Keywords

1 Introduction

Due to lack of space in vehicle compartments, an automotive PEM fuel cell stack is normally mounted on its side or mounted horizontally. It is known that this mounting style could cause the slippage among the stack cells during vehicle operations; under certain conditions, cell slippage could be observed as a downward shift in the middle of the stack [1, 2], even hydrogen leak [3], and degradation of catalyst layer in MEA [4]. The assembly design has great impact on the reliability of fuel cell stacks, especially for large power stack with high output voltage. Therefore, it is utmost important to ensure the safe operation of an automotive PEM fuel cell stack by providing a structurally sound assembly design.

There is an increasing demand on high power fuel cell stacks for applications [5], such as mining trucks, ship, high-speed trains, and hydrogen-based power generators. In comparison with the common integration approach involving multiple small stacks, a single PEM fuel cell stack has the advantage of system integration due to simplified piping and matching voltage with inverters. However, for high power stacks, this means an assembly of over hundreds or thousands of unicells which posts challenges in manufacturing and operations. In addition, vibration during operation or shipment [6,7,8] could expose structural vulnerability of these larger stacks, in comparison to smaller stacks [9].

In fact, the stack integrity highly depends on the friction force between the cells which was generated by the stack compression force and surface texture of the connecting cells. When being induced by vehicle road vibration, gravity acceleration could overcome the friction force between the cells and cause the relative shift between the cells. In fact, a study by Hou et al. showed that the hydrogen leakage rate of the stack increased by a factor of 1.5 during the test, and the hydrogen utilization rate decreased by 30.7%, with a maximum decrease of 21.0% in actual efficiency [10, 11]. A sound design principle of fuel cell stacks should be limiting the impact of gravity acceleration with three approaches: by eliminating the space between the cells and side plates, limiting the shape-change of side plates with high strength structural design, and designing stack assembly with lower intrinsic frequencies [12].

Finite element analysis (FEA) is a numerical analysis technique for obtaining approximate solutions to complex engineering problems. A model can be built to replace an object with an assemblage of discrete elements, and then analytically to obtain solutions in approximation to the governing equations. FEA is used extensively for structural evaluation and improvement, and in this paper, the structure of a high-power PEM fuel cell stack is analyzed and optimized.

Despite an increasing number of FEA analysis, there is not yet studies for structural integrity of large stack in vibration environment. Academic publications are often limited to small stack application, such as stacks of less than 100 cells. In this paper, we present a first-of-its kind overview of vibration simulation of a 300 kW single stack with 550 cells. We derive a FEA methodology and reviewed technology parameters and application requirements. The resulting method and data are then used to calculate the deformation potential under highway vibration conditions. By incorporating FEA, this study can help to reduce uncertainty around the future application of large fuel cell stacks.

2 Method and Materials

2.1 Fuel Cell Stack

A fuel cell stack with 550 unicells is assembled and selected as the object of FEA analysis. The unicells are sandwiched between anode and cathode end plates (Fig. 1), insulation plates and current collectors, and then were compressed to 100 psi over the active area. The cells and plates are then assembled by adding four pieces of upper and lower side mounting plates. The edges of the side mounting plates are bent 90° to increase the strength of the overall side plates. The side mounting plates are bolted to the end plate to complete the initial stack assembly.

Fig. 1
An illustration of a cuboid fuel cell stack consists of unicells with side plates on top and end plates at the ends.

The initial stack assembly

Full size image

To ensure the robustness of initial stack structure, a reinforced stack assembly was designed (Fig. 2a, b). In the updated version, a total of 14 side bars are added to join the top and bottom side plates. In addition, electrical insulation blocks are inserted strategically into the space between the cells and side plates to limit the movement of cells in the middle of the stack. The addition of side bars is expected to increase the strength of the overall stack structure.

Fig. 2
Two illustrations of reinforced stack assembly. Part a contains unicells. Part b doesn't contain unicells.

a The reinforced stack assembly (with 550 unicells), b the reinforced stack assembly (without 550 unicells)

Full size image

2.2 FEA Analysis

Parameters: The following parameters and are used for FEA analysis with Ansys Mechanical APDL: Bolt preload: 20,000; End plate bearing force: 11,150 N * 2; Stack compression force: 22,300 N; Properties of materials are listed in Table 1; Vibration conditions are adapted from GJB150A—2009 Lab Environmental Test Methods for Military Equipment, and then used in this analysis (Table 2).

Table 1 Materials used in the fuel cell stack
Full size table
Table 2 Highway truck vibration testing method
Full size table

Boundary setup: To simplify the model, the parts of the end hardware are set to binding (reject normal and tangential movement), and the contact surfaces between the bipolar plates, between the bipolar plate and end plate are set to friction contact, with the friction coefficient set at 0.76 [13]. However, the Ansys software will default contact as binding in actual calculation, and only mass participation is considered in the displacement caused by the vibration excitation, so the contact type has little influence on the result.

The model adopts a hybrid grid with hexahedral dominant scheme, using a multi-area structured meshing scheme for bolts, bolt gaskets and end hardware, and locally enhanced meshing scheme (enhanced meshing resolution at 2) for the screw holes and their imprint surfaces. The overall element size is 5 mm, the node order is set to 2 to obtain more accurate integration interpolation results, the total number of cells is 1,244,154, the number of nodes is 2,076,272, the total number of meshes in modal computing is 699,432, and the number of nodes is 1,352,436.

The bolt thread surface and its contact surface are equivalent to binding constraints, the smooth axial surface and its contact surface are set to friction contact with the friction coefficient at 0.7 under standard gravity [13], and the remaining contact surfaces are set to no separation under actual working conditions. In order to prevent the penetration of the contact surface during the calculation, the permeation tolerance is set to 0.9. To further prevent the gap in the 3D model causing the contacting pair to diverge in calculations, the pinball search is enabled and the radius is controlled by the software.

Ansys solver settings: The frictional contact is a nonlinear contact, and the non-separation contact is linear in nature, but a nonlinear algorithm is used in the calculation. To ensure nonlinear result convergence and computational efficiency, augmented Lagrangian algorithm and full Newton–Raphson iterative methods are enabled.

In nonlinear calculation, even if the boundary conditions are set to ensure that force is balanced on both sides of the end plates, a slight deviation of the vector of force during iteration could cause the accumulation of errors in the form of diverging results. Therefore, a weak spring as correction force is introduced to counter the iterative cumulative error.

3 Results and Discussions

3.1 Modal and Vibration Simulation Results

Modal analysis was conducted with the stack mode. In the analysis, the compression force of the fuel cell stack is set at 22,300 N, which is the same as the stack compression force in its manufacturing process. The first 10 orders of the modal analysis results are listed in Table 3.

Table 3 The first 10 order of modal analysis
Full size table

The results showed that at all orders, the frequencies are above the vehicle resonance frequency at 30 Hz, which suggests the stack structure is safe against the risk of resonance. In addition, by reviewing the mode shape at each order, one could conclude that most of the potential shape change occurs in the middle of the stack, with much lower shape change at both ends of the stack. This conclusion is consistent with the fact that the cells in very large stack are connected through surface friction between the cells, and the middle of the stack  is vulnerable under road vibration.

In the second step, the harmonic response deformation cloud was reviewed. The setting is at vertical acceleration of 9 g [14, 15] (Fig. 3). It is concluded that the maximum harmonic response is at 34 Hz which is associated with the largest phase change. Again, the harmonic response deformation result showed the largest shape change potential at this condition is at the middle of the stack (data not shown).

Fig. 3
Top. A line graph of amplitude versus frequency with highest peak at around 35 Hertz. Bottom. A line graph of phase angle versus frequency, which remains relatively flat until around 50 Hertz and then decreases with abrupt peaks toward the end. Both graphs have insets for the abrupt changes.

Shape-change in relation to frequency

Full size image

In the third step, the acceleration density spectrum PSD in the vertical direction was conducted according to Highway truck vibration testing method (Table 2). At scale factor of 1 sigma, the deformed cloud diagram (Fig. 4) showed that the largest potential shape change is in the middle of the stack.

Fig. 4
A deformed cloud diagram of a fuel cell stack plots the distribution of directional deformation using a color gradient scale. It is highest at the center and decreases as we move towards the extremes.

Deformed cloud diagram of the fuel cell stack under vibration simulation

Full size image

To summarize the above modal analysis results, the path to improve the structure of a large fuel cell stack with hundreds of connected cells is to reduce the shape change in the middle of the stack. This could be achieved by limiting the free space around the cells in the middle of the stack, and by strengthen the mechanical structure of stack assembly.

3.2 Structural Statics Analysis of Large Fuel Cell Stacks

In this section, statics analysis is used to improve the structure of the stack assembly, with the emphasis on comparison between the initial stack design (Fig. 1) and the reinforced stack design (Fig. 2a). It is expected that potential design weakness could be illustrated through the FEA analysis, and it could be addressed in the following-up design. Once the weakness is addressed, an experimental vibration test could be carried out for validation of the reinforced design.

Lateral load analysis. A load is equally added to both sides of the stack end plates (Fig. 1), and structural deformation is then observed. Under lateral load, the maximum deformation and stress distribution of the assembly is concentrated in the center of the upper and lower side plates in the original stack design (Fig. 5a). It is obvious that in the original stack design, a wider area of the two upper side plates is under higher stress than the two lower side plates.

Fig. 5
Two-part diagram of lateral load analysis on original and reinforced stack design. In both cases, the maximum value is at the center and the minimum values are at the end.

a Lateral load analysis on the original stack design, b lateral load analysis for the reinforced stack design

Full size image

To apply the same lateral load to the reinforced design, the high stress areas on the upper and lower side plates are greatly reduced (Fig. 5b). However, the upper side plates are still subject to more stress than the lower side plates. In addition, the maximum deformation on the side plates is also reduced from 0.32 mm in the original design to 0.14 mm in the reinforced design. Therefore, the reinforced design with the side bars strengthened the structure of the stack assembly.

Normal load analysis. In the second step, a normal load of 1000 N is applied to the side plates of the stack, and the degree of deformation was observed and compared between the original and reinforced designs. The results show that under normal load, the middle of the side plates is experienced larger deformation at 3.62 mm, while in the reinforced version, it is reduced to 1.02 mm (Fig. 6a, b). In addition, the area of the maximum deformation in the middle of the side plates are also reduced in the reinforced version of stack design. However, the small deformation suggests that the exist of localized Von Mises stress (results not shown), and this will be an area of further design improvement.

Fig. 6
Two-part diagram of normal load analysis on original and reinforced stack designs. In part a, the distribution is lateral, whereas in part b, the distribution is circular. The maximum value is in the center, which decreases and reaches the minimum at the ends.

a Normal load analysis results of the original stack assembly, b normal load analysis results of the reinforced stack assembly

Full size image

4 Conclusions

Modal analysis and load analysis have been conducted to illustrate the structural weakness of a large fuel cell stack. It was found that the weakest area of the stack is in the middle of the stack, and the reinforced stack design with side bars greatly improved its stability.

Results indicated that the first 10 orders of modal analysis of the stack have modal frequency over 30 Hz, so the design of the large fuel cell stack is safe to be used for highway automotive applications. Results from both harmonic response deformation cloud and acceleration density spectrum in the vertical direction point to the potential deformation in the middle of the stack. Therefore, strengthening the stack assembly structure through design improvement and limiting the middle section of cell movement by removing free space is of ultimate important for robustness of a fuel cell stack.

Results through structural statics analysis confirmed the weak area of the stack assembly is in the middle of upper and lower side plates. By adding 14 side bars (Fig. 2b), the structure of the stack assembly is greatly stabilized with reduced deformation and Von Mises stress. The concept of side bars points out directions for further design improvement and optimization. In the next phase, the authors will conduct shock and vibration tests to validate the FEA model done in this paper, and further structural improvement is expected.