Engineering analysis + design software

User Area > Advice

Pivot, diagonal decay & ill conditioning checklist

This checklist described causes and remedies for analyses that produce diagonal decay, negative pivot, zero pivot or ill-conditioned warning and error messages. These messages typically include the element, node and/or variable number that is affected by the poor conditioning. These should be located in the model and their characteristics borne in mind when using the following checklist.

More background information may be obtained from a discussion on ill-conditioning.

Mesh description

  • The aspect ratio of some elements are greater than the recommended limits. An ideal value would be 1:1. This is usually not required, however, and values up to 1:10 may be reasonable. Depending on the results required and the stress field sustained by the elements, this value may be increased further (test models would be recommended). Note that explicit dynamic elements really do require aspect ratios of 1:1
  • Some element shapes are too distorted. This refers particularly to the curvature of element sides and the central positioning of the mid-side nodes for higher order elements (see appendix B in the Element Reference Manual).  Further mesh refinement may be necessary
  • For flexible structures, the mesh refinement may be too coarse to account for significant stiffness changes across elements
  • The use of 3D beam elements with 2D geometric properties is not valid
  • Coarse mesh refinement in areas remote from structural support conditions in significantly flexible structures can cause conditioning problems. Typically the warning/error message will be associated with an element/node number at the most extreme position of the structure. Mesh refinement is required
  • 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 analyses. If the problem persists, continue with the use of fine integration but refine the mesh further
  • Elements that have large aspect ratios may cause solution problems – particularly in the presence of significant plastic strain
  • Rigid body (particularly torsional) motion may occur when connecting beam and shell elements to continuum elements due to insufficient additional restraint
  • By default, the option to "assign 6 DOF to all thick shell element nodes" is invoked in Modeller (File> Model Properties> Options> Element options…). If there are no rotational supports or loads and the shell thickness is excessively thick or thin then remove this option
  • Multiple bar elements used independently and without the use of a geometrically nonlinear analysis to generate stress stiffening are prone to zero pivots, for example a simple cantilever beam. Bars have no transverse (shear) stiffness and are particularly useful for modelling reinforcement bars or "tie" linkages where there is no moment connectivity. These elements will not present any difficulties when used in conjunction with other plane elements (shells, plates, etc.) since the transverse stiffness required to prevent a numerical mechanism will be contributed from the underlying surface elements
  • The material properties of joint elements operate in the local element directions and can be easily defined incorrectly. See the additional sections in the user area on the use of joint elements

Geometric properties

  • Specification of a zero magnitude for any shear area parameters in the geometric properties for beams
  • Specification of zero magnitude for other important properties, such as the torsional constant or thickness
  • Defining incompatible 1st and 2nd moment section properties for beams

Material properties

  • A different set of units is used to define the nodal coordinates and the material properties
  • Inconsistent units throughout the model. This would be of particular concern for dynamic analyses where SI units are recommended
  • Incorrect nonlinear material parameters such as a zero yield stress or significant variations in the magnitude of mult-hardening curves
  • The plastic and total strain-hardening definition requires that the first set of points correspond to the initial uniaxial yield stress and the elastic strain at which this stress occurs
  • Incorrect definition of orthotropic properties. There are inequalities that need to be adhered to such that a valid material is obtained. Numerical instabilities may result when the material characterisation approaches their limits
  • Ill-conditioning may occur in large strain analyses using the rubber material model in which the bulk modulus is defined to enable incompressibility approaching 100%. Reducing this modulus will alleviate such problems and permit greater strains to be attained. Note that this does not apply for membrane and plane stress analyses, since the bulk modulus is ignored in such cases
  • Joint element stiffness magnitudes may be too high (or too low) relative to the structural stiffness
  • Assigning nonlinear material properties to an element type which does not support that particular model

Support nodes

  • Are supports defined and assigned? The structure must be restrained against free body translation and rotation (except for dynamic analyses)
  • Check that there are adequate supports in all translational directions. For beams, be aware that the problem could be with unrestrained torsional motion
  • All nodes of axisymmetric elements lying on the axis of symmetry must be restrained to prevent any radial displacement across the symmetry axis (more information). MODELLER does not create such centreline supports automatically

Modelling Integrity

  • A further possibility is that the integrity of the MODELLER model geometry is questionable. This would lead to an element mesh containing gaps within it or having discontinuities in the connection of the elements - thereby permitting some of the elements in, or near, the vicinity of the gap to deform with significantly reduced restraint

Such a lack of integrity may be found by:

  • Viewing only the outline of the mesh (Mesh layer properties). The view will draw lines wherever a discontinuity occurs
  • Drawing the node numbers onto the mesh (label layer properties) to see if any node numbering is overwriting at any point (indicating two nodes at the same point). Correction would normally require either a merging or an equivalencing operation


  • Slideline interface stiffness coefficients that are too small may allow bodies to pass through each other as rigid bodies and cause pivot problems
  • Slideline interface stiffness coefficients that are too large may cause bodies to "bounce" off each other in such a way as to cause the bodies to pass through/beyond each other as rigid bodies and cause pivot problems


innovative | flexible | trusted

LUSAS is a trademark and trading name of Finite Element Analysis Ltd. Copyright 1982 - 2022. Last modified: June 19, 2024 . Privacy policy. 
Any modelling, design and analysis capabilities described are dependent upon the LUSAS software product, version and option in use.