## 2 Material and Methods
### CFD Analysis  
Numerical analysis of the simplified model of the gripper was performed using the open source CFD toolbox OpenFOAM [16]. The RANS approach coupled with the SST \(k\)-\(\omega\) turbulence model has been used to compute the flow-field. The choice of the turbulence model was motivated by its common use in many aerodynamical applications, its robustness and its low computational cost [17]. However, recent studies demonstrated that this model leads to erroneous predictions for complicated flows with streamline curvature, sharp edges, inhomogeneities and flow separation [18; 19]. This predictive discrepancy acted as a source of uncertainty in the final results of this investigation. The steady-state solver _rhoSimpleFoam_ based on the SIMPLE algorithm was first considered, but some convergence problems suggested the use of a pseudo-transient method. The _rhoSimpleFoam_ solver, based on the PIMPLE algorithm, was adopted eventually. The steady state solution was obtained while increasing the Courant Friedrichs-Lewy number (CFL) value, and the corresponding time step, to make the temporal derivative negligible. In particular, the minimum (and initial) CFL was set to one, and the maximum CFL was set to 50. In addition to the residuals' value, another criterion was defined to check the convergence of the solution. In fact, even if the residuals' value reduced by four order of magnitude, the solution was still oscillating. An algorithm written in Python [20] was integrated into the CFD code to check at runtime for a stop condition. The algorithm operates on successive time intervals \(\Delta t_{i}=2\cdot 10^{-3}\) s according to the following steps:  
1. For each \(i\)-th time interval \(\Delta t_{i}\), it computes the average values of mass flow rate (\(\overline{m_{i}}\)) and aerodynamic force (\(\overline{F_{mi}}\)). 2. Then, it computes the levels of relative change for mass flow rate and aerodynamic force. \[\Delta\dot{m}_{i}=\frac{\overline{m}_{i}-\overline{m}_{i-1}}{\overline{m}_{i- 1}}\] (8) \[\Delta F_{Mi}=\frac{\overline{F_{M}}-\overline{F_{Mi-1}}}{\overline{F_{Mi- 1}}}\] (9)
3. It stops the simulation when both \(\Delta\dot{m}_{i}\) and \(\Delta F_{Mi}\) fall below a prescribed threshold (i.e., \(3\cdot 10^{-4}\)) for the first time. The convective terms of velocity and energy were discretized with a second-order upwind scheme, and for the diffusive terms a linear second-order bounded central scheme was used. The gradient term was evaluated using a center differencing method and the first order upwind scheme approximated the turbulent quantities. At the inlet section, total initial temperature (\(T_{01}\) = 293.15 K), total pressure (\(p_{01}\) = 100 kPa) and turbulence intensity (\(\overline{I}u_{1}\) = 1%) were imposed, and static pressure (\(p_{2}\)) was prescribed at the outlet section. The inflow velocity vector was prescribed to be normal to the inlet patch. The mesh quality affects the accuracy of the results obtained from CFD simulations. A hybrid mesh was employed to discretize the computational domain. It consisted of prismatic elements near the walls and tetrahedra elsewhere. The near wall region, compared to a previous study [21], was extended to improve capture of the boundary layer. A non-dimensional distance y\({}^{+}\approx 1\) was considered for cells near the walls, because of choice not to use the wall functions. Figure 6 shows the detail of the surface mesh in the front chamber zone. To find out the optimal mesh density, a grid independence analysis was carried out on one gripper geometry (\(d\) = 0.77 mm, \(L\) = 24.2 mm, \(D\) = 3.4 mm), which from now on will be called \"reference geometry,\" using three different grid resolutions: coarse (\(0.308\times 10^{6}\) cells), medium (\(0.679\times 10^{6}\) cells) and fine (\(1.58\times 10^{6}\) cells). The meshes were characterized by a different spacing of the elements adjacent to the walls (\(y_{1}\)) and on the model surface.