C

Places a comment in the output.

SESSION:ListControls

	Mp Me St DY LP Th E3 E2 FL PP ED

Comment string, up to 75 characters.

The output from this command consists of two lines - a blank line followed by a line containing C*** and the comment. This command is similar to /COM except that the comment produced by C*** is more easily identified in the output.

Another way to include a comment is to precede it with a ! character (on the same line). The ! may be placed anywhere on the line, and any input following it is ignored as a comment. No output is produced by such a comment, but the comment line is included on the log file. This is a convenient way to annotate the log file.

This command is valid anywhere.

This command cannot be accessed directly in the menu.

Specifies "Calculation 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 >Calculations

Activates cut boundary interpolation (for submodeling).

POST1:SpecialPurpose

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (32 characters maximum) from which to read cut boundary node data. Defaults to Jobname.

File name extension (8 characters maximum). Defaults to NODE if Fname1 is blank.

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

File name (32 characters maximum) to which cut boundary D commands are written (defaults to Jobname).

File name extension (8 characters maximum). Defaults to CBDO if Fname2 is blank.

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

Position on Fname2 to write block of D commands:

0 - Beginning of file (overwrite existing file).

1 - End of file (append to existing file).

Label (8 characters maximum, including the colon) for this block of D commands on Fname2. This label is appended to the colon (:). Defaults to CBn, where n is the cumulative iteration number for the data set currently in the database. For imaginary data (see KIMG on the SET command), Clab defaults to CIn.

Shell-to-solid submodeling key:

0 - Solid-to-solid or shell-to-shell submodel.

1 - Shell-to-solid submodel.

File Fname1 should contain a node list for which boundary conditions are to be interpolated [NWRITE]. File Fname2 is created which contains interpolated boundary conditions written as a block of D commands. Boundary conditions are written for the active degree of freedom set for the element from which interpolation is performed. Interpolation is performed on the selected set of elements. The block of D commands begins with an identifying colon label and ends with a /EOF command. The colon label is of the form :Clab, where Clab is described above. Interpolation from multiple results sets can be performed by looping through the results file in a user-defined macro. Additional blocks can be appended to Fname2 by using KPOS and unique colon labels. A /INPUT command, with the appropriate colon label, may be used to read the block of commands.

Main Menu >General Postproc >Submodeling >Interpolate DOF

Reads a file of solid model and database information into the database.

PREP7:Database

	Mp Me St DY LP Th E3 E2 FL PP ED

Selects which data to read:

ALL - Read all geometry, material property, load, and component data (default). Solid model geometry and loads will be read from the file Fnamei.Exti. All other data will be read from the file Fname.Ext.

DB - Read all database information contained in file Fname.Ext. This file should contain all information mentioned above except the solid model geometry and solid model loads.

SOLID - Read the solid model geometry and solid model loads from the file Fnamei.Exti. This file could have been written by the CDWRITE or IGESOUT command.

COMB - Read the combined solid model and database information from the file Fname.Ext.

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

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

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

File name (32 characters maximum) of IGES file. Defaults to Fname. Used only if Option=ALL or SOLID.

File name extension (8 characters maximum) of IGES file. Defaults to "IGES" if Fnamei is blank.

This command causes coded files of solid model (in IGES format) and database (in command format) information to be read. These files are normally written by the CDWRITE or IGESOUT command. Note that the active coordinate system in these files has been reset to Cartesian (CSYS,0).

This command is valid in any processor.

Main Menu >Preprocessor >Archive Model >Read

Writes geometry and load database items to a file.

PREP7:Database

	Mp Me St DY LP Th E3 E2 FL PP ED

Selects which data to write:

ALL - Write all appropriate geometry, material property, load, and component data (default). Two files will be produced. Fname.Ext will contain all data items mentioned below under "Notes" except the solid model data. Fnamei.Exti will contain the solid model geometry and solid model loads data in the form of IGES commands.

COMB - Write all data mentioned, but to a single file, Fname.Ext. Solid model geometry data will be written in the form of IGES commands, followed by the remainder of the data in the form of ANSYS commands.

DB - Write all database information except the solid model and solid model loads to Fname.Ext in the form of ANSYS commands.

SOLID - Write only the solid model geometry and solid model loads data in the form of IGES commands to Fnamei.Exti.

GEOM - Write only element and nodal geometry data. No solid model geometry data will be written. One file, Fname.Ext, will be produced.

CM - Write only node and element component and geometry data to Fname.Ext.

MAT - Write only material property data (both linear and nonlinear) to Fname.Ext.

LOAD - Write only loads for current load step to Fname.Ext.

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

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

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

File name (8 characters maximum) of IGES file. Defaults to Fname. Used only if Option = ALL or SOLID. Previous data on this file, if any, are overwritten.

File name extension (8 characters maximum) of IGES file. Defaults to "IGES" if blank.

The format of the output file. Defaults to "BLOCKED" if blank.

BLOCKED - Allows faster reading of the output file. The time savings is most significant when BLOCKED is used to read .cdb files associated with very large models.

UNBLOCKED - The format used in versions of ANSYS prior to 5.4. Note that the CDWRITE output of components and assemblies will always be written in the BLOCKED style even if the UNBLOCKED option is specified..

Notes

This command causes certain selected geometry and load database items to be written to a coded file(s) as ANSYS input commands and IGES commands. Geometry data includes solid model geometry data, element types, real constants, coordinate systems, nodes, elements, material properties, coupled degrees of freedom, constraint equations, master degrees of freedom, and offsets. Load data include the current load step only. Loads applied to the solid model (if any) are automatically transferred to the finite element model when this command is issued. Component data include component definitions, but not assembly definitions. Appropriate NUMOFF commands are included at the beginning of the file; this is to avoid overlap of an existing database when the file is read in.

Solid model entities to be written must have all corresponding lower level entities selected (use ALLSEL,BELOW,ALL) before issuing the CDWRITE command. Concatenated lines are not written to the IGES file but instead the lines segments that make up the concatenated lines are written. If, however, an area that contains a concatenated line is encountered the write operation halts (because the such an area could not be recreated during the read operation). If your model has areas that contain concatenated lines, you must first list these and then unconcatenate them before issuing the CDWRITE command. Element order information (i.e. resulting from a WAVES command) is not written. The data in the database remain untouched.

The data may be re-read (on a different machine, for example) with the CDREAD command. Caution: When the file is read in, the NUMOFF,MAT command may cause a mismatch between material definitions and material numbers referenced by certain loads and element real constants. See NUMOFF for details. Also, be aware that the files created by the CDREAD command explicity set the active coordinate system to Cartesian (CSYS, 0).

If you use CDWRITE in any of the derived products (Emag 2-D, Emag 3-D, LinearPlus, LinearPlusThermal, Thermal), then before reading the file, you must edit the Jobname.cdb file to remove commands that are not available in the respective component product.

The CDWRITE command writes the PART information for any ANSYS/LS-DYNA input file to the Jobname.cdb file using the EDPREAD command. Note that EDPREAD is not an ANSYS documented command, it is written only when the CDWRITE command is issued. The PART information can be automatically read into ANSYS with the CDREAD command. However, if more than one Jobname.cdb file is read, the PART list from the last Jobname.cdb file overwrites the existing PART list of the total model. This will affect all PART-related commands contained in the Jobname.cdb file. That means the user can join models, but not PART-related inputs, which the user must modify using the newly-created PART numbers. In limited cases, an update of the PART list (EDWRITE,PUPDATE) is possible. This requires that no used combination of MAT/TYPE/REAL appears more than once in the list. However, partial changes to the PART-related commands may be necessary.

You cannot access this command for models that have been imported from IGES files using the DEFAULT translator (see the IOPTN command).

If you issue the CDWRITE command after generating a beam mesh with orientation nodes, the database file will contain all of the nodes for every beam element, including the orientation nodes. However, the orientation keypoints that were specified for the line [LATT] are no longer associated with the line and are not written out to the geometry file. The line does not recognize that orientation keypoints were ever assigned to it, and the orientation keypoints do not "know" that they are orientation keypoints. Caution: Thus, the CDWRITE command does not support (for beam meshing) any line operation that relies on solid model associativity. For example, meshing the areas adjacent to the meshed line, plotting the line that contains the orientation nodes, or clearing the mesh from the line that contains orientation nodes may not work as expected. For more information about beam meshing, see Chapter 7 of the ANSYS Modeling and Meshing Guide.

This command is also valid in SOLUTION.

In ANSYS/Ed, Option=ALL, COMB, or SOLID is not allowed, and the default is Option=DB.

Main Menu >Preprocessor >Archive Model >Write

Defines a constraint equation relating degrees of freedom.

PREP7:ConstraintEquations

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

Equation reference number (arbitrary). Defaults to highest previous equation number.

Constant term of equation.

Node for first term of equation. If -NODE1, this term is deleted from the equation.

Degree of freedom label for first term of equation. Structural labels: UX, UY, or UZ (displacements); ROTX, ROTY, or ROTZ (rotations, in radians). Thermal labels: TEMP (temperature). Electric labels: VOLT (voltage). Magnetic labels: MAG (scalar magnetic potential); AX, AY, or AZ (vector magnetic potentials).

Coefficient for first node term of equation. If zero, this term is ignored.

Node, label, and coefficient for second term.

Node, label, and coefficient for third term.

Repeat the CE command to add additional terms to the same equation. To change only the constant term, repeat the command with no node terms specified. Only the constant term can be changed during solution, and only with the CECMOD command.

Linear constraint equations may be used to relate the degrees of freedom of selected nodes in a more general manner than described for nodal coupling [CP]. The constraint equation is of the form:

where U(I) is the degree of freedom (displacement, temperature, etc.) of term (I). The following example is a set of two constraint equations, each containing three terms:

2.0 = 6.0 * (2 UX) + 10.0 * (4 UY) + 1.0 * (3 UZ)

The first unique degree of freedom in the equation is eliminated in terms of all other degrees of freedom in the equation. A unique degree of freedom is one which is not specified in any other constraint equation, coupled node set, specified displacement set, or master degree of freedom set. It is recommended that the first term of the equation be the degree of freedom to be eliminated. The first term of the equation cannot contain a master degree of freedom, and no term can contain coupled degrees of freedom. The same degree of freedom may be specified in more than one equation but care must be taken to avoid over-specification (over-constraint).

The degrees of freedom specified in the equation (i.e., UX, UY, ROTZ, etc.) must also be included in the model (as determined from the element types [ET]). Also, each node in the equation must be defined on an element (any element type containing that degree of freedom will do).

Main Menu >Preprocessor >Coupling / Ceqn >Constraint Eqn

Modifies the constant term of a constraint equation during solution.

SOLUTION:LoadStepOptions

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

Reference number of constraint equation.

New value of the constant term of equation.

Other terms of the constraint equation cannot be changed during the solution phase, but must be defined or changed within PREP7 prior to the solution. See the CE command for details.

This command is also valid in PREP7.

Main Menu >Preprocessor >Coupling / Ceqn >Modify ConstrEqn

Main Menu >Preprocessor >Loads >Other >Modify ConstrEqn

Main Menu >Solution >Other >Modify ConstrEqn

Generates the constraint equations for a cyclic symmetry analysis

PREP7:ConstraintEquations

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

Name of a component for the nodes on the low angle edge of the sector. Enclosed in single quotes.

Name of a component for the nodes on the high angle edge of the sector. Enclosed in single quotes.

Number of sectors in the complete 360 degrees.

Nodal diameter to be represented by this set of constraint equations. If NodeDia is -1, generate constraint equations for static cyclic symmetry. If NodeDia is -2, generate constraint equations for static cyclic asymmetry.

A positive tolerance is an absolute tolerance (length units), and a negative tolerance is a tolerance relative to the local element size.

0 - Nodes are not moved.

1 - HIGHNAME component nodes are moved to match LOWNAME component nodes exactly.

0 - Do not print paired nodes

l - Print table of paired nodes

The analysis can be either modal cyclic symmetry or static cyclic symmetry. For modal cyclic symmetry, this command is used within the CYCSOL macro command.

The pair of nodes for which constraint equations are written are rotated into CSYS,1.

This command cannot be accessed directly in the menu.

Deletes constraint equations.

PREP7:ConstraintEquations

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

Delete constraint equations from NEQN1 to NEQN2 (defaults to NEQN1) in steps of NINC (defaults to 1). If NEQN1 = ALL, NEQN2 and NINC will be ignored all constraint equations will be deleted.

Additional node selection control:

ANY - Delete equation set if any of the selected nodes are in the set (default).

ALL - Delete equation set only if all of the selected nodes are in the set.

Main Menu >Preprocessor >Coupling / Ceqn >Del Constr Eqn

Generates constraint equations at an interface.

PREP7:ConstraintEquations

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

Tolerance about selected elements, based on a fraction of the element dimension (defaults to 0.25 (25%)). Nodes outside the element by more than the tolerance are not accepted as being on the interface.

Degrees of freedom for which constraint equations are written. Defaults to all applicable DOFs. DOF1 accepts ALL as a valid label, in which case the rest are ignored (all DOFs are applied).

The allowed "motion" of a node (see explanation below). This distance is in terms of the element coordinates (-1.0 to 1.0). A typical value is 0.05. Defaults to 0 (do not move). MoveTol must be less than or equal to TOLER.

This command can be used to "tie" together two regions with dissimilar mesh patterns by generating constraint equations that connect the selected nodes of one region to the selected elements of the other region. At the interface between regions, nodes should be selected from the more dense mesh region, A, and the elements selected from the less dense mesh region, B. The degrees of freedom of region A nodes are interpolated with the corresponding degrees of freedom of the nodes on the region B elements, using the shape functions of the region B elements. Constraint equations are then written that relate region A and B nodes at the interface.

The "MoveTol" field lets the nodes in the previously mentioned region A change coordinates when slightly inside or outside the elements of region B. The change in coordinates causes the nodes of region A to assume the same surface as the nodes associated with the elements of region B. The constraint equations that relate the nodes at both regions of the interface are then written.

Solid elements with six degrees of freedom should only be interfaced with other six degree-of-freedom elements. The region A nodes should be near the region B elements. A location tolerance based on the smallest region B element length may be input. Stresses across the interface are not necessarily continuous. Nodes in the interface region should not have specified constraints.

Use the CPINTF command to connect nodes by coupling instead of constraint equations. Use the EINTF command to connect nodes by line elements. See also the NSEL and ESEL commands for selecting nodes and elements.

Main Menu >Preprocessor >Coupling / Ceqn >Adjacent Regions

Lists the constraint equations.

PREP7:ConstraintEquations

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

List constraint equations from NEQN1 to NEQN2 (defaults to NEQN1) in steps of NINC (defaults to 1). If NEQN1 = ALL (default), NEQN2 and NINC are ignored and all constraint equations are listed.

Node selection control:

ANY - List equation set if any of the selected nodes are in the set (default).

ALL - List equation set only if all of the selected nodes are in the set.

This command is valid in any processor.

Utility Menu >List >Other >Constraint Eqns >All CE nodes selected

Utility Menu >List >Other >Constraint Eqns >Any CE node selected

Defines a node at the center of curvature of 2 or 3 nodes.

PREP7:Nodes

	Mp Me St DY LP Th E3 E2 FL PP ED

Number to be assigned to the node generated at the center of curvature.

Three nodes used to calculated the center of curvature, as described under RADIUS.

Used to control the interpretation of NODE1, NODE2 and NODE3:

0 - NODE1, NODE2 and NODE3 lie on a circular arc. The program will calculate the center of curvature (and radius) (default).

0 - NODE1 and NODE2 are the endpoints of an arc, and RADIUS is the radius of curvature. The program will locate the center of curvature on the NODE3 side of the NODE1-NODE2 line if RADIUS > 0, and opposite to NODE3 if RADIUS < 0.

Main Menu >Preprocessor >Create >Nodes >At Curvature Ctr

Specifies "Constraint equations" as the subsequent status topic.

PREP7:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

Utility Menu >List >Status >Preprocessor >Constraint Eqns

Defines a rigid region.

PREP7:ConstraintEquations

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

Retained (or master) node for this rigid region. If MASTE = P, then graphical picking of the master and slave nodes is enabled (first node picked will be the master node, and subsequent nodes picked will be slave nodes), and subsequent fields are ignored (valid only in GUI).

Removed (or slave) node for this rigid region. If ALL, slave nodes are all selected nodes.

Degrees of freedom associated with equations:

ALL - All applicable degrees of freedom (default). If 3-D, generate 6 equations based on UX,UY,UZ,ROTX,ROTY,ROTZ; if 2-D, generate 3 equations based on UX,UY,ROTZ.

UXYZ - Translational degrees of freedom. If 3-D, generate 3 equations based on the slave nodes' UX, UY, and UZ DOFs and the master node's UX, UY, UZ, ROTX, ROTY, and ROTZ DOFs; if 2-D, generate 2 equations based on the slave nodes' UX and UY DOFs and the master node's UX, UY, and ROTZ DOFs. No equations are generated for the rotational coupling.

RXYZ - Rotational degrees of freedom. If 3-D, generate 3 equations based on ROTX,ROTY,ROTZ; if 2-D, generate 1 equation based on ROTZ. No equations are generated for the translational coupling.

UX - Slave translational UX degree of freedom only.

UY - Slave translational UY degree of freedom only.

UZ - Slave translational UZ degree of freedom only.

ROTX - Slave rotational ROTX degree of freedom only.

ROTY - Slave rotational ROTY degree of freedom only.

ROTZ - Slave rotational ROTZ degree of freedom only.

Additional degrees of freedom. Used only if more than one degree of freedom required and Ldof is not ALL, UXYZ, or RXYZ.

Defines a rigid region (link, area or volume) by automatically generating constraint equations to relate nodes in the region. Nodes in the rigid region must be assigned a geometric location before this command is used. Also, nodes must be connected to elements having the required degree of freedom set (see Ldof above). Generated constraint equations are based on small deflection theory. Generated constraint equations are numbered beginning from the highest previously defined equation number (NEQN) plus 1. Equations, once generated, may be listed [CELIST] or modified [CE] as desired. Repeat CERIG command for additional rigid region equations.

This command will generate the constraint equations needed for defining rigid lines in two or three-dimensional space. Multiple rigid lines relative to a common point are used to define a rigid area or a rigid volume. In two-dimensional space, with Ldof=ALL, three equations are generated for each pair of constrained nodes. These equations define the three rigid body motions in global Cartesian space, i.e., two in-plane translations and one in-plane rotation. These equations assume the X-Y plane to be the active plane with UX, UY, and ROTZ degrees of freedom available at each node. Other types of equations can be generated with the appropriate Ldof labels.

Six equations are generated for each pair of constrained nodes in three-dimensional space (with Ldof=ALL). These equations define the six rigid body motions in global Cartesian space. These equations assume that UX, UY, UZ, ROTX, ROTY, and ROTZ degrees of freedom are available at each node.

The UXYZ label allows generating a partial set of rigid region equations. This option is useful for transmitting the bending moment between elements having different degrees of freedom at a node. With this option only two of the three equations are generated for each pair of constrained nodes in two-dimensional space. In three-dimensional space, only three of the six equations are generated. In each case the rotational coupling equations are not generated. Similarly, the RXYZ label allows generating a partial set of equations with the translational coupling equations omitted.

Main Menu >Preprocessor >Coupling / Ceqn >Rigid Region

Generates a set of constraint equations from existing sets.

PREP7:ConstraintEquations

	Mp Me St DY LP Th E3 E2 FL PP ED

Do this generation operation a total of ITIMEs, incrementing all nodes in the existing sets by INC each time after the first. ITIME must be >1 for generation to occur.

Generate sets from sets beginning with NSET1 to NSET2 (defaults to NSET1) in steps of NINC (defaults to 1). If NSET1 is negative, NSET2 and NINC are ignored and the last |NSET1| sets (in sequence from maximum set number) are used as the sets to be repeated.

Generates additional sets of constraint equations (with same labels) from existing sets. Node numbers between sets may be uniformly incremented.

Main Menu >Preprocessor >Coupling / Ceqn >Gen w/Same DOF

Defines complex scaling factors to be used with operations.

POST26:Controls

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

Real portion of the complex scale factor used in place of FACTA.

Imaginary portion of the complex scale factor used in place of FACTA.

Real portion of the complex scale factor used in place of FACTB.

Imaginary portion of the complex scale factor used in place of FACTB.

Real portion of the complex scale factor used in place of FACTC.

Imaginary portion of the complex scale factor used in place of FACTC.

Notes

Defines complex scale factors to be used with the operations [ADD, PROD, etc.]. If this command is supplied, these complex factors override any real factors (FACTA, FACTB, FACTC) supplied on the operation commands. Factors are typically involved in scaling a specified variable, such as in the term FACTA x IA of the ADD command to scale variable IA before the ADD operation.

When the CFACT command is active, defaults are as follows: 1) if the complex factor is not specified, but the variable upon which it acts (such as IA) is specified, the factor defaults to 1.0+i0.0; 2) if the variable upon which the factor operates is not specified, but the factor is specified, the variable defaults to 1.0 so that the term in the operation becomes the complex factor itself; 3) if neither the factor nor the variable number is supplied, the term is omitted from the operation. Once the operation (such as the ADD command) has been processed, the CFACT command becomes inactive and must be specified again if it is to be used.

Main Menu >TimeHist Postpro >Math Operations >Complx ScaleFact

Closes the "command" file.

APDL:MacroFiles

	Mp Me St DY LP Th E3 E2 FL PP ED

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Opens a "command" file.

APDL:MacroFiles

	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 CMD if Fname is blank.

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

Determines whether existing file will be overwritten or appended:

(blank) - The existing file will be overwritten.

APPEND - The file will be appended to the existing file.

Data processed with the *VWRITE command will also be written to this file if the file is open when the *VWRITE command is issued.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Writes an ANSYS command (or similar string) to a "command" file.

APDL:MacroFiles

	Mp Me St DY LP Th E3 E2 FL PP ED

Command or string to be written. The standard command form of a label followed by arguments separated by commas is assumed. Command may be a parameter assignment (e.g., *CFWRITE, A=5).

Writes an ANSYS command (or similar string) to the file opened with *CFOPEN. The Command string is not executed (except that numeric and character parameter substitution and operations (with imbedded *,/,>,etc. characters) are performed before writing). When used with *GET results and parameter substitution, an ANSYS command can be created from results and then read back into the ANSYS program (or used elsewhere). For example, if the command *CFWRITE,BF,NNUM,TEMP,TVAL is used in a do-loop, where TVAL is a parameter value returned from the *GET operation and NNUM is a specified or returned parameter value, a series of BF commands, with numerical values substituted for the two parameters, will be written. To create a file without parameter substitution, use *CREATE.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Specifies the origin location of the acceleration coordinate system.

SOLUTION:Inertia

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

Global Cartesian X, Y, and Z coordinates of the acceleration coordinate system origin.

Specifies the origin location of the acceleration coordinate system with respect to the global Cartesian system. The axes of this acceleration coordinate system are parallel to the global Cartesian axes.

A structure may be rotating about the global Cartesian origin [OMEGA, DOMEGA], which may in turn be rotating about another point (the origin of the acceleration coordinate system), introducing Coriolis effects. The location of this point (relative to the global Cartesian origin) is specified with this CGLOC command. For example, if Y is vertical and the global system origin is at the surface of the earth while the acceleration system origin is at the center of the earth, YLOC should be -4000 miles (or equivalent) if the rotational effects of the earth are to be included. The rotational velocity of the global Cartesian system about this point is specified with the CGOMGA command, and the rotational acceleration is specified with the DCGOMG command.

The rotational velocities and accelerations are mainly intended to include mass effects in a static (ANTYPE=STATIC) analysis. If used in dynamic analyses, no coupling exists between the user input terms and the time history response of the structure. See also Section 15.1 of the ANSYS Theory Reference for details. Related commands are ACEL, CGOMGA, DCGOMG, DOMEGA, and OMEGA.

This command is also valid in PREP7.

Main Menu >Preprocessor >FLOTRAN Set Up >Flow Environment >Rotating Coords

Main Menu >Preprocessor >Loads >Apply >Other >Coriolis Effects

Main Menu >Preprocessor >Loads >Delete >Other >Coriolis Effects

Main Menu >Solution >Apply >Other >Coriolis Effects

Main Menu >Solution >Delete >Other >Coriolis Effects

Main Menu >Solution >FLOTRAN Set Up >Flow Environment >Rotating Coords

Main Menu >Solution >Loading Options >Acceleration CS >Delete Accel CS

Main Menu >Solution >Loading Options >Acceleration CS >Set Accel CS

Specifies the rotational velocity of the global origin.

SOLUTION:Inertia

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

Rotational velocity of the global origin about the acceleration system X, Y, and Z axes.

Specifies the rotational velocity of the global origin about each of the acceleration coordinate system axes. The location of the acceleration coordinate system is defined with the CGLOC command. Rotational velocities may be defined in analysis types ANTYPE = STATIC, HARMIC (full), TRANS (full), and SUBSTR. See also Section 15.1 of the ANSYS Theory Reference for details. Units are radians/time. Related commands are ACEL, CGLOC, DCGOMG, DOMEGA, and OMEGA.

This command is also valid in PREP7.

Main Menu >Preprocessor >FLOTRAN Set Up >Flow Environment >Rotating Coords

Main Menu >Preprocessor >Loads >Apply >Other >Coriolis Effects

Main Menu >Preprocessor >Loads >Delete >Other >Coriolis Effects

Main Menu >Solution >Apply >Other >Coriolis Effects

Main Menu >Solution >Delete >Other >Coriolis Effects

Main Menu >Solution >FLOTRAN Set Up >Flow Environment >Rotating Coords

Checks current database items for completeness.

PREP7:Database SOLUTION:AnalysisOptions

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

Specifies which elements are to be checked:

<blank> - Check all data.

ESEL - Check only elements in the selected set and unselect any elements not producing geometry check messages. The remaining elements (those producing check messages) can then be displayed and corrected. A null set results if no elements produce a message. Issue ESEL,ALL to select all elements before proceeding.

Used only with Sele = ESEL:

WARN - Select elements producing warning and error messages.

ERR - Select only elements producing error messages (default).

A similar, automatic check of all data is done before the solution begins. For the FLOTRAN elements FLUID141 and FLUID142, the CHECK command only performs geometry checking.

If the "Check Elements" option is invoked through the GUI (menu path Main Menu>Preprocessor>-Meshing-Check Elems), the CHECK,ESEL logic is used to highlight elements in the following way: good elements are blue, elements having warnings are yellow, and bad (error) elements are red. (Note: The currently selected set of elements is not changed by this GUI function).

This command is also valid in PREP7.

Main Menu >Preprocessor >Sel Bad Elems

Checks area and volume entities for previous meshes.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of component containing areas or volumes.

CHKMSH invokes a predefined ANSYS macro that checks areas and volumes to find out if they were previously meshed. This macro name will appear in the log file (Jobname.LOG) prior to area and volume meshing operations initiated through the GUI. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for use with the /INPUT command).

This command cannot be accessed directly in the menu.

Generates circular arc lines.

PREP7:Lines

	Mp Me St DY LP Th E3 E2 FL PP ED

Keypoint defining the center of the circle (in the plane of the circle). If PCENT = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Radius of the circle. If RAD is blank and PCENT = P, the radius is the distance from PCENT to PZERO.

Keypoint defining axis of circle (along with PCENT). If PCENT = P and PAXIS is omitted, the axis is normal to the working plane.

Keypoint defining the plane normal to circle (along with PCENT and PAXIS) and the zero degree location. Need not be in the plane of the circle.

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

Number of lines around circumference (defaults to minimum required for 90°-maximum arcs, i.e., 4 for 360°). Number of keypoints generated is NSEG for 360° or NSEG+1 for less than 360°.

Generates circular arc lines (and their corresponding keypoints). Keypoints are generated at regular angular locations (based on a maximum spacing of 90°). Arc lines are generated connecting the keypoints. Keypoint and line numbers are automatically assigned, beginning with the lowest available values [NUMSTR]. Adjacent lines use a common keypoint. Line shapes are generated as arcs, regardless of the active coordinate system. Line shapes are invariant with coordinate system after they are generated.

Main Menu >Preprocessor >Create >Arcs >By Cent & Radius

Main Menu >Preprocessor >Create >Arcs >Full Circle

Specifies contour labeling.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Labeling key:

0 or 1 - Label contours with legend or color (default).

-1 - No contour labeling.

N - Same as 1 except show alphabetic legend only on every Nth element.

Notes

Labels contours for identification with alphabetic legend for vector displays and color for raster displays. Number of contours is automatically reduced to 9 (or fewer) for clarity. Use /CONTOUR command to increase (24 maximum for alphabetic labeling; no limit for color labeling).

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Contours >Contour Labeling

Clears the database.

DATABASE:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

File read option:

START - Reread START5x.ANS file (default).

NOSTART - Do not reread START5x.ANS file.

Resets the ANSYS database to the conditions at the beginning of the problem. All items are deleted from the database and memory values are set to zero for items derived from database information. All files are left intact. This command is useful between multiple analyses in the same run, or between passes of a multi-pass analysis (such as between the substructure generation, use, and expansion passes). Should not be used in a do-loop since loop counters will be reset. The START5x.ANS file will be reread (by default) after the database is cleared, unless Read is set to NOSTART. Additional commands cannot be stacked (using the $ separator) on the same line as the /CLEAR command.

Use particular care in placing this command within branching constructs, such as the *DO command and the *IF command. The /CLEAR command doesn't clear the *IF stack and the number of *IF levels is retained. Also, the /CLEAR command doesn't clear the *DO stack, but does delete all parameters including the looping parameter for do-loops. You can preserve your iteration parameter by issuing a PARSAV command before the /CLEAR command and then following that with a PARRES command.

This command is valid only at the Begin level.

Utility Menu >File >Clear & Start New

Defines a local coordinate system relative to the active coordinate system.

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 active coordinate system) of the origin of the new coordinate system (R,,Z for cylindrical, R,, for spherical or toroidal).

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 and activates a local coordinate system by origin location and orientation angles relative to the active coordinate system. This local system becomes the active coordinate system, and is automatically aligned with the active system (i.e., x is radial if a cylindrical system is active, etc.). Nonzero rotation angles (degrees) are relative to this automatic rotation. See the CS, CSKP, CSWPLA, and LOCAL commands for alternate definitions. Local coordinate systems may be displayed with the /PSYMB command.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Copies the session log file to a named file.

SESSION:Files

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (32 characters maximum) to which the log file is to be copied.

File name extension (optional) (8 characters maximum).

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

This command is valid in any processor, but only during an interactive run.

This command cannot be accessed directly in the menu.

Forms the common log of a variable

POST26:Operations

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Reference number of the variable to be operated on.

Unused fields.

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

Unused fields.

Scaling factor applied to variable IA (defaults to 1.0).

Scaling factor (positive or negative) applied to the operation (defaults to 1.0).

Forms the common log of a variable according to the operation:

Menu Paths

Main Menu >TimeHist Postpro >Math Operations >Common Log

Clears meshed entities.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

When you use the GUI method to set the number of elements on specified lines, and any of those lines is connected to one or more meshed lines, areas, or volumes, ANSYS prompts you to determine whether you want to clear the meshed entities. (This occurs only when you perform this operation via the GUI; ANSYS does not prompt you when you use the command method [LESIZE].)

If you answer "yes" to the prompt, the program invokes an ANSYS macro, CLRMSHLN, that clears the meshed entities. This macro name will appear in the log file (Jobname.LOG). This macro is for the ANSYS program's internal use only. 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 cannot be accessed directly in the menu.

Groups geometry items into a component.

DATABASE:Components

	Mp Me St DY LP Th E3 E2 FL PP ED

An alphanumeric name used to identify this component. Cname may be up to 8 characters, beginning with a letter and containing only letters, numbers, and underscores. Component names beginning with an underscore (e.g., _LOOP) are reserved for use by ANSYS and should be avoided. Overwrites a previously defined name.

Label identifying the type of geometry items to be grouped:

VOLU - Volumes.

AREA - Areas.

LINE - Lines.

KP - Keypoints.

ELEM - Elements.

NODE - Nodes.

Components may be further grouped into assemblies [CMGRP]. The selected items of the specified entity type will be stored as the component. Use of this component in the select command [CMSEL] causes all these items to be selected at once, for convenience.

A component is a grouping of some geometric entity that can then be conveniently selected or unselected. Up to 500 components and assemblies may be defined in any ANSYS run, but a component may be redefined by reusing a previous component name. The following entity types may belong to a component: nodes, elements, keypoints, lines, areas, and volumes. A component may contain only 1 entity type, but an individual item of any entity may belong to any number of components. Once defined, the items contained in a component may then be easily selected or unselected [CMSEL]. Components may be listed [CMLIST] and deleted [CMDELE]. Components may also be further grouped into assemblies [CMGRP]. Other entities associated with the entities in a component (e.g., the lines and keypoints associated with areas) may be selected by the ALLSEL command.

An item will be deleted from a component if it has been deleted by another operation (see the KMODIF command for an example). Components are automatically updated to reflect deletions of one or more of their items. Components are automatically deleted and a warning message is issued if all their items are deleted. Assemblies are also automatically updated to reflect deletions of one or more of their components or subassemblies, but are not deleted if all their components and subassemblies are deleted.

This command is valid in any processor.

Utility Menu >Select >Comp/Assembly >Create Component

Changes an existing or creates a new color mapping table.

GRAPHICS:SetUp DISPLAY:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (32 characters maximum). If blank, restore default color map.

File name extension (8 characters maximum).

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

Keyword indicating that a new color map file will be created.

<blank> - Loads existing color map file.

CREATE - Starts CMAP utility and modifies or creates the specified file.

Number of contours to be defined by the CMAP program (max = 128). If no value is specified, CMAP defaults to 9, even if an existing file is being modified.

Notes

Reads the color map file (RGB index specifications) to change from current specifications. Only one color map may be active at a time. See /COLOR for other color controls. Changing the color map in ANSYS with the /CMAP command will change the meaning of the color labels on the /COLOR command.

This command is valid anywhere.

Utility Menu >PlotCtrls >Style >Colors >Load Color Map

Deletes a component or assembly definition.

DATABASE:Components

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of the component or assembly whose definition is to be removed.

Entities contained in the component, or the components within the assembly, are unaffected. Only the grouping relationships are deleted. Assemblies are automatically updated to reflect deletion of their components or subassemblies, but they are not automatically deleted when all their components or subassemblies are deleted.

This command is valid in any processor.

Main Menu >Preprocessor >Size Cntrls >Picked Lines

Utility Menu >Select >Comp/Assembly >Delete Comp/Assembly

Edits an existing component or assembly.

DATABASE:Components

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of the assembly to be edited.

Operation label:

ADD - To add more components. The level of any assembly to be added must be lower than that of the assembly Aname (see CMGRP command).

DELE - To remove components.

Names of components and assemblies to be added to or deleted from the assembly.

This command is valid in any processor.

Utility Menu >Select >Comp/Assembly >Edit Assembly

Groups components and assemblies into an assembly.

DATABASE:Components

	Mp Me St DY LP Th E3 E2 FL PP ED

An alphanumeric name used to identify this assembly. Aname may be up to 8 characters, beginning with a letter and containing only letters, numbers, and underscores. Overwrites a previously defined Aname (and removes it from higher level assemblies, if any).

Names of existing components or other assemblies to be included in this assembly.

Groups components and other assemblies into an assembly identified by a name. CMGRP is used for the initial definition of an assembly. An assembly is used in the same manner as a component. Up to 5 levels of assemblies within assemblies may be used.

An assembly is a convenient grouping of previously defined components and other assemblies. Assemblies may contain components only, other assemblies, or any combination. A component may belong to any number of assemblies. Up to 5 levels of nested assemblies may be defined. Components and assemblies may be added to or deleted from an existing assembly by the CMEDIT command. Once defined, an assembly may be listed, deleted, selected, or unselected using the same commands as for a component. Assemblies are automatically updated to reflect deletions of one or more of their components or lower-level assemblies. Assemblies are not automatically deleted when all their components or subassemblies are deleted.

This command is valid in any processor.

Utility Menu >Select >Comp/Assembly >Create Assembly

Lists the contents of a component or assembly.

DATABASE:Components

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of the component or assembly to be listed (if blank, list all components and assemblies).

This command is valid in any processor. It lists only components, and is typically used to list the defined components that make up an assembly or complex component.

Utility Menu >List >Other >Components

Utility Menu >Select >Comp/Assembly >List Comp/Assembly

Plots the entities contained in a component or assembly.

DATABASE:Components

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of the component or assembly to be plotted.

blank - All selected components and assemblies are plotted (default). If fewer than 11 components are selected, then all are plotted. If more than 11 components are selected, then only the first 11 are plotted.

N - Next set of defined components and assemblies is plotted.

P - Previous set of defined components and assemblies is plotted.

Cname - The specified component or assembly is plotted.

Set No. - The specified set number is plotted.

Components are plotted with their native entities. For assemblies, all native entities for the underlying component types are plotted simultaneously. Only a maximum of 11 components or assemblies can be plotted simultaneously.

This command is valid in any processor.

Utility Menu > Plot > Components > Selected Components

Utility Menu > Plot > Components > Next Set

Utility Menu > Plot > Components > Previous Set

Utility Menu > Plot > Components > By Name / Set Number

Selects a subset of components and assemblies.

DATABASE:Components

	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 - Select all components.

NONE - Unselect all components.

Name of component or assembly whose items are to be selected (valid only if Type=S,R,A, or U).

Selecting by component is a convenient alternate to individual item selection (e.g., VSEL, ESEL, etc.).

If Type=R for an assembly selection [CMSEL,R,<assembly-name>], the reselect operation is performed on each component in the assembly in the order in which the components make up the assembly. Thus, if one reselect operation results in an empty set, subsequent operations will also result in empty sets. For example, if the first reselect operation tries to reselect node 1 from the selected set of nodes 3, 4, and 5, the operation results in an empty set (that is, no nodes are selected). Since the current set is now an empty set, if the second reselect operation tries to reselect any nodes, the second operation also results in an empty set, and so on. This is equivalent to repeating the command CMSEL,R,<component-name> once for each component making up the assembly.

This command is valid in any processor.

Utility Menu >Select >Comp/Assembly >Select All

Utility Menu >Select >Comp/Assembly >Select Comp/Assembly

Utility Menu >Select >Comp/Assembly >Select None

Sets convergence values for nonlinear analyses.

SOLUTION:NonlinearOptions

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

Valid convergence labels are as follows: If STAT, list the status of the currently specified criteria. Structural labels: U (displacements); ROT (rotations); F (forces); M (moments). Thermal labels: TEMP (temperature); HEAT (heat flow). Fluid labels: PRES (pressures); V (velocities); FLOW (fluid flow); VF (fluid force). Electric labels: VOLT (voltage); EMF (electromotive force); CURR (current flow); AMPS (current flow); CURT (current flow). Magnetic labels: MAG (scalar magnetic potential); A (vector magnetic potentials); CURR (current flow); FLUX (scalar magnetic flux); CSG (magnetic current segments); VLTG (voltage drop).

Typical value for the above label for this analysis. If negative, and if this convergence label was previously specified explicitly, then convergence based on this label is removed. (A negative VALUE will not remove a default convergence label.) Defaults to the maximum of a program calculated reference or MINREF. For degrees of freedom, the reference is based upon the selected NORM and the current total DOF value. For forcing quantities, the reference is based upon the selected NORM and the applied loads.

When SOLCONTROL,ON, tolerance about VALUE. Defaults to 0.005 (0.5%) for force and moment, and 0.05 (5%) for displacement when rotational DOFs are not present. When SOLCONTROL,OFF, defaults to 0.001 (0.1%) for force and moment.

Specifies norm selection:

2 - L2 norm (check SRSS value) (default).

1 - L1 norm (check absolute value sum).

0 - Infinite norm (check each DOF separately).

The minimum value allowed for the program calculated reference value. If negative, no minimum is enforced. Used only if VALUE is blank. Defaults to 0.01 for force and moment convergence, 1.0E-6 for heat flow, and 0.0 otherwise. When SOLCONTROL,OFF, defaults to 1.0 for force and moment convergence. The default (1.0E-6) for heat flow and others are independent of the SOLCONTROL setting.

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.

Values may be set for the degrees of freedom (DOF) and/or the out-of-balance load for the corresponding forcing quantities. When the GUI is on, if a "Delete" operation in a "Nonlinear Convergence Criteria" dialog box writes this command to a log file (Jobname.LOG or Jobname.LGW), you will observe that Lab is blank, VALUE=-1, and TOLER is an integer number. In this case, the GUI has assigned a value of TOLER that corresponds to the location of a chosen convergence label in the dialog box's list. It is not intended that you type in such a location value for TOLER in an ANSYS session. However, a file that contains a GUI-generated CNVTOL command of this form can be used for batch input or with the /INPUT command.

This command is also valid in PREP7.

Convergence norms specified with CNVTOL may be graphically tracked while the solution is in process using the ANSYS program's Graphical Solution Tracking (GST) feature. Use the /GST command to turn GST on or off. By default, GST is ON for interactive sessions and OFF for batch runs.

Main Menu >Preprocessor >Loads >Nonlinear >Harmonic

Main Menu >Preprocessor >Loads >Nonlinear >Static

Main Menu >Preprocessor >Loads >Nonlinear >Transient

Main Menu >Preprocessor >Loads >Nonlinear >Convergence Crit

Main Menu >Solution >Nonlinear >Harmonic

Main Menu >Solution >Nonlinear >Static

Main Menu >Solution >Nonlinear >Transient

Main Menu >Solution >Nonlinear >Convergence Crit

Specifies the color mapping for various items.

GRAPHICS:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Apply color to the items specified by the following labels:

AXES - Determines the color (specified in next argument, CLAB) that the axes of a graph will be plotted in.

AXNUM - Determines the color (specified in next argument, CLAB) that the numbering on the axes of a graph will be plotted in.

NUM - Discretely numbered items (such as element types, element materials, etc., as shown on the /PNUM command). Also specify number (1 to 11) in the N1 field. For example, /COLOR,NUM,RED,3 will assign the color red to all items having the discrete number 3 (material displays would show elements having material 3 as red).

OUTL - Outline of elements, areas, and volumes. Ex: /COLOR,OUTL,BLUE.

ELEM - Elements.

LINE - Solid model lines. Use N1, N2, NINC fields for line numbers.

AREA - Solid model areas. Use N1, N2, NINC fields for area numbers.

VOLU - Solid model volumes. Use N1, N2, NINC fields for volume numbers.

ISURF - Isosurfaces (surfaces of constant stress, etc.). This option is particularly useful when capturing frames for animating a single isosurface value.

WBAK - Window background. Use N1, N2, NINC fields for window numbers.

b.c.label - Boundary condition label. Enter U, ROT, TEMP, PRES, V, ENKE, ENDS, SP01 through SP06 or their user-defined names, VOLT, MAG, A, EMF, CURR, F, M, HEAT, FLOW, VF, AMPS, FLUX, CSG, CURT, VLTG, MAST, CP, CE, NFOR NMOM, RFOR, RMOM, PATH. See the /PBC command for boundary condition label definitions.

GRBAK - Graph background.

GRID - Graph grid lines.

AXLAB - Graph X and Y axis labels.

CURVE - Graph curves (identify curve numbers (1-6) in N1, N2, NINC fields).

CM - Component group. Use N1 field for component name, ignore N2 and NINC.

CNTR - ANSYS contour stress colors. The maximum number of contours available is 128.

SMAX - Specifies that all stress values above the maximum value entered in /CONTOUR will be displayed in the color designated in the Clab field. Defaults to dark grey.

SMIN - Specifies that all stress values below the minimum value entered in /CONTOUR will be displayed in the color designated in the Clab field. Defaults to dark grey.

Valid color labels are:

MRED - Magenta-Red

CBLU - Cyan-Blue

YGRE - Yellow-Green

DGRA - Dark Gray

MAGE - Magenta

CYAN - Cyan

YELL - Yellow

LGRA - Light Gray

BMAG - Blue-Magenta

GCYA - Green-Cyan

ORAN - Orange

WHIT - White

BLUE - Blue

GREE - Green

RED - Red

BLAC - Black

Apply color to Lab items numbered N1 to N2 (defaults to N1) in steps of NINC (defaults to 1). If N1 is blank, apply color to entire selected range. If Lab is CM, use component name for N1 and ignore N2 and NINC. Used only with labels as noted above.

Notes

Issue /COLOR,STAT to display the current color mapping. Issue /COLOR,DEFA to reset the default color mapping. Note, color labels may also be reassigned any "color" with the /CMAP command.

This command is valid anywhere.

Utility Menu >PlotCtrls >Style >Colors >BC Colors

Utility Menu >PlotCtrls >Style >Colors >Component Colors

Utility Menu >PlotCtrls >Style >Colors >Entity Colors

Utility Menu >PlotCtrls >Style >Colors >Graph Colors

Utility Menu >PlotCtrls >Style >Colors >Numbered Item Colors

Utility Menu >PlotCtrls >Style >Colors >Window Colors

Places a comment in the output.

SESSION:ListControls

	Mp Me St DY LP Th E3 E2 FL PP ED

Comment string, up to 75 characters.

The output from this command consists of the comment string. This command is similar to C*** except that the comment produced by C*** is more easily identified in the output.

Another way to include a comment is to precede it with a ! character (on the same line). The ! may be placed anywhere on the line, and any input following it is ignored as a comment. No output is produced by such a comment, but the comment line is included on the log file. This is a convenient way to annotate the log file.

This command is valid anywhere.

This command cannot be accessed directly in the menu.

Creates a conical volume anywhere on the working plane.

PREP7:Primitives

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

Working plane X and Y coordinates of the center axis of the cone.

Radii of the faces of the cone. RAD1 defines the bottom face and will be located on the working plane. RAD2 defines the top face and is parallel to the working plane. A value of zero or blank for either RAD1 or RAD2 defines a degenerate face at the center axis (i.e., the vertex of the cone). The same value for both RAD1 and RAD2 defines a cylinder instead of a cone.

The perpendicular distance (either positive or negative based on the working plane Z direction) from the working plane representing the depth of the cone. DEPTH cannot be zero (see Notes below).

Defines a solid conical volume with either the vertex or a face anywhere on the working plane. The cone must have a spatial volume greater than zero. (i.e., this volume primitive command cannot be used to create a degenerate volume as a means of creating an area.) The face or faces will be circular (each area defined with four lines), and they will be connected with two areas (each spanning 180°). See the CONE command for an alternate way to create cones.

Main Menu >Preprocessor >Create >Cone

Menu Paths

Main Menu >Preprocessor >Create >Cone >By Picking

Creates a conical volume centered about the working plane origin.

PREP7:Primitives

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

Radii of the bottom and top faces of the cone. A value of zero or blank for either RBOT or RTOP defines a degenerate face at the center axis (i.e., the vertex of the cone). The same value for both RBOT and RTOP defines a cylinder instead of a cone.

Working plane Z coordinates of the cone. The smaller value is always associated with the bottom face.

Starting and ending angles (either order) of the cone. Used for creating a conical sector. The sector begins at the algebraically smaller angle, extends in a positive angular direction, and ends at the larger angle. The starting angle defaults to 0° and the ending angle defaults to 360°. See the ANSYS Modeling and Meshing Guide for an illustration.

Defines a solid conical volume centered about the working plane origin. The non-degenerate face (top or bottom) is parallel to the working plane but not necessarily coplanar with (i.e., "on") the working plane. The cone must have a spatial volume greater than zero. (i.e., this volume primitive command cannot be used to create a degenerate volume as a means of creating an area.) For a cone of 360°, top and bottom faces will be circular (each area defined with four lines), and they will be connected with two areas (each spanning 180°). See the CON4 command for an alternate way to create cones.

Main Menu >Preprocessor >Create >Cone >By Dimensions

Assigns values to ANSYS configuration parameters.

SESSION:RunControls

	Mp Me St DY -- -- -- -- FL PP --

Configuration parameter to be changed:

NRES - VALUE is maximum number of results sets (substeps) allowed on the result file. Defaults to 1000. Minimum is 10.

NBUF - VALUE is number of buffers (1 to 32) per file in the solver. Defaults to 4.

NPROC - VALUE is number of processors (system dependent). Defaults to 1.

LOCFL - File open and close actions. For VALUE use: 0 for global (default); 1 for local. Applicable to File.EROT, File.ESAV, File.EMAT, and File.TRI. Typically used for large problems where locally closed files may be deleted earlier in the run with the /FDELE command.

SZBIO - VALUE is record size (1024 to 4194304) of binary files (in integer words). Defaults to 16384 (system dependent).

NCONT - VALUE is size (number of elements) of contact surface database. Must be large enough to hold all contact elements that are near or in contact. Defaults to 1000. Minimum is zero.

ORDER - Automatic reordering scheme. For VALUE use: 0 for WSORT,ALL; 1 for WAVES; 2 for both WSORT,ALL and WAVES (default).

FSPLIT - Defines split points for binary files. VALUE is the file split point in megawords and defaults to the maximum file size for the system.

MXND - Maximum number of nodes. If not specified, defaults to 100 at first encounter. Dynamically expanded by doubling, even at first encounter, when maximum is exceeded.

MXEL - Maximum number of elements. Default and expansion as for MXND.

MXKP - Maximum number of keypoints. Default and expansion as for MXND

MXLS - Maximum number of lines. Default and expansion as for MXND.

MXAR - Maximum number of areas. Default and expansion as for MXND.

MXVL - Maximum number of volumes. Default and expansion as for MXND.

MXRL - Maximum number of sets of real constants (element attributes). Default and expansion as for MXND.

MXCP - Maximum number of sets of coupled degrees of freedom. Default and expansion as for MXND.

MXCE - Maximum number of constraint equations. Default and expansion as for MXND.

NLCONTROL- Toggle solution control on or off at the system configuration level. Default value is 1 (ON).

Value (an integer number) assigned to the configuration parameter.

All configuration parameters have initial defaults, which in most cases do not need to be changed. Where a specially configured version of the ANSYS program is desired, the parameters may be changed with this command. Issue /CONFIG,STAT to display current values. Changes must be defined before the parameter is required. These changes (and others) may also be incorporated into the CONFIG5x.ANS file which is read upon execution of the program (see the ANSYS Basic Analysis Procedures Guide). If the same configuration parameter appears in both the configuration file and this command, this command overrides.

This command cannot be accessed directly in the menu.

Forms the complex conjugate of a variable.

POST26:Operations

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

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

Reference number of the variable to be operated on.

Unused fields.

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

Unused fields.

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

Used only with harmonic analyses (ANTYPE=HARMIC).

Main Menu >TimeHist Postpro >Math Operations >Complex Conjugat

Specifies the uniform contour values on stress displays.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Number of contour values. If VMAX is not specified, NCONT defaults to 9 for XII or WIN32 and to 128 for XIIc or WIN32C. The default for 3-D devices is a smooth continuous shading effect, which is similar to 128.

Minimum contour value. If VMIN = AUTO, automatically calculate contour values based upon NCONT uniformly spaced values over the min-max extreme range. Or, if VMIN = USER, set contour values to those of the last display (useful when last display automatically calculated contours).

Value increment (positive) between contour values. Defaults to (VMAX-VMIN)/NCONT.

Maximum contour value. Ignored if both VMIN and VINC are specified.

Notes

See the /CVAL command for alternate specifications. Values represent contour lines in vector mode, and the algebraic maximum of contour bands in raster mode.

Note-No matter how many contours (NCONT) are specified by /CONTOUR, the actual number of contours that appear on your display depends also on the device name, whether the display is directed to the screen or to a file, the display mode (vector or raster), and the number of color planes. (All these items are controlled by /SHOW settings.) See Chapter 12 of the ANSYS Basic Analysis Procedures Guide for more information on changing the number of contours.

If the current ANSYS graphics are not displayed as Multi-Plots, then the following is true: If the current device is a 3-D device [/SHOW,3D], the model contours in all active windows will be the same, even if separate /CONTOUR commands are issued for each active window. For efficiency, ANSYS 3-D graphics logic maintains a single data structure (segment), which contains precisely one set of contours. The program displays the same segment in all windows. The view settings of each window constitute the only differences in the contour plots in the active windows.

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Contours >Uniform Contours

Copies a file.

SESSION:Files

	Mp Me St DY LP Th E3 E2 FL PP ED

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

File name extension (8 characters maximum).

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

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

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

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

The original file is untouched. Ex: /COPY,A,,,B copies file A to B in the same directory. /COPY,A,DAT,,,,DIR2/ copies file A.DAT to the same name in DIR2 (on a system using "." as a name component separator and "/" as a directory separator). See the ANSYS Operations Guide for details. Only ANSYS binary files should be copied. Use /SYS and system commands to copy other files.

This command is valid only at the Begin Level.

Utility Menu >File >File Operations >Copy

Specifies "Node coupling" as the subsequent status topic.

PREP7:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

Utility Menu >List >Status >Preprocessor >Coupled Sets

Defines PSD cospectral values.

SOLUTION:SpectrumOptions

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

First input PSD table number associated with this spectrum.

Second input PSD table number associated with this spectrum.

PSD cospectral values corresponding to the frequency points [PSDFRQ].

Defines PSD cospectral values to be associated with the previously defined frequency points. Two table references are required since values are off-diagonal terms. Unlike autospectra [PSDVAL], the cospectra can be positive or negative. The cospectral curve segment where there is a sign change is interpolated linearly (the rest of the curve segments use log-log interpolation). For better accuracy, choose as small a curve segment as possible wherever a sign change occurs.

Repeat COVAL command using the same table numbers for additional points (50 maximum per curve). This command is valid for SPOPT,PSD only.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Spectrum >Correlation >Cospectral

Main Menu >Solution >Spectrum >Correlation >Cospectral

Defines (or modifies) a set of coupled degrees of freedom.

PREP7:CoupledDOF

	Mp Me St DY LP Th E3 E2 FL PP ED

Set reference number:

n - Arbitrary set number.

HIGH - The highest defined coupled set number will be used (default, unless Lab=ALL). This option is useful when adding nodes to an existing set.

NEXT - The highest defined coupled set number plus one will be used (default if Lab=ALL). This option automatically numbers coupled sets so that existing sets are not modified.

Degree of freedom label for coupled nodes (in the nodal coordinate system). Defaults to label previously defined with NSET if set NSET already exists. A different label redefines the previous label associated with NSET. Valid labels are: Structural labels: UX, UY, or UZ (displacements); ROTX, ROTY, or ROTZ (rotations) (in radians). Thermal labels: TEMP (temperature). Fluid labels: PRES (pressure); VX, VY, or VZ (velocities). Electric labels: VOLT (voltage); EMF (electromotive force drop); CURR (current). Magnetic labels: MAG (scalar magnetic potential); AX, AY, or AZ (vector magnetic potentials); CURR (current). Explicit analysis labels: UX, UY, or UZ (displacements). If Lab=ALL, sets will be generated for each active degree of freedom (i.e., one set for the UX degree of freedom, another set for UY etc.), and NSET will be automatically incremented to prevent overwriting existing sets. The ALL option cannot be used to modify existing sets-NSET must be a new set number n or NEXT. The degree of freedom set is determined from all element types defined and the DOF command, if used. ALL is the only label applicable to FLOTRAN.

List of nodes to be included in set. Duplicate nodes are ignored. If a node number is input as negative, the node is deleted from the coupled set. The first node in the list is the primary (retained) node. If NODE1 = ALL, NODE2 through NODE17 are ignored and all selected nodes [NSEL] are included in the set. If NODE1 = 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 NODE1.

Do not include the same degree of freedom in more than one coupled set. Repeat CP command for additional nodes.

Coupling degrees of freedom into a set causes the results calculated for one member of the set to be the same for all members of the set. Coupling can be used to model various joint and hinge effects. A more general form of coupling can be done with constraint equations [CE]. For structural analyses, a list of nodes is defined along with the nodal directions in which these nodes are to be coupled. As a result of this coupling, these nodes are forced to take the same displacement in the specified nodal coordinate direction. The amount of the displacement is unknown until the analysis is completed. A set of coupled nodes which are not coincident, or which are not along the line of the coupled displacement direction, may produce an applied moment which will not appear in the reaction forces. The actual degrees of freedom available for a particular node depends upon the degrees of freedom associated with element types [ET] at that node. For example, degrees of freedom available with BEAM3 elements are UX, UY, and ROTZ only. For scalar field analysis, this command is used to couple nodal temperatures, pressures, voltages, etc.

A set of coupled nodes which are not coincident, or which are not along the line of the coupled displacement direction, produce an artificial moment constraint. If the structure rotates, a moment may be produced in the coupled set in the form of a force couple. This moment is in addition to the real reaction forces and may make it appear that moment equilibrium is not satisfied by just the applied forces and the reaction forces.

Additional sets of coupled nodes may be generated from a specified set. Degrees of freedom are coupled within a set but are not coupled between sets. No degree of freedom should appear in more than one coupled set. Such an appearance would indicate that at least two sets were in fact part of a single larger set. The first degree of freedom of the coupled set is the "prime" degree of freedom. All other degrees of freedom in the coupled sets are eliminated from the solution matrices by their relationship to the prime degree of freedom. Forces applied to coupled nodes (in the coupled degree of freedom direction) will be summed and applied to the prime degree of freedom. Output forces are also summed at the prime degree of freedom. Degrees of freedom with specified constraints [D] should not be included in a coupled set (unless the degree of freedom is prime).

If master degrees of freedom are defined for coupled nodes, only the prime degree of freedom should be so defined. The use of coupled nodes reduces the set of coupled degrees of freedom to only one degree of freedom. The wavefront is correspondingly decreased; however, the overall stiffness (or conductivity) matrix formulation time is increased.

Main Menu >Preprocessor >Coupling / Ceqn >Couple DOFs

Main Menu >Preprocessor >Coupling / Ceqn >Cupl DOFs w/Mstr

Deletes coupled degree of freedom sets.

PREP7:CoupledDOF

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Additional node selection control:

ANY - Delete coupled set if any of the selected nodes are in the set (default).

ALL - Delete coupled set only if all of the selected nodes are in the set.

See the CP command for a method to delete individual nodes from a set.

Main Menu >Preprocessor >Coupling / Ceqn >Del Coupled Sets

Defines coupled degrees of freedom at an interface.

PREP7:CoupledDOF

	Mp Me St DY LP Th E3 E2 FL PP ED

Degree of freedom label for coupled nodes (in the nodal coordinate system). If ALL, use all appropriate labels. Valid labels are: Structural labels: UX, UY, or UZ (displacements); ROTX, ROTY, or ROTZ (rotations, in radians). Thermal labels: TEMP (temperature). Fluid labels: PRES (pressure); VX, VY, or VZ (velocities). Electric labels: VOLT (voltage); EMF (electromotive force drop); CURR (current). Magnetic labels: MAG (scalar magnetic potential); AX, AY, or AZ (vector magnetic potentials); CURR (current).

Tolerance for coincidence (based on maximum coordinate difference in each global Cartesian direction for node locations and on angle differences for node orientations). Defaults to 0.0001. Only nodes within the tolerance are considered to be coincident for coupling.

Defines coupled degrees of freedom between coincident nodes (within a tolerance). May be used, for example, to "button" together elements interfacing at a seam, where the seam consists of a series of node pairs. One coupled set is generated for each selected degree of freedom for each pair of coincident nodes. For more than two coincident nodes in a cluster, a coupled set is generated from the lowest numbered node to each of the other nodes in the cluster. Coupled sets are generated only within (and not between) clusters. If fewer than all nodes are to be checked for coincidence, use the NSEL command to select nodes. Coupled set reference numbers are incremented by one from the highest previous set number. Use CPLIST to display the generated sets. Only nodes having the same nodal coordinate system orientations ("coincident" within a tolerance) are included. Use the CEINTF command to connect nodes by constraint equations instead of by coupling. Use the EINTF command to connect nodes by line elements instead of by coupling.

Main Menu >Preprocessor >Coupling / Ceqn >Coincident Nodes

Specifies the cutting plane for section and capped displays.

GRAPHICS:Style

	Mp Me St DY LP Th E3 E2 FL PP ED

Specifies the cutting plane:

0 - Cutting plane is normal to the viewing vector [/VIEW] and passes through the focus point [/FOCUS] (default).

1 - The working plane [WPLANE] is the cutting plane.

Notes

Defines the cutting plane to be used for section and capped displays [/TYPE,,(1,5,or 7)].

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Hidden-Line Options

Generates sets of coupled nodes from an existing set.

PREP7:CoupledDOF

	Mp Me St DY LP Th E3 E2 FL PP ED

Generate sets from existing set NSETF.

Generate sets with these labels (see CP command for valid labels). Sets are numbered as the highest existing set number + 1.

Generates additional sets of coupled nodes (with different labels) from an existing set [CP, CPNGEN]. The same node numbers are included in the generated sets. If all labels of nodes are to be coupled and the nodes are coincident, the NUMMRG command should be used to automatically redefine the node number (for efficiency).

Main Menu >Preprocessor >Coupling / Ceqn >Gen w/Same Nodes

Lists the coupled degree of freedom sets.

PREP7:CoupledDOF

	Mp Me St DY LP Th E3 E2 FL PP ED

List coupled sets from NSET1 to NSET2 (defaults to NSET1) in steps of NINC (defaults to 1). If NSET1 = ALL (default), NSET2 and NINC are ignored and all coupled sets are listed.

Node selection control:

ANY - List coupled set if any of the selected nodes are in the set (default).

ALL - List coupled set only if all of the selected nodes are in the set.

This command is valid in any processor.

Utility Menu >List >Other >Coupled Sets >All CP nodes selected

Utility Menu >List >Other >Coupled Sets >Any CP node selected

Defines, modifies, or adds to a set of coupled degrees of freedom.

PREP7:CoupledDOF

	Mp Me St DY LP Th E3 E2 FL PP ED

Set reference number [CP].

Degree of freedom label [CP].

Include in coupled set nodes NODE1 to NODE2 in steps of NINC (defaults to 1). If NODE1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). If -NODE1, delete range of nodes from set instead of including. A component name may also be substituted for NODE1 (NODE2 and NINC are ignored).

Defines, modifies, or adds to a set of coupled degrees of freedom. May be used in combination with (or in place of) the CP command. Repeat CPNGEN command for additional nodes.

This command cannot be accessed directly in the menu.

Generates sets of coupled nodes from existing sets.

PREP7:CoupledDOF

	Mp Me St DY LP Th E3 E2 FL PP ED

Do this generation operation a total of ITIMEs, incrementing all nodes in the existing sets by INC each time after the first. ITIME must be > 1 for generation to occur.

Generate sets from sets beginning with NSET1 to NSET2 (defaults to NSET1) in steps of NINC (defaults to 1). If NSET1 is negative, NSET2 and NINC are ignored and the last |NSET1| sets (in sequence from the maximum set number) are used as the sets to be repeated.

Generates additional sets of coupled nodes (with the same labels) from existing sets. Node numbers between sets may be uniformly incremented.

Main Menu >Preprocessor >Coupling / Ceqn >Gen w/Same DOF

Specifies the complete quadratic mode combination method.

SOLUTION:SpectrumOptions

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

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

Label identifying the combined mode solution output.

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

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

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

Damping is required for this mode combination method. The CQC command is also valid for PREP7.

Main Menu >Preprocessor >Loads >Spectrum >Mode Combine

Main Menu >Solution >Spectrum >Mode Combine

Opens (creates) a macro file.

APDL:MacroFiles

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (32 characters maximum) to be created.

File name extension (optional) (8 characters maximum).

Directory name (64 characters maximum). Defaults to current directory. Ext and Dir should not be used if file is to be read with the macro Name option of the *USE command.

See the *USE command for a discussion of macros. All commands following the *CREATE command, up to the *END command, are written to the specified file without being executed. An existing file of the same name, if any, will be overwritten. Parameter values are not substituted for parameter names in the commands when the commands are written to the file. Use *CFWRITE to create a file if this is desired. The resulting macro may be executed with a *USE command (which also allows parameters to be passed into the macro) or a /INPUT command (which does not allow parameters to be passed in). Several macros may be stacked into a library file [*ULIB].

This command is valid in any processor.

Utility Menu >Macro >Create Macro

Specifies the creep criterion for automatic time stepping.

SOLUTION:NonlinearOptions

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

Value between 0.0 and 0.25 (defaults to 0.1).

This command is also valid in PREP7. The CUTCONTROL command can be used for the same purpose and is the preferred command.

Main Menu >Preprocessor >Loads >Nonlinear >Creep Criterion

Main Menu >Solution >Nonlinear >Creep Criterion

Defines a local coordinate system by three node locations.

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

Node defining the origin of this coordinate system. If NORIG = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Node defining the positive x-axis orientation of this coordinate system.

Node defining the x-y plane (with NORIG and NXAX) in the first or second quadrant of this coordinate system.

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 and activates a local right-handed coordinate system by specifying three existing nodes: to locate the origin, to locate the positive x-axis, and to define the positive x-y plane. This local system becomes the active coordinate system. See the CLOCAL, CSKP, CSWPLA, and LOCAL commands for alternate definitions. 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 >By 3 Nodes

Locates the singularity for non-Cartesian local coordinate systems.

DATABASE:CoordinateSystem

	Mp Me St DY LP Th E3 E2 FL PP ED

Number of the local coordinate system in which singularity location is to be changed. Must be greater than 10.

Theta singularity location for cylindrical, spherical, and toroidal systems:

0 - Singularity at 180°.

1 - Singularity at 0° (360° ).

Phi singularity location for toroidal systems:

0 - Singularity in phi direction at 180°.

1 - Singularity in phi direction at 0° (360° ).

Notes

Continuous closed surfaces (circles, cylinders, spheres, etc.) have a singularity (discontinuity) at =180°. For local cylindrical, spherical, and toroidal coordinate systems, this singularity location may be changed to 0° (360° ).

An additional, similar singularity occurs in the toroidal coordinate system at =180° and can be moved with KPHI. Additional singularities occur in the spherical coordinate system at =90°, but cannot be moved.

This command is valid in any processor.

Utility Menu >WorkPlane >Local Coordinate Systems >Move Singularity

Deletes local coordinate systems.

DATABASE:CoordinateSystem

	Mp Me St DY LP Th E3 E2 FL PP ED

Delete coordinate systems from KCN1 (must be greater than 10) to KCN2 (defaults to KCN1) in steps of KCINC (defaults to 1). If KCN1 = ALL, KCN2 and KCINC are ignored and all coordinate systems are deleted.

This command is valid in any processor.

Utility Menu >WorkPlane >Local Coordinate Systems >Delete Local CS

Defines a local coordinate system by three keypoint locations.

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

Keypoint defining the origin of this coordinate system. If PORIG = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Keypoint defining the positive x-axis orientation of this coordinate system.

Keypoint defining the x-y plane (with PORIG and PXAXS) in the first or second quadrant of this coordinate system.

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 and activates a local right-handed coordinate system by specifying three existing keypoints: to locate the origin, to locate the positive x-axis, and to define the positive x-y plane. This local system becomes the active coordinate system. See the CLOCAL, CS, CSWPLA, and LOCAL commands for alternate definitions. 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 >By 3 Keypoints

Lists coordinate systems.

DATABASE:CoordinateSystem

	Mp Me St DY LP Th E3 E2 FL PP ED

List coordinate systems from KCN1 to KCN2 (defaults to KCN1) in steps of KCINC (defaults to 1). If KCN1 = ALL (default), KCN2 and KCINC are ignored and all coordinate systems are listed.

This command is valid in any processor.

Utility Menu >List >Other >Local Coord Sys

Defines a local coordinate system at the origin of the working plane.

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

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 and activates a local right-handed coordinate system centered at the origin of the working plane. The coordinate system's local x-y plane (for a Cartesian system) or R- plane (for a cylindrical or spherical system) corresponds to the working plane. This local system becomes the active coordinate system. See the CS, LOCAL, CLOCAL, and CSKP commands for alternate ways to define a local coordinate system. 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 WP Origin

Activates a previously defined coordinate system.

DATABASE:CoordinateSystem

	Mp Me St DY LP Th E3 E2 FL PP ED

Activate coordinate system KCN. KCN may be 0 (Cartesian), 1 (cylindrical), 2 (spherical), 4 or WP (working plane) or any previously defined local coordinate system number (>10). This system becomes the active coordinate system. CSYS,4 or CSYS,WP activates working plane tracking which causes the coordinate system to be updated to follow working plane changes. Working plane tracking can be turned off by activating any other coordinate system instead of system 4 (CSYS,11 for instance).

Notes

Activates a previously defined coordinate system for geometry input and generation. The LOCAL, CLOCAL, CS, CSKP, and CSWPLA commands also activate coordinate systems as they are defined.

Files created through the CDWRITE command have the active coordinate system set to Cartesian (CSYS, 0).

This command is valid in any processor.

Utility Menu >WorkPlane >Change Active CS to >Global Cartesian

Utility Menu >WorkPlane >Change Active CS to >Global Cylindrical

Utility Menu >WorkPlane >Change Active CS to >Global Spherical

Utility Menu >WorkPlane >Change Active CS to >Specified Coord Sys

Utility Menu >WorkPlane >Change Active CS to >Working Plane

Utility Menu >WorkPlane >Offset WP to >Global Origin

Specifies the type of contour display.

GRAPHICS:Style

	Mp Me St DY LP Th E3 E2 FL PP ED

Type of display:

0 - Standard contour display.

1 - Isosurface display.

2 - Particle gradient display.

3 - Gradient triad display.

Maximum dot density for particle gradient display (KEY=2). Density is expressed as dots per screen width (defaults to 30).

Dot size for particle gradient display (KEY=2). Size is expressed as a fraction of the screen width (defaults to 0.0 (single dot width)).

Spherical dot shape precision for particle gradient display (KEY=2). (3-D options are supported only on 3-D devices):

0 - Flat 2-D circular dot.

1 - Flat-sided 3-D polyhedron.

n - 3-D sphere with n (>1) polygon divisions per 90° of radius.

Maximum length of triads for gradient triad display (KEY=3). Value is expressed as a fraction of the screen width (defaults to 0.067).

Notes

Use /CTYPE,STAT to display the current settings. Only the standard contour display [/CTYPE,0) and the isosurface contour display [/CTYPE,1] are supported by PowerGraphics [/GRAPHICS,POWER].

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Contours >Contour Style

Calculates current flow in a two-dimensional conductor.

POST1:Magnetics

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

CURR2D invokes an ANSYS macro which calculates the total current flowing in a conducting body for a two-dimensional planar or axisymmetric magnetic field analysis. The currents may be applied source currents or induced currents (eddy currents). The elements of the conducting region must be selected before this command is issued. The total current calculated by the macro is stored in the parameter TCURR. Also, the total current and total current density are stored on a per-element basis in the element table [ETABLE] with the labels TCURR and JT, respectively. Use the PLETAB and PRETAB commands to plot and list the element table items.

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

Controls time-step cutback during a non-linear solution.

SOLUTION:AnalysisOptions

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

Specifies the criteria for causing a cutback. Possible arguments are

PLSLIMIT - Maximum equivalent plastic strain allowed within a time-step (substep). If the calculated value exceeds the VALUE, ANSYS performs a cutback (bisection). VALUE defaults to 0.15 (15%).

CRPLIMIT - Maximum equivalent creep ratio allowed within a time step (substep). If the calculated value exceeds VALUE, ANSYS performs a cutback (bisection). VALUE defaults to 0.1 (10%).

DSPLIMIT - Maximum incremental displacement within the solution field in a time step (substep). If the maximum calculated value exceeds VALUE, ANSYS performs a cutback (bisection). VALUE defaults to 1.0 x 10⁷.

NPOINT - Number of points in a cycle for a second order dynamic equation, used to control automatic time stepping. If the number of solution points per cycle exceeds VALUE, ANSYS performs a cutback in time step size. VALUE defaults to 13.

NOITERPREDICT - If VALUE is 0 (default), an internal auto time step scheme will predict the number of iterations for nonlinear convergence and perform a cutback earlier than the number of iterations specified by the NEQIT command. This is the recommended option. If VALUE is 1, the solution will iterate (if nonconvergent) to NEQIT number of iterations before a cutback is invoked. It is sometimes useful for poorly-convergent problems, but rarely needed in general.

Numeric value for the specified cutback criterion.

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.

A cutback is a method for automatically reducing the step size when either the solution error is too large or the solution encounters convergence difficulties during a non-linear analysis. Should a convergence failure occur, ANSYS will reduce the time step interval to a fraction of its previous size and automatically continue the solution from the last successfully converged time step. If the reduced time step again fails to converge, ANSYS will again reduce the time step size and proceed with the solution. This process continues until convergence is achieved or the minimum specified time step value is reached.

The CRPLIM command is functionally equivalent to Lab=crplimit.

Main Menu >Preprocessor >Loads >Nonlinear >Cutback Control

Main Menu >Solution >Nonlinear >Cutback Control

Specifies non-uniform contour values on stress displays.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Up to 8 contour values may be specified (in ascending order). The 0.0 value (if any) must not be the last value specified. If no values are specified, all contour specifications are erased and contours are automatically calculated.

Notes

This command is similar to the /CONTOUR command except that each contour value may be explicitly defined instead of generated in a uniformly spaced fashion. If both /CONTOUR and /CVAL are used, only the last is used.

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Contours >Non-uniform Contours

Computes covariance between two quantities.

POST26:SpecialPurpose

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

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

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

Defines the type of response PSD to be calculated:

0,1 - Displacement (default).

2 - Velocity.

3 - Acceleration.

Defines the reference with respect to which covariance is to be calculated:

1 - Absolute value.

2 - Relative to base (default).

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

This command computes the covariance value for the variables referenced by the reference numbers IA and IB. If DATUM=2, the variable referenced by IR will contain the individual modal contributions (i.e., the dynamic or relative values). If DATUM=1, the variable referenced by IR will contain the modal contributions followed by the contributions of pseudo-static and covariance between dynamic and pseudo-static responses. File.PSD must be available for the calculations to occur.

Main Menu >TimeHist Postpro >Calc Covariance

Generates a duplicate of the basic sector in a modal cyclic symmetry analysis.

PREP7:SpecialPurpose

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

This command is used in modal cyclic symmetry analysis to generate a duplicate sector on top of a basic sector which has already been defined by a user. It copies all internal constraint equations and couplings associated with the basic sector to the duplicate sector. CYCGEN requires no arguments.

The basic sector from which the duplicate is made can consist of finite elements, internal constraint equations, and couplings. Superelements are not allowed. The basis sector must have matching nodes on the low and high angle edges. The edges can be of any shape and need not be "flat" in cylindrical space. A proper basic sector serves as a pattern which, when repeated n times in cylindrical space, yields the entire model.

CYCGEN is one of two macros which are used to perform modal cyclic symmetry analysis. The other macro, CYCSOL, is described later in this section of the ANSYS Commands Reference. These macros can also be used for prestressed cases.

Main Menu >Preprocessor >Cyclic Sector

By-passes commands within a do-loop.

APDL:ProcessControls

	Mp Me St DY LP Th E3 E2 FL PP ED

By-passes all commands between this command and the *ENDDO command within a do-loop. The next loop (if applicable) is initiated. The cycle option may also be conditionally executed [*IF]. The *CYCLE command must appear on the same file as the *DO command.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Performs a modal cyclic symmetry analysis.

SOLUTION:DynamicOptions

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

Nodal diameter range of interest.

Number of sectors in the complete 360 degrees.

Component name of the nodes that form the lower angle edge. Enclosed in single quotes. (This field is required.)

Component name of the nodes that form the higher angle edge. Enclosed in single quotes. (This field is optional.)

Tolerance used for making the low and high nodes match

Flag indicating whether nodes should be moved to create matching pairs. Default is 0 (no move).

Flag indicating whether to print out matching pairs of nodes.

This command is used to initiate a modal cyclic symmetry analysis, for which you provide a nodal diameter range (NDMIN and NDMAX), the name of the component comprising the set of nodes at the lower angle (the name of the component comprising the set of nodes at the higher angle is optional), and the number of sectors composing the entire structure.

CYCSOL is one of two macros which are used to perform modal cyclic symmetry analysis. The other macro, CYCGEN, is described earlier in this section of the ANSYS Commands Reference. These macros can also be used for prestressed cases. In postprocessing, the results for the 360° model can be displayed by issuing the EXPAND or /EXPAND command.

It is recommended that you select the Block Lanczos eigensolver as the mode extraction method [MODOPT] when using CYCSOL. Then, select the appropriate Lagrange multiplier constraint equation processing method. (See Chapter 3 of the ANSYS Structural Analysis Guide and the description of the MODOPT command, for more information.)

Main Menu >Preprocessor >Loads >Modal Cyclic Sym

Main Menu >Solution >Modal Cyclic Sym

Creates a circular area or cylindrical volume anywhere on the working plane.

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

Working plane X and Y coordinates of the center of the circle or cylinder.

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

Starting and ending angles (either order) of the circle or faces of the cylinder. Used for creating a partial annulus or partial cylinder. The sector begins at the algebraically smaller angle, extends in a positive angular direction, and ends at the larger angle. The starting angle defaults to 0° and the ending angle defaults to 360°. See the ANSYS Modeling and Meshing Guide for an illustration.

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

Defines a circular area anywhere on the working plane or a cylindrical volume with one face anywhere on the working plane. For a solid cylinder of 360°, the top and bottom faces will be circular (each area defined with four lines) and they will be connected with two surface areas (each spanning 180°). See the CYL5, PCIRC, and CYLIND commands for alternate ways to create circles and rectangles.

When working with a model imported from an IGES file (DEFAULT import option), you must provide a value for DEPTH or the command will be ignored.

Main Menu >Preprocessor >Create >Circle >Annulus

Main Menu >Preprocessor >Create >Circle >Partial Annulus

Main Menu >Preprocessor >Create >Circle >Solid Circle

Main Menu >Preprocessor >Create >Cylinder >Hollow Cylinder

Main Menu >Preprocessor >Create >Cylinder >Partial Cylinder

Main Menu >Preprocessor >Create >Cylinder >Solid Cylinder

Menu Paths (IGES Only)

Main Menu >Preprocessor >Create >Solid Cylindr

Creates a circular area or cylindrical volume by end points.

PREP7:Primitives

	Mp Me St DY LP Th E3 E2 FL PP ED

Working plane X and Y coordinates of one end of the circle or cylinder face.

Working plane X and Y coordinates of the other end of the circle or cylinder face.

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

Defines a circular area anywhere on the working plane or a cylindrical volume with one face anywhere on the working plane by specifying diameter end points. For a solid cylinder of 360°, the top and bottom faces will be circular (each area defined with four lines) and they will be connected with two surface areas (each spanning 180°). See the CYL4, PCIRC, and CYLIND commands for alternate ways to create circles and rectangles.

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

Main Menu >Preprocessor >Create >Cylinder >By End Pts & Z

Creates a cylindrical volume centered about the working plane origin.

PREP7:Primitives

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

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

Working plane Z coordinates of the cylinder. If either Z1 or Z2 is zero, one of the faces of the cylinder will be coplanar with the working plane.

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

Defines a cylindrical volume centered about the working plane origin. The top and bottom faces are parallel to the working plane but neither face need be coplanar with (i.e., "on") the working plane. The cylinder must have a spatial volume greater than zero. (i.e., this volume primitive command cannot be used to create a degenerate volume as a means of creating an area.) For a solid cylinder of 360°, the top and bottom faces will be circular (each area defined with four lines), and they will be connected with two areas (each spanning 180°.) See the CYL4 and CYL5 commands for alternate ways to create cylinders.

Main Menu >Preprocessor >Create >Cylinder >By Dimensions