I

Specifies initial conditions at nodes.

SOLUTION:MiscLoads

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

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

Degree of freedom label for which initial condition is to be specified. If ALL, use all appropriate labels. Structural labels: UX, UY, or UZ (displacements or linear velocities); ROTX, ROTY, or ROTZ (rotations or angular velocities). Thermal label: TEMP (temperature). FLOTRAN fluid labels: PRES (pressure); VX, VY, or VZ (velocities); ENKE or ENDS (turbulent kinetic energy or turbulent energy dissipation); SP01 through SP06 (multiple species mass fractions) or their user-defined names [MSSPEC]. Electric label: VOLT (voltage). Magnetic labels: MAG (scalar magnetic potential); AX, AY, or AZ (vector magnetic potentials).

Initial value of the degree of freedom (first-order value). Defaults to the program default for that DOF (0.0 for structural analysis, TUNIF for thermal analysis, etc.). Values are in the nodal coordinate system and in radians for rotational DOF.

Second-order degree of freedom value, mainly used to specify initial structural velocity. Defaults to the program default for that DOF (0.0 for structural analysis). Values are in the nodal coordinate system and in radians/time for rotational DOF.

Specifies the same initial condition values at the range of nodes from NODE to NEND (defaults to NODE), in steps of NINC (defaults to 1).

The IC command specifies initial conditions, which are the initial values of the specified degrees of freedom. It is valid (with TIMINT,ON) only in the first load step of a transient analysis (full method only for a transient dynamic analysis [TRNOPT,FULL]). Initial conditions should always be step applied [KBC,1] and not ramped. If constraints [D, DSYM, etc.] and initial conditions are applied at the same node, the constraint specification will override. For thermal analyses, any TUNIF specification should be specified before the IC command; otherwise, the TUNIF specification will be ignored. If the IC command is input before any TUNIF specification, use the ICDELE command and then reissue any TUNIF specification and then follow with the IC command.

Caution: Be careful not to define inconsistent initial conditions. For instance, if you define an initial velocity at a single DOF, the initial velocity at every other DOF will be 0.0, potentially leading to conflicting initial conditions. In most cases, you will want to define initial conditions at every unconstrained DOF in your model.

Once a solution has been performed, the specified initial conditions are overwritten by the actual solution and are no longer available. You must respecify them if you want to perform a re-analysis. You may want to keep a database file saved prior to the first solution or write them to the cdwrite file (CDWRITE,LOAD) for subsequent re-use.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Apply >Initial Condit'n >Define

Main Menu >Solution >Apply >Initial Condit'n >Define

Deletes initial conditions at nodes.

SOLUTION:MiscLoads

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

Deletes all initial conditions previously specified with the IC command at all nodes.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Delete >Initial Condit'n

Main Menu >Solution >Delete >Initial Condit'n

Lists the initial conditions.

SOLUTION:MiscLoads

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

List initial conditions for nodes NODE1 to NODE2 (defaults to NODE1) in steps of NINC (defaults to 1). If NODE1=ALL (default), NODE2 and NINC are ignored and initial conditions for all selected nodes [NSEL] are listed. If NODE1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component name may be substituted for NODE1 (NODE2 and NINC are ignored).

Velocity key:

DISP - Specification is for first order degree of freedom value (displacements, temperature, etc.) (default).

VELO - Specification is for second order degree of freedom value (velocities).

Lists the initial conditions specified by the IC command. Listing applies to all the selected nodes [NSEL] and DOF labels. ICLIST is not the same as the DLIST command. All the initial conditions including the default conditions are listed for the selected nodes.

Initial conditions for a FLOTRAN analysis are primary (first order) degrees of freedom and are thus listed with the DISP key.

This command is valid in any processor.

Main Menu >Preprocessor >Loads >Apply >Initial Condit'n >List Picked

Main Menu >Solution >Apply >Initial Condit'n >List Picked

Utility Menu >List >Loads >Initial Conditions >On Picked Nodes

Conditionally causes commands to be read.

APDL:ProcessControls

	Mp Me St DY LP Th E3 E2 FL PP ED

First numerical value (or parameter which evaluates to numerical value) in the conditional comparison operation. VAL1 and VAL2 can also be character strings (enclosed in quotes) or parameters for Oper=EQ and NE only.

Operation label. A tolerance of 1.0E-10 is used for comparisons between real numbers:

EQ - Equal (for VAL1=VAL2).

NE - Not equal (for VAL1VAL2).

LT - Less than (for VAL1<VAL2).

GT - Greater than (for VAL1>VAL2).

LE - Less than or equal (for VAL1VAL2).

GE - Greater than or equal (for VAL1VAL2).

ABLT - Absolute values of VAL1 and VAL2 before < operation.

ABGT - Absolute values of VAL1 and VAL2 before > operation.

Second numerical value (or parameter which evaluates to numerical value) in the conditional comparison operation.

Action based on the logical expression (Oper) being true. If false, continue reading at the next line:

:label - A user-defined label (beginning with a colon (:), 8 characters maximum). The command reader will skip (and wrap to the beginning of the file, if necessary) to the first line that begins with the matching :label. Caution: this label option may not be mixed with do-loop or if-then-else constructs.

STOP - This action will cause an exit from the ANSYS program at this line.

EXIT - Exit the current do-loop [*EXIT].

CYCLE - Skip to the end of the current do-loop [*CYCLE].

THEN - Make this IF an if-then-else construct (see below).

Notes

Conditionally causes commands to be read from a specific block or at a specific location. Ten levels of nested *IF blocks are allowed. Jumping to a :label line is not allowed with keyboard entry. Jumping into, out of, or within a do-loop or an if-then-else construct to a :label line is not allowed.

The following is an example of an if-then-else construct:

*IF,VAL1,Oper,VAL2,THEN
----
*ELSEIF,VAL1,Oper,VAL2
----
*ELSEIF,VAL1,Oper,VAL2
----
*ELSE
----
*ENDIF

where "----" represents a block of any number of commands. Any number of *ELSEIF clauses (or none) may be included (in the location shown). One *ELSE clause (at most) may be included (in the location shown). The *IF command is executed by evaluating its logical expression. If it is true, the block of commands following it is executed. The construct is considered to be complete and the command following the *ENDIF is executed next. If the logical expression is false, the next *ELSEIF command (if any) following the block is executed. The execution logic is the same as for *IF. The effect is that the logical expressions in the *IF and the *ELSEIF commands are sequentially tested until one is found to be true. Then the block of commands immediately following the expression is executed, which completes the execution of the if-then-else construct. If all *IF and *ELSEIF expressions are false, the block following the *ELSE command is executed, if there is one. Only one block of commands (at most) is executed within the if-then-else construct. The *IF, *ELSEIF, *ELSE, and *ENDIF commands for each if-then-else construct must all be read from the same file (or keyboard).

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Transfers IGES data from a file into ANSYS.

AUX15:IGES

	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 CAD if Fname is blank.

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

Reads a file containing IGES data and transfers it into the ANSYS graphics database . The file transferred is the IGES Version 5.1, ASCII format file. IGES (Initial Graphics Exchange Specification) is a neutral format developed by the U.S. Dept. of Commerce, National Institute of Standards and Technology. There is no output transfer file written since the transferred data is read directly into the ANSYS database.

The IOPTN command sets the parameters for reading the file (refer to this command for the options and their support for IGES entities). The two main parameters are DEFAULT and ALTERNATE. When a file is read using the DEFAULT option, the data is stored in an enhanced graphics database.

Once the transferred data is stored, a special set of geometry repair and enhancement tools, designed specifically for use with files imported from CAD systems, are available. Files read through the ALTERNATE option use the standard graphics database.

If an IGES file has already been imported using the DEFAULT parameter for the IOPTN command, you must clear the database before loading a new IGES file (ANSYS will prompt you to do this).

Utility Menu >File >Import

Writes solid model data to a file in IGES Version 5.1 format.

PREP7:Database

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

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

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

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

Attribute key:

0 - Do not write assigned numbers and attributes of the solid model entities to the IGES file (default).

1 - Write assigned numbers and attributes of solid model entities (keypoints, lines, areas, volumes) to the IGES file. Attributes include MAT, TYPE, REAL, and ESYS specifications as well as associated solid model loads and meshing (keypoint element size, number of line divisions and spacing ratio) specifications.

Causes the selected solid model data to be written to a coded file in the IGES Version 5.1 format. Previous data on this file, if any, are overwritten. Keypoints that are not attached to any line are written to the output file as IGES entity 116 (Point). Lines that are not attached to any area are written to the output file as either IGES Entity 100 (Circular Arc), 110 (Line), or 126 (Rational B-Spline Curve) depending upon whether the ANSYS entity was defined as an arc, straight line, or spline. Areas are written to the output file as IGES Entity 144 (Trimmed Parametric Surface). Volumes are written to the output file as IGES entity 186 (Manifold Solid B-Rep Object). Solid model entities to be written must have all corresponding lower level entities selected (use ALLSEL,below,all) before issuing command. Concatenated lines and areas are not written to the IGES file; however, the entities that make up these concatenated entities are written.

Caution: If you issue the IGESOUT command after generating a beam mesh with orientation nodes, the orientation keypoints that were specified for the line [LATT] are no longer associated with the line and are not written out to the IGES 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. Thus the IGESOUT 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. See Chapter 7 of the ANSYS Modeling and Meshing Guide for more information about beam meshing.

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

Utility Menu >File >Export

Forms an imaginary variable from a complex variable.

POST26:Operations

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

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

Reference number of the variable to be operated on.

Unused fields.

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

Unused fields.

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

This command forms a new variable from a complex variable by storing the imaginary part as the real part. The imaginary part can then be used in other operations. Used only with harmonic analyses (ANTYPE=HARMIC).

Main Menu >TimeHist Postpro >Math Operations >Imaginary Part

Allows immediate display of a model as it is generated.

GRAPHICS:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Immediate mode key:

0 - Display only upon request, i.e., no immediate display (default with the GUI off).

1 - Display immediately as model is generated (default with the GUI on).

Notes

Allows immediate display of a model (as it is generated) without a screen erase or a display request. Available only during an interactive session at a graphics display terminal. A valid graphics device name must first be specified on the /SHOW command.

The IMMED command allows you to control whether or not the model is displayed immediately as it is generated in an interactive session. By default in the GUI, your model will immediately be displayed in the Graphics Window as you create new entities (such as areas, keypoints, nodes, elements, local coordinate systems, boundary conditions, etc.). This is called immediate mode graphics. Also note that symbols (such as boundary conditions, local coordinate system triads, etc.) are shown immediately and will be present on subsequent displays unless you "turn off" the appropriate symbol using the GUI plot controls function or the appropriate graphics specification command.

An immediate image will also be automatically scaled to fit nicely within the Graphics Window - a feature called automatic scaling. The new scaling is usually apparent on the automatic replot associated with immediate mode. To suppress automatic replot, issue /UIS,REPLOT,0. (With automatic replot suppressed, the immediate image may not always be automatically scaled correctly.)

Note that an immediate display in progress should not be aborted with the usual system "break" feature (or else the ANSYS session itself will be aborted). When you run the ANSYS program interactively without using the GUI, immediate mode is off by default.

This command is valid only in PREP7.

Utility Menu >PlotCtrls >Erase Options >Immediate Display

Calculates the impedance of a conductor at a reference plane.

POST1:Magnetics

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

Path name for a predefined path [PATH command] for calculating the EMF (voltage drop) from the conductor to a reference point. The path should start at the outer conductor wall and end at a reference voltage point.

Path name for a predefined path [PATH command] for calculating the MMF (current) in a conductor. The path should traverse a closed contour surrounding the conductor, and you should define the path in a counterclockwise direction.

Symmetry factor applied to the calculated EMF (voltage drop). The EMF (voltage drop) from the conductor to the reference point is multiplied by Vsymm.

Symmetry factor applied to the calculated current. The calculated current is multiplied by Isymm.

Used in a harmonic high-frequency electromagnetic analysis, IMPD calculates the impedance of a conductor at a reference plane from the EMF (voltage) and MMF (current) at the reference plane. The EMF (voltage drop) is calculated by a line integral from the input path name (specified by the Vpath argument) that extends from the conductor to a reference point. The MMF (current) is calculated by a closed path around the conductor from the input path name (specified with Ipath). In cases having modeled symmetry, you can multiply the voltage drop or current by symmetry factors (Vsymm and Isymm respectively).

This command macro returns the scalar parameters Zre and Zim, representing the real and imaginary components of the impedance.

See magnetic macros for further details.

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

Switches the input file for the commands that follow.

SESSION:RunControls

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (32 characters maximum) to be read. Defaults to the current Jobname if Ext is specified.

File name extension (8 characters maximum).

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

Line number where file reading is to begin:

0 or 1 - Begins reading at the top (default).

:label - Begins reading at the first line beginning with the matching user-defined label :label (8 characters maximum).

Indicates whether secondary input from this command should be recorded in the command log (File.LOG) and the database log:

0 - Record only the /INPUT command on the log (default).

1 - Record commands in the specified secondary file as they are executed.

Switches the input file for the next commands. Commands are read from this file until an end-of-file or another file switching directive is read. An end-of-file occurs after the last record of the file or when a /EOF command is read. An automatic switch back one level (to the previous file) occurs when an end-of-file is encountered. Twenty levels of nested file switching are allowed. Note, files including *DO, *USE, *ULIB, and the "Unknown Command" Macro have less nesting available because each of these operations also uses a level of file switching. For an interactive run, a /INPUT,TERM switches to the terminal for the next input. A /EOF read from the terminal then switches back to the previous file. A /INPUT (with a blank second field) switches back to the primary input file.

Setting LOG=1 on /INPUT causes all commands read from the specified file to be recorded in the command log (File.LOG) and the internal database command log [LGWRITE]. This option is recommended if the log file will be used later (e.g., as batch input or as an analysis file for design optimization). The LOG=1 option is only valid when the /INPUT occurs in the primary input file. Using LOG=1 on a nested /INPUT or on a /INPUT within a do-loop will have no effect (i.e., commands in the secondary input file are not written to the command log).

This command is valid in any processor.

Utility Menu >File >Read Input from

Identifies the data to be retrieved from the results file.

POST1:Controls

	Mp Me St DY LP Th E3 E2 FL PP ED

Data to be read into the database from the results file. May consist of any of the following labels:

ALL - All solution items (default).

BASIC - NSOL, RSOL, NLOAD, STRS, FGRAD, and FFLUX items.

NSOL - Nodal DOF solution.

RSOL - Nodal reaction loads.

ESOL - Element solution items (includes all of the following):

NLOAD - Element nodal loads.

STRS - Element nodal stresses.

EPEL - Element elastic strains.

EPTH - Element thermal, initial, and swelling strains.

EPPL - Element plastic strains.

EPCR - Element creep strains.

FGRAD - Element nodal gradients.

FFLUX - Element nodal fluxes.

MISC - Element miscellaneous data (SMISC and NMISC).

Identifies the type of data to be retrieved from the results file for placement into the database through commands such as SET, SUBSET, and APPEND. INRES is a companion command to the OUTRES command controlling data written to the database and the results file. Since the INRES command can only flag data that has already been written to the results file, care should be taken when using the OUTRES command to include all data you wish to retrieve for postprocessing later on.

Main Menu >General Postproc >Data & File Opts

Specifies "Inertial loads" as the subsequent status topic.

SOLUTION:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

This command cannot be accessed directly in the menu.

Integrates 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. Table values represent integrated sum of IY to current table position of IX.

Integrate variable IY with respect to IX.

Unused field.

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

Unused fields.

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

Initial value.

Integrates variables according to the operation:

Menu Paths

Main Menu >TimeHist Postpro >Math Operations >Integrate

Integrates nodal results on an exterior surface.

POST1:SpecialPurpose

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

Label indicating degree of freedom to be integrated:

PRES - Pressure.

Integrates nodal results on an exterior surface. Use node selection (such as the EXT option of the NSEL command) to indicate the exterior surface(s) of element faces to be used in the integration. An exterior surface can be "created" by unselecting elements (such as unselecting non-fluid elements that are adjacent to fluid elements for the postprocessing of fluid flow result). Element faces attached to the selected nodes will be automatically determined. All nodes on a face must be selected for the face to be used. The integration results will cancel for nodes on common faces of adjacent selected elements. The integration results are reported in global Cartesian components. Moments are also calculated and are taken about the global origin.

Main Menu >General Postproc >Nodal Calcs >Pressure Integrl

Controls options relating to importing a model.

AUX15:IGES

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the import option. The meanings of VAL1 and VAL2 will vary depending on Lab.

STAT - List overall status of import facilities, including current option values. VAL1 and VAL2 are ignored.

DEFA - Set default values for all import options. VAL1 and VAL2 are ignored.

MERG - Entity merge option. VAL1 can be:

YES - Automatic merging is performed (default).

NO - No merging of entities.

VAL2 is ignored.

SOLID - Solid option. VAL1 can be:

YES - Solid is created automatically (default).

NO - No solid created.

VAL2 is ignored.

GTOLER - Entity merging tolerance. Valid arguments for VAL1 depend on value of IGES. If IGES,DEFAULT, then GTOLER,VAL1 is a numeric value used as a multiplying factor to change the maximum model dimension. If IGES,ALTERNATE, then GTOLER,VAL1 can be:

DEFA - Use system defaults (default).

FILE - Use tolerance from the imported file.

n - A user-specified tolerance value.

VAL2 is ignored.

IGES - IGES import option. VAL1 can be:

STAT - List status of IGES related options.

DEFAULT or RV53 Use enhanced geometry database.

ALTERNATE or RV52 Use IGES revision 5.2 import function. This option is provided for backward compatibility.

SMALL - Small areas option. VAL1 can be:

YES - Small areas are deleted (default).

NO - Small areas are retained.

VAL2 is ignored.

Additional input values as described under each option for Lab.

Notes

Controls various options during a model file transfer (e.g., IGESIN command). A global solid model tolerance (GTOLER) can be specified.

IOPTN,SMALL,YES (default value) will delete small areas and can cause geometrical inconsistencies that could cause the import process to abort. Retaining the small areas will increase processor time and memory usage.

The two IGES translation options, DEFAULT and ALTERNATE, determine which graphics database will be used when IGES files are read into ANSYS. If the DEFAULT option is used (this is preferable in almost all cases), the enhanced graphics database is used and a special set of geometry repair and enhancement tools, designed specifically for use with files imported from CAD systems, are made available. If the ALTERNATE option is chosen, the data is stored in the standard ANSYS graphics database.

The DEFAULT option translates all IGES topological and geometric entities. The option ignores data such as dimensions, text, annotation entities, structure entities, and any IGES entities that the filter doesn't recognize.

The ALTERNATE option is capable of reading in any rational B-spline curve entity (type 126), or rational B-spline surface entity (type 128) with a degree less than or equal to 20. Attempts to read in B-spline curve or surface entities of degree higher than 20 may result in error messages.

If IOPTN, MERG, YES is used, merging of coincident geometry items is performed automatically when the IGESIN command is issued. (In other words, an internal NUMMRG,KP command is issued.) The model will be merged with the consideration tolerance (TOLER on NUMMRG) set to either 1E-4 or the length of the shortest line in the transferred model, whichever is smaller, and an internal solid model tolerance that is relative to the length of the lines attached to the keypoints within consideration. See the NUMMRG command for more information on these tolerances. In most cases, this default merging is appropriate. The IOPTN command should be used when you want to turn off merging operations, override the default merging and specify a global solid model tolerance value (GTOLER), or turn off the automatic creation of solids (SOLID). If used, the IOPTN command should be issued before the IGESIN command.

This command is valid in any processor.

Utility Menu >File >Import

Specifies that inertia relief calculations are to be performed.

SOLUTION:Inertia

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

Calculation key:

0 - No inertia relief calculations.

1 - Counter-balance loads with inertia relief forces.

-1 - Pre-calculate masses for summary printout only (no inertia relief).

Notes

Specifies that the program is to calculate accelerations to counter-balance the applied loads (inertia relief). Displacement constraints on the structure should be only those necessary to prevent rigid-body motions (3 are needed for a 2-D structure and 6 for a 3-D structure). The sum of the reaction forces at the constraint points will be zero. Accelerations are calculated from the element mass matrices and the applied forces. Data needed to calculate the mass (such as density) must be input. Both translational and rotational accelerations may be calculated.

This option applies only to the static (ANTYPE=STATIC) analysis. Nonlinearities, substructures and axisymmetric elements are not allowed. Models with both 2-D and 3-D element types are not recommended. Loads may be input as usual. Displacements and stresses are calculated as usual. Use IRLIST to print inertia relief calculation results. The mass and moment of inertia summary printed before the solution is accurate (because of the additional pre-calculations required for inertia relief). See Section 15.2 of the ANSYS Theory Reference for calculation details. See also the ANSYS Structural Analysis Guide for procedural details.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Other >Inertia Relief

Main Menu >Preprocessor >Loads >Output Ctrls >Incl Mass Summry

Main Menu >Solution >Other >Inertia Relief

Main Menu >Solution >Output Ctrls >Incl Mass Summry

Prints inertia relief summary table.

POST1:Listing

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

Prints the inertia relief summary data, including the mass summary table, the total load summary table, and the inertia relief summary table resulting from the inertia relief calculations. These calculations are performed in the solution phase [SOLVE or PSOLVE] as specified by the IRLF command.

This command is valid in any processor.

This command cannot be accessed directly in the menu.