2.2. Performing a Static Analysis

The procedure for a static analysis consists of these tasks:

  1. Build the Model

  2. Set Solution Controls

  3. Set Additional Solution Options

  4. Apply the Loads

  5. Solve the Analysis

  6. Review the Results

2.2.1. Build the Model

See Building the Model in the Basic Analysis Guide. For more information, see the Modeling and Meshing Guide.

2.2.1.1. Hints and Tips

When performing a static analysis:

  • You can use both linear and nonlinear structural elements.

  • Material properties can be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent.

    • You must define stiffness in some form (for example, Young's modulus (EX), hyperelastic coefficients, and so on).

    • For inertia loads (such as gravity), you must define the data required for mass calculations, such as density (DENS).

    • For thermal loads (temperatures), you must define the coefficient of thermal expansion (ALPX).

  • Note the following about mesh density:

    • Regions where stresses or strains vary rapidly (usually areas of interest) require a relatively finer mesh than regions where stresses or strains are nearly constant (within an element).

    • While considering the influence of nonlinearities, remember that the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients.

2.2.2. Set Solution Controls

Setting solution controls involves defining the analysis type and common analysis options for an analysis, as well as specifying load step options for it. When you are doing a structural static analysis, you can take advantage of a streamlined solution interface (called the Solution Controls dialog) for setting these options. The Solution Controls dialog box provides default settings that will work well for many structural static analyses, so you may need to set only a few, if any, options.

If you prefer not to use the Solution Controls dialog, you can set solution controls for your analysis using the standard set of Mechanical APDL solution commands and the standard corresponding menu paths (Main Menu> Solution> Unabridged Menu> option). For a general overview of the Solution Controls dialog box, see Using Special Solution Controls for Certain Types of Structural Analyses in the Basic Analysis Guide.

2.2.2.1. Access the Solution Controls Dialog Box

To access the Solution Controls dialog box, select menu path Main Menu> Solution> Analysis Type> Sol'n Controls. The following sections provide brief descriptions of the options that appear on each tab of the dialog box. For details about how to set these options, select the tab that you are interested in (from within the Mechanical APDL program), and then click the Help button. Nonlinear Structural Analysis also contains details about the nonlinear options introduced in this chapter.

2.2.2.2. Using the Basic Tab

The Basic tab is active when you access the dialog box.

The controls that appear on the Basic tab provide the minimum amount of data that Mechanical APDL needs for the analysis. When you are satisfied with the settings on the Basic tab, you do not need to progress through the remaining tabs unless you want to adjust the default settings for the more advanced controls. When you click OK on any tab of the dialog box, the settings are applied to the database and the dialog box closes.

You can use the Basic tab to set the options listed in Table 2.1: Basic Tab Options. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Basic tab, and click the Help button.

Table 2.1:  Basic Tab Options

OptionFor more information on this option, see:
Specify analysis type [ANTYPE, NLGEOM]
Control time settings, including: time at end of load step [TIME], automatic time stepping [AUTOTS], and number of substeps to be taken in a load step [NSUBST or DELTIM]
Specify solution data to write to database [OUTRES]

Special considerations for setting these options in a static analysis include:

  • When setting ANTYPE and NLGEOM, select Small Displacement Static if you are performing a new analysis and you want to ignore large deformation effects such as large deflection, large rotation, and large strain. Select Large Displacement Static if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem). Select Restart Current Analysis if you want to restart a failed nonlinear analysis, or if you have previously completed a static analysis and you want to specify additional loads.

  • When setting TIME, remember that this load step option specifies time at the end of the load step. The default value is 1.0 for the first load step. For subsequent load steps, the default is 1.0 plus the time specified for the previous load step. Although time has no physical meaning in a static analysis (except in the case of creep, viscoplasticity, or other rate-dependent material behavior), it is used as a convenient way of referring to load steps and substeps (see Loading in the Basic Analysis Guide).

2.2.2.3. The Transient Tab

The Transient tab contains transient analysis controls; it is available only if you select a transient analysis and remains grayed out when you select a static analysis. For these reasons, it is not described here.

2.2.2.4. Using the Sol'n Options Tab

You can use the Sol'n Options tab to set the options listed in Table 2.2: Sol'n Options Tab Options. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Sol'n Options tab, and click the Help button.

Table 2.2:  Sol'n Options Tab Options

OptionFor more information about this option, see the following section(s) in the Basic Analysis Guide:
Specify equation solver [EQSLV]
Specify parameters for multiframe restart [RESCONTROL]

Special considerations for setting these options in a static analysis include:

  • When setting EQSLV, specify one of these solvers:

    • Program chosen solver (Mechanical APDL selects a solver for you, based on the physics of the problem)

    • Sparse direct solver (default for linear and nonlinear, static and full transient analyses)

    • Preconditioned Conjugate Gradient (PCG) solver (recommended for large size models, bulky structures)

    • Iterative solver (auto-select; for linear static/full transient structural or steady-state thermal analyses only; recommended)

2.2.2.5. Using the Nonlinear Tab

You can use the Nonlinear tab to set the options listed in Table 2.3: Nonlinear Tab Options. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Nonlinear tab, and click the Help button.

Table 2.3:  Nonlinear Tab Options

OptionFor more information about this option, see the following section(s) in the Structural Analysis Guide:
Activate line search [LNSRCH]
Activate a predictor on the DOF solution [PRED]
Specify the maximum number of iterations allowed per substep [NEQIT]
Specify whether you want to include creep calculation [RATE]
Set convergence criteria [CNVTOL]
Control bisections [CUTCONTROL]

2.2.2.6. Using the Advanced NL Tab

You can use the Advanced NL tab to set the options listed in Table 2.4: Advanced NL Tab Options. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Advanced NL tab, and click the Help button.

Table 2.4:  Advanced NL Tab Options

OptionFor more information about this option, see the following section(s) in the Structural Analysis Guide:
Specify analysis termination criteria [NCNV]
Control activation and termination of the arc-length method [ARCLEN, ARCTRM]

2.2.3. Set Additional Solution Options

This section discusses additional options that you can set for the solution. These options do not appear on the Solution Controls dialog box because they are used very infrequently, and their default settings rarely need to be changed. Mechanical APDL menu paths are provided in this section to help you access these options for those cases where you want to override the program defaults.

Many of the options that appear in this section are nonlinear options, and are described further in Nonlinear Structural Analysis.

2.2.3.1. Stress Stiffening Effects

Most element types include stress stiffening effects automatically when NLGEOM is ON. To determine whether an element includes stress stiffening, refer to the appropriate element description in the Element Reference.

2.2.3.2. Newton-Raphson Option

Use this analysis option only in a nonlinear analysis. This option specifies how often the tangent matrix is updated during solution. You can specify one of these values:

  • Program-chosen (default)

  • Full

  • Modified

  • Initial stiffness

  • Full with unsymmetric matrix

Command(s): NROPT
GUI: Main Menu> Solution> Unabridged Menu> Analysis Options

2.2.3.3. Prestress Effects Calculation

Use this analysis option to perform a prestressed analysis on the same model when the base analysis is linear (such as a prestressed modal analysis). The prestress effects calculation controls the generation of the stress stiffness matrix. The default for the prestress effects calculation is OFF.

Command(s): PSTRES
GUI: Main Menu> Solution> Unabridged Menu> Analysis Options

If the base analysis is nonlinear, the linear perturbation procedure is recommended. In this case, the prestress effects are automatically included and PSTRES is not needed.

2.2.3.4. Mass Matrix Formulation

Use this analysis option if you plan to apply inertial loads on the structure (such as gravity and spinning loads). You can specify one of these values:

  • Default (depends on element type)

  • Lumped mass approximation


Note:  For a static analysis, the mass matrix formulation you use does not significantly affect the solution accuracy (assuming that the mesh is fine enough). However, if you want to do a prestressed dynamic analysis on the same model, the choice of mass matrix formulation may be important; see the appropriate dynamic analysis section for recommendations.

Command(s): LUMPM
GUI: Main Menu> Solution> Unabridged Menu> Analysis Options

2.2.3.5. Reference Temperature

This load step option is used for thermal strain calculations. Reference temperature can be made material-dependent with the MP,REFT command.

Command(s): TREF
GUI: Main Menu> Solution> Load Step Opts> Other> Reference Temp

2.2.3.6. Mode Number

This load step option is used for axisymmetric harmonic elements.

Command(s): MODE
GUI: Main Menu> Solution> Load Step Opts> Other> For Harmonic Ele

2.2.3.7. Creep Criteria

This nonlinear load step option specifies the creep criterion for automatic time stepping.

Command(s): CRPLIM
GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Creep Criterion

2.2.3.8. Printed Output

Use this load step option to include any results data on the output file (Jobname.OUT).

Command(s): OUTPR
GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Solu Printout

Caution:  Proper use of multiple OUTPR commands can sometimes be a little tricky. See Setting Output Controls in the Basic Analysis Guide for more information on how to use this command.


2.2.3.9. Extrapolation of Results

Use this load step option to review element integration point results by copying them to the nodes instead of extrapolating them (default when no material nonlinearities are present).

Command(s): ERESX
GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Output Ctrls> Integration Pt

2.2.4. Apply the Loads

After you set the desired solution options, you are ready to apply loads to the model.

2.2.4.1. Load Types

All of the following load types are applicable in a static analysis.

2.2.4.1.1. Displacements (UX, UY, UZ, ROTX, ROTY, ROTZ)

These are DOF constraints (D command) usually specified at model boundaries to define rigid support points. They can also indicate symmetry boundary conditions and points of known motion. The directions implied by the labels are in the nodal coordinate system.

2.2.4.1.2. Velocities (VELX, VELY, VELZ, OMGX, OMGY, OMGZ)

These are DOF constraints (D command) to specify the velocity field. The directions implied by the velocity load labels are in the nodal coordinate system.

For rotating structure applications using the CORIOLIS command, the nodal velocities are specified using IC and ICROTATE. See the Rotordynamic Analysis Guide for more information.

For brake squeal analysis, the CMROTATE command is used to specify the nodal velocities at the frictional contact interfaces. See Forced Frictional Sliding Using Velocity Input in the Contact Technology Guide for more information.

2.2.4.1.3. Forces (FX, FY, FZ) and Moments (MX, MY, MZ)

These are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system.

2.2.4.1.4. Pressures (PRES)

These are surface loads, also usually applied on the model exterior. Positive values of pressure act towards the element face (resulting in a compressive effect).

2.2.4.1.5. Temperatures (TEMP)

These are applied to study the effects of thermal expansion or contraction (that is, thermal stresses). The coefficient of thermal expansion must be defined if thermal strains are to be calculated. You can read in temperatures from a thermal analysis [LDREAD], or you can specify temperatures directly, using the BF family of commands.

2.2.4.1.6. Fluences (FLUE)

These are applied to study the effects of swelling (material enlargement due to neutron bombardment or other causes) or creep. They are used only if you input a swelling or creep equation.

2.2.4.1.7. Gravity, Spinning, Etc.

These are inertia loads that affect the entire structure. Density (or mass in some form) must be defined if inertia effects are to be included.

2.2.4.2. Apply Loads to the Model

Except for inertia loads (which are independent of the model) and velocity loads, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). You can also apply boundary conditions via TABLE type array parameters (see Applying Loads Using TABLE Type Array Parameters) or as function boundary conditions (see Using the Function Tool).

Table 2.5: Loads Applicable in a Static Analysis summarizes the loads applicable to a static analysis. In an analysis, loads can be applied, removed, operated on, or listed.

Table 2.5:  Loads Applicable in a Static Analysis

Load TypeCategoryFor details on commands and menu paths for defining these loads, see...
Displacement (UX, UY, UZ, ROTX, ROTY, ROTZ)ConstraintsDegree-of-Freedom Constraints in the Basic Analysis Guide
Velocities (VELX, VELY, VELZ, OMGX, OMGY, OMGZ)ConstraintsDegree-of-Freedom Constraints in the Basic Analysis Guide
Force, Moment (FX, FY, FZ, MX, MY, MZ)ForcesForces (Concentrated Loads) in the Basic Analysis Guide
Pressure (PRES)Surface LoadsSurface Loads in the Basic Analysis Guide
Temperature (TEMP), Fluence (FLUE)Body LoadsApplying Body Loads in the Basic Analysis Guide
Gravity, Spinning, and so onInertia LoadsApplying Inertia Loads in the Basic Analysis Guide

2.2.4.2.1. Applying Loads Using TABLE Type Array Parameters

You can also apply loads using TABLE type array parameters. In a structural analysis, typical primary variables are TIME, TEMP, and location (X, Y, Z). For details on using tabular boundary conditions and a complete list of primary variables, see Applying Loads Using TABLE Type Array Parameters in the Basic Analysis Guide.

When defining the table, TIME must be in ascending order in the table index (as in any table array).

You can define a table array parameter via command or interactively. For more information on defining table array parameters, see the ANSYS Parametric Design Language Guide.

2.2.4.3. Calculating Inertia Relief

You can use a static analysis to perform inertia relief calculations, which calculate the accelerations that will counterbalance the applied loads. You can think of inertia relief as an equivalent free-body analysis.

Your model should meet the following requirements:

  • The model should not contain axisymmetric or generalized plane strain elements, or nonlinearities. Models with a mixture of 2-D and 3-D element types are not recommended.

  • Symmetry models are not valid for inertia relief analysis.

  • Data required for mass calculations (such as density) must be specified.

  • Specify only the minimum number of displacement constraints - those required to prevent rigid-body motion. Three constraints (or fewer, depending on the element type) are necessary for 2-D models and six (or fewer) are necessary for 3-D models. Additional constraints, such as those required to impose symmetry conditions, are permitted, but check for zero reaction forces at all the constraints to make sure that the model is not overconstrained for inertia relief.

  • The loads for which inertia relief calculations are desired should be applied.

Issue the IRLF command before the SOLVE command as part of the inertia load commands.

Command(s): IRLF,1
GUI: Main Menu> Solution> Load Step Opts> Other> Inertia Relief

Inertia Relief for Substructures

For substructures, inertia relief calculations (MATRIX50) use the equations described in Inertia Relief in the Mechanical APDL Theory Reference. Mechanical APDL obtains the mass matrix of a substructure via matrix reduction to condense it to the master nodes (MASTER). The inertia relief calculations in a substructure are therefore consistent with the reduced mass contribution at the master nodes.

The IRLF command has no effect in the generation pass of a substructure. If you intend to perform inertia relief calculations on a substructure, do not apply DOF constraints (D) on the substructure during its generation pass; instead, apply them during the use pass. (Otherwise, the substructure reduction logic condenses out the mass associated with the constrained DOFs in the generation pass, and the inertia relief calculations in the use pass of the substructure reflect the condensed mass distribution.)

In the expansion pass, precalculation of masses for summary printout (IRLF,-1) occurs only on elements that are part of the substructure.

2.2.4.3.1. Inertia Relief Output

Use the IRLIST command to print the output from inertia relief calculations. This output consists of the translational and rotational accelerations required to balance the applied loads and can be used by other programs to perform kinematics studies. The summary listing of mass and moments of inertia (produced during solution) is accurate, not approximate. The reaction forces at the constraints will be zero because the calculated inertia forces balance the applied forces.

Inertia relief output is stored in the database rather than in the results file (Jobname.RST). When you issue IRLIST, Mechanical APDL retrieves the information from the database, which contains the inertia relief output from the most recent solution [SOLVE].

Command(s): IRLIST
GUI: No GUI equivalent.
2.2.4.3.2. Using a Macro to Perform Inertia Relief Calculations

If you need to do inertia relief calculations frequently, you can write a macro containing the above commands. Macros are described in the ANSYS Parametric Design Language Guide.

2.2.5. Solve the Analysis

You are now ready to solve the analysis.

  1. Save a backup copy of the database to a named file. You can then retrieve your model by reentering the Mechanical APDL program and issuing RESUME.

    Command(s): SAVE
    GUI: Utility Menu> File> Save as
  2. Start solution calculations.

    Command(s): SOLVE
    GUI: Main Menu> Solution> Solve> Current LS
  3. If you want the analysis to include additional loading conditions (that is, multiple load steps), you will need to repeat the process of applying loads, specifying load step options, saving, and solving for each load step. (Other methods for handling multiple load steps are described in Loading in the Basic Analysis Guide.)

  4. Leave SOLUTION.

    Command(s): FINISH
    GUI: Close the Solution menu.

2.2.6. Review the Results

Results from a static analysis are written to the structural results file, Jobname.RST. They consist of the following data:

  • Primary data:

    • Nodal displacements (UX, UY, UZ, ROTX, ROTY, ROTZ)

  • Derived data:

    • Nodal and element stresses

    • Nodal and element strains

    • Element forces

    • Nodal reaction forces

    • and so on

2.2.6.1. Postprocessors

You can review these results using POST1, the general postprocessor, and POST26, the time-history processor.

  • POST1 is used to review results over the entire model at specific substeps (time-points). Some typical POST1 operations are explained below.

  • POST26 is used in nonlinear static analyses to track specific result items over the applied load history. See Nonlinear Structural Analysis for the use of POST26 in a nonlinear static analysis. For a complete description of all postprocessing functions, see An Overview of Postprocessing in the Basic Analysis Guide.

2.2.6.2. Hints and Tips

  • To review results in POST1 or POST26, the database must contain the same model for which the solution was calculated.

  • The results file (Jobname.RST) must be available.

2.2.6.3. Reviewing Results Data

  1. Read in the database from the database file.

    Command(s): RESUME
    GUI: Utility Menu> File> Resume from
  2. Read in the desired set of results. Identify the data set by load step and substep numbers or by time. (If you specify a time value for which no results are available, the Mechanical APDL program performs linear interpolation on all the data to calculate the results at that time.)

    Command(s): SET
    GUI: Main Menu> General Postproc> Read Results> By Load Step
  3. Perform the necessary POST1 operations. Typical static analysis POST1 operations are explained below.

2.2.6.4. Typical Postprocessing Operations

Option: Display Deformed Shape

Use the PLDISP command to display a deformed shape (Main Menu> General Postproc> Plot Results> Deformed Shape). The KUND field on PLDISP gives you the option of overlaying the undeformed shape on the display.

Option: List Reaction Forces and Moments

The PRRSOL command lists reaction forces and moments at the constrained nodes (Main Menu> General Postproc> List Results> Reaction Solu).

To display reaction forces, issue /PBC,RFOR,,1 and then request a node or element display [NPLOT or EPLOT]. (Use RMOM instead of RFOR for reaction moments.)

Option: List Nodal Forces and Moments

Use the PRESOL,F (or M) command to list nodal forces and moments (Main Menu> General Postproc> List Results> Element Solution).

You can list the sum of all nodal forces and moments for a selected set of nodes. Select a set of nodes and use this feature to find out the total force acting on those nodes:

Command(s): FSUM
GUI: Main Menu> General Postproc> Nodal Calcs> Total Force Sum

You can also check the total force and total moment at each selected node. For a body in equilibrium, the total load is zero at all nodes except where an applied load or reaction load exists:

Command(s): NFORCE
GUI: Main Menu> General Postproc> Nodal Calcs> Sum @ Each Node

The FORCE command (Main Menu> General Postproc> Options for Outp) dictates which component of the forces is being reviewed:

  • Total (default)

  • Static component

  • Damping component

  • Inertia component

For a body in equilibrium, the total load (using all FORCE components) is zero at all nodes except where an applied load or reaction load exists.

Option: Line Element Results

For line elements, such as beams, spars, and pipes, use ETABLE to gain access to derived data (stresses, strains, and so on) (Main Menu> General Postproc> Element Table> Define Table). Results data are identified by a combination of a label and a sequence number or component name on the ETABLE command. See the ETABLE discussion in The General Postprocessor (POST1) in the Basic Analysis Guide for details.

Option: Error Estimation

For linear static analyses using solid or shell elements, use the PRERR command to list the estimated solution error due to mesh discretization (Main Menu> General Postproc> List Results> Percent Error). This command calculates and lists the percent error in structural energy norm (SEPC), which represents the error relative to a particular mesh discretization.

Option: Structural Energy Error Estimation

Use PLESOL,SERR to contour the element-by-element structural energy error (SERR) (Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu). Regions of high SERR on the contour display are good candidates for mesh refinement. See Estimating Solution Error in the Basic Analysis Guide for more details about error estimation.

Option: Contour Displays

Use PLNSOL and PLESOL to contour almost any result item, such as stresses (SX, SY, SZ...), strains (EPELX, EPELY, EPELZ...), and displacements (UX, UY, UZ...) (Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu or Element Solu).

The KUND field on PLNSOL and PLESOL gives you the option of overlaying the undeformed shape on the display.

Use PLETAB and PLLS to contour element table data and line element data (Main Menu> General Postproc> Element Table> Plot Element Table and Main Menu> General Postproc> Plot Results> Contour Plot> Line Elem Res).


Caution:  Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Selecting and Components in the Basic Analysis Guide) to select elements of the same material, same shell thickness, and so on before issuing PLNSOL. Alternatively, use PowerGraphics with the AVRES command (Main Menu> General Postproc> Options for Outp) to not average results across different materials and/or different shell thicknesses.


Option: Vector Displays

Use PLVECT to view vector displays (Main Menu> General Postproc> Plot Results> Vector Plot> Predefined) and PRVECT to view vector listings (Main Menu> General Postproc> List Results> Vector Data).

Vector displays (not to be confused with vector mode) are an effective way of viewing vector quantities, such as displacement (DISP), rotation (ROT), and principal stresses (S1, S2, S3).

Option: Tabular Listings

Use these commands to produce tabular listings:

Command(s): PRNSOL (nodal results), PRESOL (element-by-element results) PRRSOL (reaction data), and so on
GUI: Main Menu> General Postproc> List Results> solution option

Use the NSORT and ESORT commands to sort the data before listing them (Main Menu> General Postproc> List Results> Sorted Listing> Sort Nodes or Sort Elems).

Other Postprocessing Capabilities

Many other postprocessing functions - mapping results onto a path, load case combinations, and so on - are available in POST1. See An Overview of Postprocessing in the Basic Analysis Guide for details.


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