Model Debugging

Here are some guidelines to find the origin of computation problems.

First, note that Radioss Explicit Solver allows resolving high nonlinear dynamic problems; a computation may be wrong even if the run does not fail. If the calculation goes to the end, it illustrates a good numerical behavior but not inevitably a good physical response. However, it is required to receive the message "Normal termination" at the end of the Engine output file, to validate numerical resolution procedures.

The validity of results can be demonstrated by satisfying the following conditions:

Numerical stability
Physical behavior
Physical reliability

The numerical stability is ensured if a message "Normal termination" and energy and mass balance are verified.

If the prepared model does not really represent the physical problem, the wrong results may be obtained. To understand the problem, first you need to ask good questions, which should be answered to put in evidence the reliability of results:

How dependent is the result on friction?
How dependent is the model on rupture phenomena?
How dependent is the result on unknown material parameters?
How dependent is the model on other phenomena that are difficult to simulate?

If the results are highly dependent to a given parameter, then the experimental test must be realized to use high precision values for computation.

Note: The best model is that for which you know the values of physical parameters!

Divergence

Divergence occurs when one of the following conditions is observed:

Positive energy error (except for the first cycle)
Negative energy error by more than 15% (except for the first cycle)
Kinematic time step activation in interface TYPE7
Time step given by a rigid body
Unexplained changes in time step
Quick increase of mass

There are three types of divergence:

Quick divergence

Energy error increase is often exponential. The calculation fails in few cycles.

Potential causes are:

Incompatible kinematic conditions
Negative stiffness in spring
Negative stiffness in tabulated material law
Secondary nodes too far from the main surface in interface TYPE2

Late divergence

Time step is too low. The structure is distorted and high penetrations in a lot of interfaces are observed.

Potential cause is the mesh quality

Slow divergence

The final error is not necessarily the cause of divergence.

Potential causes:

For a linear divergence, the cause can be the existence of incompatible kinematic conditions.
For a sinusoidal divergence, it is typically liberated or generated energy (example: initial penetrations and spring stiffness functions).
Too soft of a material can also be the cause.

It is important to find which event triggered the problem. The event just before the divergence needs to be checked. If a strange behavior is observed for a given part, the connected parts and previous events also have to be studied.

Run Problems

Run Stops At Cycle 0: The data is not written in the Engine output file runname_0001.out. This is generally due to bad running procedure when the Restart file cannot be read properly.
Run Stops After Few Cycles: The data is written in the Engine output file runname_0001.out. The origin of the problem can either be the incompatible kinematic conditions (for example: rigid bodies with a common secondary node) or out of bounds values in material or element properties; although, initial penetrations may be the cause.
Run Stops During Computation: First check the required disk space, then the behavior just before and after divergence can be studied. The time step evolution and the energy error need to be observed.
Negative Volume Message: This is mainly due to high deformation of solid meshes. Fully-integrated brick elements are especially affected by this problem which may be caused by a bad interface behavior or bad material definitions. In any case, the use of co-rotational formulation is recommended to avoid bad shear deformation response.; The Stress-Strain Computation Options (/PROP) assumption can be used with /DT/BRICK/CST to avoid negative volumes (refer to Time Step and Finite Elements for more details about this option).