This section examines supported expressions for the User Defined Result as well as certain requirements and limitations for their use with the Mechanical APDL solver.
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 for node- and element-based results list 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). 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).
Go to a section topic:
Important: Review the Notes below for specific requirements and characteristics regarding certain User Defined Results as well as the topics for User Defined Results Not Displayed in Worksheet and Limitations of Vector Displays.
Node-Based Result Expressions
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 |
|---|---|
| AMPS | Nodal electric current (reaction) |
| CSG | Nodal magnetic current segments (reaction) |
| DOMG | Nodal rotational accelerations in a structural transient dynamic analysis (analogous to PRNS,DMG) |
| F | Nodal structural forces (reaction)[a] |
| HEAT | Nodal thermal heat flow (reaction) |
| LOC | Nodal locations (x,y,z) |
| LOC_DEF | Deformed nodal locations (x+ux,y+uy,z+uz) |
| M | Nodal structural moments (reaction)[a] |
| MVP_AZ | Nodal Z magnetic vector potential in an axisymmetric electromagnetic analysis (analogous to PRNS,A) |
| NDIR | Nodal THXY, THYZ, and THZX values. The NDIRVECTORS display consists of triads. |
| NAR_EPEL | Component (X, Y, Z, XY, YZ, XZ) strain and Principal (1, 2, 3, INT) elastic strain.[b] |
| NAR_EPCR | Component (X, Y, Z, XY, YZ, XZ) strain and Principal (1, 2, 3, INT) creep strain.[b] |
| NAR_EPPL | Component (X, Y, Z, XY, YZ, XZ) strain and Principal (1, 2, 3, INT) plastic strain.[b] |
| NAR_EPTH | Component (X, Y, Z, XY, YZ, XZ) strain and Principal (1, 2, 3, INT) thermal strain.[b] |
| NAR_EPTO | Component (X, Y, Z, XY, YZ, XZ) strain and Principal (1, 2, 3, INT) total strain.[b] |
| NAR_EPELEQV_RST | Equivalent elastic strain.[b] |
| NAR_EPCREQV_RST | Equivalent creep strain.[b] |
| NAR_EPPLEQV_RST | Equivalent plastic strain.[b] |
| NAR_EPTHEQV_RST | Equivalent thermal strain.[b] |
| NAR_EPTOEQV_RST | Equivalent total strain.[b] |
| NAR_S | Component (X, Y, Z, XY, YZ, XZ) stress and Principal (1, 2, 3, INT, EQV) stress.[b] |
| OMG | Nodal rotational velocities in a structural transient dynamic analysis (analogous to PRNSOL,OMG) |
| R | Nodal rotations in a structural analysis (analogous to PRNSOL,ROT) |
| REULER | Structural rotations displayed as Euler triads. |
| UACOUSTIC | Nodal displacement for an Acoustic Environment which equals the pressure value divided by the product of density and gravity. |
| UALL | UALL is the nodal displacement solution (X, Y, or Z structural displacement or vector sum) that is displayed even if the node is deactivated using the EKILL/EALIVE commands. If all elements are LIVE/ACTIVE, then the UALL result is exactly the same as the U result. This result can be useful in the study of Additive Manufacturing. |
[a] The application computes the result values of Forces and Moments (FX/MX, FY/MY, FZ/MZ, FSUM/MSUM, and FVECTORS/MVECTORS) only at constrained nodes. Consequently, if you create a User Defined Result from one of these values and scope it to a Construction Geometry Path, it is possible that no contours will display. Since Mechanical cannot properly interpolate the nodal values at the path point if a path point touches an element with unconstrained nodes, it displays no contour color.
[b] See the Nodal Average Result note below.
Element-Based Result Expressions
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 |
|---|---|
| AI | Element nodal acoustic intensity (pressure times the complex conjugate of the
acoustic velocity vector (PG)). Components include AIX, AIY, AIZ, AISUM, and AIVECTORS. Note:
|
| SPSD | Element nodal equivalent stress as calculated by the solver. See SPSD Result note below. |
| SFPRES | Surface pressure load applied to SOLID187 elements in models with cracks. The load is defined by the SF command in the solution. The SFPRES result is displayed as a vector normal to the element face. |
| ELEMENTAL_REAL | Element real data from the Mechanical APDL R command. |
| ELEMENTAL_STATUS | Element birth/death status associated with the EKILL command. If element is DEAD, the status is 1; if element is not DEAD, status is 0.. |
| 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. |
| CONTFNODE | Component (X, Y, Z) contact element forces.[a] |
| CONTHNODE | Contact element heat.[a] |
| CONTAREA | Contact element area.[a] |
| 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. |
| BEAMDIRECT | Direct Stress, the stress component due to the axial load encountered in a beam element. |
| BEAMMIN_BENDING | Minimum Bending Stress. From any bending loads a bending moment in both the local Y and Z directions will arise. This leads to the following four bending stresses: Y bending stress on top/bottom and Z bending stress on top/bottom. Minimum Bending Stress is the minimum of these four bending stresses. |
| BEAMMAX_BENDING | Maximum Bending Stress, the maximum of the four bending stresses described under Minimum Bending Stress. |
| BEAMMIN_COMBINED | Minimum Combined Stress, the linear combination of the Direct Stress and the Minimum Bending Stress. |
| BEAMMAX_COMBINED | Maximum Combined Stress, the linear combination of the Direct Stress and the Maximum Bending Stress. |
| 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.[b] |
| PNUMREAL | Real constant set numbers.[b] |
| PNUMMAT | Material set numbers.[b] |
| PNUMSEC | Section numbers.[b] |
| PNUMESYS | Element coordinate system numbers (note: a 0 value corresponds to the global Cartesian system).[b] |
| PNUMELEM | Mechanical APDL element ID.[b] |
| PNUMENAM | Mechanical APDL element identifying number (such as 181 for SHELL181 elements).[b] |
| CONTPNUMTYPE | Element type reference numbers for contact elements.[b] |
| CONTPNUMREAL | Real constant set numbers for contact elements.[b] |
| CONTPNUMMAT | Material set numbers for contact elements.[b] |
| CONTPNUMSEC | Section numbers for contact elements.[b] |
| CONTPNUMESYS | Element coordinate system numbers for contact elements.[b] |
| CONTPNUMELEM | Mechanical APDL Element ID for contact elements.[b] |
| CONTPNUMENAM | Mechanical APDL element identifying number for contact elements.[b] |
| 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.[b] |
|
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. |
| MESH_ORTHOGONAL_QUALITY |
Orthogonal Quality of meshed elements. |
| MESH_CHARACTERISTIC_LENGTH |
Characteristic Length of meshed elements. |
| COMBI250_F | Structural force (reaction) using element COMBI250. Components include X, Y, Z, Sum, and Vectors. |
| COMBI250_M | Structural moment (reaction) using element COMBI250. Components include X, Y, Z, Sum, and Vectors. |
| TARGFPRS | This expression displays fluid penetration pressure at the target side of a contact condition. The application stores this data in the result file for the target element. |
[a] The solver does not calculate these element nodal results. The application calculates these results using the centroid value of each scoped element and divides that value by the number of nodes included in the element. The application then assigns this derived value to each node. This creates an elemental-nodal result. The application does not perform any interpolation for these calculations.
Characteristics, Requirements, and Limitations
Review the following specific characteristics, requirements, and limitations associated with certain User Defined Results.
- Display Option
If the Display Option is set to:
Averaged: For the ENFO, EHEAT, and CURRENTSEG expressions, the result at each node represents the sum (or contributions) of all the elements that contain the node.
Unaveraged: The ENFO expression is analogous to PLESOL,FORCE.
- Node-based Element Reaction Results
If your User Defined Result contains an expression which is performing mathematical operations on elemental nodal Reaction results, such as ENFO, ENMO, EHEAT, CURRENTSEG, etc., the value shown in the Total/Average column of the Details pane could be incorrect. For these types of user defined results, Ansys recommends that you export all result values and manually calculate the Total/Average to verify the values.
- Contact Results
By default, Contact Results (accessible through User Defined Results via CONTSTAT or CONTFLUX) are not written to the result file in a thermal analysis.
- SPSD Result
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.
- Nodal Average Result
Note the following Nodal Average Result (NAR) requirements. NAR results are:
Supported by Mechanical APDL solver only.
Controlled by the OUTRES,NAR command.
Results averaged across all bodies.
Displayed in the Global Coordinate System only.
Not supported the MAXSHEAR component.
Not supported for Random Vibration Analyses and Response Spectrum analyses.
Not supported for Equivalent Strain data (zero is reported) for the element LINK180.
Note: If you use the OUTRES command in a Commands (APDL) object to 1) disable a tensor result and 2) enable the corresponding NAR, the application only supports the Averaged option for the Display Option and Average Across Bodies properties for the specified result. Furthermore, the label "Nodal Averaged Result" is displayed in the legend of the Geometry window for the result.
- PNUM Command
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.
Important: Mechanical supports up to 200 SVAR results (SVAR1, ..., SVAR200). Do not exceed this value. If more than 200 SVAR results exist in the result file, Mechanical does not evaluate or display any SVAR results. All SVAR results in the result file are ignored.
Note: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.
- Nonlinear Analysis Components
During a nonlinear analysis (Large Deflection property set to ), the application generates the following components for the Nonlinear (NL) Item of the PLESOL command.
Component Description User Defined Result Expression SEPL Equivalent stress (from stress-strain curve). NLSEPL SRAT Stress state ratio. NLSRAT HPRE Hydrostatic pressure. NLHPRE EPEQ Accumulated equivalent plastic strain. NLEPEQ CREQ Accumulated equivalent creep strain. NLCREQ PLWK Plastic work per volume/plastic strain energy density. NLPLWK[a] CRWK Creep strain energy density. NLCRWK[b] ELWK Elastic strain energy density. NLELWK[c] SGYT Yield stress (tensile). NLSGYT[d] PEQT Equivalent plastic strain (tensile). NLPEQT[d] - Solution Coordinate System Results
If you evaluate a User Defined Result with Element-Nodal result quantities (e.g., stress) that are 1) averaged, or 2) interpolated, the application could produce incorrect result values when using the . Commonly, you see this situation when using shell bodies, where the individual element coordinate systems may not be aligned with each other. Some examples of averaging or interpolation operations include calculating the result value on a node shared between two elements, calculating the result value on a midside node from corner nodes, and calculating result values on paths/surfaces. Standard element-nodal results in Mechanical are always automatically evaluated in , and therefore do not face this problem.
User Defined Results Not Displayed in Worksheet
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:
Select the option on the Solution Context tab.
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.
Limitations of Vector Displays
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.