Materials used in a naval collision calculation with finite element software

Collisions and groundings have a significant contribution to structural damages occurring to ships. For collision calculation are used non-linear relations between strains and deformations, considering a significant difference between the initial shape and final deformed shape of the structure, and the mechanical equilibrium equations are written on the deformed shape of the structure. Using a mechanical test to a material sample will result the connection between the engineering strain and engineering deformation. During numerical simulation, we are using the real mechanical characteristic curve, which represents the reliance between real strains and real deformations, those being calculated from the distorted material sample. For calculation, we are using Johnson – Cook plasticity model, frequently used by other authors as well during collision calculation. There is included new information, also tabular calculations using specific formulas, resulted during carried out studies, to establish the model parameters considering the measured data or using information from another material model (exponential law). Considering the materials used within ANSYS software and calculus processor LS-DYNA, are presented types of materials useful for collision calculation, describing the elasticity, plasticity and yielding. Following, it is used a procedure for dynamic explicit calculus because it is suitable for solving of nonlinear systems. During simulation with finite element of the collision, there are no strains and deformations concentrations and it is necessary to generate an artificial curve, which leads to same results, as in reality and as well finite element analysis.


Introduction
For the numerical simulation of ships' collision, it is usually used the finite element method. In order to employ this method, it is necessary to have, among other things, information about the behaviour of used materials that is as realistic as possible. During the collision process the material is subject to large deformations and possibly fractures and, therefore, the description of the materials could be rather complex. The behaviour of a material is described using the strain-deformation curve (characteristic curve). A first shape of this curve is obtained by measuring. From the mechanical testing on a material sample will result the connection between the engineering strain and the engineering deformation (conventional characteristic curve). Engineering strains and deformations are calculated on the initial shape of the material sample and therefore the conventional curve is not used in simulation. Numerical simulation uses the real mechanical characteristic curve which represents the dependence between real strains and real deformations. The real curve is deducted from the conventional curve by using simple conversion relations. The real strains and deformations are calculated on the distorted material sample. The real curve thus determined is correct until necking occurs (until the ultimate test strength or the ultimate engineering tension). In order to obtain the real characteristic curve for deformations larger than the necking deformation, additional calculations are necessary, such as simulations with the finite element method of the testing process. In order to have a complete description of the material it is necessary to define the fracture deformation or an algorithm for the progressive reduction of the material rigidity, which leads to fracture.
Numerous causes can lead to errors in the calculation results. Following are mentioned some of the causes: a. wrong mathematical model b. wrong approximation with finite element c. wrong implementation in the software d. wrong communication between the software and operating system e. the user filled in wrong data f. the user is interpreting wrong the results given by the software. Causes a and b depend on theoretical models used, c and d depend on the way in which the software was made and only e and f depend on the knowledge and skills of the user. Quality of the software can be checked only comparing the results of the calculations with results measured on real structures tested during collisions. In this way can be checked the whole modelling process starting with mathematical model used and ending with results interpretation provided by the software.
Because of the large costs involved, there is a limited number of tests carried out on real structures. If we will discuss about automobiles, where series are larger and costs of the tests are relatively reduced, finite element software is used to optimise the shape of structure and in the end there are done also tests on real structures. But for the vessels, where the series are small with tremendous costs involved during tests, mostly there are used simulations with finite element to establish the collision resistance. In order to identify the quality of the software used for the collision calculations, usually there are used relatively simple structures, made of stiffened plates, which are very similar to the plates of the vessel's side plate.
For the research purpose, there were used calculations and measurements from structures used in the existing literature and also the results of own calculations. In the existing literature there were used modified versions of a general use program. Most of the general use programs allow the advanced users (researchers) to modify them and to add new material models. This operation is not accessible to an ordinary design engineer. Taking into account that in this paper we want to check if the activity of collision calculation can be done in similar condition as an any other finite element calculation, we preferred to use predefined material models within the software database.

Material failure modelling
The behaviour of ship's structure during collision depends, to the largest extent, on the fracture of the hull and frame. These fractures take over the largest part of the energies that arise in the collision process [1]. As such, when performing simulations through calculi, it is important to use correct information about the materials' behaviour in the non-linear calculus and, especially, realistic failure criteria. When analysing the ship's strength to collision the most important parameter is the critical energy, namely the energy necessary to break the shell or the bottom or to break the double board or the double bottom, as the case may be. This critical energy is essentially dependent on the fracture deformation (yielding) [1]. In [1] it is shown that the doubling of the fracture deformation leads to (approximately) the doubling of the critical energy. The fracture of a structural element is a very complicated process which is influenced by material's features, strain, building process, environmental conditions, operation mode, etc. In the case of a finite element analysis, the fracture depends additionally on the fineness of the discretization, the elements' shape and type, etc.

Constant yielding deformation
The Germanischer Lloyd engineering guidelines [2] recommend the use of the constant yielding deformation (the actual plastic deformation) in the collision calculus, with the value: This low value (1) implies the acceptance of some reduced plastic deformations before the fracture. In correspondence to this deformation, the structure subject to collision can absorb only a small quantity of energy. A major disadvantage of this rule resides in the fact that it does not take into account the structure's finite element discretization. The calculus has shown in practice that there is a strong connection between the structure's discretization and the yielding deformation.

Yielding deformation dependent on discretization
Calculus simulation is performed using the finite element method and the fineness of discretization influences the results (deformations and strains). When the fineness of discretization is increased, so are the deformations in the most stressed areas of the structure (in the "stress concentrators"). This is a normal phenomenon, where the increase of network density leads to results that are closer to reality. The increase of network density also causes the increase of the calculation effort, which means that it would be preferable to obtain realistic results (as confirmed by tests) by using finite element networks as rough as possible. According to an empiric rule known in this field, by reducing the elements' dimension by half, one can increase the computation time by 8 times. Typical discretization used to simulate ship collisions employs elements having a side comprised between 0.1 m and 1 m [3]. For the sake of comparison, when simulating automobile collisions, are used finite elements with the side comprised between 6 and 10 mm, given their fairly reduced dimensions. Typically, the ratio between the elements' side length and their thickness is comprised between 10 and 60. In conclusion, it is preferable to use a limit deformation which depends on the finite elements discretization. Sequel to numerous tests, it is proposed the relation for the yielding deformation computation with shell type elements [4]: where f H is the yielding deformation, t is the thickness of the shell, and l is the elements' dimension.
Although still not perfect, the relation expressed in formula (2), reflected in figure 1 is extremely useful, especially if the program used to compute does not provide other means to treat material yielding.  (3) To the same purpose, Kitamura [3] proposes a rather similar way to calculate the shell yielding deformation, represented in figure 2, which actually shows the evolution of yielding deformation based on elements' length.
where , , , , A B C n m are constants which depend upon the material and can be determined by measurements. The first parenthesis in relation (4) refers to quasi-static behaviour, the second contains the influence of the deformation speed, and the third to the influence of temperature. The following denotations are used: , . The relation for computing the yield stress was proposed by Johnson and Cook [5], and their paper presents constant material examples, as well as the description of practical procedures used in order to establish the material constants.
where , 1,2,...,5 i D i are material constants and * V is the ratio between pressure and actual stress (the stress triaxiality factor):   The Johnson-Cook material model, detailed in table 1 can be applied to most metals and is valid with both high and low strain rates and even in the quasi-static case. Typical applications are: study of explosion effects, ballistic penetration, impact. table  2 and table 3 it is presented the computation of Johnson-Cook model parameters used in the collision calculations presented in this paper.   Figure 3 represents the corresponding curve .

Estimation of Johnson -Cook model parameters
To model the materials used in the computations presented by Hagbart S. Alsos et al [7,8], a modified exponential law was used. In this paper ANSYS and LS-DYNA computation programs are used. None of these programs has the respective materials implemented by default. In principle, LS-DYNA allows the addition of material models and this is what the authors of the article have done [2,3]. This implies FORTRAN coding and program recompilation naturally followed by testing. Such approach is typical of research activity. Here, we would like to find out if the collision calculus can be carried out with the available instruments, without altering them. Namely, we would like to establish if engineers who only have basic skills of using finite element software could perform a collision calculus. As such, instead of adding a new material model to the LS-DYNA material library, we will prefer to use an already existing material.

Estimation of model parameters starting from an exponential law
The Johnson-Cook model will be used from the LS-DYNA material models library and, therefore, its parameters will be estimated starting from the exponential law parameters used by Hagbart [7,8]. The issue can be approached in several ways, but the easiest way seems to be the use of the method of nonlinear least squares. As such, we will presume we know the exponential law parameters [7,8]: Using this relation, we can compute the levels: Parameter A has the value: where c V is a stress yield (initial). It is fairly easy to recognize the problem of the nonlinear least squares. The problem is easily solved, for example in Excel, by using the component "Solver add-in".
Calculus setting in Excel is expressed as in table 4: Table 4. Parameters of material model computed using an exponential law. [6] Excel computation of parameters   The graphics of the two curves is expresses in figure 4: To sum up, the hardening curve expressed by relation (13) To shed more light to the issue, it is then estimated the stress and plastic deformation corresponding to the beginning of necking, also known as ultimate plastic stress and strain (or fracture stress and strain in strength of materials course books). Necking is characterized by the condition (of maximum): Next, the EXCEL sheets presented in tables 6 and 7, are used to determine the stress 0u V and the engineering ultimate strain 0u H :

Material models implemented in ANSYS and LS-DYNA
In ANSYS a large number of material models are predefined and the software also contains a library of material constants. The selection of material models has also taken into account the fact that the collision calculus generally uses shell type elements and, consequently, the number of models offered by ANSYS is reduced. For example, to model a fracture, it can only be used the real fracture plastic strain with its alternatives, as presented further in this chapter. LS-DYNA has almost 200 predefined material models but, if a selection is made for their use in the collision calculus for ships modelled with shell type elements, the number of these models is greatly reduced. ANSYS models are essentially enough for an engineering collision modelling. Surely, both programs allow the description of new material models.
3.2.1. Elasticity. To describe elastic behaviour in ANYS, the option "Linear elastic" is used, within which "Isotropic Elasticity" is selected, if the material has an isotropic behaviour. This is the standard option when working with metallic structures. Isotropic linear elastic behaviour is described by the longitudinal elasticity model E and the Poisson coefficient Q . Based on this data the software computes the bulk modulus and the shear modulus. Alternatively, it can be used the orthotropic material model, described by three each longitudinal elasticity moduli, shear moduli and contraction coefficients, nine material constants in total.

Plasticity.
In order to describe the plastic behaviour in ANSYS, several material versions can be used.
1. Bilinear material model with isotropic hardening. Parameters , c A V are introduced, as defined by the simplified hardening curve: where c V is the yield stress, p H is the plastic strain, a Ais the plastic modulus (also called tangent modulus). It should be noted that the kinematic hardening model couldn't be used with shell elements.