M

Defines master degrees of freedom for reduced analyses.

SOLUTION:MasterDOF

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

Node number at which master degree of freedom is defined. If ALL, define master degrees of freedom at 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 also be substituted for NODE.

Master degree of freedom direction (in the nodal coordinate system). If ALL, use all appropriate labels. Valid labels are: UX UY UZ ROTX ROTY ROTZ. The ALL label should not be used except for convenience with the substructure generation (i.e., if all degrees of freedom are to be made MDOF at the substructure connection points). ALL includes all valid labels as determined by the element types defined [ET]. Scalar MDOF (VOLT) are not permitted in structural analyses if mass or damping matrices are reduced.

Define all nodes from NODE to NEND (defaults to NODE) in steps of NINC (defaults to 1) as master degrees of freedom in the specified direction.

Additional master degree of freedom labels. The nodes defined are associated with each label specified.

Defines master degrees of freedom (MDOF) for reduced (dynamic and superelement generation) analyses. If defined for other analyses, MDOF are ignored. If used in SOLUTION, this command is valid only within the first load step.

Repeat M command for additional master degrees of freedom. Limit is equal to the maximum in-memory wavefront size (see the ANSYS Basic Analysis Procedures Guide).

The buckling (ANTYPE=BUCKLE), reduced modal (ANTYPE=MODAL), reduced transient (ANTYPE=TRANS), reduced harmonic response (ANTYPE=HARMIC), and the substructure (ANTYPE=SUBSTR) analyses utilize the matrix condensation technique to reduce the structure matrices to those characterized by a set of master degrees of freedom.

Master degrees of freedom are identified by a list of nodes and their nodal directions. The actual degree of freedom directions 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. There must be some mass (or stress stiffening in the case of the buckling analysis) associated with each master degree of freedom (except for the VOLT label). The mass may be due either to the distributed mass of the element or due to discrete lumped masses at the node. If a master degree of freedom is specified at a constrained point, it is ignored. If a master degree of freedom is specified at a coupled node, it should be specified at the prime node of the coupled set. Master degrees of freedom can also be generated automatically (during solution) by issuing the TOTAL command in PREP7 or SOLUTION.

Transient displacements and forces, used to apply motion to a structure in the reduced transient or reduced harmonic response analysis, must be applied at a master degree of freedom. Substructure analysis connection points must be defined as master degrees of freedom.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Master DOFs >Define

Main Menu >Solution >Master DOFs >Define

Specifies options for a 3-D magnetostatic field analysis.

SOLUTION:LoadStepOptions

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

Option key:

0 - Calculate a complete H field solution in the entire domain using a single (reduced) potential. Caution-when used in problems with both current sources and iron regions, errors may result due to numerical cancellation.

1 - Calculate and store a preliminary H field in "iron" regions (_r1). Requires flux-parallel boundary conditions to be specified on exterior iron boundaries. Used in conjunction with subsequent solutions with VALUE=2 followed by VALUE=3. Applicable to multiply-connected iron domain problems.

2 - Calculate and store a preliminary H field in "air" regions (_r=1). The air-iron interface is appropriately treated internally by the program. Used in conjunction with a subsequent solution with VALUE=3. Applicable to singly-connected iron domain problems (with subsequent solution with VALUE=3) or to multiply-connected iron domain problems (when preceded by a solution with VALUE=1 and followed by a solution with VALUE=3).

3 - Use the previously stored H field solution(s) and calculate the complete H field.

Specifies the solution sequence options for a 3-D magnetostatic field analysis using a scalar potential (MAG). The solution sequence is determined by the nature of the problem.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Magnetics >DSP Method

Main Menu >Preprocessor >Loads >Magnetics >GSP Method

Main Menu >Preprocessor >Loads >Magnetics >RSP Method

Main Menu >Solution >Magnetics >DSP Method

Main Menu >Solution >Magnetics >GSP Method

Main Menu >Solution >Magnetics >RSP Method

Specifies magnetic solution options and initiates the solution.

SOLUTION:LoadStepOptions

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

Static magnetic solution option:

0 - Vector potential (MVP) or edge formulation (default).

1 - Combined vector potential and reduced scalar potential (MVP-RSP).

2 - Reduced scalar potential (RSP).

3 - Difference scalar potential (DSP).

4 - General scalar potential (GSP).

Number of ramped substeps for the first load step of a nonlinear MVP or MVP-RSP solution. Defaults to 3. If NRAMP=-1, ignore the ramped load step entirely. (Note-NRAMP is ignored for linear magnetostatics.)

Tolerance value on the program-calculated reference value for the magnetic current-segment convergence. Used for the MVP, the MVP-RSP, and the edge formulation solution options (OPT = 0 and 1). Defaults to 0.001.

Tolerance value on the program-calculated reference value for the magnetic flux convergence. Used for all scalar potential solution options (OPT = 2, 3, 4). Defaults to 0.001.

Maximum number of equilibrium iterations per load step. Defaults to 25.

Option to force execution of a Biot-Savart integral solution [BIOT,NEW] for the scalar potential options. Required if multiple load steps are being performed with different current source primitives (SOURC36 elements).

0 - Do not force execution of Biot-Savart calculation (default); Biot-Savart is automatically calculated only for the first solution.

1 - Force execution of Biot-Savart calculation.

MAGSOLV invokes an ANSYS macro which specifies magnetic solution options and initiates the solution. The macro is applicable to any ANSYS magnetostatic analysis using the magnetic vector potential (MVP), reduced scalar potential (RSP), difference scalar potential (DSP), general scalar potential (GSP), or combined MVP-RSP formulation options. Results are only stored for the final converged solution. (In POST1, issue SET,LIST to identify the load step of solution results.) The macro internally determines if a nonlinear analysis is required based on magnetic material properties.

If you use the BIOT option and issue SAVE after solution or postprocessing, the Biot-Savart calculations are saved to the database, but will be overwritten upon normal exit from the program. To save this data after issuing SAVE, use the /EXIT,NOSAVE command. You can also issue the /EXIT,SOLU command to exit ANSYS and save all solution data, including the Biot-Savart calculations, in the database. Otherwise, when you issue RESUME, the Biot-Savart calculation will be lost (resulting in a zero solution).

The MVP, MVP-RSP, and edge formulation options perform a two-load-step solution sequence. The first load step ramps the applied loads over a prescribed number of substeps (NRAMP), and the second load step calculates the converged solution. For linear problems, only a single load step solution is performed. The ramped load step can be bypassed by setting NRAMP to -1.

The RSP option solves in a single load step using the adaptive descent procedure. The DSP option uses two load steps, and the RSP solution uses three load steps.

The following analysis options and nonlinear options are controlled by this macro: KBC,NEQIT, NSUBST, CNVTOL, NROPT, MAGOPT, OUTRES.

Main Menu >Solution >Electromagnet >Opt&Solv

Specifies "Master DOF" as the subsequent status topic.

SOLUTION:Status

	Mp Me St DY LP Th E3 E2 FL PP ED

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

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

Utility Menu >List >Status >Solution >Master DOF

Sets the element material attribute pointer.

PREP7:Meshing PREP7:Elements

	Mp Me St DY LP Th E3 E2 FL PP ED

Assign this material number to subsequently defined elements (defaults to 1).

Notes

Identifies the material number to be assigned to subsequently defined elements. This number refers to the material number (MAT) defined with the material properties [MP]. Material numbers may be displayed [/PNUM].

Main Menu >Preprocessor >Create >Elements >Elem Attributes

Main Menu >Preprocessor >Define >Default Attribs

Specifies "Material 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.

Utility Menu >List >Status >Preprocessor >Materials

Defines the damping ratios as a function of mode.

SOLUTION:DynamicOptions

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

Starting location in table for entering data. For example, if STLOC=1, data input in the V1 field applies to the first constant in the table. If STLOC=7, data input in the V1 field applies to the seventh constant in the table, etc. Defaults to the last location filled + 1.

Data assigned to six locations starting with STLOC. If a value is already in this location, it will be redefined. Blank values for V2 to V6 leave the corresponding previous value unchanged.

Defines the damping ratios as a function of mode. Table position corresponds to mode number. Ratios not defined default to DMPRAT. Use STAT command to list current values. Applies to the mode superposition harmonic response (ANTYPE=HARMIC), the mode superposition linear transient dynamic (ANTYPE=TRANS), and the spectrum (ANTYPE=SPECTR) analyses. Repeat MDAMP command for additional constants (300 maximum).

This command is also valid in PREP7.

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

Main Menu >Solution >Time/Frequenc >Damping

Deletes master degrees of freedom.

SOLUTION:MasterDOF

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

Delete master degrees of freedom in the Lab1 direction [M] from NODE to NEND (defaults to NODE) in steps of NINC (defaults to 1). If NODE = ALL, NEND and NINC are ignored and masters for all selected nodes [NSEL] are deleted. If Lab1 = ALL, all label directions will be deleted. If NODE = 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 NODE.

Delete masters in these additional directions.

Deletes master degrees of freedom. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Master DOFs >Delete

Main Menu >Solution >Master DOFs >Delete

Activates the Graphical User Interface (GUI).

SESSION:RunControls

	Mp Me St DY LP Th E3 E2 FL PP ED

Activation key:

ON - Activates the menu system (device dependent).

GRPH - Enters non-GUI graphics mode. This option is intended for use on graphics devices that do not support the full Motif-based GUI.

Notes

Activates the Graphical User Interface (GUI). Caution: if you include the /MENU,ON command in your START5x.ANS file, it should be the last command in the file. Any commands after /MENU,ON may be ignored. (It is not necessary to include the /SHOW and /MENU,ON commands in START5x.ANS if you will be using the launcher to enter the ANSYS program.)

This command is valid in any processor.

This command cannot be accessed directly in the menu.

Specifies "Meshing" 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 >Meshing

Calculates the coefficients for, or evaluates, a Fourier series.

APDL:ArrayParameters

	Mp Me St DY LP Th E3 E2 FL PP ED

Type of Fourier operation:

FIT - Calculate Fourier coefficients COEFF from MODE, ISYM, THETA, and CURVE.

EVAL - Evaluate the Fourier curve CURVE from COEFF, MODE, ISYM, and THETA.

Name of the array parameter vector containing the Fourier coefficients (calculated if Oper=FIT, required as input if Oper=EVAL). See *SET for name restrictions.

Name of the array parameter vector containing the mode numbers of the desired Fourier terms.

Name of the array parameter vector containing the symmetry key for the corresponding Fourier terms. The vector should contain keys for each term as follows:

0 or 1 - Symmetric (cosine) term

-1 - Antisymmetric (sine) term.

Names of the array parameter vectors containing the theta vs. curve description, respectively. Theta values should be input in degrees. If Oper=FIT, one curve value should be supplied with each theta value. If Oper=EVAL, one curve value will be calculated for each theta value.

Calculates the coefficients of a Fourier series for a given curve, or evaluates the Fourier curve from the given (or previously calculated) coefficients. The lengths of the COEFF, MODE, and ISYM vectors must be the same-typically two times the number of modes desired, since two terms (sine and cosine) are generally required for each mode. The lengths of the CURVE and THETA vectors should be the same or the smaller of the two will be used. There should be a sufficient number of points to adequately define the curve-at least two times the number of coefficients. A starting array element number (1) must be defined for each array parameter vector. The vector specifications *VLEN, *VCOL, *VABS, *VFACT, and *VCUM do not apply to this command. Array elements should not be skipped with the *VMASK and the NINC value of the*VLEN specifications. The vector being calculated (COEFF if Oper is FIT, or CURVE if Oper is EVAL) must exist as a dimensioned array [*DIM].

This command is valid in any processor.

Utility Menu >Parameters >Array Operations >Matrix Fourier

Copies or transposes an array parameter matrix.

APDL:ArrayParameters

	Mp Me St DY LP Th E3 E2 FL PP ED

The name of the resulting array parameter matrix. See *SET for name restrictions. The parameter must exist as a dimensioned array [*DIM].

Copy or transpose function:

COPY - Par1 is copied to ParR

TRAN - Par1 is transposed to ParR. Rows (m) and columns (n) of Par1 matrix are transposed to resulting ParR matrix of shape (n,m).

Array parameter matrix input to the operation.

Operates on one input array parameter matrix and produces one output array parameter matrix according to:

where the function (f) is either a copy or transpose, as described above.

Functions are based on the standard FORTRAN definitions where possible. ParR may be the same as Par1. Starting array element numbers must be defined for each array parameter matrix. For example, *MFUN,A(1,5),COPY,B(2,3) copies matrix B (starting at element (2,3)) to matrix A (starting at element (1,5)). The diagonal corner elements for each submatrix must be defined: the upper left corner by the array starting element (on this command), the lower right corner by the current values from the *VCOL and *VLEN commands. The default values are the (1,1) element and the last element in the matrix. No operations progress across matrix planes (in the 3rd dimension). Absolute values and scale factors may be applied to all parameters [*VABS, *VFACT]. Results may be cumulative [*VCUM]. Array elements should not be skipped with the *VMASK and the NINC value of the *VLEN specifications. The number of rows [*VLEN] applies to the Par1 array. See the *VOPER command for details.

This command is valid in any processor.

Utility Menu >Parameters >Array Operations >Matrix Functions

Generates additional MDOF from a previously defined set.

SOLUTION:MasterDOF

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

Do this generation operation a total of ITIMEs, incrementing all nodes in the set by INC each time after the first. ITIME must be > 1 for generation to occur. All previously defined master degree of freedom directions are included in the set. A component name may also be substituted for ITIME.

Generate master degrees of freedom from set beginning with NODE1 to NODE2 (defaults to NODE1) in steps of NINC (defaults to 1). If NODE1 = ALL, NODE2 and NINC are ignored and set is all selected nodes [NSEL]. If NODE1 = P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).

Generates additional master degrees of freedom from a previously defined set. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Master DOFs >Copy

Main Menu >Solution >Master DOFs >Copy

Defines a mitered bend in a piping run.

PREP7:Piping

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

Element numbers of the two intersecting straight pipes. Defaults to the last two straight pipe elements nearest the intersection of the last two runs.

Bend radius. If LR, use long radius standard (1.5 x OD) (default). If SR, use short radius standard (1.0 x OD).

Number of divisions (elements) along bend (defaults to 2). A node is generated at the end of each division.

Number to be assigned to first element of bend (defaults to MAXEL + 1).

Element number increment (defaults to 1).

Defines a mitered bend of piecewise straight pipe elements (PIPE16) in place of the intersection of two previously defined straight pipe elements [RUN]. This command is similar to the BEND command except that straight pipe elements are used to form the bend instead of curved (elbow) elements.

Main Menu >Preprocessor >Create >Piping Models >Miter

Lists the MDOF of freedom.

SOLUTION:MasterDOF

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

List master degrees of freedom from NODE1 to NODE2 (defaults to NODE1) in steps of NINC (defaults to 1). If NODE1 = ALL (default), NODE2 and NINC are ignored and masters 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 also be substituted for NODE1 (NODE2 and NINC are ignored).

Lists the master degrees of freedom. Master degrees of freedom generated from the TOTAL command cannot be listed until after the first load step.

Main Menu >Preprocessor >Loads >Master DOFs >List All

Main Menu >Preprocessor >Loads >Master DOFs >List Picked

Main Menu >Solution >Master DOFs >List All

Main Menu >Solution >Master DOFs >List Picked

Utility Menu >List >Other >Master DOF >At All Nodes

Utility Menu >List >Other >Master DOF >At Picked Nodes

Calculates the magnetomotive force along a path.

POST1:Magnetics

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

MMF invokes an ANSYS macro which calculates the magnetomotive force (mmf) along a predefined path [PATH]. It is valid for both 2-D and 3-D magnetic field analyses. The calculated mmf value is stored in the parameter MMF.

A closed path [PATH], passing through the magnetic circuit for which mmf is to be calculated, must be defined before this command is issued. A counter-clockwise ordering of points on the PPATH command will yield the correct sign on the mmf. The mmf is based on Ampere's Law. The macro makes use of calculated values of field intensity (H), and uses path operations for the calculations. All path items are cleared upon completion. The MMF macro sets the "ACCURATE" mapping method and "MAT" discontinuity option of the PMAP command.

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

Specifies the harmonic loading term for this load step.

SOLUTION:LoadStepOptions

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

Number of harmonic waves around circumference for this harmonic loading term (defaults to 0).

Symmetry condition for this harmonic loading term (not used when MODE=0):

1 - Cosine terms (default).

-1 - Sine terms.

Notes

Used with axisymmetric elements having nonaxisymmetric loading capability (e.g., PLANE25, SHELL61, FLUID81, etc.). For analysis types ANTYPE = MODAL, HARMIC, TRANS, and SUBSTR, the term must be defined in the first load step and may not be changed in succeeding load steps.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >Other >For Harmonic Ele

Main Menu >Solution >Other >For Harmonic Ele

Controls the relationship of the solid model and the FE model.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Relationship key:

STAT - Gives status of command (default). This applies only to the CHECK option (no status is provided for the DETACH option).

NOCHECK - Deactivates the checking of the solid model and the finite element model. Allows elements and nodes generated with the mesh commands to be modified directly (EMODIF, NMODIF, EDELE, NDELE, etc.). Also deactivates solid model hierarchical checking so that areas attached to volumes may be deleted etc. Warning-use of this command allows the solid model data base to be corrupted by subsequent operations.

CHECK - Reactivates future checking of the solid model.

DETACH - Releases all associativity between the current solid model and finite element model. ANSYS deletes any element attributes that were assigned to the affected solid model entities through default attributes (that is, through the TYPE, REAL, MAT, SECNUM, and ESYS command settings and a subsequent meshing operation). However, attributes that were assigned directly to the solid model entities (via the KATT, LATT, AATT, and VATT commands) are not deleted. Warning-once used it is not possible to select or define finite element model items in terms of the detached solid model or to clear the mesh.

Affects the relationship of the solid model (keypoints, lines, areas, volumes) and the finite element model (nodes, elements, and boundary conditions).

Main Menu >Preprocessor >Checking Ctrls >Model Checking

Specifies modal analysis options.

SOLUTION:DynamicOptions

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

Mode extraction method to be used for the modal analysis.

SUBSP - Subspace iteration

LANB - Block Lanczos

REDUC - Householder (reduced)

UNSYM - Unsymmetric matrix (cannot be followed by a subsequent spectrum analysis).

DAMP - Damped system (cannot be followed by a subsequent spectrum analysis).

Number of modes to extract. For Method=REDUC, NMODE should be less than half the total number of master degrees of freedom. For Method=SUBSP, NMODE should be less than half the total number of degrees of freedom. For Method=REDUC, the default is the total number of masters defined; for Method=SUBSP, LANB, UNSYM, or DAMP, NMODE must be input.

Beginning, or lower end, of frequency range of interest.

For Method=SUBSP, LANB, UNSYM, and DAMP, FREQB also represents the first shift point for the eigenvalue iterations. FREQB defaults to -1.0 if zero or blank for SUBSP, UNSYM, and DAMP. Eigenvalue extraction is most accurate near the shift point; multiple shift points are used in the SUBSP and LANB methods. For SUBSP method, and for UNSYM, LANB, and DAMP, methods with a positive FREQB, eigenvalues are output beginning at the shift point and increase in magnitude. For UNSYM and DAMP methods with a negative FREQB, eigenvalues are output, beginning at zero magnitude, and increase.

Ending, or upper end, of frequency range of interest. FREQE defaults to 1e8 for Method=SUBSPC and LANB. The default for the other methods is to calculate all modes, regardless of their maximum frequency.

Number of reduced modes to print for Method=REDUC.

Mode shape normalization key:

OFF - Normalize the mode shapes to the mass matrix (default).

ON - Normalize the mode shapes to unity instead of to the mass matrix. If a subsequent spectrum or mode superposition analysis is planned, the mode shapes should be normalized to the mass matrix (i.e., Nrmkey=OFF).

Constraint equation (CE) processing key (applies only to Method=LANB). (See Section 3.10 of the ANSYS Structural Analysis Guide for more information about the use of this field in the SOLUTION phase of a modal cyclic symmetry analysis.)

0 - Direct elimination method (default)

1 - Lagrange multiplier method - quick solution

2 - Lagrange multiplier method - accurate solution

Specifies modal analysis (ANTYPE=MODAL) options. Additional options used only for subspace iteration eigenvalue extraction are specified by the SUBOPT command. Specifying the subspace option along with the PCG solver [EQSLV,PCG] is the same as choosing the Power Dynamics option on the GUI. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

The damped and unsymmetric methods are not available in the ANSYS/LinearPlus program.

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >Analysis Options

Controls contents of three variable fields in non-linear solution monitor file.

SOLUTION:AnalysisOptions

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

One of three variable field numbers in the monitor file whose contents can be specified by the Lab field. Valid arguments are integers 1, 2, or 3. See Notes section for default values.

The node number for which information is monitored in the specified VAR field. In the GUI, if Node=P, graphical picking is enabled. If blank, the monitor file lists the maximum value of the specified quantity (Lab field) for the entire structure.

The solution quantity to be monitored in the specified VAR field. Valid labels for solution quantities are UX, UY, and UZ (displacements); ROTX, ROTY, and ROTZ (rotations); and TEMP (temperature). Valid labels for reaction force are FX, FY, and FZ (structural force) and MX, MY, and MZ (structural moment). Valid label for heat flux is (HEAT). For defaults see the Notes section.

This command is only active when SOLCONTROL,ON.

The monitor file is an ASCII file which is automatically created and saved when SOLCONTROL is active (ON). The monitor file always has an extension of .mntr, and takes its file name from the specified Jobname. If no Jobname is specified, the file name defaults to file.

You must issue this command once for each solution quantity you want to monitor at a specified node at each load step. The variable field contents can be redefined at each load step by reissuing the command. The monitored quantities are appended to the file for each load step.

The following example shows the format of a monitor file. Note that the file only records the solution substep history when a substep is convergent.

 SOLUTION HISTORY INFORMATION FOR JOB: file.mntr                                          
                                                      
 ANSYS RELEASE  5.5                     10:12:43    05/15/1998

 LOAD SUB-  NO.   NO.  TOTL   INCREMENT    TOTAL       VARIAB 1    VARIAB 2    VARIAB 3
 STEP STEP  ATTMP ITER ITER   TIME/LFACT   TIME/LFACT  MONITOR     MONITOR     MONITOR
                                                       UZ          MZ          MxPl

   1     1    1     3     3   0.25000     0.25000      1.4145     0.19076E-06 0.78886E-30
   1     2    1     2     5   0.25000     0.50000      2.8283     0.92989E-06 0.78886E-30
   1     3    1     2     7   0.37500     0.87500      4.9467     0.33342E-05 0.78886E-30
   1     4    1     2     9   0.12500      1.0000      5.6519     0.16826E-05 0.78886E-30
   2     1    1     6    15   0.20000E-03  1.0002      4.2198      515.23     0.78886E-30
   2     2    2     6    26   0.10000E-03  1.0003      4.4849      593.03     0.78886E-30
   2     3    1     3    29   0.10000E-03  1.0004      4.7531      611.45     0.78886E-30
   2     4    1     3    32   0.15000E-03  1.0006      5.0696      621.83     0.78886E-30
   2     5    1     4    36   0.22500E-03  1.0008      5.4428      628.42     0.78886E-30
   2     6    1     4    40   0.33750E-03  1.0011      5.8928      632.78     0.78886E-30
   2     7    1     5    45   0.50625E-03  1.0016      6.4454      635.62     0.78886E-30
   2     8    1     7    52   0.75938E-03  1.0024      7.1375      637.22     0.78886E-30
   2     9    1     5    57   0.75938E-03  1.0031      7.7422      637.66     0.78886E-30
   2    10    1     6    63   0.11391E-02  1.0043      8.5588      637.42     0.78886E-30
   2    11    2     3    72   0.76887E-03  1.0050      9.0721      636.96     0.78886E-30
   2    12    1     3    75   0.76887E-03  1.0058      9.5648      636.35     0.78886E-30
   2    13    1     3    78   0.11533E-02  1.0070      10.277      635.25     0.78886E-30
   2    14    1     4    82   0.17300E-02  1.0087      11.306      633.37     0.78886E-30
   2    15    1     6    88   0.25949E-02  1.0113      12.802      630.21     0.78886E-30
   2    16    1     5    93   0.25949E-02  1.0139      14.273      626.81     0.78886E-30
   2    17    1     7   100   0.38924E-02  1.0178      16.477      621.42     0.78886E-30
   2    18    1     6   106   0.38924E-02  1.0217      18.704      615.77     0.78886E-30
   2    19    2     4   116   0.26274E-02  1.0243      20.229      611.83     0.78886E-30
   2    20    1     4   120   0.26274E-02  1.0269      21.777      607.80     0.78886E-30

The following details the contents of the various fields in the monitor file:

LOAD STEP - The current load step number.

SUB-STEP - The current substep (time step) number.

NO. ATTEMPT - The number of attempts made in solving the current substep. This number is equal to the number of failed attempts (bisections) plus one (the successful attempt).

NO. ITER -. The number of iterations used by the last successful attempt.

TOTL. ITER - Total cumulative number of iterations (including each iteration used by a bisection).

INCREMENT -

TIME/LFACT - Time or load factor increments for the current substep.

TOTAL

TIME/LFACT - Total time (or load factor) for the last successful attempt in the current substep.

VARIAB 1 - Variable field 1. In this example, the field is reporting the UZ value. By default, this field lists the CPU time used up to (but not including) the current substep.

VARIAB 2 - Variable field 2. In this example, the field is reporting the MZ value. By default, this field lists the maximum displacement in the entire structure.

VARIAB 3 - Variable field 3. By default (and in the example), this field reports the maximum equivalence plastic strain in the entire structure.

Main Menu >Preprocessor >Loads >Nonlinear >Monitor

Main Menu >Solution >Nonlinear >Monitor

Calculates Mooney-Rivlin hyperelastic constants from test data.

PREP7:Materials

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

Name of the array parameter containing the laboratory strain data. You must have previously filled this array with engineering strain values (no other measure of strain is valid) before you execute *MOONEY. If Uniaxial data (tension or compression) are to be used, they must be placed in the first column of this array. If Equibiaxial data (tension or compression) are to be used, they must be placed in the second column of this array. If Shear data are to be used, they must be placed in the third column of this array. If any test type is not used, the corresponding column of the STRAIN array should be left blank.

Name of the array parameter containing the laboratory stress data. You must have previously filled the STRESS array with engineering stress values (no other measure of stress is valid) before you execute *MOONEY. The stress values must be placed in the STRESS array in locations corresponding to the locations of the companion strain values in the STRAIN array.

Unused field

Name of the array parameter vector to which the hyperelastic material constants will be written. The CONST array must have been previously defined [*DIM] to have a dimension of either 2, 5, or 9 (corresponding to a two-term, five-term, or nine-term Mooney-Rivlin material model). Using any dimension other than 2, 5, or 9 for the CONST vector array will cause an error message to be generated.

Name of the array parameter vector in which calculated engineering stress values determined from the Mooney-Rivlin constants will be placed. For this and the following two parameters (SORTSN, SORTSS), column 1 contains uniaxial data, column 2 contains equibiaxial data, and column 3 contains shear data.

Name of the array parameter vector in which the sorted experimental strain data will be placed.

Name of the array parameter vector in which the sorted laboratory test data will be placed.

Text file name (32 characters maximum) to which the determined constants will be written (in the form of TBDATA commands). Defaults to Jobname.

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

The array parameters STRAIN, STRESS, CALC, SORTSN, and SORTSS must have been previously defined [*DIM] to have dimensions Nx3, where N is the maximum number of data points in any one of the three basic test types (uniaxial, equibiaxial, and planar or pure shear).

Calculates the Mooney-Rivlin hyperelastic material constants from laboratory stress-strain test data. Once the program determines these constants, it writes them to three places: to the database (in memory), to the array parameter CONST, and to a text file (in the form of TBDATA commands). You can use the *EVAL command to check the quality of the resulting material properties. You must have previously dimensioned [*DIM] all array parameters used by *MOONEY, and you must also have set LAB=MOONEY and TBOPT=1 on the TB command, before you execute *MOONEY.

Up to three different types of laboratory stress-strain tests can be used (in any combination):

· Equibiaxial (tension or compression)

· Shear (Planar Tension or Planar Compression)

Menu Paths

Main Menu >Preprocessor >Material Props >Mooney-Rivlin >Calculate Const

Performs matrix operations on array parameter matrices.

APDL:ArrayParameters

	Mp Me St DY LP Th E3 E2 FL PP ED

The name of the resulting array parameter matrix. See*SET for name restrictions. The parameter must exist as a dimensioned array [*DIM].

First array parameter matrix input to the operation.

Matrix operations:

MULT - Matrix multiply: Multiplies Par1 by Par2. The number of rows of Par2 must equal the number of columns of Par1 for the operation.

SOLV - Solution of simultaneous equations: Solves the set of n equations of n terms of the form
a_n1x₁ + a_n2x₂ + ^... + a_nnx_n = b_n where Par1 contains the matrix of a-coefficients, Par2 the vector of b-values, and ParR the vector of x-results. Par1 must be a square matrix. The operations must be linear, independent, and well conditioned. Warning: non-independent or ill-conditioned equations can cause erroneous results.

SORT - Matrix sort: Sorts matrix Par1 according to sort vector Par2 and places the result in Par1. Rows of Par1 are moved to the corresponding positions indicated by the values of Par2. Non-integer values are truncated to integers. Par2 may be a column of Par1 (in which case it will also be reordered). ParR is the vector of initial row positions. Sorting Par1 according to ParR should reproduce the initial ordering.

COVAR - Covariance: the measure of association between two columns of the input matrix (Par1). Par1, of size m runs (rows) by n data (columns) is first processed to produce a row vector containing the mean of each column which is transposed to a column vector (Par2) of n array elements. The Par1 and Par2 operation then produces a resulting nxn matrix (ParR) of covariances (with the variances as the diagonal terms).

CORR - Correlation: the correlation coefficient between two variables. The input matrix (Par1), of size m runs (rows) by n data (columns), is first processed to produce a row vector containing the mean of each column which is then transposed to a column vector (Par2) of n array elements. The Par1 and Par2 operation then produces a resulting nxn matrix (ParR) of correlation coefficients (with a value of 1.0 for the diagonal terms).

Second array parameter matrix input to the operation. For the COVAR and CORR operations, this parameter must exist as a dimensioned array vector without specified values since its values (means) will be calculated as part of the operations.

Operates on two input array parameter matrices and produces one output array parameter matrix according to:

where the operations (o) are described above. Each array starting element number must be defined for each array parameter matrix. For example, *MOPER,A(2,3),B(1,4),MULT,C(1,5) multiplies submatrix B (starting at element (1,4)) by submatrix C (starting at element (1,5)) and puts the result in matrix A (starting at element (2,3)).

The diagonal corner elements for each submatrix must be defined: the upper left corner by the array starting element (on this command), the lower right corner by the current values from the *VCOL and *VLEN commands. The default values are the (1,1) element and the last element in the matrix. No operations progress across matrix planes (in the 3rd dimension). Absolute values and scale factors may be applied to all parameters [*VABS, *VFACT]. Results may be cumulative [*VCUM]. Array elements should not be skipped with the *VMASK and the NINC value of the *VLEN specifications. See the *VOPER command for details.

This command is valid in any processor.

Utility Menu >Parameters >Array Operations >Matrix Operations

Specifies meshing options.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Meshing option to be specified (dictates the meaning of Value):

EXPND - Area mesh expansion (or contraction) option. (This option is the same as SMRTSIZE,,,EXPND.) This option is used to size internal elements in an area based on the size of the elements on the area's boundaries. Value is the expansion (or contraction) factor. For example, issuing MOPT,EXPND,2 before meshing an area will allow a mesh with elements that are approximately twice as large in the interior of an area as they are on the boundary. If Value is less than 1, a mesh with smaller elements on the interior of the area will be allowed. Value for this option should be greater than 0.5 but less than 4. Value defaults to 1, which does not allow expansion or contraction of internal element sizes (except when meshing flat areas and using the IESZ option). If Value=0, the default value of 1 will be used. The actual size of the internal elements will also depend on the TRANS and IESZ options, if used.

TETEXPND - Tet-mesh expansion (or contraction) option. This option is used to size internal elements in a volume based on the size of the elements on the volume's boundaries. Value is the expansion (or contraction) factor. For example, issuing MOPT,TETEXPND,2 before meshing a volume will allow a mesh with elements that are approximately twice as large in the interior of the volume as they are on the boundary. If Value is less than 1, a mesh with smaller elements on the interior of the volume will be allowed. Value for this option should be greater than 0.1 but less than 3. Value defaults to 1, which does not allow expansion or contraction of internal element sizes. If Value=0, the default value of 1 will be used. If Value is greater than 2, mesher robustness may be affected. The TETEXPND option is supported for both the VMESH and FVMESH commands. Tet-mesh expansion is the only mesh control supported by FVMESH.

TRANS - Mesh transition option. (This option is the same as SMRTSIZE,,,,TRANS.) This option is used to control how rapidly elements are permitted to change in size from the boundary to the interior of an area. Value is the transitioning factor. Value defaults to 2.0, which permits elements to approximately double in size as they approach the interior of the area. (If Value=0, the default value of 2 will be used.) Value must be greater than 1 and, for best results, should be less than 4. The actual size of the internal elements will also depend on the EXPND and IESZ options, if used.

IESZ - Internal element size option. Value is the default internal element edge length for flat areas. This option is similar to the ESIZE,SIZE option, except that IESZ applies only to elements on the interior of an area (rather than on the boundary of the area). This option only works with completely flat areas. Value may be any positive number. If Value=0 (default), the IESZ option is turned off. The actual size of the internal elements will also depend on the EXPND and TRANS options, if used.

AMESH - Triangle surface meshing option. Valid inputs for Value are:

DEFAULT - Let ANSYS choose which triangle mesher to use. In most cases, ANSYS will choose the main triangle mesher, which is the Riemann space mesher. If the chosen mesher fails for any reason, ANSYS invokes the alternate mesher and re-tries the meshing operation. (Default.)

MAIN - ANSYS uses the main triangle mesher (Riemann space mesher), and it does not invoke an alternate mesher if the main mesher fails. The Riemann space mesher is well suited for most surfaces.

ALTERNATE - ANSYS uses the first alternate triangle mesher (3-D tri-mesher), and it does not invoke another mesher if this mesher fails. This option is not recommended due to speed considerations. However, for surfaces with degeneracies in parametric space, this mesher often provides the best results.

ALT2 - ANSYS uses the second alternate triangle mesher (2-D parametric space mesher), and it does not invoke another mesher if this mesher fails. This option is not recommended for use on surfaces with degeneracies (spheres, cones, etc.) or poorly parameterized surfaces because poor meshes may result.

QMESH - Quadrilateral surface meshing option. (Quadrilateral surface meshes will differ based on which triangle surface mesher is selected. This is true because all free quadrilateral meshing algorithms use a triangle mesh as a starting point.) Valid inputs for Value are:

DEFAULT - Let ANSYS choose which quadrilateral mesher to use. In most cases, ANSYS will choose the main quadrilateral mesher, which is the Q-Morph (quad-morphing) mesher. For very coarse meshes, ANSYS may choose the alternate quadrilateral mesher instead. In most cases, the Q-Morph mesher results in higher quality elements. If either mesher fails for any reason, ANSYS invokes the other mesher and re-tries the meshing operation. (Default.)

MAIN - ANSYS uses the main quadrilateral mesher (Q-Morph mesher), and it does not invoke the alternate mesher if the main mesher fails.

ALTERNATE - ANSYS uses the alternate quadrilateral mesher, and it does not invoke the Q-Morph mesher if the alternate mesher fails. To use the alternate quadrilateral mesher, you must also select MOPT,AMESH,ALTERNATE or MOPT,AMESH,ALT2.

VMESH - Tetrahedral element meshing option. Valid inputs for Value are:

DEFAULT - Let ANSYS choose which tetrahedra mesher to use. ANSYS always uses the alternate tetrahedra mesher when meshing with p-elements. Otherwise, it usually uses the main tetrahedra mesher. (Default.)

MAIN - Use the main tetrahedra mesher (Delaunay technique mesher). (GHS3D meshing technology by P.L. George, INRIA, France.) For most models, this mesher is significantly faster than the alternate mesher.

ALTERNATE - Use the alternate tetrahedra mesher (advancing front mesher). This mesher is the ANSYS Revision 5.2 tetrahedra mesher. It does not support the generation of a tetrahedral volume mesh from facets [FVMESH]. If this mesher is selected and you issue the FVMESH command, ANSYS uses the main tetrahedra mesher to create the mesh from facets and issues a warning message to notify you.

SPLIT - Quad splitting option for non-mapped meshing. If Value=1, ON, or ERR, quadrilateral elements in violation of shape error limits are split into triangles (default). If Value=2 or WARN, quadrilateral elements in violation of either shape error or warning limits are split into triangles. If Value=OFF, splitting does not occur, regardless of element quality.

LSMO - Line smoothing option. Value can be ON or OFF. If Value=ON, smoothing of nodes on area boundaries is performed during smoothing step of meshing. During smoothing, node locations are adjusted to achieve a better mesh. If Value=OFF (default), no smoothing takes place at area boundaries.

CLEAR - This option affects the element and node numbering after clearing a mesh. If Value=ON (default), the starting node and element numbers will be the lowest available number after the nodes and elements are cleared. If Value=OFF, the starting node and element numbers are not reset after the clear operation (which was the default behavior for ANSYS versions prior to Release 5.3).

PYRA - Transitional pyramid elements option. Value can be ON or OFF. If Value=ON (default), ANSYS automatically creates transitional pyramid elements, when possible. Pyramids may be created at the interface of tetrahedral and hexahedral elements, or directly from quadrilateral elements. For pyramids to be created, you must also issue the command MSHAPE,1,3D (degenerate three-dimensional elements). If Value=OFF, ANSYS does not create transitional pyramid elements.

TIMP - Identifies the level of tetrahedra improvement to be performed when the next free volume meshing operation is initiated [VMESH, FVMESH]. (For levels 2-5, improvement occurs primarily through the use of face swapping and node smoothing techniques.) Valid inputs for Value are:

0 - Turn off tetrahedra improvement. Although this value can lead to faster tetrahedral mesh creation, it is not recommended because it often leads to poorly shaped elements and mesh failures.

1 - Do the minimal amount of tetrahedra improvement. (Default.) This option is supported by the main tetrahedra mesher only [MOPT,VMESH,MAIN]. If the alternate tetrahedra mesher [MOPT,VMESH,ALTERNATE] is invoked with this setting, ANSYS automatically performs tetrahedra improvement at level 3 instead [MOPT,TIMP,3].

2 - Perform the least amount of swapping/smoothing. No improvement occurs if all tetrahedral elements are within acceptable limits.

3 - Perform an intermediate amount of swapping/smoothing. Some improvement is always done.

4 - Perform the greatest amount of swapping/smoothing. Meshing takes longer with this level of improvement, but usually results in a better mesh.

5 - Perform the greatest amount of swapping/smoothing, plus additional improvement techniques. This level of improvement usually produces results that are similar to those at level 4, except for very poor meshes.

6 - For linear tetrahedral meshes, this value provides the same level of improvement as MOPT,TIMP,5. For quadratic tetrahedral meshes, this value provides an additional pass of cleanup. This value is supported for both the main [MOPT,VMESH,MAIN] and alternate [MOPT,VMESH,ALTERNATE] tetrahedra meshers.

STAT - Display status of MOPT settings. Value is ignored.

DEFA - Set all MOPT options to default values. Value is ignored.

Value, as described for each different Lab above.

See Chapter 7 of the ANSYS Modeling and Meshing Guide for more information on the MOPT command and its options.

Main Menu >Preprocessor >Mesher Opts

Main Menu >Preprocessor >Size Cntrls >Area Cntrls

Main Menu >Preprocessor >Size Cntrls >Volu Cntrls

Utility Menu >List >Status >Preprocessor >Solid Model

Calculates and moves a node to an intersection.

PREP7:Nodes

	Mp Me St DY LP Th E3 E2 FL PP ED

Move this node. If NODE = 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 NODE.

First coordinate system number. Defaults to 0 (global Cartesian).

Input one or two values defining the location of the node in this coordinate system. Input "U" for unknown value(s) to be calculated and input "E" to use an existing coordinate value. Fields are R1,1,Z1 for cylindrical, or R1,1,1 for spherical or toroidal.

Second coordinate system number.

Input two or one value(s) defining the location of the node in this coordinate system. Input "U" for unknown value(s) to be calculated and input "E" to use an existing coordinate value. Fields are R2,2,Z2 for cylindrical, or R2,2,2 for spherical or toroidal.

Calculates and moves a node to an intersection location. The node may have been previously defined (at an approximate location) or left undefined (in which case it is internally defined at the SOURCE location). The actual location is calculated from the intersection of three surfaces (implied from three coordinate constants in two different coordinate systems). The three (of six) constants easiest to define should be used. The program will calculate the remaining three coordinate constants. All arguments, except KC1, must be input. Use the repeat command [*REPEAT] after the MOVE command to define a line of intersection by repeating the move operation on all nodes of the line.

Surfaces of constant value are implied by some commands by specifying a single coordinate value. Implied surfaces are used with various commands [MOVE, KMOVE, NSEL, etc.]. Three surfaces are available with each of the four coordinate system types. Values or X, Y, or Z may be constant for the Cartesian coordinate system; values of R, , or Z for the cylindrical system; and values of R, , for the spherical and toroidal systems. For example, an X value of 3 represents the Y-Z plane (or surface) at X=3. In addition, the parameters for the cylindrical and spherical coordinate systems may be adjusted [CS, LOCAL] to form elliptical surfaces. For surfaces in elliptical coordinate systems, a surface of "constant" radius is defined by the radius value at the X-axis. Surfaces of constant value may be located in local coordinate systems [LOCAL, CLOCAL, CS, or CSKP] to allow for any orientation.

The intersection calculation is based on an iterative procedure (250 iterations maximum) and a tolerance of 1.0E-4. The approximate location of a node should be sufficient to determine a unique intersection if more than one intersection point is possible. Tangent "intersections" should be avoided. If an intersection is not found, the node is placed at the last iteration location.

Main Menu >Preprocessor >Move / Modify >To Intersect

Defines a linear material property as a constant or a function of temperature.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Valid material property label. Applicable labels are listed under "Material Properties" in the input table for each element type in the ANSYS Elements Reference. See Section 2.4 of the ANSYS Elements Reference for more complete property label definitions:

EX - Elastic moduli (also EY, EZ).

ALPX - Coefficients of thermal expansion (also ALPY, ALPZ).

REFT - Reference temperature. Must be defined as a constant; C1 through C4 are ignored.

PRXY - Major Poisson's ratios (also PRYZ, PRXZ).

NUXY - Minor Poisson's ratios (also NUYZ, NUXZ).

GXY - Shear moduli (also GYZ, GXZ).

DAMP - K matrix multiplier for damping.

MU - Coefficient of friction.

DENS - Mass density.

C - Specific heat.

ENTH - Enthalpy.

KXX - Thermal conductivities (also KYY, KZZ).

HF - Convection or film coefficient.

EMIS - Emissivity.

QRATE - Heat generation rate.

VISC - Viscosity.

SONC - Sonic velocity.

RSVX - Electrical resistivities (also RSVY, RSVZ).

PERX - Electrical permittivities (also PERY, PERZ).

MURX - Magnetic relative permeabilities (also MURY, MURZ).

MGXX - Magnetic coercive forces (also MGYY, MGZZ).

LSST - Dielectric loss tangent. Valid for high-frequency electromagnetic analyses only.

Material reference number to be associated with the elements (defaults to the current MAT setting [MAT]).

Material property value, or if a property-versus-temperature polynomial is being defined, the constant term in the polynomial.

Coefficients of the linear, quadratic, cubic, and quartic terms, respectively, in the property-versus-temperature polynomial. Leave blank (or set to zero) for a constant material property.

MP defines a linear material property as a constant or in terms of a fourth order polynomial as a function of temperature. See the TB command for nonlinear material property input. Linear material properties typically require a single substep for solution, whereas nonlinear material properties require multiple substeps; see Section 2.4 of the ANSYS Elements Reference for details.

If the constants C1 - C4 are input, the polynomial

is evaluated at discrete temperature points with linear interpolation between points (i.e., piece-wise linear representation) and a constant-valued extrapolation beyond the extreme points. The MPTEMP or MPTGEN commands must be used for second and higher order properties to define appropriate temperature steps. Constant and first-order properties use two discrete points (9999°) by default.

This command is also valid in SOLUTION.

In ANSYS without Emag 3-D or Emag 2-D enabled, the MUR_ and MG__ properties are not allowed. In ANSYS/LinearPlus and ANSYS/Thermal, all structural and thermal properties are allowed except DAMP and MU. In ANSYS/Emag 3-D and ANSYS/Emag 2-D, only the RSV_, PER_, MUR_, and MG__ properties are allowed. The LSST property is available only for products that include ANSYS/Emag 3-D, and can be used only in high-frequency analyses.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Polynomial

Main Menu >Preprocessor >Material Props >Polynomial

Main Menu >Solution >Other >Change Mat Props >Polynomial

Modifies temperature-dependent coefficients of thermal expansion.

PREP7:Materials

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

Material number for which the coefficients of thermal expansion (CTE's) are to be modified. Defaults to 1.

Definition temperature at which the existing CTE-versus-temperature tables were defined. Defaults to zero.

This command converts temperature-dependent CTE data (properties ALPX, ALPY, ALPZ) from the definition temperature (DEFTEMP) to the reference temperature defined by MP,REFT or TREF. If both the MP,REFT and TREF commands have been issued, the reference temperature defined by the MP,REFT command will be used.

See Section 2.4 of the ANSYS Elements Reference and Section 2.1.3 of the ANSYS Theory Reference for more details.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Convert ALPx

Main Menu >Preprocessor >Material Props >Convert ALPx

Main Menu >Solution >Other >Change Mat Props >Convert ALPx

Changes the material number attribute of an element.

PREP7:Materials SOLUTION:MiscLoads

	Mp Me St DY LP Th E3 E2 FL PP ED

Assign this material number to the element. Material numbers are defined with the material property commands [MP].

Element for material change. If ALL, change materials for all selected elements [ESEL].

Changes the material number of the specified element. Between load steps in SOLUTION, material properties cannot be changed from linear to nonlinear, or from one nonlinear option to another.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Change Mat Num

Main Menu >Preprocessor >Material Props >Change Mat Num

Main Menu >Solution >Other >Change Mat Props >Change Mat Num

Defines property data to be associated with the temperature table.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Valid property label. Applicable labels are listed under "Material Properties" in the input table for each element type in the ANSYS Elements Reference. See Section 2.4 of the ANSYS Elements Reference for more complete property label definitions:

EX - Elastic moduli (also EY, EZ).

ALPX - Coefficients of thermal expansion (also ALPY, ALPZ). (See also MPAMOD command for adjustment to reference temperature).

REFT - Reference temperature.

PRXY - Major Poisson's ratios (also PRYZ, PRXZ).

NUXY - Minor Poisson's ratios (also NUYZ, NUXZ).

GXY - Shear moduli (also GYZ, GXZ).

DAMP - K matrix multiplier for damping.

MU - Coefficient of friction.

DENS - Mass density.

C - Specific heat.

ENTH - Enthalpy.

KXX - Thermal conductivities (also KYY, KZZ).

HF - Convection or film coefficient.

EMIS - Emissivity.

QRATE - Heat generation rate.

VISC - Viscosity.

SONC - Sonic velocity.

RSVX - Electrical resistivities (also RSVY, RSVZ).

PERX - Electrical permittivities (also PERY, PERZ).

MURX - Magnetic relative permeabilities (also MURY, MURZ).

MGXX - Magnetic coercive forces (also MGYY, MGZZ).

LSST - Dielectric loss tangent.

Material reference number to be associated with the elements (defaults to 1 if you specify zero or no material number).

Starting location in table for generating data. For example, if STLOC=1, data input in the C1 field is the first constant in the table. If STLOC=7, data input in the C1 field is the seventh constant in the table, etc. Defaults to the last location filled + 1.

Property data values assigned to six locations starting with STLOC. If a value is already in this location, it is redefined. A blank (or zero) value for C1 resets the previous value in STLOC to zero. A value of zero can only be assigned by C1. Blank (or zero) values for C2 to C6 leave the corresponding previous values unchanged.

The MPDATA command may also be used to enter temperature dependent properties for fluids in a CFD analysis with FLOTRAN via FLUID141 and FLUID142. Valid MPDATA labels for a CFD analysis in a non-solid region are:

Density of fluid. This is the same as the label used to specify mass density with the FLDATA command.

Specific heat of fluid. This is equivalent to the SPHT label used to specify conductivity with the FLDATA command.

Thermal conductivity of fluid.

Viscosity of fluid. This is the same as the label used to specify kinematic velocity with the FLDATA command.

Defines a table of property data to be associated with the temperature table. Repeat MPDATA command for additional values (100 maximum). Temperatures must be defined first [MPTEMP]. Also stores assembled property function table (temperature and data) in virtual space.

This command is also valid in SOLUTION.

In ANSYS without Emag 3-D or Emag 2-D enabled, the MUR_ and MG__ properties are not allowed. In ANSYS/LinearPlus and ANSYS/Thermal, all structural and thermal properties are allowed except DAMP and MU. In ANSYS/Emag 3-D and ANSYS/Emag 2-D, only the RSV_, PER_, MUR_, and MG__ properties are allowed. Only products that include ANSYS/Emag 3-D can use the LSST property.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Prop Table

Main Menu >Preprocessor >Material Props >Prop Table

Main Menu >Solution >Other >Change Mat Props >Prop Table

Deletes linear material properties.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Material property label (see MP command for valid labels). If ALL, delete properties for all applicable labels.

Delete materials from MAT1 to MAT2 (defaults to MAT1) in steps of INC (defaults to 1). If MAT1 = ALL, MAT2 and INC are ignored and the properties for all materials are deleted.

This command is also valid in SOLUTION.

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

Main Menu >Preprocessor >Material Props >Define MAT Model

Main Menu >Preprocessor >Material Props >Delete Mat Props

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

Reassembles existing material data with the temperature table.

PREP7:Materials

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

Material property label associated with MATF.

Material reference number of property to restore from virtual space.

Material property label associated with MATT (defaults to label associated with MATF).

Material reference number assigned to generated property (defaults to MATF).

Restores into the database (from virtual space) a data table previously defined [MP] for a particular property, assembles data with current database temperature table, and stores back in virtual space as a new property.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Modify Temps

Main Menu >Preprocessor >Material Props >Modify Temps

Main Menu >Solution >Other >Change Mat Props >Modify Temps

Sets the default material library read and write paths.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Determines what path is being set. Possible values are:

READ - Set the read path.

WRITE - Set the write path.

STAT - Report what read and write paths are currently in use.

The directory path to be used for material library files.

The /MPLIB command sets two path strings used in conjunction with the material library feature and the MPREAD and MPWRITE commands.

For MPREAD, when you use the LIB option and the directory portion of the specification for the material library file is blank, the command searches for the file in these locations: the current working directory, the user's home directory, the user-specified material library directory (as defined by the /MPLIB,READ,PATH command), and /ansys_dir/matlib.

For MPWRITE, when you use the LIB option and the directory portion of the specification for the material library file is blank, the command writes the material library file to the directory specified by the /MPLIB,WRITE,PATH command (if that path has been set). If the path has not been set, the default is to write the file to the current working directory.

The Material Library files supplied with the distribution disks are meant for demonstration purposes only. These files are not intended for use in customer applications.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Lib Path Status

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Library Path

Main Menu >Preprocessor >Material Props >Material Library >Lib Path Status

Main Menu >Preprocessor >Material Props >Material Library >Library Path

Main Menu >Solution >Other >Change Mat Props >Material Library >Lib Path Status

Main Menu >Solution >Other >Change Mat Props >Material Library >Library Path

Lists linear material properties.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

List materials from MAT1 to MAT2 (defaults to MAT1) in steps of INC (defaults to 1). If MAT1 = ALL (default), MAT2 and INC are ignored and properties for all material numbers are listed.

Material property label (see the MP command for labels). If ALL (or blank), list properties for all labels. If EVLT, list properties for all labels evaluated at TEVL.

Evaluation temperature for Lab=EVLT listing (defaults to BFUNIF).

This command is valid in any processor.

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

Main Menu >Preprocessor >Material Props >List

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

Utility Menu >List >Properties >All Materials

Utility Menu >List >Properties >All Matls, All Temps

Utility Menu >List >Properties >All Matls, Specified Temp

Utility Menu >List >Properties >Specified Matl, All Temps

Associates the material properties to an explicit dynamics material model.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Material property number identifying the material model. This number must correspond to a material type number on the MP command.

Number identifying the type of explicit dynamics material model to be used for material properties. Valid MODTYPE numbers are listed below.

MPMOD associates a material ID (MATNUM) with a valid explicit dynamics material model so that the material model can be viewed and edited in the Graphical User Interface (GUI). In interactive mode, MPMOD is issued automatically when explicit materials are defined. For batch (command) input, appropriate MPMOD commands should be included in the input stream if you intend to read the input into an interactive session at some later time. However, MPMOD is not required if you intend to run the analysis entirely in batch mode. If you make an incorrect material association with MPMOD, use MPUNDO to remove the association.

Main Menu >Preprocessor >Material Props >Define MAT Model

Removes an incorrectly-specified material model association.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Material property number identifying the material model. This number must correspond to a material number on the MP command.

Use this command to undo an incorrectly-specified material number or material model type number (MATNUM or MODTYPE on MPMOD). Issue MPUNDO,MATNUM to remove the material model association with the specified material property number. To respecify the material number with another material model, re-issue MPMOD with the correct material number and material model type number.

Main Menu >Preprocessor >Material Props >Define MAT Model

Plots linear material properties as a function of temperature.

PREP7:Materials

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

Linear material property label (EX, EY, etc.) [MP].

Material reference number.

Minimum abscissa value to be displayed.

Maximum abscissa value.

Minimum property (ordinate) value to be displayed.

Maximum property value.

This command is valid in any processor.

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

Main Menu >Preprocessor >Material Props >Graph

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

Utility Menu >Plot >Materials

Reads a file containing material properties.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Name of a material file. (32 characters maximum). Defaults to JOBNAM.

File name extension (eight characters maximum). If you do not specify the Lib option, the default extension is MP. If you use the Lib option, the default extension is units_MPL,where units is the system of units currently being used. (See the description of the /UNITS command.) For example, if /UNITS is set to SI, the extension defaults to .SI_MPL. If /UNITS is set to BIN, the default extension is .BIN_MPL

Name of the directory (64 characters maximum) into which the named file will be written. If you omit the LIB option, the default is the current working directory. If you specify the LIB option, the default is the following search path: the current working directory, the user's home directory, MPLIB_DIR (as specified by the /MPLIB,READ,PATH command), and /ansys_dir/matlib (as defined by installation).

Reads material library files previously written with the MPWRITE command. (See the description of the LIB option for the MPWRITE command.) The only allowed value for LIB is LIB.

The LIB field indicates that the specified file was written by MPWRITE using the LIB option, and that the file is consistent with the material library file format. When the MPREAD command executes, the ANSYS program reads material properties defined in the specified file into the current ANSYS working database. The currently selected material, as defined by the MAT command (MAT,MAT), determines the material number used when reading the material properties. The LIB option for MPREAD and MPWRITE supports storing and retrieving both linear and nonlinear properties.

Material properties written to a file without the LIB option do not support nonlinear properties. Also, properties written to a file without the LIB option are restored in the same material number as originally defined. To avoid errors, use MPREAD with the LIB option only when reading files written using MPWRITE with the LIB option.

If you omit the LIB option for MPREAD, this command supports only linear properties.

Material numbers are hardcoded. If you write a material file without specifying the LIB option, then read that file in using the MPREAD command with the LIB option, the ANSYS program will not write the file to a new material number. Instead, it will write the file to the "old" material number (the number specified on the MPWRITE command that created the file.)

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Export Library

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Import Library

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Select Units

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Read from File

Main Menu >Preprocessor >Material Props >Material Library >Export Library

Main Menu >Preprocessor >Material Props >Material Library >Import Library

Main Menu >Preprocessor >Material Props >Material Library >Select Units

Main Menu >Preprocessor >Material Props >Read from File

Main Menu >Solution >Other >Change Mat Props >Material Library >Export Library

Main Menu >Solution >Other >Change Mat Props >Material Library >Import Library

Main Menu >Solution >Other >Change Mat Props >Material Library >Select Units

Main Menu >Solution >Other >Change Mat Props >Read from File

Specifies that radiation matrices are to be printed.

AUX12:RadiationSubstructures

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

Print key:

0 - Do not print matrices.

1 - Print matrices.

Notes

Specifies that the element and node radiation matrices are to be printed when the WRITE command is issued. If KEY=1, form factor information for each element will also be printed.

Main Menu >Radiation Matrix >Write Matrix

Defines a temperature table for material properties.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Starting location in table for entering temperatures. For example, if STLOC=1, data input in the T1 field applies to the first constant in the table. If STLOC=7, data input in the T1 field applies to the seventh constant in the table, etc. Defaults to the last location filled + 1.

Temperatures assigned to six locations starting with STLOC. If a value is already in this location, it will be redefined. A blank (or zero) value for T1 resets the previous value in STLOC to zero. A value of zero can only be assigned by T1. Blank (or zero) values for T2 to T6 leave the corresponding previous values unchanged.

Notes

Defines a temperature table to be associated with the property data table [MPDATA]. These temperatures are also used for polynomial property evaluation, if defined [MP]. Temperatures must be defined in non-descending order. Issue MATER $STAT to list the current temperature table. Repeat MPTEMP command for additional temperatures (100 maximum). If all arguments are blank, the temperature table is erased.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Temp Table

Main Menu >Preprocessor >Material Props >Temp Table

Main Menu >Solution >Other >Change Mat Props >Temp Table

Adds temperatures to the temperature table by generation.

PREP7:Materials

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

Starting location in table for generating temperatures. Defaults to last location filled + 1.

Number of temperatures to be generated (1-100).

Temperature assigned to STLOC location.

Increment previous temperature by TINC and assign to next location until all NUM locations are filled.

Adds temperatures to the temperature table by generation. May be used in combination (or in place of) the MPTEMP command.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Generate Temp

Main Menu >Preprocessor >Material Props >Generate Temp

Main Menu >Solution >Other >Change Mat Props >Generate Temp

Restores a temperature table previously defined.

PREP7:Materials

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

Material property label [MP].

Material reference number.

Restores into the database (from virtual space) a temperature table previously defined [MP] for a particular property. The existing temperature table in the database is erased before this operation.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Restore Temps

Main Menu >Preprocessor >Material Props >Restore Temps

Main Menu >Solution >Other >Change Mat Props >Restore Temps

Writes linear material properties in the database to a file (if the Lib option is not specified) or writes both linear and nonlinear material properties (if Lib is specified) from the database to a file.

PREP7:Materials

	Mp Me St DY LP Th E3 E2 FL PP ED

Material library file name (32 characters maximum). Defaults to JOBNAM.

Extension of the material library file name (eight characters maximum). If you omit the Lib option, the default extension is MP. If you specify the Lib option, the default extension is units_MPL, where units is the system of units currently in use. (See the description of the /UNITS command.). For example, if/UNITS is set to BIN, the extension defaults to .BIN_MPL.

The name of the directory (64 characters maximum) into which the named file will be written. If you do not specify the LIB option, the default directory is the current working directory. If you specify LIB, and you have specified a material library directory (via the/MPLIB command), that directory is the default. Otherwise, the default is the current working directory.

The only value allowed for this field is the string "LIB."

The LIB option indicates that you wish to have properties associated with the material (MAT) written to the specified material library file using the material library file format. The material library file format is ASCII-text-based ANSYS command input. Certain commands associated with this format have been modified to interpret the string "_MATL" to mean the currently selected material. This feature makes the material library file independent of the material number in effect when the file was written; this enables you to restore the properties into the ANSYS database using the material number of your choice. The LIB option also enables you to save both linear and nonlinear properties. If you omit the LiB option, you can save linear properties only.

Specifies the material to be written to the named material library file. There is no default; you must either specify a material or omit the MAT argument. Even if you specify a MAT value, the ANSYS program ignores it if the LIB argument is not specified.

Writes linear material properties currently in the database to a file. The file is rewound before and after writing.

This command is also valid in SOLUTION.

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Export Library

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Import Library

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Material Library >Select Units

Main Menu >Preprocessor >Loads >Other >Change Mat Props >Write to File

Main Menu >Preprocessor >Material Props >Material Library >Export Library

Main Menu >Preprocessor >Material Props >Material Library >Import Library

Main Menu >Preprocessor >Material Props >Material Library >Select Units

Main Menu >Preprocessor >Material Props >Write to File

Main Menu >Solution >Other >Change Mat Props >Material Library >Export Library

Main Menu >Solution >Other >Change Mat Props >Material Library >Import Library

Main Menu >Solution >Other >Change Mat Props >Material Library >Select Units

Main Menu >Solution >Other >Change Mat Props >Write to File

Enables you to reissue the graphics command macro "name" during a replot or zoom operation.

GRAPHICS:SetUp

	Mp Me St DY LP Th E3 E2 FL PP ED

The name identifying the macro file or macro block on a macro library file. The name can contain up to eight characters maximum and must begin with a letter.

Values to be passed into the file or block.

This command reissues the graphics command macro "name" during a replot operation [/REPLOT] or a zoom [/ZOOM] operation. The ANSYS program passes the command macro arguments to the replot and zoom feature for use by the graphics macro. You should place the /MREP command at the end of the graphics command macro, following the last graphics command within the macro, to enable the replot or zoom feature.

This command cannot be accessed directly in the menu.

Specifies the approach to discretize the advection term in a species transport equation.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Choice of approach to discretize the advection term:

MSU - Monotone Streamline Upwind approach (default).

SUPG - Streamline Upwind / Petrov-Galerkin approach.

This command is valid for the multiple species transport option in a FLOTRAN analysis. See the ANSYS Theory Reference for more information on the advection term.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Main Menu >Solution >FLOTRAN Set Up >Multiple Species

Activates and controls mass fraction capping for a species.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Key to activate mass fraction capping:

OFF - Capping not enforced (default).

ON - Capping will be enforced.

Upper and lower bounds on mass fraction if capping is activated. Default to 1.0 and 0.0 respectively.

Notes

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Defines multiple species data applicable to all species.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

The algebraic species number whose mass fraction is calculated by subtracting the sum of the mass fractions of all other species from 1.0. This ensures that the sum of the mass fractions of all the species is 1.0. Defaults to 2.

The universal gas constant. Defaults to 8314.3 (SI units).

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Writes an output message via the ANSYS message subroutine.

APDL:MacroFiles

	Mp Me St DY LP Th E3 E2 FL PP ED

Label for output and termination control:

INFO - Writes the message with no heading (default).

NOTE - Writes the message with a "NOTE" heading.

WARN - Writes the message with a "WARNING" heading. Also writes the message to the errors file, Jobname.ERR.

ERROR - Writes the message with a "ERROR" heading and causes run termination (if batch) at earliest "clean exit" point. Also writes the message to the errors file, Jobname.ERR.

FATAL - Writes the message with a "FATAL ERROR" heading and causes run termination immediately. Also writes the message to the errors file, Jobname.ERR.

UI - Writes the message with a "NOTE" heading and displays it in the message dialog box. This option is most useful in GUI mode.

Numeric or alphanumeric character values to be included in message. Values may be the results of parameter evaluations. All numeric values are assumed to be double precision. The FORTRAN nearest integer (NINT) function is used to form integers for the %I specifier.

Allows writing an output message via the ANSYS message subroutine. Also allows run termination control. This command is used only when contained in a prepared file read into the ANSYS program (i.e., *USE,/INPUT, etc.). A message format must immediately follow the *MSG command (on a separate line, without parentheses, as described below).

The message format may be up to 80 characters long, consisting of text strings and predefined "data descriptors" between the strings where numeric or alphanumeric character data are to be inserted. The descriptors are %I for integer data, %G for double precision data, %C for alphanumeric character data, and %/ for a line break. The corresponding FORTRAN data descriptors are I9, 1PG16.9 and A8, respectively. Each descriptor must be preceded by a blank. There must be one data descriptor for each specified value (8 maximum) in the order of the specified values.

Do not begin *MSG format lines with *IF, *ELSE, *ELSEIF, or *ENDIF. If the last non-blank character of the message format is an ampersand (&), a second line will also be read as a continuation of the format. Up to nine continuations (ten total lines) may be read. Consecutive blanks are condensed into one blank upon output, and a period is appended. Up to ten lines of output of 72 characters each may be produced (using the %/ descriptor). An example of the *MSG command and a format to print a message with two integer values and one real value is:

*MSG, INFO, 'Inner',25,1.2,148
Radius ( %C) = %I, Thick = %G, Length = %I

The output line is

Radius (Inner) = 25, Thick = 1.2, Length = 148.

Note that the /UIS,MSGPOP command controls which messages are displayed in the message dialog box when the GUI is active. All messages produced by the *MSG command are subject to the /UIS specification, with one exception, If Lab=UI, the message will be displayed in the dialog box regardless of the /UIS specification.

This command is valid in any processor.

This command cannot be accessed directly in the menu.

For elements that support multiple shapes, specifies the element shape to be used for meshing.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Key indicating the element shape to be used:

0 - Mesh with quadrilateral-shaped elements when Dimension=2D; mesh with hexahedral-shaped elements when Dimension=3D.

1 - Mesh with triangle-shaped elements when Dimension=2D; mesh with tetrahedral-shaped elements when Dimension=3D.

Specifies the dimension of the model to be meshed:

2D - 2-D model (area mesh).

3D - 3-D model (volume mesh).

Your action...	How it affects the mesh...
You issue the MSHAPE command with no arguments.	ANSYS uses quadrilateral-shaped or hexahedral-shaped elements to mesh the model, depending on whether you are meshing an area or a volume.
You do not specify an element shape, but you do specify the type of meshing to be used [MSHKEY].	ANSYS uses the default shape of the element to mesh the model. It uses the type of meshing that you specified.
You specify neither an element shape nor the type of meshing to be used.	ANSYS uses the default shape of the element to mesh the model. It uses whichever type of meshing is the default for that shape.

Notes

If no value is specified for Dimension, the value of KEY determines the element shape that will be used for both 2-D and 3-D meshing. In other words, if you specify MSHAPE,0, quadrilateral-shaped and hexahedral-shaped elements will be used. If you specify MSHAPE,1, triangle-shaped and tetrahedral-shaped elements will be used.

The MSHAPE, MSHKEY, and MSHMID commands replace the functionality that was provided by the ESHAPE command in ANSYS 5.3 and earlier releases.

Main Menu >Preprocessor >Mesher Opts

Main Menu >Preprocessor >Mesh >Mapped >4 to 6 sided

Specifies whether free meshing or mapped meshing should be used to mesh a model.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Key indicating the type of meshing to be used:

0 - Use free meshing (the default).

1 - Use mapped meshing.

2 - Use mapped meshing if possible; otherwise, use free meshing. If you specify MSHKEY,2, SmartSizing will be inactive even while free meshing non-map-meshable areas.

Notes

The MSHKEY, MSHAPE, and MSHMID commands replace the functionality that was provided by the ESHAPE command in ANSYS 5.3 and earlier releases.

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

Main Menu >Preprocessor >Mesh >Mapped >4 to 6 sided

Main Menu >Preprocessor >Mesh >Target Surf

Main Menu >Preprocessor >Mesher Opts

Specifies placement of midside nodes.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Key indicating placement of midside nodes:

0 - Midside nodes (if any) of elements on a region boundary follow the curvature of the boundary line or area (the default).

1 - Place midside nodes of all elements so that element edges are straight. Allows coarse mesh along curves.

2 - Do not create midside nodes (elements will have removed midside nodes).

The MSHMID, MSHAPE, and MSHKEY commands replace the functionality that was provided by the ESHAPE command in ANSYS 5.3 and earlier releases.

Main Menu >Preprocessor >Mesher Opts

Specifies pattern to be used for mapped triangle meshing.

PREP7:Meshing

	Mp Me St DY LP Th E3 E2 FL PP ED

Key indicating triangle pattern to be used (the figures below illustrate the pattern that will be used for each value of KEY):

0 - Let ANSYS choose the pattern (the default). ANSYS maximizes the minimum angle of the triangular-shaped elements that are created.

1 - Unidirectional split at node I.

2 - Unidirectional split at node J.

Notes

"Mapped triangle meshing" refers to the ANSYS program's ability to take a map-meshable area and mesh it with triangular elements, based on the value of MSHPATTERN,KEY. This type of meshing is particularly useful for analyses that involve the meshing of rigid contact elements.

The MSHPATTERN command is valid only when you have specified that ANSYS use triangle-shaped elements [MSHAPE,1,2D] (or you are meshing with an element that supports only triangles), and you have also specified mapped meshing [MSHKEY,1] to mesh an area.

For details about mapped meshing with triangles, see Chapter 7 of the ANSYS Modeling and Meshing Guide.

Main Menu >Preprocessor >Mesher Opts

Specifies the method of solution of the species transport equations.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Key defining the method of solution for the specified species number:

0 - No solution of equations for species SPNUM.

1 - Tri-Diagonal Matrix Algorithm (TDMA) (default).

2 - Conjugate residual method.

3 - Preconditioned conjugate residual method.

Notes

The TDMA (Tri-Diagonal Matrix Algorithm) method is a special version of the standard Gauss-Seidel iterative method for the solution of sets of algebraic equations. It is a good method for providing solutions for the momentum and turbulence equations since exact solutions are not required. The number of iterations (sweeps) to be performed is specified with the MSSOLU command. No convergence criterion is required for the TDMA method.

The other two methods are semi-direct solution methods based on search directions. They are conjugate direction iterative techniques which develop a solution as a linear combination of search directions. The conjugate residual method requires the least storage, but stalls when solving ill-conditioned problems. The preconditioned conjugate residual method is provided as an alternative to solve any of the ill-conditioned matrix problems that might arise in species transport. The number of search vectors and the convergence criterion are specified with the MSSOLU command. See the ANSYS CFD FLOTRAN Analysis Guide on the FLOTRAN Solvers for additional information.

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Specifies the initial value of nominal mass fraction for a species.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

The initial mass fraction of the entire problem domain for this species. Defaults to 0.0. The sum of the mass fractions for all species should equal 1.0.

This command is valid for the multiple species transport option in a FLOTRAN analysis and is required if the CMIX option has been activated for a property [FLDATA7,PROT,Label,CMIX].

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Defines the fluid properties of a species.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Label identifying the property being defined:

DENS - Density.

VISC - Viscosity.

COND - Thermal conductivity.

MDIF - Mass diffusion coefficient.

SPHT - Specific heat.

Type of property:

CONSTANT - Constant property (default). The property does not vary with temperature.

LIQUID - Liquid property. Density varies according to a second order polynomial relationship, and all other properties follow Sutherland's law for liquids.

GAS - Gas property. Density varies according to the ideal gas law, and all other properties follow Sutherland's law for gases.

Nominal value of the property being defined. For CONSTANT fluid types, the property remains at this value and does not vary. For GAS and LIQUID property types, this is the value of the property corresponding to the temperature defined by COF1.

Temperature corresponding to the NOMINAL value of the property (for GAS and LIQUID property types only; see Notes section). Not required for label=SPHT.

Second and third coefficients for temperature variation of the property. Not required for label=SPHT.

If the property type is CONSTANT, the equation used is as follows:

If the property type is LIQUID, a second order polynomial relationship is used for density, and Sutherland's law for liquids is used for the other properties:

where T is the temperature of the node where the property is being calculated.

If the property type is GAS, the ideal gas law is used for density, and Sutherland's law for gases is used for other properties:

where P and T are the pressure and temperature of the node where the property is being calculated.

Specific heat is always a CONSTANT. Also, property types (Type) such as TABLE, USER, POWL, BIN, etc. are not available for individual species. They are valid only for the bulk fluid.

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Specifies the quadrature order for multiple species elements.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Quadrature order for diffusion term integration:

0 - One-point quadrature (default).

1 - Same as 0, except a distributed value of temperature is used to evaluate temperature-dependent properties.

2 - Two-point quadrature (default for axisymmetric models).

Quadrature order for source term integration:

0 - One-point quadrature (default).

1 - Same as 0, except a distributed value of temperature is used to evaluate temperature-dependent properties.

2 - Two-point quadrature (default for axisymmetric models).

Notes

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Specifies relaxation factors for a multiple species transport analysis.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Species concentration relaxation factor. Defaults to 0.5.

Mass diffusion coefficient relaxation factor. Defaults to 0.5.

Effective mass diffusion coefficient relaxation factor (used for turbulent flow). Defaults to 0.5.

Inertial relaxation factor for solution of the transport equation. Defaults to 1.0x10⁺²⁰.

Notes

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Specifies solution options for multiple species transport.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Number of TDMA sweeps. Valid only for the TDMA (Tri-Diagonal Matrix Algorithm) method [MSMETH]. Defaults to 100.

Maximum number of iterations allowed for the semi-direct methods (conjugate residual and preconditioned conjugate residual methods, chosen with the MSMETH command). Defaults to 100.

Number of search vectors used for the semi-direct methods. Defaults to 2. New search vectors are made orthogonal to NSRCH previous vectors in the solution of the unsymmetric matrix systems.

Convergence criterion for the semi-direct methods. It represents the factor by which the inner product of the residual vector is reduced during the solution of the equations at any global iteration. Defaults to 1.0x10^-5. If the convergence criterion has not been achieved, the algebraic solver issues a warning message, and the execution of FLOTRAN continues normally.

Minimum normalized rate of change which will permit the semi-direct solution methods to continue. Used to terminate the semi-direct solvers in the event that stall occurs. Defaults to 1.0x10^-9. If the methods stall, the solver increments the solution only a very small amount despite the fact that the correct solution has been not been achieved (or perhaps even approached). The maximum nodal difference between the solutions, normalized to the value of the variable, is compared to DELMAX, and the solution is terminated if the value is less than DELMAX. Termination of the algebraic solver due to the small rate of change is considered a normal function, and no warning message is printed. Execution of FLOTRAN continues normally.

Notes

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Specifies the name, molecular weight, and Schmidt number of a species.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Name to be assigned to the species, up to 4 characters long. Defaults to SP01 for species 1, SP02 for species 2, ..., SP06 for species 6. This name can be used in place of the species number when specifying mass fraction boundary conditions and in postprocessing. (Note that the GUI always shows the default names, not the user-defined names.) Name should not be the same as an existing degree of freedom label.

Molecular weight for the species. Required only for gases (determined by the property type on MSPROP command). Defaults to 29.0.

Schmidt number (diffusion term divisor) for the species. Required only for gases (determined by the property type on MSPROP command). Defaults to 1.0.

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Controls the initial GUI components.

SESSION:RunControls

	Mp Me St DY LP Th E3 E2 FL PP ED

Label identifying the GUI component:

MAIN - Main menu, on by default.

INPUT - Input window, on by default.

GRPH - Graphics window, on by default.

TOOL - Toolbar, on by default.

ZOOM - Pan-Zoom-Rotate dialog box, off by default.

WORK - Offset Working Plane dialog box, off by default.

WPSET - Working Plane Settings dialog box, off by default.

ABBR - Edit Abbreviations dialog box, off by default.

PARM - Scalar Parameters dialog box, off by default.

SELE - Select Entities dialog box, off by default.

ANNO - Annotation dialog box, off by default.

HARD - Hard Copy dialog box, off by default.

HELP - ANSYS Help System, off by default.

Switch value:

OFF or 0 - Component does not appear when GUI is initialized.

ON or 1 - Component appears when GUI is initialized.

Notes

Controls which components appear when the Graphical User Interface (GUI) is initially brought up. This command is valid only before the GUI is brought up [/MENU,ON] and is intended to be used in the START5x.ANS file. It only affects how the GUI is initialized; you can always bring up or close any component once you are in the GUI.

This command is valid only at the Begin Level.

This command cannot be accessed directly in the menu.

Sets the convergence monitors for species.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Termination criteria for steady-state analysis. Defaults to 1x10^-8.

Termination criteria for transient analysis. Defaults to 1x10^-6.

Repeat command to set each species number as required.

All specified criteria must be met before the case is terminated.

If a termination criterion for a specific species number is set negative, the termination check is ignored for that particular species.

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Main Menu >Solution >FLOTRAN Set Up >Multiple Species

Allows species properties to vary between global iterations.

PREP7:FLOTRANMultipleSpecies

	Mp -- -- -- -- -- -- -- FL PP ED

Species number, from 1 to 6. Must be specified.

Label identifying the species property:

DENS - Density.

VISC - Viscosity.

COND - Thermal conductivity.

MDIF - Mass diffusion coefficient.

Key to allow property variation between global iterations:

OFF - Variation not allowed (default).

ON - Variation allowed.

Notes

This command is valid for the multiple species transport option in a FLOTRAN analysis.

Main Menu >Preprocessor >FLOTRAN Set Up >Multiple Species

Specifies the number of modes to expand and write for a modal or buckling analysis.

SOLUTION:DynamicOptions SOLUTION:NonlinearOptions

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

Number of modes to expand and write. If blank, expand and write all modes within the frequency range specified.

Beginning, or lower end, of frequency range of interest. If FREQB and FREQE are both blank, expand and write the number of modes specified without regard to the frequency range. Defaults to the entire range.

Ending, or upper end, of frequency range of interest.

Element calculation key:

NO - Do not calculate element results and reaction forces (default).

YES - Calculate element results and reaction forces, as well as the nodal degree of freedom solution..

Expand only those modes whose significance level exceeds the SIGNIF threshold. 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 expanded. The higher the SIGNIF threshold, the fewer the number of modes expanded. SIGNIF defaults to 0.001. If SIGNIF is specified as 0.0, it is taken as 0.0. SIGNIF value is only used for single-point or DDAM response (SPOPT,SPRS or DDAM) analyses.

Notes

Specifies the number of modes to expand and write over a frequency range for a modal (ANTYPE=MODAL) or buckling (ANTYPE=BUCKLE) analysis. For reduced analyses, an expansion is required. If used in SOLUTION, this command is valid only within the first load step.

This command is also valid in PREP7.

Main Menu >Preprocessor >Loads >ExpansionPass >Expand Modes

Main Menu >Preprocessor >Loads >Analysis Options

Main Menu >Solution >ExpansionPass >Expand Modes

Main Menu >Solution >Analysis Options