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> Solution>
Element…). 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
Slidelines
- 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
|
