Finite element modeling
A human first premolar was scanned using a Micro-CT scanner (Skyscan 1076, Bruker Corp., Belgium, scanned using voxel size of 0.127 mm and 720 image slices) to obtain DICOM images. The medical image processing software (Mimics 16.0, Materialise, USA) was used to construct the three-dimensional surface of the premolar (STL file format). The premolar model then underwent post-processing through computer-aided-design software (Geomagic 12, 3D Systems, USA) to produce a three-dimensional geometric model.
On the premolar model, a cavity containing an occlusal valley with an open proximal box was designed, and a class II inlay and a DME layer were created using the finite element analysis software (ANSYS 15.0, ANSYS Inc., USA). The premolar was placed into a cylindrical bone block with a top layer of 2 mm thick as cortical bone and the remainder as cancellous bone. The final model contained six components: enamel, dentin, inlay, DME layer, cortical bone, and cancellous bone. Three types of inlay material were considered, including composite resin (CO), ceramic (CE), and lithium disilicate (LD). The material of the DME layer was fixed as a type of flowable resin. The material of all components in the finite element model were assumed to be linearly elastic, homogeneous, and isotropic, and their Young’s moduli and Poisson’s Ratios were [18.6 GPa, 0.31] for dentin, [84.1 GPa, 0.33] for enamel, [13.7 GPa, 0.3] for cortical bone, [1.37 GPa, 0.31] for cancellous bone, [15 GPa, 0.35] for CO inlay, [45 GPa, 0.25] for CE inlay, [90 GPa, 0.25] for LD inlay, [5 GPa, 0.35] for DME layer. [14, 15, 21,22,23,24,25,26].
The mesh used 10-node tetrahedral structural solid (Solid 187) elements. A study of mesh convergence was performed by evaluating the mesh size between 0.15 and 0.7 mm to ensure the accuracy of the numerical results. The convergence was found at the mesh size smaller than 0.22 mm, but the computation time would greatly increase when the mesh size was smaller than 0.2 mm. Therefore, the global mesh size was set as 0.2 mm for optimizing both numerical accuracy and computation cost, and it resulted in approximately 435,500 nodes and 265,900 elements for the entire model (where the numbers of nodes and elements of individual parts are 152,682 and 90,653 for dentin, 86,331 and 49,580 for enamel, 19,140 and 10,869 for the restoration, 2,534 and 1,335 for resin, 22,477 and 13,488 for cortical bone, and 126,372 and 83,547 for cancellous bone. Note that the numbers slightly varied in different design configurations). A 4-mm–diameter round indenter applied a compressive load of 600 N to the premolar, parallel to the long axis of the tooth. In general, 100–800 N of biting forces can be measured from healthy persons and patients of various muscle efficiencies [27]. To proper simulate the biting force, a 600 N load which has been used for the premolar in a numerical study [28] was chosen in the present study. Before simulating the compressive loading, the indenter was centered to the long axis of the tooth with a short distance away from the tooth top and simulated to move downward until contacting the tooth. This pre-simulation step was to find the realistic contact condition between the tooth and the indenter, which consequently occurred on the premolar at two points (located at the buccal and lingual slopes of the occlusal surface, respectively). The bottom of the bone block was constrained in all directions (Fig. 1). Since this study focused on the inlay design, cement failure is not of concern. Therefore, the dental restoration cement layer was not modeled and the contacts between materials in the model were assigned perfect bounding conditions. This simplification is reasonable and well accepted in the literature [37,38,39]. The quasi-static stress analysis with ANSYS was carried out to evaluate the inlay designs. Seven design parameters and the considered design space were defined as follows, the width of isthmus (W, 1.6 mm–2.4 mm), angle of divergence (A, 85°–120°), length of isthmus (Li, 1–2 mm), length of proximal box (Lp, 2.3–3 mm), depth of isthmus (Di, 4.6–6 mm, measured from the highest point of the tooth to the cavity location), depth of proximal box (Dp, 7–9 mm), and elevation height (Le, 0.35–1 mm). Note that these measurements were not directly from the tooth surface (see Fig. 1a), so it should not lead to any pulpal damage.
Validation experiment
Compression tests were conducted (Fig. 2). The materials of the specimen were CNC-milled zirconia (VITA YZ, VITA Zahnfabrik, Germany) for the tooth model (210 GPa) and PMMA (VITA CAD-Temp®, VITA Zahnfabrik, Germany) for the cylindrical bone blocks (2.8 GPa). An adhesive (3 M U200, 3 M, USA) was applied to bond the tooth model and bone block. The specimen was tested in a universal testing machine (AG-I, Shimadzu Corp., Japan) at 2 N/s until 400 N (a moderate human bite force was chosen) was achieved, which was then maintained for 60 s. Strain gauges (KFGS-02-120-C1-11, Kyowa Electronic Instruments Co., Ltd. Japan) were attached to the mesial side (Strain 1) and distal side (Strain 2) of the bone block. The data-acquisition system, including a 4-slot USB chassis (cDAQ-9174, National Instruments, USA) and an 8-channel capture module (NI-9235, National Instruments, USA), was used to record the strain values generated during the loading. The measured strains were compared with the results of a finite element simulation that used the same experimental setting.
Mechanical analysis for design suggestions
Eight stress indexes (Fig. 1b) were retrieved from the results of stress analysis to assess the mechanical performance of the tooth and inlay restoration. Two types of stress items were obtained, which were peak interfacial tensile stress (ITS) at the various interfaces, and peak maximum principal stress (MPS) in all components of the tooth. Four peak ITS items (on the right-hand side of Fig. 1b) were obtained by retrieving the most negative value of the contact pressure at the interface between each contact pair of materials that were of interests. Four peak MPS items were the highest values of MPS found in each selected material component (on the left-hand side of Fig. 1b). An analysis of variance was conducted to assess the influence of each of the seven design parameters on each stress index and calculate the main effect. The design parameters that demonstrated a significant influence on each stress index were identified, and a response surface of each stress index to those critical design parameters was established through Latin Hyper Cube Sampling. By assessing these response surfaces, guidelines were proposed for design choices to enhance the mechanical performance of the tooth and inlay restoration.