User Area
> Advice
Causes and Remedies of Convergence Problems
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…
 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
 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
 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 nonconverging 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…
 Increase the number of iterations permitted per increment to 2025 (Load case
properties> Nonlinear> Set…> Solution strategy> "Max number if
iterations")
 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"
 Make sure that full NewtonRaphson iterations are being used rather than modified
(modified NR is the only option in MODELLER)
 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 roundoff 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 NMKg whilst the rest of the model is in
NMMKg
 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
(displacementbased 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 nonconvergence
If this fails to point to the cause of the problem, the next step is to remove the
nonlinear effects one by one from the analysis and solve again – continuing to
"strip back" the analysis complexities until convergence is achieved. This will
show the cause of the convergence problem and the particular facility can then be
investigated more closely. Another helpful method is to reduce the nonlinear effects
within each facility, e.g. if using slidelines, change from the general sliding to a tied
slideline option – if using material nonlinearity, increase the initial yield stress
and/or strain hardening values to approach an elastic material behaviour, if using a
nonlinear joint material change to the linear model
