The procedure for a static analysis consists of these tasks:
See Building the Model in the Basic Analysis Guide. For more information, see the Modeling and Meshing Guide.
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.
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. For more information on the Solution Controls dialog box, see Using Special Solution Controls for Certain Types of Structural Analyses in the Basic Analysis Guide.
If you prefer not to use the Solution Controls dialog, you can specify solution controls using the standard set of Mechanical APDL solution commands (see SOLUTION Commands in the Command Reference). GUI menu paths for all commands are listed at the end of each command description in the Command Reference, and shown in some example problems (GUI Method). Some commands cannot be accessed from a menu and must be entered in the command input area in interactive mode or via a batch file.
To access the Solution Controls dialog box, select menu path . 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 click the button or find the GUI menu path listed at the end of the command description in the Command Reference. For details about nonlinear options, see Performing a Nonlinear Static Analysis.
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 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 the table below. 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 button.
Table 2.1: Basic Tab Options
| Option | For 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).
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.
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 button.
Table 2.2: Sol'n Options Tab Options
| Option | For 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)
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 button.
Table 2.3: Nonlinear Tab Options
| Option | For more information about this option, see the following section(s) in the Structural Analysis Guide: |
|---|---|
| Activate line search (LNSRCH) | |
| Activate a predictor on the degree-of-freedom 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) |
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 button.
Table 2.4: Advanced NL Tab Options
| Option | For 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) |
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.
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. For a theoretical description of stress stiffening, see Stress Stiffening in the Theory Reference.
Use the Newton-Raphson option (NROPT) 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
Issue PSTRES 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.
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.
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 (LUMPM)
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.
This load step option is used for thermal strain calculations.
To define the reference temperature, issue TREF. To define a
material-dependent reference temperature, issue
MP,REFT,CO.
To specify harmonic loading, issue the MODE command. This load step option is used for axisymmetric harmonic elements that have nonaxisymmetric loading capability (such as PLANE25).
This nonlinear load step option (CUTCONTROL) specifies the creep criterion for automatic time stepping.
Use this load step option (OUTPR) to include any results data on the output file (Jobname.out).
Caution: Proper use of multiple OUTPR commands can sometimes be tricky. See Setting Output Controls in the Basic Analysis Guide for more information about how to use the command.
Use this load step option (ERESX) to review element integration point results by copying them to the nodes instead of extrapolating them (default when no material nonlinearities are present).
After you set the desired solution options, you are ready to apply loads to the model.
All of the following load types are applicable in a static analysis.
These are degree-of-freedom 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.
These are degree-of-freedom 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.
These are concentrated loads usually specified on the model exterior. The directions implied by the labels are in the nodal coordinate system.
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).
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.
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.
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 via Tabular Input) 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 Type | Category | For details on commands for defining these loads, see... |
|---|---|---|
| Displacement (UX, UY, UZ, ROTX, ROTY, ROTZ) | Constraints | Degree-of-Freedom Constraints in the Basic Analysis Guide |
| Velocities (VELX, VELY, VELZ, OMGX, OMGY, OMGZ) | Constraints | Degree-of-Freedom Constraints in the Basic Analysis Guide |
| Force, Moment (FX, FY, FZ, MX, MY, MZ) | Forces | Forces (Concentrated Loads) in the Basic Analysis Guide |
| Pressure (PRES) | Surface Loads | Surface Loads in the Basic Analysis Guide |
| Temperature (TEMP), Fluence (FLUE) | Body Loads | Applying Body Loads in the Basic Analysis Guide |
| Gravity, Spinning, and so on | Inertia Loads | Applying Inertia Loads in the Basic Analysis Guide |
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 more information about using tabular boundary conditions and a complete list of primary variables, see Applying Loads Using Tabular Input 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, see Tabular Input via Table Array Parameters in the Ansys Parametric Design Language Guide.
You can use a static analysis to perform inertia relief calculations (IRLF command) that compute the accelerations to exactly counterbalance the applied loads, thus simulating a minimally constrained structure.
For details on the model requirements, commands used, and inertia relief output see Including Inertia Relief Calculations in the Basic Analysis Guide. For a theoretical discussion, see Inertia Relief in the Theory Reference.
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.
You are now ready to solve the analysis.
Save a backup copy of the database to a named file (SAVE). You can then retrieve your model by reentering the Mechanical APDL program and issuing RESUME.
Start solution calculations (SOLVE).
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.)
Leave the SOLUTION processor (FINISH).
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
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.
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.
Read in the database from the database file (RESUME).
Read in the desired set of results using the SET command. 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.)
Perform the necessary POST1 operations. Typical static analysis POST1 operations are explained below.
Option: Display Deformed Shape
Use the PLDISP command to display a 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.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. You can list the sum of all nodal forces and moments for a selected set of nodes. Select a set of nodes and issue FSUM to list the total force acting on selected nodes. You can also check the total force and total moment at each selected node (NFORCE). For a body in equilibrium, the total load is zero at all nodes except where an applied load or reaction load exists.
The FORCE command 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). 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. 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). 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...).
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.
Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. 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 to not average results across different materials and/or different shell thicknesses.
Option: Vector Displays
Use PLVECT to view vector displays and PRVECT to view vector listings.
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 commands like PRNSOL, PRESOL, and PRRSOL to produce tabular listings of nodal results, element results, and reaction data, respectively.
Use the NSORT and ESORT commands to sort the data before listing them.
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.