8.6ANSYS非线性静力分析步骤帮助学习

8.6. Performing a Nonlinear Static Analysis
The procedure for performing a nonlinear static analysis consists of these tasks:
∙Build the Model
∙Set Solution Controls
∙Set Additional Solution Options
∙Apply the Loads
∙Solve the Analysis
∙Review the Results
∙Terminating a Running Job; Restarting
8.6.1. Build the Model
This step is essentially the same for both linear and nonlinear analyses, although a nonlinear analysis might include special elements or nonlinear material properties. See Using Nonlinear (Changing-Status) Elements, and Modeling Material Nonlinearities, for more details. If your analysis includes large-strain effects, your stress-strain data must be expressed in terms of true stress and true (or logarithmic) strain. For more information on building models in ANSYS, see the Modeling and Meshing Guide.
After you have created a model in ANSYS, you set solution controls (analysis type, analysis options, load step options, and so on), apply loads, and solve. A nonlinear solution will differ from a linear solution in that it often requires multiple load increments, and always requires equilibrium iterations. The general procedure for performing these tasks follows. See Sample Nonlinear Analysis (GUI Method)for a sample problem that walks you through a specific nonlinear analysis.
8.6.2. Set Solution Controls
Setting solution controls for a nonlinear analysis involves the same options and method of access (the Solution Controls dialog box) as those used for a linear structural static analysis. For a nonlinear analysis, the default settings in the Solution Controls dialog box are essentially the same settings employed by the automatic solution control method described in Running a Nonlinear Analysis in ANSYS. See the following sections in Structural Static Analysis, with exceptions noted:
∙Set Solution Controls
∙Access the Solution Controls Dialog Box
∙Using the Basic Tab
∙The Transient Tab
∙Using the Sol'n Options Tab
∙Using the Nonlinear Tab
∙Using the Advanced NL Tab
8.6.2.1. Using the Basic Tab: Special Considerations
Special considerations for setting these options in a nonlinear structural static analysis include:
∙When setting ANTYPE and NLGEOM, choose Large Displacement Static if you are performing a new analysis. (But, keep in mind that not all nonlinear analyses will produce large deformations. See Using Geometric Nonlinearities for further discussion of large
deformations.) Choose Restart Current Analysis if you want to
restart a failed nonlinear analysis. You cannot change this setting after the first load step (that is, after you issue your first SOLVE
command). You will usually choose to do a new analysis, rather than
a restart. Restarts are discussed in the Basic Analysis Guide.
∙When working with time settings, remember that these options can be changed at any load step. See "Loading" in the Basic Analysis Guide for more information on these options. Advanced
time/frequency options, in addition to those available on the
Solution Controls dialog box, are discussed in Advanced Load Step Options You Can Set on the Solution Controls Dialog Box.
A nonlinear analysis requires multiple substeps (or time steps; the
two terms are equivalent) within each load step so that ANSYS can apply the specified loads gradually and obtain an accurate solution.
The NSUBST and DELTIM commands both achieve the same effect
(establishing a load step's starting, minimum, and maximum step
size), but by reciprocal means. NSUBST defines the number of
substeps to be taken within a load step, whereas DELTIM defines the time step size explicitly. If automatic time stepping is off
[AUTOTS], then the starting substep size is used throughout the load step.
∙OUTRES controls the data on the results file (Jobname.RST). By default, only the last substep is written to the results file in
a nonlinear analysis.
Only 1000 results sets (substeps) can be written to the results file, but you can use the command /CONFIG,NRES to increase the limit (see the Basic Analysis Guide).
8.6.2.2. Advanced Analysis Options分析选项You Can Set on the Solution Controls Dialog Box
The following sections provide more detail about some of the advanced analysis options that you can set on the Solution Controls dialog box.
8.6.2.2.1. Equation Solver
ANSYS' automatic solution control activates the sparse direct solver (EQSLV,SPARSE) for most cases. Other options include the PCG and ICCG solvers. For applications using solid elements (for example, SOLID92 or SOLID45), the PCG solver may be faster, especially for 3-D modeling.
If using the PCG solver, you may be able to reduce memory usage via the MSAVE command. The MSAVE command triggers an element-by-element approach for the parts of the model that use SOLID45, SOLID92, SOLID95, SOLID185, SOLID186, SOLID187SOLID272, SOLID273, and/or SOLID285 elements with linear material properties. (MSAVE does not support the layered option of the SOLID185 and SOLID186 elements.) To use MSAVE, you must be performing a static or a modal analysis with PCG Lanczos enabled. When using SOLID185, SOLID186, and/or SOLID187, only small strain (NLGEOM,OFF) analyses are allowed. Other parts of the model that do not meet the above criteria are solved using global assembly for the stiffness matrix. MSAVE,ON can result in a memory savings of up to 70 percent for the part of the model that meets the criteria, although the solution time may increase depending on the capabilities of your computer and the element options selected.
The sparse direct solver, in sharp contrast to the iterative solvers included in ANSYS, is a robust solver. Although the PCG solver can solve indefinite matrix equations, when the PCG solver encounters an
ill-conditioned matrix, the solver will iterate to the specified number of iterations and stop if it fails to converge. When this happens, it triggers bisection. After completing the bisection, the solver continues the solution if the resulting matrix is well-conditioned. Eventually, the entire nonlinear load step can be solved.
Use the following guidelines for selecting either the sparse or the PCG solver for nonlinear structural analysis:
∙If it is a beam/shell or beam/shell and solid structure, choose the sparse direct solver.
∙If it is a 3-D solid structure and the number of DOF is relatively large (that is, 200,000 or more DOF), choose the PCG solver.
∙If the problem is ill-conditioned (triggered by poor element shapes), or has a big difference in material properties in different regions of the model, or has insufficient displacement boundary
constraints, choose the sparse direct solver.
8.6.2.3. Advanced Load Step Options载荷步选项 You Can Set on the Solution Controls Dialog Box
The following sections provide more detail about some of the advanced load step options that you can set on the Solution Controls dialog box.
8.6.2.3.1. Automatic Time Stepping
ANSYS' automatic solution control turns automatic time stepping on [AUTOTS,ON]. An internal auto-time step scheme ensures that the time step variation is neither too aggressive (resulting in many bisection/cutbacks) nor too conservative (time step size is too small). At the end of a time step, the size of the next time step is predicted based on four factors:
∙Number of equilibrium iterations used in the last time step (more iterations cause the time step size to be reduced) ∙Predictions for nonlinear element status change (time step sizes are decreased when a status change is imminent)
∙Size of the plastic strain increment
∙Size of the creep strain increment
8.6.2.3.2. Convergence Criteria
The program will continue to do equilibrium iterations until the convergence criteria [CNVTOL] are satisfied (or until the maximum number of equilibrium equations is reached [NEQIT]). You can define custom criteria if the default settings are not suitable.
ANSYS' automatic solution control uses L2-norm of force (and moment) tolerance (TOLER) equal to 0.5%, a setting that is appropriate for most cases. In most cases, an L2-norm check on displacement with TOLER equal to 5% is also used in addition to the force norm check. The check that the displacements are loosely set serves as a double-check on convergence.
By default, the program will check for force (and, when rotational degrees of freedom are active, moment) convergence by comparing the square root
sum of the squares (SRSS) of the force imbalances against the product of VALUE*TOLER. The default value of VALUE is the SRSS of the applied loads (or, for applied displacements, of the Newton-Raphson restoring forces), or MINREF (which defaults to 0.01), whichever is greater. The default value of TOLER is 0.005. If SOLCONTROL,OFF, TOLER defaults to 0.001 and MINREF defaults to 1.0 for force convergence.
You should almost always use force convergence checking. You can also add displacement (and, when applicable, rotation) convergence checking. For displacements, the program bases convergence checking on the change in deflections (Δu) between the current (i) and the previous (i-1)
iterations: Δu=u
i -u
i-1
.
Note: If you explicitly define any custom convergence criteria [CNVTOL], the entire default criteria will be overwritten. Thus, if you define displacement convergence checking, you will have to redefine force convergence checking. (Use multiple CNVTOL commands to define
multiple convergence criteria.)
Using tighter convergence criteria will improve the accuracy of your results, but at the cost of more equilibrium iterations. If you want to tighten (or loosen, which is not recommended) your criteria, you should change TOLER by one or two orders of magnitude. In general, you should continue to use the default value of VALUE; that is, change the convergence criteria by adjusting TOLER, not VALUE. You should make certain that the default value of MINREF= 0.001 makes sense in the context of your analysis. If your analysis uses certain sets of units or has very low load levels, you might want to specify a smaller value for MINREF.
Also, we do not recommend putting two or more disjointed structures into one model for a nonlinear analysis because the convergence check tries to relate these disjointed structures, often producing some unwanted residual force.
Checking Convergence in a Single and Multi-DOF System
To check convergence in a single degree of freedom (DOF) system, you compute the force (and moment) imbalance for the one DOF, and compare this value against the established convergence criteria (VALUE*TOLER). (You can also perform a similar check for displacement (and rotation) convergence for your single DOF.) However, in a multi-DOF system, you might want to use a different method of comparison.
The ANSYS program provides three different vector norms to use for convergence checking:
∙The infinite norm repeats the single-DOF check at each DOF in your model.
∙The L1 norm compares the convergence criterion against the sum of the absolute values of force (and moment) imbalance for all DOFs.
∙The L2 norm performs the convergence check using the square root sum of the squares of the force (and moment) imbalances for all DOFs.
(Of course, additional L1 or L2 checking can be performed for a
displacement convergence check.)
Example
For the following example, the substep will be considered to be converged if the out-of-balance force (checked at each DOF separately) is less than or equal to 5000*0.0005 (that is, 2.5), and if the change in displacements (checked as the square root sum of the squares) is less than or equal to 10*0.001 (that is, 0.01).
CNVTOL,F,5000,0.0005,0
CNVTOL,U,10,0.001,2
8.6.2.3.3. Maximum Number of Equilibrium Iterations
ANSYS' automatic solution control sets the value of NEQIT to between 15 and 26 iterations, depending upon the physics of the problem. The idea is to employ a small time step with fewer quadratically converging iterations.
This option limits the maximum number of equilibrium iterations to be performed at each substep (default = 25 if solution control is off). If the convergence criteria have not been satisfied within this number of equilibrium iterations, and if auto time stepping is on [AUTOTS], the analysis will attempt to bisect. If bisection is not possible, then the analysis will either terminate or move on to the next load step, according to the instructions you issue in the NCNV command.
8.6.2.3.4. Predictor-Corrector Option
ANSYS' automatic solution control will set PRED,ON if there are no SOLID65 elements present. If the time step size is reduced greatly in the current substep, PRED is turned off. For transient analysis, the predictor is also turned off.
You can activate a predictor on the DOF solution for the first equilibrium iteration of each substep. This feature accelerates convergence and is particularly useful if nonlinear response is relatively smooth, as in the case of ramped loads.
8.6.2.3.5. VT Accelerator
This option selects an advanced predictor-corrector algorithm based on Variational Technology to reduce the overall number of iterations [STAOPT,VT for static analyses, TRNOPT,VT for transient]. This option requires an HPC license. It is applicable to analyses that include large deflection [NLGEOM], hyperelasticity, viscoelasticity, and creep nonlinearities. Rate-independent plasticity and nonlinear contact analyses may not show any improvement in convergence rates; however, you may choose this option with these nonlinearities if you wish to rerun the analysis with changes to the input parameters later.
8.6.2.3.6. Line Search Option
ANSYS' automatic solution control will toggle line search on and off as needed. For most contact problems, LNSRCH is toggled on. For most
non-contact problems, LNSRCH is toggled off.
This convergence-enhancement tool multiplies the calculated displacement increment by a program-calculated scale factor (having a value between 0 and 1), whenever a stiffening response is detected. Because the line search algorithm is intended to be an alternative to the adaptive descent option [NROPT], adaptive descent is not automatically activated if the line search option is on. We do not recommend activating both line search and adaptive descent simultaneously.
When an imposed displacement exists, a run cannot converge until at least one of the iterations has a line search value of 1. ANSYS scales the entire ΔU vector, including the imposed displacement value; otherwise, a "small" displacement would occur everywhere except at the imposed DOF. Until one of the iterations has a line search value of 1, ANSYS does not impose the full value of the displacement.
8.6.2.3.7. Cutback Criteria
For finer control over bisections and cutback in time step size, use [CUTCONTROL, Lab, VALUE, Option]. By default, for Lab= PLSLIMIT (maximum plastic strain increment limit), VALUE is set to 15%. This field is set to such a large value for avoiding unnecessary bisections caused by high plastic strain due to a local singularity which is not normally of interest
to the user. For explicit creep (Option= 0), Lab= CRPLIM (creep increment limit) and VALUE is set to 10%. This is a reasonable limit for creep analysis. For implicit creep (Option = 1), there is no maximum creep criteria by default. You can however, specify any creep ratio control. The number of points per cycle for second order dynamic equations (Lab = NPOINT) is set to VALUE = 13 by default to gain efficiency at little cost to accuracy.
8.6.3. 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 infrequently, and their default settings rarely need to be changed. ANSYS menu paths are provided in this section to help you access these options for those cases in which you choose to override the ANSYS-assigned defaults.
8.6.3.1. Advanced Analysis Options You Cannot Set on the Solution Controls Dialog Box
The following sections describe some advanced analysis options that you can set for your analysis. As noted above in Set Additional Solution Options, you cannot use the Solution Controls dialog box to set the options described below. Instead, you must set them using the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.6.3.1.1. Stress Stiffness
To account for buckling, bifurcation behavior, ANSYS includes stress stiffness in all geometrically nonlinear analyses. If you are confident of ignoring such effects, you can turn stress stiffening off (SSTIF,OFF). This command has no effect when used with several ANSYS elements; see the Element Reference for the description of the specific elements you are using.
Command(s):
SSTIF
GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options 8.6.3.1.2. Newton-Raphson Option
ANSYS' automatic solution control will use the FULL Newton-Raphson option with adaptive descent off if there is a nonlinearity present. However, when node-to-node, node-to-surface contact elements are used for contact
analysis with friction, then adaptive descent is automatically turned on (for example, PIPE20, BEAM23, BEAM24, and PIPE60). The underlying contact elements require adaptive descent for convergence.
Command(s):
NROPT
GUI: Main Menu> Solution> Unabridged Menu> Analysis Type> Analysis Options Use this option only in a nonlinear analysis.This option specifies how often the tangent matrix is updated during solution.If you choose to override the default, you can specify one of these values: ∙Program-chosen (NROPT,AUTO): The program chooses which of the options to use, based on the kinds of nonlinearities present in your model. Adaptive descent will be automatically activated, when
appropriate.
∙Full (NROPT,FULL): The program uses the full Newton-Raphson procedure, in which the stiffness matrix is updated at every
equilibrium iteration.
If adaptive descent is on (optional), the program will use the
tangent stiffness matrix only as long as the iterations remain
stable (that is, as long as the residual decreases, and no negative main diagonal pivot occurs). If divergent trends are detected on an iteration, the program discards the divergent iteration and
restarts the solution, using a weighted combination of the secant and tangent stiffness matrices. When the iterations return to a
convergent pattern, the program will resume using the tangent
stiffness matrix. Activating adaptive descent will usually enhance the program's ability to obtain converged solutions for complicated nonlinear problems but is supported only for elements indicated
under "Special Features" in the Input Summary table (Table 4.n.1 for an element, where n is the element number) in the Element
Reference.
∙Modified (NROPT,MODI): The program uses the modified
Newton-Raphson technique, in which the tangent stiffness matrix is updated at each substep. The matrix is not changed during
equilibrium iterations at a substep. This option is not applicable to large deformation analyses. Adaptive descent is not available.
∙Initial Stiffness (NROPT,INIT): The program uses the initial stiffness matrix in every equilibrium iteration. This option can be less likely to diverge than the full option, but it often requires
more iterations to achieve convergence. It is not applicable to
large deformation analyses. Adaptive descent is not available.
∙Full with unsymmetric matrix (NROPT,UNSYM): The program uses the full Newton-Raphson procedure, in which the stiffness matrix is
updated at every equilibrium iteration. In addition, it generates and uses unsymmetric matrices that you can use for any of the
following:
o If you are running a pressure-driven collapse analysis, an unsymmetric pressure load stiffness might be helpful in
obtaining convergence. You can include pressure load
stiffness using SOLCONTROL,INCP.
o If you are defining an unsymmetric material model using TB,USER, you would need NROPT,UNSYM to fully use the property
you defined.
o If you are running a contact analysis, an unsymmetric contact stiffness matrix would fully couple the sliding and the
normal stiffnesses. See Determining Contact Stiffness and
Allowable Penetration in the Contact Technology Guide for
details.
You should first try NROPT,FULL; then try NROPT,UNSYM if you
experience convergence difficulties. Note that using an
unsymmetric solver requires more computer time to obtain a solution, than if you use a symmetric solver.
∙If a multistatus element is in the model, however, it would be updated at the iteration in which it changes status, irrespective of the Newton-Raphson option.
8.6.3.2. Advanced Load Step Options You Cannot Set on the Solution Controls Dialog Box
The following sections describe some advanced load step options that you can set for your analysis. As noted above in Set Additional Solution Options, you cannot use the Solution Controls dialog box to set the options described below. Instead, you must set them using the standard set of ANSYS solution commands and the standard corresponding menu paths.
8.6.3.2.1. Creep Criteria
If your structure exhibits creep behavior, you can specify a creep criterion for automatic time step adjustment [CRPLIM,CRCR, Option]. (If automatic time stepping [AUTOTS] is off, this creep criterion will have no effect.) The program will compute the ratio of creep strain increment , the change in creep strain in the last time step) to the elastic (Δε
cr
strain (ε
el
), for all elements. If the maximum ratio is greater than the criterion CRCR, the program will then decrease the next time step size; if it is less, the program might increase the next time step size. (The program will also base automatic time stepping on the number of equilibrium iterations, impending element status change, and plastic strain increment. The time step size will be adjusted to the minimum size calculated for any of these items.) For explicit creep (Option = 0), if
the ratio Δε
cr / ε
el
is above the stability limit of 0.25, and if the
time increment cannot be decreased, a divergent solution is possible and the analysis will be terminated with an error message. This problem can be avoided by making the minimum time step size sufficiently small [DELTIM and NSUBST]. For implicit creep (Option = 1), there is no maximum creep limit by default. You can however, specify any creep ratio control.
Command(s):
CRPLIM
GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Creep Criterion
Note: If you do not want to include the effects of creep in your analysis, use the RATE command with Option = OFF, or set the time steps to be longer than the previous time step, but not more than 1.0e-6 longer.
8.6.3.2.2. Time Step Open Control
This option is available for thermal analysis. (Remember that you cannot perform a thermal analysis using the Solution Controls dialog box; you must use the standard set of ANSYS solution commands or the standard corresponding menu paths instead.) This option's primary use is in unsteady state thermal analysis where the final temperature stage reaches a steady state. In such cases, the time step can be opened quickly. The default is that if the TEMP increment is smaller than 0.1 in three (NUMSTEP = 3) contiguous substeps, the time step size can be "opened-up" (value = 0.1 by default). The time step size can then be opened continuously for greater solution efficiency.
Command(s):
OPNCONTROL
GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Open Control
8.6.3.2.3. Solution Monitoring
This option provides a facility to monitor a solution value at a specified node in a specified DOF. The command also provides a means to quickly review the solution convergence efficiency, rather than attempting to gather this information from a lengthy output file. For instance, if an excessive number of attempts were made for a substep, the information contained in the file provides hints to either reduce the initial time step size or increase the minimum number of substeps allowed through the NSUBST command to avoid an excessive number of bisections.
Command(s):
MONITOR
GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Monitor
Additionally, the NLHIST command allows you to monitor results of interest in real time during solution. Before starting the solution, you can request nodal data such as displacements or reaction forces at specific nodes. You can also request element nodal data such as stresses and strains at specific elements to be graphed. Pair-based contact data are also available. The result data are written to a file named Jobname.nlh.
For example, a reaction force-deflection curve could indicate when possible buckling behavior occurs. Nodal results and contact results are monitored at every converged substep while element nodal data are written as specified via the OUTRES setting.
You can also track results during batch runs. To execute, either access the ANSYS Launcher and select File Tracking from the Tools menu, or type nlhist120in the command line. Use the supplied file browser to navigate to your Jobname.nlh file, and select it to invoke the tracking utilty. You can use this utilty to read the file at any time, even after the solution is complete.
Command(s):
NLHIST
GUI: Main Menu> Solution> Results Tracking
Note: Results tracking is not available with FLOTRAN analyses.
8.6.3.2.4. Birth and Death
Specify birth and death options as necessary. You can deactivate [EKILL] and reactivate [EALIVE] selected elements to model the removal or addition of material in your structure. As an alternative to the standard birth
and death method, you can change the material properties for selected elements [MPCHG] between load steps.
Command(s): EKILL,
EALIVE
GUI: Main Menu> Solution> Load Step Opts> Other> Birth & Death> Kill Elements
Main Menu> Solution> Load Step Opts> Other> Birth & Death> Activate Elem
The program "deactivates" an element by multiplying its stiffness by a very small number (which is set by the ESTIF command), and by removing its mass from the overall mass matrix. Element loads (pressure, heat flux, thermal strains, and so on) for inactive elements are also set to zero. You need to define all possible elements during preprocessing; you cannot create new elements in SOLUTION.
Those elements to be "born" in later stages of your analysis should be deactivated before the first load step, and then reactivated at the beginning of the appropriate load step. When elements are reactivated, they have a zero strain state, and (if NLGEOM,ON) their geometric configuration (length, area, and so on) is updated to match the current displaced positions of their nodes. See the Advanced Analysis Techniques Guide for more information on birth and death.
Another way to affect element behavior during solution is to change the material property reference number for selected elements:
Command(s):
MPCHG
GUI: Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Change Mat Num
Note: Use MPCHG with caution. Changing material properties in a nonlinear analysis may produce unintended results, particularly if you change nonlinear [TB] material properties.
8.6.3.2.5. Output Control
In addition to OUTRES, which you can set on the Solution Controls dialog box, there are several other output control options that you can set for an analysis:。