Printer Friendly

Industrial Framework for Identification and Verification of Hot Spots in Automotive Composite Structures.

1. Introduction

The automotive industry has relied on numerical simulation using finite element analysis (FEA) for decades. Ever since the improvements of the TRIA3 and QUAD4 elements in FE solvers in the early 1980s [1], together with introduction of tools to transfer geometries, e.g. IGES, between different computer-aided systems in the early 1980s [2], numerical simulations as we know them to today have become the working horse in the analysis and sizing of automotive structures. In the late 1980s, crash simulations in FE environments became available [3, 4]. Over the last decade, even more interest and resources are spent on FEA to not only cover analysis and sizing but also virtual verification as this is more economical and faster compared to traditional testing. The ever shorter lead times for development of car platforms and models require focus on fast methods to be able to drive the design process.

Today, analysis of metal and plastic structures is performed using complete car models or models of large subsystems, e.g. the body in white (BIW), complete door structures or front ends. Such models are addressed to ensure accurate boundary conditions and load distribution in the structure. The models are built using subshell elements due to their computational efficiency. The assumption made with conventional shell elements, based on Mindlin-Reissner [5] or Kirchhoff-Love [6] theory, that the normal stress component can be ignored and therefore a plane stress state is predicted is justifiable for ductile isotropic materials, e.g. metals and conventional polymers.

The assumption of a plane stress state that is traditionally made for sheet metal structures in the automotive industry is not applicable to laminated composite structures. For sheet metal structures, subjected to complex load cases in automotive bodies, the normal stress components are still small compared to the strength of the material. However, for laminated composites, especially non-crimp fabric (NCF) reinforced composites where the strength in the normal direction is only about a percent of the fibre tensile strength [7], the use of models based on plane stress can be detrimental as even very small out-of-plane stress components can be detrimental and have been found to cause failure [7, 8, 9]. The use of such highly orthotropic materials in structures with complicated geometry and loading conditions will increase the risks in design further. That is, complex geometries and loads tend to cause high out-of-plane normal and shear stresses [10]. As composite structures often are integrated and subjected to multiple loads, it becomes difficult to assess critical areas with very simplified modelling techniques. Composite designs in the automotive industry tend to be more complicated in shape compared to what have been used within aerospace. Such geometries often show more complex stress states even under simple load cases compared to less geometrically complex structures. In this article we explore a methodology which allows for efficient and reliable design of automotive composite structures.

1.1. Analysis Strategies

Different approaches to ensure that critical failure modes are not missed in the design of a structure can be used. The easiest way is to use conservative design guidelines that can eliminate certain failure modes. However, as this leads to excessive use of expensive materials, adds weight and limits the freedom in design, it is an undesirable approach.

Another approach is to incorporate the building block approach [H] used by the aerospace industry, illustrated in Figure 1 (a). Knowledge from experimental tests and simulations on each level is gained and combined to drive design at that level. This is then done in a bottom-up approach for each level from coupons to the complete structure at the full-scale level. This approach is very time-consuming as testing and simulation are done in parallel, with no guarantee that the simulation models are predictive as the level is increased. Also, during the design process, all load cases on the complete structure level need to be transferred to lower levels of complexity, which can significantly complicate modelling and testing. The advantage with the building block approach is that models used in simulation only need to capture the failure modes that are detected from physical testing at the corresponding level. This can simplify the modelling significantly, as all physics does not necessarily need to be captured.

During the last decade, advanced non-linear models have been introduced in the aerospace industry to better capture the behaviour of large structures. In parallel more detailed models of coupons and elements have been developed that can better capture the failure behaviour of composites. In the Wishbone framework [12], these methods are applied at multiple scales, breaking down the full assembly to lower scales, using sub-modelling to drive the lower scale models. This gives the behaviour of the structure at different scales of modelling. In order to accurately predict failure onset, detailed models of materials, features like a joint, etc. are built and validated at increasing scale. In the Wishbone analysis framework [12], these types of models are combined. Accuracy in predictions is verified by comparison to results from physical experiments at each level. By this approach, illustrated in Figure 1 (b), confidence in design can be reached at a minimum of physical testing [12].

Comparing the two approaches, the building block approach yields simpler modelling and simplification of features, but the true physics is easily missed when moving up in the pyramid. As relevant failure criteria are needed, all loads and constraints need to be transferred through different modelling steps. As the Wishbone framework utilise more complex models, possibly including non-linear effects, it is much easier to apply the actual forces and constraints that act on geometries as these are used directly from the global models without simplifications through different scales of modelling.

1.2. Objectives and Limitations

To assess large and complex structures, there is no simple and straightforward element formulation readily available where a large number of load cases can be analysed using a set of state-of-the-art (SotA) failure criteria. In this study, we propose an efficient analysis approach for automotive composite structures, which is adapted to contemporary industrial tools and uses existing analysis methods in concert. In this analysis framework, different modelling techniques are used to address different parts of the building block pyramid (see Figure 2). However, the same set of failure criteria is used on all levels. The proposed design framework uses a top-down approach in terms of analysis of structures, to avoid unwanted simplifications in loads and boundary conditions. The approach uses a screening step to identify potentially critical locations. Subsequently, these locations are analysed using higher-fidelity models to examine the detailed stress states. The proposed framework is first illustrated for a simple test coupon and thereafter applied to a real car structure. The purpose of the application to a real structure is not to assess the actual structure but to illustrate how the proposed process can be used. For this reason, a detailed information about the structure and the loads is omitted.

The proposed framework is developed from a durability perspective in terms of analyses. This means that the focus is on first ply failure in the structure. Hence, the analysis process does not consider progressive failure and is therefore not pertinent for use in crash simulations. The framework is developed for laminated composite materials made from continuous fibres, e.g. tape-based and NCF composite systems.

The proposed analysis process uses tools readily available to the industry. In this work, Ansa [13] and Metapost [14] are used as pre- and post-processing tools for FE models, and Abaqus [15] is used as solver. The process can be defined for several software and is not limited to those used in this implementation.

2. Method for Detailed Analysis of Hot Spot in Composite Structures

Critical locations found in the global model need to be addressed in a systematic way. To analyse these in greater detail, the loads need to be captured as the model is refined. This global-local approach combines knowledge from different levels (i.e. length scales) in the building block pyramid [11] in a fashion similar to the Wishbone analysis framework [12]. This allows for an efficient approach where large assemblies can be used for the evaluation of structural composite components.

The proposed framework consists of three different parts for complete assessment of the full structure. These are shown in Figure 3. The first part concerns screening of the structure for potential hot spots. In the second part, detailed models of these locations are created using a model of higher fidelity than that used in the global analysis. The third part is a postprocessing step to ease analysis of the results from the higher-fidelity model to evaluate the design.

A detailed view of each part in the process is given in the following sub-sections, where the different tasks are discussed in detail and input/output from each task is specified.

In order to assess multiple hot spots in an efficient way, automation of the proposed framework is of uttermost importance. Furthermore, a highly automated process guarantees the quality of results independent of user and allows for introduction of updates to the process when needed.

To illustrate the proposed analysis process, an out-of-plane test specimen is used. This type of specimen was proposed by Jackson and Martin [16] for the determination of the interlaminar tensile strength of a unidirectional (UD) composite. The specimen is illustrated in Figure 4 together with the applied loads. The specimen is made from a UD layup of AS4/3501-6 [16] composite material. Elastic properties are given in Table 1 and strength data are given in Table 2. The dimensions of the specimen are chosen such that out-of-plane failure is triggered at the centre of the 90[degrees] bend [10]. The specimen has an inner radius of 5.0 mm and a thickness of 3.0 mm with an applied load of P = 839 N.

2.1. Global Model for Efficient Hot Spot Identification

To make the process as efficient as possible, it is important to consider the potential need for subsequent generation of high-fidelity local models already when creating the database for the global model, i.e. in the Ansa file of the built model. The global model is created as a shell model based on the middle surfaces of the geometry. In this sub-section, the different tasks for generation and analysis of the global model are outlined, following part (A) in Figure 3.

The laminate layup is defined using a ply-based [18] modelling approach. Thus, it is easy to define and keep track of layers and to apply material directions. The material directions should preferably be based on manufacturing process simulations [19] to include effects from draping and compaction in the structural analysis. As the database will be reused for subsequent detailed local analysis, with a different modelling strategy, it is important to keep the middle surface and apply the laminate to the geometrical definitions in the model.

The difference in the global model, proposed here, compared to standard global models used in the industry is that second-order elements are used. The reason for this is the Extended 2D FEM approach, proposed by Rolfes et al. [20]. that is used to predict the full 3D stress state requires this. The full 3D stress prediction is done in a post-processing step considering the global displacement results. Finally, the mesh size follows the guideline from Molker et al. [10], which takes the laminate thickness and curvature into account. For the current geometry, this gives an element size of 2.0 mm.

2.1.1. Failure Prediction in the Global Model Most SotA set of failure criteria considers the influence of out-of-plane stresses, e.g. LaRC05 [21], Cuntze [22] and Carrere [23], all among the top ranked criteria in the WWFE-II [24]. To use such set of criteria in the global model, the full 3D stress state is needed. As stated above, the Extended 2D FEM approach proposed by Rolfes et al. [20] is used to extract the 3D stress state. This is done in task Al, Figure 3. The advantage is that this post-processing can be applied to the deformation results from a standard shell-based global model, with the prerequisite that second-order shell elements are used. A more detailed description of hot spot identification using the Extended 2D FEM approach in combination with failure prediction can be found in [10].

The hot spot identification is done using a SotA set of failure criteria in task A2, Figure 3. The set of failure criteria should be applicable to the material system used; e.g. for transversely isotropic materials, LaRC05 can be used [21], and for orthotropic materials, LaRC05NCF can be considered [25]. The most important thing is that the chosen set of failure criteria is able to predict all potential failure modes that may occur in the material.

The Extended 2D FEM approach for the full stress tensor is not available in the solver of the commercial CAE tools used. Furthermore, the chosen set of failure criteria is not available within the post-processor. Therefore, the stress recovery and the failure initiation prediction are made outside the commercial tools. The predicted failure initiation data, i.e. failure index, fracture plane, failure mode, critical ply and the stress state, achieved in the external tools are exported as an ASCII file that can be read by the post-processor for visualisation. These predictions are performed using Matlab.

Failure Initiation Criteria. In this work the LaRC05 [21] and LaRC05NCF [25] are suggested for transversely isotropic materials and orthotropic materials, respectively. LaRC05 is a physically based set of criteria that addresses five different failure modes for first ply failure: fibre tensile failure, fibre compressive failure (fibre kinking or fibre splitting) and intra-laminar matrix failure (tensile or compressive). The set of criteria is based on the current 3D stress state at each location and is evaluated at a number of potential fracture planes. The resulting stress state at each fracture plane is then used to evaluate the different failure modes.

Matrix related failure in the transverse direction, illustrated in Figure 5 (a) for tensile loading and Figure 5 (b) for compressive loading, is governed by the properties of the matrix material. Both tensile and compressive matrix failures are combined to one criterion for matrix related failure [FI.sub.M] as found in LaRC05 [21]:

[mathematical expression not reproducible] Eq. (1)

where [< >.sub.+] denotes the Macaulay bracket and differentiates between tensile and compressive normal stresses on the fracture plane. The tractions on a potential fracture plane, [[tau].sub.T], [[tau].sub.L] and [[sigma].sub.N], are compared to the allowable [], [] and [] taking in situ effects into account [21]. Friction stress from the micro-cracks on the fracture plane is calculated from the normal stress, [[sigma].sub.N], and a friction coefficient in the transverse, [[eta].sub.T], and longitudinal directions, [[eta].sub.L].

Fibre tensile failure, shown in Figure 5 (c). is governed by the strength of the fibres and the stress in the fibre direction, [[sigma].sub.11]. The failure index for fibre tensile failure [FI.sub.FT] is evaluated according to the criterion:

[mathematical expression not reproducible] Eq. (2)

where [X.sub.T] is the strength measured in the 1-direction.

Fibre compressive failure exhibits two different failure modes, fibre kinking, illustrated in Figure 5 (d), and fibre splitting, illustrated in Figure 5 (e). These are in fact matrix controlled failure modes and occur at a misaligned fracture plane denoted with superscript "m". The criterion for fibre kinking [FI.sub.KINK] and [FI.sub.SPLITT] is evaluated in LaRC05 [21] as

[mathematical expression not reproducible] Eq. (3)

The two failure modes are predicted with the same criterion, given in Equation 2. The distinction between fibre kinking and splitting according to Equation 3 is empirical in LaRC05. Fibre kinking and fibre splitting are distinguished with the magnitude of the fibre direction stress according to Equation 4.

[mathematical expression not reproducible] Eq. (4)

where [[sigma].sub.11] is the stress in the fibre direction, and [X.sub.C] is the measured compressive strength.

The most critical failure mode and failure index are then determined by the maximum of all calculated failure indices, given by Equation 5.

FI = max([FI.sub.M], [FI.sub.FT], [FI.sub.KINK|SPLITT]). Eq. (5)

LaRC05NCF [25] is used for orthotropic NCF reinforced composite materials. In addition to the failure modes in LaRC05, a failure mode for interlaminar failure is evaluated, and this is illustrated in Figure 6.

Interlaminar matrix failure is driven imperfections and defects between the fibre bundles in the normal direction in NCF reinforced composite materials [25]. For transverse failure in the out-of-plane direction that occurs within the matrix interface (MI), the following criterion is used:

[mathematical expression not reproducible] Eq. (6)

where [Z.sub.T] is the measured out-of-plane tensile strength. This is evaluated under pure tensile loading for a fracture plane [alpha] = 90[degrees].

2.1.2. Hot Spot Identification Based on the failure initiation predictions, potentially critical areas (alias hot spots) are found identifying all elements with a failure index exceeding a certain threshold. This is done in task A3 in Figure 3.

These elements are presented to the analyst together with a default sub-model volume in task A4 in Figure 3. This is illustrated in Figure 7. This task is not made as an automatic task for two reasons. Firstly, all marked elements may not be relevant. Some stress concentrations may be inherent to load introduction and boundary conditions and must be neglected. Other regions, which are complex and poorly resolved in the global model, may need to be manually marked as potential hot spots for further analysis. Information about the location of each hot spot and the proposed size are exported to a common ASCII file in task A5 (see Figure 3) for the remaining operations in the process.

If the two external tasks in the first step are not performed, and the hot spot identification is based on results available in Abaqus [15] (using the set of criteria proposed by Hashin [26] and a 2D stress state), potential failure modes will be missed. This is illustrated in Figure 8 where the same L-beam is analysed and failure initiation predictions from Abaqus [15] and from LaRC05 [21] based on stresses calculated with the Extended 2D FEM approach [20].

The results from Abaqus predict fibre compressive failure in the innermost ply with FI = 0.08, while the proposed approach with Extended 2D and LaRC05 predicts intralaminar failure at a ply close to the middle, FI = 1.00.

2.2. Analysis of Identified Hot Spots

The analyses of the identified hot spots are performed using sub-modelling. Sub-modelling is a technique that has been available for more than 20 years [27]. Similar approaches have recently been proposed for analysis of composite aircraft structures [28]. The main reason for not utilising sub-modelling to a greater extent in industry is that it is labour intensive.

Man-hours needed to create the new detailed models are often more critical than computer time. To overcome this, the process of creating sub-models is automated and follows the procedure outlined by Moller and Sundlo [29] developed for isotropic materials. In this sub-section the process is modified to fit layered composite structures, following step B in Figure 3.

2.2.1. Creation of Sub-model Volume The creation of the sub-models is done using the database for the global model. This is to make sure that the same geometry and laminate data are used for both the global and local models. The same procedure is applied for all identified hot spots. The different sub-models are solved independently, which allows for parallelisation of the analyses to reduce the total time of the process.

In the process of creating the sub-models, intervention by the analyst is required for some of the tasks. Manual operations are required as the hot spot can be located in an area of complex geometry, where decisions on how to cut out the model must be made by the experienced stress engineer. Furthermore, inclusion of loads and/or joints with other parts is important to consider. For these reasons, the sub-modelling task does not lend itself to a fully automated process. To ease manual work, the proposed sub-models are visualised together with the global model so that the selections can be changed by the stress engineer. After this step, all accepted sub-models are created one by one as described below.

In these following automatic tasks, B3 to B6, a sphere with the same size as the sub-model is created. The sphere is intersected with the geometry of the global model. Only the original surfaces within the sphere are kept. These surfaces are meshed according to mesh criteria suited for the local analysis, based on reasonable aspect ratio compared to the ply thickness and the total thickness. The total thickness needs to be considered as the elements on the outer radius will have a larger aspect ratio than elements at the midsurface where the shell mesh is created. The local model is built with first-order elements. When the mesh is created, the material orientations defined in the global model are recreated. This ensures that the local model represents the global model for the laminate definition. After this, the shell elements are volumised according to the stacking in the laminate definition with one solid element over the thickness for each ply, either with hexahedral or pentahedral elements (C3D8 or C3D6). The choice of the element type for the solid elements maybe sensitive to the overall deformation. For example, elements as the C3D8 undergo locking under bending, and in such cases elements with reduced integration, e.g. C3D8R, are a better choice. The solid elements are assigned their orientation based on the default material orientation, combined with each ply orientation. This includes draping effects from manufacturing simulations if such are available. This means that each element will have its own orientation defined in an orientation table [15].

2.2.2. Application of Composite Data and Boundary Conditions In the next task, B7, in Figure 3, the boundary conditions are applied to the sub-model. This step again requires interaction by the analyst. The reason is that inside the sub-model volume loads may be applied or several parts may be connected, e.g. co-cured parts [30], clips, screws, etc. All such joints need to be addressed individually to ensure an accurate description and that all loads are introduced in the sub-model.

All nodes on the bounding faces of the sub-model are used as driven nodes, as shown in Figure 9. These faces are the ones that originate from the perimeter of the middle surface used for the shell modelling.

Loads applied inside the sub-model volume in the global analysis must be added to the local model. This is also the case for connections to other parts positioned within the sub-model volume, e.g. clips, or boundary conditions. These can be handled by including additional nodes to the driven node set [29].

2.2.3. Solution of the Detailed Model The final task in this step, B8, illustrated in Figure 3, is to solve the sub-model. This is done automatically for each local model. Information from the global model in terms of how many load steps are included and where the original model can be found are transferred to Abaqus. These information may comprise information for user materials (UMAT) or user output variables (UVARM) in Abaqus for failure prediction in the local model.

Sub-modelling in Abaqus. Sub-modelling is incorporated into the general capabilities of Abaqus [15]. The global model can be solved using large deformations and non-linear material models. An important thing is to consider what can be found in the global model and that the sub-model is a viable representation of that area. With a local sub-model, it is possible to capture phenomena that were not sufficiently resolved in the global analysis in a subsequent second analysis. For all driven nodes in the sub-model, the boundary conditions are calculated based on the displacements and rotations from the global model. In Figure 10 the flat projection of sub-model node A onto the midsurface of the global element to image node AI, with the vector D connecting node AI with node A is illustrated. The interpolated displacements [u.sub.AI] and rotations [[phi].sub.AI] at AI are then applied to sub-model node A according to Equation 7 [15]:

[u.sub.A] = [u.sub.AI] + [[phi].sub.AI] x D Eq. (7)

The sub-model follows the solution history from the global model. This allows for non-linear results and use of large displacements and/or inelastic deformation results from the global model in the sub-model. In addition to the rotation of the image node in Equation 7. the finite rotations need to be accounted for in the analysis with large displacement according to Equation 8 [15] (see Figure 11). where d is the rotated vector connecting node AI' with node AI.

[u.sub.A] = [u.sub.AI] + d - D For large deformations Eq. (8)

For first ply failure in multidirectional laminates, the strains are typically small, and thereby the inelastic deformations would be very small. This allows for faster simulations even though large displacements need to be accounted for.

To avoid overlocking in the sub-model in the normal direction, a centre zone is defined for the application of the boundary conditions as illustrated in Figure 12 [15]. Sub-model nodes that are within the centre zone are constrained both in directions parallel to the shell and normal to the shell. Nodes outside of the centre zone are only constrained in directions parallel to the global shell element. The thickness of the centre zone is by default 10% of the sub-model thickness.

2.3. Post-Processing of the Sub-models

Results from the sub-models can be hard to interpret as the cut-out volume often is small. One can easily misunderstand the overall global behaviour and even the location of the submodel in the global model. Without this knowledge, it is difficult to draw correct conclusions on why the structure behaves like it does. To overcome this problem, a simple postprocessing scheme is applied where the sub-models are loaded, as shown in Figure 13 (a). Both deformation results (odb file) and composite failure results (ASCII file) for the global model and deformation and failure results (odb file) for the local model are loaded into the same session. By having both models available at the same time, it is easy to switch between them to ease the work for the analyst. In Figure 13 (b), the sub-model is cropped to visualise the global model, and in Figure 13 (c) the global model is made transparent to show the result through the thickness in the local model.

The design is then evaluated based on the results from the local sub-models to determine if it complies with the strength allowable.

3. Case Study of an Automotive Structure

The proposed analysis framework is applied to an automotive structure, shown in Figure 14 (a). The structure is known as the backplate, which is the wall that separates the passenger compartment from the rear trunk space in sedan cars. This part creates support for the rear seat and the parcel shelf. The structure contributes significantly to the car body's torsional stiffness. The structure can also support fixings for seat belts, top tether (attachment point for child seats), speakers, etc. and often has cut-outs for cables, access during manufacturing, etc., which increase the geometric complexity. In this study the backplate is made from a UD AS4/3501-6 [16] composite material. Stiffness properties are given in Table 1 and strength data are given in Table 2. The layup in the structure is an eight ply UD laminate. The material orientation is defined by projecting the global x-axis on all elements in the model. The model consists of ~148,300 second-order elements, 145,000 quadrilateral elements (S8R) and 3,300 triangular elements (STRI65).

The structure is subjected to a point load simulating a belt anchorage and is constrained along the upper and lower edges, as shown in Figure 14 (b). The global modelling of the backplate follows the description in sub-section 2.1.

The resulting failure index predictions according to LaRC05 [21] from the global analysis of the structure are presented in Figure 15. As the current implementation from Molker et al. [10] for the Extended 2D FEM approach does not yet support doubly curved elements, these areas are not analysed. In Figure 15 (a), proposed volumes for each sub-model at the identified hot spots are included. Together with the proposed hot spots, a histogram showing the failure index values is introduced in Figure 15 (b). As this example only serves as an illustration, only the hot spot with the highest FI is analysed with a local model.

The sub-model is created according to the process presented in sub-section 2.2. The hot spot with the highest failure index is analysed, and the results are imported in the global model for common post-processing, as shown in Figure 16 (a). A closer view of the detailed model is shown in Figure 16 (b). In this case, the predicted failure index by the global model agrees well to that predicted by the local model.

4. Discussion

Even if the proposed framework is generic and can be implemented in different commercial software, each implementation quickly becomes unique. This is due to the transfer of information from one program to another through customised scripts and programs running outside of the commercial tools. Also, the ability to create volumised models based on information available in a laminate definition for shell elements can be limited if the geometry is complex.

The simple case of the bending-loaded T-beam in Section 2, used to demonstrate the process, clearly illustrates that there will be differences between the global model and the local detailed sub-models. In the case of the T-beam, these differences are attributed to the small inner radius, which with the chosen thickness requires an even finer mesh to be more accurately resolved in the global model. This can be seen in the study by Molker et al. [10], where the effect of the model resolution of the global model on predicted out-of-plane stresses is assessed and explained.

The case with the car backplate reveals some difficulties in how a complex geometry can be volumised using the selected tools and in some cases becomes a manual task. Volumisation is often developed for visualisation in pre-processors rather than creating really detailed meshes used in analyses. Creating volume elements from shells is not always as easy as just to follow the normal direction. For geometries with small radius compared to the thickness, more advanced procedures allowing for different resolution in the in-plane direction for different plies may be needed. These will then require other constraints, e.g. TIE constraints, rather than common nodes to connect the plies. If this is not done, the aspect ratios on the outer radius can become too large.

4.1. Threshold for Local Analysis

In Section 2.1.2, a certain threshold is mentioned to define a cut-off level to identify locations that need to be studied further using local models. As this threshold to a large extent defines the number of sub-models that will be studied, a strategy for selection of the threshold is needed.

In the analysed backplate, two different locations are identified as potential hot spots. The failure indices for each of the locations are found in Figure 16 (b). It is for the analyst to decide if these are to be studied further or not. The knowledge on how well the global model is constructed at the current locations is probably most important to allow the analyst to make this decision. This can be judged based on element size in relation to curvature as described by Molker et al. [10] or the mesh quality.

The quality of the available material data is also important. Similar to the A-basis and B-basis allowable values that are used within aerospace [31], a quantification of the accuracy can be a guide to select the level at which the threshold is to be set. Moreover, certain design allowable values may not be applicable to the structure or parts of the structure. For example, out-of-plane strength is a property that is difficult to measure and may only be valid for certain dimensions, i.e. thickness and/or curvature [32, 33].

Manufacturing simulations can also give insights that affect the selection of the threshold. For example, if an area is likely to have voids, large deviations in fibre angle or fibre wrinkles [19], then the threshold value must be decreased.

5. Summary and Outlook

Failure associated with out-of-plane failure modes is difficult to predict in global FE models as these often are built using shell elements, where the out-of-plane stress components are neglected. Neglect of the out-of-plane stresses can lead to an unpredicted stress component causing failure. Complex geometries and intersection of features are often cumbersome to model in global models. The creation of midsurfaces for such areas can be complicated, and the mesh quality, or representation of the geometry, is often compromised. However, building and solving detailed solid models are far too time consuming. To overcome this, a framework for analysis of complex composite structures is proposed where the global structure is screened for potential hot spots, which are subsequently analysed in detailed local FE models made from solid elements.

The proposed analysis framework is based on tools available in commercial software. Key in the analysis framework is a certain degree of automation, which guarantees that all points are analysed in the same way, independent of the analyst. However, the most important aspect of the semi-automated process is that it allows for many potential hot spots to be analysed in parallel as the user interaction is very limited. This allows for very fast analyses, even if many hot spots are identified.

The parts that are not yet available inside commercial tools are solved using Matlab functions. These functions read the model information and the results from the global model. The output is ASCII-based result files for common commercial post-processors. Incorporating these parts into the commercial tools is the most important future work to simplify the process.

The proposed methodology is developed with the intent to be a semi-automated and integrated part of the development process for composite structures at Volvo Cars. This is by combining existing bricks, aligning and connecting them with appropriate mortar. The idea is then that different bricks can be exchanged to suit other material systems, modelling strategies, etc., while the framework still can be followed.

Contact Information

Corresponding author: Henrik Molker

Phone: +46-72-9774555


The work was partly funded through Volvo Car Industrial PhD Program (VIPP) and the Swedish Research Council (VR), project no. 2012-4320. In addition, financial support from VINNOVA, via LIGHTer Academy, is gratefully acknowledged.


[1.] Mac Neal, R.H., "The Evolution of Lower Order Plate and Shell Elements in MSC/NASTRAN," Finite Element Analysis and Design 5:197-222, 1989, doi:10.1016/0168-874X(89)90044-9.

[2.] Nagel, R.N., Braithwaite, W.W., and Kennicott, P.R., "Initial Graphics Exchange Specification IGES Version 1.0," Nagel, Roger N. Internet Archive, 1980.

[3.] Car Crash Simulation|Make Software, Change the World! |Computer History Museum, n.d., (accessed March 18, 2019).

[4.] Benson D.J, "The History of LS-DYNA[R]," 2006, Livermore Software Technology Corporation, (accessed Mar. 21, 2019).

[5.] Mindlin, R., "Influence of Rotatory Inertia and Shear on Flexural Motions of Isotropic, Elastic Plates," ASME Journal of Applied Mechanics 18:31-38, 1951.

[6.] A.E.H., L., "On the Small Free Vibrations and Deformations of Elastic Shells," Philosophical Transcription of the Royal Society 17:491-549, 1888.

[7.] Bru, T., Hellstrom, P., Gutkin, R., Ramantani, D. et al., "Characterisation of the Mechanical and Fracture Properties of a Uni-Weave Carbon Fibre/Epoxy Non-crimp Fabric Composite," Data in Brief 6:680-695, 2016, doi:10.1016/i.dib.2016.01.010.

[8.] Paul, P.C., Saff, C.R., Sanger, K.B., Mahler, M.A. et al, "Out of Plane Analysis for Composite Structures," in 8th Department of Defence (NASA) FAA Conference on Fibrous Composite in Structural Design Part 1, NASA Technical Report N92-32527, NASA Langley Research Center, 1990, 263-279.

[9.] Olsson, R., "Experimental Observations on the Orthotropic Transverse Strength of Non-Crimp Fabrics Composites [TN15006],"Pitea, 2015.

[10.] Molker, H, Gutkin, R., Pinho, S., and Asp, L.E., "Hot Spot Analysis in Complex Composite Material Structures," Composite Structures 207:776-786, 2019, doi:10.1016/J.COMPSTRUCT.2018.09.088.

[11.] Rouchon, J., "Certification of Large Airplane Composite Structures, Recent Progress and New Trends in Compliance Philosophy," in Proceeding 17th ICAS Conference, Stockholm, Sweden, 1990, 2, 1439-1447

[12.] Ostergaard, M.G., Ibbotson, A.R., Roux, O.L., and Prior, A.M., "Virtual Testing of Aircraft Structures," CEAS Aeronautical Journal 1:83-103, 2011, doi:10.1007/sl3272-011-0004-x.

[13.] "Ansa Pre Processor Users Guide. 18.0.x," Luzern: BETA CAE Systems, 2017.

[14.] "Meta Post Processor Users Guide. 18.0.x," Luzern: BETA CAE Systems, 2017.

[15.] "ABAQUS Documentation. 6.14," Providence, RI, USA: Dassault Systemes, 2014.

[16.] Jackson, W.C. and Martin, R.H., "An Interlaminar Tensile Strength Specimen," NASA Technical Report 19960026751, 1993.

[17.] Soden, P.D., Hinton, M.J., and Kaddour, A.S., "Lamina Properties, Lay-Up Configurations and Loading Conditions for a Range of Fibre-Reinforced Composite Laminates," Composite Science & Technology 58:1011-1022, 1998, doi:10.1016/S0266-3538(98)00078-5.

[18.] Stelzmann, U. and Hormann, M., "Ply-Based Composite Modeling with the New *ELEMENT_SHELL_COMPOSITE Keyword," in Proceeding 8th European LS-DYNA Users Conference, Strasbourg, 2011.

[19.] Klintworth, J. and Long, A.C, "The Use of Draping Simulation in Composite Design," In: Long A.C, editor. Composites Forming Technology. First Edition. (Cambridge, Woodhead Publishing, 2007), 277-292, doi:10.1533/9781845692537.277.

[20.] Rolfes, R., Rohwer, K., and Ballerstaedt, M., "Efficient Linear Transverse Normal Stress Analysis of Layered Composite Plates," Computers and Structures 68:643-652, 1998, doi:10.1016/S0045-7949(98)00097-2.

[21.] Pinho, S., Darvizeh, R., Robinson, P., Schuecker, C. et al., "Material and Structural Response of Polymer-Matrix Fibre-Reinforced Composites," Journal of Composite Materials 46:2313-2341, 2012, doi:10.1177/0021998312454478.

[22.] Cuntze, R., "The Predictive Capability of Failure Mode Concept-Based Strength Conditions for Laminates Composed of Unidirectional Laminae under Static Triaxial Stress States," Journal of Composite Materials 46:2563-2594, 2012, doi:10.1177/0021998312449894.

[23.] Carrere, N, Laurin, F., and Maire, J.-F., "Micromechanical-Based Hybrid Mesoscopic Three-Dimensional Approach for Non-linear Progressive Failure Analysis of Composite Structures-Part B: Comparison with Experimental Data," Journal of Composite Materials 47:743-762, 2012, doi:10.1177/0021998312460558.

[24.] Kaddour, A.S. and Hinton, M.J., "Maturity of 3D Failure Criteria for Fibre-Reinforced Composites: Comparison between Theories and Experiments: Part B of WWFE-II," Journal of Composite Materials 47:925-966, 2013, doi:10.1177/0021998313478710.

[25.] Molker, H., Wilhelmsson, D., Gutkin, R., and Asp, L.E., "Orthotopic Criteria for Transverse Failure of Non-Crimp Fabric-Reinforced Composites," Journal of Composite Materials 50:2445, 2016, doi:10.1177/0021998315605877.

[26.] Hashin, Z., "Failure Criteria for Unidirectional Fiber Composites," Journal of Applied Mechanics 47:329-334, 1980, doi:10.1115/1.3153664.

[27.] "ABAQUS Documentation. 5.8," Pawtucket, RI, USA: Hibbit, Karlsson &Sorensen Inc., 1998.

[28.] Gigliotti, L. and Pinho, S.T., "Multiple Length/Time-Scale Simulation of Localized Damage in Composite Structures Using a Mesh Superposition Technique," Composite Structures 121:395-405, 2015, doi:10.1016/j.compstruct.2014.11.005.

[29.] Moller, C. and Sundlo, O., "Method for Merging Scales in Finite Element Analyses-Framework for Automated Global/Local Analyses," Chalmers University of Technology, 2017.

[30.] Molker, H., Gutkin, R., and Asp, L.E., "Verification of Hot-Spot in Complex Composite Structures Using Detailed FEA," in Proceeding ECCM18-18th European Conference on Composite Materials, Athens, Greece, 2018.

[31.] Department of Defence, Composite Materials Handbook, MIL-HDBK-17-1F (2002).

[32.] Charrier, J.-S., Laurin, F., Carrere, N, and Mahdi, S., "Determination of the Out-of-Plane Tensile Strength Using Four-Point Bending Tests on Laminated L-Angle Specimens with Different Stacking Sequences and Total Thicknesses," Composite Part A-Applied Science and Manufacturing 81:243-253, 2016, doi:10.1016/i.compositesa.2015.11.018.

[33.] Molker, H., Gutkin, R., and Asp, L.E., "Implementation of Failure Criteria for Transverse Failure of Orthotropic Non-Crimp Fabric Composite Materials," Composite Part A-Applied Science and Manufacturing 92, 2017, doi:10.1016/j.compositesa.2016.09.021.

Henrik Molker and Renaud Gutkin, Volvo Car Corporation, Sweden

Leif E. Asp, Chalmers University of Technology, Sweden


Received: 06 Dec 2018

Revised: 21 Mar 2019

Accepted: 22 Apr 2019

e-Available: 16 May 2019

TABLE 1 Elastic properties of the AS4/3501-6 composite at the
homogenised ply level [16, 17].

[E.sub.xx]   [E.sub.yy]   [E.sub.zz]
(GPa)        (GPa)        (GPa)        [v.sub.xy]   [v.sub.xz]

140.0        11.0         11.0 (a)     0.3          0.3

             [G.sub.xy]   [G.sub.xz]   [G.sub.yz]
[v.sub.yz]   (GPa)        (GPa)        (GPa)

0.4          5.8          5.8          3.9

(a) Assumed transversely isotropic.

TABLE 2 Strength properties of the AS4/3501-6 composite at the
homogenised ply level [17].

[X.sub.T]   [X.sub.C]   [Y.sub.T]   [Y.sub.C]   [Z.sub.T]   [Z.sub.C]
(MPa)       (MPa)       (MPa)       (MPa)       (MPa)       (MPa)

1950        1400        48          200         48 (b)      200 (b)

 [S.sub.L]   [[alpha].sub.0]   ILSS
 (MPa)       (deg)             (MPa)

 78          53                78

(b) Assumed transversely isotropic.
COPYRIGHT 2019 SAE International
No portion of this article can be reproduced without the express written permission from the copyright holder.
Copyright 2019 Gale, Cengage Learning. All rights reserved.

Article Details
Printer friendly Cite/link Email Feedback
Author:Molker, Henrik; Gutkin, Renaud; Asp, Leif E.
Publication:SAE International Journal of Materials and Manufacturing
Date:May 1, 2019
Previous Article:Erosion Wear Response of Linz-Donawitz Slag Coatings: Parametric Appraisal and Prediction Using Imperialist Competitive Algorithm and Neural...
Next Article:A Review on Electromagnetic Sheet Metal Forming of Continuum Sheet Metals.

Terms of use | Privacy policy | Copyright © 2019 Farlex, Inc. | Feedback | For webmasters