L

Defines a line between two keypoints.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Keypoint at the beginning of line. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Keypoint at the end of line.

Number of element divisions within this line. Normally this field is not used; specifying divisions with LESIZE, etc. is recommended.

Spacing ratio. Normally this field is not used, as specifying spacing ratios with the LESIZE command is recommended. If positive, SPACE is the nominal ratio of the last division size (at P2) to the first division size (at P1). If the ratio is greater than 1, the division sizes increase from P1 to P2, and if less than 1, they decrease. If SPACE is negative, then jSPACEj is the nominal ratio of the center division size to those at the ends.

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

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

Location of the head of the "slope vector" corresponding to the slope at the P2 end of the line.

Defines a line between two keypoints from P1 to P2. The line shape may be generated as "straight" (in the active coordinate system) or curved. The line shape is invariant with coordinate system after it is generated. Note that solid modeling in a toroidal coordinate system is not recommended. A curved line is limited to 180°. Lines may be redefined only if not yet attached to an area.

Main Menu >Preprocessor >Create >Lines >In Active Coord

Generates a line at an angle with two existing lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the first line to be hit (touched by the end of the new line). If negative, assume P1 (see below) is the second keypoint of the line instead of the first. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Number of the second line to be hit. If negative, assume P3 is the second keypoint of the line instead of the first.

Angle of intersection (usually zero or 180) of generated line with tangent to first line.

Angle of intersection (usually zero or 180) of generated line with tangent to second line.

Number to be assigned to keypoint generated at hit location on first line (defaults to lowest available keypoint number [NUMSTR]).

Number to be assigned to keypoint generated at hit location on second line (defaults to lowest available keypoint number [NUMSTR]).

Generates a straight line (PHIT1-PHIT2) at an angle (ANG1) with an existing line NL1 (P1-P2) and which is also at an angle (ANG2) with another existing line NL2 (P3-P4). If the angles are zero the generated line is tangent to the two lines. The PHIT1 and PHIT2 locations on the lines are automatically calculated. Line P1-P2 becomes P1-PHIT1, P3-P4 becomes P3-PHIT2, and new lines PHIT1-P2, PHIT2-P4, and PHIT1-PHIT2 are generated. Line divisions are set to zero (use LESIZE, etc. to modify).

Main Menu >Preprocessor >Create >Lines >Angle to 2 Lines

Main Menu >Preprocessor >Create >Lines >Norm to 2 Lines

Generates a line tangent to two lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the first line generated line is tangent to. If negative, assume P1 (see below) is the second keypoint of the line instead of the first. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Number of the second line generated line is tangent to. If negative, assume P3 is the second keypoint of the line instead of the first.

Generates a line (P2-P3) tangent at point P2 to line NL1 (P1-P2) and tangent at point P3 to line NL2 (P3-P4).

Main Menu >Preprocessor >Create >Lines >Tan to 2 Lines

Generates a straight line at an angle with a line.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the line to be hit (touched by the end of the new line). If negative, assume P1 (see below) is the second keypoint of the line instead of the first. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Keypoint at which generated line must end.

Angle of intersection of generated line PHIT-P3 with tangent to line P1-P2 at PHIT. If 0 (default), the generated line is tangent to NL1; if 90, the generated line is perpendicular to NL1. ANG can be any value, but is adjusted to the corresponding acute angle with respect to LOCAT. See Notes section for a discussion of accuracy.

Number to be assigned to keypoint generated at hit location (defaults to lowest available keypoint number [NUMSTR]).

Approximate location of PHIT in terms of the ratio of the distance along the line (NL1) to the length of the line. LOCAT can range from 0 to 1. If LOCAT is blank, the point will be located with less speed and accuracy, and an arbitrary location may result.

Generates a straight line (PHIT-P3) at an angle (ANG) with a line NL1 (P1-P2). The location of PHIT on the line is automatically calculated. Line P1-P2 becomes P1-PHIT and new lines PHIT-P2 and PHIT-P3 are generated. Line divisions are set to zero (use LESIZE, etc. to modify).

PHIT is positioned closest to LOCAT for the given angle, ANG. To ensure better performance, it is recommended that LOCAT be input, even if it is 0.

The program uses an iterative procedure to position PHIT. The procedure is not exact, with the result that the actual value of ANG will sometimes differ slightly from the specified value.

Main Menu >Preprocessor >Create >Lines >At angle to line

Main Menu >Preprocessor >Create >Lines >Normal to Line

Creates annotation arcs (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Arc X center location (-1.0 < X < 1.0).

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

Arc radius length.

Starting angle of arc.

Ending angle of arc. The arc is drawn counterclockwise from the starting angle, ANGLE1, to the ending angle, ANGLE2.

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

All arcs are shown on subsequent displays unless the annotation is turned off or deleted. Use the /LSPEC command to set the attributes of the arc.

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Defines a circular arc.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Keypoint at one end of circular arc line. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Keypoint at other end of circular arc line.

Keypoint defining plane of arc and center of curvature side (with positive radius). Must not lie along the straight line from P1 to P2. PC need not be at the center of curvature.

Radius of curvature of the arc. If negative, assume center of curvature side is opposite to that defined by PC. If RAD = <blank>, RAD will be calculated from a curve fit through P1, PC, and P2.

Defines a circular arc line from P1 to P2. The line shape is generated as circular, regardless of the active coordinate system. The line shape is invariant with coordinate system after it is generated.

Main Menu >Preprocessor >Create >Arcs >By End KPs & Rad

Main Menu >Preprocessor >Create >Arcs >Through 3 KPs

Generates the shortest line between two keypoints on an area.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

First keypoint of line to be generated. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Second keypoint of line to be generated.

Area containing P1 and P2, or area to which generated line is to be parallel.

Generates the shortest line between two keypoints, P1 and P2, both of which lie on an area. The generated line will also lie on the area. P1 and P2 may also be equidistant (in global Cartesian space) from the area (and on the same side of the area), in which case a line parallel to the area is generated.

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

Finds the largest (the envelope) of three variables.

POST26:Operations

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

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

Unused fields.

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

Creates a new variable by finding the largest of up to three variables according to the operation:

The comparison is done at each time location, so that the new variable is the "envelope" of the three existing variables.

Main Menu >TimeHist Postpro >Math Operations >Find Maximum

Associates element attributes with the selected, unmeshed lines.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Material number, real constant set number, type number, and coordinate system number to be associated with selected, unmeshed lines.

Beginning and ending orientation keypoints to be associated with selected, unmeshed lines. ANSYS uses the location of these keypoints to determine how to orient beam cross sections during beam meshing. Beam elements may be created along a line with a constant orientation by specifying only one orientation keypoint (KB), or a pre-twisted beam may be created by selecting different orientation keypoints at each end of the line (KB and KE). (For a line bounded by two keypoints (KP1 and KP2), the orientation vector at the beginning of the line extends from KP1 to KB, and the orientation vector at the end of the line extends from KP2 to KE. The orientation vectors are used to compute the orientation nodes of the elements.)

Section identifier to be associated with selected, unmeshed lines. For details, see the description of the SECTYPE and SECNUM commands.

The element attributes specified by the LATT command will be used when the lines are meshed.

Lines subsequently generated from the lines will also have the attributes specified by MAT, REAL, TYPE, ESYS, and SECNUM. If a line does not have these attributes associated with it (by this command) at the time it is meshed, the attributes are obtained from the then current MAT, REAL, TYPE, ESYS, and SECNUM command settings.

In contrast, the values specified by KB and KE apply only to the selected lines; that is, lines subsequently generated from these lines will not share these attributes. Similarly, if a line does not have KB and KE attributes associated with it via the LATT command at the time it is meshed, ANSYS cannot obtain the attributes from elsewhere. See the discussion on beam meshing in Chapter 7 of the ANSYS Modeling and Meshing Guide for more information.

Reissue the LATT command (before lines are meshed) to change the attributes. A zero (or blank) argument removes the corresponding association.

In some cases, ANSYS can proceed with a line meshing operation even when no logical element type has been assigned via LATT,,,TYPE or TYPE. See Chapter 7 of the ANSYS Modeling and Meshing Guide for more information about setting element attributes.

Main Menu >Preprocessor >Define >All Lines

Main Menu >Preprocessor >Define >Picked Lines

Specifies the element layer for which data are to be processed.

POST1:Controls

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

Layer number for layered element types (SHELL91, SOLID46 or SHELL99) with KEYOPT(8)=1. If NUM=FCMAX, use the layer at which the maximum failure criterion occurs. By default, results data are from the bottom of the bottom layer and the top of the top layer.

Notes

Specifies the element layer for which results data are to be listed, plotted, or otherwise processed. Applies to stress and strain data for layered elements SOLID46, SHELL91 and SHELL99. Also applies to body load temperatures for SHELL99. The SHELL command may then be used (with shell elements) to specify a location (TOP, MID, BOT) within the layer for output. Transverse shear stresses for MID are linearly averaged from TOP and BOT, and do not reflect a parabolic distribution.

For the ANSYS/LS-DYNA product, this command works differently than described above. For SHELL163, you must first use EDINT during the solution phase to define the integration points for which you want output data. Be aware that the output location for SHELL163 data is always at the integration point, so "top" and "bottom" refer to the top or bottom integration point, not necessarily the top or bottom surface. For more information, see the ANSYS/LS-DYNA User's Guide.

Main Menu >General Postproc >Options for Outp

Utility Menu >List >Results >Options

Specifies the element layer for which data are to be stored.

POST26:Controls

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

Layer number for layered element types (SHELL91, SOLID46 or SHELL99) with KEYOPT(8)=1. For layered element types with KEYOPT(8)=0, if NUM=FCMAX, use the layer at which the maximum failure criterion occurs.

Notes

Defines the element layer for which results data are to be stored for postprocessing. Applies to stress and strain data for layered elements SOLID46, SHELL91 and SHELL99. Also applies to body load temperatures for SHELL99. The SHELL command may then be used (for shell elements) to specify a location (TOP, MID, BOT) within the layer for selection on the ESOL command. Transverse shear stresses for MID are linearly averaged from TOP and BOT, and do not reflect a parabolic distribution.

For the ANSYS/LS-DYNA product, this command works differently than described above. For SHELL163 and BEAM161, you must first use EDINT during the solution phase to define the integration points for which you want output data. Be aware that the output location for SHELL163 data is always at the integration point, so "top" and "bottom" refer to the top or bottom integration point, not necessarily the top or bottom surface. For more information, see the ANSYS/LS-DYNA User's Guide.

Main Menu >TimeHist Postpro >Define Variables

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

Lists real constants material properties for layered elements.

PREP7:Elements

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

Element number to be listed. If ALL, list all selected elements [ESEL] of the appropriate type. If blank and the current element type is a layered element type, list data from the current real constant table in the layered format.

Range of layer numbers to be listed. If LAYR1 is greater than LAYR2, a reverse order list is produced. LAYR1 defaults to 1. LAYR2 defaults to LAYR1 if LAYR1 is input or to the number of layers if LAYR1 is not input.

Material property labels (e.g., EX) to be listed along with the layer real constants.

Lists real constants and any two material properties for layered shell and solid elements. Only elements of type SOLID46, SHELL91, and SHELL99 are listed.

If matrix input is selected (KEYOPT(2) = 2 or 3), LAYR1, LAYR2, Mplab1, and Mplab2 are not used.

This command is valid in any processor.

Utility Menu >List >Elements >Layered Elements

Utility Menu >List >Properties >Layer Data

Displays the layer stacking sequence for layered elements.

PREP7:Elements

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

Element number for the display. If blank and the current element type is a layered element type, display data from the current real constant table.

Range of layer numbers to be displayed. If LAYR1 is greater than LAYR2, a reversed order display is produced. Up to 20 layers may be displayed at a time. LAYR1 defaults to 1. LAYR2 defaults to LAYR1 if LAYR1 is input or to the number of layers (or to 19+LAYR1, if smaller) if LAYR1 is not input.

Displays the layer stacking sequence (as defined in the real constant table) for layered shell and solid elements in a form where the layers are visible (like a sheared deck of cards). Layers are cross-hatched and color coded for clarity. The hatch lines indicate the layer angle (real constant THETA) and the color coding is for material identification (real constant MAT). Only valid for elements of type SOLID46, SHELL91, and SHELL99. Layered elements can be displayed using the EPLOT and /ESHAPE commands.

This command is valid in any processor.

Utility Menu >Plot >Layered Elements

Specifies absolute values for load case operations.

POST1:LoadCaseCalculations

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

Load case pointer number. If ALL, apply to all selected load cases [LCSEL].

Absolute value key:

0 - Use algebraic values of load case LCNO in operations.

1 - Use absolute values of load case LCNO in operations.

Notes

Causes absolute values to be used in the load case operations [LCASE or LCOPER]. Absolute values are taken prior to assigning a load case factor [LCFACT] and are applied only to defined load cases [LCDEF].

Main Menu >General Postproc >Load Case >Absolut Value

Reads a load case into the database.

POST1:LoadCaseCalculations

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

Load case pointer number [LCDEF,STAT]. Defaults to 1.

Notes

Reads a load case into the database. Load cases are created as described on the LCDEF or LCWRITE commands. The results portion of the database is cleared before reading the data in. Absolute values [LCABS] and scale factors [LCFACT] can be applied during the read operation. Harmonic element data read from a result file load case is processed at the zero-degree position.

Main Menu >General Postproc >Load Case >Read Load Case

Specifies "Load case settings" as the subsequent status topic.

POST1:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

Utility Menu >List >Status >General Postproc >Load Case Calcs

Concatenates multiple lines into one line for mapped meshing.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Lines to be concatenated. If NL1 = ALL, NL2 is ignored and all selected lines [LSEL] are concatenated. If NL1 = 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 NL1 (NL2 is ignored).

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

LCCAT is meant to be used solely for meshing and cannot be used for any other purposes. Specifically, (a) the output line and any areas that have the output line on their line list [ALIST] cannot be used as input to any other solid modeling operation (not even another LCCAT command); and (b) the output line cannot accept solid model boundary conditions [DL, SFL].

The output line will take on the element divisions of the input lines and will not accept element divisions that are directly assigned [LESIZE]. The output line from the LCCAT operation will be coincident with the input lines and the input lines will be retained. Consider the LCOMB command instead of LCCAT if you wish to delete the input lines and if the lines to be combined have similar slopes at the common keypoint(s). When an LCCAT command is issued, area line lists [ALIST] that contain all of the input lines will be updated so that the area line lists refer to the output line instead of the the input lines. Deletion of the output line [LDELE] effectively reverses the LCCAT operation and restores area line lists to their original condition.

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

Main Menu >Preprocessor >Concatenate >Lines

Main Menu >Preprocessor >Delete >Lines

Main Menu >Preprocessor >Mesh >Mapped >Lines

Creates a load case from a set of results on a results file.

POST1:LoadCaseCalculations

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

Arbitrary pointer number (1-99) to be assigned to the load case specified by LSTEP, SBSTEP and by the FILE command. Defaults to 1 + previous value.

Load step number to be defined as the load case. Defaults to one.

Substep number. Defaults to the last substep of the load step.

Used only with results from complex analyses:

0 - Use real part of complex solution

1 - Use imaginary part.

Creates a load case by establishing a pointer to a set of results on a results file (written during the ANSYS solution phase). This pointer (LCNO) can then be used on the LCASE or LCOPER commands to read the load case data into the database.

Issue LCDEF,ERASE to delete all load case pointers (and all loadcase files, if any). Issue LCDEF,LCNO,ERASE to delete only the specific load case pointer LCNO (and its file, if any). With the ERASE options, all pointers are deleted; however only files with the default extension [LCWRITE] are deleted. Issue LCDEF,STAT for status of all selected load cases [LCSEL], or LCDEF,STAT,ALL for status of all load cases. The STAT command may be used to list all load cases. See also LCFILE to establish a pointer to a set of results on a load case file (written by LCWRITE).

Main Menu >General Postproc >Load Case >Create Load Case

Main Menu >General Postproc >Load Case >Erase Load Case

Main Menu >General Postproc >Load Case >List Load Cases

Defines scale factors for load case operations.

POST1:LoadCaseCalculations

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

Load case pointer number. If ALL, apply to all selected load cases [LCSEL].

Scale factor applied to load case LCNO. Zero (or blank) defaults to 1.0. Use a small number for a "zero" scale factor.

Notes

Defines scale factors to be used in the load case operations [LCASE or LCOPER]. Scale factors are applied after an absolute value operation [LCABS] and are applied only to defined load cases [LCDEF].

Main Menu >General Postproc >Load Case >Scale Factor

Creates a load case from an existing load case file.

POST1:LoadCaseCalculations

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

Arbitrary (1-99) pointer number assigned to this load case.

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

File name extension (8 characters maximum). Defaults to LCNO value preceded by an "L" for values 10-99 or by "L0" for values 1-9.

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

Creates a load case by establishing a pointer to an existing load case file [LCWRITE]. This pointer (LCNO) can then be used on the LCASE or LCOPER commands to read the load case data into the database. This command is typically used to reestablish load case pointers in a new ANSYS session (pointers are not saved on the database file), or when more than one pointer to a single load case is desired. See the LCDEF command for status and erase operations. See also LCDEF to establish a pointer to a set of results on a results file (written during the ANSYS solution phase).

Main Menu >General Postproc >Load Case >Create Load Case

Deletes nodes and line elements associated with selected lines.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Delete mesh for lines NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL, NL2 and NINC are ignored and the mesh for all selected lines [LSEL] is deleted. If NL1 = 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 NL1 (NL2 and NINC are ignored).

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

Main Menu >Preprocessor >Clear >Lines

Combines adjacent lines into one line.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the first line to be combined. If NL1 = ALL, NL2 is ignored and all selected lines [LSEL] are combined. If NL1 = 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 NL1 (NL2 is ignored).

Number of the second line to be combined.

Specifies whether to keep the input entities:

0 - Delete lines NL1 and NL2 and their common keypoint. Keypoints will not be deleted if they are meshed or if they are attached to other lines. Lines will not be deleted if they are attached to different areas.

1 - Keep NL1, NL2, and their common keypoint. (The common keypoint will not be attached to the output line.)

Combines adjacent lines into one line (the output line). This operation will effectively "undo" the LDIV operation. Line divisions are set to zero (use LESIZE, etc. to modify). Lines attached to the same area(s) can also be combined. See also the LCCAT command for line concatenation capability.

Main Menu >Preprocessor >Operate >Add >Lines

Performs load case operations.

POST1:LoadCaseCalculations

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

Valid operations are:

ZERO - Zero results portion of database (LCASE1 ignored).

SQUA - Square database values (LCASE1 ignored).

SQRT - Square root of database (absolute) values (LCASE1 ignored).

LPRIN - Recalculate line element principal stresses (LCASE1 ignored). Stresses are as shown for the NMISC items of the ETABLE command for the specific line element type.

ADD - Add LCASE1 to database values.

SUB - Subtract LCASE1 from database values.

SRSS - Square root of the sum of the squares of database and LCASE1.

MIN - Compare and save in database the algebraic minimum of database and LCASE1.

MAX - Compare and save in database the algebraic maximum of database and LCASE1.

ABMN - Compare and save in database the absolute minimum of database and LCASE1 (based on magnitudes, then apply the corresponding sign).

ABMX - Compare and save in database the absolute maximum of database and LCASE1 (based on magnitudes, then apply the corresponding sign).

First load case in the operation (if any). See LCNO of the LCDEF command. If ALL, repeat operations using all selected load cases [LCSEL].

Valid operations are:

MULT - Multiplication: LCASE1*LCASE2

Second load case. Used only with Oper2 operations.

LCOPER operates on the database and one or two load cases according to:

where operations o (Oper) and o2 (Oper2) are as described above. Absolute values and scale factors may be applied to the load cases before the operations [LCABS, LCFACT]. If LCASE1 is not specified, only operation o is performed on the current database. If LCASE2 is specified, operation o2 will be performed before operation o. If LCASE2 is not specified, operation o2 is ignored. Solution items not contained [OUTRES] in either the database or the applicable load cases will result in a null item during a load case operation. Harmonic element data read from a result file load case are processed at zero degrees. All load case combinations are performed in the solution coordinate system, and the data resulting from load case combinations are stored in the solution coordinate system. The resultant data are then transformed to the active results coordinate system [RSYS] when listed or displayed.

Main Menu >General Postproc >Load Case >Add

Main Menu >General Postproc >Load Case >Line Elem Stress

Main Menu >General Postproc >Load Case >Min & Max

Main Menu >General Postproc >Load Case >SRSS

Main Menu >General Postproc >Load Case >Square Root

Main Menu >General Postproc >Load Case >Square

Main Menu >General Postproc >Load Case >Subtract

Selects a subset of load cases.

POST1:LoadCaseCalculations

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

Label identifying the type of select:

S - Select a new set.

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.

Minimum value of load case pointer range.

Maximum value of load case pointer range. LCMAX defaults to LCMIN.

Value increment within range. Defaults to 1. LCINC cannot be negative.

Notes

Selects a subset of load cases for other operations. For example, to select a new set of load cases based on load cases 1 through 7, use LCSEL,S,1,7. The subset is used when the ALL label is entered (or implied) on other commands, such as LCFACT, LCABS, LCOPER, etc. Load cases are flagged as selected and unselected; no load case pointers [LCDEF, LCWRITE, LCFILE] are actually deleted from the database.

Main Menu >General Postproc >Load Case >Sele Ld Cases

Divides intersecting lines at their point(s) of intersection.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of lines to be intersected. If NL1=ALL, NL2 to NL9 are ignored and the intersection of all selected lines is found. If NL1=P, use graphical picking to specify lines (NL2 to NL9 are ignored).

Divides intersecting (classifies) lines at their point(s) of intersection. The original lines (and their corresponding keypoint(s)) 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.

This command cannot be accessed directly in the menu.

Specifies whether to process non-summable items in load case operations.

POST1:Results

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

Combination option

<blank> - Only combine summable items [default].

ALL - Combine all items including non summable items.

Allows non-summable items (e.g. plastic strains) to be included in load combinations. Issue LCSUM,ALL before the first load case operation (LCxx command). May also be used to include non-summable items in the appending of a results file (RAPPND command).

Not available through the GUI.

LCWRITE, LCNO, Fname, Ext, Dir

Creates a load case by writing results to a load case file.

POST1:LoadCaseCalculations

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

Arbitrary pointer number (1-99) to be assigned to this load case.

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

File name extension (8 characters maximum). Defaults to LCNO value preceded by the character "L" (values 1-9 will include "0" as a prefix, such as L01, L02, etc.).

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

Creates a load case by writing the results data in the database to a load case file. The database remains unchanged by this operation. A pointer is also established to the written set of results on the load case file. This pointer (LCNO) can then be used on the LCASE or LCOPER commands to read the load case data into the database. By default, only summable results data (such as displacements, stresses, elastic strains) and constant results data (such as volume) are written to the load case file unless requested (LCSUM command). Non-summable results data (such as plastic strains, strain energy), boundary conditions, and nodal loads are not written to the load case file. The load case file may be named by default or by a user name. Rewriting to the same file overwrites the previous data. See the LCDEF command for status and erase operations.

Main Menu >General Postproc >Load Case >Write Load Case

Zeroes the results portion of the database.

POST1:LoadCaseCalculations

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

Often used before the LCOPER command. Same as LCOPER,ZERO.

Main Menu >General Postproc >Load Case >Zero Load Case

Deletes unmeshed lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Delete lines from NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL, NL2 and NINC are ignored and all selected lines [LSEL] are deleted. If P1 = 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 NL1 (NL2 and NINC are ignored).

Specifies whether keypoints are also to be deleted:

0 - Delete lines only.

1 - Delete lines, as well as keypoints attached to lines but not attached to other lines.

A line attached to an area cannot be deleted unless the area is first deleted.

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

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

Menu Paths

Main Menu >Preprocessor >Concatenate >Lines

Main Menu >Preprocessor >Delete >Lines

Main Menu >Preprocessor >Mesh >Mapped >Lines

Main Menu >Preprocessor >Delete >Line and Below

Main Menu >Preprocessor >Delete >Lines Only

Divides a single line into two or more lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the line to be divided. If negative, assume P1 (see below) is the second keypoint of the line instead of the first for RATIO. If ALL, divide all selected lines [LSEL]. If NL1 = 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 NL1.

Ratio of line length P1-PDIV to line length P1-P2. Must be between 0.0 and 1.0. Input ignored if NDIV > 2.

Number to be assigned to keypoint generated at division location (defaults to lowest available keypoint number [NUMSTR]). Input ignored if NL1 = ALL or NDIV > 2. If PDIV already exists and lies on line NL1, divide line at PDIV (RATIO must also be 0.0). If PDIV already exists and does not lie on line NL1, PDIV is projected and moved to the nearest point on line NL1 (if possible). PDIV cannot be attached to another line, area, or volume.

The number of new lines to be generated from old line (defaults to 2).

Specifies whether to keep the input entities:

0 - Modify old line to use new keypoints and slopes.

1 - Do not modify old line. New lines will overlay old line and have unique keypoints.

Divides a single line NL1 (defined from keypoint P1 to keypoint P2) into two or more lines. Line NL1 becomes the new line beginning with keypoint P1 and new lines are generated ending at keypoint P2. If the line is attached to an area, the area will also be updated. Line divisions are set to zero (use LESIZE, etc. to modify).

Main Menu >Preprocessor >Operate >Divide >Line into 2 Ln's

Main Menu >Preprocessor >Operate >Divide >Line into N Ln's

Main Menu >Preprocessor >Operate >Divide >Lines w/ Options

Generates lines by sweeping a keypoint pattern along path.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

List of keypoints in the pattern to be dragged (6 maximum if using keyboard entry). If NK1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). If NK1=ALL, all selected keypoints (except those that define the drag path) will be swept along the path. A component name may also be substituted for NK1.

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 lines (and their corresponding keypoints) by sweeping a given keypoint 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 (NL1, NL2, etc.). If the drag path is a single line (NL1), the drag direction is from the keypoint on the drag line that is closest to the first keypoint of the given 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 and line numbers are automatically assigned (beginning with the lowest available values [NUMSTR]). 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

Reads results from the results file and applies them as loads.

SOLUTION:FEConstraints SOLUTION:FEBodyLoads

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

Valid load label:

TEMP - Temperatures from a thermal analysis applied as body force loads [BF] in a structural (or other type of) analysis.

FORC - Forces from a magnetic analysis applied as force loads [F] in a structural analysis or a FLOTRAN analysis. For a full harmonic magnetic analysis, FORC represents the time-averaged force (use in conjunction with KIMG=2). Values are in the nodal coordinate system for the force loads [F].

HGEN - Heat generations from a magnetic analysis applied as body force loads [BFE] in a thermal or a FLOTRAN analysis. For a full harmonic analysis, HGEN represents the time-averaged heat generation load (use in conjunction with KIMG=2).

HFLU - Heat fluxes from a FLOTRAN analysis applied as surface loads in a thermal analysis.

EHFLU - Surface losses from a high frequency electromagnetic analysis applied as time-average surface heat flux in a thermal analysis.

JS - Source current density from a current-conduction analysis applied as body force loads [BFE]. Values are in the global Cartesian coordinate system.

PRES - Pressures from a FLOTRAN analysis applied as surface loads [SFE] in a structural analysis. For shell elements, use the KIMG parameter to establish the face on which to apply the pressure.

REAC - Reaction loads from any analysis applied as force loads [F] in any analysis. Values are in the nodal coordinate system.

HFLM - FLOTRAN predicted film coefficient (and associated bulk temperature), applied as surface loads (film coefficient and bulk temperature) [SFE] in a thermal analysis. FLOTRAN film coefficents may be either positive or negative, depending on the direction of heat transfer, but ANSYS thermal analyses require positive film coefficients. If the FLOTRAN film coefficient is negative, LDREAD adjusts the bulk temperature to be equal to twice the wall temperature minus the bulk temperature. The adjusted bulk temperature and the now positive film coefficient make the amount and direction of heat transfer consistent with the FLOTRAN analysis.

Load step number of the data set to be read. Defaults to 1. If LAST, ignore SBSTEP and TIME and read the last data set.

Substep number (within LSTEP). If zero (or blank), LSTEP represents the last substep of the load step.

Time-point identifying the data set to be read. Used only if both LSTEP and SBSTEP are zero (or blank). If TIME is between two solution time points on the results file, a linear interpolation is done between the two data sets. If TIME is beyond the last time point on the file, use the last time point.

When used with results from harmonic analyses (ANTYPE=HARMIC) KIMG establishes which set of data to read:

0 - Read the real part of the solution. Valid also for Lab=EHFLU to read in time-average heat flux.

1 - Read the imaginary part of the solution.

2 - Calculate and read the time-average part. Meaningful for Lab=HGEN or FORC.

When used with the PRES label, KIMG represents the shell element face on which to apply the pressure:

1 - Apply pressure to face 1

2 - Apply pressure to face 2

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

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

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

Reads results data from the results file and applies them as loads. You also can use LDREAD to apply results from an analysis defined with one physics environment as loads on a second analysis using a different physics environment. The values are applied as loads for field coupling effects (such as output temperatures from a thermal analysis as input to a structural analysis). Nodal loads are applied only to selected nodes. Element loads are applied only to selected elements. Element surface loads are applied only to selected elements where all face nodes for that surface are selected. Additionally, to assure proper distribution of the surface loads, select only the nodes on the element face where the surface load is to be applied. Scaling and accumulation specifications are applied as the loads are read (BFCUM for body force loads, SFCUM for surface loads, and FCUM for force loads). Use the appropriate list command to list the results (BFLIST or BFELIST for body force loads,SFELIST for surface loads, and FLIST for force loads). Values may be redefined as desired after being read.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Apply >Boundary >-Temperature- >From Therm Analy

Main Menu >Preprocessor >Loads >Apply >Convection >From Fluid Analy

Main Menu >Preprocessor >Loads >Apply >Excitation >From Elec An

Main Menu >Preprocessor >Loads >Apply >Force/Moment >From Mag Analy

Main Menu >Preprocessor >Loads >Apply >Force/Moment >From Reactions

Main Menu >Preprocessor >Loads >Apply >Forces >From Mag Analy

Main Menu >Preprocessor >Loads >Apply >Heat Flux >From EMAG Analy

Main Menu >Preprocessor >Loads >Apply >Heat Flux >From FluidAnaly

Main Menu >Preprocessor >Loads >Apply >Heat Generat >From Mag Analy

Main Menu >Preprocessor >Loads >Apply >Pressure >From Fluid Analy

Main Menu >Preprocessor >Loads >Apply >Temperature >From Therm Analy

Main Menu >Solution >Apply >Boundary >-Temperature- >From Therm Analy

Main Menu >Solution >Apply >Convection >From Fluid Analy

Main Menu >Solution >Apply >Excitation >From Elec An

Main Menu >Solution >Apply >Force/Moment >From Mag Analy

Main Menu >Solution >Apply >Force/Moment >From Reactions

Main Menu >Solution >Apply >Forces >From Mag Analy

Main Menu >Solution >Apply >Heat Flux >From EMAG Analy

Main Menu >Solution >Apply >Heat Flux >From FluidAnaly

Main Menu >Solution >Apply >Heat Generat >From Mag Analy

Main Menu >Solution >Apply >Pressure >From Fluid Analy

Main Menu >Solution >Apply >Temperature >From Therm Analy

Specifies the divisions and spacing ratio on unmeshed lines.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the line to be modified. If ALL, modify all selected lines [LSEL]. If NL1 = 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 NL1.

If NDIV is blank, SIZE is the division (element edge) length. The number of divisions is automatically calculated from the line length (rounded upward to next integer). If SIZE is zero (or blank), use ANGSIZ or NDIV.

The division arc (in degrees) spanned by the element edge (except for straight lines, which always result in one division). The number of divisions is automatically calculated from the line length (rounded upward to next integer).

If positive, NDIV is the number of element divisions per line. If -1 (and KFORC=1), NDIV is assumed to be zero element divisions per line. If NDIV is negative (not -1), there are no elements defined yet, but there are divisions.

Spacing ratio. If positive, nominal ratio of last division size to first division size (if > 1.0, sizes increase, if < 1.0, sizes decrease). If negative, |SPACE| is nominal ratio of center division(s) size to end divisions size. Ratio defaults to 1.0 (uniform spacing). For layer-meshing, a value of 1.0 normally is used.

KFORC 0-3 are used only with NL1 = ALL. Specifies which selected and unmeshed lines are to be modified.

0 - Modify only selected unmeshed lines having undefined (zero) divisions.

1 - Modify all selected unmeshed lines.

2 - Modify only selected unmeshed lines having fewer divisions (including zero) than specified with this command.

3 - Modify only selected unmeshed lines having more divisions than specified with this command.

4 - Modify only non-zero settings for SIZE, ANGSIZ, NDIV, SPACE, LAYER1, and LAYER2. If KFORC = 4, blank or 0 settings remain unchanged.

Layer-meshing control parameter. Distance which defines the thickness of the inner mesh layer, LAYER1. Elements in this layer are uniformly-sized with edge lengths equal to the specified element size for the line (either through SIZE or line-length/NDIV). A positive value for LAYER1 is interpreted as an absolute length, while a negative value in interpreted as a multiplier on the specified element size for the line. As a general rule, the resulting thickness of the inner mesh layer should be greater than or equal to the specified element size for the line. If LAYER1 = OFF, layer-meshing control settings are cleared for the selected lines. The default value is 0.0

Layer-meshing control parameter. Distance which defines the thickness of the outer mesh layer, LAYER2. Elements in this layer transition in size from those in LAYER1 to the global element size. A positive value of LAYER2 is interpreted as an absolute length, while a negative value is interpreted as a mesh transition factor. A value of LAYER2 = -2 would indicate that elements should approximately double in size as the mesh progresses normal to LAYER1. The default value is 0.0.

Defines the number of divisions and the spacing ratio on selected unmeshed lines. Lines with previously specified divisions may also be changed.

Main Menu >Preprocessor >Size Cntrls >All Lines

Main Menu >Preprocessor >Size Cntrls >Clr Layers

Main Menu >Preprocessor >Size Cntrls >Clr Size

Main Menu >Preprocessor >Size Cntrls >Copy Divs

Main Menu >Preprocessor >Size Cntrls >Flip Bias

Main Menu >Preprocessor >Size Cntrls >Picked Lines

Extends a line at one end by using its slope.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the line to be extended. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Number of keypoint at the end of line NL1 to be extended.

Distance that the line will be extended.

Specifies whether to keep the input entities:

0 - Modify old line to use new keypoints and slopes.

1 - Do not modify old line. New line will overlay old line and have unique keypoints.

Extends a line at one end by using its slope. Lines may be redefined only if not yet attached to an area. Line divisions are set to zero (use LESIZE, etc. to modify). Note that solid modeling in a toroidal coordinate system is not recommended.

Main Menu >Preprocessor >Operate >Extend Line

Generates a fillet line between two intersecting lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the first intersecting line. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Number of the second intersecting line.

Radius of fillet to be generated. Radius should be less than the lengths of the two lines specified with NL1 and NL2.

Number to be assigned to generated keypoint at fillet arc center. If zero (or blank), no keypoint is generated.

Generates a fillet line between two intersecting lines NL1 (P1-PINT) and NL2 (P2-PINT). Three keypoints may be generated, two at the fillet tangent points (PTAN1 and PTAN2) and one (optional) at the fillet arc center (PCENT). Line P1-PINT becomes P1-PTAN1, P2-PINT becomes P2-PTAN2, and new arc line PTAN1-PTAN2 is generated. Generated keypoint and line numbers are automatically assigned (beginning with the lowest available values [NUMSTR]). Line divisions are set to zero (use LESIZE, etc. to modify).

Main Menu >Preprocessor >Create >Line Fillet

Generates surface elements overlaid on the edge 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 lines of the meshed solid areas.

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 plane elements and, based on proximity, to determine and assign the extra node for each surface element. The underlying areas of the solid region and the fluid lines must be meshed prior to calling this command macro.

The surface lines 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., 'SLINE') when the LFSURF command is manually typed in.

The macro is applicable for the SURF151 and FLUID116 element types.

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

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

Generates additional lines from a pattern of lines.

PREP7:Lines

	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 > 1 for generation to occur.

Generate lines from pattern beginning with NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL, NL2 and NINC are ignored and pattern is all selected lines [LSEL]. If NL1 = 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 NL1 (NL2 and NINC are ignored).

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

Keypoint 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 lines, if they exist.

1 - Do not generate nodes and elements.

Specifies whether to redefine the existing lines:

0 - Generate additional lines as requested with the ITIME argument.

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

Generates additional lines (and their corresponding keypoints and mesh) from a given line pattern. The MAT, TYPE, REAL, and ESYS attributes are based upon the lines in the pattern and not upon the current settings. 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, etc. Generations which produce lines 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. Note that solid modeling in a toroidal coordinate system is not recommended. New line numbers are automatically assigned (beginning with the lowest available values [NUMSTR]).

Main Menu >Preprocessor >Copy >Lines

Main Menu >Preprocessor >Move / Modify >Lines

Generates new lines by "gluing" lines.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of the lines to be glued. If NL1 = ALL, all selected lines will be glued (NL2 to NL9 will be ignored). If NL1 = 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 NL1.

Generates new lines by "gluing" input lines. The glue operation redefines the input lines so that they share keypoints at their common ends. The new lines encompass the same geometry as the original lines. This operation is only valid if the intersections of the input lines are keypoints at the ends of those lines. 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 >Glue >Lines

Writes the database command log to a file.

SESSION:Files

	Mp Me St DY LP Th E3 E2 FL PP ED

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

File name extension (8 characters maximum). Defaults to LGW if Fname and Ext are blank.

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

Flag to suppress nonessential commands:

NONE - Do not suppress any commands (default).

COMMENT - Write nonessential commands as comments (starting with !).

REMOVE - Do not write nonessential commands or comments.

Writes the database command log to a named file. The database command log contains all commands that were used to create the current database. These commands are recorded in the database as they are issued, and saved in the database file (File.DB) whenever the database is saved. The LGWRITE command extracts these commands from the database and writes them to a file. Nonessential commands (for listing, graphics displays, help, etc.) can be excluded from the file by using the Kedit field. The file resulting from LGWRITE can be used as command input to the program. This command is most useful if the session log file (File.LOG), which is normally saved during an interactive session, has been lost or corrupted. LGWRITE cannot be used after design optimization looping because the database is cleared [/CLEAR] automatically at each loop; use File.LOG instead.

This command is valid in any processor.

Utility Menu >File >Write DB Log File

Specifies the light direction for the display window.

GRAPHICS:Style

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Ambient or directional light key:

0 - Ambient light (default).

1 - Directional light.

Light intensity factor (defaults to 0.3 for ambient, 1.0 for directional) This option is valid only for 3-D devices).

Light direction (valid only for NUM=1). The directional light source is parallel to the line from point XV, YV, ZV to the origin, in the global Cartesian system origin. Defaults to the viewing direction [/VIEW].

Light reflectance factor (valid only for NUM=1 and 3-D devices).

Notes

Defines the light direction for the window. Use this command only with 3-D graphics devices or 2-D devices when Z-buffering is used [/TYPE,,(6 or 7)]. The ambient light has no direction, only an intensity. You can position the directional light source by defining a point (in the global Cartesian coordinate system) representing a point along the light directional line. This point, and the global Cartesian coordinate system origin, define the line along which the light is positioned looking toward the origin. You can use any point along the light line; for example, both (1.,1.,1.) and (2.,2.,2.) give the same light effect. For 3-D graphics devices only, the directional light source also has intensity and reflectance factors.

By choosing the highest intensity ambient light for 3-D graphics devices (via the command /LIGHT,WN,0,1), you can nullify color shading and other effects of directional lighting.

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Light Source

Finds the intersection of a line with an area.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of line to be intersected. If NL = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Number of area to be intersected.

Finds the intersection of a line with an area. New lines will be generated where the lines intersect the areas. If the regions of intersection are only points, new keypoints 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 >Line with Area

Creates annotation lines (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Line X starting location (-1.0 < X < 2.0).

Line Y starting location (-1.0 < Y < 1.0).

Line X ending location (-1.0 < X < 2.0).

Line Y ending location (-1.0 < Y < 1.0).

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

All lines are shown on subsequent displays unless the annotation is turned off or deleted. Use the /LSPEC command to set the attributes of the line.

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Specifies "Lines" 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.

Specifies the length of a printed page.

POST26:Listing

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of lines per page (defaults to 50). (Minimum allowed = 21).

Notes

Specifies the length of a printed page (for use in reports, etc.).

Main Menu >TimeHist Postpro >Settings >List

Finds the common intersection of lines.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of lines to be intersected. If NL1 = ALL, find the intersection of all selected lines and NL2 to NL9 are ignored. If NL1 = 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 NL1.

Finds the common (not pairwise) intersection of lines. The common intersection is defined as the regions shared (in common) by all lines listed on this command. New lines will be generated where the original lines intersect. If the regions of intersection are only points, new keypoints 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 >Lines

Finds the pairwise intersection of lines.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of lines to be intersected pairwise. If NL1 = ALL, find the pairwise intersection of all selected lines and NL2 to NL9 are ignored. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for NL1.

Finds the pairwise intersection of lines. The pairwise intersection is defined as any and all regions shared by at least two lines listed on this command. New lines will be generated where the original lines intersect pairwise. If the regions of pairwise intersection are only points, new keypoints 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 >Lines

Finds the intersection of a line with a volume.

PREP7:Booleans

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

Number of line to be intersected. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Number of volume to be intersected.

Finds the intersection of a line with a volume. New lines will be generated where the lines intersect the volumes. If the regions of intersection are only points, new keypoints 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 >Line with Volume

Displays the contents of an external, coded file.

SESSION:Files

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (32 characters maximum) to be displayed.

File name extension (8 characters maximum).

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

Displays the contents of an external, coded file. The file to be listed cannot be in use (open) at the time (except for the error file, File.ERR, which may be displayed with *LIST,ERR).

Use caution when you are listing active ANSYS files via the List>Files>Other and File>List>Other menu paths. File I/O buffer and system configurations can result in incomplete listings unless the files are closed.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Lists the defined lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

List lines from NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL (default), NL2 and NINC are ignored and all selected lines [LSEL] are listed. If NL1 = 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 NL1 (NL2 and NINC are ignored).

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

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

RADIUS - Prints the radius of any circular arcs, along with the keypoint numbers of each line. Non-circular arcs will print a radius value of zero.

LAYER - Prints layer-mesh control specifications.

HPT - Prints information about only those lines that contain hard points. HPT is not supported in the GUI.

ORIENT - Prints a list of lines, and identifies any orientation keypoints and any cross section IDs that are associated with the lines. Used for beam meshing with defined orientation nodes and cross sections.

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 LATT 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). The number of line divisions (NDIV) is unassigned if listed as a zero; NDIV was assigned by the user (and will not be reset to zero if the mesh is cleared) if listed as a positive value; NDIV was calculated and assigned during meshing (and will be reset to zero if the mesh is cleared) if listed as a negative value. A "-1" in the "nodes" column indicates that the line has been meshed but there are no interior nodes.

This command is valid in any processor.

Utility Menu >List >Lines

Utility Menu >List >Picked Entities >Lines

Calculates an inductance matrix for an N-winding system.

SOLUTION:AnalysisOptions

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

Geometric symmetric factor. Inductance terms are scaled by this factor which represents the fraction of the total device modeled.

Alpha-numeric prefix identifier for coil label used in defining named element coil components.

Name of a predefined parameter array containing the nominal coil currents of the system. The array must be defined (see *DIM command) prior to calling the LMATRIX macro.

Name of the array parameter to be created by LMATRIX containing the calculated inductance coefficients. A text file of the same name with an extension .TXT is created containing the matrix data.

LMATRIX calculates an inductance matrix for an N-winding system where N is the number of coils in the system.

To invoke the LMATRIX macro, the elements for each coil must be grouped into a component using the CM command. Each set of independent coil elements is assigned a component name with a prefix followed by the coil number.

To invoke the LMATRIX macro, a vector array parameter with dimension N must be defined and named using the *DIM command. Each entry of the vector array represents a unique coil. The vector array entries are set equal to the nominal current per turn in the coils at the operating point. Zero current values must be approximated by a negligibly small applied current.

All name-strings must be enclosed in single quotes in the LMATRIX command line.

See Chapter 5 of the ANSYS Theory Reference and Chapter 11 of the ANSYS Electromagnetic Field Analysis Guide for details.

Main Menu >Solution >Electromagnet >Induct Matrix

Generates nodes and line elements along lines.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Mesh lines from NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL, NL2 and NINC are ignored and all selected lines [LSEL] are meshed. If NL1 = 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 NL1 (NL2 and NINC are ignored).

Generates nodes and line elements along lines. Missing nodes required for the generated elements are created and assigned the lowest available numbers.

Main Menu >Preprocessor >Mesh >Lines

Collapse a line segment to a keypoint (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

The ID of the line segment to be collapsed.

The ID of the existing keypoint (one of the keypoints connected to the line segment) that will remain after the collapse operation.

This command is available only for repairing the geometry of models imported from CAD systems (Default IGES option).

This command does not check for any entity penetration resulting from the collapse.

Main Menu >Preprocessor >Simplify >Collapse Lines

Detaches lines from neighboring geometric entity (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

Detach lines from LINE1 to LINE2 (defaults to LINE1) in steps of LNINC (defaults to 1).

Use this command to detach non-manifold lines from their neighboring geometric entities. This command is available only for repairing the geometry of models imported from CAD systems.

Main Menu >Preprocessor >Geom Repair >Detach Lines

Creates a straight line between two keypoints (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

Creates a straight line from keypoint defined by KP1 to keypoint defined by KP2. If NL1 = P; graphical picking is enabled and the remaining command field is ignored.

This command is available only for repairing the geometry of models imported from CAD systems (Default IGES option).

Main Menu >Preprocessor >Geom Repair >Fill Lines

Merges two or more connected line segments (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 set of line segments to merge into one or more line segments. The command merges all the lines from the selected set that are connected to only one other line. 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 merged and all remaining arguments are ignored. The connected lines are automatically grouped together to form a set of merged lines.

Use the LNMERGE command to merge disproportionately small line segments into a single line segment. This command is available only for repairing the geometry of models imported from CAD systems (Default IGES option). Only those line segments specified in the LN1 through LN10 list that are connected together will be joined by the merge operation. The command considers two lines to be connected if those two lines(and only those two lines) connect together at a single keypoint.

While the LNMERGE command allows you to join multiple lines in one merge operation, the preferred method is to merge pairs of line segments to successively build a single line segment. Using this technique can prevent problems during meshing.

The LNMERGE command does not check the angle of inclination between adjacent lines during the merge operation.

Main Menu >Preprocessor >Simplify >Merge Lines

Splits a line segment into two line segments (for models imported from CAD files).

PREP7:CADRepair

	Mp Me St DY LP Th E3 E2 FL PP ED

ID identifying the line to be split.

Arc length parameter specifying the location of the keypoint which will join the two new line segments (the "split point"). Valid arguments are values between 0 and 1, measured from the line's starting keypoint. Negative values between 0 and -1 are measured from the line's ending keypoint.

This command is available only for repairing the geometry of models imported from CAD systems (Default IGES option).

Main Menu >Preprocessor >Simplify >Split Lines

Activates a line search to be used with Newton-Raphson.

SOLUTION:NonlinearOptions

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

Line search key:

OFF - Do not use a line search.

ON - Use a line search. Note, adaptive descent is suppressed when LNSRCH is on unless explicitly requested on the NROPT command. Having line search on and adaptive descent on at the same time is not recommended.

AUTO - ANSYS automatically switches line searching ON and OFF between substeps of a load step as needed. This option is recommended.

Notes

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

Activates a line search to be used with the Newton-Raphson method [NROPT]. Line search is an alternative to adaptive descent (see Section 15.9 of the ANSYS Theory Reference).

LNSRCH,AUTO can be very efficient for problems in which LNSRCH is needed at only certain substeps.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Nonlinear >Line Search

Main Menu >Solution >Nonlinear >Line Search

Defines a local coordinate system by a location and orientation.

DATABASE:CoordinateSystem

	Mp Me St DY LP Th E3 E2 FL PP ED

Arbitrary reference number assigned to this coordinate system. Must be greater than 10. A coordinate system previously defined with this number will be redefined.

Coordinate system type:

0 or CART - Cartesian

1 or CYLIN - Cylindrical (circular or elliptical)

2 or SPHE - Spherical (or spheroidal)

3 or TORO - Toroidal

Location (in the global Cartesian coordinate system) of the origin of the new coordinate system.

First rotation about local Z (positive X toward Y).

Second rotation about local X (positive Y toward Z).

Third rotation about local Y (positive Z toward X).

Used for elliptical, spheroidal, or toroidal systems. If KCS=1 or 2, PAR1 is the ratio of the ellipse Y-axis radius to X-axis radius (defaults to 1.0 (circle)). If KCS=3, PAR1 is the major radius of the torus.

Used for spheroidal systems. If KCS=2, PAR2 = ratio of ellipse Z-axis radius to X-axis radius (defaults to 1.0 (circle)).

Defines a local coordinate system by origin location and orientation angles. The local coordinate system is parallel to the global Cartesian system unless rotated. Rotation angles are in degrees and redefine any previous rotation angles. See the CLOCAL, CS, CSWPLA, and CSKP commands for alternate definitions. This local system becomes the active coordinate system [CSYS]. Local coordinate systems may be displayed with the /PSYMB command.

This command is valid in any processor.

Utility Menu >WorkPlane >Local Coordinate Systems >Create Local CS >At Specified Loc

Overlaps lines.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of lines to be overlapped. If NL1 = ALL, NL2 to NL9 are ignored and all selected lines are overlapped. If NL1 = 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 NL1.

Overlaps lines. Generates new lines which encompass the geometry of all the input lines. The new lines are defined by the regions of intersection of the input lines, and by the complementary (non-intersecting) regions. See the ANSYS Modeling and Meshing Guide for an illustration. This operation is only valid when the region of intersection is a line. 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 >Lines

Displays the selected lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Display lines from NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL (default), NL2 and NINC are ignored and display all selected lines [LSEL].

This command is valid in any processor.

Utility Menu >Plot >Lines

Utility Menu >Plot >Specified Entities >Lines

Partitions lines.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Numbers of lines to be operated on. If NL1 = ALL, NL2 to NL9 are ignored all selected lines are used. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for NL1.

Partitions lines. Generates new lines which encompass the geometry of all the input lines. The new lines are defined by both the regions of intersection of the input lines and the complementary (non-intersecting) regions. 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 >Lines

Refines the mesh around specified lines.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Lines (NL1 to NL2 in increments of NINC) around which the mesh is to be refined. NL2 defaults to NL1, and NINC defaults to 1. If NL1=ALL, NL2 and NINC are ignored and all selected lines are used for refinement. If NL1=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 NL1 (NL2 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 lines (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.

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

LREFINE refines all area elements and tetrahedral volume elements that are adjacent to the specified lines. Any volume elements that are adjacent to the specified lines, 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. For additional restrictions on mesh refinement, see Chapter 8 of the ANSYS Modeling and Meshing Guide.

Main Menu >Preprocessor >Modify Mesh >Lines

Reverses the normal of a line, regardless of its connectivity or mesh status.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Line number of the line whose normal direction is to be reversed. If LNUM=ALL, the normals of all selected lines will be reversed. If LNUM=P, graphical picking is enabled. A component name may also be substituted for LNUM.

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

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

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

You cannot use the LREVERSE 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.

For more information, see Chapter 8 of the ANSYS Modeling and Meshing Guide.

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

Generates circular lines by rotating a keypoint pattern about an axis.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

List of keypoints in the pattern to be rotated (6 maximum if using keyboard entry). If NK1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). If NK1=ALL, all selected keypoints (except PAX1 and PAX2) will define the pattern to be rotated. A component name may also be substituted for NK1.

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

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

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

Generates circular lines (and their corresponding keypoints) by rotating a 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. Keypoint and line numbers are automatically assigned (beginning with the lowest available values [NUMSTR]).

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

Subtracts areas from lines.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Line (or lines, if picking is used) to be subtracted from. If ALL. use all selected lines. If NL = 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 NL.

Area (or areas, if picking is used) to be subtracted. If ALL, use all selected areas. A component name may also be substituted for NA.

Behavior if the intersection of the lines and the areas is a keypoint or keypoints:

<blank> - The resulting lines will share keypoint(s) where they touch.

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

Specifies whether NL lines are to be deleted:

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

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

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

Specifies whether NA areas are to be deleted:

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

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

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

Generates new lines by subtracting the regions common to both NL lines and NA areas (the intersection) from the NL lines. The intersection can be a line(s) or keypoint(s). If the intersection is a keypoint and SEPO is blank, the NL line is divided at the keypoint and the resulting lines will be connected, sharing a common keypoint where they touch. If SEPO is set to SEPO, NL is divided into two unconnected lines with separate keypoints where they touch. 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 >Divide >Line by Area

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

Subtracts lines from lines.

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Line (or lines, if picking is used) to be subtracted from. If ALL, use all selected lines. Lines specified in this argument are not available for use in the NL2 argument. If P, graphical picking is enabled (valid only in the GUI) and all remaining fields are ignored. A component name may also be substituted for NL1.

Line (or lines, if picking is used) to subtract. If ALL, use all selected lines (except those included in the NL1 argument). A component name may also be substituted for NL2.

Behavior if the intersection of the NL1 lines and the NL2 lines is a keypoint or keypoints:

<blank> - The resulting lines will share keypoint(s) where they touch.

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

Specifies whether NL1 lines are to be deleted:

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

DELETE - Delete NL1 lines after LSBL operation (override BOPTN command settings).

KEEP - Keep NL1 lines after LSBL operation (override BOPTN command settings).

Specifies whether NL2 lines are to be deleted:

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

DELETE - Delete NL2 lines after LSBL operation (override BOPTN command settings).

KEEP - Keep NL2 lines after LSBL operation (override BOPTN command settings).

Generates new lines by subtracting the regions common to both NL1 and NL2 lines (the intersection) from the NL1 lines. The intersection can be a line(s) or point(s). If the intersection is a point and SEPO is blank, the NL1 line is divided at the point and the resulting lines will be connected, sharing a common keypoint where they touch. If SEPO is set to SEPO, NL1 is divided into two unconnected lines with separate keypoints where they touch. 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. LSBL,ALL,ALL will have no effect since all the lines (in NL1) will be unavailable as NL2 lines.

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

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

Main Menu >Preprocessor >Operate >Subtract >Lines

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

Subtracts volumes from lines.

PREP7:Booleans

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

Line (or lines, if picking is used) to be subtracted from. If ALL. use all selected lines. If NL = 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 NL.

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

Behavior if the intersection of the NL lines and the NV volumes is a keypoint or keypoints:

<blank> - The resulting lines will share keypoint(s) where they touch.

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

Specifies whether NL lines are to be deleted:

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

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

KEEP - Keep NL lines after LSBV 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 NV volumes after LSBV operation (override BOPTN command settings).

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

Generates new lines by subtracting the regions common to both NL lines and NV volumes (the intersection) from the NL lines. The intersection can be a line(s) or point(s). If the intersection is a point and SEPO is blank, the NL1 line is divided at the point and the resulting lines will be connected, sharing a common keypoint where they touch. If SEPO is set to SEPO, NL1 is divided into two unconnected lines with separate keypoints where they touch. 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. LSBL,ALL,ALL will have no effect since all the lines (in NL1) will be unavailable as NL2 lines.

Main Menu >Preprocessor >Operate >Line by Volu

Menu Paths

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

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

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

PREP7:Booleans

	Mp Me St DY LP Th E3 E2 FL PP ED

Line (or lines, if picking is used) to be subtracted from. If NL=ALL, use all selected lines. If NL = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may also be input for NL.

Behavior of the created boundary.

<blank> - The resulting lines will share keypoint(s) where they touch.

SEPO - The resulting lines will have separate, but coincident keypoint(s).

Specifies whether NL lines are to be deleted:

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

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

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

Generates new lines by subtracting the intersection of the working plane from the NL lines. The intersection will be a keypoint(s). The working plane must not be in the same plane as the NL line(s). If SEPO is blank, the NL line is divided and the resulting lines will be connected, sharing a common keypoint where they touch. If SEPO is set to SEPO, NL is divided into two unconnected lines with separate keypoints. 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. Areas that completely contain the input lines will be updated if the lines are divided by this operation.

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

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

Menu Paths (IGES Only)

Main Menu >Preprocessor >Operate >Line by WrkPlane

Clears loads and load step options from the database.

SOLUTION:LoadStepOperations

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

Label identifying the data to be cleared:

SOLID - Delete only solid model loads.

FE - Delete only finite element loads.

INER - Delete only inertia loads (ACEL, etc.).

LFACT - Initialize only load factors (on DCUM, FCUM, SFCUM, etc.).

LSOPT - Initialize only load step options.

ALL - Delete all loads and initialize all load step options and load factors.

Loads are deleted, and load step options are initialized to their default values.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Delete >All Load Data >All F.E. Loads

Main Menu >Preprocessor >Loads >Delete >All Load Data >All Inertia Lds

Main Menu >Preprocessor >Loads >Delete >All Load Data >All Loads & Opts

Main Menu >Preprocessor >Loads >Delete >All Load Data >All SolidMod Lds

Main Menu >Preprocessor >Loads >Reset Options

Main Menu >Preprocessor >Loads >Settings >Reset Factors

Main Menu >Solution >Delete >All Load Data >All F.E. Loads

Main Menu >Solution >Delete >All Load Data >All Inertia Lds

Main Menu >Solution >Delete >All Load Data >All Loads & Opts

Main Menu >Solution >Delete >All Load Data >All SolidMod Lds

Main Menu >Solution >Reset Options

Main Menu >Solution >Settings >Reset Factors

Deletes load step files.

SOLUTION:LoadStepOperations

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

Range of load step files to be deleted, from LSMIN to LSMAX in steps of LSINC. LSMAX defaults to LSMIN, and LSINC defaults to 1. If LSMIN=ALL, all load step files are deleted (and LSMAX and LSINC are ignored). The load step files are assumed to be named Jobname.Sn, where n is a number assigned by the LSWRITE command (01-09,10,11, etc.). On systems with a 3-character limit on the extension, the "S" is dropped for numbers > 99.

Deletes load step files in the current directory (written by the LSWRITE command).

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Operate >Delete LS Files

Main Menu >Solution >Operate >Delete LS Files

Selects a subset of lines.

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 LINE.

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

Minimum value of item range. Ranges are line numbers, coordinate values, attribute numbers, etc., as appropriate for the item. If VMIN = 0.0, a tolerance of 1.0E-6 is used, or 0.005xVMIN if VMIN=VMAX. 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, ESYS, or NDIV 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 LLIST command for a discussion of signed attributes.

Maximum value of item range. VMAX defaults to VMIN. If VMAXVMIN, a tolerance of 1.0E-8x(VMAX-VMIN) is used.

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

Specifies whether only lines are to be selected:

0 - Select lines only.

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

Notes

Selects lines based on values of a labeled item and component. For example, to select a new set of lines based on line numbers 1 through 7, use LSEL,S,LINE,,1,7. The subset is used when the ALL label is entered (or implied) on other commands, such as LLIST,ALL. Only data identified by line number are selected. Data are flagged as selected and unselected; no data are actually deleted from the database.

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

If ITEM=HPT, the command selects only those lines that contain hard points.

ITEM=RADIUS is only valid for lines that are circular arcs.

LSEL is valid in any processor.

Utility Menu >Select >Entities

Selects those lines contained in the selected areas.

DATABASE:Selecting

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the type of line 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

Selects those lines containing the selected keypoints.

DATABASE:Selecting

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the type of line 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 line keypoints must be selected [KSEL]:

0 - Select line if any of its keypoints are in the selected keypoint set.

1 - Select line only if all of its keypoints are in the selected keypoint set.

This command is valid in any processor.

Utility Menu >Select >Entities

Specifies "Load step operations" 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 >Load Step Operations

Specifies annotation line attributes (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Line color:

0 - Black

1 - Red-Magenta

2 - Magenta

3 - Blue-Magenta

4 - Blue

5 - Cyan-Blue

6 - Cyan

7 - Green-Cyan

8 - Green

9 - Yellow-Green

10 - Yellow

11 - Orange

12 - Red

13 - Dark Gray

14 - Light Gray

15 - White

Line style:

0 - Solid line.

1 - Dashed line.

Line width multiplier (1.0 to 20.0). Defaults to 1.0.

Specifies annotation line attributes to control certain characteristics of the lines created via the /LINE, /LARC, /LSYMBOL, /POLYGON,/PMORE, /PCIRCLE and /PWEDGE commands. This is a command generated by the Graphical User Interface (GUI) and will appear in the log file (Jobname.LOG) if annotation is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Reads load and load step option data into the database.

SOLUTION:LoadStepOperations

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

Identification number of the load step file to be read. Defaults to 1 + highest number read in the current session. Issue LSREAD,STAT to list the current value of LSNUM. Issue LSREAD,INIT to reset LSNUM to 1. The load step files are assumed to be named Jobname.Sn, where n is a number assigned by the LSWRITE command (01-09,10,11, etc.). On systems with a 3-character limit on the extension, the "S" is dropped for LSNUM > 99.

Reads load and load step option data from the load step file into the database. LSREAD will not clear the database of all current loads. However, if a load is respecified with LSREAD, then it will overwrite the existing load. See the LSWRITE command to write load step files, and the LSDELE command to delete load step files. LSREAD removes any existing SFGRAD specification.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Read LS File

Main Menu >Solution >Read LS File

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

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Set of lines (NL1 to NL2 in steps of NINC) that defines the pattern to be scaled. NL2 defaults to NL1, NINC defaults to 1. If NL1=ALL, NL2 and NINC are ignored and the pattern is defined by all selected lines. If NL1 = 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 NL1 (NL2 and NINC are ignored).

Scale factors to be applied to the X, Y, Z keypoint coordinates in 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 line elements associated with the original lines will be generated (scaled) if they exist.

1 - Nodes and line elements will not be generated.

Specifies whether lines will be moved or newly defined:

0 - Additional lines will be generated.

1 - Original lines will be moved to new position (KINC and NOELEM are ignored). Use only if the old lines 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 lines (and their corresponding keypoints and mesh) from a pattern of lines. The MAT, TYPE, REAL, and ESYS attributes are based on the lines in the pattern and not the current settings. Scaling is done in the active coordinate system. Lines in the pattern could have been generated in any coordinate system.

Main Menu >Preprocessor >Operate >Scale >Lines

Reads and solves multiple load steps.

SOLUTION:LoadStepOperations

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

Range of load step files to be read and solved, from LSMIN to LSMAX in steps of LSINC. LSMAX defaults to LSMIN, and LSINC defaults to 1. If LSMIN is blank, a brief command description is displayed. The load step files are assumed to be named Jobname.Sn, where n is a number assigned by the LSWRITE command (01-09,10,11, etc.). On systems with a 3-character limit on the extension, the "S" is dropped for numbers > 99.

LSSOLVE invokes an ANSYS macro to read and solve multiple load steps. The macro loops through a series of load step files written by the LSWRITE command. The macro file called by LSSOLVE is called LSSOLVE.MAC.

Main Menu >Solution >From LS Files

Defines a straight line irrespective of the active coordinate system.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Keypoint at the beginning of line. If P1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI)

Keypoint at the end of line.

Defines a straight line from P1 to P2 using the global Cartesian coordinate system. The active coordinate system will be ignored. The line shape is invariant with the coordinate system after it is generated. Lines may be redefined only if not yet attached to an area.

Main Menu >Preprocessor >Create >Lines >Straight Line

Calculates and prints geometry statistics of the selected lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Calculates and prints geometry statistics (length, centroid, moments of inertia, etc.) associated with the selected lines. Geometry items are reported in the global Cartesian coordinate system. A unit density is assumed, irrespective of any material associations [LATT, MAT]. Items calculated by LSUM and later retrieved by a *GET or *VGET command are valid only if the model is not modified after the LSUM command is issued.

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

Writes load and load step option data to a file.

SOLUTION:LoadStepOperations

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

Number to be assigned to the load step file name for identification purposes. Defaults to 1 + highest LSNUM used in the current session. Issue LSWRITE,STAT to list the current value of LSNUM. Issue LSWRITE,INIT to reset to 1. The load step file will be named Jobname.Sn, where n is the specified LSNUM value (preceded by "0" for values 1-9). On systems with a 3-character limit on the file name extension, the "S" is dropped for LSNUM > 99.

Notes

Writes all load and load step option data for the selected model to a load step file for later use. LSWRITE does not capture changes made to real constants (R) or material properties (MP). Solid model loads, if any, are transferred to the finite element model. Issue LSCLEAR,FE to delete finite element loads. One file is written for each load step. Use the LSREAD command to read a single load step file, and the LSDELE command to delete load step files. Use the LSSOLVE command to read and solve the load steps sequentially.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Write LS File

Main Menu >Solution >Write LS File

Creates annotation symbols (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

X location for symbol (-1.0 < X < 2.0).

Y location for symbol (-1.0 < Y < 1.0).

Symbol orientation angle.

Symbol type:

1 - Arrow.

2 - Tee.

3 - Circle.

4 - Triangle.

5 - Star.

Symbol size multiplier (0.1 to 20.0). Defaults to 1.0.

Defines annotation symbols to be written directly onto the display at a specified location. 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).

All symbols are shown on subsequent displays unless the annotation is turned off or deleted. Use the /LSPEC command to set the attributes of the symbol.

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Generates lines from a line pattern by symmetry reflection.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Symmetry key:

X - X symmetry (default).

Y - Y symmetry.

Z - Z symmetry.

Reflect lines from pattern beginning with NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL, NL2 and NINC are ignored and pattern is all selected lines [LSEL]. If Ncomp = 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 NL1 (NL2 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 lines, if they exist.

1 - Do not generate nodes and elements.

Specifies whether areas will be moved or newly defined:

0 - Generate additional lines.

1 - Move original lines to new position retaining the same keypoint numbers (KINC and NOELEM are ignored). Valid only if the old lines 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 lines (and their corresponding keypoints and mesh) from a given line pattern by a symmetry reflection (see analogous node symmetry command, NSYM). The MAT, TYPE, REAL, and ESYS attributes are based upon the lines 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 Cartesian. Lines in the pattern may have been generated in any coordinate system. However, solid modeling in a toroidal coordinate system is not recommended. Lines are generated as described in the LGEN command.

Main Menu >Preprocessor >Reflect >Lines

Generates a line at the end of, and tangent to, an existing line.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the line the generated line is tangent to. If negative, assume P1 (see below), instead of P2, is the second keypoint of line NL1. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Keypoint at which generated line must end.

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

Location (in the active coordinate system) of the head of the "slope vector" corresponding to the slope at the P3 end of the line. The tail of the vector is at the coordinate system origin.

Generates a line (P2-P3) tangent at end point (P2) of line NL1 (P1-P2).

Main Menu >Preprocessor >Create >Lines >Tangent to Line

Transfers a pattern of lines to another coordinate system.

PREP7:Lines

	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 lines from pattern beginning with NL1 to NL2 (defaults to NL1) in steps of NINC (defaults to 1). If NL1 = ALL, NL2 and NINC are ignored and pattern is all selected lines [LSEL]. If NL1 = 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 NL1 (NL2 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 lines, if they exist.

1 - Do not generate nodes and elements.

Specifies whether lines will be moved or newly defined:

0 - Generate additional lines.

1 - Move original lines to new position retaining the same keypoint numbers (KINC and NOELM are ignored). Valid only if the old lines 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 lines (and their corresponding keypoints and mesh) from one coordinate system to another (see analogous node transfer command, TRANSFER). The MAT, TYPE, REAL, and ESYS attributes are based upon the lines 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. Lines are generated as described in the LGEN command.

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

Specifies a lumped mass matrix formulation.

SOLUTION:AnalysisOptions

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

Formulation key:

OFF - Use the element-dependent default mass matrix formulation (default).

ON - Use a lumped mass approximation.

Notes

This command is also valid in PREP7. If used in SOLUTION, this command is valid only within the first load step.

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Scales the load vector for mode superposition analyses.

SOLUTION:DynamicOptions

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

Scale factor applied to load vector. Defaults to 0.0.

Notes

Specifies the scale factor for the load vector that was created in a modal (ANTYPE=MODAL) analysis. Applies only to the mode superposition transient (ANTYPE=TRANS), mode superposition harmonic response (ANTYPE=HARMIC), and PSD spectrum (pressure PSD) analyses.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Apply >Load Vector >For Mode Super

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

Main Menu >Preprocessor >Loads >Delete >Load Vector >For Mode Super

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

Main Menu >Solution >Apply >Load Vector >For Mode Super

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

Main Menu >Solution >Delete >Load Vector >For Mode Super

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

Defines the working plane normal to a location on a line.

DATABASE:WorkingPlane

	Mp Me St DY LP Th E3 E2 FL PP ED

Window number whose viewing direction will be modified to be normal to the working plane (defaults to 1). If WN is a negative value, the viewing direction will not be modified.

Number of line to be used. If NL1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Location on NL1, specified as a ratio of the line length. Must be between 0.0 and 1.0. If RATIO = P, use graphical picking to specify location on the line.

Notes

Defines a working plane (to assist in picking operations) normal to a location on a line. See WPSTYL command to set the style of working plane display.

This command is valid in any processor.

Utility Menu >WorkPlane >Align WP with >Plane Normal to Line