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, 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.
  • An animation file before run terminates. This is very useful to identify areas:
    • Where the velocity is out of range (>> 100 m/s)
    • Mass is getting added
    • Deformation is excessive (check plastic strain)
    • Stress is unrealistic (> 2 Gpa)
      In HyperView, review the animation and check visually for any obvious issues:
      • Velocity is not applied to all the nodes of the vehicle
      • Incorrect boundary conditions
      • Missing connections (seatbelt is not connected properly, etc.)
      • Review basic contours:
        • von Mises Stress: check for values that are out of bounds
        • Added Mass: check for very big mass
        • Velocity: check for very big velocity In many cases, the nodes with the highest velocity or high mass added will be in the same area.
  • A point in the T01 file. This is useful to identify:
    • The part which have sudden increase in internal/kinetic energy. Plot the internal and kinetic energy of all the parts in HyperGraph (you need to put all the parts in time history).
    • Plot global energy balance to identify, if the divergence is due to the internal energy, kinematic energy, external work force.
  • Information at the end of the listing file (_0001.out).

    For example, in the case below, the information provided at the end of the _0001.out is very useful in trying to understand the area of the model causing the simulation to stop.

    The solver reports:
    • Which parts have the highest kinetic (1) / internal energy (2)
    • Which nodes have the highest velocity (3) / mass change (4)


    Figure 1.
    For example, in the case below, before the simulation fails with an error termination, the following message may be printed in the _0001.out: 
    CYCLE    TIME      TIME-STEP  ELEMENT          ERROR  I-ENERGY    K-ENERGY T  K-ENERGY R  EXT-WORK MAS.ERR
62100   18.53     0.2985E-03    SOLID      230440718     -1.3%    0.3484E+05  0.1313E+06     109.7   1523.       
RUPTURE OF SOLID ELEMENT NUMBER 230025298
	DELETE CONNECTION SOLID ELEMENT 110010956, ENERGY= 4.732011155E-05
RUPTURE OF SOLID ELEMENT NUMBER 230024559
**WARNING MINIMUM TIME STEP	0.5976E-05 IN INTERFACE NB	2300040(DTMIN=	0.1000E-04)
SECONDARY NODES NB       230373002  230373019
MAIN NODES NB            230373003  230373004
	DELETE SECONDARY LINE FROM INTERFACE
    An initial intersection causes high distortion and eventually ERROR termination.


    Figure 2.
    For example, in the case below, the run is killed, due to contact with a rigid causes the ERROR termination. The output file prints:


    Figure 3.


    Figure 4.
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).