Setting condition file

Start directory

startDir mention a directory which store CFD simulation results and syntax is the name of the directory (default is 20000). When the CFD simulation result is stored a directory named 100, it is:

startDir 100

Solver

The solver provides three numerical methods for integrating Newton's equations of motion:

1. Euler: This method is a first-order numerical procedure utilized for solving equations of motion. It approximates the future value of the function based on its current rate of change, providing a straightforward but less accurate solution for dynamic systems.

2. Hybrid: This approach integrates the equations using the Euler method but switches to an analytical solution when both the Stokes number and Mach number are sufficiently small, indicating conditions where Stokes' law is applicable. This method combines numerical and analytical techniques to enhance accuracy in specific scenarios.

3. EulerIL (Euler Inertia-less): This variation of the Euler method integrates the equations while neglecting the inertia of the particles. It is particularly useful for systems where the effect of inertia on the particles is minimal, allowing for simplification of the calculations.

This syntax is needed to set in prior to setting following syntax. Example is

solver Euler

Drag model

The dragModel function allows users to select from four different drag models: Singh, Stokes-Millikan, Morsi, and Loth, with the syntax for selection being identical to the model name (defaulting to Singh).

• Singh: This drag model, based on Singh et al. (2021), stands out for its applicability across a wide range of Reynolds and Mach numbers, including supersonic flows. It is thus considered a general drag model.

• Loth: The Loth model, according to Loth (2008), is also suitable for a broad range of conditions.

• Morsi: The Morsi and Alexander model, as presented in Morsi and Alexander (2006), is typically used for incompressible flows.

• Stokes-Millikan: This model is specifically designed for flows with low Reynolds numbers and has more limited applicability compared to the others.

An example of implementing the Singh drag model is provided as follows:

dragModel Singh

Total calculation time

totalTime specifies the total simulation time, and its value is given in seconds. Ideally, this time is set to infinity, as particles may exit the calculation domain or deposit on the wall surface after a long enough time. However, particles may also become trapped by the circulation, leading to longer simulation times. The wall time is set to prevent the situation where the simulation never finishes. For example, if the wall time is set to 100 seconds:

totalTime 100

This means that the simulation will terminate after 100 seconds of simulated time, regardless of whether or not all particles have exited the calculation domain or deposited on the wall surface. It is important to set an appropriate wall time value to ensure that the simulation finishes in a reasonable amount of time, while also allowing enough time for the particles to travel through the domain.

Time step

In this particle trajectory calculation the time step is automatically determined by selecting the smallest time steps from: (1) Residence time in a cell, $t_{cell}$ (2) Particle characteristic time, $\tau$ (3) Duration of the eddy, $t_{turb}$. The (1) residence time in a cell is estimated by $t_{cell}=L_{cell}/v$, where $L_{cell}$ is the cell size and $v$ is the particle velocity. You need to set small enough cell size manually in this particle trajectory code as (example below is 1um of cell size):

cellSize 1e-6

In terms of (2) particle relaxation time, this code utilize $1/40$ of particle relaxation time since the time step should be sufficiently to make sure the time step is sufficiently smaller than the particle relaxation time. For small particle, this time scale dominate, slowing the calculation. In that case inertia less calculation may be useful. On the (3) duration of the eddy, it is considered in only the case of turbulent dispersion "on" (see dispersion Turbulent dispersion or original paper, Gosmas and Loannides, 1983, for more details). When value is mentioned, the code uses fixed time step as that value (unit is second).

Observation interval

observeTime mentions the interval of the intermediate trajectory simulation results that are the particle location and the velocity. Following syntax is the interval in the unit of second (default value is 1e-6). When you export particle location and velocity every 1 ms, it becomes:

observeime 1e-3

Compressibility

compressible mention the compressibility of the fluid. Available syntax is:

• Yes: compressible

• No: incompressible; constant temperature and density is needed to specify (see example)

When it is Yes, temperature and density profiles (T and $\rho$) are needed to be located in the CFD simulation result directory, hence the compressible CFD simulation must to be performed. Here is one example when it is incompressible flow at 300 K of temperature and 1.2 kg/m3 of fluid density:

compressible No 300 1.2

Dimension

dimension set the dimension as 3D, 2D, and 2D axi-symetric that syntaxes are 3D, 2D, and 2Daxi, respectively. Two more syntax is required for 2D and 2Daxi cases to indicate the plane of the interest as x-y, y-z, z-x etc... (order does not matter). and 001 respectively indicate the direction of the axis is x, y, and z coordinate. This example is when you calculate trajectories with 2D axi-symmetric at x-y plane:

dimension 2Daxi x-y

Reflecting boundary condition

reflect set the reflecting boundary condition.

reflect x 0 1

This example describes a scenario where particles reflect off a boundary located at $x=0$. The direction in which the particles remain after reflection is determined by specifying either $1$ or $-1$: a specification of $1$ indicates that particles will remain on the side where $x>0$, while specifying $−1$ indicates that particles will remain on the side where $x<0$.

Turbulent dispersion

Dispersion mention the turbulent dispersion and syntax is Yes or No (default is No). On the turbulent flow, the eddy repeat to generate and dissipate which mean the flow becomes random. One of the approach to treat such turbulent flow as a steady state is the Reynolds Averaged Navier-Stokes (RANS) model approach in CFD, e.g., $k-\epsilon$ model. This code also able to treat the effect of this random eddy from the parameters used in RANS model that are turbulent kinetic energy, $k$ and the dissipation rate of the eddy, $\epsilon$ by following this method (Gosmas and Loannides, 1983). This simulation with this model require $k$ and $\epsilon$ profiles under CFD simulation result directory. Currently, available syntax is:

• No: without dispersion

• k-e: standard $k-\epsilon$ model

• k-w: $k-\omega$ model

Here is one example when it is ON:

Dispersion k-e

Diffusion

This is not validated yet but is implemented

diffusion Yes

Gravity

This is not validated yet but is implemented

gravity 0 0 -9.8