## 3 Numerical Settings  
The flow is modelled based on the homogeneous Unsteady Reynolds-Averaged Navier-Stokes (U-RANS) equations assuming thermodynamic and mechanical equilibrium [18]. Discarding the energy equation, only the mass and momentum conservation equations are solved. The Reynolds stresses are modelled using the [PERSON]'s assumption that introduces a turbulent viscosity \(\mu_{t}\) computed with the SST turbulence model [19]. At the wall, the turbulence model is coupled with an automatic wall function. The phase change due to cavitation is modelled using the model proposed by [PERSON] with the standard values for the parameters [20]. Additional details regarding the flow modelling are available in [17]. Other simulations have also been performed by [PERSON] [21].  
The computational domain considered includes a part of the inlet pipe, the spiral case, the stay vanes, the guide vanes, the runner and the draft tube (see Figure 2). The mesh is a structured hexahedral one based on a blocking technique and made with ICEM CFD (see Figure 2). The number of nodes is slightly above 11.5 million with 2.6 million of nodes in the runner domain and 4.3 million in the draft tube. The minimum angle is above 20 degrees and only 9% of the cells have an angle below 50 degrees. The \(y^{+}\) value does not exceed 85 and the averaged value over each solid walls is lower than 20. A study of the grid sensitivity has been done and published in [17], showing around 2% of differences at the BEP between the computed \(T_{ED}\), \(Q_{ED}\) and \(n_{ED}\).  
The flow rate is imposed at the inlet, whereas the pressure is set at the outlet. The rotational speed of the runner is imposed on the experimental value. For all the solid walls, a no slip condition is imposed.  
The convective fluxes in the momentum equation are computed with a high order scheme [22], whereas the turbulence convective fluxes are computed with an upwind scheme. Regarding the time scheme, the second order backward Euler scheme is applied [23] excepted for the volume fraction equation that is discretized with a first order backward Euler scheme (In Ansys CFX 17.2, for rotating turbomachineries, this option is the only one available.). The time step, the CFL number, the number of internal loops per time step and the time duration of the simulation expressed as the number of runner revolutions achieved are given in Table 1 for each case considered. _Case 1_ corresponds to the standard set up in Ansys CFX for a flow in a Francis turbine with a time step set  
Figure 1: Experimental visualization of the vortex rope at full load.  
to less than one degree of revolution per time step and five internal loops per time step. This set up has been validated against experimental data for stable cavitating vortex rope in [17]. _Case 2_ differs from _Case 1_ only by the number of internal loops, which is set to 15. _Case 3_ differs from the other two cases since the time step is not imposed by the user but is computed automatically by imposing a limitation on the CFL number to a value of 2. This value is sufficiently small to deal with the accuracy of the first order backward Euler scheme used for the volume fraction equation keeping advantage of an implicit formulation. In addition, the number of internal loops is decreased to a value of 3 even if two internal loops are enough to reach a second order time accuracy (see [24]) for the equations discretized with a second order scheme. The unsteady simulations are started from a converged steady simulation (see [17]).  
Even if CFX used a coupled solver, the volume fraction equation is treated in a segregated manner. The interfaces between the stationary and rotating domains are handled using a General Grid Interface (GGI) algorithm.