the singularity is at 0°.

Slope value (load per unit length or per degree).

Specifies a gradient (slope) for surface loads. All surface loads issued with the SF, SFE, SFL, or SFA commands while this specification is active will have this gradient applied (for convections, only the bulk temperature will be affected). The load value, CVALUE, calculated at each node is:

where VALUE is the load value specified on the subsequent SF, SFE, SFL, or SFA commands and COORD is the coordinate value (in the Sldir direction of coordinate system SLKCN) of the node. Only one SFGRAD specification may be active at a time (repeated use of this command replaces the previous specification with the new specification). Issue SFGRAD (with blank fields) to remove the specification. Issue SFGRAD,STAT to show the current command status. The SFGRAD specification (if active) is removed when the LSREAD (if any) command is issued.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Settings >Gradient

Main Menu >Solution >Settings >Gradient

Specifies surface loads on lines of an area.

SOLUTION:SolidSurfaceLoads

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

Line to which surface load applies. If ALL, apply load to all selected lines [LSEL]. If LINE = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for LINE.

Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each element type in the ANSYS Elements Reference. Structural label: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux); RAD (radiation). Fluid labels: FSI (fluid-structure interaction flag); IMPD (impedance). Magnetic label: MXWF (Maxwell force flag). Electric labels: MXWF (electrostatic force flag), CHRGS (surface charge density). Infinite element label: INF (Exterior surface flag for INFIN110 and INFIN111). Note: VALI through VAL2J not used with flag labels. Thermal labels CONV and HFLUX are mutually exclusive. If Lab=FSI, only the fluid elements must be selected for the flag to be applied.

Surface load values at the first keypoint (VALI) and at the second keypoint (VALJ) of the line, or table name for specifying tabular boundary conditions. If VALJ is blank, it defaults to VALI. If VALJ is zero, a zero is used. If Lab=CONV, VALI and VALJ are the film coefficients and VAL2I and VAL2J are the bulk temperatures. To specify a table, enclose the table name in percent signs (%), e.g., %tabname%. Use the *DIM command to define a table. If Lab=CONV and VALI=-N, the film coefficient may be a function of temperature and is determined from the HF property table for material N [MP]. If Lab=RAD, VALI and VALJ values are surface emissivities. and VAL2I and VAL2J are ambient temperatures. The temperature used to evaluate the film coefficient is usually the average between the bulk and wall temperatures, but may be user defined for some elements.

Second surface load values (if any). If Lab=CONV, VAL2I and VAL2J are the bulk temperatures. If Lab=RAD, VAL2I and VAL2J are the ambient temperatures. VAL2I and VAL2J are not used for other surface load labels. If VAL2J is blank, it defaults to VAL2I. If VAL2J is zero, a zero is used. To specify a table (Lab=CONV), enclose the table name in percent signs (%), e.g., %tabname%. Use the *DIM command to define a table.

Specifies surface loads on the selected lines of area regions. The lines represent either the edges of area elements or axisymmetric shell elements themselves. Surface loads may be transferred from lines to elements with the SFTRAN or SBCTRAN commands. See the SFE command for a description of surface loads. Loads input on this command may be tapered. See the SFGRAD command for an alternate tapered load capability.

You can specify a table name only when using structural (PRES) and thermal (CONV (film coefficient and/or bulk temperature), HFLUX) surface load labels. VALJ and VAL2J are ignored for tabular boundary conditions.

This command is also valid in PREP7.

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

Main Menu >Preprocessor >Loads >Apply >Flag >On Lines

Main Menu >Preprocessor >Loads >Apply >Fluid-Struct >On Lines

Main Menu >Preprocessor >Loads >Apply >Impedance >On Lines

Main Menu >Preprocessor >Loads >Apply >Other >On Lines

Main Menu >Preprocessor >Loads >Apply >Rad Matrix >On Lines

Main Menu >Preprocessor >Loads >Apply >Radiation >On Lines

Main Menu >Solution >Apply >Excitation >On Lines

Main Menu >Solution >Apply >Flag >On Lines

Main Menu >Solution >Apply >Fluid-Struct >On Lines

Main Menu >Solution >Apply >Impedance >On Lines

Main Menu >Solution >Apply >Other >On Lines

Main Menu >Solution >Apply >Rad Matrix >On Lines

Main Menu >Solution >Apply >Radiation >On Lines

Deletes surface loads from lines.

SOLUTION:SolidSurfaceLoads

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

Line to which surface load deletion applies. If ALL, delete load from all selected lines [LSEL]. If LINE = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for LINE.

Valid surface load label. If ALL, use all appropriate labels. See the SFL command for labels.

Deletes surface loads (and all corresponding finite element loads) from selected lines.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Delete >Convection >On Lines

Main Menu >Preprocessor >Loads >Delete >Excitation >On Lines

Main Menu >Preprocessor >Loads >Delete >Flag >On Lines

Main Menu >Preprocessor >Loads >Delete >Fluid-Struct >On Lines

Main Menu >Preprocessor >Loads >Delete >Heat Flux >On Lines

Main Menu >Preprocessor >Loads >Delete >Impedance >On Lines

Main Menu >Preprocessor >Loads >Delete >Other >On Lines

Main Menu >Preprocessor >Loads >Delete >Pressure >On Lines

Main Menu >Preprocessor >Loads >Delete >Rad Matrix >On Lines

Main Menu >Preprocessor >Loads >Delete >Radiation >On Lines

Main Menu >Preprocessor >Loads >Delete >All Load Data >On All Lines

Main Menu >Solution >Delete >Convection >On Lines

Main Menu >Solution >Delete >Excitation >On Lines

Main Menu >Solution >Delete >Flag >On Lines

Main Menu >Solution >Delete >Fluid-Struct >On Lines

Main Menu >Solution >Delete >Heat Flux >On Lines

Main Menu >Solution >Delete >Impedance >On Lines

Main Menu >Solution >Delete >Other >On Lines

Main Menu >Solution >Delete >Pressure >On Lines

Main Menu >Solution >Delete >Rad Matrix >On Lines

Main Menu >Solution >Delete >Radiation >On Lines

Main Menu >Solution >Delete >All Load Data >On All Lines

Lists surface loads.

SOLUTION:FESurfaceLoads

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

Node at which surface load is to be listed. If ALL (or blank), list for all selected nodes [NSEL]. If NODE = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for NODE.

Valid surface load label. If ALL (or blank), use all appropriate labels. Structural labels: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux); RAD (radiation). Fluid labels: FSI (fluid-structure interaction flag); IMPD (impedance). Magnetic labels: MXWF (Maxwell force flag); MCI (magnetic circuit interface). Electric label: CHRGS (surface charge density); MXWF (Maxwell force flag). High-frequency electromagnetic labels: PORT (waveguide port number); SHLD (surface shielding properties). Infinite element label: INF (exterior surface flag for INFIN110 and INFIN111). If Lab=FSI, only the fluid elements must be selected for the flag to be applied.

Lists the surface loads as applied with the SF command. Loads are listed only for the specified nodes on external faces of selected area and volume elements. Use SFELIST for line elements.

This command is valid in any processor.

Utility Menu >List >Loads >Surface Loads >On All Nodes

Utility Menu >List >Loads >Surface Loads >On Picked Nodes

Lists the surface loads for lines.

SOLUTION:SolidSurfaceLoads

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

Line at which surface load is to be listed. If ALL (or blank), list for all selected lines [LSEL]. If LINE = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for LINE.

Valid surface load label. If ALL (or blank), use all appropriate labels. See the SFL command for labels.

Lists the surface loads for the specified line.

This command is valid in any processor.

Utility Menu >List >Loads >Surface Loads >On All Lines

Utility Menu >List >Loads >Surface Loads >On Picked Lines

Scales surface loads on elements.

SOLUTION:FESurfaceLoads

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

Valid surface load label. If ALL, use all appropriate labels. Structural label: PRES (pressure). Thermal labels: CONV (convection); HFLUX (heat flux). Substructure label: SELV (Load vector number). Electric labels: CHRGS (surface charge density). Thermal labels CONV and HFLUX are mutually exclusive.

Scale factor for the first surface load value. Zero (or blank) defaults to 1.0. Use a small number for a zero scale factor.

Scale factor for the second surface load value. Zero (or blank) defaults to 1.0. Use a small number for a zero scale factor.

Scales surface loads (pressure, convection, etc.) in the database on the selected elements. Surface loads are applied with the SF, SFE, or SFBEAM commands. Issue the SFELIST command to list the surface loads. Solid model boundary conditions are not scaled by this command, but boundary conditions on the FE model are scaled. (Note that such scaled FE boundary conditions may still be overwritten by unscaled solid model boundary conditions if a subsequent boundary condition transfer occurs.)

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Operate >Surface Loads

Main Menu >Solution >Operate >Surface Loads

Transfer the solid model surface loads to the finite element model.

SOLUTION:SolidSurfaceLoads

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

Surface loads are transferred only from selected lines and areas to all selected elements. The SFTRAN operation is also done if the SBCTRAN command is issued or automatically done upon initiation of the solution calculations [SOLVE].

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Operate >Surface Loads

Main Menu >Solution >Operate >Surface Loads

Defines the type of surface shading used with Z-buffering.

GRAPHICS:Style

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Shading type:

FACET or 0 - Facet shading (one color per area face) (default).

GOURAUD or 1 - Gouraud smooth shading (smooth variation of color based on interpolated vertex colors).

PHONG or 2 - Phong smooth shading (smooth variation of color based on interpolated vertex normals).

Notes

Defines the type of surface shading used on area, volume, and PowerGraphics [/GRAPHICS,POWER] displays when software Z-buffering is enabled [/TYPE]. This command is only functional for 2-D display devices.

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Hidden-Line Options

Selects a shell element or shell layer location for results output.

POST1:Controls POST26:Controls

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

Location within shell element (or layer) to obtain stress results:

TOP - Top of shell element (or layer) (default).

MID - Middle of shell element (or layer). Calculated from the average of TOP and BOT.

BOT - Bottom of shell element (or layer).

Notes

Selects the location within a shell element (or a shell layer) for results output (nodal stresses, strains, etc.). Applies to POST1 selects, sorts, and output [NSEL, NSORT, PRNSOL, PLNSOL, PRPATH, PLPATH, etc.], and is used for storage with the POST26 ESOL command. For example, SHELL,TOP causes item S of the POST1 PRNSOL command or the POST26 ESOL command to be the stresses at the top of the shell elements. For layered shell elements, use the LAYER (POST1) or LAYERP26 (POST26) command to select the layer. For PowerGraphics [/GRAPHICS,POWER], the SHELL command affects only printed output. The SHELL command is not applicable to PowerGraphics displays because with PowerGraphics, shell element results are displayed at both the top and bottom layers simultaneously.

Main Menu >General Postproc >Options for Outp

Main Menu >TimeHist Postpro >Define Variables

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

Utility Menu >List >Results >Options

Specifies the device and other parameters for graphics displays.

GRAPHICS:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Device name, filename, or keyword, as listed below:

<devicename> - Any valid graphics display device name (e.g., X11, 3D, etc.). Defaults to X11 for most systems. See Chapter 8 of the ANSYS Basic Analysis Procedures Guide for details. A device name must be defined before activating the Graphical User Interface (GUI). Once the GUI is activated, the device name cannot be changed for that ANSYS session, except for switching between X11 and X11C.

<filename> - Name of graphics file to which graphics displays are to be diverted (32 characters maximum). Should not be the same as a valid device name or any other Fname option.

TERM - Graphics displays are switched back to the last-specified device name.

FILE - Graphics displays are switched back to the last-specified file name.

OFF - Graphics display requests are ignored.

<blank> - If blank in interactive mode, graphics will be displayed on screen as requested by display commands (no file written); If blank in batch mode, graphics data will be written to Jobname.GRPH.

PSCR - Creates PostScript graphic files that are named jobname00.eps. (See the PSCR command for options.) Ignores the Ext and NCPL fields.

HPGL - Creates Hewlett-Packard Graphics Language files that are named jobnamenn.hpgl, where nn is a numeric value that is incremented by one as each additional file is created; that is, jobname00.hpgl, jobname01.hpgl, jobname02.hpgl, and so on. (See the HPGL command for options.) Ignores the Ext and NCPL fields.

HPGL2 - Creates Hewlett-Packard Graphics Language files that are named jobnamenn.hpgl, where nn is a numeric value that is incremented by one as each additional file is created; that is, jobname00.hpgl, jobname01.hpgl, jobname02.hpgl, and so on. The HPGL2 files have enhanced color. (See the HPGL command for options.) Ignores the Ext and NCPL fields.

VRML - Creates Virtual Reality Meta Language files named file00.wrl that can be displayed on 3-D Internet web browsers. Ignores the Ext and NCPL fields.

Filename extension (optional, 8 characters maximum).

Specifies raster or vector display mode. This affects area, volume, and element displays, as well as geometric results displays such as contour plots. See the /DEVICE command for an alternate way to toggle between raster and vector mode. Changing VECT also resets the /TYPE command to its default.

0 - Raster display (color filled entities; default)

1 - Vector display (outlined entities; i.e., "wireframe")

Sets the number of color planes (4 to 8). Default is device-dependent. NCPL is not supported by all graphics devices.

Notes

Specifies the device to be used for graphics displays, and specifies other graphics display parameters. Display may be shown at the time of generation (for interactive runs at a graphics display terminal) or diverted to a file for later processing with the DISPLAY program. Issue /PSTATUS for display status.

This command is valid in any processor.

Utility Menu >PlotCtrls >Device Options

Utility Menu >PlotCtrls >Redirect Plots >To File

Utility Menu >PlotCtrls >Redirect Plots >To Screen

Defines the display driver name.

DISPLAY:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Valid driver name (see Chapter 8 of the ANSYS Basic Analysis Procedures Guide for details):

<devicename> - Any linked terminal driver (such as X11, TEKTRONIX, etc.)

HPGL - Hewlett-Packard Graphics Language

HPGL2 - Hewlett-Packard Graphics Language with enhanced color. (See the HPGL command for options.) Ignores the NCPL field.

INTERLEAF - Interleaf ASCII Format, OPS Version 5.0

POSTSCRIPT - PostScript, Version 1.0 Minimally Conforming

DUMP - ASCII Text Dump

Unused fields.

Number of color planes (4 to 8). Default is device-dependent.

DISPLAY Program

Controls element shape checking.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Shape checking option. (When Lab=WARN, STATUS, SUMMARY, or DEFAULT, the remaining arguments are ignored.)

ON - Activates element shape checking. New elements, regardless of how they are created, are tested against existing warning and error limits. (The existing limits may be the default limits, or previously modified limits.) Elements that violate error limits produce error messages and either (a) cause a meshing failure, or (b) for element creation or storage other than AMESH or VMESH, are not stored. Elements that violate warning limits produce warning messages. If shape checking was previously turned off [SHPP,OFF] and you turn it on, existing elements are marked as untested; use the CHECK command to retest them. With this option, you may also specify a value for VALUE1 to turn individual shape tests on. If you do not specify a value for VALUE1, all shape tests are turned on.

WARN - Activates element shape checking; however, in contrast to SHPP,ON, elements that violate error limits do not cause either a meshing or element storage failure. Instead, they produce warning messages to notify you that error limits have been violated. This option does not alter current shape parameter limits. Since the default shape parameter error limits are set to allow almost any usable element, the elements this option allows, which would otherwise be forbidden, are likely to be very poorly shaped.

OFF - Deactivates element shape checking. This setting does not alter current shape parameter limits. Use of this option is risky, since poorly shaped elements can lead to analysis results that are less accurate than would otherwise be expected for a given mesh density. With this option, you may also specify a value for VALUE1 to turn individual shape tests off. If you do not specify a value for VALUE1, all element shape tests are turned off.

SILENT - Determines whether element shape checking runs in silent mode. In silent mode, ANSYS checks elements without issuing warnings, with the exception of the generic warnings that it issues at solution. With this option, you must also specify a value for VALUE1. (During the execution of certain commands, ANSYS automatically runs element shape checking in silent mode, then internally summarizes the shape test results for all of the new or modified elements. ANSYS does this when it executes any of the following commands: AGEN, AMESH, AREFINE, ARSYM, ATRAN, CDREAD, EBLOCK, EGEN, ENGEN, ENSYM, EREAD, EREFINE, ESYM, ET, FVMESH, KREFINE, LREFINE, NREFINE, TIMP, VEXT, VGEN, VIMP, VMESH, VOFFST, VROTAT, VSWEEP, VSYMM, and VTRAN.)

STATUS - Lists the shape parameter limits currently in effect, along with status information about element shape checking (for example, whether any individual shape tests are off, whether any of the shape parameter limits have been modified, and so on).

SUMMARY - Lists a summary of element shape test results for all selected elements.

DEFAULT - Resets element shape parameter limits to their default values. Also, if any individual tests were turned off, turns them back on. (The SHPP,DEFAULT command may be useful if any parameter limits were previously altered by using the MODIFY option.)

OBJECT - Determines whether element shape test results data is stored in memory. When this option is turned on, an "object" is created for storing test results in memory. When this option is turned off, no object is created and no data is stored; thus, any operation that requires shape parameters for an existing element (such as use of the CHECK command) causes the shape parameters to be recomputed. (Note the distinction between storing the data in memory and storing it in the database; regardless of whether this option is turned on or off, no element shape test results data will be stored in the database. The element shape parameter object is deleted automatically before any solution.) This setting is independent of shape checking status, with one exception-if shape checking is turned off [SHPP,OFF], the object is not created. Keep in mind that recomputing shape parameters is more computationally expensive than retrieving them from the object. With this option, you must also specify a value for the VALUE1 argument; the VALUE2 argument is ignored.

MODIFY - Indicates that you want to respecify a shape parameter limit. With this option, you must also specify values for the VALUE1 and VALUE2 arguments.

Valid for the ON, OFF, SILENT, OBJECT, and MODIFY options only. When Lab=ON or Lab=OFF, use VALUE1 to individually control (that is, turn off or turn on) specific element shape tests. Thus, VALUE1 can be ANGD (SHELL28 corner angle deviation tests), ASPECT (aspect ratio tests), PARAL (deviation from parallelism of opposite edges tests), MAXANG (maximum corner angle tests), JACRAT (Jacobian ratio tests), WARP (warping factor tests), or ALL (all tests). When Lab=SILENT, VALUE1 can be ON (to turn silent mode on) or OFF (to turn silent mode off). When Lab=OBJECT, VALUE1 can be either 1, YES, or ON to turn on storage of element shape test data (the default); or it can be 0, NO, or OFF to turn off storage of element shape test data (delete the data and recompute as necessary). When Lab=MODIFY, VALUE1 is the numeric location (within the shape parameter limit array) of the shape parameter limit to be modified. Locations are identified in the element shape checking status listing [SHPP,STATUS]. For more information, see the examples in the Notes section.

Valid for the MODIFY option only. Specifies the new limit for the shape parameter that is in the location indicated by the VALUE1 argument. See the examples in the Notes section.

Notes

The following examples illustrate how to use the SHPP,MODIFY,VALUE1,VALUE2 command to respecify shape parameter limits. Assume that you issued the SHPP,STATUS command, and you received the output below:

 ASPECT RATIO (EXCEPT FLOTRAN OR EMAG)
    QUAD OR TRIANGLE ELEMENT OR FACE
         WARNING TOLERANCE ( 1) =   20.00000
         ERROR TOLERANCE   ( 2) =  1000000.
 		·
		·
		·
 MAXIMUM CORNER ANGLE IN DEGREES (EXCEPT FLOTRAN OR EMAG)
    TRIANGLE ELEMENT OR FACE
         WARNING TOLERANCE (15) =   165.0000
         ERROR TOLERANCE   (16) =   179.9000

Notice that in the sample output, the warning tolerance for aspect ratios is set to 20. Now assume that you want to "loosen" this shape parameter limit so that it is less restrictive. To allow elements with aspect ratios of up to 500 without causing warning messages, you would issue this command:

SHPP,MODIFY,1,500

Also notice that each shape parameter's numeric location within the shape parameter limit array appears in the sample output within parentheses. For example, the numeric location of the aspect ratio shape parameter (for warning tolerance) is 1, which is why "1" is specified for the VALUE1 argument in the example command above.

Now notice that the sample output indicates that any triangle element with an internal angle that is greater than 179.9 degrees will produce an error message. Suppose that you want to "tighten" this shape parameter limit, so that it is more restrictive. To cause any triangle or tetrahedron with an internal angle greater than 170 degrees to produce an error message, you would issue this command:

SHPP,MODIFY,16,170

Changing any shape parameter limit marks all existing elements as untested; use the CHECK command to retest them.

Since the shape parameter limit array was completely reorganized at ANSYS 5.4, you should revise any input files created prior to 5.4 that contain limit changes so that they reflect the reorganized data structure. (Using the SHPP command to alter shape parameter limits was possible, but not documented, in releases prior to ANSYS 5.4. However, some users were told about this option.)

For more information about element shape checking, see Chapter 7 of the ANSYS Modeling and Meshing Guide.

Main Menu >Preprocessor >Checking Ctrls >Shape Checking

Main Menu >Preprocessor >Checking Ctrls >Toggle Checks

Shrinks elements, lines, areas, and volumes for display clarity.

GRAPHICS:Scaling

	Mp Me St DY LP Th E3 E2 FL PP ED

Shrinkage ratio (input as a decimal (0.0 to 0.5)). Defaults to 0.0 (no shrinkage). Values greater than 0.5 default to 0.1 (10% shrinkage).

Notes

Shrinks the elements, lines, areas, and volumes so that adjacent entities are separated for clarity. This command is not valid with p-elements.

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Size and Shape

Summarizes the section properties for all defined sections in the current session of ANSYS.

PREP7:CrossSections

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

First section ID to be summarized, defaults to first available section in the database.

Last section ID to be summarized, defaults to last available section in the database.

Increment of the section ID, defaults to 1.

Lists only the section integrated properties, such as Area, Iyy, Iyz, and does not list the section nodal coordinates and cell mesh nodal connectivity information.

PRSSOL prints the BEAM188 and BEAM189 section nodal and section integration point results. Stresses and strains are printed at section nodes, and plastic strains and plastic work are printed at section integration points.

Here is sample output from the SLIST,BRIEF command for a rectangle section subtype:

SECTION ID NUMBER:         1
BEAM SECTION TYPE:     Rectangle       
BEAM SECTION NAME IS:             
BEAM SECTION DATA SUMMARY:
 Area                 = 0.40000    
 Iyy                  = 0.13333E-02
 Iyz                  = 0.37947E-18
 Izz                  = 0.13333    
 Warping Constant     = 0.00000E+00
 Torsion Constant     = 0.51195E-02
 Center of Gravity Y  =-0.86736E-17
 Center of Gravity Z  =-0.10842E-17

 Beam Section is offset to CENTROID of cross section

Main Menu >Preprocessor >Sections >List Sections

Displays line loops smaller than a specified size (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

Preference for line loop display. If Prefer = FACTOR, the command displays all line loops whose radius is smaller than the radius of the model (taken between the two most distant keypoints) times VALUE. This is the default preference. If Prefer = RADIUS, the command displays all line loops whose radius is smaller than that specified by VALUE.

Numeric argument for Prefer.

Use this command to locate and display disproportionately small line loops when repairing the geometry of models imported from CAD files. Line loops matching the criteria specified in Prefer and VALUE both display in a different color and include their IDs. This command is available only for models imported through the Default IGES option.

Main Menu >Preprocessor >Simplify >Small Loops

Displays line segments smaller than a specified size (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

Preference for line segment display. If Prefer = FACTOR, the command displays all line segments whose length is smaller than the average length of lines within the model times VALUE. This is the default preference. If Prefer = LENGTH, the command displays all line lengths smaller than that specified by VALUE.

Numeric argument for Prefer.

Use this command to locate and display disproportionately small line segments when repairing the geometry of models imported from CAD files. Line lengths matching the criteria specified in Prefer and VALUE both display in a different color and include their IDs. This command is available only for models imported through the Default IGES option.

Main Menu >Preprocessor >Simplify >Small Lines

Finds the smallest of three variables.

POST26:Operations

	Mp Me St DY LP Th E3 E2 FL 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 numbers of the three variables to be operated on. If only two, leave IC blank. If only one, leave IB blank also.

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

Unused fields.

Scaling factors (positive or negative) applied to the corresponding variables (defaults to 1.0).

Finds the smallest of three variables according to the operation:

Menu Paths

Main Menu >TimeHist Postpro >Math Operations >Find Minimum

Forms an element table item from the maximum of two other items.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to results. If same as existing label, the existing values will be overwritten by these results.

First labeled result item in operation.

Second labeled result item in operation (may be blank).

Scale factor applied to Lab1 (defaults to 1.0).

Scale factor applied to Lab2 (defaults to 1.0).

Forms a labeled result item (see ETABLE command) for the selected elements by comparing two existing labeled result items according to the operation:

where "cmx" means "compare and save maximum." If absolute values are requested [SABS,1], the absolute values of Lab1 and Lab2 are used.

Main Menu >General Postproc >Element Table >Find Maximum

Specifies "Body loads on the solid model" as the subsequent status topic.

SOLUTION: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 >Solution >Body Loads

Specifies "Constraints on the solid model" as the subsequent status topic.

SOLUTION: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 >Solution >DOF Constraints

Specifies "Forces on the solid model" as the subsequent status topic.

SOLUTION: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 >Solution >Forces

Forms an element table item from the minimum of two other items.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to results. If same as existing label, the existing values will be overwritten by these results.

First labeled result item in operation.

Second labeled result item in operation (may be blank).

Scale factor applied to Lab1 (defaults to 1.0).

Scale factor applied to Lab2 (defaults to 1.0).

Forms a labeled result item (see ETABLE command) for the selected elements by comparing two existing labeled result items according to the operation:

where "cmn" means "compare and save minimum." If absolute values are requested [SABS,1], the absolute values of Lab1 and Lab2 are used.

Main Menu >General Postproc >Element Table >Find Minimum

Specifies meshing parameters for automatic (smart) element sizing.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Overall element size level for meshing. The level value controls the fineness of the mesh. (Any input in this field causes remaining arguments to be ignored.) Valid inputs are:

n - Activate SmartSizing and set the size level to n. Must be an integer value from 1 (fine mesh) to 10 (coarse mesh). Remaining arguments are ignored, and argument values are set as shown in the table under Notes.

STAT - List current SMRTSIZE settings.

DEFA - Set all SMRTSIZE settings to default values (as shown in the table for size level 6).

OFF - Deactivate SmartSizing. Current settings of DESIZE will be used. To reactivate SmartSizing, issue SMRTSIZE,n.

Scaling factor applied to the computed default mesh sizing. Defaults to 1 for h-elements (size level 6), which is medium. Values from 0.2 to 5.0 are allowed.

Mesh expansion (or contraction) factor. (This factor is the same as MOPT,EXPND,Value.) EXPND is used to size internal elements in an area based on the size of the elements on the area's boundaries. For example, issuing SMRTSIZE,,,2 before meshing an area will allow a mesh with elements that are approximately twice as large in the interior of an area as they are on the boundary. If EXPND is less than 1, a mesh with smaller elements on the interior of the area will be allowed. EXPND should be greater than 0.5 but less than 4. EXPND defaults to 1 for h-elements (size level 6), which does not allow expansion or contraction of internal element sizes (except when meshing flat areas and using the MOPT,IESZ option). (If EXPND is set to zero, the default value of 1 will be used.) The actual size of the internal elements will also depend on the TRANS and MOPT,IESZ options, if used.

Mesh transition factor. (This factor is the same as MOPT,TRANS,Value.) TRANS is used to control how rapidly elements are permitted to change in size from the boundary to the interior of an area. TRANS defaults to 2.0 for h-elements (size level 6), which permits elements to approximately double in size from one element to the next as they approach the interior of the area. (If TRANS is set to zero, the default value will be used.) TRANS must be greater than 1 and, for best results, should be less than 4. The actual size of the internal elements will also depend on the EXPND and MOPT,IESZ options, if used.

Maximum spanned angle per lower-order element for curved lines. Defaults to 22.5 degrees per element (size level 6). This angle limit may be exceeded if the mesher encounters a small feature (hole, fillet, etc.). (This value is NOT the same as that set by DESIZE,,,,ANGL.) This option does not apply to p-element meshes.

Maximum spanned angle per higher-order element for curved lines. Defaults to 30 degrees per element (size level 6). This angle limit may be exceeded if the mesher encounters a small feature (hole, fillet, etc.). (This value is NOT the same as that set by DESIZE,,,,,ANGH.)

Allowable growth ratio used for proximity checking. Defaults to 1.5 for h-elements (size level 6). Values from 1.2 to 5.0 are allowed; however, values from 1.5 to 2.0 are recommended.

Small hole coarsening key, can be ON (default for size level 6) or OFF. If ON, this feature suppresses curvature refinement that would result in very small element edges (i.e., refinement around small features).

Small angle coarsening key, can be ON (default for all levels) or OFF. If ON, this feature restricts proximity refinement in areas where it is ill-advised (that is, in tight corners on areas, especially those that approach 0 degrees).

Maximum number of sizing iterations (defaults to to 4 for all levels).

Surface proximity refinement key, can be off (SPRX=0, which is the default for all levels) or on via two different values (SPRX=1 or SPRX=2). If SPRX=1, surface proximity refinement is performed and any shell elements that need to be modified are modified. If SPRX=2, surface proximity refinement is performed but no shell elements are altered.

Notes

If a valid level number (1 to 10) is input on SIZLVL, inputs for remaining arguments are ignored, and the argument values are set as shown in the table below. Note that the settings are different for h-elements and p-elements (indicated by the "h" and "p" headings in the table).

^*Default

SmartSizing will use ESIZE as a starting size, but will locally override it for proximity and curvature. ESIZE,,NDIV is ignored when SmartSizing is on.

Lines with LESIZE specifications will be honored by SmartSizing. However, all lines not fixed by LESIZE are meshed as well as they can be.

KESIZE values are assigned as starting values for the region close to the keypoint. However, KESIZE will be overridden as needed for curvature and proximity.

DESIZE settings are not used unless one of the following is true: SmartSizing is turned off, mapped meshing is being done [MSHKEY,1 or 2], or KSCON (for stress concentrations or crack tips) is specified.

Main Menu >Preprocessor >Size Cntrls >Adv Opts

Main Menu >Preprocessor >Size Cntrls >Basic

Main Menu >Preprocessor >Size Cntrls >Status

Specifies "Surface loads on the solid model" as the subsequent status topic.

SOLUTION: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 >Solution >Surface Loads

Forms an element table item by multiplying two other items.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Label assigned to results. If same as existing label, the existing values will be overwritten by these results.

First labeled result item in operation.

Second labeled result item in operation (may be blank).

Scale factor applied to Lab1 (defaults to 1.0).

Scale factor applied to Lab2 (defaults to 1.0).

Forms a labeled result item (see ETABLE command) for the selected elements by multiplying two existing labeled result items according to the operation:

May also be used to scale results for a single labeled result item. If absolute values are requested [SABS,1], the absolute values of Lab1 and Lab2 are used.

Main Menu >General Postproc >Element Table >Multiply

Specifies whether to use optimized nonlinear solution defaults and some enhanced internal solution algorithms.

SOLUTION:AnalysisOptions

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

Optimized defaults activation key:

ON or 1 - Activates optimized defaults for a set of commands applicable to nonlinear solutions. This is the default. The majority of solution command defaults are listed under the Notes section below. See also the description of individual solution commands for default values.

OFF or 0 - Restores defaults to pre-ANSYS 5.4 values (see the Default States table below). Internal solution algorithms work as for pre-ANSYS 5.4.

Check contact state key. This key is operable only when the optimized defaults are active (Key1=ON) and a contact or nonlinear status element is present in the model. When check contact state is active, ANSYS will base the time step size on the specifications of KEYOPT(7) for all contact elements. KEYOPT(7) for contact elements can be used to ensure that the time step interval accounts for changes in the contact status. Also, when Key2=ON, ANSYS ensures the time step is small enough to account for changes in nonlinear element status (applies to LINK10, COMBIN7, COMBIN14, COMBIN39, and COMBIN40 elements). Valid arguments for the key are:

ON or 1 - Activate time step predictions based on specifications of element KEYOPT(7) or the nonlinear status of the element (applies to LINK10, COMBIN7, COMBIN14, COMBIN39, and COMBIN40 elements).

OFF or 0 - Time step predictions not based on contact status or nonlinear element status (default).

The SOLCONTROL command is designed to provide reliable and efficient default solution settings for single-field full structural nonlinear or full transient analysis, or single-field thermal analysis. (It is not applicable for reduced transient analysis.) The optimized default settings and advanced internal solution algorithms can be used to solve the majority of structural/thermal, nonlinear/transient problems with the least amount of user intervention. The SOLCONTROL command is ON by default. In most cases, to successfully solve a problem the user only needs to:

· Provide the initial step size through the NSUB or DELTIM command.

To achieve this, the SOLCONTROL command chooses better default settings for a number of commands within ANSYS and uses optimized internal solution algorithms. Note that the state of the SOLCONTROL command is not written by the CDWRITE or LSWRITE commands (so that the CDWRITE file does not rigidly define an individual solution command). Also note that switching SOLCONTROL ON and OFF between loadsteps is not recommended.

The SOLCONTROL command also serves as a "reset" command; when you issue SOLCONTROL, all the control commands set earlier in the interactive or input session are reset to their original default values.

Text database files (*.CDB files created by CDWRITE) and loadstep files (*.S01, *.S02, *.Snn, etc. files created by LSWRITE) should be handled with care when SOLCONTROL,ON (default). Files of these types sometimes contain control commands that you did not issue intentionally. These extra commands can overwrite the default settings specified by SOLCONTROL. To avoid overwriting the SOLCONTROL settings when you are using *.CDB files, use the following procedure:

2 Enter the solution processor [/SOLU].

3 Issue SOLCONTROL,ON.

4 Issue the desired control commands to overwrite the SOLCONTROL defaults as needed.

To use *.Snn files properly, you should preview and edit them. Delete the unwanted solution commands before you execute the LSSOLVE command.

The following table lists the nonlinear solution parameters and algorithm differences when the command is active and inactive.

Main Menu >Solution >Solution Ctrl

Enters the solution processor.

SESSION:ProcessorEntry SOLUTION:AnalysisOptions

	Mp Me St DY LP Th E3 E2 FL PP ED

This command is valid only at the Begin Level.

Main Menu >Solution

Specifies solution summary data per substep 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]).

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

Component of the item (if required). Valid component labels are shown in the table below. None are currently required.

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.

See also the PRITER command of POST1 to display some of these items directly. Valid item and component labels for solution summary values are:

Main Menu >TimeHist Postpro >Define Variables

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

Specifies "Solution options" as the subsequent status topic.

SOLUTION: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 >Solution >General

Starts a solution.

SOLUTION:AnalysisOptions

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

Starts the solution of one load step of a solution sequence based on the current analysis type and option settings.

Main Menu >Solution >Current LS

Main Menu >Solution >Run FLOTRAN

Main Menu >Solution >Solve

Specifies "Sort 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 >Sort Module

Defines a default location for undefined nodes or keypoints.

PREP7:Keypoints PREP7:Nodes

	Mp Me St DY LP Th E3 E2 FL PP ED

Global Cartesian coordinates for source nodes or keypoints (defaults to the origin).

Notes

Defines a global Cartesian location for undefined nodes or keypoints moved during intersection calculations [MOVE or KMOVE].

This command cannot be accessed directly in the menu.

Defines a space node for radiation.

AUX12:RadiationSubstructures

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

Node defined to be the space node.

Notes

A space node is required in an open system to account for radiation losses.

Main Menu >Radiation Matrix >Other Settings

Calculates scattering (S) parameters between ports of a waveguide.

POST1:Magnetics

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

Port number of the excited port with a TE10 mode or COAX mode excitation. (See the description of the PORTOPT command.)

Port number of the output port. This could be used for a multiport system. All ports but Porti must be matched.

The SPARM command macro returns the following scalar S parameters:

SII and SIJ, where "I" is the port number for the excited port and "J" is the output port number; and sBSII and dBSIJ, where dB is the log₁₀ equivalent of the S parameters.

See magnetic macros for further details.

Main Menu >General Postproc >Elec&Mag Calc >S-Parameters

Specifies "Miscellaneous specifications" 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 >Output Options

Creates a spherical volume anywhere on the working plane.

PREP7:Primitives

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

Working plane X and Y coordinates of the center of the sphere.

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

Defines either a solid or hollow spherical volume anywhere on the working plane. The sphere 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.) A sphere of 360° will be defined with two areas, each consisting of a hemisphere. See the SPHERE and SPH5 commands for other ways to create spheres.

When working with a model imported from an IGES file (DEFAULT import option), you can create only solid spheres. If you enter a value for both RAD1 and RAD2, the command is ignored.

Main Menu >Preprocessor >Create >Solid Sphere

Menu Paths

Main Menu >Preprocessor >Create >Sphere >Hollow Sphere

Main Menu >Preprocessor >Create >Sphere >Solid Sphere

Creates a spherical volume by diameter end points.

PREP7:Primitives

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

Working plane X and Y coordinates of one edge of the sphere.

Working plane X and Y coordinates of the other edge of the sphere.

Defines a solid spherical volume anywhere on the working plane by specifying diameter end points. The sphere 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.) A sphere of 360° will be defined with two areas, each consisting of a hemisphere. See the SPHERE and SPH4 commands for other ways to create spheres.

Main Menu >Preprocessor >Create >Sphere >By End Points

Creates a spherical volume centered about the working plane origin.

PREP7:Primitives

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

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

Starting and ending angles (either order) of the sphere. Used for creating a spherical 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 either a solid or hollow sphere or spherical sector centered about the working plane origin. The sphere 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.) For a solid sphere of 360°, it will be defined with two areas, each consisting of a hemisphere. See the SPH4 and SPH5 commands for the other ways to create spheres.

Main Menu >Preprocessor >Create >Sphere >By Dimensions

Generates a segmented spline through a series of keypoints.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Keypoints through which the spline is fit. At least two must be defined. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

The following fields are used only if specified end slopes on the line are desired, otherwise zero curvature end slopes will be automatically calculated to produce a line which is "straight" in the active coordinate system. To specify end slopes, use the following fields to define a "slope vector" (one for each end of the line, if desired) that has its tail at the origin and its head at the point XV,YV,ZV in the active coordinate system [CSYS]. The corresponding end slope of the line will then be parallel to this "slope vector."

Location (in the active coordinate system) of the head of the "slope vector" corresponding to the slope at the P1 end of the spline. The tail of the vector is at the origin of the coordinate system.

Location of the head of the "slope vector" corresponding to the slope at the P6 (or the last keypoint if fewer than six specified) end of the spline.

The output from this command is a series of connected lines (one line between each pair of keypoints) that together form a spline. Note that solid modeling in a toroidal coordinate system is not recommended.

Main Menu >Preprocessor >Create >Splines >Segmented Spline

Main Menu >Preprocessor >Create >Splines >With Options >Segmented Spline

Defines a point for moment summations.

POST1:SpecialPurpose

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

Node number of the desired point. If zero, use X,Y,Z to describe point.

Global Cartesian coordinates of the desired summation point. Used if NODE is 0. Defaults to (0,0,0).

Notes

Defines a point (any point other than the origin) about which the tabular moment summations are computed [NFORCE, FSUM]. If force summations are desired in other than the global Cartesian directions, a node number must be specified on the NODE field, and the desired coordinate system must be activated with RSYS.

Main Menu >General Postproc >Nodal Calcs >At Node

Main Menu >General Postproc >Nodal Calcs >At XYZ Loc

Selects the spectrum type and other spectrum options.

SOLUTION:SpectrumOptions

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

Spectrum type:

SPRS - Single point excitation response spectrum (default). See also the SVTYP command.

MPRS - Multiple point excitation response spectrum.

DDAM - Dynamic design analysis method.

PSD - Power spectral density.

Use the first NMODE modes from the modal analysis. Defaults to all modes.

Element calculation key (for Sptype=PSD only):

NO - Do not include stress responses in the calculations (default).

YES - Include stress responses in the calculations.

Valid only for a spectrum analysis (ANTYPE=SPECTR). This operation must be preceded by a modal solution (ANTYPE=MODAL) with the appropriate files available. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

Only Sptype=SPRS is allowed in ANSYS/LinearPlus.

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Turns on a dashed tolerance curve for the subsequent curve plots.

POST26:Display

	Mp Me St DY LP Th E3 E2 FL PP ED

Amount of tolerance. For example, 0.1 is 10%.

Menu Paths

Main Menu >TimeHist Postpro >Settings >Graph

Specifies "Spectrum analysis options" as the subsequent status topic.

SOLUTION: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 >Loads >Spectrum >Show Status

Main Menu >Solution >Spectrum >Show Status

Utility Menu >List >Status >Solution >Spectrum Options

Forms the square root of a variable.

POST26:Operations

	Mp Me St DY LP Th E3 E2 FL 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 the square root of a variable according to the operation:

Menu Paths

Main Menu >TimeHist Postpro >Math Operations >Square Root

Calculates terminal parameters for a stranded coil in a linear static analysis.

POST1:Magnetics

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

Number of turns in the coil winding. Input the total number of windings regardless of the symmetry used in the model.

Current per turn applied to the coil. Required only for a three-dimensional analysis (the value is calculated for a two-dimensional analysis and is returned as the parameter IWIND).

Harmonic frequency of coil current (in Hertz). Required only if terminal voltage (VLTG) is to be calculated. Assumes that eddy currents are neglected.

Planar symmetry factor. Used when a symmetric model is used through the cross-section of the coil. The factor is applied to the terminal parameter calculations. For example, if an axisymmetric coil is modeled with symmetry about the X-axis, the symmetry factor would be 2. Defaults to 1.

Circumferential symmetry factor. Used only for three-dimensional analysis when a circular-symmetric model is used. For example, if a 90 degree sector is modeled, the symmetry factor (to scale to a full 360 degree model) would be 4. Defaults to 1.

SRCS invokes an ANSYS macro which calculates terminal parameters for a stranded coil in a linear static analysis (constant properties, i.e. no B-H curve). The following terminal parameters are calculated: energy input to the coil (stored in the parameter WIN), terminal inductance (INDL), terminal voltage (VLTG), and flux linkages (FLNK). The elements making up the coil must be selected [ESEL] before this command is issued. The macro is valid for a static 2-D or 3-D analysis using a vector potential formulation. In addition, the vector potential must be either Neumann (Natural) or zero at the far-field boundary (explicitly set or by use of infinite elements). If these conditions are not met, apply the LMATRIX macro instead of SRCS to obtain the correct inductance. LMATRIX does not have these restrictions.

Main Menu >General Postproc >Elec&Mag Calc >Terminal Par

Specifies the square root of sum of squares mode combination method.

SOLUTION:SpectrumOptions

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

Combine only those modes whose significance level exceeds the SIGNIF threshold. For single point, multipoint, or DDAM response (SPOPT,SPRS, MPRS or DDAM), the significance level of a mode is defined as the mode coefficient of the mode, divided by the maximum mode coefficient of all modes. Any mode whose significance level is less than SIGNIF is considered insignificant and is not contributed to the mode combinations. The higher the SIGNIF threshold, the fewer the number of modes combined. SIGNIF defaults to 0.001. If SIGNIF is specified as 0.0, it is taken as 0.0. (This mode combination method is not valid for SPOPT,PSD.)

Label identifying the combined mode solution output.

DISP - Displacement solution (default). Displacements, stresses, forces, etc., are available.

VELO - Velocity solution. Velocities, "stress velocities," "force velocities," etc., are available.

ACEL - Acceleration solution. Accelerations, "stress accelerations," "force accelerations," etc., are available.

This command is also valid for PREP7.

Main Menu >Preprocessor >Loads >Spectrum >Mode Combine

Main Menu >Solution >Spectrum >Mode Combine

Sets the contour multiplier for topographic displays.

GRAPHICS:Scaling

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Contour multiplier that factors in results based on the product of the multiplier and the result being plotted. Defaults to 0.0 (no topographic effects).

Notes

Use this command to scale values to the geometry when the contours are shown elevated. For section displays [/TYPE], the elevation is performed perpendicular to the section face.

Non-zero contour multipliers factoring in large results (stresses or displacements) can produce very large distortion, causing images to disappear. To bring a distorted image back into view, reduce the contour multiplier value.

Utility Menu >PlotCtrls >Style >Contours >Contour Style

Selects and displays small lines in the model.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Factor used to determine small lines. FACT times the average line length in the model is used as the line length limit below which lines will be selected.

Line length limit for line selection. Lines that have a length less than or equal to SIZE will be selected. Used only if FACT is blank.

SSLN invokes a predefined ANSYS macro for selecting small lines in a model. Lines that are smaller than or equal to the specified limit (FACT or SIZE) are selected and line numbers are displayed. This command macro is useful for detecting very small lines in a model that may cause problems (i.e., poorly shaped elements or a meshing failure) during meshing. All lines that are not "small" will be unselected and can be reselected with the LSEL command.

Main Menu >Preprocessor >Check Geom >Sel Small Lines

Activates stress stiffness effects in a nonlinear analysis.

SOLUTION:NonlinearOptions

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

Stress stiffening key:

OFF - No stress stiffening is included (default unless NLGEOM,ON).

ON - Stress stiffening is included (default if NLGEOM,ON).

Notes

Activates stress stiffness effects in a nonlinear analysis (ANTYPE = STATIC or TRANS). (The PSTRES command also controls the generation of the stress stiffness matrix and therefore should not be used in conjunction with SSTIF.) If used in SOLUTION, this command is valid only within the first load step.

When SOLCONTROL and NLGEOM are ON, SSTIF defaults to ON. This normally forms all of the consistent tangent matrix. However, for some special nonlinear cases, this can lead to divergence due to some elements which do not provide a complete consistent tangent. In such a case, we recommend setting SSTIF OFF to achieve convergence.

The default values given for this command assume SOLCONTROL,ON (the default). See the description of SOLCONTROL 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 >Analysis Options

Main Menu >Solution >Analysis Options

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Calculates and prints the sum of element table items.

POST1:ElementTable

	Mp Me St DY LP Th E3 E2 FL PP ED

Calculates and prints the tabular sum of each existing labeled result item [ETABLE] for the selected elements. If absolute values are requested [SABS,1], absolute values are used.

Main Menu >General Postproc >Element Table >Sum of Each Item

Displays the status of database settings.

DATABASE:SetUp DISPLAY:Action

	Mp Me St DY LP Th E3 E2 FL PP ED

In the DISPLAY program, STAT will show the current status of the program settings.

In the ANSYS program, STAT is a command 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. Generally, STAT will be preceded by one of the commands listed below, which specifies the particular topic that status was requested for.

If entered directly into the program, the STAT command should be immediately preceded by the desired topic command listed below. In processors other than those listed below (e.g., AUX12), no topic command should proceed STAT.

This command is valid in any processor.

PREP7 topic commands (and their corresponding topics) are:

Topic Command - Topic

ETYPE - Element types.

RCON - Real constants.

MATER - Material properties.

TBLE - Data table properties.

PRIM - Solid model primitives.

KEYPTS - Keypoints.

LINE - Lines.

AREAS - Areas.

VOLUMES - Volumes.

GEOMETRY - Solid model information.

MESHING - Meshing.

BOOL - Booleans.

NODES - Nodes.

ELEM - Elements.

SELM - Superelements.

PIPE - Pipe modeling.

DIGIT - Node digitizing.

COUPLE - Node coupling.

CEQN - Constraint equations.

REORDER - Model reordering.

SOLUTION topic commands (and their corresponding topics) are:

Topic Command - Topic

ATYPE - Analysis types.

MASTER - Master DOF.

GAP - Reduced transient gap conditions.

DEACT - Element birth and death (deactivation).

LSOPER - Load step operations.

FECONS - Constraints on nodes.

FEFOR - Forces on nodes.

FESURF - Surface loads on elements.

FEBODY - Body loads on elements.

SMCONS - Constraints on the solid model.

SMFOR - Forces on the solid model.

SMSURF - Surface loads on the solid model.

SMBODY - Body loads on the solid model.

INRTIA - Inertial loads.

GENOPT - General options.

DYNOPT - Dynamic analysis options.

NLOPT - Nonlinear analysis options.

OUTOPT - Output options.

BIOOPT - Biot-Savart options.

SPTOPT - Spectrum analysis options.

SOLUOPT - Solution options.

FLOTRAN - FLOTRAN data settings.

POST1 topic commands (and their corresponding topics) are:

Topic Command - Topic

DEFINE - Data definition settings.

SORT - Sort settings.

PRINT - Print settings.

DISPLAY - Display settings.

CALC - Calculation settings.

PATH - Path data settings.

LCCALC - Load case settings.

DATADEF - Directly defined data status.

FATIGUE - Fatigue data status.

POINT - Point flow tracing settings.

SPEC - Miscellaneous specifications.

POST26 topic commands (and their corresponding topics) are:

Topic Command - Topic

DEFINE - Data definition settings.

OPERATE - Operation data.

PRINT - Print settings.

PLOTTING - Plotting settings.

Utility Menu >List >Status >(type of status)

Lists the current parameters and abbreviations.

APDL:Parameters

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of parameter to be listed. For array parameters, use IMIN, IMAX, etc. to specify ranges. If blank, list all scalar parameter values, array parameter dimensions, and abbreviations. If ARGX, list the active set of local macro parameters (ARG1 to AR99) [*USE].

Range of array elements to display (in terms of the three dimensions (row, column, and plane). Minimum values default to 1. Maximum values default to the maximum dimension values. Zero may be input to display the index numbers.

This command does not list parameters whose name starts or ends with an underscore.

This command is valid in any processor.

Utility Menu >List >Other >Named Parameter

Utility Menu >List >Other >Parameters

Utility Menu >List >Status >Parameters >All Parameters

Utility Menu >List >Status >Parameters >Named Parameters

Lists the status of items for the run.

SESSION:RunControls

	Mp Me St DY LP Th E3 E2 FL PP ED

Items to list status for:

ALL - List all below (default).

TITLE - List only titles, Jobname, and revision number.

UNITS - List only units.

MEM - List only scratch data statistics.

DB - List only database statistics

CONFIG - List only configuration parameters.

GLOBAL - Provides a global status summary.

SOLU - Provides a solution status summary.

PHYS - List all active element types, key options, real constants, material properties, and coordinate systems.

Displays various items active for the run (such as the ANSYS revision number, Jobname, titles, units, configuration parameters, database statistics, etc.).

The /STATUS,PHYS command performs the same function as the PHYSICS command.

This command is valid in any processor.

Utility Menu >List >Status >Global Status

Specifies Stefan-Boltzmann radiation constant.

AUX12:RadiationSubstructures

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

Stefan-Boltzmann constant (defaults to 0.119E-10 Btu/hr/in²/°R⁴).

Notes

You can use this command in the general preprocessor (PREP7) and in the Solution processor to specify the Stefan-Boltzmann constant for a FLOTRAN analysis using radiation surface boundary conditions.

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

Main Menu >Preprocessor >Loads >Apply >Radiation >On Elements

Main Menu >Preprocessor >Loads >Apply >Radiation >On Lines

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

Main Menu >Radiation Matrix >Other Settings

Main Menu >Solution >Apply >Radiation >On Areas

Main Menu >Solution >Apply >Radiation >On Elements

Main Menu >Solution >Apply >Radiation >On Lines

Main Menu >Solution >Apply >Radiation >On Nodes

Defines subtitles.

DATABASE:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Subtitle line number (1 to 4). Defaults to 1.

Input up to 70 alphanumeric characters. Parameter substitution may be forced within the title by enclosing the parameter name or parametric expression within percent (%) signs. If Title is blank, this subtitle is deleted.

Subtitles (4 maximum) are displayed in the output along with the main title [/TITLE]. Subtitles do not appear in GUI windows or in ANSYS plot displays. The first subtitle is also written to various ANSYS files along with the main title. Previous subtitles may be overwritten or deleted. Issue /STATUS to display titles.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Stores data in the database for the defined variables.

POST26:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Valid labels:

MERGE - Merge data from results file for the time points in memory with the existing data using current specifications (default).

NEW - Store a new set of data (replacing any previously stored data and erasing any previously calculated data) with current specifications.

APPEN - Append data from results file to the existing data.

ALLOC - Allocate (and zero) space for NPTS data points.

PSD - Create a new set of frequency points for PSD calculations (replacing any previously stored data and erasing any previously calculated data).

The number of time points (or frequency points) for storage (used only with Lab=ALLOC or PSD). The value may be input when using POST26 with data supplied from other than a results file. This value is automatically determined from the results file data with the NEW, APPEN, and MERGE options. For the PSD option, NPTS determines the resolution of the frequency vector (valid numbers are between 1 and 10, defaults to 5).

Notes

This command stores data from the results file in the database for the defined variables [NSOL, ESOL, SOLU] per specification [FORCE, LAYERP26, SHELL]. See the ANSYS Basic Analysis Procedures Guide for more information.

The STORE,PSD command will create a new frequency vector (variable 1) for response PSD calculations [RPSD]. This command should first be issued before defining variables [NSOL, ESOL, RFORCE] for which response PSD's are to be calculated.

Main Menu >TimeHist Postpro >Store Data

Specifies options for subspace iteration eigenvalue extraction.

SOLUTION:NonlinearOptions SOLUTION:DynamicOptions

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

Subspace working size. Defaults to NMODE + 4 (where NMODE is input on the the MODOPT or BUCOPT command). Minimum is 8. Maximum is NMODE+NPAD. The larger the value, the smaller the number of iterations (but more time per iteration).

Number of extra vectors used in the iterations. Defaults to 4. The total number of vectors used is NMODE+NPAD.