3.2. Solution Output

Solution output is written to the:

The output file is viewable via the GUI. The database and results file data can be postprocessed.

The following solution-output topics are available:

3.2.1. Output File Contents

The output file contains the nodal degree-of-freedom solution, nodal and reaction loads, and the element solutions, depending on the OUTPR settings.

The element solutions are the solution values at the integration points or centroid. They are controlled by KEYOPTs in certain elements.

3.2.2. Results File and Database Contents

The results file contains data for all requested (OUTRES) solutions, or load steps. In POST1, the SET command identifies the load step that you intend to postprocess.

Results items for area and volume elements are generally retrieved from the database via standard results output commands (such as PRNSOL, PLNSOL, PRESOL, and PLESOL).

The labels on these commands correspond to the labels shown in the input and output description tables for each element. For example, postprocessing the stress in the material x direction (typically labeled SX) is identified as item S and component X on the postprocessing commands. Coordinate locations XC, YC, ZC are identified as item CENT and component X, Y, or Z.

Only items shown both on the given results command and in the element input/output tables are available for use with that command. (An exception is EPTO, the total strain, which is available for all structural solid and shell elements even though it is not shown in the output description tables for those elements.)

Generic labels do not exist for some results data, such as integration point data, all derived data for structural line elements (such as spars, beams, and pipes) and contact elements, all derived data for thermal line elements, and layer data for layered elements. Instead, a sequence number identifies those items.

3.2.3. Element Solution

The element output items (and their definitions) are shown along with the element type description. Not all of the items shown in the output table will appear at all times for the element. Normally, items not appearing are either not applicable to the solution or have all zero results and are suppressed to save space. However, except for the coupled-field elements PLANE223, SOLID226, and SOLID227, coupled-field forces appear if they are computed to be zero. The output is, in some cases, dependent on the input. For example, for thermal elements accepting either surface convection (CONV) or nodal heat flux (HFLUX), the output will be either in terms of convection or heat flux. Most of the output items shown appear in the element solution listing. Some items do not appear in the solution listing but are written to the results file.

Most elements have two tables which describe the output data and ways to access that data for the element. These tables are the "Element Output Definitions" table and the "Item and Sequence Numbers" tables used for accessing data through the ETABLE and ESOL commands.

Stresses and strains are two primary element solution quantities in structural elements used for stress analysis. Current-technology elements output Cauchy stresses, and logarithmic strains in large deflection analysis (NLGEOM,ON) or engineering strains in a small-deflection analysis (NLGEOM,OFF). Stresses and strains are directly evaluated at element integrations points, and may be extrapolated to element nodes or averaged at element centroid for output. Generalized stresses and strains, such as linearized stresses, forces, moments, and curvature changes, are available in beam, pipe, elbow, and shell elements. The Element Output Definitions Table

The first table, "Element Output Definitions," describes possible output for the element. In addition, this table outlines which data are available for solution printout (Jobname.OUT and/or display to the terminal), and which data are available on the results file (Jobname.RST, Jobname.RTH, Jobname.RMG, etc.). Only the data which you request with the solution commands (OUTPR and OUTRES) are included in printout and on the results file, respectively.

As an added convenience, items in the table which are available via the Component Name method of the ETABLE command are identified by special notation (:) included in the output label. ( See The General Postprocessor (POST1) in the Mechanical APDL Basic Analysis Guide for more information.) The label portion before the colon corresponds to the Item field on the ETABLE command, and the portion after the colon corresponds to the Comp field. For example, S:EQV is defined as equivalent stress, and the ETABLE command for accessing this data would be:


where ABC is a user-defined label for future identification on listings and displays. Other data having labels without colons can be accessed through the Sequence Number method, discussed with the "Item and Sequence Number" tables below.

In some cases there is more than one label which can be used after the colon, in which case they are listed and separated by commas. The Definition column defines each label and, in some instances, also lists the label used on the printout, if different. The O column indicates those items which are written to the output window and/or the output file. The R column indicates items which are written to the results file and which can be obtained in postprocessing; if an item is not marked in the R column, it cannot be stored in the "element table." The Item and Sequence Number Table

Many elements also have a table, or set of tables, that list the Item and sequence number required for data access using the Sequence Number method of the ETABLE command. (See The General Postprocessor (POST1) in the Mechanical APDL Basic Analysis Guide for an example.)

The number of columns in each table and the number of tables per element vary depending on the type of data available and the number of locations on the element where data was calculated.

See Table 182.2: PLANE182 Item and Sequence Numbers for a sample item and sequence number table. Items listed as SMISC refer to summable miscellaneous items, while NMISC refers to non-summable miscellaneous items. Surface Loads

Pressure output for structural elements shows the input pressures expanded to the element's full linearly or bilinearly varying load capability.

See the SF, SFE, and SFBEAM commands for pressure input. Beam elements which allow an offset from the node on the SFBEAM command an have additional output labeled OFFST.

To save space, pressure output is often omitted when values are zero. Similarly, other surface load items (such as convection (CONV) and heat flux (HFLUX)), and body load input items (such as temperature (TEMP), fluence (FLUE), and heat generation (HGEN)), are often omitted when the values are zero (or, for temperatures, when the T-TREF values are zero).

To save space, surface output is often omitted when all values are zero.

For output of ocean-loading information on supported element types, see the OCTYPE and OCDATA commands. Integration Point Solution (Output Listing Only)

Integration point output is available in the output listing with most current-technology elements. The location of the integration point is updated if large deflections are used. See the element descriptions in the Mechanical APDL Theory Reference for details about integration point locations and output. Also the ERESX command may be used to request integration point data to be written as nodal data on the results file. Centroidal Solution (Output Listing Only)

Output (such as stress, strain, and temperature) in the output listing is given at the centroid (or near center) of certain elements. The location of the centroid is updated if large deflections are used.

The output quantities are calculated as the average of the integration point values. The component output directions for vector quantities correspond to the input material directions which, in turn, are a function of the element coordinate system. For example, the SX stress is in the same direction as EX.

In postprocessing, the ETABLE command can calculate the centroidal solution of each element from its nodal values. Surface Solution

Surface output is available in the output on certain free surfaces of solid elements. A free surface is a surface not connected to any other element and not having any degree-of-freedom constraint or nodal force load on the surface.

Surface Output Limitations

The following limitations apply to surface output:

  • Not valid on surfaces which are not free or for elements having nonlinear material properties

  • Not valid for layered solids

  • Not valid for generalized plane strain

  • Not valid for elements deactivated (EKILL) and then reactivated (EALIVE)

  • Does not include large-strain effects

The surface output is automatically suppressed if the element has nonlinear material properties. Surface calculations are of the same accuracy as the displacement calculations. Values are not extrapolated to the surface from the integration points but are calculated from the nodal displacements, face load, and the material property relationships. Transverse surface shear stresses are assumed to be zero. The surface normal stress is set equal to the surface pressure. Surface output should not be requested on condensed faces or on the zero-radius face (center line) of an axisymmetric model.

For 3-D solid elements, the face coordinate system has the x-axis in the same general direction as the first two nodes of the face, as defined with pressure loading. The exact direction of the x-axis is on the line connecting the midside nodes or midpoints of the two opposite edges. The y-axis is normal to the x-axis, in the plane of the face.

The following table lists output available via the ETABLE command using the Sequence Number method (Item = SURF). See the appropriate table in the individual element descriptions for definitions of the output quantities.

Table 3.3:  Output Available via ETABLE

Element Dimensionality
snum 3-D 2-D Axisymm
1400SSH [1]

  1. Axiharmonic only

If an additional face has surface output requested, then snum 1-19 are repeated as snum 20-38. Element Nodal Solution

The term element nodal means element data reported for each element at its nodes. This type of output is available for 2-D and 3-D solid elements, shell elements, and various other elements.

Element nodal data consist of the element derived data (such as strains, stresses, fluxes, and gradients) evaluated at each of the element's nodes. These data are usually calculated at the interior integration points and then extrapolated to the nodes.

Exceptions occur if an element has active (nonzero) plasticity, creep, or swelling at an integration point or if ERESX,NO is input. In such cases the nodal solution is the value at the integration point nearest the node.

Output is usually in the element coordinate system. Averaging of the nodal data from adjacent elements is done within the POST1 postprocessor. Element Nodal Loads

Element nodal loads refer to an element's loads (forces) acting on each of its nodes. They are printed out at the end of each element output in the nodal coordinate system and are labeled as static loads.

If the problem is dynamic, the damping loads and inertia loads are also printed.

You can control the output of element nodal loads via the OUTPR,NLOAD command (for printed output) and the OUTRES,NLOAD command (for results file output).

Element nodal loads relate to the reaction solution in the following way: the sum of the static, damping, and inertia loads at a particular degree of freedom, summed over all elements connected to that degree of freedom, plus the applied nodal load (F or FK command), is equal to the negative of the reaction solution at that same degree of freedom. Nonlinear Solutions

For information about nonlinear solutions due to material nonlinearities, see Structures with Material Nonlinearities in the Mechanical APDL Theory Reference.

Nonlinear strain data (EPPL, EPCR, EPSW, etc.) are always the value from the nearest integration point.

If creep is present, stresses are computed after the plasticity correction but before the creep correction.

Elastic strains are printed after any creep corrections. 2-D and Axisymmetric Solutions

A 2-D solid analysis is based upon a per-unit-of-depth calculation, and all appropriate output data are on a per-unit-of-depth basis. Many 2-D solids, however, allow an option to specify the depth (thickness).

An axisymmetric analysis is based on 360°. Calculation and all appropriate output data are on a full 360° basis. In particular, the total forces for the 360° model are output for an axisymmetric structural analysis and the total convection heat flow for the 360° model is output for an axisymmetric thermal analysis.

For axisymmetric analyses, the X, Y, Z, and XY stresses and strains correspond to the radial, axial, hoop, and in-plane shear stresses and strains, respectively. The global Y axis must be the axis of symmetry, and the structure should be modeled in the +X quadrants. Member Force Solution

Member force output is available with most structural line elements. The listing of this output is activated via a KEYOPT described with the element and is in addition to the nodal load output.

Member forces are in the element coordinate system and the components correspond to the degrees of freedom available with the element. Failure Criteria

Failure criteria are commonly used for determining the damage initiation in orthotropic materials. Based on various assumptions on the material damage mechanism, failure criteria are usually formulated with functions of element solution (stresses or strains) and material strength limits.

Two types of failure criteria results are possible: those that are available during any type of analysis, and those that are available only during a progressive failure damage analysis. Failure criteria results are accessible via standard postprocessing output commands (PLESOL, PRESOL, PLNSOL, and PRNSOL) and the ETABLE command:

  • Available during any type of analysis (accessible via the FAIL item)

    These failure criteria are computed on the fly when requested, using stored element strains and stresses in the result file. This type of failure criteria are suitable for determining whether and where the material damage may first occur. If the material is damaged, the stresses used for this calculation are calculated from the strains and the damaged material stiffnesses.
  • Available only during a progressive failure damage analysis (accessible via the PFC item)

    These failure criteria are calculated from element strains and effective stresses (stresses that would occur if the material were undamaged) during solution and stored in the result file. They indicate whether the material damage may be expected to continue.

For more information, see Failure Criteria in the Mechanical APDL Theory Reference and Specifying Failure Criteria for Composites in the Mechanical APDL Structural Analysis Guide. Linearized Stresses

Linearized stresses, including axial, membrane, bending, and peak stresses, are available in beam, pipe, elbow, shell, and solid shell elements. These quantities are generally output as SMISC records (accessible via the ETABLE and ESOL postprocessing commands).

The stress linearization procedure for the solid shell element (SOLSH190) and shell elements (SHELL181, SHELL281, SHELL208, and SHELL209) is defined in ASME Boiler and Pressure Vessel Code (2007 Section VIII, Division 2, Annex 5.A). For the linearization procedure used for other elements, see the documentation for those individual elements.

3.2.4. Nodal Solution

The nodal solution from an analysis consists of:

  • the degree-of-freedom solution, such as nodal displacements, temperatures, and pressures

  • the reaction solution calculated at constrained nodes - forces at displacement constraints, heat flows at temperature degree-of-freedom constraints, fluid flows at pressure degree-of-freedom constraints, and so on.

The degree-of-freedom solution is calculated for all active degrees of freedom in the model, which are determined by the union of all degree-of-freedom labels associated with all the active element types. It is output at all degrees of freedom that have a nonzero stiffness or conductivity and can be controlled by OUTPR,NSOL (for printed output) and OUTRES,NSOL (for results file output).

The reaction solution is calculated at all nodes that are constrained (D, DSYM, etc.). Its output can be controlled by OUTPR,RSOL and OUTRES,RSOL.

For vector degrees of freedom and corresponding reactions, the output during solution is in the nodal coordinate system. If a node was input with a rotated nodal coordinate system, the output nodal solution will also be in the rotated coordinate system. For a node with the rotation θxy = 90°, the printed UX solution will be in the nodal X direction, which in this case corresponds to the global Y direction. Rotational displacements (ROTX, ROTY, ROTZ) are output in radians, and phase angles from a harmonic analysis are output in degrees.

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