Engineering analysis + design software

User Area > Advice

Analysis Checklist

Pre-Analysis Checks | Post-Analysis 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.

0div.gif (1132 bytes)

Pre-Analysis Checks

  1. Check consistency of coordinate systems between the finite element model and the engineering drawing.
  2. Check key drawing dimensions against coordinates of respective points in the model.
  3. Check mesh for cracks and voids. Checks for cracks must be made to ensure that the features form a continuous structure. Double-click 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'.
  4. 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.

  1. 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!
  2. Check correct orientation of beam properties. Double click on Mesh in the tree view and tick on Show element Axes check box.
  3. Check correct loads and boundary conditions are applied. Use attributes in the layers tree view and also Load case properties > Assignments.
  4. Check element thicknesses against drawing (plates/shells). See item 4 for plotting procedure.
  5. Check reversed normals for plates/shells. Use 'Show element axes' or 'Show normals' in Mesh properties.
  6. Check element shapes for aspect ratio/skew/warp/taper/curvature/central mid- side nodes. Warning messages are given in the output file. 
  7. 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.
  8. Check adequate mesh density is being used. A sensitivity analysis might be performed for this purpose.
  9. Check output control gives sufficient check-out information in output file (e.g. reactions).
  10. Pilot analysis on crude model to check load paths and equilibrium.
  11. Compare finite element results with estimates of stress/deflection from hand calculations if possible.
  12. 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.


  1. Obtain an estimate of the first natural frequency of the model by hand calculations if possible.
  2. 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.


  1. 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

0div.gif (1132 bytes)

Post-Analysis Checks


  1. 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.
  2. 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.
  3. 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
  4. Check LUSAS Solver text output file (*.OUT) for matrix ill-conditioning (Pivot & diagonal decay) messages . Small pivot and diagonal decay warning messages are invoked when the stiffness matrix is poorly conditioned.  Diagonal decay means that round-off 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).
  5. 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.
  6. 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.
  7. Check the output file (.OUT) for other warning or error messages.  This may identify areas in the model which could be improved.
  8. 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.


  1. Check first natural frequency against hand calculation.


  1. Check convergence for non-linear and eigenvalue runs. More on causes and remedies of convergence problems
  2. Eliminate any negative eigenvalues 

innovative | flexible | trusted

LUSAS is a trademark and trading name of Finite Element Analysis Ltd. Copyright 1982 - 2022. Last modified: November 29, 2022 . Privacy policy. 
Any modelling, design and analysis capabilities described are dependent upon the LUSAS software product, version and option in use.