Stress Analysis of Printed Circuit Board with Different Thickness and Composite Materials Under Shock Loading

: In this study, the deformation and stress distribution of printed circuit board (PCB) with different thickness and composite materials under a shock loading were analyzed by the finite element analysis. The standard 8-layer PCB subjected to a shock loading 1500 g was evaluated first. Moreover, the finite element models of the PCB with different thickness by stacking various number of layers were discussed. In addition to changing thickness, the core material of PCB was replaced from woven E-glass/epoxy to woven carbon fiber/epoxy for structural enhancement. The non-linear material property of copper foil was considered in the analysis. The results indicated that a thicker PCB has lower stress in the copper foil in PCBs under the shock loading. The stress difference between the thicker PCB (2.6 mm) and thinner PCB (0.6 mm) is around 5%. Using woven carbon fiber/epoxy as core material could lower the stress of copper foil around 6.6% under the shock loading 1500 g for the PCB with 0.6 mm thickness. On the other hand, the stress level is under the failure strength of PCBs with carbon fiber/epoxy core layers and thickness 2.6 mm when the peak acceleration changes from 1500 g to 5000 g. This study could provide a reference for the design and proper applications of the PCB with different thickness and composite materials.


Introduction
Printed circuit board (PCB) is an important part to connect active and passive components for current electronic devices. Therein, electronic circuits in PCB and the components form a conductive connection during the operation of devices [Wang (2012)]. A good PCB design could provide a stable working environment for communication between components. Three major types of PCB are used in current industry for various considerations, including the single-sided PCB, double-sided PCB and multilayer PCB [Ebnesajjad (2013)]. The single-sided PCB has the advantage of lower cost, but the capacity of mounting components is limited due to single-side usage only. The doublesided PCB has two conductive pads on top and bottom sides for mounted components and connection of two sides by via. Compared with the single-sided PCB, the doublesided PCB could save more area to make a package compact. For more complex electronic circuit design, the multilayer PCB is chosen for the package with smaller space. Conductive and insulating layers are sandwiched to form the multi-layer PCB [Tummala (2001)]. The number of layers in the PCB as motherboard of electronic devices depends on its requirements. The PCB with four to eight layers is common in the industry. The PCB consists of dielectric substrates and conductors; and the copper foil is a general material as the conductor because of its low rate of surface oxidation and compatibility of substrates [Grout (2008) ;Hanafi, Jobiliong, Christiani et al. (2012)]. FR-4, a composite material of woven fiberglass cloth and epoxy resin binder, is the most popular material used as substrate of PCB since it is versatile, including electrical insulation with high dielectric strength, high strength-to-weight ratio, moisture resistance, and relative temperature resistance [Nanotech Elektronik (2019)]. Therefore, a lot of portable products adopt FR-4 PCB as the motherboard. Many situations might induce failure of PCB, including circuit failure due to improper component design, environmental factors and operation. These environmental factors, such as temperature and moisture, cause delamination between layers and material crack inside the PCB. Some literatures investigated the effect of these factors, including studying the temperature effect by thermal cycling [Zhang, Ding and Sheng (2009);Zhang, Liu, Wang et al. (2015)]. On the other hand, the impact drop test for PCB is quite important before mass production for the development of PCB, especially for application of portable products. Reiff et al. [Reiff and Bradley (2005)] evaluated the lead-free ball grid array (BGA) solder joint reliability by a mechanical shock test and identified the failure of BGA by the strain rate. Wang et al. [Wang, Low, Che et al. (2003)] performed the simulation of the PCB drop test and focused on the displacement and acceleration of the PCB during the drop test. Ong et al. [Ong, Shim, Chai et al. (2003)] indicated the bias between the product-level and board-level drop impact test by comparing the mechanical responses of PCBs. Wong et al. [Wong, Lim, Lee et al. (2002)] studied the mechanics and physics of the board-level drop test to provide the fundamental understanding for PCB and interconnection design. They found geometrical stress concentration is critical in the impact of strength of the interconnections. Jie et al. [Jie, Lim and Tay (2004)] performed the dynamic drop impact test by the finite element analysis and predicted the critical failure location by the bending curvature of PCB. In this paper, the deformation and stress distribution of the PCB during the mechanical shock test were investigated. Various PCB models with different thickness and composite materials were used to discuss the strength of PCB during the shock loading by the finite element analysis.

Finite element analysis
The commercial finite element software ANSYS [ANSYS (2009)] was used to build the finite element models of the PCB and to perform the dynamic analysis by giving the PCB an acceleration loading in this study. The deformation and stress distribution in the PCB were discussed, after the models were subjected to an external load by referring to the industry criteria [Integrated Service Technology (2019)]. In addition, the PCBs with different thickness and composite materials were also evaluated.

Finite element models
According to the JEDEC standard for board level drop test, JESD22-B111 [JESD22 B111 (2003)], the length and width of the PCB in this study are 132 mm and 77 mm respectively, as shown in Fig. 1. Two different stacking structures were built. One is a standard 8-layer stacked PCB, which consists of 8 layers of copper foil and 7 layers of woven E-glass/epoxy, and a total thickness of 1.6 mm [Pcbcart (2019)], as shown in Fig.  2. For considering the strength of the PCB with different thickness, the other stacking structure of the PCB with different thickness of E-glass/epoxy and copper foil layers was adopted from literature [Wang, Low, Pang et al. (2006)], as shown in Fig. 3. Therein, the thickness of each E-glass/epoxy layer is 0.178 mm and inner and outer copper foil are 0.0178 mm and 0.035 mm respectively. The material properties of woven E-glass/epoxy composites used in finite element models are shown in Tab. 1 [Tan, Tong and Steven (2001); Rahman, Rangari and Jeelani (2015)]. The non-linear material property of copper foil was considered in the analysis, as shown in Tab. 2 [Iannuzzelli (1991)]. Except the finite element model of the PCB with woven Eglass/epoxy composites, the PCB model with woven carbon fiber/epoxy composites was also analyzed. Tab. 3 shows the material properties of woven carbon fiber/epoxy composites [Qrimli, Mahdi and Ismail (2015); Performance Composites (2009)].
The finite element models of PCB were built with the above-mentioned dimensions and material properties. The solid-shell element SOLSH190, adopted for modeling the PCB structures, has eight nodes and three degree of freedom for each node in the x, y, z directions. In this paper, the applied load, normal to the PCB, for dynamic analysis was given to simulate a shock test [Integrated Service Technology (2019)]. The support excitation scheme was used in the finite element analysis, so the four screw holes in the PCB were fixed as boundary condition [Yeh and Lai (2006); MIL-STD-883E (1997)]. Fig. 4 shows the finite element model of the PCB and boundary condition.

Convergence analysis
In order to ensure the accuracy of simulation, the convergence of the finite element model of PCB was analyzed first. The maximum von Mises stress in E-glass/epoxy layer for finite element models of the PCB with different element numbers under the shock loading was obtained, as shown in Tab. 4. When the element number of the analysis model of PCB is over 11,527, the difference of the maximum von Mises stress is under 2%, as shown in Fig. 6. Therefore, the finite element model of the PCB with 11,527 elements was adopted for the subsequent analyses. Fig. 4(a) shows the meshed finite element model with 11,527 elements.

Results and discussion
The results of the finite element analysis are discussed in three parts. At first, the deformation and stress distribution of the standard 8-layer PCB under the shock loading were analyzed. Then, the deformation and stress distribution of the PCB with different thickness were evaluated. The failure of PCB was assessed based on the stress states in each ingredient material and ignored the possibility of interfacial failure. Lastly, the finite element model of the PCB with a lower strength was selected to change the composite material from E-glass/epoxy to carbon fiber/epoxy for discussion of strength enhancement.

The standard PCB under shock loading 3.1.1 The deformation of standard PCB under shock loading
Large deformation of PCB might induce failure of interconnection between the chip and the PCB, or the failure of PCB and chip. This study focused on the deformation at the central region of the PCB since the chips were located at the central region of PCB generally. Moreover, the deformation of PCB during the shock loading was contributed by the out-of-plane displacement in the direction of shock loading in the finite element analysis. Fig. 7(a) shows the out-of-plane displacement variation at the central region of PCB under the shock loading from the finite element analysis. The maximum out-ofplane displacement of PCB occurred at 1.98 ms during the shock loading and the deformation of PCB is shown in Fig. 7(b).

The stress distribution of standard PCB under shock loading
In addition to the deformation of PCB, the von Mises stress variation of the PCB under the shock loading from the finite element analysis was obtained, as shown in Fig. 8. The maximum von Mises stress at 1.98 ms, which occurred at the maximum out-of-plane displacement of PCB, is 195.5 MPa. Since this stress level is much lower than the failure strength of copper foil, 318 MPa [Yin, Peng, Kayani et al. (2016)], the failure of PCB may not happen by the shock loading. It is consistent with the practical operation in industry. The maximum principal stress of each layer at the central cross section of PCB was extracted and plotted, as shown in Fig. 9. The results show that the principal stress distribution is symmetric about the middle plane of the cross section of PCB and the principal stress increases from inner to outer part of PCB. The highest principal stress in E-glass/epoxy occurred at the top and bottom layers of PCB.

The PCB with different thickness under shock loading
The deformation and stress distribution of the PCB with different number of layers under the shock loading were investigated by the finite element analysis to understand the correlation between the thickness of PCB and stress level under the shock loading. The PCBs with a thickness ranging from 0.6 mm to 2.6 mm according to stacked layers are discussed. The number of copper foil layer and composite layer in the PCBs with different thickness is summarized in Tab. 5. Fig. 10 shows the maximum von Mises stress of the top-layer copper foil in the PCBs with different thickness by the finite element analysis. The maximum von Mises stress of top copper foil layer decreases 5% when the thickness of PCBs increases from 0.6 mm to 2.6 mm.  The deformation and principal stress of the PCB with 2.6 mm thickness under the shock loading at 1.98 ms are discussed. Since the maximum deformation occurs at the central region of PCB, as shown in Fig. 11, and the electronic devices are practically located around the central region of PCB, this study focused on the principal stress distribution in core layer 1 at the central region of PCB, as shown in Fig. 12. According to the results of the finite element analysis, the PCB with 2.6 mm thickness has the lowest stress under the shock loading. Failure strength of materials, including copper foil, woven E-glass/epoxy, and woven carbon fiber/epoxy, are shown in Tab. 6 [Tan, Tong and Steven (2001); Qrimli, Mahdi and Ismail (2015); Yin, Peng, Kayani et al. (2016)]. The maximum principal stress of E-glass/epoxy layer in the PCB with 2.6 mm thickness under the shock loading by the finite element analysis is 49.6 MPa and is smaller than its failure strength 587 MPa.

The PCB with different composite materials under shock loading
The maximum von Mises stress of copper foil of the PCB with 0.6 mm thickness under the shock loading 1500 g by the finie element analysis is higer than those in the PCBs with different thickness. To improve the strength of the PCB with 0.6 mm thickness, the thinner and weaker one, the woven E-glass/epoxy core layer of PCB was replaced by woven carbon fiber/epoxy composites. The finite element results are summarized in Tab. 7. The maximum displacement of PCB decreases 14.6%, when using carbon fiber/epoxy as the core layer. A smaller deformation was obtained since the PCB with carbon fiber/epoxy under the shock loading had a higher stiffness. Furthermore, the maximum von Mises stress in copper foil at the central region of PCB reduced 6.6% by adopting the carbon fiber/epoxy as the core layer in PCB. The carbon fiber/epoxy shared a part of stress with copper foil during the shock loading. Although the maximum principal stress in the core layer of PCB increased around 64.9% at the central region of PCB by using carbon fiber/epoxy, the stress is still under its failure strength. The results indicate that the PCB with carbon fiber/epoxy has a higher strength and a lower possibility for the failure of PCB than that with E-glass/epoxy.

The PCB under higher level shock loading
For harsh operating conditions, such as those used in the automotive industry and military, the acceleration peak during the shock loading is higher than the condition used for portable devices. Referring to the standard MIL-STD-883 Method [MIL-STD-883E (1997)], the finite element model of the PCB with 2.6 mm, the thicker and stronger one, is subjected to a shock loading with a peak value of 5000 g and 0.3 ms for pulse duration.
The results show that the stresses in both copper foil layer and core layer increase significantly in the PCB with carbon fiber/epoxy as core layer, as shown in Tab. 8. However, the stress levels for both core layer and copper foil are still lower than the failure strengths of carbon fiber/epoxy and copper foil. These results show the integrity of the PCB structure with 2.6 mm thickness, under 5000 g shock loading, when using carbon fiber/epoxy as the core layer.

Conclusions
This study evaluated the deformation and stress of the PCB with different thickness and composite materials under the shock loading by the finite element analysis. The possibility of failure for the PCB under the shock loading was discussed by comparing the finite element results and the failure strength of materials used in analysis. The summary is as follows.
(1) The maximum out-of-plane displacement and von Mises stress of the standard PCB occurred at 1.98 ms and the stress level is lower than the failure strength of woven Eglass/epoxy under the shock loading 1500 g. Moreover, a higher principal stress located in copper foil at the top and bottom layer of PCB.
(2) For the PCB with different thickness, the thicker PCB (2.6 mm) could reduce the maximum von Mises of copper foil in PCB around 5% than that for the thinner PCB (0.6 mm). (3) Adopting the carbon fiber/epoxy as the core layer material instead of E-glass/epoxy could reduce the stress of copper foil around 6.6%. (4) For the applications in harsh environment, the maximum stresses of fiber/epoxy core layer and copper foil in the PCB with 2.6 mm thickness under the shock loading 5000 g are smaller than their corresponding failure strengths.