ETABLE, Lab, Item, Comp, Option
Fills a table of element values for further processing.

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | DYNA


Any unique user-defined label for use in subsequent commands and output headings. A valid label has a maximum of eight characters and is not a general predefined Item label. Default: An eight-character label formed by concatenating the first four characters of the Item and Comp labels.

If the same as a previous user label, the result item is included under the same label. Up to 200 different labels can be defined.

The following predefined labels are reserved:



Refills all tables previously defined with the ETABLE commands (not the CALC module commands) according to the latest ETABLE specifications. It is convenient for refilling tables after the load step (SET) has changed. Remaining fields are ignored.



Displays stored table values.



Erases the entire table.


Label identifying the item. General item labels are shown in the table below. Some items also require a component label. Character parameters are valid. Item = ERAS erases a Lab column.


Component of the item (if required). General component labels are shown in the table below. Character parameters can be used.


Option for storing element table data:



Store minimum element nodal value of the specified item component.



Store maximum element nodal value of the specified item component.



Store averaged element centroid value of the specified item component (default).


ETABLE defines a table of values per element (the element table) for use in further processing. The element table is organized similar to a spreadsheet, with rows representing all selected elements and columns consisting of result items which have been moved into the table (Item,Comp) via ETABLE. Each column of data is identified by a user-defined label (Lab) for listings and displays.

After entering the data into the element table, you are not limited to merely listing or displaying your data (PLESOL, PRESOL, etc.). You can also perform many types of operations on your data, such as adding or multiplying columns (SADD, SMULT), defining allowable stresses for safety calculations (SALLOW), or multiplying one column by another (SMULT). See Getting Started in the Mechanical APDL Basic Analysis Guide for more information.

Various results data can be stored in the element table. For example, many items for an element are inherently single-valued (one value per element). The single-valued items include: SERR, SDSG, TERR, TDSG, SENE, SEDN, TENE, KENE, AENE, JHEAT, JS, VOLU, and CENT. All other items are multivalued (varying over the element, such that there is a different value at each node). Because only one value is stored in the element table per element, an average value (based on the number of contributing nodes) is calculated for multivalued items. Exceptions to this averaging procedure are FMAG and all element force items, which represent the sum only of the contributing nodal values.

Two methods of data access can be used with the ETABLE command. The method you select depends upon the type of data that you want to store. Some results can be accessed via a generic label (Component Name method), while others require a label and number (Sequence Number method).

The component name method is used to access the general element data (that is, element data which is generally available to most element types or groups of element types). All of the single-valued items and some of the more general multivalued items are accessible with the Component Name method. Various element results depend on the calculation method and the selected results location (AVPRIN, RSYS, LAYER, SHELL, and ESEL).

Although nodal data is readily available for listings and displays (PRNSOL, PLNSOL) without using the element table, you can also use the Component Name method to enter these results into the element table for further "worksheet" manipulation. (See Getting Started in the Mechanical APDL Basic Analysis Guide for more information.) A listing of the General Item and Comp labels for the component name method is shown below.

The sequence number method enables you to view results for data that is not averaged (such as pressures at nodes, temperatures at integration points, etc.), or data that is not easily described in a generic fashion (such as all derived data for structural line elements and contact elements, all derived data for thermal line elements, layer data for layered elements, etc.). A table illustrating the Items (such as LS, LEPEL, LEPTH, SMISC, NMISC, SURF, etc.) and corresponding sequence numbers for each element is shown in the Output Data section of each element description.

Some element table data are reported in the results coordinate system. These include all component results (for example, UX, UY, etc.; SX, SY, etc.). The solution writes component results in the database and on the results file in the solution coordinate system. When you issue the ETABLE command, these results are then transformed into the results coordinate system (RSYS) before being stored in the element table. The default results coordinate system is global Cartesian (RSYS,0). All other data are retrieved from the database and stored in the element table with no coordinate transformation.

To display the stored table values, issue the PRETAB, PLETAB, or ETABLE,STAT command. To erase the entire table, issue ETABLE,ERAS. To erase a Lab column, issue ETABLE,Lab,ERAS.

When the GUI is enabled, if a Delete operation in a Define Element Table Data dialog box writes this command to a log file (Jobname.LOG or Jobname.LGW), the program sets Lab = blank, Item = ERASE, and Comp = an integer number. In this case, the program has assigned a value of Comp that corresponds to the location of a chosen variable name in the dialog list. It is not intended that you type in such a location value for Comp in a session; however, a file that contains a GUI-generated ETABLE command of this form can be used for batch input or the /INPUT command.

The MIN and MAX options are not available for thermal elements.

The element table data option (Option) is not available for all output items. See the table below for supported items.

Table 125:  ETABLE - General Item and Component Labels

General Item and Component Labels ETABLE, Lab, Item, Comp
Valid Item Labels for Degree of Freedom Results
UX, Y, ZX, Y, or Z structural displacement.
ROTX, Y, ZX, Y, or Z structural rotation.
TEMP [1] Temperature.
PRES Pressure.
VOLT Electric potential.
MAG Magnetic scalar potential.
VX, Y, ZX, Y, or Z fluid velocity.
AX, Y, ZX, Y, or Z magnetic vector potential.
CONC Concentration.
CURR Current.
EMF Electromotive force drop.
Valid Item and Component Labels for Element Results
S [2]X, Y, Z, XY, YZ, XZComponent stress.
1, 2, 3Principal stress.
INTStress intensity.
EQVEquivalent stress.
EPEL [2]X, Y, Z, XY, YZ, XZComponent elastic strain.
1, 2, 3Principal elastic strain.
INTElastic strain intensity.
EQVElastic equivalent strain.
EPTH [2]X, Y, Z, XY, YZ, XZComponent thermal strain.
1, 2, 3Principal thermal strain.
INTThermal strain intensity.
EQVThermal equivalent strain.
EPPL [2]X, Y, Z, XY, YZ, XZComponent plastic strain.
1, 2, 3Principal plastic strain.
INTPlastic strain intensity.
EQVPlastic equivalent strain.
EPCR [2]X, Y, Z, XY, YZ, XZComponent creep strain.
1, 2, 3Principal creep strain.
INTCreep strain intensity.
EQVCreep equivalent strain.
EPSW [2] Swelling strain.
EPTO [2]X, Y, Z, XY, YZ, XZComponent total mechanical strain (excluding thermal) (EPEL + EPPL + EPCR).
1, 2, 3Principal total mechanical strain.
INTTotal mechanical strain intensity.
EQVTotal equivalent mechanical strain.
EPTT [2]X, Y, Z, XY, YZ, XZComponent total strain including thermal and swelling (EPEL + EPTH + EPPL + EPCR + EPSW).
1, 2, 3Principal total strain.
INTTotal strain intensity.
EQVTotal equivalent strain.
NL [2]SEPLEquivalent stress (from stress-strain curve).
SRATStress state ratio.
HPRESHydrostatic pressure.
EPEQAccumulated equivalent plastic strain.
SEND [2]ELASTICElastic strain energy density.
PLASTICPlastic strain energy density.
CREEPCreep strain energy density.
DAMAGEDamage strain energy density.
VDAMViscoelastic dissipation energy density.
VREGVisco-regularization strain energy density.
ENTOTotal strain energy density.
SVAR1 to MAXState variable.
CDMDMGDamage variable.
LMMaximum previous strain energy for virgin material.
FAILMAX [1][4]Maximum of all active failure criteria defined at the current location (FCTYP) .
EMAX [1][4] Maximum Strain Failure Criterion.
SMAX [1][4]Maximum Stress Failure Criterion.
TWSI [1][4] Tsai-Wu Strength Index Failure Criterion.
TWSR [1][4] Inverse of Tsai-Wu Strength Ratio Index Failure Criterion.
HFIB [1][4][6]Hashin Fiber Failure Criterion.
HMAT [1][4][6] Hashin Matrix Failure Criterion.
PFIB [1][4][6]Puck Fiber Failure Criterion.
PMAT [1][4][6]Puck Matrix Failure Criterion.
L3FB [1][4][6]LaRc03 Fiber Failure Criterion.
L3MT [1][4][6]LaRc03 Matrix Failure Criterion.
L4FB [1][4][6]LaRc04 Fiber Failure Criterion.
L4MT [1][4][6]LaRc04 Matrix Failure Criterion.
USR1, USR2, ..., USR9 [1][4][5][6]User-defined failure criteria.
PFCMAX [7]Maximum of all failure criteria defined at current location
FT [7]Fiber tensile failure criteria
FC [7]Fiber compressive failure criteria
MT [7]Matrix tensile failure criteria
MC [7]Matrix compressive failure criteria
PDMGSTATDamage status (0 - undamaged, 1 - damaged, 2 - completely damaged)
FTFiber tensile damage variable
FCFiber compressive damage variable
MTMatrix tensile damage variable
MCMatrix compressive damage variable
SShear damage variable (S)
SEDEnergy dissipated per unit volume
SEDVEnergy per unit volume due to viscous damping
FCMX [1][4]LAYLayer number where the maximum of all active failure criteria over the entire element occurs.

Number of the maximum-failure criterion over the entire element:

1 - EMAX
2 - SMAX
3 - TWSI
4 - TWSR
5 - PFIB
6 - PMAT
7 - HFIB
8 - HMAT
9 - L3FB
10 - L3MT
11 - L4FB
12 - L4MT
13~21 - USR1~USR9
VALValue of the maximum failure criterion over the entire element.
TGX, Y, Z, SUMComponent thermal gradient or vector sum.
TFX, Y, Z, SUMComponent thermal flux or vector sum.
PGX, Y, Z, SUMComponent pressure gradient or vector sum.
EFX, Y, Z, SUMComponent electric field or vector sum.
DX, Y, Z, SUMComponent electric flux density or vector sum.
HX, Y, Z, SUMComponent magnetic field intensity or vector sum.
BX, Y, Z, SUMComponent magnetic flux density or vector sum.
CGX, Y, Z, SUMComponent concentration gradient or vector sum.
DFX, Y, Z, SUMComponent diffusion flux density or vector sum.
FMAG [5]X, Y, Z, SUMComponent electromagnetic forces or vector sum.
SERR [6] Structural error energy.
SDSG [6] Absolute value of maximum variation of any nodal stress component.
TERR [6] Thermal error energy.
TDSG [6] Absolute value of the maximum variation of any nodal thermal gradient component.
FX, Y, ZComponent structural force. Sum of element nodal values.
MX, Y, ZComponent structural moment. Sum of element nodal values.
HEAT Heat flow. Sum of element nodal values.
FLOW Fluid flow. Sum of element nodal values.
AMPS Current flow. Sum of element nodal values.
FLUX Magnetic flux. Sum of element nodal values.
CSGX, Y, ZComponent magnetic current segment.
RATE Diffusion flow rate. Sum of element nodal values.
SENE "Stiffness" energy or thermal heat dissipation (applies to all elements where meaningful). Same as TENE.
SEDN Strain energy density.
AENE Artificial energy of the element. This includes the sum of hourglass control energy and energy generated by in-plane drilling stiffness from shell elements (applies to all elements where meaningful). It also includes artificial energy due to contact stabilization. The energy is used for comparisons to SENE energy to predict the solution error due to artificial stiffness. See the Mechanical APDL Theory Reference.
TENE Thermal heat dissipation or "stiffness" energy (applies to all elements where meaningful). Same as SENE.
KENE Kinetic energy (applies to all elements where meaningful).
STEN Elemental energy dissipation due to stabilization.
JHEAT Element Joule heat generation.
JSX, Y, Z, SUMSource current density for low-frequency magnetic analyses. Total current density (sum of conduction and displacement current densities) in low frequency electric analyses. Components (X, Y, Z) and vector sum (SUM).
JTX, Y, Z, SUMTotal measureable current density in low-frequency electromagnetic analyses. (Conduction current density in a low-frequency electric analysis.) Components (X, Y, Z) and vector sum (SUM).
JCX, Y, Z, SUMConduction current density for elements that support conduction current calculation. Components (X, Y, Z) and vector sum (SUM).
MRE Magnetics Reynolds number
VOLU Element volume. Based on unit thickness for 2-D plane elements (unless the thickness option is used) and on the full 360 degrees for 2-D axisymmetric elements.
CENTX, Y, ZUndeformed X, Y, or Z location (based on shape function) of the element centroid in the active coordinate system.
BFE [2]TEMPBody temperatures (calculated from applied temperatures) as used in solution (area and volume elements only).
SMISCsnumElement summable miscellaneous data value at sequence number snum (shown in the Output Data section of each applicable element description in the Element Reference).
NMISCsnumElement non-summable miscellaneous data value at sequence number snum (shown in the Output Data section of each applicable element description found in the Element Reference).
SURFsnumElement surface data value at sequence number snum.
CONTSTAT [4]Contact status:
3-closed and sticking
2-closed and sliding
1-open but near contact
0-open and not near contact
PENEContact penetration (zero or positive).
PRESContact pressure.
SFRICContact friction stress.
STOTContact total stress (pressure plus friction).
SLIDEContact sliding distance.
GAPContact gap distance (0 or negative).
FLUXTotal heat flux at contact surface.
CNOSTotal number of contact status changes during substep.
FPRSFluid penetration pressure
TOPO Densities used for topological optimization.
CAPC0,X0,K0,ZONE, DPLS,VPLSMaterial cap plasticity model only: Cohesion; hydrostatic compaction yielding stress; I1 at the transition point at which the shear and compaction envelopes intersect; zone = 0: elastic state, zone = 1: compaction zone, zone = 2: shear zone, zone = 3: expansion zone; effective deviatoric plastic strain; volume plastic strain.
EDPCCSIG,CSTRMaterial EDP creep model only (not including the cap model): Equivalent creep stress; equivalent creep strain.
ESIG [2]X,Y,Z,XY,YZ,ZXComponents of Biot’s effective stress.
1, 2, 3Principal stresses of Biot’s effective stress.
INTStress intensity of Biot’s effective stress.
EQVEquivalent stress of Biot’s effective stress.
DPARTPORTotal porosity (Gurson material model).
GPORPorosity due to void growth.
NPORPorosity due to void nucleation.
FFLXX,Y,ZFluid flow flux in poromechanics.
FICT [2]TEMPFictive temperature.
PMSVVRAT, PPRE, DSAT, RPERVoid volume ratio, pore pressure, degree of saturation, and relative permeability for coupled pore-pressure CPT elements.
YSIDXTENS,SHEAYield surface activity status for Mohr-Coloumb, soil, concrete, and joint rock material models: 1 = yielded, 0 = not yielded.
FPIDX TF01,SF01, TF02,SF02, TF03,SF03, TF04,SF04Failure plane surface activity status for concrete and joint rock material models: 1 = yielded, 0 = not yielded. Tension and shear failure status are available for all four sets of failure planes.
NSX, Y, Z, XY, YZ, XZNominal strain for hyperelastic material, reported in the current configuration (unaffected by RSYS).
MPLADMAC, DMAXMicroplane damage, macroscopic and maximum values.

  1. For SHELL131 and SHELL132 elements with KEYOPT(3) = 0 or 1, use labels TBOT, TE2, TE3, . . ., TTOP instead of TEMP.

  2. Element table option (Option) is available for this element output data item.

  3. For the CONT items for elements CONTA171 through CONTA177, the reported data is averaged across the element.

  4. For MPC-based contact definitions, the value of STAT can be negative, indicating that one or more contact constraints were intentionally removed to prevent overconstraint. STAT = -3 is used for MPC bonded contact; STAT = -2 is used for MPC no-separation contact.

  5. When using the EMFT procedure to calculate electromagnetic force (PLANE121, SOLID122, SOLID123, PLANE233, SOLID236 or SOLID237 elements only), the FMAG sum will be zero or near zero.

  6. Some element- and material-type limitations apply. For more information, see PRERR.

  7. Failure criteria are based on the effective stresses in the damaged material.

Menu Paths

Main Menu>General Postproc>Element Table>Define Table
Main Menu>General Postproc>Element Table>Erase Table

Release 18.2 - © ANSYS, Inc. All rights reserved.