*2.2. Multi-Point Constraint (MPC)*

When the gears are engaged, the stress field gradient near the contact line is very large. The contact area needs high-density mesh to capture the contact state. The smaller the element size of the FEM model is, the smaller the stress difference between the elements is, and the higher the solution accuracy of the model is, but the longer the solution time of the model is. In order to balance the contradiction between solution accuracy and solution time, it is necessary to determine a reasonable mesh density transition boundary.

In order to ensure the solution accuracy of the FEM, it is necessary to refine the mesh of the contact area. In this paper, MPC is used to connect the refined mesh with the non-refined mesh. As shown in Figure 3, the orange part is the refined area of the tooth mesh. Partial FEM parameters are shown in Table 2.

**Figure 3.** The refined area of the tooth mesh.

**Table 2.** The finite element method (FEM) parameters.


MPC, that is, multi-point constraint, establishes a multi-point constraint relationship. Through MPC, different meshes can be connected. If the geometry is not connected in the topology, different geometric parts can be meshed respectively, and then the FEM models can be connected with the MPC. A simple example is shown in Figure 4; Figure 4a shows the MPC connection of refined mesh and non-refined mesh, while Figure 4b shows no MPC connection and the entire mesh has been refined. Both models are solved using SHELL181 element, in which the shell element thickness is 0.01 m, the elastic modulus E = 2.1 × 10<sup>5</sup> MPa, and the Poisson's ratio μ = 0.3. Figure 4c shows the loading type and boundary conditions, and the two models have the same type of boundary conditions and linear pressure loads, in which the linear pressure is 10 N/m. Figure 4d,e show the analysis results of FEM, and the maximum stress on both models is 6.63 MPa. According to the stress nephogram and solution results, for the FEM model of MPC connection, when the size of the refined area is large enough, that is to say, when the distance between the MPC connection position and the stress analysis position is far enough, the solution results are basically consistent with the results of the entire refined mesh model. Therefore, in this paper, the mesh of the refined area and non-refined area is connected by the MPC, and in order to save the time of FEM analysis, and at the same time ensure the accuracy of the solution, the optimal size of the refined area will be studied and analyzed to determine the mesh transition boundary position.

**Figure 4.** Multi-point constraint (MPC) connection.
