# Aerodynamic Drag Reduction on Speed Skating Helmet by Surface Structures
## 2 Numerical Approach  
### Computational Conditions and Helmet Models  
The CFD method was used in this study to observe the fluid detail around the helmet models. The actual flow field around the athlete is very complex, so reasonable and necessary assumptions are made in the CFD process. To easily construct the surface structure on the helmet surface, an ellipsoid was used to approximate the shape of the helmet. The dimensions of the ellipsoid are shown in Figure 1, and it was very close to the helmet in geometry. Here, it was assumed that the ellipsoid model was similar to the actual helmet in terms of flow field properties, and the influence of the details of the actual helmet could be omitted. At the same time, we also assumed that the movement of the athlete's arms and legs in skating had little effect on the helmet, as they were moving behind and below the shoulders of the skater. Underneath the simulated helmet model, a support structure was designed to simulate the off-the-ground position in the actual process. The support consisted of two parts: one was a cylindrical shape close to the helmet, which was used to simulate the athlete's face, and the other had a variable cross-section to simulate the athlete's neck and below. In order to reduce the calculation task, the influence of the torso far from the helmet was ignored here. The support with a smooth surface was extended to the ground, so that there were no cross-sections in the computational domain and its impact on the flow field would be avoided. The height between the center of the helmet and the ground was \(H=1\) m, and the helmet was tilted forward \(45^{\circ}\) to simulate the athlete's position, which agreed with the mannequin used in wind tunnel experiments.  
As shown in Figure 2, the computational domain was a rectangular box, which was \(2H\) in width and height and \(6H\) in the streamwise direction. The helmet model was located \(1.5H\) from the inlet surface. A uniform velocity field of \(x\) direction (\(U=14\) m/s) was set on the inlet surface with zero turbulence intensity. The outlet surface was defined as the pressure outlet with zero gauge pressure. The helmet surface, as well as the support surface, was set as the smooth no-slip wall, on which the air had no relative velocity to the model because of the viscosity. The ground surface was also set with a no-slip condition, and defined as the moving wall with the same velocity (\(U=14\) m/s) at \(x\) direction as defined at the inlet face, which could simulate the relative velocity between the athlete and the ground during skating competitions. Other surfaces on the rectangular domain were set as the symmetry boundary, which means that the velocity and pressure gradient were zero in the normal direction of the surface. It was assumed that the property of air remained constant in the skating process. Reference density, temperature, and pressure of \(1.225\) kg/m\({}^{3}\), \(15\)\({}^{\circ}\)C, and \(101\),\(325\) Pa were adopted in the simulation, respectively.  
Figure 1: The simplified helmet model with geometrical dimensions used in CFD simulations.  
Figure 2: The computational domain in CFD simulations.  
Another two types of structured helmet models, as shown in Figure 3, were simulated in the CFD analysis besides the original one. The height of the riblets in Figure 3a is \(h=1\) mm, and the cross section is an equilateral triangle. The space between two riblets is \(s=10\) mm. Figure 3b is the helmet model with bumps in the middle region. The height and diameter of the bumps is \(h=0.5\) mm and \(d=3\) mm, respectively. The bumps have a staggered arrangement on the helmet surface, and the space between two bumps is \(s=6\) mm.