10
Finite element modelling of cohesive crack propagation using crack-bridging rupture elements
S Hadidi-Moud [1], A D Crocombe [2] and G Richardson [3]
Mechanical Engineering Department, Ferdowsi University, Mashhad, Iran
Abstract
Due to the extensive use of adhesive materials in structural bonding on one hand and the lack of a unified design tool for failure prediction in such structures on the other hand, development of failure prediction techniques has received much interest in recent years. A series of rupture elements have been developed and used to representing the process of failure initiation and propagation in elastic and elasto-plastic continua. The rupture elements form a line of crack bridging elements along the assumed crack extension path and are integrated into a 2-D finite element model. The user-defined elements are incorporated into the analysis using subroutine UEL called by ABAQUS finite element commercial code.
Pre-cracked compact tension, C(T), specimens of bulk adhesive E27 and double cantilever beam, DCB, specimens with Aluminium substrates and a 1mm thick adhesive E27 binding layer have been used in an extensive fracture testing programme and the results are used to validate the predictive models. The proposed models are then discussed in the framework of conventional fracture mechanics and compared with the well-established linear elastic fracture mechanics (LEFM) and elasto-plastic or “non-linear” fracture mechanics (NLFM) procedures.
Keywords: cohesive crack propagation; rupture modelling; Finite element; Adhesive materials
10
Introduction
Force controlled interface elements [1,2] have been used to model crack propagation in an elastic continuum. Direct failure prediction in an elastic continuum, following crack initiation and its subsequent propagation, has been achieved by use of strain tripped elements with energy based unloading [3 - 5]. Related work on energy based modelling of crack propagation [6] and the use of crack bridging displacement controlled elements in modelling de-lamination in composites [7] can be found in the literature. Development of a local damage based approach to modelling crack propagation and predicting the corresponding failure load has been discussed in this work. The suggested model has been assessed through the comparison of its prediction with the experimental results from this work and previous tests carried out on pre-cracked compact tension specimens made from an epoxy adhesive.
First the experimental programme carried out to provide data for assessment of the predictive models is briefly explained. Second, different rupture elements developed to model progressive crack extension are introduced together with their limitation of application. The user elements are then integrated into the finite element model of fracture specimens to predict the conditions of failure. Details of finite element simulations are briefly described and the results of the analyses are demonstrated. The model predictions are compared with the experimental data. Finally the strengths and weaknesses of the proposed models are discussed in relation to their use in predicting failure initiation and /or propagation in bulk adhesives and adhesively bonded structures.
The experimental programme
The experimental work includes manufacturing and testing of bulk epoxy adhesive flat tensile, F(T) compact tension, C(T) and double cantilever beam, DCB joint specimens. The results of flat tensile tests are used to characterise the non-linear constitutive response of the adhesive continua. Fracture data, obtained from C(T) and DCB tests together with results from previous research, where cleavage fracture specimens were tested, are used in the assessment of the proposed rupture models.
Development of rupture elements
The load-displacement behaviour of the rupture elements is shown in Figure 1. A range of user elements are developed and used to predict the conditions of failure initiation and/ or propagation. The rupture elements are initially rigid-like and represent connectivity along the crack line. The system is then loaded in a quasi-static manner. Once
the condition of the continuum is reached a critical state (i.e. strain reaches a specified value representing a level of continuum plasticity) the rupture element is allowed to loose rigidity (tripped) and extend freely while the load acting on it is dropping to zero representing the release state. A convergence algorithm is used to prevent analysis instability at the turning points of the stiffness of the rupture elements (i.e. tripping and release stage). The line of elements along the crack extension path are tripped and released subsequently throughout this process in a sequential order (progressive propagation). The applied load to the system at this stage is referred to as the failure load. Various unloading schemes shown in figure 1 have been considered and discussed. Potentially the rupture elements used to predict the failure load of a pre-cracked component are also applicable to a non-cracked model and similar analyses can be used to predict the onset (initiation) of fracture. Three types of rupture elements are briefly described.
· Strain tripped rupture element with no unloading (type 1)
This rupture element follows the load-displacement scheme of figure 1(a). The element’s stiffness is set to zero when the critical continuum strain is reached. The rupture element will then continue to extend at a constant load, corresponding to the tripping condition. This represents crack opening but does not include unloading and release states. Using a series of rupture elements of this type along the crack line of a CT specimen model, an alternative solution to the conventional LEFM has been achieved. The area under the curve (ER) represents the energy absorbed by these elements. The element definition is illustrated in figure 2.
· Strain tripped rupture element with energy based unloading (type 2)
A direct representation of the process of crack propagation and failure prediction can be achieved by including unloading and release in the rupture element definition. The scheme of figure 1(b) absorbs a critical value of energy (ER) during unloading. The element itself is quite similar to that of figure 2.
· Strain tripped rupture element with time based unloading (type 3)
Use of the previous types of rupture elements in modelling progressive crack propagation in an elastic-plastic continuum, generally results in a non-sequential release of the elements thus causing an irregular crack front opening profile. This phenomenon, referred to as “locking”, is due to the dependence of the level of plastic deformation around the crack tip area on the loads acting on the rupture element. Studies indicate that the unloading curve may not be controlled independently in presence of plasticity. To overcome this problem a rupture element using the multi-step time based unloading profile as shown in figure 1(c) has been developed. This element uses an average strain based on nodal displacements to detect the tripping condition. This element simulates the process of progressive crack propagation and yet it has a much simpler structure compared with the other element types as shown in figure 3.
Characteristics of rupture elements
Type 1 local damage based rupture elements are used to predict the failure load in an elastic continuum while rupture elements type 2 are also capable of representing the process of failure initiation and propagation in the presence of plasticity. It has been shown that in the case of an elastic continuum this approach is an alternative representation to the conventional LEFM virtual crack closure technique with the additional advantages of visualising the process of progressive crack propagation and direct calculation of the failure load. Using the rupture elements rather than the conventional fracture mechanics, one can also predict the onset of fracture. Investigations have revealed that with elastic-plastic continua, the unloading process cannot be controlled independently but it is also governed by the continuum conditions. Therefore, the definition of the rupture element has been modified. The result is the rupture element type 2, a strain controlled element whose behaviour is decided by the strain state ahead of the crack extension path. Validation of these elements in failure prediction is verified through their application to a pre-cracked C(T) specimen model made of epoxy adhesive E27. The predicted failure loads are found in very good agreement with the experimental results. The validation of the elements type 1 and type 2 however is limited to symmetric models failing under mode-I fracture only. These limitations have been addressed by introducing the generalised rupture element type 3. This element is tripped at a specified critical strain parameter of the continuum to which it is incorporated and follows a time-based unloading scheme. The strain parameter is calculated from the incrementally updated elements’ nodal relative displacement vectors, projected along the element direction. Details are shown in Figure 4. This would result in a generalised version of the element that is applicable to non-symmetric models and may also be used for failure prediction under mixed mode loading. This model could also represent progressive crack propagation along the assumed pre-specified path.
The local damage based rupture element has been used to interfacial failure prediction in adhesively bonded structures. The modelling technique accounts for material plasticity and is applicable to both cracked and non-cracked problems under mode-I and mixed mode quasi-static loading. Experimental data obtained from extensive tests of standard fracture specimens, as described earlier, have been used to validate the developed technique.
Description of Finite Element models
The FE model of continuum C(T) specimen
The CT specimen model of an epoxy adhesive under mode I loading for which experimental data was obtained in previous research has been used in this work. The continuum is modelled using 8-node quadrilateral elements and a refined mesh has been applied to the crack tip area with the smallest element size equal to around 1.5 mm.
To validate the proposed model a line of rupture elements have been incorporated along the adhesion- substrate interface of a cleavage fracture specimen model consisted of Aluminium substrates bonded by an epoxy adhesive. A Drucker-Prager material model using the results obtained from tensile tests carried out on the bonding adhesive in previous research and confirmed by others has been used. The FE analysis has been performed for mode-I and mixed mode configurations using the cleavage specimen model.
The FE Model of Cleavage joint specimen
The finite element model of the cleavage test specimen is shown in figure 5. The model consists of aluminium substrates bonded with a 2 mm-thick layer of Permabond E27 epoxy adhesive. Using PATRAN pre-processor, a localised refinement scheme has been generated at different crack lengths along the interface as shown in figure 5. The continuum element used for both the adhesive layer and the aluminium substrates was the 4-node quadrilateral plane strain element as defined in ABAQUS element library. An exponent Drucker-Prager material model was used to model the non-linear response of the adhesive layer whereas the response of the aluminium substrates was considered linear elastic.
The Rupture Element
The 3-node rupture element, type 3, has two nodes connecting the crack faces and a third node that is coincident with a node in the continuum. The element structure and its correlation with the continuum elements is shown in figure 6. The algorithm used in the development of the rupture element is described in figure 7.
The Element Implementation
A series of rupture elements incorporated into the finite element model along the assumed crack line (the upper interface) are used to model progressive crack propagation. A calibrated tripping strain is used for failure prediction in cracked and non-cracked specimens under mode-I and also in mixed mode loading. To assess and validate the predictive technique, experimental data is compared with the model predictions. Figure 8 shows the deformed model with the crack length of around 3 mm. The extended crack from the initial tip at 3 mm towards the end of the refined mesh (where the rupture elements are incorporated), can be seen in figure 9.
Analysis of results
Failure modelling in elastic continuum
The rupture elements of type 1 and 2 have been used to model crack propagation in the CT specimen described above. A series of the rupture elements, forming a line of crack bridging elements, have been integrated along the assumed crack line in the continuum model and non-linear finite element analysis has been performed. Figure 10 shows the formulation used to calculate the energy release rate from the results of the analysis of the model that uses rupture elements of type 1. The critical value (fracture energy) is compared with the result of LEFM crack closure technique in table 1. The good correlation validates the proposed solution. Using the rupture energy with the energy based unloading-release scheme (type 2), a direct prediction of the failure load has been achieved and the process of progressive crack propagation in the elastic continuum has been successfully presented as illustrated in figure 11.
Failure modelling in plastic continua
Using rupture elements of type 3 the technique could provide promising results in failure prediction within an elasto-plastic continua. An exponent Drucker-Prager model is used for this purpose. A physically justifiable presentation of progressive crack propagation has been obtained as shown in figure 9.
Finite element analyses have been also carried out for Non-cracked and pre-cracked (for a range of crack lengths) cases for each configuration and results have been compared well with available results reported elsewhere [2,6].
The user routine “Rupture element” has been developed based on the algorithm shown in figure 7 using Fortran programming language. In the element definition two nodes (i.e. nodes 2 and 3) span the potential crack line whilst nodes 1 and 2 are used to calculate the average strain in the continuum from the co-related nodal displacements. A very high stiffness is introduced into the element to represent the connectivity of the crack surfaces through nodes 2 and 3. This situation remains until the average strain in the direction normal to the crack reaches a specified level representing the level of continuum plasticity. The assigned stiffness is then removed and the element is unloaded over a very small time period. The fully unloaded element represents the material rupture.
Mode-I Analyses
To calibrate the tripping strain, a number of analyses using different tripping strains were performed and the failure predictions were compared with the experimental failure load. Using the calibrated values of tripping strain, finite element analyses were performed for the cleavage model with rupture elements incorporated along the crack line. The analyses were repeated for a number of locally refined crack tip locations (corresponding to a range of crack lengths from 0.0 to 3.0 mm). Mode-I predicted failure loads were obtained. Results, showing the variation of the normalised (based on experimental failure load for mode-I non-cracked specimen) experimental and predicted failure load with the crack length, are plotted in Figure 12.