Nonlinear Implicit Analysis Notes

In Nonlinear Implicit Analyses, when the element formulations are different between the stiffness matrix building and the internal force calculation (same as explicit one), convergence issues are often observed; this is especially true for the reduced integration elements with perturbation hourglass controls. On the other hand, it is possible to obtain converged results with elements of similar formulations such as QEPH and QBAT for shells, or HA8, HC8, S8 and HEPH for solids. In any case, same formulations are preferred.

As mentioned before, Radioss uses only the elastic part of the material parameters to build the stiffness matrix which allows working with all available Radioss materials. Another advantage of using the elastic stiffness matrix is that convergence issues are avoided with certain materials (such as elastoplastic). Some example tests have shown that the elastic stiffness matrix associated with line-search provides reasonable convergence for nonlinear material computations. Of course, the Newton-Raphson (using tangent matrix) method could also be added in the future.

The only exception to using the elastic part of material is in the case of spring elements, which are not associated with any material laws. When a nonlinear function is defined in the spring property for Implicit Nonlinear Analyses, the tangent stiffness elementary matrix will be computed. However, to avoid the convergence issues in Nonlinear Analysis, the elastic stiffness matrix is still used for elastoplastic springs (H>0). In Linear Analyses with spring elements, if nonlinear stiffness functions have been defined, a linear stiffness is calculated taking only the first points (besides 0, 0) of this function.

Convergence issues are frequently encountered in nonlinear analyses, in which the control parameters play an important role. These parameters are problem-dependent and the input values could determine the convergence or failure of a computation. The best values are often a good compromise between the quality and the performance.

First, control parameters for the nonlinear solver should be input.

/IMPL/NONLIN/n
L_A Itol Tol

L_A

This parameter sets the maximum number of iterations for reforming the stiffness matrix; a value of 3 for iterative solver and a value of 6 for direct or mixed solver is recommended.

Itol

Criteria used for run termination.

1

Relative residual in energy

2

Relative residual in force

Tol

Tolerance value; iteration is considered to be converging if the relative residual value (residual value versus reference value) is equal to or less than the tolerance.

The reference values are computed at zero iteration (Output Messages).

With Radioss, updated stiffness matrix has the sense mainly in geometry (using elastic parameter for nonlinear materials); therefore, a small value for L_A will provide faster convergence, depending on the displacement increment level, but with more computation cost for stiffness matrix reforming; that is especially true with direct solver.

Usually, stop criteria in force (Itol =2) provides a better result on balance, which is the default criteria. Criteria in energy might converge easily and is better suited for the simulation of elasto-plastic materials under monotonically increasing loading; because in this case, energy increases more strongly than the force (which is yield by the plastic admissible stresses), the convergence becomes easier due to the same evolutions of reference values (the higher the reference value easier the convergence).

Second, time step control should be chosen when using the keywords /IMPL/DT/n and /IMPL/DTINI. If a time step control method is not defined, constant time step is used during the nonlinear simulation (not recommended).

To manage time step more efficiently, two automatic time step control methods are available (n=1 or 2). The first method is a line-search method that works only according to converged iteration numbers. The second method is an arc-length like displacement control method and is recommended for general use.

When automatic time step control is used at each step (cycle), the Radioss solver automatically adjusts the time step with the input scale factors. If the iteration diverges, Radioss will scale down the time step and then restart the iteration.

The default scaling factors are 0.67 (for decreasing factor) and 1.1 (for max increasing that is maximum factor by which time step will be increased).

Using a max increasing factor closer to one, for example: 1.01, will enable easier convergence for difficult analyses, like buckling.

One should also define an initial time step using the keyword /IMPL/DTINI. This provides an approximate number of steps needed for the simulation.

Restarting Radioss is also available with implicit analysis. In this case, different parameters can be defined for converging strategies.

Nonlinear Analysis with Contact

The relative force residual (default) is recommended for Nonlinear Analyses with contact.

Like Explicit Analysis, a larger gap for contacts leads to better convergence. This is especially true for interface TYPE11, where a sufficient gap value has to be set in order to avoid termination of computation due to decreased time step. For simulations with contact (for example: initial state of stamping under gravity, parts constrained by contacts) using interface TYPE7 with a small initial gap, defining Gap_min slightly larger than the initial gap will lead to better convergence. The initial penetrations will recover quickly.

If contact is defined with friction, then incremental stiffness formulation (I_form =2) is recommended.

Since it is difficult to choose an appropriate reference value in analyses with contacts (especially in simulations involving rigid parts with imposed displacement impacting a deformable part), Radioss makes an exception by modifying the reference value in the first iteration. If the relative residual becomes too large (>>1), Radioss will restart the iteration with a smaller time step and a higher reference value. The modified reference value is sometimes arbitrary and too high, so you should examine this value (printout at zero iteration at each step), as this may lead to convergence with the wrong result. This could also be true when high initial penetrations are present in an interface definition.

When interface TYPE7 is used, the contact stiffness plays an important role in convergence and therefore, I_stf = 4 (which takes the minimum of main and secondary stiffness's for contact) is recommended. This is due to the reason mentioned in the previous paragraph and also because the penalty contact force will be balanced with the internal force of deformable impacted part. That means the stiffness near the effective stiffness one will converge easier than a higher one. Sometimes, a stiffness with a scaling factor reduction (for example: Stfac 0.01) or reduction in impactor thickness (if rigid one) might reduce unbalanced forces and improve convergence, particularly in shell structures under bending where the effective stiffness is much lower than membrane stiffness; but it should be noted that too low of a value could also lead to divergence.