Refer to the PRNSOL and PRESOL command pages in the Mechanical APDL application Commands Reference for descriptions of most Component and Expression entries in the table. Some other entries are self-explanatory (SUM for example). VECTORS refer to vector plot results that include arrows in the display.
The following tables include descriptions of additional user defined result names not included in the PRESOL/PRNSOL listings. The Solution object Worksheet lists these result options following a solution (see Application).
The following table lists the available expressions that you can use to define your User Defined Result. Node-based user defined results are most often associated with degree of freedom solutions (like nodal reactions).
| Name | Description |
|---|---|
| R | Nodal rotations in a structural analysis (analogous to PRNS,ROT) |
| OMG | Nodal rotational velocities in a structural transient dynamic analysis (analogous to PRNS,OMG) |
| DOMG | Nodal rotational accelerations in a structural transient dynamic analysis (analogous to PRNS,DMG) |
| MVP_AZ | Nodal Z magnetic vector potential in an axisymmetric electromagnetic analysis (analogous to PRNS,A) |
| LOC | Nodal locations (x,y,z) |
| LOC_DEF | Deformed nodal locations (x+ux,y+uy,z+uz) |
| F | Nodal structural forces (reaction)1 |
| M | Nodal structural moments (reaction)1 |
| CSG | Nodal magnetic current segments (reaction) |
| HEAT | Nodal thermal heat flow (reaction) |
| AMPS | Nodal electric current (reaction) |
| NDIR | Nodal THXY, THYZ, and THZX values. The NDIRVECTORS display consists of triads. |
| REULER | Structural rotations displayed as Euler triads. |
1 - When user defined results FX, FY, FZ, FSUM, and FVECTORS (and MX, MY, MZ, MSUM, and MVECTORS) are scoped to a path, then it is possible that no contours will be displayed. The reason is that these types of forces/moments are solved only at constrained nodes. The result value at a path point is interpolated from the nodal values of the elements that contain the path point. If a path point touches an element in which some nodes have undefined reactions, then Mechanical cannot properly interpolate the nodal values for the path point. No contour color is displayed at such a path point.
The following table lists the available expressions that you can use to define your element-based User Defined Result. Element-based user defined results can exist at the nodes (like stress and strain) or can exist at the centroid (like volume).
| Name | Description |
|---|---|
| SPSD | Element nodal equivalent stress as calculated by the solver. |
| ELEMENTAL_REAL | Element real data from the Mechanical APDL R command. |
| EPCREQV_RST | Element nodal equivalent creep strain as calculated by the solver. |
| EPELEQV_RST | Element nodal equivalent elastic strain as calculated by the solver. |
| EPPLEQV_RST | Element nodal equivalent plastic strain as calculated by the solver. |
| EPTTEQV_RST | Element nodal equivalent total strain (plus thermal strain) as calculated by the solver, that is, EPTTEQV_RST is total mechanical and thermal strain: EPTTEQV_RST = EPELEQV_RST + EPPLEQV_RST + EPCREQV_RST + EPTHEQV_RST. |
| EPTOEQV_RST | Element nodal equivalent total strain as calculated by the solver, that is, EPTOEQV_RST is total mechanical strain: EPTOEQV_RST = EPELEQV_RST + EPPLEQV_RST + EPCREQV_RST. |
| ETOP | Element nodal densities used for topological optimization (same as TOPO). |
| BEAM | Element nodal beam stresses: direct, minimum bending, maximum bending, minimum combined, maximum combined. |
| SVAR | Element nodal state variable data. |
| CONTJHEA | Element nodal Joule heat for CONTA174. |
| CONTFORC | Element nodal contact normal forces for CONTA175. |
| BEAM_AXIAL_F | Element nodal axial force vectors for BEAM188/189. |
| BEAM_BENDING_M | Element nodal bending moment vectors for BEAM188/189. |
| BEAM_TORSION_M | Element nodal torsion moment vectors for BEAM188/189. |
| BEAM_SHEAR_F | Element nodal shear force vectors for BEAM188/189. |
| PIPE_INTERNAL_PRESSURE | Internal pressure at integration point for PIPE288. |
| PIPE_EXTERNAL_PRESSURE | External pressure at integration point for PIPE288. |
| PIPE_EFFECTIVE_TENSION | Effective tension at integration point for PIPE288. |
| PIPE_HOOP_STRESS | Maximum Hoop Stress at integration point for PIPE288/PIPE289. |
| ENFO | Element nodal reaction forces for structural analyses. |
| ENMO | Element nodal reaction moments for structural analyses. |
| EHEAT | Element nodal heat values for thermal analyses. |
| CURRENTSEG | Element nodal magnetic current segments. |
| VOLUME | Element volumes. |
| ENERGY | Element potential and kinetic energies. |
| RIGID_ANG | Element Euler angles for MASS21 elements (rotation about x-axis, rotation about y-axis, rotation about z-axis). |
| CONTSMISC | Element summable miscellaneous data for contact elements. CONTSMISC is completely analogous in implementation to SMISC (see “User Defined Results Not Displayed in Worksheet” below), except that CONTSMISC, for display purposes, extrapolates the single elemental value to the corner nodes. |
| CONTNMISC | Element non-summable miscellaneous data for contact elements. CONTNMISC is completely analogous in implementation to NMISC (see “User Defined Results Not Displayed in Worksheet” below), except that CONTSMISC, for display purposes, extrapolates the single elemental value to the corner nodes. |
| EDIR | Elemental THXY, THYZ, and THZX values: (1) currently only angles of first node in solution record are employed; (2) the EDIRVECTORS display consists of triads. |
| ECENT | Element centroids (x,y,z) |
| PNUMTYPE | Element type reference numbers. |
| PNUMREAL | Real constant set numbers. |
| PNUMMAT | Material set numbers. |
| PNUMSEC | Section numbers. |
| PNUMESYS | Element coordinate system numbers (note: a 0 value corresponds to the global Cartesian system). |
| PNUMELEM | Mechanical APDL element ID. |
| PNUMENAM | Mechanical APDL element identifying number (such as 181 for SHELL181 elements). |
| CONTPNUMTYPE | Element type reference numbers for contact elements. |
| CONTPNUMREAL | Real constant set numbers for contact elements. |
| CONTPNUMMAT | Material set numbers for contact elements. |
| CONTPNUMSEC | Section numbers for contact elements. |
| CONTPNUMESYS | Element coordinate system numbers for contact elements. |
| CONTPNUMELEM | Mechanical APDL Element ID for contact elements. |
| CONTPNUMENAM | Mechanical APDL element identifying number for contact elements. |
| SMISC | Element summable miscellaneous data. |
| NMISC | Element non-summable miscellaneous data. |
| EFFNU_ZERO_EPTOEQV |
Element nodal equivalent total strain (EPEL + EPPL + EPCR) as calculated by the post-processor. For average results, the solver averages the element nodal component strains at common nodes and performs a Von Mises calculation with effective Poisson's Ratio set to ZERO. |
| EFFNU_ZERO_EPTTEQV |
Element nodal equivalent total strain plus thermal strain (EPEL + EPPL + EPCR + EPTH) as calculated by the post-processor. For average results, the solver averages the element nodal component strains at common nodes and performs a Von Mises calculation with effective Poisson's Ratio set to ZERO. |
|
LAYNUMBER |
Number of layers, as defined by the section database, for a shell element. If no section database exists, the number of layers is displayed as zero. |
|
LAYTHICK |
Thickness of a layer, as defined by the section database, for a shell element. The layer number is specified using the Layer property. If the Layer property is set to , the thickness of the entire element is displayed. |
|
LAYMATERIAL |
Material number for
an element, displayed in a manner similar to
Mechanical APDL's graphic for
/PNUM,MAT,1. If a shell element contains
layers defined by the section database and if the
Layer property is set to a
layer number greater than
|
|
LAYANGLE |
Angle of a layer's coordinate system with respect to the element coordinate system, as defined by the section database, for a shell element. The layer number is specified by the Layer property. If the Layer property is set to , a value of zero is displayed. |
|
LAYOFFY |
Section offset in the Y direction, as defined by the section database, for a shell element. The Y offset is the same for all layers. |
| THERMAL_FLUID_HT_COND_RATE |
Rate of fluid flow through a specified Line Body. |
| THERMAL_FLUID_FLOW_RATE |
Heat flow rate due to conduction within the fluid of a Line Body. |
| MESH_ELEMENT_QUALITY |
Composite quality of meshed elements. |
| MESH_ASPECT_RATIO |
Aspect ratio for triangles and quadrilaterals of meshed elements. |
| MESH_JACOBIAN_RATIO |
Jacobian Ratio of meshed elements. |
| MESH_WARPING_FACTOR |
Warping Factor of meshed elements. |
| MESH_PARALLEL_DEVIATION |
Parallel Deviation of meshed elements. |
| MESH_MAXIMUM_CORNER_ANGLE |
Maximum Corner Angle of meshed elements. |
| MESH_SKEWNESS |
Skewness of meshed elements. |
Using this data, you can explicitly define your user defined result,
such as total deformation by using the component deformations across
all of the nodes in the model, identified by
UX, UY, and
UZ. You can use these component values
to mathematically produce a user defined result for total
deformation: SQRT(UX^2+UY^2+UZ^2).
Notes
For complete descriptions of the mesh-based element results listed above, see the Mesh Metric section in the Meshing User's Guide.
If the Display Option is set to Averaged, then for the results ENFO, EHEAT, and CURRENTSEG, the result at each node represents the sum (or contributions) of all the elements that contain the node.
If the Display Option is set to Unveraged, the ENFO result is analogous to PLES,FORCE.
SPSD is a User Defined Result that is unique to the Mechanical APDL result file. For any element that supports stresses, the SPSD result represents the equivalent stress, for each corner node in the element, as stored on the result file. Hence, SPSD is the equivalent stress as calculated by the Mechanical APDL solver for the corner nodes. For this result, SPSD is the expression displayed in the Type column and Stress is displayed in the Output Unit column. Prior to release 13.0, SPSD represented the equivalent stress as calculated from component stresses during postprocessing, that is, it was not calculated by the Mechanical APDL solver.
By default, Contact Results (accessible through User Defined Results via CONTSTAT or CONTFLUX) are not written to the result file in a thermal analysis.
Displays of /PNUM results are analogous to EPLOTs with the following commands in Mechanical APDL:
/PNUM,TYPE,1
/PNUM,REAL,1
/PNUM,MAT,1
/PNUM,SEC,1
/PNUM,ESYS,1
/PNUM,ELEM,1
For example, the range of the values of the PNUMTYPE result vary from the smallest element type to the largest element type, as created by ANSYS ET commands.
PNUM results are available for all analysis types.
When you are analyzing shell elements, the PNUMMAT result displays a Material Number for each layer when the following conditions are met:
The shell element contains layers defined by the section database (via SECDATA command).
And...
The Layer property of
the User Defined Result is set to a number greater
than 0.
Mechanical supports up to 64 SVAR results (SVAR1, ..., SVAR64). If you define more than 64 SVAR results, the solver ignores all entries.
For non-linear analyses, user defined results corresponding to Mechanical APDL PLES commands with NL as an Item are available with the following components:
SEPL, SRAT, HPRE, EPEQ, PSV, PLWK, CRWK, ELWK, SGYT, and PEQT
Although there are no user defined results with SEND in Mechanical, you can use the following:
| Use This | For This |
| NLPLWK | PLES,SEND,PLASTIC |
| NLCRWK | PLES,SEND,CREEP |
| NLELWK | PLES,SEND,ELASTIC |
For the Mechanical APDL solver, there are User Defined Results associated with summable miscellaneous data (SMISC) and non-summable miscellaneous data (NMISC) on the result file. These results are not listed in the Solution Worksheet. Because this data can be voluminous, by default, Mechanical does not write it to the result file for all element types in the model (examples of MISC records always written to the result file include beam, joint, and spring element types). You activate miscellaneous output for all elements or just contact elements using the Output Controls available in the Details of the Analysis Settings object. Mechanical has adopted a convention that miscellaneous data for contact elements be called CONTSMISC and CONTNMISC. This means that SMISC and NMISC data will only display on non-contact elements and that CONTSMISC and CONTNMISC data will only display on contact elements. You can also request and store state variables such as USERMAT or USERCREEP if you wish to utilize user-defined materials. Like miscellaneous data, SMISC and NMISC, the state variables do not display in the Solution Worksheet. You access state variables using the expression field entry SVAR followed by the state variable number.
To display these results:
Click on the toolbar button.
In the Details view Expression field, type the string SMISC or NMISC followed by the sequence number which indicates the desired datum.
For example, to display the 2nd sequence number for SMISC, enter SMISC2 for the Expression. The graphics contour display will be similar to the Mechanical APDL display for the command PLESOL,SMISC,2. When you evaluate this result, the Details view will show no units and no coordinate system for this data. That is, no unit conversions and no coordinate transformations are performed. If you enter a data expression that does not exist on the result file, the result will not be evaluated. To display the 2nd sequence number for summable miscellaneous data on scoped contact elements, enter CONTSMISC2 for the Expression.
The following limitations are associated with vector display for user defined results:
The beam is defined by nodes I(end 1) and J(end 2) and an optional orientation node K. Depending upon direction from node I to node J, the displayed vector for these results may be flipped 180 degrees.