# Removing failed elements from mesh in Abaqus model

This tutorial demonstrates how to remove failed elements from the mesh of a finite-element model developed using Abaqus/CAE (Standard/Explicit). Specifically, the focus will be on the interaction between metals in a penetration-type problem using the Johnson-Cook plasticity and damage models for ductile metals. Although there are options in Abaqus/CAE to turn element deletion on and remove elements from the computational grid based on some damage criteria, additional contact properties must be specified within the input file so that interior elements of the target that were not initially exposed to the penetrator are assigned a proper contact algorithm. The tutorial assumes that the reader has some experience using Abaqus, so some elementary aspects of building a model are not described in detail.

## Scenario

This problem consists of a cylindrical object (called penetrator or projectile) impacting a disk (called plate or target). The penetrator is 0.58 inches long, has a radius of 0.2475 inches, is traveling at a speed of 3,000 fps, and is composed of 4340 steel. The target is 0.2450 inches thick, has a radius of 6.0 inches, is fixed in space, and is composed of A36 steel. To minimize the number of elements in the problem, a quarter symmetry was assumed.

## Model setup

The FEA model has two deformable solids subjected to a dynamic event and solved using explicit integration. Although both parts are composed of different materials, most of the same parameters are used to define their material behaviors. These include their density, isotropic modulus of elasticity, Poisson's ratio, and a rate-dependent plasticity that uses Johnson-Cook hardening parameters. The A36 steel plate has additional information for its Johnson-Cook damage model, which makes use of a linear damage evolution based on a zero fracture energy. This approach is consistent with Iqbal et al[1]. All of the information used to specify these parameters are obtained from Johnson and Cook[2] for the 4340 steel, and from Seidt et al[3] for the A36 steel.

Given that this is a quarter symmetry problem, symmetric boundary conditions are specified in the two faces of both parts that are aligned with the two planes of symmetry. Moreover, the outer circumferential face of the plate is restricted so that it does not rotate or displace. A predefined velocity of 36,000 inches per second in the direction of the target is specified for the penetrator, which is offset 0.01-in. from the plate. This velocity is applied during a dynamic and explicit step lasting 3.0e-4 seconds.

In the initial setup of the problem, surface-to-surface contact is specified between the projectile (first surface) and the plate (second surface), which controls the tangential and normal behavior between them. Because of the relatively small thickness of the plate, a friction coefficient of zero is assumed. These definitions are modified to allow the projectile to erode the plate upon penetration. To achieve this behavior, interior surface specifications have to be manually added to the input file because Abaqus/CAE does not support this feature. The lines that are specifically modified to allow this behavior are mentioned in the Input File section.

The mesh consists of C3D8R elements, 8-node linear hex bricks, with reduced integration and enhanced hourglass control. The number of elements for each part is chosen so that the plate has at least 4 elements through its thickness. The resulting mesh has 36652 elements for the plate and 135 elements for the projectile. Also, in the element type window, Element Deletion was turned on for the plate part. For the projectile, this was left as "default".

Finally, two sets are created on the "Assembly" module. The first one, called "Set-1", includes both parts. This particular set is important and necessary, as it will be used when adding the extra lines to the input file to allow the erosion on the plate. The second set, called "Set-2", is composed of a single node at the top of the penetrator to allow one to track its velocity.

At this point, we are ready to export the input file and manually edit it.

## Input file

The resulting input file can be obtained here.

There are 3 sections in the input that need to be modified. Two of the modifications are keywords that need to be added, while the third one is just commenting out two lines.

1. Immediately before the *End Assembly keyword, the following lines need to be added:

 ```*Elset, elset=Set-1, instance=Part-1-1, generate 1, 135, 1 *Elset, elset=Set-1, instance=Part-2-1, generate 1, 36652, 1 *Surface,type=element,name=surf1 , Set-1,interior ```

Notice that Set-1 is a set composed of all the elements of the projectile (Part-1-1) and the plate (Part-2-1). Recall that the projectile and plate have 135 and 36652 elements, respectively. Also, a new set is created called surf1 that will be referenced in the next modification.

2. Right after the *Bulk Viscosity keyword (including 0.06, 1.2), the following lines need to be added:

 ```*contact, op=NEW *contactinclusions surf1, *contact controls assignment, nodal erosion=no ```

Notice that the "surf1" set created in the previous step is referenced here.

3. Finally, the following two lines need to be commented out under the ** INTERACTIONS section:

 ```*Contact Pair, interaction=IntProp-1, mechanical constraint=KINEMATIC, cpset=Int-1 _PickedSurf45, _PickedSet46_CNS_ ```

By commenting them out, these lines become:

 ```**Contact Pair, interaction=IntProp-1, mechanical constraint=KINEMATIC, cpset=Int-1 **_PickedSurf45, _PickedSet46_CNS_ ```

Notice that only one asterisk (*) is added to the first line (**Contact Pair...) to comment it out.

The resulting modified input file can be obtained here.

## Afterword

As can be seen in Figure 1, the projectile erodes the elements of the plate upon impact. Note that, although the simulation was done for a quarter symmetry model, the animation is mirrored about one of the orthogonal axes for visualization purposes, resulting in what looks like a half-symmetry model.

Additionally, there are two things that the user should be aware of when modeling this type of problem:

1. Mesh-dependency: this problem is highly mesh-dependent. If one is investigating the effect that the impact velocity has on the residual velocity, a mesh convergence analysis should be performed so that an appropriate mesh is selected. For the sake of this tutorial, a coarse mesh was used to speed up the calculations although it was not the most optimal one.

2. Damage evolution: Abaqus has different options for specifying the Johnson-Cook damage evolution. The two main types are displacement-based and energy-based. For both of these, one can specify their corresponding value at failure. Additionally, one can specify the softening behavior as being linear, exponential or tabular. Moreover, the degradation can be specified as maximum or multiplicative. For the sake of this tutorial, a zero energy-based damage evolution was specified. As mentioned before, this is consistent with Iqbal et al[1].

 Figure 1: Animation of projectile penetrating a plate showing von Misses stresses.

## References

1. 1.0 1.1 M.A. Iqbal, S.H. Khan, R. Ansari and N.K Gupta. 2013. "Experimental and numerical studies of double‐nosed projectile impact on aluminum plates."
2. G.R. Johnson and W.H. Cook. "Fracture characteristics of three metals subjected to various strains, strain rates, temperatures and pressures". Engineering Fracture Mechanics, Vol. 21, No. 1. 1985.
3. J.D. Seidt, A. Gilat, J.A. Klein, and J.R. Leach. "High strain, high temperature constitutive and failure models for EOD impact scenarios". SEM Annual Conference & Exposition on Experimental and Applied Mechanics. 2007.