A recommended and efficient approach to nonlinear analyses typically involves the following steps…

• Perform and scrutinise the results from a static linear analysis to check the integrity and behaviour of the basic model. This is one of the first questions that FEA technical support will ask!
• It is strongly recommended that small tests be performed to gain experience of each proposed nonlinear facility, to understand its limitations and to ensure that it does provide the required behaviour for the actual simulation to be carried out. Single element tests are preferable since it is so much quicker and easier to verify the input and to evaluate the response with only a few degrees of freedom. There are a number of sources of examples and benchmarks available that may help in this regard…

1. The LUSAS examples manual. This contains an increasing amount of worked examples written with the express intention of demonstrating the use of the facilities clearly
2. The LUSAS verification manual. This was provided in versions 9, 10 and 11 of the software, was dropped in version 12, but has now been included again in version 13.3 by popular demand. It is in LUSAS Solver format only. The data files associated with this manual can be located in the LUSAS install directory
3. The NAFEMS suite of examples. The User area has a link to the NAFEMS website ("useful links") where further information is available on the benchmark tests that they provide. FEA have performed a number of these benchmarks and the resulting data files are available in the LUSAS install directory

• If buckling is expected, a linear buckling analysis should be performed to obtain the linear buckling load. This will act as both a benchmark value to compare against as well as a useful aid in determining the load magnitude to be applied in the geometrically nonlinear analysis
• Add each of the nonlinearities one by one to determine their effect on the solution and it’s convergence behaviour. For instance, start with slidelines, adding next any material nonlinearity and then geometric nonlinearity, etc.

The accuracy of the nonlinear analysis can then be assessed by performing further analyses with refined data, e.g. smaller load steps or finer mesh discretisation in areas of high stress. If no significant differences in the solution are observed, then the solution is close to optimal for the given modelling assumptions

However, faced with a stubbornly non-converging analysis, the key question is "what is causing the failure?". The following list comprises the more frequent causes and remedies of convergence problems…

• The LUSAS output file should be investigated in the first instance. If there are pivot or diagonal decay warnings these should be dealt with. See the additional checklist on the more frequent causes and remedies of pivot warnings or use the search facility in the user area to locate further details on other messages that may be found
• Are there warning messages that indicate specific problems within the iterative procedure? These should be examined closely and acted upon
• The load increment specified may be too large. If manual nonlinear incrementation has been selected, change to automatic nonlinear incrementation and increase the load more gradually. If automatic incrementation is already being utilised, reduce the load increment still further. The first increment in contact analyses is typically more difficult as the initial contact conditions are established
• If the solution was converging slowly, but required a few more iterations than was specified for an increment then…

1. Increase the number of iterations permitted per increment to 20-25 (Load case properties> Nonlinear> Set…> Solution strategy> "Max number if iterations")
2. Reduce the load increment applied by reducing the "Starting load factor" (Load case properties> Nonlinear> Set…> Incrementation…) and/or decrease the desired number of iterations per increment (Load case properties> Nonlinear> Set…> Incrementation> "Iterations per increment"
3. Make sure that full Newton-Raphson iterations are being used rather than modified (modified NR is the only option in MODELLER)
4. Make sure that the line search method has not been switched off (Load case properties> Nonlinear> Set…> Solution strategy> Advanced…> "Max number of line searches")

• Relatively stiff elements can produce numerical round-off problems as well as propagate the effects of nonlinearity throughout a mesh in an uncontrolled manner. This can be the case, for instance when simulating rigid links using joint or bar elements. Reducing the stiffness by one or two orders of magnitude can have significant effects on the convergence rate
• Elements that have poor aspect ratios (greater than 1:10) can produce significant difficulties in the nonlinear solution process – particularly if the elements are subject to large stress gradients of sufficient magnitude to cause material failure (with materially nonlinear analyses) or large deformations (with geometrically nonlinear analyses)
• Has the model been fully merged and/or equivalenced to ensure that there are no cracks present?
• Have inconsistent units been specified in the model? For instance, the nonlinear material properties may have been specified in N-M-Kg whilst the rest of the model is in N-MM-Kg
• Have the nonlinear convergence criteria been slackened? This can allow initial increments to converge but may be causing convergence problems later in the incremental procedure since the slackness is not allowing the solution to follow the equilibrium path sufficiently accurately. The default setting for the displacement and residual norms should be used in general – particularly for geometrically nonlinear analyses
• Element mechanisms may have been excited by the loading patterns that may be eliminated by invoking the fine integration rule for these elements. To check that the element does support fine integration see the specific element section in the Element Reference Manual. The Semiloof shell elements are known to be prone to such mechanisms in the case of very thin, curved surface meshes. If the problem persists, continue with the use of fine integration but refine the mesh further
• The enhanced strain formulation elements (QPM4M, HX8M, etc.) have been known to cause numerical problems when used in conjunction with material nonlinearity. If this is suspected, revert to the standard continuum versions of these elements
• For contact analyses involving slidelines, there are a number of possibilities that can cause problems. More information
• A section of the structure assigned with a nonlinear material model may be close to complete collapse. This can be brought about in the presence of single point supports and loads where the element(s) associated with such a support can fail and, hence, no longer provide support to the structure. Alternatively the effects of a single point load can generate such a stress singularity that the elements across the section can fail (displacement-based finite elements will try to reproduce an infinite stress at the point of application of a point load). In such circumstances, smaller load increments or a finer mesh may be used. Ideally, however, the point support or load should be applied over a number of nodes to simulate the reality in the structure more closely
• Do the element types used support the nonlinearity specified? It is permissible to mix linear and nonlinear elements in the same model – as long as the model area in which the linear elements are used are expected to accord with small deformation, small strain, elastic behaviour
• "Element locking" can occur on highly constrained structures in a materially nonlinear analysis as well as analyses in which massive plastic strain is developed. The effective plastic strain magnitude should be displayed to check this. Linear triangular elements are notoriously guilty of this numerical phenomenon. In general, higher order elements are recommended where possible, in conjunction with fine integration
• If geometric nonlinearity has not been invoked, it is possible that large rotation effects are causing undue stiffening in the structure and leading to convergence problems
• If geometric nonlinearity is already invoked try invoking an arc length procedure and guide the solution with the current stiffness parameter (Load case properties> Nonlinear> Set…> Incrementation> Advanced…)

If convergence is not achievable in the first increment it can be very helpful to specify that solver continues – even if an increment fails to converge. This means that a MODELLER results file will be generated that can give valuable clues to the cause of the convergence failure. To do this…

• Force solver to continue by file> Model Properties> Solution> Nonlinear options… and invoke "continue solution after convergence failure"
• Suppress step reductions (Load case properties> Nonlinear & Transient> Nonlinear> Advanced… and unset the "allow step reduction" flag
• Ensure that the termination criteria is set to 1 increment (Load case properties> Nonlinear & Transient> Nonlinear… set "max time steps or increments" to unity
• Read in the results file, set the unconverged load case active and exaggerate the deformation to see if there are any localised effects in the mesh that can be attributable to any of the above possible causes of non-convergence