Springback analyses are sometimes numerically difficult to solve. Some typical causes of convergence difficulties and actions you can take to resolve them are listed below.
Dynamic effects due to a high punch speed used in the explicit (LS-DYNA) run.
Use a lower punch speed in the explicit run. You can do this by redefining the tool speed in the explicit analysis (EDLOAD command).
Slenderness of the structure; the ratio of part size to its thickness is large.
A more refined mesh may reduce this slenderness effect.
The model contains local instabilities: the part, being very thin, tends to wrinkle along edges or sharp curvatures.
Use a refined mesh to accurately model curvatures of the formed part.
The model is improperly constrained.
Verify the boundary conditions in the springback analysis. This requires some engineering judgment on how and where to apply the boundary conditions in the springback phase. When the tools are removed, the part should be free to move except for restraints against rigid body movement. It is important to simulate this carefully in the finite element model. A commonly recommended approach is to use displacement constraints at a minimum of three non-colinear nodes. One node should be restricted from motion in all directions, another node should be restricted from motion in two directions, and the last node should be restricted from motion in only one direction. You must select these three nodes carefully so that the expected springback behavior is not prevented. The magnitude and direction of the displacements in the springback analysis should be viewed as relative quantities to the plane formed by these three nodes.
If you have checked all of the above conditions and the analysis is still not converging, try the following methods (in the order listed):
Attempt incremental springback by using a higher number of substeps.
Use a linear springback analysis (if such an approximation is acceptable) with the command NLGEOM,OFF.
Invoke springback stabilization (which is described below).
If convergence difficulties persist, you should activate springback stabilization
using the SPSCALE and MSCALE
arguments of the RIMPORT command. The stabilization method is
analogous to attaching artificial springs to all unconstrained degrees of freedom.
The stiffnesses of these springs are directly proportional to the stiffnesses of the
elements.
In each substep, ANSYS will assign the artificial springs large default stiffnesses to simulate a total restraint of the motion of the model at the beginning of each load step. The artificial stiffness is scaled down exponentially with the progress of iterations. (The picture below illustrates rapid decline of artificial spring stiffness over an iterative cycle.) The substep is considered to be converged only when the equilibrium convergence tolerances are met (as in a normal nonlinear analysis) and the artificial stiffness has reached an insignificantly small value. This may slow down the conversion of the solution in some cases; however, the benefit is more robust behavior of the model.
The SPSCALE parameter on the RIMPORT
command is a scale factor that you input to scale (up or down) the default initial
stiffness of the springs. (You must input SPSCALE to
activate springback stabilization.) You can also specify an acceptable small
stiffness value using the MSCALE parameter on the
RIMPORT command.
The springback stabilization method is valid only when the geometric nonlinear option is active (NLGEOM,ON).
