# Engine Error Messages

## MASS OR ENERGY ERROR DUE TO CONTACT

**WARNING MINIMUM TIME STEP    0.248E-04 IN INTERFACE       11(DTMIN=  0.2500E-04)
REMOVED SECONDARY NODE 63086879 FROM INTERFACE

MESSAGE ID :         206
**  RUN STOPPED : ENERGY ERROR LIMIT REACHED

***  NODE WITH HIGHEST MASS CHANGE
Description:

In several cases, the simulation can fail with ERROR termination because too much mass is added to maintain a constant time step for the contact.

Why does mass need to be added to maintain stability of the contact?
• Time step is constant when /DT/NODA/CST, /DT/NODA/CST2 or /DT/INTER/CST are used.
• Interface time step is computed as $\text{Δ}t=\sqrt{\frac{2m}{K}}$
Stiffness increases in function of the penetration $K={K}_{\text{0}}\frac{Ga{p}^{2}}{{\left(Gap-p\right)}^{2}}$ .
As the penetration in the contact increases, stiffness increase leads mass to be increased to maintain time step constant.
For example, the tire stack up against the rigid barrier. Behind the tire, the brake disk (or caliber) compresses the tire against the barrier. The global contact is not stiff enough and leads to large penetrations.
• Stiffness increased
• Mass is added to maintain time step constant
Suggestion for Resolution:
A typical solution for this problem is to create a local contact with a higher gap and stiffness. Increasing the initial stiffness leads to a smaller time step at the beginning of the penetration, but it will increase the time step, if the penetration is large.

Contact between two rigid parts is possible with interface TYPE7 and TYPE11 or TYPE19. The main issue is that it will generate deep penetrations in the contact, which can lead to mass being added to maintain the timestep to the value specified in /DT/NODA/CST or /DT/NODA/CST2.

There are two solution to resolve this type of issue:
• Switch at least one of the parts to deformable
• Add a local contact with a higher gap and stiffness

## MASS OR ENERGY ERROR DUE TO HIGH DISTORTION

***  NODES WITH HIGHEST VELOCITY

***  NODES WITH HIGHEST MASS CHANGE
Description:
When there is very large plastic deformation, the simulation can become unstable and fail with ERROR termination, due to energy error or mass error.
Suggestion for Resolution:
Based on the results, there are different ways to resolve this issue:
• Define proper strain failure
• Material may be incorrect (unit system) or type (plastic instead of steel, yield point is too low…)

Initially, there is an intersection that generates the local distortion. To resolve this issue, correct the intersection and define proper strain failure in the material.

## RIGID BODY BECOMES UNSTABLE

WARNING ID :          542
** WARNING RIGID BODY INERTIA
DESCRIPTION :
-- RIGID BODY ID : 713264
-- RIGID BODY TITLE : NULL
UNPHYSICAL INERTIA :
PRINCIPAL INERTIA 150.0050404753 IS GREATER THAN THE SUM
OF THE 2 OTHER ONES 0.60340391378794E-02 + 0.3645995262784E-02
Description:

When the rigid body inertia is not physical, the rigid body can become unstable. When the rigid body inertia is not physical, Radioss will print the warning in the Starter.

If those warnings are not corrected, the following can occur:
• The rigid body becomes unstable and is propelled at a very high speed in the vehicle
• The rigid secondary nodes are still in the global contact and will generate unrealistic deformation
• Numerical issues as the impact velocity is very high (>1500 m/s)
Suggestion for Resolution:

Correct the unphysical rigid body inertia.

## NEGATIVE INERTIA OR STIFFNESS

NEGATIVE INERTIA ON NODE ID=823767293
Description:
This issue typically occurs more often in Radioss v12.x than more recent versions (2017.x). It occurs when the node of an interface TYPE2 projects outside of the closest main segment. The error is not related to the height of the secondary node relative to the main segment, but that its projection is outside of the main segment.
A warning in the Starter is printed for the nodes that project outside of the main segment.
WARNING ID:          345
** WARNING : CHECK TIED INTERFACE
DESCRIPTION :
-- INTERFACE ID : 557392358
-- INTERFACE TITLE : CONNECTION.37
8238684 2 823767497 823767293 823767296 823767504 -1.279664112565 -0.9934883789504 0.7066172931858
Use HyperCrash Model Checker to check “Secondary nodes no proj.” which allows to identify the nodes that project out of the closest main segment.
Suggestion for Resolution:
There are several ways to resolve this issue:
• Remove the nodes that project outside the closest main segment from the interface TYPE2
• Translate the nodes so that they do not project outside the segment anymore