News / Blog
Significance of Energies in FE Simulation – Part-1
Solving Problems with Local Instabilities
Energy balance is an important part in a Non-linear FEA analysis. In a static analysis, the Total Energy should ideally be zero. In a transient dynamic analysis, the Total Energy may not necessarily be close to zero, especially with initial Kinetic Energy, but should remain constant throughout the solution duration. Energies are often overlooked in FEA, leading inappropriate response in the structure. Comparisons between various energy components should be used to evaluate whether an analysis is providing an appropriate response. This is highly required in problem involving significant instabilities.
Instabilities can be global or local. Global instabilities may arise due to the release of accumulated strain energy as a result of buckling or snap through behavior of the structure. This behavior can be simulated using RIKS method in ABAQUS or using a transient dynamic procedure. On the other hand, local instabilities in a non-linear static analysis could be a result of localized buckling, localized material softening and contact separation.
In the first part of this topic let us take a look on handling local instabilities in a non-linear static analysis and validating the analysis using energy output. Localized instabilities due to the above said reasons can be viewed as convergence difficulties the solver is facing. This can be typically viewed in the ABAQUS status file (job-name.sta) as cutbacks in the time increment. In the message file (job-name.msg) at the respective problematic increment, one may typically view the warning messages corresponding to the localized instability. Warning messages could include “negative eigenvalues”, “element distortion”, “strain increment exceeding” etc. for localized buckling and material softening, and “numerical singularity” in the middle of the analysis due to contact separation. One has to understand that in these above situations the problem has essentially become dynamic i.e. releasing the accumulated strain energy. In a static analysis this released strain energy cannot be dissipated into kinetic energy as the underlaying principle of static analysis is to capture a stable configuration. Hence some form of damping is required.
ABAQUS offers automated viscous damping to help obtain a solution for these class of unstable problems. It automatically applies damping forces to local regions that develop sudden instabilities and smoothes severe discontinuity in response. The functionality uses a mass component with unit density and a damping factor calculated automatically in the finite element equation to stabilize the response. It can be turned on while creating a static step (*STATIC, STABILIZE) as shown in the image below. The stabilization is applied based on the underlying assumption that the model’s response in the first increment of a step to which damping is applied is stable. This is to ensure that the dissipated energy is significantly small. So enough care must be taken to start the analysis under stable conditions when using automatic stabilization. If possible, it is recommended to split the analysis into two steps, start the first step without stabilization until it hits instability and then start a second step with stabilization to complete the analysis. This will ensure that the model is in static equilibrium when stabilization is applied. Never use this form of stabilization for initial rigid body motion. Also note that automatic stabilization does not carry over automatically to subsequent steps of the analysis.
To conclude, automatic stabilization can be used to find equilibirium solution for problems with local instabilities but enough care should be taken to ensure that the model is in static equilibirium when stabilization is applied. Finally, the energy balance needs to checked using the history output plots. Check and ensure that the viscous dissipated energy (ALLSD) is very small. Typically ALLSD should be less than 5% of total strain energy (ALLSE) in the model. Similarly viscous forces/moments (VFn/VMn) should also be compared against applied forces/moments and ensure that they are small to validate the accuracy of the solution.
In the upcoming tips and tricks we shall review significance of other energies in finite element simulation as well as using contact stabilization.