A

Defines an area by connecting keypoints.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

List of keypoints defining the area (18 maximum if using keyboard entry). At least 3 keypoints must be entered. If P1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI).

Keypoints (P1 through P18) must be input in a clockwise or counter-clockwise order around the area. This order also determines the positive normal direction of the area according to the right-hand rule. Existing lines between adjacent keypoints will be used; missing lines are generated "straight" in the active coordinate system and assigned the lowest available numbers [NUMSTR]. If more than one line exists between two keypoints, the shorter one will be chosen. If the area is to be defined with more than four keypoints, the required keypoints and lines must lie on a constant coordinate value in the active coordinate system (such as a plane or a cylinder). Areas may be redefined only if not yet attached to a volume. Solid modeling in a toroidal coordinate system is not recommended.

Main Menu >Preprocessor >Create >Arbitrary >Through KPs

Adds separate areas to create a single area.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of areas to be added. If NA1 = ALL, add all selected areas and ignore NA2 to NA9. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1.

The areas must be coplanar. The original areas (and their corresponding lines and keypoints) will be deleted by default. See the BOPTN command for the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated. Concatenated entities are not valid with this command.

Main Menu >Preprocessor >Operate >Add >Areas

Associates element attributes with the selected, unmeshed areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

The material number to be associated with selected, unmeshed areas.

The real constant set number to be associated with selected, unmeshed areas.

The type number to be associated with selected, unmeshed areas.

The coordinate system number to be associated with selected, unmeshed areas.

Areas subsequently generated from the areas will also have these attributes. These element attributes will be used when the areas are meshed. If an area does not have attributes associated with it (by this command) at the time it is meshed, the attributes are obtained from the then current MAT, REAL, TYPE, and ESYS command settings. Reissue the AATT command (before areas are meshed) to change the attributes. A zero (or blank) argument removes the corresponding association.

In some cases, ANSYS can proceed with an area meshing operation even when no logical element type has been assigned via AATT,,,TYPE or TYPE. For more information, see the discussion on setting element attributes in Chapter 7 of the ANSYS Modeling and Meshing Guide.

Main Menu >Preprocessor >Define >All Areas

Main Menu >Preprocessor >Define >Picked Areas

Defines an abbreviation.

APDL:Abbreviations

	Mp Me St DY LP Th E3 E2 FL PP ED

The abbreviation (up to 8 alphanumeric characters) used to represent the string String. If Abbr is the same as an existing ANSYS command, the abbreviation overrides. Avoid using an Abbr which is the same as an ANSYS command. A string may be mapped to a function key on some terminals by using the function key for Abbr.

String of characters (60 maximum) represented by Abbr. Cannot include a $ or any of the commands C***, /COM, /GOPR, /NOPR, /QUIT, /UI, or *END. Parameter names and commands of the *DO and *IF groups may not be abbreviated. If String is blank, the abbreviation is deleted. To abbreviate multiple commands, create an "unknown command" macro or define String to execute a macro file [*USE] containing the desired commands.

Once the abbreviation Abbr is defined, you can issue it at the beginning of a command line and follow it with a blank (or with a comma and appended data), and the program will substitute the string String for Abbr as the line is executed. Up to 100 abbreviations may exist at any time and are available throughout the program. Abbreviations may be redefined or deleted at any time.

Use *STATUS to display the current list of abbreviations. For abbreviations repeated with *REPEAT, substitution occurs before the repeat increments are applied. There are a number of abbreviations that are predefined by the program (these can be deleted by using the blank String option described above). Note that String will be written to the File.LOG.

This command is valid in any processor.

Utility Menu >Macro >Edit Abbreviations

Utility Menu >MenuCtrls >Edit Toolbar

Reads abbreviations from a coded file.

APDL:Abbreviations

	Mp Me St DY LP Th E3 E2 FL PP ED

Label that specifies the read operation:

NEW - Replace current abbreviation set with these abbreviations (default).

CHANGE - Extend current abbreviation set with these abbreviations, replacing any of the same name that already exist.

Name of file to be read (32 characters maximum). Defaults to Jobname.

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

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

The abbreviation file may have been written with the ABBSAV command.

This command is valid in any processor.

Utility Menu >Macro >Restore Abbr

Utility Menu >MenuCtrls >Restore Toolbar

Writes the current abbreviation set to a coded file.

APDL:Abbreviations

	Mp Me St DY LP Th E3 E2 FL PP ED

Label that specifies the write operation:

ALL - Write all abbreviations (default).

Name of file to be written (32 characters maximum). Defaults to Jobname.

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

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

Existing abbreviations on this file, if any, will be overwritten. The abbreviation file may be read with the ABBRES command.

This command is valid in any processor.

Utility Menu >Macro >Save Abbr

Utility Menu >MenuCtrls >Save Toolbar

Forms the absolute value 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).

The new variable is calculated as:

For a complex number (a+ib), the absolute value is the magnitude, where the IA values are obtained from . See Section 19.10 of the ANSYS Theory Reference for details.

Main Menu >TimeHist Postpro >Math Operations >Absolute Value

Concatenates multiple areas in preparation for mapped meshing.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Areas to be concatenated. If NA1 = ALL, NA2 will be ignored and all selected areas [ASEL] will be concatenated. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 is ignored).

Concatenates multiple, adjacent areas (the input areas) into one area (the output area) in preparation for mapped meshing. A volume that contains too many areas for mapped meshing can still be mapped meshed if some of the areas in that volume are first concatenated (see Chapter 7 of the ANSYS Modeling and Meshing Guide for details on mapped meshing restrictions).

Because of modeling restrictions that result from its use, ACCAT is meant to be used solely for meshing. Specifically, (a) the output area and any volumes that have the output area on their area list [VLIST] cannot be used as input to any other solid modeling operation (not even another ACCAT command); and (b) the output area cannot accept solid model boundary conditions [DA, SFA].

The output area (or volumes which contain it) will be meshed [AMESH, VMESH] by meshing the input areas, which themselves must be meshable. The output area from the ACCAT operation will be coincident with the input areas and the input areas will be retained. Consider the AADD command instead of ACCAT if you wish to delete the input areas. When an ACCAT command is issued, volume area lists [VLIST] that contain all of the input areas will be updated so that the volume area lists refer to the output area instead of the the input area. Deletion of the output area [ADELE] effectively reverses the ACCAT operation and restores volume area lists to their original condition. ACCAT operations on pairs of adjacent four-sided areas automatically concatenate appropriate lines [LCCAT]; in all other situations, line concatenations must be addressed by the user.

You can use the ASEL command to select areas that were created by concatenation, and then follow it with an ADELE,ALL command to delete them. See Chapter 7 of the ANSYS Modeling and Meshing Guide for a discussion on how to easily select and delete concatenated areas in one step.

Main Menu >Preprocessor >Concatenate >Areas

Main Menu >Preprocessor >Delete >Areas

Main Menu >Preprocessor >Mesh >Mapped >Areas

Specifies the linear acceleration of the structure.

SOLUTION:Inertia

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

Linear acceleration of the structure in the global Cartesian X, Y, and Z axis directions.

Related commands for rotational effects are CGLOC, CGOMGA, DCGOMG, DOMEGA, and OMEGA.

Defines the linear acceleration of the structure in each of the global Cartesian axis directions. To simulate gravity (by using inertial effects), accelerate the structure in the direction opposite to gravity. For example, apply a positive ACELY to simulate gravity acting in the negative Y direction. Units are length/time².

Accelerations may be defined in analysis types ANTYPE=STATIC, HARMIC (except reduced), TRANS, and SUBSTR. For all but the reduced transient dynamic (ANTYPE=TRANS) analysis, accelerations are combined with the element mass matrices to form a body force load vector term. The element mass matrix may be formed from a mass input constant or from a nonzero density (DENS) property, depending upon the element type. Units of acceleration and mass must be consistent to give a product of force units. For analysis type ANTYPE=HARMIC, the acceleration is assumed to be the real component with a zero imaginary component. For ANTYPE=TRANS (reduced), the acceleration is applied to the reduced mass matrix.

This command is also valid in PREP7.

Main Menu >Preprocessor >FLOTRAN Set Up >Flow Environment >Gravity

Main Menu >Preprocessor >Loads >Apply >Gravity

Main Menu >Preprocessor >Loads >Delete >Gravity

Main Menu >Solution >Apply >Gravity

Main Menu >Solution >Delete >Gravity

Main Menu >Solution >FLOTRAN Set Up >Flow Environment >Gravity

Deletes nodes and area elements associated with selected areas.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Delete mesh for areas NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL, NA2 and NINC are ignored and the mesh for all selected areas [ASEL] is deleted. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Deletes all nodes and area elements associated with selected areas (regardless of whether the nodes or elements are selected). Nodes shared by adjacent meshed areas and nodes associated with non-area elements will not be deleted. Attributes assigned as a result of AATT are maintained. In the program's response to the command, if an area, line, or keypoint is tallied as "cleared," it means either its node or element reference was deleted.

Main Menu >Preprocessor >Clear >Areas

Adaptively meshes and solves a model.

SOLUTION:AnalysisOptions

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

Number of solutions allowed (1 or more) (defaults to 5).

Target percentage for structural percent error in energy norm (SEPC) (defaults to 5). If -1, no target value is used.

Target percentage for thermal percent error in energy norm (TEPC) (defaults to 1). If -1, no target value is used.

Minimum factor for the keypoint element size changes (defaults to 0.25).

Maximum factor for the keypoint element size changes (defaults to 2.0).

Specifies whether element size is to be modified at selected keypoints:

0 - Modify element size regardless of selected keypoint set (default).

1 - Modify element size only at selected keypoints.

Specifies which user-written auxiliary macro files are to be used:

0 - Ignore user-written auxiliary macro files, if any (default).

1 - Use user-written auxiliary macro files (if they exist) as follows: Use ADAPTMSH.MAC instead of the default meshing command sequence. Use ADAPTSOL.MAC instead of the default solution command sequence (/SOLU...SOLVE...FINISH).

ADAPT invokes a predefined ANSYS macro for adaptive meshing and solution. The macro causes repeated runs of the PREP7, SOLUTION, and POST1 phases of the ANSYS program with mesh density refinements based upon the percentage error in energy norm. See the ANSYS Advanced Analysis Techniques Guide for additional details. After the adaptive meshing process is complete, the ADAPT macro automatically turns element shape checking on (SHPP,ON).

A copy of the macro, called UADAPT.MAC, is available on the ANSYS distribution medium (system dependent), and may be copied and modified by the user to suit a particular need. The modified file should be given a suitable name (cmd.MAC) and run as described above with the ADAPT command name replaced by your "cmd" name.

This command is also valid at the Begin level.

Main Menu >Solution >Adaptive Mesh

Adds 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 variables, leave IC blank. If only one, leave IB and IC blank.

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 (default to 1.0).

Adds variables (up to three at once) according to the operation:

Main Menu >TimeHist Postpro >Math Operations >Add

Specifies the acceleration spectrum computation constants for the analysis of shock resistance of shipboard structures.

SOLUTION:SpectrumOptions

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

Direction-dependent acceleration coefficient for elastic or elastic-plastic analysis option (Default = 0).

Coefficients for the DDAM acceleration spectrum equations. See Section 17.7.4 of the ANSYS Theory Reference. Default for these coefficients is zero.

The minimum acceleration value in inch/sec². It defaults to 2316 inch/sec² which equals 6g, where g is acceleration due to gravity (g = 386 inch/sec²).

This command specifies acceleration coefficients to analyze shock resistance of shipboard equipment. These coefficients are used to compute mode coefficients according to the equations given in Section 17.7.4 of the ANSYS Theory Reference. The form of these equations is based on the Naval NRL Dynamic Design Analysis Method. This command, along with the VDDAM and SED commands, is used with the spectrum (ANTYPE=SPECTR) analysis as a special purpose alternative to the SV, FREQ, and SVTYP commands. The mass and length units of the model must be in pounds and inches, respectively.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Spectrum >DDAM Options

Main Menu >Solution >Spectrum >DDAM Options

Deletes unmeshed areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Delete areas from NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL, NA2 and NINC are ignored and all selected areas [ASEL] are deleted. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Specifies whether keypoints and lines are also to be deleted:

0 - Delete areas only (default).

1 - Delete areas, as well as keypoints and lines attached to specified areas but not shared by other areas.

An area attached to a volume cannot be deleted unless the volume is first deleted.

Main Menu >Preprocessor >Delete >Area and Below

Main Menu >Preprocessor >Delete >Areas Only

Menu Paths (IGES Only)

Main Menu >Preprocessor >Topo Repair >Delete >Area and Below

Main Menu >Preprocessor >Topo Repair >Delete >Areas Only

Lists keypoints of an area that lie on a parametric degeneracy.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

List keypoints that lie on a parametric degeneracy on areas from NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL (default), NA2 and NINC will be ignored and keypoints on all selected areas [ASEL] will be listed. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may be substituted in NA1 (NA2 and NINC will be ignored).

See the ANSYS Modeling and Meshing Guide for details on parametric degeneracies.

This command is valid in any processor.

Main Menu >Preprocessor >Check Geom >Show Degeneracy >List Degen Areas

Main Menu >Preprocessor >Operate >Show Degeneracy >List Degen Areas

Generates areas by dragging a line pattern along a path.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

List of lines in the pattern to be dragged (6 maximum if using keyboard entry). Lines should form a continuous pattern (no more than two lines connected to any one keypoint. If NL1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). If NL1=ALL, all selected lines (except those that define the drag path) will be swept along the path. A component name may also be substituted for NL1.

List of lines defining the path along which the pattern is to be dragged (6 maximum if using keyboard entry). Must be a continuous set of lines.

Generates areas (and their corresponding keypoints and lines) by sweeping a given line pattern along a characteristic drag path. If the drag path consists of multiple lines, the drag direction is determined by the sequence in which the path lines are input (NLP1, NLP2, etc). If the drag path is a single line (NLP1), the drag direction is from the keypoint on the drag line that is closest to the first keypoint of the given line pattern to the other end of the drag line.

The magnitude of the vector between the keypoints of the given pattern and the first path keypoint remains constant for all generated keypoint patterns and the path keypoints. The direction of the vector relative to the path slope also remains constant so that patterns may be swept around curves.

Keypoint, line, and area numbers are automatically assigned (beginning with the lowest available values [NUMSTR]). Adjacent lines use a common keypoint. Adjacent areas use a common line. For best results, the entities to be dragged should be orthogonal to the start of the drag path. Drag operations that produce an error message may create some of the desired entities prior to terminating.

Main Menu >Preprocessor >Operate >Extrude / Sweep >Along Lines

Generates a fillet at the intersection of two areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the first intersecting area. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI).

Number of the second intersecting area.

Radius of fillet to be generated.

Generates an area of constant fillet radius at the intersection of two areas using a series of Boolean operations. Corresponding lines and keypoints are also generated. See BOPTN command for an explanation of the options available to Boolean operations. If areas do not initially intersect at a common line, use the AINA command.

Main Menu >Preprocessor >Create >Area Fillet

Lists the current data in the database.

PREP7:Database

	Mp Me St DY LP Th E3 E2 FL PP ED

Lists the current data and specifications in the database. If batch, lists all appropriate data. If interactive, lists only summaries.

Utility Menu >List >Other >Database Summary

Generates surface elements overlaid on the surface of existing solid elements and assigns the extra node as the closest fluid element node.

PREP7:Elements

	Mp Me -- -- -- Th -- -- -- -- ED

Component name for the surface areas of the meshed solid volumes.

Component name for the target lines meshed with fluid elements.

This command macro is used to generate surface effect elements overlaid on the surface of existing solid elements and, based on proximity, to determine and assign the extra node for each surface element. The underlying volumes of the solid region and the fluid lines must be meshed prior to calling this command macro.

The surface areas of the solid and the target lines of the fluid are grouped into components and named using the CM command. The names must be enclosed in single quotes (e.g., 'SAREA') when the AFSURF command is manually typed in.

The macro is applicable for the SURF152 and FLUID116 element types.

Main Menu >Preprocessor >Create >Elements >Surf Effect >Area to Fluid

Main Menu >Preprocessor >Create >Elements >Surf Effect >Line to Fluid

Specifies units for angular functions in parameter expressions.

APDL:Parameters

	Mp Me St DY LP Th E3 E2 FL PP ED

Specifies the units to be used:

RAD - Use radians for input and output of parameter angular functions (default).

DEG - Use degrees for input and output of parameter angular functions.

STAT - Show current setting (DEG or RAD) for this command.

Notes

Only the SIN, COS, TAN, ASIN, ACOS, ATAN, ATAN2, ANGLEK, and ANGLEN functions [*SET, *VFUN] are affected by this command.

Utility Menu >Parameters >Angular Units

Generates additional areas from a pattern of areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Do this generation operation a total of ITIMEs, incrementing all keypoints in the given pattern automatically (or by KINC) each time after the first. ITIME must be more than 1 for generation to occur.

Generate areas from the pattern of areas NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL, NA2 and NINC are ignored and the pattern is all selected areas [ASEL]. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Keypoint location increments in the active coordinate system (-,D,DZ for cylindrical; -,D,- for spherical).

Keypoint number increment between generated sets. If zero, the lowest available keypoint numbers are assigned [NUMSTR].

Specifies if elements and nodes are also to be generated:

0 - Generate nodes and elements associated with the original areas, if they exist.

1 - Do not generate nodes and elements.

Specifies whether to redefine the existing areas:

0 - Generate new areas as requested with the ITIME argument.

1 - Move original areas to new position, retaining the same keypoint numbers (ITIME, KINC, and NOELM are ignored). If the original areas are needed in the original position (e.g., they may be attached to a volume), they are not moved, and new areas are generated instead. Meshed items corresponding to moved areas are also moved if not needed at their original position.

Generates additional areas (and their corresponding keypoints, lines and mesh) from a given area pattern. The MAT, TYPE, REAL, and ESYS attributes of the new areas are based upon the areas in the pattern and not upon the current settings of the pointers. End slopes of the generated lines remain the same (in the active coordinate system) as those of the given pattern. For example, radial slopes remain radial. Generations which produce areas of a size or shape different from the pattern (i.e., radial generations in cylindrical systems, radial and phi generations in spherical systems, and theta generations in elliptical systems) are not allowed. Solid modeling in a toroidal coordinate system is not recommended. Area and line numbers are automatically assigned, beginning with the lowest available values [NUMSTR].

Main Menu >Preprocessor >Copy >Areas

Main Menu >Preprocessor >Move / Modify >Areas

Generates new areas by "gluing" areas.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of the areas to be glued. If NA1 = ALL, all selected areas will be glued (NA2 to NA9 will be ignored). If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1.

Generates new areas by "gluing" input areas. The glue operation redefines the input areas so that they share lines along their common boundaries. The new areas encompass the same geometry as the original areas. This operation is only valid if the intersection of the input areas are lines along the boundaries of those areas. See the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for an explanation of the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to new entities generated.

Main Menu >Preprocessor >Operate >Glue >Areas

Finds the intersection of areas.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of areas to be intersected. If NA1 = ALL, NA2 to NA9 are ignored and the intersection of all selected areas is found. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1.

Finds the common (not pairwise) intersection of areas. The common intersection is defined as the regions shared (in common) by all areas listed on this command. New areas will be generated where the original areas intersect. If the regions of intersection are only lines, new lines will be generated instead. See the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Intersect >Areas

Finds the pairwise intersection of areas.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of areas to be intersected pairwise. If NA1 = ALL, NA2 to NA9 are ignored and the pairwise intersection of all selected areas is found. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may be substituted for NA1.

Finds the pairwise intersection of areas. The pairwise intersection is defined as all regions shared by any two or more areas listed on this command. New areas will be generated where the original areas intersect pairwise. If the regions of pairwise intersection are only lines, new lines will be generated. See the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Intersect >Areas

Finds the intersection of an area with a volume.

PREP7:Booleans

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

Number of area to be intersected. If P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI).

Number of volume to be intersected.

New areas will be generated where the areas intersect the volumes. If the regions of intersection are only lines, new lines will be generated instead. See the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Intersect >Area with Volume

Generates an area bounded by previously defined lines.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

List of lines defining area. The minimum number of lines is 3. The positive normal of the area is controlled by the direction of L1 using the right-hand rule. A negative value of L1 reverses the normal direction. If L1 = ALL, use all selected lines with L2 defining the normal (L3 to L10 are ignored and L2 defaults to the lowest numbered selected line). If L1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for L1.

Lines may be input (once each) in any order and must form a simply connected closed curve. If the area is defined with more than four lines, the lines must also lie in the same plane or on a constant coordinate value in the active coordinate system (such as a plane or a cylinder). Note that solid modeling in a toroidal coordinate system is not recommended. Areas may be redefined only if not yet attached to a volume.

This command is valid in any processor.

Main Menu >Preprocessor >Create >Arbitrary >By Lines

Lists the defined areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

List areas from NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL (default), NA2 and NINC are ignored and all selected areas [ASEL] are listed. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Determines what type of listing is used (one of the following):

<blank> - Prints information about all areas in the specified range.

HPT - Prints information about only those areas that contain hard points.

An attribute (TYPE, MAT, REAL, or ESYS) listed as a zero is unassigned; one listed as a positive value indicates that the attribute was assigned with the AATT command (and will not be reset to zero if the mesh is cleared); one listed as a negative value indicates that the attribute was assigned using the attribute pointer [TYPE, MAT, REAL, or ESYS] that was active during meshing (and will be reset to zero if the mesh is cleared). A "-1" in the "nodes" column indicates that the area has been meshed but there are no interior nodes. The area size is listed only if an ASUM command has been performed on the area.

Utility Menu >List >Areas

Utility Menu >List >Picked Entities >Areas

Fills in an area loop within an existing 2-D area (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

List of lines that define the loop. If LN1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). If LN1 = ALL, all selected lines will be checked for possible closure.

If all of the lines in the list are not continuous or closed, ANSYS will automatically find the subset of continuous lines within the list.

Use this command to fill in small area loops in models imported from CAD files (this is a geometry "clean-up" tool). This tool is available only for models imported from CAD files (Default IGES option). .

Main Menu >Preprocessor >Simplify >Fill Loops

Selects all entities with a single command.

DATABASE:Selecting

	Mp Me St DY LP Th E3 E2 FL PP ED

Type of selection to be made:

ALL - Selects all items of the specified entity type and all items of lower entity types (default).

BELOW - Selects all items directly associated with and below the selected items of the specified entity type.

Entity type on which selection is based:

ALL - All entity types (default).

VOLU - Volumes.

AREA - Areas.

LINE - Lines.

KP - Keypoints.

ELEM - Elements.

NODE - Nodes.

ALLSEL is a convenience command that allows the user to select all items of a specified entity type or to select items associated with the selected items of a higher entity.

An entity hierarchy is used to decide what entities will be available in the selection process. This hierarchy from top to bottom is as follows: volumes, areas, lines, keypoints, elements, and nodes. The hierarchy may also be divided into two branches: the solid model and the finite element model. The label ALL selects items based on one branch only, while BELOW uses the entire entity hierarchy. For example, ALLSEL,ALL,VOLU selects all volumes, areas, lines, and keypoints in the data base. ALLSEL,BELOW,AREA selects all lines belonging to the selected areas; all keypoints belonging to those lines; all elements belonging to those areas, lines, and keypoints; and all nodes belonging to those elements.

This command is valid in any processor.

Utility Menu >Select >Everything Below >Selected Areas

Utility Menu >Select >Everything Below >Selected Elements

Utility Menu >Select >Everything Below >Selected Keypoints

Utility Menu >Select >Everything Below >Selected Lines

Utility Menu >Select >Everything Below >Selected Volumes

Utility Menu >Select >Everything

Defines the mass matrix multiplier for damping.

SOLUTION:DynamicOptions

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

Mass matrix multiplier for damping.

Defines the mass matrix multiplier, , for damping. One form of the viscous damping matrix [C] is given by [M] + [K], where [M] is the mass matrix and [K] is the stiffness matrix. Damping is not used in the static (ANTYPE=STATIC) or buckling (ANTYPE=BUCKLE) analyses.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Time/Frequenc >Damping

Main Menu >Solution >Time/Frequenc >Damping

Generates a 2-D mapped mesh based on specified area corners.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Area number of area to be meshed. If AREA=P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI).

Keypoints defining corners of the mapped mesh. Three or four corners may be specified, and may be input in any order.

Only one area at a time can be meshed with this command. The program internally concatenates all lines between the specified keypoints, then meshes the area with all quadrilateral elements. If line divisions are set, the mesh will follow the rules for mapped meshing (see Chapter 7 of the ANSYS Modeling and Meshing Guide).

If the area being meshed has concatenated lines, the program will ask if those concatenations should be removed (in batch, the concatenations will automatically be removed). Nodes required for the generated elements are created and assigned the lowest available node numbers. If a mapped mesh is not possible due to mis-matched line divisions or poor element shapes, the meshing operation is aborted.

Main Menu >Preprocessor >Mesh >Mapped >By Corners

Generates nodes and area elements within areas.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Mesh areas from NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL, NA2 and NINC are ignored and all selected areas [ASEL] are meshed. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Any undefined nodes required for the generated elements are created and assigned the lowest available numbers.

Main Menu >Preprocessor >Mesh >Free

Main Menu >Preprocessor >Mesh >Mapped >3 or 4 sided

Main Menu >Preprocessor >Mesh >Target Surf

Produces an animated sequence of a contoured deformed shape.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of frames captures (defaults to 5).

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

ANCNTR involves an ANSYS macro which produces an animation of a contoured deformed shape of the last plot action command. This command operates only on graphic display platforms supporting the /SEG command. After executing ANCNTR, you can replay the animated sequence by issuing the ANIM command.

The command functions only in the postprocessor.

Utility Menu >PlotCtrls >Animate >Deformed Results

Produces an animated sequence of Q-slices.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of frames captures (defaults to 5).

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

Q-slice working plane increment (defaults to .1 half screens).

Topological effect on or off (YES or NO; default is NO).

Topological offset (default is .1 half screens).

Node 1 for start of the Q-slice.

Node 2 for direction of the Q-slice.

Node 3 for plane of the Q=slice.

ANCUT involves an ANSYS macro which produces an animation of Q-slices of the last plot action command. This command operates only on graphic display platforms supporting the /SEG command. After executing ANCUT, you can replay the animated sequence by issuing the ANIM command.

The command functions only in the postprocessor.

Utility Menu >PlotCtrls >Animate >Q-Slice Contours

Utility Menu >PlotCtrls >Animate >Q-Slice Vectors

Produces a sequential contour animation over a range of results data.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Time delay during animation (defaults to 0.5 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

The type of results data to be used for the animation sequence. This can be:

0 - Current load step data (default).

1 - Range of load step data.

2 - Range of results data.

The range minimum value. If left blank or 0, defaults to the first data point.

The range maximum value. If left blank or 0, defaults to the last data point.

The increment between result data (defaults to 1).

Key to force the last result data item in a load step to be animated (defaults to 0).

Auto-scales contour values, based on the overall subset range of values. The auto-scaling option defaults to 0, no auto-scaling.

The ANDATA command operates only on graphic display platforms supporting the /SEG command. It uses an ANSYS macro to produce an animation based on the last plot action command (e.g., PLDISP).

This command functions only in the postprocessor.

Utility Menu>PlotCtrls>Animate>Over Results

Produces an animated sequence of a deformed shape.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of frames captured (defaults to 5).

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

ANDSCL involves an ANSYS macro which produces an animation of displacement of the last plot action command (for example, PLDISP). This command operates only on graphic display platforms supporting the /SEG command. After executing ANDSCL, you can replay the animated sequence by issuing the ANIM command.

The command functions only in the postprocessor.

Utility Menu >PlotCtrls >Animate >Deformed Shape

Produces an animated sequence of contour values through substeps.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

Number of the starting substep (defaults to 1).

Number of the ending substep (defaults to the maximum substep).

Increment between substeps (defaults to 1).

Auto-scales contour values, based on the overall subset range of values (defaults to 0, no auto-scaling).

ANDYNA involves an ANSYS macro which produces an animation of contour values through all the substeps of the last plot action command. This command operates only on graphic display platforms supporting the /SEG command. After executing ANDYNA, you can replay the animated sequence by issuing the ANIM command.

The command functions only in the postprocessor.

Utility Menu >PlotCtrls >Animate >Dynamic Results

Saves or resumes an animation sequence to or from a file.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Label type.

SAVE - Save the current animation to a file.

RESUME - Resume an animation from a file.

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

File name extension (eight characters maximum). Defaults to ANIM if you specify no file name.

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

This command saves an animation to a file from local terminal segments or resumes an animation from a file to local terminal segments. See the /SEG command for details on segment storage. See the ANCNTR macro for a convenient method of storing graphics frames in terminal memory segments. This command is device dependent and is valid in any processor.

Utility Menu >PlotCtrls >Animate >Restore Animation

Utility Menu >PlotCtrls >Animate >Save Animation

Produces an animated sequence of particle flow in a flowing fluid or a charged particle traveling in an electric or magnetic field.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of frames captured (defaults to 5).

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Non-UI mode only.

Total Trace Time (seconds) (defaults to 0, which is the full flow trace).

Particle spacing in seconds (defaults to 0).

Particle size (defaults to 0, which is a line).

Particle length fraction (defaults to .1).

ANFLOW invokes an ANSYS macro which produces an animation of particle flow in a flowing fluid or charged particle motion in an electric or magnetic field by the last plot action command (i.e., PLTRAC). This command is only operational on graphic display platforms supporting the /SEG command. After executing ANFLOW, you can replay the animated sequence by issuing the ANIM command. This command is functional only in the PostProcessor.

The TIME option lets you set the time interval of forward travel for the trace. The SPACING option is used to define the particle spacing in seconds from adjacent particles in the stream line. The SIZE variable sets the radius of the particle. The LENGTH variable is used to define the particle length fraction. By default, the LENGTH is set to .1, which means the particle occupies 10% of the flow region and the other 90% is a color-code line. The SPACING and LENGTH variables only make sense when the SIZE variable is non-zero (i.e., the particle is bigger than the line).

Utility Menu >PlotCtrls >Animate >Particle Flow

Rotates the display about an axis.

GRAPHICS:Views

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Angle (degrees) for changing display orientation (positive, counter-clockwise about specified axis).

Rotation axis: XS, YS, or ZS (default) for the screen axes; XM, YM, or ZM for the global Cartesian model axes. ZS is normal to the screen; all axes pass through the focus point.

Cumulative rotation key:

0 - Do not use cumulative successive rotations.

1 - Use cumulative rotations. Rotations are relative to the previous rotation. View settings (/VIEW) are recalculated.

Default orientation is YS vertical.

This command is valid in any processor.

Utility Menu >PlotCtrls >Pan, Zoom, Rotate

Utility Menu >PlotCtrls >View Settings >Angle of Rotation

Displays graphics data in animated form.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of cycles associated with the animation (defaults to 5 in non-GUI mode only)

Animation mode:

0 - Continuous animation cycle (forward-reverse-forward-etc.) (default).

1 - Discontinuous animation cycle (forward-reset-forward-etc.).

Time delay (seconds) between animation frames (defaults to 0.1 seconds).

Displays graphics data stored in local terminal segments in animated form. See the /SEG command for details on segment storage. See the ANCNTR macro for a convenient method of storing graphics frames in terminal memory segments. This command is device-dependent.

This command is valid in any processor.

Utility Menu >PlotCtrls >Animate >Replay Animation

Utility Menu >PlotCtrls >Animate >Restore Animation

Produces an animated sequence of an isosurface.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of frames captures (defaults to 9).

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

ANISOS involves an ANSYS macro which produces an animation of an isosurface of the last plot action command (for example, PLNSOL,S,EQV). The ANISOS command operates only on graphic display platforms supporting the /SEG command. After executing ANISOS, you can replay the animated sequence by issuing the ANIM command.

This command functions only in the postprocessor.

Utility Menu >PlotCtrls >Animate >Isosurfaces

Produces an animated sequence of a mode shape.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of frames captures (defaults to 5).

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

Acceleration type;

0 - Linear acceleration.

1 - Sinusoidal acceleration.

ANMODE involves an ANSYS macro which produces an animation of mode shape of the last plot action command (for example, PLDISP). The ANMODE command operates only on graphic display platforms supporting the /SEG command. After executing ANMODE, you can replay the animated sequence by issuing the ANIM command.

This command functions only in the postprocessor.

Utility Menu >PlotCtrls >Animate >Mode Shape

Activates graphics for annotating displays (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Annotation control key:

OFF - Turns off annotation for each subsequent display (default).

ON - Turns on annotation for each subsequent display.

DELE - Deletes all annotation.

SAVE - Saves annotation on a file. Use VAL1 for file name (defaults to Jobname) and VAL2 for the extension (defaults to ANO).

SCALE - Sets annotation scale factor (direct input only). Use VAL1 for value (0.1 to 10.0) (defaults to 1.0).

XORIG - Sets the annotation x origin (direct input only). Use VAL1 for value (-3.0 to 3.0).

YORIG - Sets annotation y origin (direct input only). Use VAL1 for value (-3.0 to 3.0).

SNAP - Sets annotation snap (menu button input only). Use VAL1 for value (0.002 to 0.2) (defaults to 0.002).

STAT - Displays current annotation status.

DEFA - Sets annotation specifications to the default values.

REFR - Redisplays annotation graphics.

Value (or file name) as noted with label above.

Value (or file name extension) as noted with label above.

This is a command generated by the GUI and will appear in the log file (Jobname.LOG) if annotation is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

/ANNOT activates annotation graphics for adding annotation to displays. Commands representing the annotation instructions are automatically created by the annotation functions in the GUI and written to Jobname.LOG. The annotation commands are /ANNOT, /ANUM, /TLABEL, /LINE, /LARC, /LSYMBOL, /POLYGON, /PMORE, /PCIRCLE, /PWEDGE, /TSPEC, /LSPEC and /PSPEC. Annotation graphics are relative to the full Graphics Window and are not affected by ANSYS window-specific commands (/WINDOW, /VIEW, etc.).

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Reorients area normals.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Area number having the normal direction that the reoriented areas are to match.

Indicates whether you want to change the normal direction of the existing elements on the reoriented area(s) so that they are consistent with each area's new normal direction.

0 - Make the normal direction of existing elements on the reoriented area(s) consistent with each area's new normal direction (default).

1 - Do not change the normal direction of existing elements on the reoriented area(s).

Reorients areas so that their normals are consistent with that of a specified area.

If any of the areas have inner loops, the ANORM command will consider the inner loops when it reorients the area normals.

You cannot use the ANORM command to change the normal direction of any element that has a body or surface load. We recommend that you apply all of your loads only after ensuring that the element normal directions are acceptable.

Real constants (such as non-uniform shell thickness and tapered beam constants) may be invalidated by an element reversal.

See Chapter 8 of the ANSYS Modeling and Meshing Guide for more information.

Main Menu >Preprocessor >Move / Modify >Area Normals

Produces a sequential contour animation over a range of time.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of frame captures (defaults to 5).

Time delay during animation (defaults to 0.1 seconds).

Number of animation cycles (defaults to 5). Available in non-UI mode only.

Auto-scales contour values, based on the overall subset range of values. The auto-scaling option defaults to 0, no auto-scaling.

The results data to be used for the animation sequence. This can be:

0 - Current load step data (default).

1 - Range of load step data.

2 - Range of time data.

The range minimum value. If left blank defaults to the first data point.

The range maximum value. If left blank defaults to the last data point.

The ANTIME command operates only on graphic display platforms supporting the /SEG command. It uses an ANSYS macro to produce an animation of contour values for the last plot action command (for example, PLDISP). After executing ANTIME, the ANIM command will replay the animated sequence.

This command functions only in the postprocessor.

Utility Menu >PlotCtrls >Animate >Animate Over Time

Specifies the analysis type and restart status.

SOLUTION:AnalysisOptions

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

Analysis type (defaults to the previously specified analysis type, or to STATIC if none specified):

STATIC - Perform a static analysis. Valid for all degrees of freedom.

BUCKLE - Perform a buckling analysis. Implies that a previous static solution was performed with prestress effects calculated [PSTRES,ON]. Valid for structural degrees of freedom only.

MODAL - Perform a modal analysis. Valid for structural and fluid degrees of freedom.

HARMIC - Perform a harmonic analysis. Valid for structural, fluid, magnetic, and electrical degrees of freedom.

TRANS - Perform a transient analysis. Valid for all degrees of freedom.

SUBSTR - Perform a substructure analysis. Valid for all degrees of freedom.

SPECTR - Perform a spectrum analysis. Implies that a previous modal analysis was performed. Valid for structural degrees of freedom only.

Specifies the status of the analysis (new or restart):

NEW - Specifies a new analysis (default).

REST - Specifies a restart of a previous analysis. Valid only for static, harmonic (2-D magnetic only), full transient, and substructure analyses.

Notes

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

This command is also valid in PREP7.

Only Antype=STATIC, BUCKLE, MODAL, HARMIC, TRANS, or SPECTR is allowed in ANSYS/LinearPlus. Only Antype=STATIC or TRANS is allowed in ANSYS/Thermal. Only Antype=STATIC, HARMIC, or TRANS is allowed in ANSYS/Emag 3-D and ANSYS/Emag 2-D.

Main Menu >Preprocessor >Loads >New Analysis

Main Menu >Preprocessor >Loads >Restart

Main Menu >Solution >New Analysis

Main Menu >Solution >Restart

Specifies the annotation number, type, and hot spot (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Annotation number. ANSYS automatically assigns the lowest available number. You cannot assign a higher number if a lower number is available; ANSYS will substitute the lowest available number in place of any user-specified higher number.

Annotation internal type number. If TYPE=DELE, delete annotation NUM.

1 - Text

2 - Block text (not available in GUI)

3 - Dimensions

4 - Lines

5 - Rectangles

6 - Circles

7 - Polygons

8 - Arcs

9 - Wedges, pies

11 - Symbols

12 - Arrows

X hot spot (-1.0 < X < 2.0). Used for menu button item delete.

Y hot spot (-1.0 < Y < 1.0). Used for menu button item delete.

Notes

This is a command generated by the GUI and will appear in the log file (Jobname.LOG) if annotation is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Generates an area, offset from a given area.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Area from which generated area is to be offset. If NAREA = ALL, offset from all selected areas [ASEL]. If NAREA = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI).

Distance normal to given area at which keypoints for generated area are to be located. Positive normal is determined from the right-hand-rule keypoint order.

Keypoint increment between areas. If zero, the lowest available keypoint numbers are assigned [NUMSTR].

Generates an area (and its corresponding keypoints and lines) offset from a given area. The direction of the offset varies with the given area normal. End slopes of the generated lines remain the same as those of the given pattern. Area and line numbers are automatically assigned, beginning with the lowest available values [NUMSTR].

Main Menu >Preprocessor >Create >Arbitrary >By Offset

Overlaps areas.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of areas to be operated on. If NA1 = ALL, use all selected areas and ignore NA2 to NA9. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1.

Generates new areas which encompass the geometry of all the input areas. The new areas are defined by the regions of intersection of the input areas, and by the complementary (non-intersecting) regions. See Chapter 5 of the ANSYS Modeling and Meshing Guide for an illustration. This operation is only valid when the region of intersection is an area. See the BOPTN command for an explanation of the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Overlap >Areas

Displays the selected areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Displays areas from NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL (default), NA2 and NINC are ignored and all selected areas [ASEL] are displayed.

Degeneracy marker:

<blank> - No degeneracy marker is used (default).

DEGE - A red star is placed on keypoints at degeneracies (see the ANSYS Modeling and Meshing Guide ). Not available if /FACET,WIRE is set.

Scale factor for the size of the degeneracy-marker star. The scale is the size in window space (-1 to 1 in both directions) (defaults to .075).

This command is valid in any processor. The degree of tessellation used to plot the selected areas is set through the /FACET command.

Main Menu >Preprocessor >Check Geom >Show Degeneracy >Plot Degen Areas

Main Menu >Preprocessor >Operate >Show Degeneracy >Plot Degen Areas

Utility Menu >Plot >Areas

Utility Menu >Plot >Specified Entities >Areas

Reads data from the results file and appends it to the database.

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. If FIRST, ignore SBSTEP and TIME and read the first data set. If LAST, ignore SBSTEP and TIME and read the last data set. If NEXT, ignore SBSTEP and TIME and read the next data set. If already at the last data set, the next set is the first data set. If NEAR, ignore SBSTEP and read the data set nearest to TIME. If TIME is blank, read the first data set. If LIST, scan the results file to produce a summary of each load step (FACT, KIMG, TIME and ANGLE are ignored).

Substep number (within LSTEP) (defaults to last substep of load step). For the Buckling (ANTYPE=BUCKLE) or Modal (ANTYPE=MODAL) analysis, the substep corresponds to the mode number (defaults to first mode). If LSTEP=LIST, SBSTEP=0 or 1 will list the basic load step information; SBSTEP=2 will also list the load step title, and label the imaginary data sets if they exist.

Scale factor applied to data read from the file. If zero (or blank), a value of 1.0 is used. Harmonic velocities or accelerations may be calculated from the displacement results from a 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.

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 is NEAR, read the data set nearest to TIME. If both LSTEP and SBSTEP are zero (or blank), read data set at time = TIME. 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 is used.

Circumferential location (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.

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 APPEND,LIST. To determine if data sets are real or imaginary, issue APPEND,LIST,2 which labels imaginary data sets.

Reads a data set from the results file and appends it to the existing data in the database for the selected model only. The existing database is not cleared (or overwritten in total), allowing the requested results data to be merged into the database. Various operations may also be performed during the read operation. The database must have the model geometry available (or used the RESUME command before the APPEND command to restore the geometry from File.DB).

Main Menu >General Postproc >By Load Step

Main Menu >General Postproc >By Set Number

Main Menu >General Postproc >By Time/Freq

Partitions areas.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of areas to be operated on. If NA1 = ALL, NA2 to NA9 are ignored and all selected areas are used. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may be substituted for NA1.

Partitions areas that intersect. This command is similar to the combined functionality of the ASBA and AOVLAP commands. If the intersection of two or more areas is an area (i.e., planar), new areas will be created with boundaries that conform to the area of intersection and to the boundaries of the non-intersecting portions of the input areas [AOVLAP]. If the intersection is a line (i.e., not planar), the areas will be subtracted, or divided, along the line(s) of intersection [ASBA]. Both types of intersection can occur during a single APTN operation. Areas that do not intersect will not be modified. See the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for an explanation of the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Partition >Areas

Activates the arc-length method.

SOLUTION:NonlinearOptions

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

Arc-length key:

OFF - Do not use the arc-length method (default).

ON - Use the arc-length method.

Maximum multiplier of the reference arc-length radius (default = 10).

Minimum multiplier of the reference arc-length radius (default = 1/1000).

Activates the arc-length method and sets the minimum and maximum multipliers for the arc-length radius. The reference arc-length radius is calculated from the load or displacement increment of the first iteration of the first substep. This increment is determined by the following formula:

where NSBSTP is the number of substeps specified on the NSUBST command.

The factors MAXARC and MINARC are used to define the limits of the arc-length radius by using the following formulas:

In each subsequent substep, a new arc-length radius is first calculated based on the arc-length radius of the previous substep and the solution behavior. Next, the newly calculated arc-length radius is further modified so that it falls between the range of the upper limit and lower limit. If the solution does not converge even when using the lower limit of the arc-length radius, the solution will terminate.

These values, together with the reference arc-length radius, define the limit for the new arc-length radius.

ARCLEN must be turned OFF for any load step without an applied load or displacement.

Main Menu >Preprocessor >Loads >Nonlinear >Arc-Length Opts

Main Menu >Solution >Nonlinear >Arc-Length Opts

Collapses specified area to a specified line segment (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

The ID of the area to collapse.

The ID of a line belonging to AREA; only the specified line will remain after the area is collapsed.

Use this command to simplify the geometry of a model imported from a CAD file (this is a geometry "clean-up" tool). This tool is available only for models imported from CAD files.

If AREA has any attached loads or boundary conditions, these must be reattached after the collapse operation (Default IGES option).

Main Menu >Preprocessor >Simplify >Collapse Areas

Controls termination of the arc-length solution.

SOLUTION:NonlinearOptions

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

Specifies the basis of solution termination:

OFF - Does not use ARCTRM to terminate analysis (default).

L - Terminates the analysis if the first limit point has been reached. The first limit point is that point in the response history when the tangent stiffness matrix becomes singular (i.e., the point at which the structure becomes unstable). If Lab=L, arguments VAL, NODE, DOF are ignored.

U - Terminates the analysis when the displacement first equals or exceeds the maximum desired value.

Maximum desired displacement (absolute value). Valid only if Lab=U. The analysis terminates whenever the calculated displacement first equals or exceeds this value. For rotational degrees of freedom, VAL must be in radians (not degrees).

Node number corresponding to displacement used to compare with displacement specified by VAL. If blank, the maximum displacement will be used. Valid only if Lab=U.

Valid degree of freedom label for nodal displacement specified by NODE. Valid labels are UX, UY, UZ, ROTX, ROTY, ROTZ. Valid only if NODE>0 and Lab=U.

It can be convenient to use this command to terminate the analysis when the first limit point is reached. In addition, the NCNV command should be used to limit the maximum number of iterations. If the ARCTRM command is not used, and the applied load is so large that the solution path can never reach that load, the arc-length solution will continue to run until a CPU time limit or a "maximum number of iterations" is reached.

Main Menu >Preprocessor >Loads >Nonlinear >Arc-Length Opts

Main Menu >Solution >Nonlinear >Arc-Length Opts

Detaches areas from neighboring geometrical entities (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

Detach areas from AREA1 to AREA2 (defaults to AREA1) in steps of AINC (defaults to 1).

Use this command to detach non-manifold areas from their neighboring geometric entities. This command is available only for repairing the geometry of models imported from CAD systems (Default IGES option).

Main Menu >Preprocessor >Geom Repair >Detach Areas

Specifies "Areas" as the subsequent status topic.

PREP7:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

This command cannot be accessed directly in the menu.

Refines the mesh around specified areas.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Areas (NA1 to NA2 in increments of NINC) around which the mesh is to be refined. NA2 defaults to NA1, and NINC defaults to 1. If NA1=ALL, NA2 and NINC are ignored and all selected areas are used for refinement. If NA1=P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Amount of refinement to be done. Specify the value of LEVEL as an integer from 1 to 5, where a value of 1 provides minimal refinement, and a value of 5 provides maximum refinement (defaults to 1).

Depth of mesh refinement in terms of the number of elements outward from the indicated areas (defaults to 1).

Type of postprocessing to be done after element splitting, in order to improve element quality:

OFF - No postprocessing will be done.

SMOOTH - Smoothing will be done. Node locations may change.

CLEAN - Smoothing and cleanup will be done. Existing elements may be deleted, and node locations may change (default).

Flag indicating whether quadrilateral elements must be retained in the refinement of an all-quadrilateral mesh. (The ANSYS program ignores the RETAIN argument when you are refining anything other than a quadrilateral mesh.)

ON - The final mesh will be composed entirely of quadrilateral elements, regardless of the element quality (default).

OFF - The final mesh may include some triangular elements in order to maintain element quality and provide transitioning.

AREFINE performs local mesh refinement around the specified areas. By default, the indicated elements are split to create new elements with 1/2 the edge length of the original elements (LEVEL=1).

AREFINE refines all area elements and tetrahedral volume elements that are adjacent to the specified areas. Any volume elements that are adjacent to the specified areas, but are not tetrahedra (for example, hexahedra, wedges, and pyramids), are not refined.

You cannot use mesh refinement on a solid model that contains initial conditions at nodes [IC], coupled nodes [CP family of commands], constraint equations [CE family of commands], or boundary conditions or loads applied directly to any of its nodes or elements. This applies to nodes and elements anywhere in the model, not just in the region where you want to request mesh refinement. See Chapter 8 of the ANSYS Modeling and Meshing Guide for additional restrictions on mesh refinement.

Main Menu >Preprocessor >Modify Mesh >Areas

Reverses the normal of an area, regardless of its connectivity or mesh status.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Area number of the area whose normal is to be reversed. If ANUM=ALL, the normals of all selected areas will be reversed. If ANUM=P, graphical picking is enabled. A component name may also be substituted for ANUM.

Indicates whether you want to change the normal direction of the existing elements on the reversed area(s) so that they are consistent with each area's new normal direction.

0 - Make the normal direction of existing elements on the reversed area(s) consistent with each area's new normal direction (default).

1 - Do not change the normal direction of existing elements on the reversed area(s).

You cannot use the AREVERSE command to change the normal direction of any element that has a body or surface load. We recommend that you apply all of your loads only after ensuring that the element normal directions are acceptable.

Real constants (such as non-uniform shell thickness and tapered beam constants) may be invalidated by an element reversal.

See Chapter 8 of the ANSYS Modeling and Meshing Guide for more information.

Main Menu >Preprocessor >Move / Modify >Reverse Normals >of Areas

Creates an area based on a set of singly-connected lines (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

List of lines that define the new area. If LN1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). If LN1 = ALL, all selected lines will be checked for possible closure and all open areas will be filled with lines (lines will be added) that form closed loops.

The ARFILL command creates an area based on the boundary defined by a set of singly-connected lines. No lines in the selected set can be connected to two areas. The area created is the minimum surface defined by the boundary line set.

This tool is available only for models imported from CAD files (Default IGES option).

Main Menu >Preprocessor >Geom Repair >Fill Areas

Merges two or more singly-connected adjacent areas (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

List of areas that define the set of areas to merge. If A1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). If A1 = ALL, all selected areas will be merged and all remaining arguments are ignored.

The ARMERGE command can concatenate more than two adjacent areas; however, for best results you should limit each merge to two areas. Also, you should restrict merge operations to areas that are clearly simple extensions of each other.

If the areas specified in the list have any attached loads or boundary conditions, these will be removed and must be reattached after the merge operation. If the merge operation would result in abnormal parameterization, the command will fail.

Use this command to simplify the geometry of a model imported from a CAD file (this is a geometry "clean-up" tool). This tool is available only for models imported from CAD files (Default IGES option)..

Main Menu >Preprocessor >Simplify >Merge Areas

Generates cylindrical areas by rotating a line pattern about an axis.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

List of lines in the pattern to be rotated (6 maximum if using keyboard entry of NL1 to NL6). The lines must lie in the plane of the axis of rotation. If NL1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). If NL1 = ALL, all selected lines will define the pattern to be rotated. A component name may also be substituted for NL1.

Keypoints defining the axis about which the line pattern is to be rotated.

Arc length (in degrees). Positive follows right-hand rule about PAX1-PAX2 vector. Defaults to 360°.

Number of areas (8 maximum) around circumference. Defaults to minimum number required for 90°-maximum arcs, i.e., 4 for 360°, 3 for 270°, etc.

Generates cylindrical areas (and their corresponding keypoints and lines) by rotating a line pattern (and its associated keypoint pattern) about an axis. Keypoint patterns are generated at regular angular locations, based on a maximum spacing of 90°. Line patterns are generated at the keypoint patterns. Arc lines are also generated to connect the keypoints circumferentially. Keypoint, line, and area numbers are automatically assigned, beginning with the lowest available values [NUMSTR]. Adjacent lines use a common keypoint. Adjacent areas use a common line.

Main Menu >Preprocessor >Operate >Extrude / Sweep >About Axis

Generates a scaled set of areas from a pattern of areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Set of areas, NA1 to NA2 in steps of NINC, that defines the pattern to be scaled. NA2 defaults to NA1, NINC defaults to 1. If NA1=ALL, NA2 and NINC are ignored and the pattern is defined by all selected areas. If NA1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Scale factors to be applied to the X, Y, and Z keypoint coordinates in the active coordinate system. (RR, R, RZ for cylindrical; RR, R, R for spherical). Note that the R and R scale factors are interpreted as angular offsets. For example, if CSYS=1, RX,RY,RZ input of (1.5,10,3) would scale the specified keypoints 1.5 times in the radial and 3 times in the Z direction, while adding an offset of 10 degrees to the keypoints. Zero, blank, or negative scale factor values are assumed to be 1.0. Zero or blank angular offsets have no effect.

Increment to be applied to keypoint numbers for generated set. If zero, the lowest available keypoint numbers will be assigned [NUMSTR].

Specifies whether nodes and elements are also to be generated:

0 - Nodes and elements associated with the original areas will be generated (scaled) if they exist.

1 - Nodes and elements will not be generated.

Specifies whether areas will be moved or newly defined:

0 - Additional areas will be generated.

1 - Original areas will be moved to new position (KINC and NOELEM are ignored). Use only if the old areas are no longer needed at their original positions. Corresponding meshed items are also moved if not needed at their original position.

Generates a scaled set of areas (and their corresponding keypoints, lines, and mesh) from a pattern of areas. The MAT, TYPE, REAL, and ESYS attributes are based on the areas in the pattern and not the current settings. Scaling is done in the active coordinate system. Areas in the pattern could have been generated in any coordinate system. However, solid modeling in a toroidal coordinate system is not recommended.

Main Menu >Preprocessor >Operate >Scale >Areas

Splits an area between two keypoints (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

The ID for the area to be split.

The ID of an existing keypoint within the area. This will be the starting keypoint for the boundary line. You cannot specify a keypoint for KP1 that is already connected to KP2.

The ID of an existing keypoint within the area that will become the end point for the boundary line.

Label to activate user-definable area tolerance. If TOL=TIGHT user-definable tolerances are used and the tolerance factor is specified by Factor.

The user-definable tolerance factor. Valid entries are integer values from 1 (the tightest setting) to 10 (the loosest and default setting). This is only used when TOL=TIGHT.

The ARSPLIT command creates a new boundary line between the specified keypoints, splitting the specified area into two areas sharing that boundary. The command will allow you to specify a keypoint pair such that the resultant boundary line will fall outside of the confines of the specified area; make sure that the keypoints you select do not create such a line.

Use this command to simplify the geometry of a model imported from a CAD file (this is a geometry "clean-up" tool). This tool is available only for models imported from CAD files (Default IGES option).

Normally, the default area tolerance is adequate for the ARSPLIT command. However, occasionally when attempting to split an extremely narrow area the ARSPLIT command can fail due to what the error message calls "numerical inadequacies" and you'll be prompted to try another location for the split. You may be able to split the area at the selected keypoints by tightening the area tolerance. To do this, issue the ARSPLIT command with TOL=TIGHT and Factor as an integer between 1 (the default, and loosest tolerance) and 10. You should remove any areas that are split through these arguments. If such areas remain, they may cause Boolean operations involving those areas to fail.

Main Menu >Preprocessor >Simplify >Split areas

Generates areas from an area pattern by symmetry reflection.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Symmetry key:

X - X symmetry (default).

Y - Y symmetry.

Z - Z symmetry.

Reflect areas from pattern beginning with NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL, NA2 and NINC are ignored and the pattern is all selected areas [ASEL]. If Ncomp = P, use graphical picking to specify areas and ignore NL2 and NINC. A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Keypoint increment between sets. If zero, the lowest available keypoint numbers are assigned [NUMSTR].

Specifies whether nodes and elements are also to be generated:

0 - Generate nodes and elements associated with the original areas, if they exist.

1 - Do not generate nodes and elements.

Specifies whether areas will be moved or newly defined:

0 - Generate additional areas.

1 - Move original areas to new position retaining the same keypoint numbers (KINC and NOELEM are ignored). Valid only if the old areas are no longer needed at their original positions. Corresponding meshed items are also moved if not needed at their original position.

Generates a reflected set of areas (and their corresponding keypoints, lines and mesh) from a given area pattern by a symmetry reflection (see analogous node symmetry command, NSYM). The MAT, TYPE, REAL, and ESYS attributes are based upon the areas in the pattern and not upon the current settings. Reflection is done in the active coordinate system by changing a particular coordinate sign. The active coordinate system must be a Cartesian system. Areas in the pattern may have been generated in any coordinate system. However, solid modeling in a toroidal coordinate system is not recommended. Areas are generated as described in the AGEN command.

Main Menu >Preprocessor >Reflect >Areas

Subtracts areas from areas.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Area (or areas, if picking is used) to be subtracted from. If ALL, use all selected areas. Areas specified in this argument are not available for use in the NA2 argument. If P, graphical picking is enabled (valid only in the GUI) and remaining fields are ignored. A component name may also be substituted for NA1.

Area (or areas, if picking is used) to subtract. If ALL, use all selected areas (except those included in the NA1 argument). A component name may also be substituted for NA2.

Behavior if the intersection of the NA1 areas and the NA2 areas is a line or lines:

<blank> - The resulting areas will share line(s) where they touch.

SEPO - The resulting areas will have separate, but coincident line(s) where they touch.

Specifies whether NA1 areas are to be deleted:

<blank> - Use the setting of BKEEP on the BOPTN command.

DELETE - Delete NA1 areas after ASBA operation (override BOPTN command settings).

KEEP - Keep NA1 areas after ASBA operation (override BOPTN command settings).

Specifies whether NA2 areas are to be deleted:

<blank> - Use the setting of BKEEP on the BOPTN command.

DELETE - Delete NA2 areas after ASBA operation (override BOPTN command settings).

KEEP - Keep NA2 areas after ASBA operation (override BOPTN command settings).

Generates new areas by subtracting the regions common to both NA1 and NA2 areas (the intersection) from the NA1 areas. The intersection can be an area(s) or line(s). If the intersection is a line and SEPO is blank, the NA1 area is divided at the line and the resulting areas will be connected, sharing a common line where they touch. If SEPO is set to SEPO, NA1 is divided into two unconnected areas with separate lines where they touch. See Chapter 5 of the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for an explanation of the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated. ASBA,ALL,ALL will have no effect since all the areas (in NA1) will be unavailable as NA2 areas.

Main Menu >Preprocessor >Operate >Divide >Area by Area

Main Menu >Preprocessor >Operate >Divide >With Options >Area by Area

Main Menu >Preprocessor >Operate >Subtract >Areas

Main Menu >Preprocessor >Operate >Subtract >With Options >Areas

Subtracts lines from areas.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Area (or areas, if picking is used) to be subtracted from. If ALL, use all selected areas. If P, graphical picking is enabled (valid only in the GUI) and remaining fields are ignored. A component name may also be substituted for NA.

Line (or lines, if picking is used) to subtract. If ALL, use all selected lines. A component name may also be substituted for NL.

Specifies whether NA areas are to be deleted:

<blank> - Use the setting of BKEEP on the BOPTN command.

DELETE - Delete NA areas after ASBL operation (override BOPTN command settings).

KEEP - Keep NA areas after ASBL operation (override BOPTN command settings).

Specifies whether NL lines are to be deleted:

<blank> - Use the setting of BKEEP on the BOPTN command.

DELETE - Delete NL lines after ASBL operation (override BOPTN command settings).

KEEP - Keep NL lines after ASBL operation (override BOPTN command settings).

Generates new areas by subtracting the regions common to both the areas and lines (the intersection) from the NA areas. The intersection will be a line(s). See Chapter 5 of the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for an explanation of the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Divide >Area by Line

Main Menu >Preprocessor >Operate >Divide >With Options >Area by Line

Subtracts volumes from areas.

PREP7:Booleans

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

Area (or areas, if picking is used) to be subtracted from. If ALL, use all selected areas. If P, graphical picking is enabled (valid only in the GUI) and remaining fields are ignored. A component name may also be substituted for NA.

Volume (or volumes, if picking is used) to subtract. If ALL, use all selected volumes. A component name may also be substituted for NV.

Behavior if the intersection of the areas and the volumes is a line or lines:

<blank> - The resulting areas will share line(s) where they touch.

SEPO - The resulting areas will have separate, but coincident line(s) where they touch.

Specifies whether NA areas are to be deleted:

<blank> - Use the setting of BKEEP on the BOPTN command.

DELETE - Delete NA areas after ASBV operation (override BOPTN command settings).

KEEP - Keep NA areas after ASBV operation (override BOPTN command settings).

Specifies whether NV volumes are to be deleted:

<blank> - Use the setting of BKEEP on the BOPTN command.

DELETE - Delete volumes after ASBV operation (override BOPTN command settings).

KEEP - Keep volumes after ASBV operation (override BOPTN command settings).

Generates new areas by subtracting the regions common to both NA areas and NV volumes (the intersection) from the NA areas. The intersection can be an area(s) or line(s). If the intersection is a line and SEPO is blank, the NA area is divided at the line and the resulting areas will be connected, sharing a common line where they touch. If SEPO is set to SEPO, NA is divided into two unconnected areas with separate lines where they touch. See Chapter 5 of the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for an explanation of the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Area by Volu

Menu Paths

Main Menu >Preprocessor >Operate >Divide >Area by Volume

Main Menu >Preprocessor >Operate >Divide >With Options >Area by Volume

Subtracts the intersection of the working plane from areas (divides areas).

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Area (or areas, if picking is used) to be subtracted from. If NA=ALL, use all selected areas. If NA=P, graphical picking is enabled (valid only in the GUI). A component name may also be input for NA.

Behavior of the created boundary.

<blank> - The resulting areas will share line(s) where they touch.

SEPO - The resulting areas will have separate, but coincident line(s).

Specifies whether NA areas are to be deleted.

<blank> - Use the setting of BKEEP on the BOPTN command.

DELETE - Delete NA areas after ASBW operation (override BOPTN command settings).

KEEP - Keep NA areas after ASBW operation (override BOPTN command settings).

Generates new areas by subtracting the intersection of the working plane from the NA areas. The intersection will be a line(s). The working plane must not be in the same plane as the NA areas(s). If SEPO is blank, the NA area is divided at the line and the resulting areas will be connected, sharing a common line where they touch. If SEPO is set to SEPO, NA is divided into two unconnected areas with separate lines. See Chapter 5 of the ANSYS Modeling and Meshing Guide for an illustration. See the BOPTN command for an explanation of the options available to Boolean operations. Element attributes and solid model boundary conditions assigned to the original entities will not be transferred to the new entities generated.

Main Menu >Preprocessor >Operate >Area by WrkPlane

Menu Paths

Main Menu >Preprocessor >Operate >Divide >Area by WrkPlane

Main Menu >Preprocessor >Operate >Divide >With Options >Area by WrkPlane

Selects a subset of areas.

DATABASE:Selecting

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the type of select:

S - Select a new set (default)

R - Reselect a set from the current set.

A - Additionally select a set and extend the current set.

U - Unselect a set from the current set.

ALL - Restore the full set.

NONE - Unselect the full set.

INVE - Invert the current set (selected becomes unselected and vice versa).

STAT - Display the current select status.

The following fields are used only with Type=S,R,A, or U:

Label identifying data. Valid item labels are shown in the table below. Some items also require a component label. If Item=P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). Defaults to AREA.

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

Minimum value of item range. Ranges are area numbers, coordinate values, attribute numbers, etc., as appropriate for the item. A component name (as specified on the CM command) may also be substituted for VMIN (VMAX and VINC are ignored). If Item = MAT, TYPE, REAL, or ESYS and if VMIN is positive, the absolute value of Item is compared against the range for selection; if VMIN is negative, the signed value of Item is compared. See the ALIST command for a discussion of signed attributes.

Maximum value of item range. VMAX defaults to VMIN. If VMAX = VMIN, a tolerance of 0.005 x VMIN is used, or 1.0E-6 if VMIN = 0.0. If VMAX VMIN, a tolerance of 1.0E-8 x (VMAX-VMIN) is used.

Value increment within range. Used only with integer ranges (such as for area numbers). Defaults to 1. VINC cannot be negative.

Specifies whether only areas are to be selected:

0 - Select areas only.

1 - Select areas, as well as keypoints, lines, nodes, and elements associated with selected areas. Valid only with Type=S.

Notes

Selects a subset of areas. For example, to select those areas with area numbers 1 through 7, use ASEL,S,AREA,,1,7. The selected subset is then used when the ALL label is entered (or implied) on other commands, such as ALIST,ALL. Only data identified by area number are selected. Data are flagged as selected and unselected; no data are actually deleted from the database.

If Item=ACCA, the command selects only those areas that were created by concatenation. The KSWP field is processed, but the Comp, VMIN, VMAX, and VINC fields are ignored.

This command is valid in any processor.

Utility Menu >Select >Entities

Prompts the user to input a parameter value.

APDL:Parameters

	Mp Me St DY LP Th E3 E2 FL PP ED

An alphanumeric name used to identify the scalar parameter. See *SET for name restrictions.

Text string to be displayed on the next line as the query (32 characters maximum). Characters having special meaning (such as $ ! ,) should not be included.

Default value assigned to the parameter if the user issues a blank response. May be a number or character string (up to 8 characters enclosed in single quotes). If a default is not assigned, a blank response will delete the parameter.

Intended primarily for use in macros, the command prints the query (after the word "ENTER") on the next line and waits for a response. The response is read from the keyboard, except in batch mode [/BATCH], when the response(s) must be the next-read input line(s). The response may be a number, a character string (up to 8 characters enclosed in single quotes), a parameter (numeric or character) or an expression that evaluates to a number. The scalar parameter is then set to the response value. For example, *ASK,NN,PARAMETER NN will set NN to the value entered on the next line (after the prompt "ENTER PARAMETER NN").

The *ASK command is not written to File.LOG, but the responses are written there as follows: If *ASK is contained in a macro, the response(s) (only) is written to File.LOG on the line(s) following the macro name. If not contained in a macro, the response is written to File.LOG as a parameter assignment (i.e., Par="user-response").

If used within a do-loop that is executed interactively, *ASK should be contained in a macro. If not contained in a macro, *ASK will still query the user as intended, but the resulting log file will not reproduce the effects of the original run.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Generates an area by "skinning" a surface through guiding lines.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

The first guiding line forming the skinned area. If NL1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NL1. If NL1 is negative, the line beginnings and ends will be used to direct the skinning of the remaining lines (see "Changing the ASKIN Algorithm" below).

The additional guiding lines for the skinned area (up to 9 total lines, including NL1, if using keyboard entry). If negative (and NL1 is negative), the line beginning and end will be temporarily interchanged for the skinning operation (see "Changing the ASKIN Algorithm" below).

Generates an area by "skinning" a surface through specified guiding lines. The lines act as a set of "ribs" over which a surface is "stretched." Two opposite edges of the area are framed by the first (NL1) and last (NLn) guiding lines specified. The other two edges of the area are framed by splines-fit lines which the program automatically generates through the ends of all guiding lines. The interior of the area is shaped by the interior guiding lines. Once the area has been created, only the four edge lines will be attached to it. In rare cases, it may be necessary to change the default algorithm used by the ASKIN command (see "Changing the ASKIN Algorithm" below).

When skinning from one guiding line to the next, the program can create the transition area in one of two ways: one more spiraled and one less spiraled ("flatter"). By default, the program attempts to produce the flatter transition, instead of the more spiraled transition. This algorithm can be changed by inputting NL1 as a negative number, in which case the program connects all the keypoints at the line "beginnings" (/PSYMB,LDIR command) as one edge of the area, and all the line "ends" as the opposite edge, irrespective of the amount of spiraling produced in each transition area.

To further control the geometry of the area (if NL1 is negative), the beginning and end of any specified line (other than NL1) can be temporarily interchanged (for the skinning operation only) by inputting that line number as negative. See Chapter 5 of the ANSYS Modeling and Meshing Guide for an illustration.

Main Menu >Preprocessor >Create >Arbitrary >By Skinning

Selects those areas containing the selected lines.

DATABASE:Selecting

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the type of area select:

S - Select a new set (default).

R - Reselect a set from the current set.

A - Additionally select a set and extend the current set.

U - Unselect a set from the current set.

Specifies whether all contained area lines must be selected [LSEL]:

0 - Select area if any of its lines are in the selected line set.

1 - Select area only if all of its lines are in the selected line set.

This command is valid in any processor.

Utility Menu >Select >Entities

Selects those areas contained in the selected volumes.

DATABASE:Selecting

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

Label identifying the type of area select:

S - Select a new set (default).

R - Reselect a set from the current set.

A - Additionally select a set and extend the current set.

U - Unselect a set from the current set.

This command is valid in any processor.

Utility Menu >Select >Entities

Reassigns a file name to an ANSYS file identifier.

SESSION:Files

	Mp Me St DY LP Th E3 E2 FL PP ED

ANSYS file name identifier. Valid identifiers are: EMAT, ESAV, FULL, REDM, MODE, RDSP, RFRQ, TRI, RST, RTH, RMG, EROT, OSAV, RFL, and SELD. See the ANSYS Basic Analysis Procedures Guide for file descriptions. If blank, list currently reassigned files.

File name (32 characters maximum) to be assigned.

File name extension (8 characters maximum).

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

The reassignment of file names is valid only if it is done before the file is used. All file reassignments are retained (not cleared) even if the database is cleared [/CLEAR] or the jobname is changed [/FILNAME]. Assigned files may be overwritten. If file name arguments (Fname,Ext,Dir) are blank, the default ANSYS assignment is restored. Use SEOPT for SUB files and SEEXP for DSUB files.

This command is valid only at the Begin Level.

Utility Menu >File >ANSYS File Options

Generates an area using the shape of an existing area.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Existing area number whose shape is to be used. If P1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI).

Keypoint defining starting corner of area.

Keypoint defining second corner of area.

Keypoint defining third corner of area.

Keypoint defining fourth corner of area (defaults to P3).

The new area will overlay the old area. Often used when the area to be subdivided consists of a complex shape that was not generated in a single coordinate system. Keypoints and any corresponding lines must lie on the existing area. Missing lines are generated to lie on the given area. The active coordinate system is ignored.

Main Menu >Preprocessor >Create >Arbitrary >Overlaid on Area

Calculates and prints geometry statistics of the selected areas.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Controls the degree of tessellation used in the calculation of area properties. If LAB = DEFAULT, area calculations will use the degree of tessellation set through the /FACET command. If LAB = FINE, area calculations are based on a finer tessellation.

Calculates and prints geometry statistics (area, centroid location, moments of inertia, volume, etc.) associated with the selected areas. Geometry items are reported in the global Cartesian coordinate system. A unit density (and thickness) is assumed unless the areas have a material (and real constant) association via the AATT command. Items that are calculated by ASUM and later retrieved by a *GET or *VGET command are valid only if the model is not modified after the ASUM command is issued.

Setting a finer degree of tessellation will provide area calculations with greater accuracy, especially for thin, hollow models. However, using a finer degree of tessellation requires longer processing.

For very narrow (sliver) areas, such that the ratio of the minimum to the maximum dimension is less than 0.01, the ASUM command can provide erroneous area information. To ensure that such calculations are accurate, make certain that you subdivide such areas so that the ratio of the minimum to the maximum is at least 0.05.

Main Menu >Preprocessor >Operate >Calc Geom Items >Of Areas

Forms the arctangent of a complex variable.

POST26:Operations

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

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

Reference number of the complex 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). Usually FACTA should be set to 1. FACTA may affect the position of the angle by a multiple of , resulting in a quadrant change.

Forms the arctangent of a complex variable according to the operation:

where a and b are the real and imaginary parts, respectively, of the complex variable IA (which is of the form a+ib). The arctangent represents the phase angle (in radians), and is valid only for a harmonic analysis (ANTYPE = HARMIC).

Since the scaling factor is applied uniformly to b/a, applying any positive or negative scaling factor will not affect the size of the phase angle, with the exception that a negative scaling factor will change the results quadrant by . The magnitude of a complex number is still obtained through the ABS command. See Section 19.10 of the ANSYS Theory Reference for details.

Main Menu >TimeHist Postpro >Math Operations >Arctangent

Transfers a pattern of areas to another coordinate system.

PREP7:Areas

	Mp Me St DY LP Th E3 E2 FL PP ED

Reference number of coordinate system where the pattern is to be transferred. Transfer occurs from the active coordinate system. The coordinate system type and parameters of KCNTO must be the same as the active system.

Transfer area pattern beginning with NA1 to NA2 (defaults to NA1) in steps of NINC (defaults to 1). If NA1 = ALL, NA2 and NINC are ignored and the pattern is all selected areas [ASEL]. If P1 = P, graphical picking is enabled and all remaining arguments are ignored (valid only in the GUI). A component name may also be substituted for NA1 (NA2 and NINC are ignored).

Keypoint increment between sets. If zero, the lowest available keypoint numbers are assigned [NUMSTR].

Specifies whether elements and nodes are also to be generated:

0 - Generate nodes and elements associated with the original areas, if they exist.

1 - Do not generate nodes and elements.

Specifies whether to redefine the existing areas:

0 - Generate additional areas.

1 - Move original areas to new position retaining the same keypoint numbers (KINC and NOELM are ignored). Valid only if the old areas are no longer needed at their original positions. Corresponding meshed items are also moved if not needed at their original position.

Transfers a pattern of areas (and their corresponding lines, keypoints and mesh) from one coordinate system to another (see analogous node TRANSFER command). The MAT, TYPE, REAL, and ESYS attributes are based upon the areas in the pattern and not upon the current settings. Coordinate systems may be translated and rotated relative to each other. Initial pattern may be generated in any coordinate system. However, solid modeling in a toroidal coordinate system is not recommended. Coordinate and slope values are interpreted in the active coordinate system and are transferred directly. Areas are generated as described in the AGEN command.

Main Menu >Preprocessor >Move / Modify >Transfer Coord >Areas

Specifies "Analysis types" 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 >Analysis Type

Resets the focus and distance specifications to "automatically calculated."

GRAPHICS:Views

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Focus point and distance will be automatically calculated during next display. Settings may still be changed with the /FOCUS and /DIST commands after this command has been issued. See also the /USER command.

This command is valid in any processor.

Utility Menu >PlotCtrls >Pan, Zoom, Rotate

Utility Menu >PlotCtrls >View Settings >Automatic Fit Mode

Specifies whether to use automatic time stepping or load stepping.

SOLUTION:LoadStepOptions

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

Automatic time stepping key:

OFF - Do not use automatic time stepping.

ON - Use automatic time stepping.

Notes

Specifies whether to use automatic time stepping (or load stepping) over this load step. If Key=ON, both time step prediction and time step bisection will be used. Used only if DTIME (specified on the DELTIM command) is less than the time span or conversely, if NSBSTP (on the NSUBST command) is greater than one.

If you run an analysis with SOLCONTROL,ON, but do not issue the AUTOTS command, ANSYS will choose whether or not to use automatic time stepping. The program-chosen option will be recorded on the log file as AUTOTS,-1.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Time/Frequenc >Time - Time Step

Main Menu >Preprocessor >Loads >Time/Frequenc >Time and Substps

Main Menu >Solution >Time/Frequenc >Time - Time Step

Main Menu >Solution >Time/Frequenc >Time and Substps

Enters the binary file dumping processor.

AUX2:BinaryFiles SESSION:ProcessorEntry

	Mp Me St DY LP Th E3 E2 FL PP ED

Enters the binary file dumping processor (ANSYS auxiliary processor AUX2). This processor is used to dump the contents of certain ANSYS binary files for visual examination.

This command is valid only at the Begin Level.

Utility Menu >File >List >Binary Files

Utility Menu >List >Files >Binary Files

Enters the radiation matrix generation processor.

AUX12:RadiationSubstructures SESSION:ProcessorEntry

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

Enters the substructure radiation matrix generation processor (ANSYS auxiliary processor AUX12). This processor is used to calculate radiation view factors and the resulting superelement, which can then be used in a thermal analysis.

This command is valid only at the Begin Level.

Main Menu >Radiation Matrix

Enters the IGES file transfer processor.

AUX15:IGES SESSION:ProcessorEntry

	Mp Me St DY LP Th E3 E2 FL PP ED

Enters the IGES file transfer processor (ANSYS auxiliary processor AUX15), used to read an IGES data file into the ANSYS program.

This command is valid only at the Begin Level.

Utility Menu >File >Import

Specifies how principal and vector sums are to be calculated.

POST1:Controls

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

Averaging key:

0 - Average the component values from the elements at a common node, then calculate the principal or vector sum from the averaged components (default).

1 - Calculate the principal or vector sum values on a per element basis, then average these values from the elements at a common node.

EFFNU

Effective Poisson's ratio used for computing the von Mises equivalent strain (EQV). The default is 0.0.

Selects the method of combining components for certain derived nodal results when two or more elements connect to a common node. The methods apply to the calculations of derived nodal principal stresses, principal strains, and vector sums for selects, sorts, and output [NSEL, NSORT, PRNSOL, PLNSOL, etc.]. Also defines the effective Poisson's ratio used for equivalent strain calculations. See Section 19.12 of the ANSYS Theory Reference.

Main Menu >General Postproc >Element Table >Define Table

Main Menu >General Postproc >List Results >Nodal Solution

Main Menu >General Postproc >Options for Outp

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

Main Menu >General Postproc >Plot Results >Element Solu

Main Menu >General Postproc >Plot Results >Nodal Solu

Utility Menu >List >Results >Nodal Solution

Utility Menu >List >Results >Options

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

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

Specifies how results data will be averaged when PowerGraphics is enabled.

POST1:Controls

	Mp Me St DY LP Th E3 E2 FL PP ED

Averaging key.

1 - Average results at all common subgrid locations.

2 - Average results at all common subgrid locations except where material type [MAT] discontinuities exist.

3 - Average results at all common subgrid locations except where real constant [REAL] discontinuities exist.

4 - Average results at all common subgrid locations except where material type [MAT] or real constant [REAL] discontinuities exist.

Notes

AVRES specifies how results data will be averaged at subgrid locations that are common to 2 or more elements. This command is valid only when PowerGraphics is enabled [/GRAPHICS,POWER]. This command affects nodal solution contour plots [PLNSOL], nodal solution printout [PRNSOL], and subgrid solution results accessed through the Query Results function (under General Postprocessing) in the GUI. AVRES has no effect on the nodal degree of freedom solution values (UX, UY, UZ, TEMP, etc.).

Main Menu >General Postproc >Options for Outp

Utility Menu >List >Results >Options

Labels the X and Y axes on graph displays.

GRAPHICS:Graphs

	Mp Me St DY LP Th E3 E2 FL PP ED

Axis specifier:

X - Apply label to X axis.

Y - Apply label to Y axis.

Axis label (user defined text up to 30 characters long). Leave blank to reestablish the default for Axis axis.

Notes

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Graphs