User Area
> Advice
Analysis Checklist
PreAnalysis Checks
 PostAnalysis Checks
The LUSAS support team are happy to answer queries
and help
with problems that users encounter. However, identifying the cause of a problem can
create delay to a project, especially if the analysis is large. Users can
often eliminate such delays by thorough checking using the checklists
below. It is good practice to systematically carry
out these checks as a matter of course whether or not there appears to be a problem with
the solution obtained.
 Start with the simple
checklist, only 4 points, applicable to linear static analyses.
 Read the LUSAS Solver text output file (*.OUT):
Check for warning and error messages (search for ***) and read
the explanation
Check the model output summary (search for E S T I M A T E)
Is the OUT file echoing the input data that you think
you've specified?
Is there anything described in the file that you were not expecting (e.g.
unexpected constraint equations appear)?
In
particular check MATERIAL PROPERTIES.
 Check the current
software problems/ limitations list
for any known issues which could be causing your problem.
 If you encounter a problem do not suppress the data input printout with
OPTIONS 44 and 45.
 Carry out your own QA check on your model (see below).
Thorough checking leads to greater efficiency, productivity
and hence profitability. Users should create their own set of QA checks that will be particular to the type of
analyses for which they are responsible. The following are some of checks undertaken by the
consultancy department at LUSAS UK when carrying out an analysis for a
client, giving a general guide as to the sort of checks that should be
included.
PreAnalysis Checks
ALL ANALYSIS TYPES
 Check consistency of coordinate systems between the finite element model
and the engineering drawing.
 Check key drawing dimensions against coordinates of respective points in
the model.
 Check mesh for cracks and voids. Checks for cracks must be made to ensure that the features form a continuous structure.
Doubleclick on the Mesh layer to display its properties. Click on outline only and press the Apply button to drawn the outline of the mesh only. Select the Geometry layer and delete it to hide the geometry from the current window.
For further information search the online manuals for 'How to visualise and fix cracks in the mesh'.
 Check the material and geometric assignments are
correct. To visualise the assignments:
 Double click on Geometry in the tree view to get
Geometry properties
 Tick on the solid box
 Choose: Colour by: Assigned attributes
 Click on Set... and choose material
(or other attributes) in the obtained menu.
This will
then give a colour coded display of elements which have been assigned the same
attributes.
 Check for consistent
units. i.e. comply with one system of units. [N,m,kg,s]
is a consistent set of units [N,mm,kg,s] is not!
 Check correct orientation of beam properties. Double
click on Mesh in the tree view and tick on Show element Axes check box.
 Check correct loads and boundary conditions are
applied. Use attributes in the layers tree view and also Load case
properties > Assignments.
 Check element thicknesses against drawing (plates/shells).
See item 4 for plotting procedure.
 Check reversed normals for plates/shells. Use 'Show element
axes' or 'Show normals' in Mesh properties.
 Check element shapes for aspect
ratio/skew/warp/taper/curvature/central
mid side nodes. Warning messages are given in the output file.
 Check for duplicate nodes and elements. Warning messages are given in the
output file. You might need to SET OPTION 2 via command bar to see all
the warnings.
 Check adequate mesh density is being used. A
sensitivity analysis might be performed for this purpose.
 Check output control gives sufficient checkout information in output
file (e.g. reactions).
 Pilot analysis on crude model to check load paths and equilibrium.
 Compare finite element results with estimates of stress/deflection from
hand calculations if possible.
 Keep an up to date log book, with adequate plots to
cover all parts of the model. Set up an adequate reference system to select individual
regions of the model. Use Groups facility in Modeller which can be accessed
via Geometry > Group menu.
DYNAMIC ANALYSIS TYPES
 Obtain an estimate of the first natural frequency of the model by hand
calculations if possible.
 Preliminary linear static analysis. It is always best to do this first
and no time is really wasted as the data file can easily be converted for the dynamic
analysis.
NONLINEAR ANALYSIS TYPES
 Preliminary linear static analysis. It is always best to do this first
and no time is really wasted as the data file can easily be converted for the nonlinear
analysis.
Back to top
PostAnalysis Checks
ALL ANALYSIS TYPES
 Check reactions for equilibrium. Compare the reactions
calculated by hand with those using Utilities > Print results wizard
> Entity=Reaction, Type=Summary.
It is essential to check all loadcases in this manner to identify gross errors.
 Check the magnitudes of displacements and stresses (Utilities
> Print results wizard > Entity=Displacement, Type=Summary). Compare to hand
calculations. How do they compare to the "expected" behaviour of the model? On reflection is it modelling
assumptions/errors or the expectations that require further scrutiny?
This check is particularly useful in identifying problems concerning
inconsistent units, material/geometric properties or missing supports.
 Check mesh refinement.
Plot stress contours, then use TreeView > Layers tab > (double
click) Contours > Contour display tab > (uncheck) Smoothed.
Check for reasonable continuity of stresses across elements. Further
information
 Check LUSAS Solver text output file (*.OUT) for matrix illconditioning
(Pivot & diagonal
decay) messages .
Small pivot and diagonal decay warning messages are invoked when the stiffness matrix is
poorly conditioned. Diagonal decay means that roundoff error during the solution has
become significant which could lead to inaccurate results. A poorly conditioned stiffness
matrix is the result of a large variation in magnitude of the diagonal terms. This could
be caused by large stiff elements being connected to small less stiff elements or elements
with highly disparate stiffnesses (e.g. a beam may have a bending stiffness that is orders
of magnitude less than its axial stiffness).
 A negative pivot in a nonlinear analysis usually means that a limit or
bifurcation point has been encountered. However, negative pivots sometimes occur during
the iterative solution (which sometimes means that the load step is too big) but disappear
when the solution has converged. If negative pivots occur and the solution will not
converge then first try reducing the load step.
 If the solution still does not converge a limit or bifurcation point may
have been encountered in which case the solution procedure may need to be changed. Running
the problem under arc length control gives the best chance of negotiating a limit or
bifurcation point. A load limit point can also be overcome by using prescribed
displacement loading.
 Check the output file (.OUT) for other warning or error messages.
This may identify areas in the model which could be improved.
 Check the model summary. This gives the total length, area, volume and
mass for the structure together with the centre of gravity, moments of inertia and
resultant applied load at the origin.
DYNAMIC ANALYSIS TYPES
 Check first natural frequency against hand calculation.
NONLINEAR ANALYSIS TYPES
 Check convergence for nonlinear and eigenvalue runs.
More on causes and
remedies of convergence problems.
 Eliminate any
negative eigenvalues
