D1. General information on numerical calculations

D.1.1 Calculation time

Computation time (in the broadest sense: solving the system of equations and storing the results) is an essential point of reflection to be associated with Finite Element modeling.

It must remain compatible with the budget and timeframe associated with the project. The search for an optimized computation time is even one of the key elements when considering the economy of a project.

The calculation time is influenced by different factors.

The finite element model:

Number of degrees of freedom,
Formulation of the elements, number of integration points.

One can optimize the computation time by using simplified models, sub-models, sub-structures, symmetries, or locally adapted mesh sizes. However, be careful with explicit calculations because the time step is set based on the dimension of the smallest element.

The computing capacity:

RAM: random access memory (temporary storage),
the operating system (32 or 64 bits),
is the calculation done locally (on the user's workstation)? on a local server? on an external server? Model and results copy times, or the time it takes to launch other calculations on the same server can be long,
the capacity and number of processors: the "CPU time" (Central Processing Unit) usually provided by the software should be checked.

Optimizing a given computing system can consist of performing the calculation in batch (launching the calculation in command lines without the interface), or parallelizing the calculations (on several processor cores), and/or performing further calculations if the software allows it.

The type of analysis:

Linear/non-linear and the associated algorithms,
Numerical integration scheme (direct integration/modal-based projection, implicit/explicit scheme) and the choice of the solver for dynamic calculations.

The type of analysis is specific to the problem and the desired accuracy of the results. Therefore, the modeler oversees the optimization. However, it is emphasized that in the case of a transient calculation, the duration of the calculation (in terms of loading and response of the structure) should not be overestimated so as not to add unnecessary calculation time (machine time).

The anticipation of "post-processing":

for some software, it is possible to select (and keep) only the quantities of interest chosen by the user, as well as the instants (in the case of transient or phase calculations): the machine time to write the results is then reduced,
the number of saved/reused modes in the case of a modal analysis can generally be modified (definition of variable filters depending on the software),
the real-time visualization of results can be used to stop a calculation in progress (but it generally leads to an increase in calculation times),
the analysis of the results can be performed using post-processors independent of the Finite Element Calculation software to reduce the operating time.

The automation of the calculations and post-processing (after validation of the first calculation round and using appropriate verifications ) is interesting when the user has to perform the same calculation several times on different models or similar calculations on the same model.

The acceptability of the calculation time must be assessed because the model will run many times and will become more complex as the study phases progress.

D.1.2 Convergence of the software – The case of direct elastic calculations

In direct elastic calculations (linear static calculation and spectral modal calculation), there are very few reasons for the software not to converge:

either the structure is unstable,
or the inversion of the stiffness matrix is impossible because there are stiffness differences between the elements that are too large.

All error messages, at this stage, are related to these two cases.

Due to the boundary conditions in place, the displacements, translation(s), and/or rotation(s) of certain nodes of the structure are imposed (a blockage is a zero imposed displacement). However, the set of these blocked displacements may appear insufficient to prevent an overall movement of the structure.

It is advised, by choosing an appropriate reference frame, to analyze the effects of all the blockages on the overall movements of the structure and to add one or more restraints to ensure the stability of the structure. At the end of the calculations, it must be verified that the reactions due to these additional blockages are null or negligible: effort for a blockage in displacement, moment for a blockage in rotation.

Some software, for specific geometries of structures, ignore the problem of instability. In this case, the stresses and deformations are correct, but some displacements are somewhat unreasonable. Another instability issue often encountered is related to the connection between different types of structural elements. This is specified in paragraph C.6.3.3.

It should be noted that software error messages are sometimes not very explicit about the global, local, and/or numerical nature of the instabilities.

Furthermore, some software programs allow the calculation to be completed despite a warning or error message. This can help understanding or visualizing where the problem comes from, but the results are not satisfactory in this context.

In the end, it is necessary to have a model that runs without errors.

These problems of global and local instabilities can be detected by performing simple calculations:

either linear static calculations by applying a global acceleration (10 m/s² for example) to the structure. Three load cases can be created according to the 3 main directions,
or a modal calculation (determination of the first eigenfrequencies).

If the structure presents global instabilities, the static calculation is unlikely to succeed whereas the modal calculation will present rigid modes.

If the structure presents discontinuities, they will be highlighted by the shape of the deformation or the eigenmodes. Be careful, taking into account the shear stress deformations leads to failures in the deformed shape.

D.1.3 Convergence of the software - Case of iterative calculations

For non-linear calculations, the convergence of a Finite Elements calculation is obtained with a function interpolating the solution for each of the finite elements (principle of discretization).

The convergence criteria are either given by the user or taken as default values by the software. The finite element calculation consists of a series of iterations and stops either when the maximum number of iterations has been reached or when certain deviation measures between two successive iterations are below the predefined thresholds (this is called the convergence criteria).

On the other hand, a calculation that has stopped does not mean that it did not converge towards a valid solution. For example, deformation criteria that are too loose compared to reality, or a maximum number of iterations that are too low, can output a result that is not realistic.

D.1.4 Model Convergence

A model is considered to have converged when a small change in the size and geometry of the meshes does not significantly disturb the results.

To be rigorous, it is advised to carry out a sensitivity study of the mesh to the post-processed quantities. Thus, carrying out the same analysis on different meshes (reduction of the mesh size, for example), should - if not provide similar results (acceptable tolerance) - converge towards an acceptable solution to the user. It is important not to focus on peak values and to bear in mind that several successive refinements of meshes can lead to divergent results.

It is also advised to analyze the software's warning messages ("Warning" on mesh size or shape) to assess whether they are likely to alter the results.