Introduction
A static structural analysis determines the displacements, stresses, strains, and forces in structures or components caused by loads that do not induce significant inertia and damping effects. Steady loading and response conditions are assumed; that is, the loads and the structure's response are assumed to vary slowly with respect to time. A static structural load can be performed using the Ansys, Samcef, or ABAQUS solver. The types of loading that can be applied in a static analysis include:
Externally applied forces and pressures
Steady-state inertial forces (such as gravity or rotational velocity)
Imposed (nonzero) displacements
Temperatures (for thermal strain)
Point to Remember
Note the following for this analysis type:
A static structural analysis can be either linear or nonlinear. All types of nonlinearities are allowed - large deformations, plasticity, stress stiffening, contact (gap) elements, hyperelasticity and so on. This chapter focuses on linear static analyses, with brief references to nonlinearities. Details of how to handle nonlinearities are described in Nonlinear Controls.
When 2D geometry is used, Generalized Plane Strain is not supported for the Samcef or ABAQUS solver.
Note that available nonlinearities can differ from one solver to another.
As needed throughout the analysis, refer to the General Analysis Workflow section for an overview the general analysis workflow.
Define Engineering Data
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, hyperelastic coefficients, and so on). For inertial loads (such as Standard Earth Gravity), you must define the data required for mass calculations, such as density.
Define Part Behavior
You can define a Point Mass for this analysis type.
A "rigid" part is essentially a point mass connected to the rest of the structure via joints. Hence in a static structural analysis the only applicable loads on a rigid part are acceleration and rotational velocity loads. You can also apply loads to a rigid part via joint loads. The output from a rigid part is the overall motion of the part plus any force transferred via that part to the rest of the structure. Rigid behavior cannot be used with the Samcef or ABAQUS solver.
If your model includes nonlinearities such as large deflection or hyperelasticity, the solution time can be significant due to the iterative solution procedure. Hence you may want to simplify your model if possible. For example you may be able to represent your 3D structure as a 2-D plane stress, plane strain, or axisymmetric model or you may be able to reduce your model size through the use of symmetry or antisymmetry surfaces. Similarly if you can omit nonlinear behavior in one or more parts of your assembly without affecting results in critical regions it will be advantageous to do so.
Define Connections
This analysis supports:
Contact, joints, springs, beams, mesh connections, and end releases.
(Samcef and ABAQUS solvers only), contacts, springs, and beams are supported. Joints are not supported.
Apply Mesh Controls/Preview Mesh
Provide an adequate mesh density on contact surfaces to allow contact stresses to be distributed in a smooth fashion. Likewise, provide a mesh density adequate for resolving stresses; areas where stresses or strains are of interest require a relatively fine mesh compared to that needed for displacement or nonlinearity resolution. If you want to include nonlinearities, 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.
Establish Analysis Settings
For simple linear static analyses you typically do not need to change these settings. For more complex analyses the basic Analysis Settings include:
- Large Deflection
Large Deflection is typically needed for slender structures. Use large deflection if the transverse displacements in a slender structure are more than 10% of the thickness.
Small deflection and small strain analyses assume that displacements are small enough that the resulting stiffness changes are insignificant. Setting Large Deflection to On will take into account stiffness changes resulting from changes in element shape and orientation due to large deflection, large rotation, and large strain. Therefore the results will be more accurate. However this effect requires an iterative solution. In addition it may also need the load to be applied in small increments. Therefore, the solution may take longer to solve.
You also need to turn on large deflection if you suspect instability (buckling) in the system. Use of hyperelastic materials also requires large deflection to be turned on.
- Step Controls for Static and Transient Analyses
Step Controls are used to i) control the time step size and other solution controls and ii) create multiple steps when needed. Typically analyses that include nonlinearities such as large deflection or plasticity require control over time step sizes as outlined in the Automatic Time Stepping section. Multiple steps are required for activation/deactivation of displacement loads or pretension bolt loads. This group can be modified on a per step basis.
Note: Time Stepping is available for any solver.
- Rotordynamics Controls
Specify these properties as needed when setting up a Rotordynamic analysis.
- Output Controls
Output Controls allow you to specify the time points at which results should be available for postprocessing. In a nonlinear analysis it may be necessary to perform many solutions at intermediate load values. However i) you may not be interested in all the intermediate results and ii) writing all the results can make the results file size unwieldy. This group can be modified on a per step basis except for Stress and Strain.
- Nonlinear Controls
Nonlinear Controls allow you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control. This group can be modified on a per step basis. If you are performing a nonlinear Static Structural analysis, the Newton-Raphson Type property becomes available. This property only affects nonlinear analyses. Your selections execute the Mechanical APDL NROPT command. The default option, , allows the application to select the appropriate NROPT option or you can make a manual selection and choose , , or .
See the Help section for the NROPT command in the Mechanical APDL Command Reference for additional information about the operation of the Newton-Raphson Type property.
- Analysis Data Management
Settings enable you to save specific solution files from the Static Structural analysis for use in other analyses. You can set the Future Analysis field to Pre-Stressed Analysis if you intend to use the static structural results in a subsequent Harmonic Response, Modal, or Eigenvalue Buckling (Eigenvalue Buckling is applicable to Static Structural systems only) analysis. If you link a structural system to another analysis type in advance, the Future Analysis field defaults to Pre-Stressed Analysis. A typical example is the large tensile stress induced in a turbine blade under centrifugal load. This causes significant stiffening of the blade resulting in much higher, realistic natural frequencies in a modal analysis. More details are available in the section Define Initial Conditions.
Note: Scratch Solver Files, Save Ansys db, Solver Units, and Solver Unit System are applicable to Static Structural systems only.
Define Initial Conditions
Initial condition is not applicable for Static Structural analyses.
Apply Boundary Conditions
For a Static Structural analysis applicable loads include:
Applicable structural Supports, certain Conditions Type Boundary Conditions, as well as supported Direct FE Type Boundary Conditions are also available.
For the Samcef and ABAQUS solvers, the following loads and supports are not available: Hydrostatic Pressure, Bearing Load, Bolt Pretension, Joint Load, Interface, Motion Loads, Compression Only Support, Elastic Support.
Loads and supports vary as a function of time even in a static analysis as explained in the Role of Time in Tracking. In a static analysis, the load's magnitude could be a constant value or could vary with time as defined in a table or via a function. Details of how to apply a tabular or function load are described in Specifying Boundary Condition Magnitude. In addition, for more information about time stepping and ramped loads, see the Applying Stepped and Ramped Loads section.
Note: A static analysis can be followed by a "pre-stressed" analysis such as modal or linear (eigenvalue) buckling analysis. In this subsequent analysis the effect of stress on stiffness of the structure (stress-stiffness effect) is taken into account. If the static analysis has a pressure or force load applied on faces (3D) or edges (2D) this could result in an additional stiffness contribution called "pressure load stiffness" effect. This effect plays a significant role in linear (eigenvalue) buckling analyses. This additional effect is computed during the Eigenvalue Buckling analysis using the pressure or force value calculated at the time in the static analysis from which the perturbation occurs. See the Applying Pre-Stress Effects section for more information on this topic.
When using the Samcef or ABAQUS solver, boundary conditions are not available.
Solve
When performing a nonlinear analysis you may encounter convergence difficulties due to a number of reasons. Some examples may be initially open contact surfaces causing rigid body motion, large load increments causing non-convergence, material instabilities, or large deformations causing mesh distortion that result in element shape errors. To identify possible problem areas some tools are available under Solution Information object Details view.
Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section.
You can display contour plots of Newton-Raphson Residuals in a nonlinear static analysis. Such a capability can be useful when you experience convergence difficulties in the middle of a step, where the model has a large number of contact surfaces and other nonlinearities. When the solution diverges identifying regions of high Newton-Raphson residual forces can provide insight into possible problems.
Result Tracker (applicable to Static Structural systems only) is another useful tool that enables you to monitor displacement and energy results as the solution progresses. This is especially useful in case of structures that possibly go through convergence difficulties due to buckling instability. Result Tracker is not available to the Samcef or ABAQUS solver.
Review Results
All structural result types except frequencies are available as a result of a static structural analysis. You can use a Solution Information object to track, monitor, or diagnose problems that arise during a solution.
Once a solution is available you can contour the results or animate the results to review the response of the structure.
As a result of a nonlinear static analysis you may have a solution at several time points. You can use probes to display the variation of a result item as the load increases. An example might be large deformation analyses that result in buckling of the structure. In these cases it is also of interest to plot one result quantity (for example, displacement at a vertex) against another results item (for example, applied load). You can use the Charts feature to develop such charts.