I'm currently trying to run a ballistic impact simulation on Kevlar composite plates on ABAQUS CAE through the dynamic explicit simulation. However, each time I try to run my simulations, this error will appear and I am left with aborted simulations. Additionally, the properties of my Kevlar material may be inaccurate especially with the Hashin Damage properties.
Can anyone assist with this issue?
Dear Danial Sharudin
This can occur due to the high load rate or size of components that are defined as deformable. This error generally occurs in analyzes in which the material undergoes many deformations.
To fix this error, preparations must be taken so that the elements do not deform too much during the "job" solution. Using the following tips can help:
1-Minimizing the size of the elements and changing the meshing techniques of the structure in such a way as to increase the quality of the created elements can help to completely solve the analysis.
2-Changing the order of the elements from 1 to 2, although it significantly increases the amount of analysis and space occupied by the computer's RAM, it is one of the easiest ways to increase the probability of completing the analysis.
3-In some cases, it is possible that the level of calculated strains may be so high that the material enters the area of its damage, and to continue the analysis from a certain point onwards, the damage criterion for the material must Have been defined. Failure to define the appropriate onset and growth criterion of damage is one of the common mistakes of Abacus users that can cause this error.
4-In cases such as some shaping analysis in which increasing the mesh density and increasing the order of the elements alone do not complete the analysis, the Arbitrary Lagrangian-Eulerian adaptive meshing algorithm can be properly defined for "parts" with high deformation. To a large extent, led to the completion and advancement of the analysis. using this technique in simulation, like other solutions, increases the analysis time.
Dear Danial Sharudin , I don't have access to ABAQUS right now, however, if we ask Dr. @Nils Wagner, he might have time for helping you.
if there are excessive element distortion warnings in the message file the mesh pattern has a mismatch with the design geometry. These messages are issued in the message (.msg) file, when the volume at an integration point of an element becomes negative. When parts and assemblies are used, error messages involving element and node numbers report these numbers in terms of the part instance. When troubleshooting excessive element distortion warnings, consider the following: • Check the deformed shape for the last converged increment. Is the mesh refinement reasonable considering the deformation in the element that is distorting? If not, try refining the mesh in the areas of large deformation. • Are the elements hourglassing? Check Hourglassing to identify the causes and what to do about them. • Check the model definition including boundary conditions, loading, and material properties. The problem could also be due to contact overclosures. • If the error occurs in the first increment and the model contains contact pairs or tie constraints, have the slave nodes been adjusted to lie on the master surface? If nodes on the slave surface are adjusted onto the master surface by an amount that is significant compared to an element length, the elements may be highly distorted after the adjustment.
- Badges
- Science topic