9.3 Common Issues

In this section we take a look at some of the most common problems you may run into when solving a finite element problem with FEBio. We'll discuss possible causes of and solutions to these issues.

Inverted elements

When an element inverts, the element becomes so distorted that in certain areas of the element the Jacobian becomes zero or negative. In order to obtain a physically realistic solution, the Jacobian of the deformation must be positive at all points of the domain. Thus, when a negative Jacobian is found in an element, FEBio cannot continue. Fortunately, FEBio's automatic time-stepping algorithm can usually circumvent this problem by cutting the time step back and retrying the step using a smaller time step. In addition, FEBio will recalculate the global stiffness matrix. The combination of a reduced time step and a refactored stiffness matrix will often be sufficient to overcome the negative Jacobian. However, when it is not, you may have run into a more serious problem. These are some of the common causes that may require additional user intervention.

By default, when FEBio encounters inverted elements, it will print an error message stating that “negative jacobians” were detected. You can request FEBio to print out a detailed list of the inverted elements, by setting the output_negative_jacobians configuration flag in the FEBio configuration file. (see 7)

Material instability

At large deformations, some materials can become unstable. This is usually caused by a softening of the material at large deformations. When the material softens too much the global stiffness matrix can become ill-conditioned and FEBio will not be able to find the correct solution. Unfortunately, there is no easy solution around this issue and you may need to consider using a different constitutive model.

Time step too large

Although the auto-time stepper will automatically adjust the time step in case of trouble, it is designed to work within user defined limits and sometimes they are not set properly to solve the problem. The most common issue is that the minimum time step is set too large. Cutting back the minimum in addition to the initial time step can often help in preventing negative Jacobians.

Elements too distorted

When elements get too distorted they might not be able to deform any further without inverting the element. In this case, it may be necessary to adjust the mesh in the area where the elements are inverting.

Shells are too thick

A shell is an element where it is assumed that one dimension is much smaller compared to the other two directions. When the mesh is really fine, this assumption may no longer be valid and it could happen that the shell becomes too thick. When a shell gets too thick it can create negative Jacobians in the out-of-plane integration points, especially in areas of high curvature. To overcome this, you may need to remesh the affected area, adjust the shell thickness or even replace the shells with solid elements.

Rigid body modes

A rigid body mode is a mode of deformation that does not alter the stress in the body. Uniform translation or rotation of the entire model are two possible rigid body modes. In the presence of a rigid body mode, the solution is not uniquely defined and FEBio will most likely throw negative Jacobians. The solution is to identify the rigid body mode and to eliminate it by applying additional constraints to the model.

Failure to converge

FEBio uses an iterative method to solve the nonlinear finite element equations. This means that for each time step the solution for that step is obtained by a succession of iterations, where each iteration brings the model (hopefully) closer to the solution for that step. An iterative method requires a convergence criterion to decide when to stop iterating and FEBio uses no less than three criteria. (In biphasic and multiphasic problems additional convergence criteria are used for the pressure and concentration degrees of freedom.) The convergence norm for each of these criteria is defined by the user in the control section of the input file.

Sometimes it happens that FEBio cannot converge on a time step. We'll take a look at some of the most common causes in the next following sections. Also take a look at possible causes of element inversions above. Sometimes, the issues that cause an element inversion may also manifest themselves in convergence problems before the element actually inverts.

No loads applied

Perhaps surprisingly, when no loads are applied, FEBio will often struggle to find a solution. The reason (and solution!) is simple. Although no loads are applied, FEBio still performs many calculations and due to round-off errors, the result of these calculations may render the convergence norms not exactly zero. FEBio then tries to apply the convergence criteria to these really small norms and again due to round-off error will not be able to satisfy the convergence criteria.

FEBio can actually detect this situation. It looks at the residual norm and when this is smaller than a user-defined limit it assumes that no loads are present and moves on to the next time step. However, this limit is actually problem dependent and it can happen that for your particular problem the limit is set too small. In that case, the solution is to increase the limit. This can be done by setting the _min_residual parameter in the Control _section of the input file. For example,

<min_residual>1e-15</min_residual>

If the residual norm now drops below this value, FEBio will consider the time step converged and move on to the next time step.

Convergence Tolerance Too Tight

In some cases, the default convergence tolerances are too tight and FEBio will not be able to converge. In that case, adjusting the affected convergence norms is a possible solution. This is done by editing the corresponding norms in the Control section of the input file. However, this should only be done when no other cause can be identified for the convergence problems.

Forcing convergence

It is possible to force a time step to converge. This can be done by interrupting the run (using ctrl+c) and then enter the conv command at the FEBio prompt. This will force the time step to converge and FEBio will continue with the next time step. This is not a recommended practice as the solution may become unstable and in fact it is unlikely that FEBio will be able to converge any of the following time steps. However, it can be useful in some scenarios. For example, if there is no load applied in the initial time step and FEBio has trouble getting past this initial step (see Section No loads applied) or when you want to store the current state to the plot file without having to rerun the problem in debug mode (although the plot command or debug command might be better alternatives).

Problems due to Contact

When contact interfaces are defined, convergence problems can often be traced back to problems with the contact interfaces. See Section Guidelines for Contact Problems for more details on how to properly use contact interfaces in FEBio.