get#

ParameterDefinition.get(par='', entity='', entnum='', item1='', it1num='', item2='', it2num='', **kwargs)#

Retrieves a value and stores it as a scalar parameter or part of an array parameter.

Mechanical APDL Command: *GET

Parameters:
parstr

The name of the resulting parameter. See starset for name restrictions.

entitystr

Entity keyword. Valid keywords are NODE, ELEM, KP, LINE, AREA, VOLU, etc., as shown for Entity = in the tables below.

entnumstr

The number or label for the entity (as shown for ENTNUM = in the tables below). In some cases, a zero (or blank) ENTNUM represents all entities of the set.

item1str

The name of a particular item for the given entity. Valid items are as shown in the Item1 columns of the tables below.

it1numstr

The number (or label) for the specified Item1 (if any). Valid IT1NUM values are as shown in the IT1NUM columns of the tables below. Some Item1 labels do not require an IT1NUM value.

item2str

A second set of item labels and numbers to further qualify the item for which data are to be retrieved. Most items do not require this level of information.

it2numstr

A second set of item labels and numbers to further qualify the item for which data are to be retrieved. Most items do not require this level of information.

Notes

get retrieves a value for a specified item and stores the value as a scalar parameter, or as a value in a user-named array parameter. An item is identified by various keyword, label, and number combinations. Usage is similar to the starset command except that the parameter values are retrieved from previously input or calculated results.

Example: get Usage

get,A,ELEM,5,CENT,X returns the centroid x location of element 5 and stores the result as parameter A.

get command operations, and corresponding get functions, return values in the active coordinate system ( csys for input data or rsys for results data) unless stated otherwise.

A get function is an alternative in-line function that can be used instead of the get command to retrieve a value. For more information, see.

Both get and starvget retrieve information from the active data stored in memory. The database is often the source, and sometimes the information is retrieved from common memory blocks that the program uses to manipulate information. Although POST1 and POST26 operations use a *.rst file, get data is accessed from the database or from the common blocks. Get operations do not access the *.rst file directly. For repeated gets of sequential items, such as from a series of elements, see the starvget command.

Most items are stored in the database after they are calculated and are available anytime thereafter. Items are grouped according to where they are usually first defined or calculated. Preprocessing data will often not reflect the calculated values generated from section data. Do not use get to obtain data from elements that use calculated section data, such as beams or shells.

When the value retrieved by get is a component name, the resulting character parameter is limited to 32 characters. If the component name is longer than 32 characters, the remaining characters are ignored.

Most of the general items listed below are available from all modules. Each of the sections for accessing get parameters are shown in the following order:

The get command is valid in any processor.

General Items

*GET General Entity Items#

*GET General Items, Entity = ACTIVE#

Entity = ACTIVE, ENTNUM = 0 (or blank)#

get, Par, ACTIVE, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

INT

Current interactive key: 0=off, 2=on.

IMME

Current immediate key: 0=off, 1=on.

MENU

Current menu key: 0=off, 1=on.

PRKEY

Printout suppression status: 0= nopr, 1= gopr or slashgo

UNITS

Units specified by units command: 0 = USER, 1 = SI, 2 = CGS, 3 = BFT, 4 = BIN, 5 = MKS, 6 = MPA, 7 = uMKS.

ROUT

Current routine: 0 = Begin level, 17 = PREP7, 21 = SOLUTION, 31 = POST1, 36 = POST26, 52 = AUX2, 53 = AUX3, 62 = AUX12, 65 = AUX15.

TIME

WALL,CPU

Current wall clock or CPU time. Current wall clock will continue to accumulate during a run and is not reset to zero at midnight.

DBASE

LDATE

Date of first modification of any database quantity required for POST1 operation. The parameter returned is Par = YEAR*10000 + MONTH*100 + DAY.

DBASE

LTIME

Time of last modification of any database quantity required for POST1 operation. The parameter returned is Par = HOURS*10000 + MINUTES*100 + SECONDS.

REV

Minor release revision number (5.6, 5.7, 6.0 etc.). Letter notation (for example, 5.0A) is not included.

TITLE

0,1,2,3,4

Item2: START IT2NUM: N Current title string of the main title ( IT1NUM =0 or blank) or subtitle 1, 2, 3, or 4 ( IT1NUM =1,2,3, or 4). A character parameter of up to 8 characters, starting at position N, is returned.

JOBNAM

Item2: START IT2NUM: N Current Jobname. A character parameter of up to 8 characters, starting at position N, is returned. Use dim and *DO to get all 32 characters.

PLATFORM

The current platform.

NPROC

CURR, MAX, MAXP

The number of processors being used for the current session, or the maximum total number of processors (physical and virtual) available on the machine, or the maximum number of physical processors available on the machine. This only applies to shared-memory parallelism.

NUMCPU

Number of distributed processes being used (distributed-memory parallel solution).

*GET General Items, Entity = CMD#

Entity = CMD, ENTNUM = 0 (or blank) The following items are valid for all commands except star (2) commands and non-graphics slash (/) commands.#

get, Par, CMD, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

STAT

Status of previous command: 0=found, 1=not found (unknown).

NARGS

Field number of last nonblank field on the previous command.

FIELD

2,3… N

Numerical value of the N th field on the previous command. Field 1 is the command name (not available)

*GET General Items, Entity = COMP#

Entity = COMP, ENTNUM = 0 (or blank)#

get, Par, COMP, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

NCOMP

Total number of components and assemblies currently defined.

*GET General Items, Entity = GRAPH#

Entity =GRAPH, ENTNUM = N (window number)#

get, Par, GRAPH, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

ACTIVE

Windowing operations status: 0=off, 1=on.

ANGLE

angle THETA angle.

CONTOUR

Name

contour value for Name, where Name = VMIN, VINC, or NCONT.

DIST

dist DVAL value.

DSCALE

DMULT

slashdscale DMULT value.

EDGE

edge KEY value.

FOCUS

X, Y, Z

focus CIN, YF, or ZF value.

GLINE

gline STYLE value.

MODE

NumPy user guide or auto setting: 0=user, 1=auto.

NORMAL

normal KEY value.

RANGE

XMIN, XMAX, YMIN, YMAX

Windowing operations XMIN, XMAX, YMIN, or YMAX screen coordinates.

RATIO

X, Y

ratio RATOX or RATOY value.

SSCALE

SMULT

sscale SMULT value.

TYPE

slashtype Type value.

VCONE

ANGLE

vcone PHI angle.

VIEW

X, Y, Z

View XV, YV, or ZV value.

VSCALE

VRATIO

vscale VRATIO value.

*GET General Items, Entity = PARM#

Entity = PARM, ENTNUM = 0 (or blank)#

get, Par, PARM, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

MAX

Total number of parameters currently defined.

BASIC

Number of scalar parameters (excluding parameters beginning with an underscore _, array parameters, and character parameters).

LOC

Num

Name of the parameter at the Num location in the parameter table. A character parameter is returned.

*GET General Items, Entity = TBTYPE#

Entity = TBTYPE, ENTNUM = MatID (where TBTYPE is the material table type as defined via the tb command, such (ELASTIC, CTE, etc.), and MatID is the material ID) Evaluates a material property coefficient for a given set of input field variables.#

get, Par, TBTYPE, MatID, Item1, IT1NUM, Item2, IT2NUM, Fld1, Fld2,…

Item1

IT1NUM

Description

TBEV: Material table evaluation for query at a given field variable

SINDEX = Subtable index (1 - max number of subtables)

Item2 : CINDEX = Coefficient index

IT2NUM : N = Number of field variables input

Fld1, Fld2, …, : Val = Value of the field variable(s), entered in the same order specified via the tbfield command(s)

Preprocessing Items

*GET Preprocessing Entity Items#

*GET Preprocessing Items, Entity = ACTIVE#

Entity = ACTIVE, ENTNUM = 0 (or blank)#

get, Par, ACTIVE, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

SEG

Segment capability of graphics driver: 0=no segments available, 1=erasable segments available, 2=non-erasable segments available.

CSYS

Active coordinate system.

DSYS

Active display coordinate system.

MAT

Active material.

TYPE

Active element type.

REAL

Active real constant set.

ESYS

Active element coordinate system.

SECT

Active section.

CP

Maximum coupled node set number in the model (includes merged and deleted sets until compressed out).

CE

Maximum constraint equation set number in the model (includes merged and deleted sets until compressed out).

*GET Preprocessing items, Entity = AREA#

Entity = AREA, ENTNUM = N (area number)#

get, Par, AREA, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

ATTR

Name

Number assigned to the attribute, Name, where Name =MAT, TYPE, REAL, ESYS, KB,KE,SECN, NNOD, NELM, or ESIZ. (NNOD=number of nodes, NELM=number of elements, ESIZ=element size.)

ASEL

Select status of area N : -1=unselected, 0=undefined, 1=selected. Alternative get function: ASEL( N ).

NXTH

Next higher area number above N in selected set (or zero if none found).

NXTL

Next lower area number below N in selected set (or zero if none found).

AREA

Area of area N. ( asum or gsum must have been performed sometime previously with at least this area N selected).

LOOP

1,2,…, I

Item2 : LINE, IT2NUM : 1,2,…, p Line number of position p of loop I

*GET Preprocessing Items, Entity = AXIS#

Entity = AXIS, ENTNUM = 0 (or blank)#

get, Par, AXIS, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

Number of defined sections.

NUM

MAX

Largest section number defined.

*GET Preprocessing Items, Entity = CDSY#

Entity = CDSY, ENTNUM = N (coordinate system number)#

get, Par, CDSY, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

LOC

X, Y, Z

X, Y, or Z origin location in global Cartesian system.

ANG

XY, YZ, ZX

THXY, THYZ, or THZX rotation angle (in degrees) relative to the global Cartesian coordinate system.

ATTR

Name

Number assigned to Name, where Name =KCS, KTHET, KPHI, PAR1, or PAR2. The value -1.0 is returned for KCS if the coordinate system is undefined.

NUM

MAX

The maximum coordinate system number

*GET Preprocessing Items, Entity = CE#

Entity = CE, ENTNUM = N (constraint equation set)#

get, Par, CE, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

If N = 0, then

MAX

Maximum constraint equation number

NUM

Number of constraint equations

If N > 0, then

NTERM

Number of terms in this constraint equation

CONST

Constant term for this constraint equation

TERM

number

Item2 = NODE: Gives the node for this position in the constraint equation. Item2 = DOF: Gives the DOF number for this position in the constraint equation. (1-UX, 2-UY, 3-UZ, 4-ROTX, etc.) Item2 = COEF: Gives the coefficient for this position in the constraint equation.

*GET Preprocessing Items, Entity = CMPB#

Entity = CMPB, ENTNUM = N (composite beam section identification number)#

get, Par, CMPB, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

Number of defined sections. If Item1 = COUNT, then N is blank.

NUM

MAX

Largest section number defined. If IT1NUM = MAX, then N is blank.

EXIS

Returns a 1 if the section exists and if it is a CMPB section.

NAME

The 8-character section name defined via the sectype command.

One of the following: * CBMX * CBTE * CBMD

Item2 = NTEM (the number of temperatures for cbmx, cbte, or cbmd data).

One of the following: * CBMX * CBTE * CBMD

Item2 = TVAL; IT2NUM = nnn where nnn is the temperature value (< = NTEM).

One of the following: * CBMX * CBTE * CBMD

nnn

Item2 = TEMP; IT2NUM = tval Where nnn is the location in the cbmx, cbte, or cbmd command for the given coefficient number, and tval is the temperature value.

*GET Preprocessing Items, Entity = CP#

Entity = CP, ENTNUM = N (coupled node set)#

get, Par, CP, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

If N = 0, then

MAX

Maximum coupled set number

NUM

Number of coupled sets

If N > 0, then

DOF

The degree of freedom for this set (1-UX, 2-UY, 3-UZ, 4-ROTX, etc.)

NTERM

Number of nodes in this set.

TERM

number

Item2 = NODE: Gives the node for this position number in the coupled set.

*GET Preprocessing Items, Entity = CSEC#

Entity = CSEC, ENTNUM = 0 (or blank)#

get, Par, CSEC, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

Number of defined sections.

NUM

MAX

Largest section number defined.

*GET Preprocessing Items, Entity = ELEM#

Entity = ELEM, ENTNUM = N (element number)#

get, Par, ELEM, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

NODE

1, 2,… 20

Node number at position 1,2,… or 20 of element N. Alternative get function: NELEM( n,npos ), where npos is 1,2,…20.

CENT

X, Y, Z

Centroid X, Y, or Z location (based on shape function) in the active coordinate system. The original locations is used even if large deflections are active. Alternative get functions: CENTRX( N ), CENTRY( N ), and CENTRZ( N ) always retrieve the element centroid in global Cartesian coordinates, and are determined from the selected nodes on the elements.

ADJ

1, 2,… 6

Element number adjacent to face 1,2,…6. Alternative get function: ELADJ( N, face ). Only elements (of the same dimensionality) adjacent to lateral faces are considered.

ATTR

Name

Number assigned to the attribute Name, where Name = MAT, TYPE, REAL, ESYS, PSTAT, LIVE, or SECN. Returns a zero if the element is unselected. If Name = LIVE, returns a 1 if the element is selected and active, and a -1 if it is selected and inactive. Name = SECN returns the section number of the selected beam element.

LENG

Length of line element (straight line between ends).

LPROJ

X, Y, Z

Projected line element length (in the active coordinate system). X is x-projection onto y-z plane, Y is y projection onto z-x plane, and Z is z-projection onto x-y plane.

AREA

Area of area element.

APROJ

X, Y, Z

Projected area of area element area (in the active coordinate system). X is x-projection onto y-z plane, Y is y projection onto z-x plane, and Z is z-projection onto x-y plane.

VOLU

Element volume. Based on unit thickness for 2D plane elements (unless the thickness option is used) and on the full 360 degrees for 2D axisymmetric elements. For general axisymmetric elements SOLID272 and SOLID273, only the area of the element on the master plane is reported before solving, not the volume. After solving, the volume is reported. If results data are in the database, the volume returned is the volume calculated during solution.

ESEL

Select status of element N : -1 = unselected, 0 = undefined, 1 = selected. Alternative get function: ESEL( N ).

NXTH

Next higher element number above N in selected set (or zero if none found). Alternative get function: ELNEXT( N )

NXTL

Next lower element number below N in selected set (or zero if none found).

HGEN

Heat generation on selected element N.

DGEN

Diffusing substance generation on selected node N (returns 0.0 if node is unselected, or if the DOF is inactive).

HCOE

face

Heat coefficient for selected element N on specified face. Returns the value at the first node that forms the face.

TBULK

face

Bulk temperature for selected element N on specified face. Returns the value at the first node that forms the face.

PRES

face

Pressure on selected element, N on specified face. Returns the value at the first node that forms the face.

SHPAR

Test

Element shape test result for selected element N, where Test = ANGD, ASPE (aspect ratio), JACR (Jacobian ratio), MAXA (maximum corner angle), PARA (deviation from parallelism of opposite edges), or WARP (warping factor).

MEMBER

COUNT

Number of reinforcing members (individual reinforcings) in the element N.

EGID

COUNT

Number of non-duplicate global identifiers in the element N.

MIN, MAX

Lowest or highest global identifier in the element N.

*GET Preprocessing Items, Entity = ETYP#

Entity = ETYP, ENTNUM = N (element type number)#

get, Par, ETYP, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

ATTR

Name

Number assigned to the attribute Name, where Name =ENAM, KOP1, KOP2,…, KOP9, KO10, KO11, etc.

*GET Preprocessing Items, Entity = GCN#

Entity = GCN, ENTNUM = 0 (or blank)#

get, Par, GCN, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

MAT

Sect1

Item2 = 0 or blank; IT2NUM = Sect2. Material ID to be used for general contact between Sect1 and Sect2 . Alternative get function: SECTOMAT( Sect1, Sect2 ).

REAL

Sect1

Item2 = 0 or blank; IT2NUM = Sect2. Real constant ID to be used for general contact between Sect1 and Sect2 . Alternative get function: SECTOREAL( Sect1, Sect2 ).

DEF

Sect1

Item2 = 0 or blank; IT2NUM = Sect2. Number indicating the type of contact for the general contact definition between Sect1 and Sect2 : * = 0 - Excluded general contact between Sect1 / Sect2 * = 1 - Asymmetric general contact between Sect1 (contact) / Sect2 (target) * = 2 - Asymmetric general contact between Sect1 (target) / Sect2 (contact) * = 3 - Symmetric general contact between Sect1 / Sect2

Sect1 and Sect2 are section numbers associated with general contact surfaces.

*GET Preprocessing Items, Entity = GENB#

Entity = GENB, ENTNUM = N (nonlinear beam general section identification number)#

get, Par, GENB, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

(Blank)

Number of defined sections. If Item1 = COUNT, then N is blank.

NUM

MAX

Largest section number defined. If IT1NUM = MAX, then N is blank.

EXIS

(Blank)

Returns a 1 if the section exists and if it is a GENB section.

SUBTYPE

(Blank)

Section subtype for the section ID specified via the sectype command.

NAME

(Blank)

The 8-character section name defined via the sectype command.

One of the following: * BSAX * BSM1 * BSM2 * BSTQ * BSS1 * BSS2 * BSMD * BSTE

(Blank)

Item2 = NTEM, the number of temperatures for bsax, bsm1, bsm2, bstq, bss1, bss2, bsmd, or bste data.

One of the following: * BSAX * BSM1 * BSM2 * BSTQ * BSS1 * BSS2 * BSMD * BSTE

(Blank)

Item2 = TVAL; IT2NUM = nnn Where nnn is the temperature value (<= NTEM).

One of the following: * BSAX * BSM1 * BSM2 * BSTQ * BSS1 * BSS2 * BSMD * BSTE

nnn

Item2 = TEMP; IT2NUM = tval Where nnn is the location in the bsax, bsm1, bsm2, bstq, bss1, bss2, bsmd, or bste command for the given coefficient number, and tval is the temperature value. Examples for nnn : * nnn = 1 for STRAIN(1) * nnn = 2 for STRESS(1) * nnn = 3 for STRAIN(2) * nnn = 4 for STRESS(2) * nnn = 5 for STRAIN(3) *

One of the following: * BSAX * BSM1 * BSM2 * BSTQ * BSS1 * BSS2 * BSMD * BSTE

(Blank)

Item2 = TEMP; IT2NUM = tval ; Item3 = NCONST The number of constants at tval.

*GET Preprocessing Items, Entity = GENS#

Entity = GENS, ENTNUM = N (preintegrated shell general section identification number)#

get, Par, GENS, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

(Blank)

Number of defined sections. If Item1 = COUNT, then N is blank.

NUM

MAX

Largest section number defined. If IT1NUM = MAX, then N is blank.

EXIS

(Blank)

Returns a 1 if the section exists and if it is a GENS section.

NAME

(Blank)

The 8-character section name defined via the sectype command.

One of the following: * SSPA * SSPB * SSPD * SSPE * SSMT * SSBT * SSPM

(Blank)

Item2 = NTEM, the number of temperatures for sspa, sspb, sspd, sspe, ssmt, ssbt, or sspm data.

One of the following: * SSPA * SSPB * SSPD * SSPE * SSMT * SSBT * SSPM

(Blank)

Item2 = TVAL; IT2NUM = nnn Where nnn is the temperature value (<= NTEM).

One of the following: * SSPA * SSPB * SSPD * SSPE * SSMT * SSBT * SSPM

nnn

Item2 = TEMP; IT2NUM = tval Where nnn is the location in the sspa, sspb, sspd, sspe, ssmt, ssbt, or sspm command for the given coefficient number, and tval is the temperature value.

*GET Preprocessing Items, Entity = KP#

Entity = KP, ENTNUM = N (keypoint number)#

get, Par, KP, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

LOC

X, Y, Z

X, Y, or Z location in the active coordinate system. Alternative get functions: KX( N ), KY( N ), KZ( N ). Inverse get function: KP( x,y,z ) returns the number of the selected keypoint nearest the x,y,z location (in the active coordinate system, lowest number for coincident keypoints).

ATTR

Name

Number assigned to the attribute Name, where Name = MAT, TYPE, REAL, ESYS, NODE, or ELEM.

KSEL

Select status of keypoint N : -1 = unselected, 0 = undefined, 1 = selected. Alternative get function: KSEL( N ).

NXTH

Next higher keypoint number above N in selected set (or zero if none found). Alternative get function: KPNEXT( N ).

NXTL

Next lower keypoint number below N in selected set (or zero if none found).

DIV

Divisions (element size setting) from kesize command.

*GET Preprocessing Items, Entity = LINE#

Entity = LINE, ENTNUM = N (line number)#

get, Par, LINE, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

KP

1,2

Keypoint number at position 1 or 2.

ATTR

Name

Number assigned to the attribute, Name, where Name =MAT, TYPE, REAL, ESYS, NNOD, NELM, NDIV, NDNX, SPAC, SPNX, KYND, KYSP, LAY1, or LAY2. (NNOD=number of nodes, returns –1 for meshed line with no internal nodes, NELM=number of elements, NDIV=number of divisions in an existing mesh, NDNX=number of divisions assigned for next mesh, SPAC=spacing ratio in an existing mesh, SPNX=spacing ratio for next mesh, KYND=soft key for NDNX, KYSP=soft key for SPNX, LAY1=LAYER1 setting, LAY2=LAYER2 setting.)

LSEL

Select status of line N : -1=unselected, 0=undefined, 1=selected. Alternative get function: LSEL( N ).

NXTH

Next higher line number above N in the selected set (or zero if none found). Alternative get function: LSNEXT( N )

NXTL

Next lower line number below N in selected set (or zero if none found).

LENG

Length. A get function LX( n,lfrac ) also exists to return the X coordinate location of line N at the length fraction lfrac (0.0 to 1.0). Similar LY and LZ functions exist.

*GET Preprocessing Items, Entity = MAT#

Entity = MAT, ENTNUM = 0 (or blank)#

get, Par, MAT, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

Number of materials.

NUM

MAX

Largest material number for which at least one property is defined.

*GET Preprocessing Items, Entity = MPLAB#

Entity = MPlab, ENTNUM = N ( MPlab = material property label from mp command; N = material number.)#

get, Par, MPlab, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

TEMP

val

Material property value at temperature of val . For temperature dependent materials, the program interpolates the property at temperature input for val.

*GET Preprocessing Items, Entity = NODE#

Entity = NODE, ENTNUM = N (node number)#

get, Par, NODE, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

LOC

X, Y, Z

X, Y, Z location in the active coordinate system. Alternative get functions: NX( N ), NY( N ), NZ( N ). Inverse get function. NODE( x,y,z ) returns the number of the selected node nearest the x,y,z location (in the active coordinate system, lowest number for coincident nodes).

ANG

XY, YZ, ZX

THXY, THYZ, THZX rotation angle.

NSEL

Select status of node N : -1=unselected, 0=undefined, 1=selected. Alternative get function: NSEL( N ).

NXTH

Next higher node number above N in selected set (or zero if none found). Alternative get function: NDNEXT( N ).

NXTL

Next lower node number below N in selected set (or zero if none found).

F

FX, MX,…

Applied force at selected node N in direction IT1NUM (returns 0.0 if no force is defined, if node is unselected, or if the DOF is inactive). If ITEM2 is IMAG, return the imaginary part.

D

UX, ROTX,…

Applied constraint force at selected node N in direction IT1NUM (returns a large number, such as 2e100, if no constraint is specified, if the node is unselected, or if the DOF is inactive). If ITEM2 is IMAG, return the imaginary part.

HGEN

Heat generation on selected node N (returns 0.0 if node is unselected, or if the DOF is inactive).

NTEMP

Temperature on selected node N (returns 0.0 if node is unselected)

CPS

Lab

Couple set number with direction Lab = any active DOF, which contains the node N.

DGEN

Diffusing substance generation on selected node N (returns 0.0 if node is unselected, or if the DOF is inactive).

*GET Preprocessing Items, Entity = OCEAN#

Entity = OCEAN, ENTNUM = Type (where Type is a valid label on the DataType field of the octype command)#

get, Par, OCEAN, Type, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

NAME

Name defined for a given Type

DATA

1

Depth when Type = BASI

2

Material ID when Type = BASI

8

KFLOOD when Type = BASI

9

Cay when Type = BASI

10

Cb when Type = BASI

11

Zmsl when Type = BASI

13

Caz when Type = BASI

14

Ktable when Type = BASI

1

KWAVE when Type = WAVE

2

THETA when Type = WAVE

3

WAVELOC when Type = WAVE

4

KCRC when Type = WAVE

5

KMF when Type = WAVE

6

PRKEY when Type = WAVE

PROP

NROW

Number of rows defined by octable command

TABL

i

Data in table defined by octable command i = row number; Item2 = column number

This command contains some tables and extra information which can be inspected in the original documentation pointed above.

*GET Preprocessing Items, Entity = OCZONE#

Entity = OCZONE, ENTNUM = Name (where Name is a valid label on the ZoneName field of the oczone command)#

get, Par, OCZONE, Name, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

DATA

8

KFLOOD for a given ENTNUM = Name

9

Cay for a given ENTNUM = Name

10

Cb for a given ENTNUM = Name

13

Caz for a given ENTNUM = Name

PROP

NROW

Number of rows defined by octable command

TABL

i

Data in table defined by octable command i = row number; Item2 = column number

TYPE

Ocean zone type (returns 1, 2 or 3 for ZLOC-, COMP-, or PIP-type zones, respectively)

COMP

Component name when the given ocean zone type is COMP, or internal component name when the given ocean zone type is PIP

COMP2

External component name when the type of given ocean zone is PIP

This command contains some tables and extra information which can be inspected in the original documentation pointed above.

This command contains some tables and extra information which can be inspected in the original documentation pointed above.

*GET Preprocessing Items, Entity = PIPE#

Entity = PIPE, ENTNUM = 0 (or blank)#

get, Par, PIPE, NUM, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

Number of defined sections

NUM

MAX

Largest section number defined

*GET Preprocessing Items, Entity = PART#

Entity = PART, ENTNUM = N (PART number)#

get, Par, PART, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

TYPE

Element type number assigned to PART N.

MAT

Material number assigned to PART N.

REAL

Real constant number assigned to PART N.

*GET Preprocessing Items, Entity = RCON#

Entity = rcon, ENTNUM = N (real constant set number)#

get, Par, RCON, N, Item1, IT1NUM, Item2, IT2NUM

CONST

1, 2,…, m

Value of real constant number m in set N.

get

[*GET ,Par, RCON,0, Item1, IT1NUM, Item2, IT2NUM]

NUM

MAX

The maximum real constant set number defined

*GET Preprocessing Items, Entity = REIN#

Entity = REIN, ENTNUM = N (reinforcing section identification number)#

get, Par, REIN, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

TYPE

Section type, for ID – sectype command (always REIN for reinforcing sections).

SUBTYPE

Section subtype for ID – sectype command.

NAME

Name defined for a given ID number.

NREIN

Number of reinforcing fibers. For reinforcing sections generated ( ereinf ) via the standard method, the number of fibers defined via secdata. For reinforcing sections generated ( ereinf ) via the mesh-independent method, the total number of fibers in the section.

TABL

ReinfNum,I

Reinforcing fiber data, as defined via secdata. This item is not allowed for reinforcing sections generated ( ereinf ) via the mesh-independent method.

*GET Preprocessing Items, Entity = SCTN#

Entity = SCTN, ENTNUM = N (pretension section ID number)#

get, Par, SCTN, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

1

Section ID number.

2

Section type (always 5 for pretension section).

3

Pretension node number.

4

Coordinate system number.

Section normal NX.

5

Coordinate system number.

Section normal NY.

6

Coordinate system number.

Section normal NZ.

7 or 8

Eight character section name.

9

Initial action key. Returns 0 or 1 for lock, 2 for “free-to-slide,” or 3 for tiny.

10

Force displacement key. Returns 0 or 1 for force, or 2 for displacement.

11

First preload value.

12

Load step in which first preload value is to be applied.

13

Load step in which first preload value is to be locked.

14…

14 through 17 is a repeat of 10 through 13, but for the second preload value; 18 through 21 is for the third preload value; and so forth.

*GET Preprocessing Items, Entity = SECP#

Entity = SECP, ENTNUM = 0 (or blank)#

get, Par, SECP, NUM, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

COUNT

Number of defined sections

NUM

MAX

Largest section number defined

*GET Preprocessing Items, Entity = SHEL#

Entity = SHEL, ENTNUM = N (shell section identification number)#

get, Par, SHEL, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

TYPE

Section type, for id – sectype command. (always SHEL for shell sections)

NAME

Name defined for a given id number.

PROP

TTHK

Total thickness.

NLAY

Number of layers.

NSP

Number of section integration points.

POS

Node position (as defined by secoffset ).

0 = User Defined.

1 = Middle.

2 = Top.

3 = Bottom.

OFFZ

User-defined section offset (POS = 0).

TS11

Transverse shear stiffness factors.

TS22

Transverse shear stiffness factors.

TS12

Transverse shear stiffness factors.

HORC

Homogeneous or complete section flag.

0 = Homogeneous.

1 = Composite.

FUNC

Tabular function name for total thickness.

UT11

User transverse shear stiffness 11.

UT22

User transverse shear stiffness 22.

UT12

User transverse shear stiffness 12.

AMAS

Added mass.

MSCF

Hourglass control membrane scale factor.

BSCF

Hourglass control bending scale factor.

DSTF

Drill stiffness scale factor.

LDEN

Laminate density.

FKCN

KCN field value from the secfunction command, in which the array or table is interpreted.

ABD

Section membrane and bending stiffness matrix. Valid ITEM2 = 1,6 and IT2NUM = 1,6.

E

Section transverse shear stiffness matrix. Valid ITEM2 = 1,2 and IT2NUM = 1,2.

LAYD

LayerNumber,THIC

Layer thickness.

LayerNumber,MAT

Layer material.

LayerNumber,ANGL

Layer orientation angle.

LayerNumber,NINT

Number of layer integration points.

*GET Preprocessing Items, Entity = TBFT#

Entity = TBFT, ENTNUM = blank#

get, Par, TBFT, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

nmat

Number of defined material models.

matnum

index

Material number in array (index varies for 1 to num materials).

Entity = TBFT, ENTNUM = matid (For getting names of constitutive function, matid = the material ID number)

get

[*GET ,Par, TBFT,matid,nfun,IT1NUM,Item2,IT2NUM]

Item1

IT1NUM

Description

nfun

Number of constitutive functions for this material.

Entity = TBFT, ENTNUM = matid (To query constitutive function data, matid = the material ID number)

get

[*GET ,Par, TBFT,matid,func,fname,Item2,IT2NUM]

Item1

IT1NUM

Description

func

index

If Item2 = fname, the name of the constitutive function is returned.

func

function name

If Item2 = ncon, the number of constants is returned for the function specified in IT1NUM by the constitutive function name.

If Item2 = cons, set Item2num to index to return the value of the constant.

If Item2 = fixe, set Item2num to index to return the fix flag status.

If Item2 = RESI, returns the residual error while fitting the data.

If Item2 = type, returns the category of the constitutive model (moon, poly, etc.)

If Item2 = sord, returns the shear order of the prony visco model.

If Item2 = bord, returns the bulk order of the prony visco model.

If Item2 = shif, returns the shift function name of the prony visco model.

Entity = TBFT, ENTNUM = matid (For getting names of experimental data, matid = the material ID number)

get

[*GET ,Par, TBFT,matid,nexp,IT1NUM,Item2,IT2NUM]

Item1

IT1NUM

Description

nexp

Number of experiments for this material.

Entity = TBFT, ENTNUM = matid (To query experimental data, matid = the material ID number))

get

[*GET ,Par, TBFT,matid,func,fname,Item2,IT2NUM]

Item1

IT1NUM

Description

expindex

If Item2 = type, returns experiments type string.

If Item2 = numrow, returns number of rows in the data.

If Item2 = numcol, returns the number of cols in a row (set Intem2num = Row index)

If Item2 = data, returns the value of the data in row, col of exp expindex (set item2Num = row index and item3 = column index. All indices vary from 1 to the maximum value.

If Item2 = natt, returns the number of attributes.

If Item2 = attname, returns the attribute name (set Item2Num = Attr index).

If Item2 = attvald, returns double value of attribute (set Item2Num = Attr index).

If Item2 = attvali, returns integer valud of attribute (set Item2Num = Attr index).

If Item2 = attvals, returns the string value of the attribute (set Item2Num = Attr index).

*GET Preprocessing Items, Entity = TBLAB#

Entity = TBLAB, ENTNUM = N..( TBlab = data table label from the tb command; N = material number.)#

get, Par, TBlab, N, Item1, IT1NUM, Item2, IT2NUM, TBOPT

Item1

IT1NUM

Description

TEMP

T

Item2 : CONST IT2NUM : Num Value of constant number Num in the data table at temperature T. For constants, input an X,Y point; the constant numbers are consecutive with the X constants being the odd numbers, beginning with one.

To get all necessary output for materials defined via the tb command, you must specify the final argument TBOPT as indicated in the syntax description above.

*GET Preprocessing Items, Entity = VOLU#

Entity = VOLU, ENTNUM = N (volume number)#

get, Par, VOLU, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

ATTR

Name

Number assigned to the attribute Name, where Name =MAT, TYPE, REAL, ESYS, NNOD, or NELM. (NNOD=number of nodes, NELM=number of elements.)

VSEL

Select status of volume N : -1=unselected, 0=undefined, 1=selected. Alternative get function: VSEL( N ).

NXTH

Next higher volume number above N in selected set (or zero if none found). Alternative get function: VLNEXT( N ).

NXTL

Next lower volume number below N in selected set (or zero if none found).

VOLU

Volume of volume N. ( vsum or gsum must have been performed sometime previously with at least this volume N selected).

SHELL

1, 2,…, m

Item2 : AREA IT2NUM : 1,2,…, p Line number of position p of shell m

Solution Items

*GET Solution Entity Items#

*GET Solution Items, Entity = ACTIVE#

Entity = ACTIVE, ENTNUM = 0 (or blank)#

get, Par, ACTIVE, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

ANTY

Current analysis type.

SOLU

DTIME

Time step size.

NCMLS

Cumulative number of load steps.

NCMSS

Number of substeps. NOTE: Used only for static and transient analyses.

EQIT

Number of equilibrium iterations.

NCMIT

Cumulative number of iterations.

CNVG

Convergence indicator: 0=not converged, 1=converged.

MXDVL

Maximum degree of freedom value.

RESFRQ

Response frequency for 2nd order systems.

RESEIG

Response eigenvalue for 1st order systems.

DSPRM

Descent parameter.

FOCV

Force convergence value.

MOCV

Moment convergence value.

HFCV

Heat flow convergence value.

MFCV

Magnetic flux convergence value.

CSCV

Current segment convergence value.

CUCV

Current convergence value.

FFCV

Fluid flow convergence value.

DICV

Displacement convergence value.

ROCV

Rotation convergence value.

TECV

Temperature convergence value.

VMCV

Vector magnetic potential convergence value.

SMCV

Scalar magnetic potential convergence value.

VOCV

Voltage convergence value.

PRCV

Pressure convergence value.

VECV

Velocity convergence value.

CRPRAT

Maximum creep ratio.

PSINC

Maximum plastic strain increment.

CGITER

Number of iterations in the PCG and symmetric JCG (non-complex version) solvers.

*GET Solution Items, Entity = ELEM#

Entity = ELEM, ENTNUM = 0 (or blank)#

get, Par, ELEM, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

MTOT

X, Y, Z

Total mass components.

MC

X, Y, Z

Center of mass components.

IOR

X, Y, Z, XY, YZ, ZX

Moment of inertia about origin.

IMC

X, Y, Z, XY, YZ, ZX

Moment of inertia about the center of mass.

IPRIN

X, Y, Z

Principal moments of inertia.

IANG

XY, YZ, ZX

Angles of the moments of inertia principal axes.

FMC

X, Y, Z

Force components at mass centroid ( 1).

MMOR

X, Y, Z

Moment components at origin ( 1).

MMMC

X, Y, Z

Moment components at mass centroid ( 1).

Items ( 1) are available only after inertia relief solution ( irlf,1) or pre-calculation of masses ( irlf,-1).

Item values are consistent with the mass summary printed in the output file. They are based on

unscaled mass properties (see mascale command).

*GET Solution Items, Entity = MODE#

Entity = MODE, ENTNUM = N (mode number)#

get, Par, MODE, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

FREQ

Frequency of mode N. Returned values are valid for modal analyses which calculate real eigensolutions.

STAB

Stability value of mode N. Returned values are valid for modal analyses which calculate complex eigensolutions. The stability value is the real part of the complex eigenvalue. It contains information on the mode damping in a damped modal analysis.

DFRQ

Damped frequency of mode N. Returned values are valid for modal analyses which calculate complex eigensolutions. The damped frequency is the imaginary part of the complex eigenvalue.

PFACT

Participation factor of mode N. * If retrieved after a modal analysis, the real part of the participation factor is returned unless IT1NUM = IMAG. The direction is specified using Item2 = DIREC and IT2NUM = X, Y, Z, ROTX, ROTY, or ROTZ * If retrieved after a spectrum analysis, the spectrum number M is specified using Item2 = SPECT and IT2NUM = M. For a PSD analysis with spatial correlation or wave excitation, the retrieved participation factors will correspond to the first degree of freedom that is excited.

EFFM

Effective mass of mode N. Returned values are valid only after a modal analysis with effective mass calculation has been solved. The direction is specified using Item2 = DIREC and IT2NUM = X, Y, Z, ROTX, ROTY, or ROTZ.

GENM

Generalized mass (also called modal mass) of mode N. Returned values are valid only after a modal analysis with generalized mass calculation has been solved.

MCOEF

Mode coefficient of mode N. Returned values are valid only after a spectrum analysis has been solved. The spectrum number M is specified using Item2 = SPECT and IT2NUM = M. In a SPRS analysis, the values returned are based on the curve with the lowest damping. After a PSD analysis, the diagonal of the dynamic modal covariance matrix is retrieved for the displacement solution.

DAMP

Damping ratio of mode N. If retrieved after a modal analysis that creates complex solutions (DAMP, QRDAMP, or UNSYM eigensolvers) returned value is calculated from the complex frequencies. If retrieved after a spectrum analysis, returned value is the effective damping ratio. Not a function of direction. Also retrievable following a harmonic analysis or transient analysis with mode-superposition.

For all items except PFACT and MCOEF (as noted above), only the first 10000 values corresponding to significant modes will be returned.

The MODE file must be available to retrieve items PFACT and MCOEF with specified Item2. If Item2 is not specified, the last calculated value will be returned.

All values retrieved correspond to the first load step values. For a Campbell diagram analysis (multistep modal), get with Entity = CAMP must be used.

*GET Solution Items, Entity = DDAM#

Entity = DDAM, ENTNUM = N (mode number)#

get, Par,DDAM, N, Item1, IT1NUM

Item1

IT1NUM

Description

DSHOCK

Shock design value of mode N.

If multiple DDAM analyses are performed, the last calculated value will be returned.

Postprocessing Items

*GET Postprocessing Entity Items#

*GET Postprocessing Items, Entity = ACTIVE#

Entity = ACTIVE, ENTNUM = 0 (or blank)#

get, Par, ACTIVE, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

SET

LSTP

Current load step number.

SBST

Current substep number.

TIME

Time associated with current results in the database.

FREQ

Frequency (for ANTYPE=MODAL, HARMIC, SPECTR; load factor for ANTYPE=BUCKLE).

NSET

If Item2 is blank, number of data sets on result file. * If Item2 = FIRST, IT2NUM = Loadstep, get set number of first substep of loadstep * If Item2 = LAST, IT2NUM = Loadstep, get set number of last substep of loadstep

RSYS

Active results coordinate system.

*GET Postprocessing Items, Entity = ACUS#

Entity = ACUS, ENTNUM = 0 (or blank)#

get, Par, ACUS, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

PWL

Radiated sound power level

PRES

Far-field pressure at a given point

PHASE

Far-field pressure phase at a given point

SPL

Far-field sound pressure level at a given point

SPLA

Far-field a-weighted sound pressure level at a given point

DG

Far-field directivity at a given point

PS

Far-field scattered pressure at a given point

TS

Far-field target strength at a given point

DFIN

Diffuse sound field incident power

SIMP

Magnitude of specific acoustic impedance on the selected surface

AIMP

Magnitude of acoustic impedance on the selected surface

MIMP

Magnitude of mechanical impedance on the selected surface

APRES

Magnitude of average pressure on the selected surface

FORC

Magnitude of average force on the selected surface

POWER

Acoustic power through the selected surface

BSPL

SPL over frequency band

BSPA

A-weighted SPL over frequency band

PWRF

Reference sound power

TL

Transmission loss

RL

Return loss

Item1 = PWL, PRES, SPL, SPLA, PHASE, DG, PS, and TS are available after issuing the prfar or plfar command. The maximum values are obtained from the current command. Item1 = SIMP, AIMP, MIMP, APRES, FORC, POWER, TL, and RL are available after issuing the corresponding pras command at the current frequency. The values are obtained at the current frequency, or at the last frequency for multiple load step and substep cases. Item1 = DFIN is available after the diffuse sound field solution.

*GET Postprocessing Items, Entity = CAMP#

Available after plcamp or prcamp command is issued. Entity = CAMP, ENTNUM = N (mode number)#

get, Par, CAMP, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

NBMO

Number of modes in the Campbell diagram ( ENTNUM not required). This value is the maximum value for N.

NBST

Number of steps in the Campbell diagram: modal load steps with rotational velocity ( ENTNUM not required). This value is the maximum value for M (see Item1 = FREQ).

WHRL

M

Whirl of mode N at step M : -1 is backward whirl, 1 is forward whirl, and 0 is undetermined. For default IT1NUM, it corresponds to the whirl at the maximum rotational velocity.

VCRI

Critical speed for mode N. This value is available if an excitation is defined via the plcamp or prcamp command’s SLOPE argument. (The unit of speed depends upon the UNIT value specified in those commands.) N does not correspond to the mode number if FREQB ( prcamp or plcamp command) is used. Instead, it represents the Nth mode number listed in the output of prcamp or plcamp.

FREQ

M

Natural frequency of mode (Hz) N at step M. It represents the complex part of the eigenvalue.

STAB

M

Stability value (Hz) of mode N at step M. It represents the real part of the eigenvalue.

UKEY

M

Instability key for mode N at step M : 0 is stable and 1 is unstable. For default IT1NUM, it corresponds to the stability over the whole rotational velocity range.

VSTA

Stability limit for mode N. This value is available when SLOPE is zero on the plcamp or prcamp command. (The unit of speed depends upon the UNIT value specified in those commands.) N does not correspond to the mode number if FREQB ( prcamp or plcamp command) is used. Instead, it represents the Nth mode number listed in the output of prcamp or plcamp.

If the sorting is activated (Option= ON on the prcamp and plcamp commands), all the parameters retrieved are in the sorted order.

*GET Postprocessing Items, Entity = CINT#

Entity = CINT, ENTNUM = CrackId (required Crack ID number)#

get, Par, CINT, CrackId, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

CTIP

ctnum

IT1NUM = Crack tip node number (required) Item2 = CONTOUR IT2NUM = Contour number (default 1) Returns JINT value if crack ID is JINT type; otherwise, returns 0. Item1 defaults to CTIP, Item2 defaults to CONTOUR.

Entity= CINT, ENTNUM = CrackID (required Crack ID number)

*GET , Par, CINT, CrackId, Item1, IT1NUM, Item2, IT2NUM, Item3, IT3NUM, Item4, IT4NUM

Item1

IT1NUM

Description

CTIP

ctnum

IT1NUM = Crack tip node number (required) Item2 = CONTOUR IT2NUM = Contour number (default 1) Item3 = DTYPE IT3NUM = Data type (JINT, IIN1, IIN2, IIN3, K1, K2, K3, G1, G2, G3, GT, MFTX, MFTY, MFTZ, TSTRESS, CEXT, STTMAX, PSMAX, CSTAR, DLTA, DLTN, DLTK, R, UFAC, CRDX, CRDY, CRDZ, and APOS) FOR IT3NUM = STTMAX or PSMAX: * Item4 = AINDEX (angle index) * IT4NUM = Index value (1 to N+1; N = Maximum number of intervals for the sweep ( cint,RSWEEP). Returns specified data type value. FOR IT3NUM = DLTA, DLTN, DLTK, R, UFAC, CRDX, CRDY, CRDZ, APOS: * Set IT2NUM = 1 Returns specified data type value. Item1 defaults to CTIP, Item2 defaults to CONTOUR, Item3 defaults to DTYPE. DLTK in a 3D XFEM-based fatigue crack-growth analysis is evaluated based on the smoothed SIFS values. The actual DLTK value can be easily calculated by issuing get for SIFS values and the stress (load) ratio.

Entity= CINT, ENTNUM = CrackID (required Crack ID number)

*GET , Par, CINT, CrackId, Item1, IT1NUM, Item2, IT2NUM ,

Item1

IT1NUM

Description

NNOD

Maximum number of nodes along the crack front.

Entity= CINT, ENTNUM = CrackID (required Crack ID number)

*GET , Par, CINT, CrackId, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

NODE

ipos

IT1NUM = Position along the crack front (from 1 to NNOD). Default = 1. Returns node number at the given position along the crack front. (For XFEM, an internal node number is returned.)

*GET Postprocessing Items, Entity = CYCCALC#

Entity = CYCCALC, ENTNUM = cycspec specification number Generate date for cyclic results using cyccalc before retrieving those items.#

get, Par,CYCCALC, spec, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Item2

IT2NUM

Description

FREQ

frequency point

SECTOR

sector

cycspec result at the IT1NUM frequency and IT2NUM sector

SECMAX

cycspec maximum result at the IT1NUM frequency

SECNUM

cycspec sector with the maximum result at the IT1NUM frequency

SECNODE

cycspec node in the sector with the maximum result at the IT1NUM frequency

The frequency point refers to the harmonic solution data set number (NSET on the Set displays command)

*GET Postprocessing Items, Entity = ELEM#

Entity = elem, ENTNUM = N (element number)#

get, Par, ELEM, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

SERR Some element- and material-type limitations apply. For more information, see the documentation for the prerr command.

Structural error energy.

SDSG

Absolute value of the maximum variation of any nodal stress component.

TERR

Thermal error energy.

TDSG

Absolute value of the maximum variation of any nodal thermal gradient component.

SENE

“Stiffness” energy or thermal heat dissipation. Same as TENE.

TENE

Thermal heat dissipation or “stiffness” energy. Same as SENE.

KENE

Kinetic energy.

ASENE

Amplitude “stiffness” energy.

PSENE

Peak “stiffness” energy.

AKENE

Amplitude kinetic energy.

PKENE

Peak kinetic energy.

DENE

Damping energy.

WEXT WEXT is calculated for element-based loading only (and not for nodal-force loading). WEXT is stored on elements to which loading has been applied; if surface elements are added on top of other elements, for example, and pressure loading is applied to the surface elements, WEXT is available for the surface elements only.

Work due to external load.

JHEAT

Element Joule heat generation (coupled-field calculation).

JS

X, Y, Z

Source current density (coupled-field calculation) in the global Cartesian coordinate system.

HS

X, Y, Z

Average element magnetic field intensity from current sources.

VOLU

Element volume, as calculated during solution.

ETAB

Lab

Value of element table item Lab for element N (see etable command).

EFOR

Nnum

Element force at node Nnum. The force label is specified using Item2 = FX, FY, FZ, MX, MY, MZ, or HEAT. In a dynamics analysis, the element forces returned are based on the type of force requested. It is specified using the force command for all dynamics analyses, except for spectrum analyses where ForceType is used on the combination commands ( srss, psdcom, etc.).

SMISC

Snum

Value of element summable miscellaneous data at sequence number Snum (as used on etable command).

NMISC

Snum

Value of element non-summable miscellaneous data at sequence number Snum (as used on etable command).

FSOU

Element fluid flow source loading (poromechanics).

*GET Postprocessing Items, Entity = ETAB#

Entity = ETAB, ENTNUM = N (column number)#

get, Par, ETAB, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

LAB

Label for column N of the element table ( etable ). Returns a character parameter.

ELEM

E

Value in etable column N for element number E.

*GET Postprocessing Items, Entity = FSUM#

Entity = fsum, ENTNUM = 0 (or blank)#

get, Par, FSUM, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

ITEM

Lab

Value of item Lab from last fsum command. Valid labels are FX, FY, FZ, MX, MY, MZ, FLOW, HEAT, FLUX, etc.

*GET Postprocessing Items, Entity = GSRESULT#

Entity = GSRESULT, ENTNUM = 0 (or blank) for generalized plane strain results in fiber direction#

get, Par, GSRESULT, 0, Item1, IT1NUM

Item1

IT1NUM

Description

LFIBER

Fiber length change at ending point.

ROT

X,Y

Rotation angle of end plane about X or Y axis.

F

Reaction force at ending point.

M

X,Y

Reaction moment on ending plane.

*GET Postprocessing Items, Entity = MEMBER#

Entity = MEMBER, ENTNUM = N (GroupID)#

get, Par,MEMBER, N, Item1, IT1NUM

Item1

IT1NUM

Description

TEMP

MIN, MAX

Minimum or maximum temperature of members (individual reinforcings) with GroupID = N in the selected set of reinforcing elements.

*GET Postprocessing Items, Entity = NODE#

Entity = NODE, ENTNUM = N (node number) for nodal degree-of-freedom results:#

get, Par, NODE, N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

U

X, Y, Z, SUM

X, Y, or Z structural displacement or vector sum. Alternative get functions: UX( N ), UY( N ), UZ( N ).

ROT

X, Y, Z, SUM

X, Y, or Z structural rotation or vector sum. Alternative get functions: ROTX( N ), ROTY( N ), ROTZ( N ).

TEMP

Temperature. For SHELL131 and SHELL132 elements with KEYOPT(3) = 0 or 1, use TBOT, TE2, TE3,…, TTOP instead of TEMP. Alternative get functions: TEMP( N ), TBOT( N ), TE2( N ), etc.

PRES

Pressure. Alternative get function: PRES( N ).

GFV1, GFV2, GFV3

Nonlocal field values 1, 2, and 3.

VOLT

Electric potential. Alternative get function: VOLT( N ).

CONC

Concentration.

MAG

Magnetic scalar potential. Alternative get function: MAG( N ).

V

X, Y, Z, SUM

X, Y, or Z fluid velocity or vector sum in a fluid analysis. X, Y, or Z nodal velocity or vector sum in a structural transient analysis (analysis with antype,TRANS). Alternative get functions: VX( N ), VY( N ), VZ( N ).

A

X, Y, Z, SUM

X, Y, or Z magnetic vector potential or vector sum in an electromagnetic analysis. X, Y, or Z nodal acceleration or vector sum in a structural transient analysis (analysis with antype,TRANS). Alternative get functions: AX( N ), AY( N ), AZ( N ).

CURR

Current.

EMF

Electromotive force drop.

RF

FX, FY, FZ, MX, MY, MZ, CSGZ, BMOM, RATE, DVOL, FLOW, HEAT, AMPS or CHRG, FLUX, CURT, VLTG

Nodal reaction forces in the nodal coordinate system. The reaction forces returned are the total forces: static, plus damping, plus inertial, as appropriate based on analysis type (see prrsol command). The first exception is modal analyses and mode-superposition transient analyses where static forces are returned. The second exception is spectrum analyses where the prrfor logic is used internally. In this case, the reaction forces are based on the type of force requested (using ForceType with combination commands, such as srss, psdcom, etc.).

ORBT

A, B, PSI, PHI, YMAX, ZMAX, Whirl

Whirl orbit characteristics: * A is the semi-major axis. * B is the semi-minor axis. * PSI is the angle between the local axis y and the major axis Y. * PHI is the angle between initial position (t = 0) and major axis. * YMAX is the maximum displacement along local y axis. * ZMAX is the maximum displacement along local z axis. * Whirl is the direction of an orbital motion (-1 is backward whirl, 1 is forward whirl, and 0 is undetermined). Angles PSI and PHI are in degrees and within the range of -180 through +180. Orbits are available only after issuing a prorb command.

Use this command carefully when N represents an internal node, as the nodal degrees of freedom may have different physical meanings.

*GET Postprocessing Items, Entity = PATH#

Entity = PATH, ENTNUM = 0 (or blank)#

get, Par, PATH, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

MAX

Lab

Maximum value of path item Lab from last path operation. Valid labels are the user-defined labels on the pdef or pcalc command.

MAXPATH

Returns the maximum path number defined.

MIN

Lab

Minimum value of path item Lab from last path operation. Valid labels are the user-defined labels on the pdef or pcalc command.

LAST

Lab

Last value of path item Lab from last path operation. Valid labels are the user-defined labels on the pdef or pcalc command.

NODE

Value providing the number of nodes defining the path referenced in the last path operation.

ITEM

Lab

Item2 = PATHPT, IT2NUM = n The value of Lab at the n th data point from the last path operation.

POINT

n

Item2 = X,Y,Z, or CSYS. Returns information about the nth point on the current path.

NVAL

The number of path data points (the length of the data table) from the last path operation.

SET

n

Item2 = NAME. Returns the name of the n th data set on the current path.

NUMPATH

Returns the number of paths defined.

*GET Postprocessing Items, Entity = PLNSOL#

Entity = plnsol You must issue the show command before commands that produce a graphical output when running in batch mode to produce/export graphic files. For more details, see External Graphics Options, ENTNUM = 0 (or blank)#

get, Par, PLNSOL, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

MAX

Maximum value of item in last contour display ( plnsol, plesol ).

MIN

Minimum value of item in last contour display ( plnsol, plesol ).

BMAX

Maximum bound value of item in last contour display ( plnsol, plesol ).

BMIN

Minimum bound value of item in last contour display ( plnsol, plesol ).

*GET Postprocessing Items, Entity = PRENERGY#

Available after the prenergy command is issued. Entity = PRENERGY, ENTNUM = N (component number)#

get, Par, PRENERGY, N, Item1, IT1NUM

Item1

IT1NUM

Description

NCMP

Number of components ( ENTNUM not required). This value is the maximum value for N.

NENE

Number of energy types ( ENTNUM not required). This value is the maximum value for M.

TOTE

M

Total energy of type M of the model ( ENTNUM not required). Energy value is non-zero when Cname1 is blank on prior prenergy command.

ENG

M

Energy of type M of component N. Energy value is non-zero when Cname1 is specified on prior prenergy command.

PENG

M

Percentage of energy of type M of component N. Percentage of energy value is non-zero when Cname1 is specified on prior prenergy command.

Ordering of N and M corresponds to prenergy output.

*GET Postprocessing Items, Entity = PRERR#

Entity = PRERR, ENTNUM = 0 (or blank)#

get, Par, PRERR, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

SEPC[ starget_prerr_limits ]

Structural percent error in energy norm ( prerr ).

TEPC[ starget_prerr_limits ]

Thermal percent error in energy norm ( prerr ).

SERSM[ starget_prerr_limits ]

Structural error energy summation ( prerr ).

TERSM[ starget_prerr_limits ]

Thermal error energy summation ( prerr ).

SENSM[ starget_prerr_limits ]

Structural energy summation ( prerr ).

TENSM[ starget_prerr_limits ]

Thermal energy summation ( prerr ).

Some element- and material-type limitations apply. For more information, see the documentation for the prerr command.

*GET Postprocessing Items, Entity = RAD#

Entity = RAD, ENTNUM = 0 (or blank)#

get, Par, RAD, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

VFAVG

Value of the average view factor computed from the previous VFQUERY command.

*GET Postprocessing Items, Entity = RSTMAC#

Available after rstmac command is issued. Entity = rstmac, ENTNUM = N (solution number on File1 )#

get, Par, RSTMAC, 0 or N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

NS1

Total number of solutions (modes for example) read on File1. See Sbstep1 on the rstmac command. This value is the maximum value for N.

NS2

Total number of solutions (modes for example) read on File2. See Sbstep2 on the rstmac command. This value is the maximum value for M

MAC

M

Modal assurance criterion value (MAC) between the solution N read on File1 and the solution M read on File2. N and M do not correspond to the substep (or mode) numbers if NS1 and NS2 are different from the total number of substeps (or modes).

MACCYC

M

Modal assurance criterion value (MAC) from compressed table for cyclic between the solution N read on File1 and the solution M read on File2. N and M do not correspond to the substep (or mode) numbers if NS1 and NS2 are different from the total number of substeps (or modes).

*GET Postprocessing Items, Entity = SECR#

Entity = SECR, ENTNUM = n (element number) For beam and pipe (including elbow) section results, return values for all elements if the element number ( n ) is blank or ALL.#

get, Par, SECR, n, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

Item2

IT2NUM

S

X, Y, Z, XY, YZ, XZ

Component total stress

MAX - Returns maximum MIN - Returns minimum MAXY - Returns section Y location of maximum MAXZ - Returns section Z location of maximum MINY - Returns section Y location of minimum MINZ - Returns section Z location of minimum IVAL - Returns value at node or integration point at element I node JVAL - Returns value at node or integration point at element J node KVAL - Returns value at node or integration point at element K node ( ELBOW290 ) — For IVAL, JVAL, and KVAL: The ALL (or blank) option for the element number is not valid. You must specify an element ( n ).

These values are applicable only when Item2 = IVAL, JVAL, or KVAL: When KEYOPT(15) = 0, this value is the section node number (which can be visualized via secplot,,2). When KEYOPT(15) = 1 (or when using elbow elements), this value is the integration point number.

1, 2, 3

Principal stress value

INT

Stress intensity value

EQV

Equivalent stress value

EPTO

X, Y, Z, XY, YZ, XZ

Component total strain

1, 2, 3

Principal total strain value

INT

Total strain intensity value

EQV

Equivalent total strain value

EPEL

X, Y, Z, XY, YZ, XZ

Component elastic strain

1, 2, 3

Principal elastic strain value

INT

Elastic strain intensity value

EQV

Equivalent elastic strain value

EPTH

X, Y, Z, XY, YZ, XZ

Component thermal strain

1, 2, 3

Principal thermal strain value

INT

Thermal strain intensity value

EQV

Equivalent thermal strain value

EPPL

X, Y, Z, XY, YZ, XZ

Component plastic strain

1, 2, 3

Principal plastic strain value

INT

Plastic strain intensity value

EQV

Equivalent plastic strain value

EPCR

X, Y, Z, XY, YZ, XZ

Component creep strain

1, 2, 3

Principal component creep strain value

INT

Component creep strain intensity value

EQV

Equivalent component creep strain value

EPTT

X, Y, Z, XY, YZ, XZ

Component total mechanical and thermal and swelling strain

1, 2, 3

Principal total mechanical and thermal and swelling strain value

INT

Total mechanical and thermal and swelling strain intensity value

EQV

Equivalent total mechanical and thermal and swelling strain value

EPDI

X, Y, Z, XY, YZ, XZ

Component diffusion strain

1, 2, 3

Principal diffusion strain value

INT

Diffusion strain intensity value

EQV

Equivalent diffusion strain value

NL

SEPL

Plastic yield stress

SRAT

Plastic yielding (1 = actively yielding, 0 = not yielding)

HPRES

Hydrostatic pressure

EPEQ

Accumulated equivalent plastic strain

CREQ

Accumulated equivalent creep strain

PLWK

Plastic work/volume

YSIDX

TENS,SHEA

Yield surface activity status: 1 for yielded and 0 for not yielded.

FPIDX

TF01,SF01, TF02,SF02, TF03,SF03, TF04,SF04

Failure plane surface activity status: 1 for yielded and 0 for not yielded. Tension and Shear failure status are available for all four sets of failure planes.

*GET Postprocessing Items, Entity = SECTION#

Entity = SECTION, ENTNUM = component (listed below). Generate data for section stress results, using prsect before retrieving these items. Valid labels for ENTNUM are MEMBRANE, BENDING, SUM (Membrane+Bending), PEAK, and TOTAL. (The following items are not stored in the database and the values returned reflect the last quantities generated by prsect or plsect.) Only MEMBRANE, BENDING, and SUM data are available after a plsect command. The MEMBRANE label is only valid with Item1 = INSIDE.#

get, Par, SECTION, component, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Item2

Description

INSIDE

S

X, Y, Z, XY, YZ, XZ

Stress component at beginning of path.

1, 2, 3

Principal stress at beginning of path.

INT, EQV

Stress intensity or equivalent stress at beginning of path.

CENTER

S

X, Y, Z, XY, YZ, XZ

Stress component at midpoint of path.

1, 2, 3

Principal stress at midpoint of path.

INT, EQV

Stress intensity or equivalent stress at midpoint of path.

OUTSIDE

S

X, Y, Z, XY, YZ, XZ

Stress component at end of path.

1, 2, 3

Principal stress at end of path.

INT, EQV

Stress intensity or equivalent stress at end of path.

*GET Postprocessing Items, Entity = SORT#

Entity = SORT, ENTNUM = 0 (or blank)#

get, Par, SORT, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

MAX

Maximum value of last sorted item ( nsort or esort command).

MIN

Minimum value of last sorted item ( nsort or esort command).

IMAX

Node/Element number where maximum value occurs.

IMIN

Node/Element number where minimum value occurs.

*GET Postprocessing Items, Entity = SSUM#

Entity = SSUM, ENTNUM = 0 (or blank)#

get, Par, SSUM, 0, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

ITEM

Lab

Value of item Lab from last ssum command. Valid labels are the user-defined labels on the etable command.

*GET Postprocessing Items, Entity = VARI#

Entity = VARI, ENTNUM = N (variable number after POST26 data storage) (for complex values, only the real part is returned with Item1 = EXTREM)#

get, Par,VARI,N, Item1, IT1NUM, Item2, IT2NUM

Item1

IT1NUM

Description

EXTREM

VMAX

Maximum extreme value.

TMAX

Time or frequency corresponding to VMAX.

VMIN

Minimum extreme value.

TMIN

Time or frequency corresponding to VMIN.

VLAST

Last value.

TLAST

Time or frequency corresponding to VLAST.

CVAR

Covariance

REAL

f

Real part of variable N at time or frequency f.

IMAG

f

Imaginary part of variable N at frequency f.

AMPL

f

Amplitude value of variable N at frequency f

PHASE

f

Phase angle value of variable N at frequency f

RSET

Snum

Real part of variable N at location Snum.

ISET

Snum

Imaginary part of variable N at location Snum.

*GET Postprocessing Items, Entity = XFEM#

Entity = XFEM, ENTNUM = 0 (or blank)#

get, Par, XFEM, 0, Item1, IT1NUM

Item1

IT1NUM

Description

STAT

Element Number

Status of the element: 0 = uncracked, 1 = cracked