T

Defines the temperature table for safety factor calculations.

POST1:ElementTable

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

Input up to six temperatures covering the range of nodal temperatures. Temperatures must be input in ascending order.

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

Main Menu >General Postproc >Safety Factor >Reset Temps

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

Activates a data table for nonlinear material properties or special element input.

PREP7:DataTables

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

Type of data table:

BKIN - Bilinear kinematic hardening plasticity. (This and the next seven labels are applicable to the following elements: LINK1, PLANE2, LINK8, PIPE20, BEAM23, BEAM24, PLANE42, SHELL43, SOLID45, SHELL51, PIPE60, SOLID62, SOLID65, PLANE82, SHELL91, SOLID92, SHELL93, SOLID95) The BKIN label is also applicable to these explicit dynamics elements: LINK160, BEAM161, and SOLID164. See also the TBOBT field.

MKIN - Multilinear kinematic hardening plasticity. See also the TBOPT field.

MISO - Multilinear isotropic hardening plasticity. (The MISO label is also applicable to SHELL181, PLANE182, SOLID185, BEAM 188 and BEAM189.)

BISO - Bilinear isotropic hardening plasticity. (The BISO label is also applicable to SHELL181, PLANE182, SOLID185, BEAM188 and BEAM189, and to these explicit dynamics elements: SHELL163, and SOLID164.)

ANISO - Anisotropic plasticity.

DP - Drucker-Prager plasticity.

MELAS - Multilinear elasticity.

USER - User-defined plasticity, viscoplasticity, or hyperelasticity.

KINH - Multilinear kinematic hardening plasticity. (This is also applicable to the following elements: LINK1, PLANE2, LINK8, PIPE20, BEAM23, PLANE42, SHELL43, SOLID45, SHELL51, PIPE60, SOLID62, PLANE82, SOLID92, SHELL93, and SOLID95.) KINH is the same as MKIN with TBOPT=2, but with less restrictions on the number of points per curve and the number of temperatures.

ANAND - Anand plasticity (VISCO106, VISCO107, VISCO108).

CREEP - Creep constants (LINK1, PLANE2, LINK8, PIPE20, BEAM23, BEAM24, PLANE42, SHELL43, SOLID45, SHELL51, PIPE60, SOLID62, SOLID65, PLANE82, SOLID92, and SOLID95).

SWELL - Swelling constants (Applicable to the same elements as CREEP).

BH - Magnetic field data (SOLID5, PLANE13, PLANE53, SOLID62, SOLID96, SOLID98).

PIEZ - Piezoelectric matrix data (SOLID5, PLANE13, SOLID98)

FAIL - Composite material failure data (SOLID46, SHELL91, SHELL99).

MOONEY - Mooney-Rivlin hyperelastic element data (HYPER56, HYPER58, HYPER74, HYPER84, HYPER86, HYPER158, SHELL181 and explicit dynamics elements SHELL163 and SOLID164). See also the TBOPT field.

WATER - Water motion table data (PIPE59).

ANEL - Anisotropic elastic matrix (SOLID5, PLANE13, SOLID64, SOLID98).

CONCR - Concrete element data (SOLID65).

HFLM - Film coefficient data (FLUID116).

FCON - Fluid conductance data (FLUID116).

PFLOW - Pipe flow empirical data (FLUID66).

EVISC - Viscoelastic element data (VISCO88, VISCO89, and explicit dynamics elements BEAM161 and SOLID164).

PLAW - Plasticity laws (explicit dynamics elements BEAM161, SHELL163, and SOLID164). See also the TBOPT field.

FOAM - Foam material models (explicit dynamics element SOLID164). See also the TBOPT field.

HONEY - Honeycomb material models (explicit dynamics element SOLID164).

COMP - Composite material models (explicit dynamics elements SHELL163 and SOLID164).

NL - User-defined data table.

EOS - Equations of state (explicit dynamics elements only). See also the TBOPT field.

Material reference number (defaults to 1).

The number of temperatures for which data will be provided (if applicable). Temperatures are specified on the TBTEMP command. For Lab=MISO and MELAS, the default is 1 and the maximum is 20. For BKIN, BISO, MOONEY, ANEL, CONCR, and FAIL, the default is 6 and the maximum is 6. For KINH the default is 1 and the maximum is 40. For MKIN, the default is 5 and the maximum is 5. For all other labels, this field is ignored. For an explicit dynamics analysis, this field is ignored.

The number of data points to be specified for a given temperature (if applicable). Data points are defined with the TBDATA or TBPT commands. For Lab=MISO, MELAS, and BH, the default is 20 and the maximum is 100. For KINH, the default is 20 and the maximum is 20. For USER, the default is 48 and the maximum is user defined. For all others labels, this field is ignored. For an explicit dynamics analysis, this field is ignored.

Indicates how the material constants will be input. The possible input for this field will vary depending on the type of data table being input (i.e., the Lab value). See the table below for valid TBOPT input.

Indicates which equation of state model will be used. Used only for explicit dynamics.

1 - Linear polynomial equation of state

2 - Gruneisen equation of state

Hyperelastic material options (Lab=MOONEY). This TBOPT input is not needed for an explicit dynamics analysis.

0 - Direct input of hyperelastic material constants (default).

1 - Material constants to be determined from experimental data (for use with the *MOONEY command).

Plasticity options for explicit elements (Lab=PLAW) (no default - must specify).

1 - Isotropic/kinematic hardening model.

2 - Strain rate dependent plasticity model used for metal and plastic forming analyses.

3 - Anisotropic plasticity model (Barlat and Lian).

4 - Strain rate dependent plasticity model used for superplastic forming analyses.

5 - Strain rate dependent isotropic plasticity model used for metal and plastic forming analyses.

6 - Anisotropic plasticity model (Barlat, Lege, and Brem) used for forming processes.

7 - Fully iterative anisotropic plasticity model for explicit shell elements only.

8 - Piecewise linear plasticity model for explicit elements only.

Foam material options for explicit elements (Lab=FOAM) (no default - must specify).

1 - Rigid, closed cell, low density polyurethane foam material model.

2 - Highly compressible urethane foam material model.

3 - Energy absorbing foam material model.

4 - Crushable foam material model (crushes one-dimensionally).

Stress-strain options for BKIN (Lab=BKIN).

0 - No stress relaxation with temperature increase (this is not recommended for nonisothermal problems).

1 - Rice's hardening rule, which takes into account stress relaxation with increasing temperature (default).

Stress-strain options for MKIN (Lab=MKIN).

0 - No stress relaxation with temperature increase (this is not recommended for nonisothermal problems); also produces thermal ratcheting (default).

1 - Recalculate total plastic strain using new weight factors of the subvolume.

2 - Scale layer plastic strains to keep total plastic strain constant; agrees with Rice's model (TB, BKIN with TBOPT=1). Produces stable stress-strain cycles.

Options for Equations of State (Lab=EOS) (no default - must specify).

1 - Johnson-Cook material model - for strain, strain rate, and temperature dependent impact/forming analyses.

2 - Null material model - for allowing equations of state to be considered without computing deviatoric stresses.

TB activates a data table to be used with subsequent TBDATA or TBPT commands. The table space is initialized to zero values. Data from this table are used for certain nonlinear material descriptions as well as for special input for some elements. See the MP command for linear material property input. See Section 2.5 of the ANSYS Elements Reference for a description of table types (Lab) or the elements that require the table for special data. The type of data table remains active until the TB command is reissued. More than one type of data table may be defined for each material (e.g., MISO and CREEP), except that only one type of plasticity/elasticity may be used for each material.

This command is also valid in SOLUTION.

Lab=BH is allowed in ANSYS only with the Emag 3-D and Emag 2-D options. Only Lab=FAIL is allowed in ANSYS/LinearPlus. Only Lab=BH is allowed in ANSYS/Emag 3-D or ANSYS/Emag 2-D.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Define/Activate

Main Menu >Preprocessor >Material Props >Data Tables >Define/Activate

Main Menu >Preprocessor >Material Props >Define MAT Model

Main Menu >Preprocessor >Material Props >Mooney-Rivlin >Define Table

Main Menu >Solution >Other >Change Mat Props >Data Tables >Define/Activate

Copies a data table from one material to another.

PREP7:DataTables

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

Data table label (see the TB command for valid labels).

Material reference number where data table is to be copied from.

Material reference number where data table is to be copied to.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Copy

Main Menu >Preprocessor >Material Props >Data Tables >Copy

Main Menu >Solution >Other >Change Mat Props >Data Tables >Copy

Defines data for the data table.

PREP7:DataTables

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

Starting location in table for entering data. For example, if STLOC=1, data input in the C1 field applies to the first table constant, C2 applies to the second table constant, etc. If STLOC=5, data input in the C1 field applies to the fifth table constant, etc. Defaults to the last location filled + 1. The last location is reset to 1 with each TB or TBTEMP command.

Data values assigned to six locations starting with STLOC. If a value is already in this location, it is redefined. A blank value leaves the existing value unchanged.

Defines data for the table specified on the last TB command at the temperature specified on the last TBTEMP command (if applicable).

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Material Props >Define MAT Model

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Edit Active

Main Menu >Preprocessor >Material Props >Data Tables >Edit Active

Main Menu >Solution >Other >Change Mat Props >Data Tables >Edit Active

Deletes previously defined data tables.

PREP7:DataTables

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

Data table label (see the TB command for valid labels). If ALL, delete all data tables.

Delete tables for materials MAT1 to MAT2 (defaults to MAT1) in steps of INC (defaults to 1). If MAT1 = ALL, ignore MAT2 and INC and delete data tables for all materials.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Delete

Main Menu >Preprocessor >Material Props >Data Tables >Delete

Main Menu >Preprocessor >Material Props >Define MAT Model

Main Menu >Solution >Other >Change Mat Props >Data Tables >Delete

Specifies "Data table properties" 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.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Status

Main Menu >Preprocessor >Material Props >Data Tables >Status

Main Menu >Solution >Other >Change Mat Props >Data Tables >Status

Utility Menu >List >Status >Preprocessor >Data Tables

Lists the data tables.

PREP7:DataTables

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

Data table label (see the TB command for labels). Defaults to the active table. If ALL, list data for all labels.

Material number to be listed (defaults to the active material). If ALL, list data tables for all materials.

This command is a utility command, valid anywhere.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >List

Main Menu >Preprocessor >Material Props >Data Tables >List

Main Menu >Solution >Other >Change Mat Props >Data Tables >List

Utility Menu >List >Properties >Data Tables

Modifies data for the data table (GUI).

PREP7:DataTables

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

The row and column numbers of the table entry to be modified.

The new value to be used in the ROW, COL location.

Modifies data for the table specified on the last TB command. For temperature-dependent data, the temperature specified on the last TBTEMP command is used. This is a command generated by the Graphical User Interface (GUI). It will appear in the log file (Jobname.LOG) if a TB data table is graphically edited in spreadsheet fashion. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Edit Active

Main Menu >Preprocessor >Material Props >Data Tables >Edit Active

Main Menu >Solution >Other >Change Mat Props >Data Tables >Edit Active

Displays the data table.

PREP7:DataTables

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

Data table label. Valid labels are: MKIN, KINH, MELAS, MISO, BKIN, BISO, and BH. Defaults to the active table label. For B-H data, also valid are: NB to display NU-B², MH to display MU vs. H, and SBH, SNB, SMH to display the slopes of the corresponding data.

Material number to be displayed (defaults to the active material).

Only data for stress-strain and B-H curves may be displayed.

This command is valid in any processor.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Graph

Main Menu >Preprocessor >Material Props >Data Tables >Graph

Main Menu >Solution >Other >Change Mat Props >Data Tables >Graph

Utility Menu >Plot >Data Tables

Defines a point on a stress-strain or B-H curve.

PREP7:DataTables

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

Operation to perform:

DEFI - Defines a new data point (default). The point is inserted into the table in ascending order of X. If a point already exists with the same X value, it is replaced.

DELE - Deletes an existing point. The X value must match the X value of the point to be deleted (Y is ignored).

The X value of the point (strain or H).

The corresponding Y value of the point (stress or B).

Defines a point on a stress-strain curve or a B-H curve (depending on the TB command) at the temperature specified on the last TBTEMP command. Valid only for TB command labels MISO, MELAS, KINH, and BH.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Edit Active

Main Menu >Preprocessor >Material Props >Data Tables >Edit Active

Main Menu >Solution >Other >Change Mat Props >Data Tables >Edit Active

Defines a temperature for the data table.

PREP7:DataTables

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

Temperature value (defaults to 0.0 if KMOD is blank).

If blank, TEMP defines a new temperature. If an integer, 1 to NTEMP (from the TB command), modify that previously defined temperature to the TEMP value, unless TEMP is blank, then that previously defined temperature is reactivated. Use TBLIST to list temperatures and data. The next TBDATA or TBPT commands also add or change the data at this temperature. If KMOD=CRIT (and TEMP is blank), the next TBDATA values are failure criteria keys as described for SOLID46, SHELL91, and SHELL99. If KMOD=STRAIN (and TEMP is blank), the next TBDATA values are strains as described for the MKIN property option (see Section 2.5 of the ANSYS Elements Reference).

Defines a temperature to be associated with the data on the subsequent TBPT or TBDATA commands. The temperature remains active until the next TBTEMP command is input. Data values must be defined with the temperatures in ascending order. Temperatures previously associated with a data table may also be modified.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Data Tables >Set Temp Table

Main Menu >Preprocessor >Material Props >Data Tables >Set Temp Table

Main Menu >Solution >Other >Change Mat Props >Data Tables >Set Temp Table

Converts 20-node degenerate tetrahedral elements to their 10-node non-degenerate counterparts.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Name (or the number) of the 20-node tetrahedron element that you want to convert. The value of ELEM1 must be SOLID95, SOLID90, or SOLID122 (or 95, 90, or 122). Only certain combinations of ELEM1 and ELEM2 are allowed; see the Notes section for details. This argument is required.

Name (or the number) of the 10-node tetrahedron element to which you want to convert the ELEM1 elements. The value of ELEM2 must be SOLID92, SOLID87, or SOLID123 (or 92, 87, or 123). Only certain combinations of ELEM1 and ELEM2 are allowed; see the Notes section for details. This argument is required.

Element TYPE reference number for ELEM2. If ETYPE2 is 0 or is not specified, ANSYS chooses the element TYPE reference number for ELEM2. See the Notes section for details. This argument is optional.

Using TCHG, you are limited to converting the combinations of elements that are presented in the following table:

When the TCHG command is issued, only selected elements of type ELEM1 are converted to type ELEM2. ANSYS ignores any elements that are type ELEM1 that are not degenerate tetrahedra; for example, ANSYS will ignore SOLID95 elements that have a hexahedral, pyramidal, or prism shape.

The TCHG command is useful when used in conjunction with the MOPT,PYRA command. Twenty-node pyramid shaped elements may be used in the same volume with 10-node tetrahedra.

Performing a conversion is likely to create circumstances in which more than one element type is defined for a single volume.

If specified, ETYPE2 will usually be the same as the local element TYPE number (ET,ITYPE) that was assigned to ELEM2 with the ET command. You can specify a unique number for ETYPE2 if you prefer. Although ETYPE2 is optional, it may be useful when two or more ITYPEs have been assigned to the same element (for example, if two SOLID92 elements have been established in the element attribute tables for the current model, use the ETYPE2 argument to distinguish between them). If ETYPE2 is non-zero and it has not already been assigned to an element via ET, ANSYS assigns the ETYPE2 value to ELEM2 as its element TYPE reference number.

If ETYPE2 is 0 or is not specified, ANSYS determines the element TYPE reference number for ELEM2 in one of these ways:

· If ETYPE2 is 0 or is not specified, and ELEM2 appears in the element attribute tables, ANSYS uses ELEM2's existing element TYPE reference number for ETYPE2. (If there is more than one occurrence of ELEM2 in the element attribute tables (each with its own TYPE reference number), ANSYS uses the first ELEM2 reference number for ETYPE2.)

See Chapter 7 of the ANSYS Modeling and Meshing Guide for detailed information about converting degenerate tetrahedral elements.

Main Menu >Preprocessor >Modify Mesh >Change Tets

Defines a tee in a piping run.

PREP7:Piping

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

Node where three straight pipes intersect forming a tee (or "Y"). Defaults to last starting branch node [BRANCH].

Type of tee:

WT - Welding tee (default).

UFT - Unreinforced fabricated tee.

Element number to be assigned to first tee leg (defaults to MAXEL + 1).

Element number increment (defaults to 1).

Tee leg lengths (corresponding in order of increasing straight pipe element numbers). Must be less than the straight pipe length. Defaults to 2 x OD of straight pipe (for each leg).

Defines a tee in place of the tee intersection of three previously defined straight pipe elements. See the PREP7 RUN command. The new tee is also composed of three PIPE16 straight pipe elements, but of the leg lengths specified and with the appropriate tee factors calculated. Three new nodes are generated at the ends of the tee. The original three straight pipes are automatically "shortened" to meet the ends of the tee. The tee specifications and loadings are taken from the corresponding three straight pipes.

Main Menu >Preprocessor >Create >Piping Models >Pipe Tee

Specifies various terminal driver options.

DISPLAY:Drivers

	Mp Me St DY LP Th E3 E2 FL PP ED

NCOPY

Activate hard copy device for NCOPY (0,1,2, etc.) copies.

NLOOP

Loop NLOOP times back to beginning of file when end of file is reached.

Pause PAUSE seconds between plots.

KEY

Prompt key:

0 - Display prompt line for prompt.

1 - Use terminal bell for prompt.

Used only with terminal driver names on /SHOWDISP command.

This command is also valid in PREP7.

DISPLAY Program

Sets the time for a load step.

SOLUTION:LoadStepOptions

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

Time at the end of the load step.

Notes

Associates the boundary conditions at the end of the load step with a particular TIME value. TIME must be a positive, nonzero, monotonically increasing quantity that "tracks" the input history. Typically, for the first load step TIME defaults to 1. However, for the first load step of a reduced transient analysis (ANTYPE=TRANS and TRNOPT,REDUC) or mode superposition transient analysis (ANTYPE=TRANS and TRNOPT,MSUP), the TIME command is ignored and a static solution is performed at TIME=0. TIME is not used for the modal (ANTYPE=MODAL), harmonic response (ANTYPE=HARMIC), or substructure (ANTYPE=SUBSTR) analyses. Units of time should be consistent with those used elsewhere (for properties, creep equations, etc.).

This command is also valid in PREP7.

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

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

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

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

Main Menu >Solution >LS-DYNA Controls >Control Options

Specifies the time range for which data are to be stored.

POST26:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Minimum time (defaults to first time (or frequency) point on the file).

Maximum time (defaults to last time (or frequency) point on the file).

Notes

Defines the time (or frequency) range for which data are to be read from the file and stored in memory. Use the NSTORE command to define the time increment.

Main Menu >TimeHist Postpro >Settings >Data

Turns on transient effects.

SOLUTION:DynamicOptions

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

Transient effects key:

OFF - No transient effects (static or steady-state).

ON - Include transient (mass or inertia) effects.

Degree of freedom label:

ALL - Apply this key to all appropriate labels (default).

STRUC - Apply this key to structural DOFs.

THERM - Apply this key to thermal DOFs.

ELECT - Apply this key to electric DOFs.

MAG - Apply this key to magnetic DOFs.

FLUID - Apply this key to fluid DOFs.

Notes

Indicates whether this load step in a full transient analysis should use time integration, that is, whether it includes transient effects (e.g. structural inertia, thermal capacitance) or whether it is a static (steady-state) load step for the indicated DOFs. Transient initial conditions are introduced at the load step having Key=ON. Initial conditions are then determined from the previous two substeps. Zero initial velocity and acceleration are assumed if no previous substeps exist. See the ANSYS Structural Analysis Guide, the ANSYS Thermal Analysis Guide, and the ANSYS Electromagnetic Field Analysis Guide for details.

This command is also valid in PREP7.

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

Main Menu >Solution >Time/Frequenc >Time Integration

Improves the quality of tetrahedral elements that are not associated with a volume.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Identifies the tetrahedral elements to be improved. Valid values are ALL and P. If ELEM=ALL (default), improve all selected tetrahedral elements. If ELEM=P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Specifies whether to allow boundary modification. Boundary modification includes such things as changes in the connectivity of the element faces on the boundary and the addition of boundary nodes. (Also see the Notes section below for important usage information for CHGBND.)

0 - Do not allow boundary modification.

1 - Allow boundary modification (default).

Identifies the level of improvement to be performed on the elements. (Improvement occurs primarily through the use of face swapping and node smoothing techniques.)

0 - Perform the least amount of swapping/smoothing.

1 - Perform an intermediate amount of swapping/smoothing.

2 - Perform the greatest amount of swapping/smoothing.

3 - Perform the greatest amount of swapping/smoothing, plus additional improvement techniques (default).

The TIMP command enables you to improve a given tetrahedral mesh by reducing the number of poorly-shaped tetrahedral elements (in particular, the number of sliver tetrahedral elements)-as well as the overall number of elements-in the mesh. It also improves the overall quality of the mesh.

TIMP is particularly useful for an imported tetrahedral mesh for which no geometry information is attached.

Regardless of the value of the CHGBND argument, boundary midnodes can be moved as long as you are not using p-method analysis. When CHGBND=0 and you are using p-method analysis, boundary midnodes cannot be moved. (ANSYS issues an error message if it would be necessary to move boundary midnodes in order to generate valid quadratic elements.)

When loads or constraints have been placed on boundary nodes or midnodes, and boundary midnodes are later moved, ANSYS issues a warning message to let you know that it will not update the loads or constraints.

No boundary modification is performed if shell or beam elements are present in the mesh, even when CHGBND=1.

Main Menu >Preprocessor >Modify Mesh >Improve Tets >Detached Elems

Defines transient integration parameters.

SOLUTION:DynamicOptions

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

Amplitude decay factor for 2nd order transient integration, e.g. structural dynamics (used only if ALPHA and DELTA are blank). Defaults to 0.005.

2nd order transient integration parameter (used only if GAMMA is blank). Defaults to 0.2525.

2nd order transient integration parameter (used only if GAMMA is blank). Defaults to 0.5050.

1st order transient (e.g. thermal transient) integration parameter. Defaults to 1.0.

Specifies the oscillation limit criterion for automatic time stepping of 1st order transients (e.g., thermal transients). Defaults to 0.5 with a tolerance of TOL.

Tolerance applied to OSLM. Defaults to 0.0.

Used to define the transient integration parameters. In a transient piezoelectric analysis, required input for this command is ALPHA = 0.25, DELTA = 0.5, and THETA = 0.5.

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.

This command is also valid in PREP7.

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

Main Menu >Solution >Time/Frequenc >Time Integration

Defines a main title.

DATABASE:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

Input up to 72 alphanumeric characters. Parameter substitution may be forced within the title by enclosing the parameter name or parametric expression within percent (%) signs.

The title is carried through the printout and written on various files. The title written to a file is the title defined at that time. Special characters may be used within the title text. Subtitles may also be defined [/STITLE].

This command is valid in any processor.

Utility Menu >File >Change Title

Creates annotation text (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

Text string (60 characters maximum). Parameter substitution may be forced within the text by enclosing the parameter name or parametric expression within percent (%) signs.

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

All text is shown on subsequent displays unless the annotation is turned off or deleted. Use the /TSPEC command to set the attributes of the text.

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Specifies the temperature offset from absolute zero to zero.

SOLUTION:AnalysisOptions

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

Degrees between absolute zero and zero of temperature system used (should be positive).

Specifies the difference (in degrees) between absolute zero and the zero of the temperature system used. Absolute temperature values are required in evaluating certain expressions, such as for creep, swelling, radiation heat transfer, MASS71, etc. (The offset temperature is not used in evaluating emissivity.) Examples are 460° for the Fahrenheit system and 273° for the Centigrade system. The offset temperature is internally included in the element calculations and does not affect the temperature input or output. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

Main Menu >Preprocessor >FLOTRAN Set Up >Flow Environment >Ref Conditions

Main Menu >Solution >FLOTRAN Set Up >Flow Environment >Ref Conditions

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Defines and initializes the parameters for topological optimization.

OPTIMIZATION:Specifications

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

The percent of the original volume to be reduced. For example, you would specify VREDUCE=60 to remove 60% of the material. Default=0.

Number of load cases to be treated in a collective manner for topological optimization.

Accuracy used for termination and convergence checking. Default=0.0005.

To treat several load cases collectively (NUMLC>1), use the LSWRITE and LSSOLVE commands to define and solve the analysis.

Main Menu >Solution >Topologic opt

Executes one topological optimization iteration.

OPTIMIZATION:Run

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

This command runs one topological optimization iteration, leading to the prediction of a new shape, defined by means of element densities. You must issue SOLVE or LSSOLVE (if treating multiple load steps) before issuing TOPEXE. This command performs a convergence test based on volume reduction and accuracy as specified by the TOPDEF command.

Main Menu >Solution >Topologic opt

Executes several iterations of topological optimization.

OPTIMIZATION:Run

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

Number of iterations to be performed, with a maximum of 30. Defaults to 1.

Controls the display of topological densities for each iteration:

0 - Do not display the results of each iteration (default).

1 - Display the results of each iteration.

This command invokes an ANSYS macro to solve, postprocess, and plot the shape of each iteration. You must write at least one load step (LSWRITE) before issuing this command. TOPITER uses the LSSOLVE command internally, whether treating single or multiple load steps, as well as PLNSOL,TOPO and TOPEXE for each iteration. This command terminates when either the maximum number of iterations is reached or when convergence occurs, as specified by TOPDEF,,,ACCUR. This command treats single or multiple loads.

Main Menu >Solution >Topologic opt

Calculates torque on a body in a magnetic field.

POST1:Magnetics

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

TORQ2D invokes an ANSYS macro which calculates mechanical torque on a body in a magnetic field. The body must be completely surrounded by air (symmetry permitted), and a closed path [PATH] passing through the air elements surrounding the body must be available. A counter-clockwise ordering of nodes on the PPATH command will give the correct sign on the torque result. The macro is valid for two-dimensional planar analysis.

The calculated torque is stored in the parameter TORQUE. A node plot showing the path is produced in interactive mode. The torque is calculated using a Maxwell stress tensor approach. Path operations are used for the calculation, and all path items are cleared upon completion. See the TORQC2D command for torque calculation based on a circular path.

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

Calculates torque on a body in a magnetic field based on a circular path.

POST1:Magnetics

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

Radius of the circular path. The nodes for the path are created at this radius.

Number of nodes to be created for the circular path. The greater the number of nodes, the higher the accuracy of the torque evaluation. Defaults to 18.

(Optional) Local coordinate system number to be used for defining the circular arc of nodes and the path. Defaults to 99. (If a local system numbered 99 already exists, it will be overwritten by this default.)

TORQC2D invokes an ANSYS macro which calculates the mechanical torque on a body using a circular path. It is used for a circular or cylindrical body such as a rotor in an electric machine. The body must be centered about the global origin and must be surrounded by air elements. The air elements surrounding the path at radius RAD must be selected, and elements with a high-permeability material should be unselected prior to using the macro. The macro is valid for two-dimensional planar analyses only. For a harmonic analysis, the macro calculates the time-average torque. Radial symmetry models are allowed, i.e., the model need not be a full 360-degree model.

The calculated torque is stored in the parameter TORQUE. If the model is not a full 360-degree model, TORQUE should be multiplied by the appropriate factor (such as 4.0 for a 90-degree sector) to obtain the total torque. A node plot showing the path is produced in interactive mode.

The torque is calculated via a circular path integral of the Maxwell stress tensor. The circular path and the nodes for the path are created by the macro at the specified radius RAD. Path operations are used for the calculation, and all path items are cleared upon completion. See the TORQ2D command for torque calculation based on an arbitrary, non-circular path.

Main Menu >General Postproc >Elec&Mag Calc >Circular Torq

Summarizes electromagnetic torque calculations on element components.

POST1:Magnetics

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

Names of existing element components for which Maxwell or virtual work boundary conditions were applied in the preprocessor. Must be enclosed in single quotes (e.g., 'CNAM1') when the command is manually typed in.

TORQSUM invokes an ANSYS macro that summarizes the Maxwell and virtual work torque values. The element components must have had appropriate Maxwell or virtual work boundary conditions established in the preprocessor prior to solution in order to retrieve torques (see the FMAGBC command). The torque values are stored on a per-element basis for the adjacent air layer elements surrounding the components and are retrieved and summed by the macro. For a harmonic analysis, the calculated torque represents a time-average value.

TORQSUM is valid only for two-dimensional planar analysis.

Main Menu >General Postproc >Elec&Mag Calc >Comp. Torque

Creates a toroidal volume.

PREP7:Primitives

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

Three values that define the radii of the torus. You can specify the radii in any order. The smallest of the values is the inner minor radius, the intermediate value is the outer minor radius, and the largest value is the major radius. (There is one exception regarding the order of the radii values-if you want to create a solid torus, specify zero or blank for the inner minor radius, in which case the zero or blank must occupy either the RAD1 or RAD2 position.) At least two of the values that you specify must be positive values; they will be used to define the outer minor radius and the major radius. See the diagram in the Notes section for a view of a toroidal sector showing all radii.

Starting and ending angles (either order) of the torus. Used for creating a toroidal 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°.

Defines a toroidal volume centered about the working plane origin. A solid torus of 360° will be defined with four areas, each area spanning 180° around the major and minor circumference.

To create the toroidal sector shown below, the command TORUS,5,1,2,0,180 was issued. Since "1" was the smallest radii value specified, it defined the inner minor radius; since "2" was the intermediate radii value specified, it defined the outer minor radius; and since "5" was the largest radii value specified, it defined the major radius. The values "0" and "180" defined the starting and ending angles of the torus.

Menu Paths

Main Menu >Preprocessor >Create >Torus

Specifies automatic MDOF generation.

SOLUTION:MasterDOF

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

Total number of master degrees of freedom to be used in the analysis, including specified (NS, see below) master degrees of freedom. NTOT must be greater than NS if any automatic generation is to be done.

Rotational masters key:

0 - Include all degrees of freedom in automatic master selection.

1 - Exclude rotational degrees of freedom (and VOLT degrees of freedom in a piezoelectric analysis) from automatic selection.

Notes

Specifies automatic master degree of freedom (MDOF) generation. The limit on the number of MDOF is equal to the maximum in-memory wavefront size (see the ANSYS Basic Analysis Procedures Guide). If NS is defined as the number of master degrees of freedom specified with the M or MGEN command, NTOT-NS additional master degrees of freedom will be automatically generated during the solution phase if TOTAL is used. NS may be zero, i.e., all master degrees or freedom can be automatically generated. After the solution phase, generated masters become specified masters (NS=NTOT) so that they may be listed, displayed, modified, etc. The TOTAL command is ignored in subsequent solutions unless masters are deleted, such that NS<NTOT. If used in SOLUTION, this command is valid only within the first load step.

During the matrix triangulation (wavefront) operation, the first NTOT degrees of freedom are temporarily identified as masters and then are replaced as degrees of freedom with lower K/M ratios are found. Degrees of freedom matching the user specified set (if any) are permanently identified. The wavefront builds to NTOT and will have a minimum (and final) value of NTOT. The final set of automatic masters identified will be those corresponding to the lowest modes of the structure.

Constrained degrees of freedom are excluded from the automatic master selection. Constraints may be defined to prevent undesirable modes from being present (thus preventing the corresponding MDOF from being selected). For example, if symmetry constraints are imposed, degrees of freedom producing only symmetric modes will be selected. In-plane rotational degrees of freedom for shell elements lying in a global plane are automatically excluded. All rotational degrees of freedom can be excluded during the automatic selection if desired.

If automatic master selection is used in the reduced linear transient dynamic (ANTYPE=TRANS) analysis or the reduced harmonic response (ANTYPE=HARMIC) analysis, be sure to force the selection [M] of any degrees of freedom having non-zero displacement or force inputs. If automatic master selection is used in the superelement generation pass (ANTYPE=SUBSTR), be sure to force the selection of connection points to non-superelements.

Automatically selected masters are shown in the solution listing (and not in preprocessing listings) as follows:

· in the reduced eigenvector solution for modal (ANTYPE=MODAL).

· in the reduced displacement solution for harmonic response (ANTYPE=HARMIC).

· in the reduced displacement solution for linear transient dynamic (ANTYPE=TRANS).

· in the matrix or load vector printout for substructures (ANTYPE=SUBSTR).

In the substructure generation pass (ANTYPE=SUBSTR), a mass matrix must be available if the TOTAL option is to be used.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Master DOFs >Program Selected

Main Menu >Solution >Master DOFs >Program Selected

Reformats File.GRPH for improved performance with plotters.

DISPLAY:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

File name (8 characters maximum) to be written. Defaults to TRAN33.

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

Directory name (32 characters maximum). Defaults to current directory.

Reformats current File.GRPH data (based on color) for improved performance with pen plotters.

DISPLAY Program

Transfers a pattern of nodes to another coordinate system.

PREP7:Nodes

	Mp Me St DY LP Th E3 E2 FL PP ED

Reference number of coordinate system where the pattern is to be transferred. Transfer occurs from the active coordinate system.

Increment all nodes in the given pattern by INC to form the transferred node pattern.

Transfer nodes from pattern beginning with NODE1 to NODE2 (defaults to NODE1) in steps of NINC (defaults to 1). If NODE1 = ALL, NODE2 and NINC are ignored and the pattern is all selected nodes [NSEL]. If NODE1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI). A component may be substituted for NODE1 (NODE2 and NINC are ignored).

Transfers a pattern of nodes from one coordinate system to another. Coordinate systems may be translated and rotated relative to each other. Initial pattern may be generated in any coordinate system. Coordinate values are interpreted in the active coordinate system and are transferred directly.

A model generated in one coordinate system may be transferred to another coordinate system. The user may define several coordinate systems (translated and rotated from each other), generate a model in one coordinate system, and then repeatedly transfer the model to other coordinate systems. The model may be generated in any type of coordinate system (Cartesian, cylindrical, etc.) and transferred to any other type of coordinate system. Coordinate values (X,Y,Z, or R,,Z, or etc.) of the model being transferred are interpreted in the active coordinate system type, regardless of how they were generated. Values are transferred directly and are interpreted according to the type of coordinate system being transferred to. For example, transferring from a Cartesian coordinate system to a cylindrical coordinate system (not recommended) would cause X=2.0 and Y=3.0 values to be directly interpreted as R=2.0 and =3.0 values, respectively.

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

Reads data from an external file into a table array parameter.

APDL:Parameters

	Mp Me St DY LP Th E3 E2 FL PP ED

Table array parameter name as defined by the *DIM command.

File name (32 characters maximum) to be read. No default.

File name extension (optional) (8 characters maximum). No default.

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

Number of comment lines at the beginning of the file being read that will be skipped during the reading. Default=0.

Use this command to read in a table of data from an external file into an ANSYS table array parameter. The external file may be created using a text editor or by an external application or program. The ANSYS TABLE type array parameter must be defined before you can read in an external file. See *DIM for more information.

Utility Menu >Parameters >Array Parameters >Read from File

Defines the reference temperature for the thermal strain calculations.

SOLUTION:LoadStepOptions

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

Reference temperature for thermal expansion. Note, if the uniform temperature [TUNIF] is undefined, it is also set to this value.

Notes

Defines the reference temperature for the thermal strain calculations in structural analyses. Thermal strains are given by *(T-TREF), as explained in Section 2.1 of the ANSYS Theory Reference, where is the coefficient of thermal expansion material property and T is the element temperature. Units should be consistent with .

Reference temperatures may also be input per material by using the label REFT on the material property [MP] command, such as MP,REFT,MAT,C0. Only a constant (non-temperature-dependent) value is allowed. The value input on the TREF command applies to all materials not having a specified material property definition.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Other >Reference Temp

Main Menu >Preprocessor >Loads >Settings >Reference Temp

Main Menu >Solution >Other >Reference Temp

Main Menu >Solution >Settings >Reference Temp

Shows the global XYZ coordinate triad on displays.

GRAPHICS:Labeling

	Mp Me St DY LP Th E3 E2 FL PP ED

Display triad as follows:

ORIG - Display triad at global origin (default).

OFF - Turn off triad display.

LBOT - Display triad in lower left screen corner.

RBOT - Display triad in lower right screen corner.

LTOP - Display triad in upper left screen corner.

RTOP - Display triad in upper right screen corner.

For efficiency, ANSYS 3-D graphics logic maintains a single data structure (segment), which includes the triad as a 3-D data object. If a 3-D device is involved (/SHOW,3D), and the ANSYS graphics are not being displayed as multi-plots, then the triad location is determined by the view settings for Window #1. A request for triad display anywhere except for the origin could yield an improper display in windows 2 through 5. The program displays the same segment in all windows. The view settings of each window constitute the only difference in the display in the active windows.

This command is valid in any processor.

Utility Menu >PlotCtrls >Window Controls >Reset Window Options

Utility Menu >PlotCtrls >Window Controls >Window Options

Specifies the level of translucency.

GRAPHICS:Style

	Mp Me St DY LP Th E3 E2 FL PP ED

Apply translucency level to the items specified by the following labels:

ELEM - Elements. Use N1, N2, NINC fields for element 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., value). Translucency varies with result value, to a maximum of the specified translucency level.

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

CURVE - Filled areas under curves of line graphs. Use N1, N2, NINC fields or curve numbers.

Translucency level: 0.0 (opaque) to 1.0 (transparent).

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

Notes

Specifies the level of translucency for various items. Issue /TRLCY,DEFA to reset the default translucency levels. This command is valid only on selected 2D and 3-D graphics devices; see the ANSYS Basic Analysis Procedures Guide.

For 2-D devices, ANSYS displays only the visible faces of the items being displayed. The information behind the facing planes is not displayed. Issuing the /SHRINK command will force the hardware to display information behind the translucent items .

This command is valid in any processor.

Utility Menu >PlotCtrls >Style > Translucency

Specifies transient analysis options.

SOLUTION:DynamicOptions

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

Solution method for the transient analysis:

FULL - Full method (default).

REDUC - Reduced method.

MSUP - Mode superposition method.

Largest mode number to be used to calculate the response (for Method=MSUP). Defaults to the highest mode calculated in the preceding modal analysis.

Damping option (for Method=REDUC):

DAMP - Include the effects of damping if present (default).

NODAMP - Ignore the effects of damping, even if present.

Smallest mode number to be used (for Method=MSUP). Defaults to 1.

Specifies transient analysis (ANTYPE=TRANS) options. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

In ANSYS/LinearPlus, Method defaults to MSUP instead of FULL; Method=FULL and REDUC are not allowed.

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Deletes particle flow or charged particle trace points.

POST1:TracePoints

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

Delete points from NTRP1 to NTRP2 (defaults to NTRP1) in steps of TRPINC (defaults to 1). If NTRP1 = ALL, NTRP2 and TRPINC are ignored and all trace points are deleted. If NTRP1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Deletes particle flow or charged particle trace points defined with the TRPOIN command.

Main Menu >General Postproc >Plot Results >Dele Trace Pt

Lists the particle flow or charged particle trace points.

POST1:TracePoints

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

List points from NTRP1 to NTRP2 (defaults to NTRP1) in steps of TRPINC (defaults to 1). If NTRP1 = ALL, NTRP2 and TRPINC are ignored and all trace points are listed. If NTRP1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Lists the particle flow or charged particle trace points in the active display coordinate system [DSYS]. Trace points are defined with the TRPOIN command.

Main Menu >General Postproc >Plot Results >List Trace Pt

Defines a point through which a particle flow or charged particle trace will travel.

POST1:TracePoints

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

Coordinate location of the trace point (in the active coordinate system). If X = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Particle velocities in the X, Y and Z directions (in the active coordinate system).

Particle charge.

Particle mass.

Defines a point through which a particle flow or charged particle trace [PLTRAC] will travel. Multiple points (50 maximum) may be defined which will result in multiple flow traces. Use TRPLIS to list the currently defined trace points and TRPDEL to delete trace points.

The VX, VY, VZ, CHRG, and MASS arguments only apply to charged particles.

Main Menu >General Postproc >Plot Results >Defi Trace Pt

Defines the options used for the PLTRACE (particle flow or charged particle trace) command.

POST1:Animation

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Particle spacing in seconds (defaults to 0).

Particle offset in seconds (defaults to 0). Used internally for animation.

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

Particle length fraction (defaults to .1).

Notes

The TRTIME command is used to vary the type of PLTRACE display that is produced. Particle flow or charged particle traces normally trace a particle's path in the forward and backward direction of travel and color-code the line by the selected DOF. The TIME option lets you set the time interval of forward travel for the trace. The SPACING option is used to define the particle spacing in seconds from adjacent particles in the stream line. The OFFSET variable defines the offset in seconds from the particle SPACING. The OFFSET variable is used internally in the ANFLOW macro to produce an animation of particle flow in a flowing fluid or charged particle motion in an electric or magnetic field. The SIZE variable sets the radius of the particle. The LENGTH variable is used to define the particle length fraction. By default, the LENGTH is set to .1, which means the particle occupies 10% of the flow region, and the other 90% is a color-coded line. The SPACING, OFFSET and LENGTH variables only make sense when the SIZE variable is non-zero (i.e., the particle is bigger than the line).

Main Menu >General Postproc >Plot Results >Time Interval

Defines simple 2-D and 3-D geometric surfaces for target segment elements.

PREP7:Elements

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

Specifies the geometric shapes for target segment elements TARGE169 and TARGE170.

lINE - Straight line (2-D) (Default for 2-D)

PARA - Parabola (2-D)

ARC - Clockwise arc (2-D)

CARC - Counterclockwise arc (2-D)

CIRC - Complete circle (2-D)

TRIA - Three-node triangle (3-D) (Default for 3-D)

TRI6 - Six-node triangle (3-D)

QUAD - Four-node quadrilateral (3-D)

QUA8 - Eight-node quadrilateral (3-D)

CYLI - Cylinder (3-D)

CONE - Cone (3-D)

SPHE - Sphere (3-D)

PILO - Pilot node (2-D, 3-D)

Use this command to generate the rigid target surface for surface-to-surface contact (TARGE169, CONTA171, CONTA172 (2-D) and TARGE170, CONTA173, and CONTA174 (3-D)). Once you issue TSHAP, all subsequent elements generated via this command will have the same shape, until you issue TSHAP again with a different Shape.

Main Menu >Preprocessor >Create >Elements >Elem Attributes

Creates annotation text attributes (GUI).

GRAPHICS:Annotation

	Mp Me St DY LP Th E3 E2 FL PP ED

Text color (0 TCOLOR 15):

0 - Black.

1 - Red-Magenta.

2 - Magenta.

3 - Blue-Magenta.

4 - Blue.

5 - Cyan-Blue.

6 - Cyan.

7 - Green-Cyan.

8 - Green.

9 - Yellow-Green.

10 - Yellow.

11 - Orange.

12 - Red.

13 - Dark Gray.

14 - Light Gray.

15 - White.

Text size factor.

Text thickness key:

1 - normal.

2 - twice as thick.

3 - three times as thick.

4 - four times as thick.

Text path angle (0.0 < angle< 360.0).

Text italic angle (0.0 < angle< 45.0).

Defines annotation text attributes to control certain characteristics of the text created via the /TLABEL command. This is a command generated by the Graphical User Interface (GUI) and will appear in the log file (Jobname.LOG) if annotation is used. This command is not intended to be typed in directly in an ANSYS session (although it can be included in an input file for batch input or for use with the /INPUT command).

This command is valid in any processor.

Utility Menu >PlotCtrls >Annotation >Create Annotation

Defines an array of keytimes at which the time-stepping strategy changes.

SOLUTION:LoadStepOptions

	Mp Me St DY LP Th E3 E2 FL PP ED

Identifies an Nx1x1 array parameter containing the keytimes at which the heat transfer time-stepping strategy changes (the time step is reset to the initial time step based on DELTIM or NSUBST settings). The array name must be enclosed by % signs (e.g., %array%). See *DIM for more information on array parameters.

This command is valid only in a heat transfer analysis and if the selected set of elements consist of some combination of thermal only, thermal-electric, thermal surface effect, or thermal-fluid pipe elements.

Time values in the array parameter must be in ascending order. The time increment between time points in the array list must be larger than the initial time step defined on the DELTIM or NSUBST command. Results can be output at the requested time points if the array or time values in the array are also specified in the OUTRES command using FREQ=%array%. Use this command to reset the time-stepping strategy within a load step. You may need to reset the time-stepping strategy when using tabular time-varying boundary conditions.

See Chapter 2 of the ANSYS Thermal Analysis Guide for more information on applying boundary conditions via tabular input. See Chapter 3 of the ANSYS Thermal Analysis Guide for more information on defining keytimes.

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

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

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

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

Assigns a uniform temperature to all nodes.

SOLUTION:FEBodyLoads

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

Uniform temperature assigned to the nodes. If TEMP is blank, the uniform temperature is set to zero.

Notes

In a transient or nonlinear thermal analysis, the uniform temperature is used during the first iteration of a solution as follows: (a) as the starting nodal temperature (except where temperatures are explicitly specified [D, DK]), and (b) to evaluate temperature-dependent material properties. In a structural analysis, the uniform temperature is used as the default temperature for thermal strain calculations and material property evaluation (except where body load temperatures are specified [BF, BFE, BFK, LDREAD]). In other scalar field analyses, the uniform temperature is used for material property evaluation.

TUNIF is a convenient form of the more general BFUNIF command.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Apply >Boundary >-Temperature- >Uniform Temp

Main Menu >Preprocessor >Loads >Apply >Temperature >Uniform Temp

Main Menu >Preprocessor >Loads >Settings >Uniform Temp

Main Menu >Solution >Apply >Boundary >-Temperature- >Uniform Temp

Main Menu >Solution >Apply >Temperature >Uniform Temp

Main Menu >Solution >Settings >Uniform Temp

Changes time to the cumulative iteration number.

POST26:Controls

	Mp Me St DY LP Th E3 E2 FL PP ED

Time key:

0 - Time is used for the variable TIME.

1 - NCUMIT is used for the variable TIME.

Notes

Changes the meaning of the time variable to the cumulative iteration number (NCUMIT) variable. Data can be read from the file, printed, and displayed as a function of NCUMIT rather than time. All POST26 descriptions applying to TIME then apply to NCUMIT.

Main Menu >TimeHist Postpro >Settings >Data

Defines the type of display.

GRAPHICS:Style

	Mp Me St DY LP Th E3 E2 FL PP ED

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

Display type. Defaults to ZBUF for raster mode displays or BASIC for vector mode displays:

BASIC or 0 - Basic display (no hidden or section operations).

SECT or 1 - Section display (plane view). Use the /CPLANE command to define the cutting plane.

HIDC or 2 - Centroid hidden display (based on item centroid sort).

HIDD or 3 - Face hidden display (based on face centroid sort).

HIDP or 4 - Precise hidden display (like HIDD but with more precise checking).

CAP or 5 - Capped hidden display (same as combined SECT and HIDD with model in front of section plane removed).

ZBUF or 6 - Z-buffered display (like HIDD but using software Z-buffering).

ZCAP or 7 - Capped Z-buffered display (same as combined SECT and ZBUF with model in front of section plane removed).

ZQSL or 8 - QSLICE Z-buffered display (same as SECT but the edge lines of the remaining 3-D model are shown).

HQSL or 9 - QSLICE precise hidden display (like ZQSL but using precise hidden).

Notes

Defines the type of display, such as section display or hidden-line display. Use the /DEVICE command to specify either raster or vector mode.

The SECT, CAP, ZCAP, ZQSL, and HQSL options produce section displays. The section or "cutting" plane is specified on the /CPLANE command as either normal to the viewing vector at the focus point (default), or as the working plane.

The HIDC, HIDD, HIDP, ZBUF, ZQSL, and HQSL options produce displays with "hidden" lines removed. Hidden lines are lines obscured from view by another element, area, etc. The choice of non-Z-buffered hidden-line procedure types is available only for raster mode [/DEVICE] displays. For vector mode displays, all non-Z-buffered "hidden-line" options use the same procedure (which is slightly different from the raster procedures). Both geometry and postprocessing displays may be of the hidden-line type. Interior stress contour lines within solid elements can also be removed as hidden lines, leaving only the stress contour lines and element outlines on the visible surfaces. Midside nodes of elements are ignored on postprocessing displays. Overlapping elements will not be displayed.

The ZBUF, ZCAP, and ZQSL options use a specific hidden-line technique called software Z-buffering. This technique allows a more accurate display of overlapping surfaces (common when using Boolean operations or /ESHAPE on element displays), and allows smooth shaded displays on all interactive graphics displays. Z-buffered displays can be performed faster than HIDP and CAP type displays for large models. See also the /LIGHT, /SHADE, and /GFILE commands for additional options when Z-buffering is used.

This command is valid in any processor.

Utility Menu >PlotCtrls >Style >Hidden-Line Options

Sets the element type attribute pointer.

PREP7:Meshing PREP7:Elements

	Mp Me St DY LP Th E3 E2 FL PP ED

Assign this type number to the elements (defaults to 1).

Notes

Activates an element type number to be assigned to subsequently defined elements. This number refers to the element type number (ITYPE) defined with the ET command. Type numbers may be displayed [/PNUM].

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

Main Menu >Preprocessor >Create >Elements >Elem Attributes

Main Menu >Preprocessor >Define >Default Attribs