Within Europoort Rotterdam, a tankpit of 37m diameter and 21m height was intended to be repurposed for storing a blend of Naphtha and Reformate. Reformate, a product of Naphtha, shares similar chemical properties, with both fluids being miscible (they mix well together). Dynaflow Research Group performed a CFD analysis on the tankpit to investigate the time of mixing required to achieve complete homogenization of an 80%-20% Naphtha-Reformate mixture. The study considers two inlets, a nozzle and a diffuser. The CFD analysis is performed in Helyx 4.2.0 using OpenFOAM v2412.
The inlet nozzle, S9, injects liquid into the tank at relatively high velocities, creating a jet of 8m/s during maximum inflow. This nozzle is manually adjustable, allowing it to be directed upwards or downwards; however, when in operation, this is impractical due to the nozzle requiring manual intervention. For the purposes of the study, the nozzle was set to its maximum angle of 39°.
The second inlet of the diffuser, S7, introduces fluid into the tank through a series of 20 slotted holes located on down the length of the diffuser on each side, inducing an outlet flow of 1.22m/s during maximum inflow conditions. The diffuser is of a cylindrical shape with holes angles downward at 30°. Using BOSfluids, the pressure drop across the holes were calculated, concluding that the flow velocity variation between the first and last holes is less than 0.1%. Hence, the flow rate can be considered uniform across all holes.
Figure 1 | Meshing of Inlet Diffuser and Inlet Nozzle.
The geometry of the tankpit walls and nozzles were developed, with local refinements being generated around local discontinuities. To enhance the stability and efficiency of the computational solution, simplifications were made to the geometry, reducing non-orthogonality and cell skewness. Specifically, the cylindrical diffuser is modelled as a cuboid with the same width and height of the cylinder’s diameter, and the diffuser inlet is represented as a single strip with an equivalent surface area to the slotted holes whilst maintaining the same downward flow direction of 30°.
An outlet flow is located at the outlet nozzle, S4, which features a bend directed towards the bottom of the tank with a 100mm gap between the tank floor and nozzle. The outlet flow from this nozzle can be pumped directly back into the tank, which is the assumed state of operation during the mixing calculations.
Figure 2 | Meshing of Outlet Nozzle.
Analysis
Fluid mixing is inherently a transient process. Due to the mesh refinement around the detailed regions requiring mesh sizing of ~7.8mm alongside high velocities of ~8m/s, for an accurate CFD analysis, very small timesteps of ~10-4s are required. These small timesteps combined with the size of the tank, number of elements, and the homogenous mixing timeframe estimated in the order of hours, a full transient simulation of the mixing would be infeasible.
Instead an alternative approach is adopted, wherein the problem was divided into two separate simulations:
Step 1: Solve Steady-State flow field
In this step, a steady state solution is acquired using the RANS equations with a k-ω SST turbulence model used to close the system of equations. Fluid properties are calculated to be equivalent to the 80% Naphtha to 20% Reformate volume ratio, the flow field should not be significantly affected by the differences in fluid properties between the flow components due to the similarities of the components. This step assumed the flow to be steady, which is a safe assumption based on the nature of flow within the large tankpit.
Step 2: Solve a transport equation to simulate mixing
The mixing behaviour is simulated using the computed steady-state flow field on the same mesh. Using the velocity field, an advection-diffusion equation is solved, which does not require a time step as small as for transient CFDs and is a much faster equation to solve compared to the Navier-Stokes equations.
The advection component represents the transport of the volume fraction due to the bulk flow. The velocity vector, u, is obtained from the previous steady-state flow field step.
The diffusion component describes the “smearing” of the concentration gradients due to diffusion and turbulent mixing. This depends on the diffusion coefficient which quantifies the extent to which the Naphtha and Reformate mix. This coefficient is derived using the Wilke-Chang equation, providing a correlation for diffusion coefficients in liquid mixtures suitable for non-polar solvents like Naphtha and Reformate.
Load Cases
Using this calculation approach, two load cases were defined:
- Case 1: Maximum inflow rate of 1500m3/hr is applied with S9 flow velocity at 8m/s and S7 flow velocity at 1.22m/s
- Case 2: all inflow is directed exclusively through nozzle S9 at a flow velocity of 8m/s.
The case 2 scenario was explored based on the hypothesis that the diffuser may not contribute effectively to fluid mixing due to the outlets being oriented directly towards the outlet without traversing a significant path through the tankpit and that the two opposite flows of the diffuser tend to converge and counteract each other, stalling overall flow dynamics.
For both cases, the system was initialised so that the denser Reformate is settled on the bottom of the tank with a flat interface with no initial mixing between the Naphtha and Reformate.
Figure 3 | Initialisation State.
Results
The calculations found inefficient mixing from the diffuser due to the outlet positioning. However, a number of streamlines on the innermost side of the diffuser were found to bypass the outlet and travel a significantly longer path through the tankpit.
Figure 4 | Flow streamlines from diffuser.
However, a velocity field comparison between case 1 and case 2 shows that the inclusion of the diffuser does introduce some “randomness” to the flow, lessening the “deadzones” with little to no velocity and thus no mixing. Therefore, it is concluded that whilst the positioning of the diffuser with respect to the outlet leads to inefficient mixing from the diffuser itself, the presence of the diffuser improves the mixing of the fluids.
Figure 5 | Velocity field comparison of case 1 and case 2.
Through the calculations, the Reformate volume fraction is tracked at multiple locations within the vessel. Once the volume fraction at these locations stabilises at a fraction of 0.2, the fluid mixture at the location can be considered too of mixed, achieving complete homogenization of the flow.
Figure 6 | Volume fraction probes.
Figure 7 and Figure 8 show the mixing times required for both load case 1 and load case 2. A mesh refinement study (with the mesh resolution doubled) was performed within load case 1 where the mixing deviations were found to remain similar throughout the analysis concluding an acceptable mesh density.
Figure 7 | Case 1 Mixing Time.
Figure 8 | Case 2 Mixing Time.
The analysis concluded that whilst the diffuser provided limited mixing itself due to its orientation and proximity to the outlet nozzle, using the diffuser and inlet nozzle in conjunction with each other results in an improved mixing time per the following.
- Case 1 mixing time = 5 hours 30 minutes
- Case 2 mixing time = 15 hours and 53 minutes
It was further noted and recommended that whilst the mesh refinement study confirmed the validity of the findings, minor numerical variations within the solution suggest adopting a conservative approach in practical applications and therefore a safety margin on the mixing time should also be incorporated, resulting in a recommended 6 hour mixing duration where both the inlet nozzle and diffuser are active in full flow conditions.
This project shows how CFD can be used to investigate mixing of fluids in an efficient and effective way, concluding that the inclusion of disrupting elements (various inlet/outlet sources and geometric discontinuities) into a mixing process helps to improve mixing times.