Setting Initial Conditions for Compressible Flows

For compressible flows that use the Coupled Flow model, you can initialize the flow field manually or use the automatic Grid Sequencing (GS) method. GS performs the normal initialization followed by the computation of an approximate inviscid solution to the flow problem.

When initializing compressible flow cases, the following isentropic relations are useful:

Figure 1. EQUATION_DISPLAY

\frac{T_{t}}{T} = 1 + \frac{(γ - 1)}{2} M^{2}

(179)

Figure 2. EQUATION_DISPLAY

\frac{P_{t}}{P} = {(1 + \frac{(γ - 1)}{2} M^{2})}^{γ / (γ - 1)}

(180)

Figure 3. EQUATION_DISPLAY

V = M \sqrt{γ R T}

(181)

Figure 4. EQUATION_DISPLAY

\frac{\dot{m}}{A} = \sqrt{\frac{γ}{R}} \frac{P_{t}}{\sqrt{T_{t}}} M {(1 + \frac{(γ - 1)}{2} M^{2})}^{1 / 2 - γ / (γ - 1)}

(182)

Figure 5. EQUATION_DISPLAY

γ = \frac{C_{p}}{C_{p} - R}

(183)

Figure 6. EQUATION_DISPLAY

R = \frac{R_{u}}{M_{r} (X)}

(184)

where $A$ is area, $\dot{m}$ is mass flow rate, $M$ is Mach number, $M_{r} (X)$ is molecular weight (relative molecular mass) of molecular entity $X$ , $P$ is static pressure, $P_{t}$ is total pressure, $R$ is specific gas constant, $R_{u}$ is universal gas constant [8314.4621 J/kmol K], $T$ is static temperature, $T_{t}$ is total temperature, $V$ is velocity magnitude, and $γ$ is ratio of specific heats.

To initialize the flow field:

Depending on the initialization method, do one of the following:

Method	Steps
Manual	The steps depend on whether you want to start the simulation from the initial state of the model (initial run) or continue from a previously computed solution (restart run). For an initial run: Expand the Continua > [physics continuum] > Initial Conditions node. Select the Velocity node and set the initial velocity: For uni-directional ducts and free-stream flows over slender bodies, it is best to initialize the flow to the inlet or free-stream values. For curved ducts or bluff bodies, it can help to reduce the velocity significantly in these cases. Furthermore, techniques such as changing boundary conditions or ramping boundary values may be required to aid solution convergence. Select the Pressure node and specify the initial pressure: If there are no pressure boundaries, the specified initial pressure must not result in a non-physical absolute pressure. For free-stream flows, choose the initial pressure such that it is equal to the free-stream pressure. For duct flows, choose the initial pressure such that it is equal to or higher than the outlet pressure. Choosing a value higher than the outlet pressure can inhibit temporary reversed flow occurring at the outlet. For a restart run: In the previous simulation, create an XYZ Internal Table and fill it with the Velocity[i], Velocity[j], Velocity[k], and Pressure values. Export the table to a .csv file. Read the table data file in the current simulation. Expand the Continua > [physics continuum] > Initial Conditions node and set the initial values for Velocity and Pressure using the imported tabular data. For detailed information on working with tables, see Table Tasks and Setting Values Using a Table.
Automatic (only for the implicit integration scheme)	Set an initial guess of the flow field as described for the Manual method. Select the Solvers > [Coupled Implicit] > Expert Initialization node and set Method to Grid Sequencing. Select the Grid sequencing sub-node and set the following properties: Maximum Grid Levels Maximum Iterations per Level Convergence Tolerance per Level CFL Number Explicit Relaxation See Coupled Flow Solver Reference—Expert Initialization. You can change the settings at any time during the GS initialization process. The solver acknowledges the change through a message in the Output window. You can also interrupt GS at any time by clicking the (Abort) button next to the status bar. If GS fails (for example due to aggressive settings), the solver attempts to recover from it. At worst, you can simply get a normal (uniform) initialization. In this case, change the GS settings. For example, choose smaller values for the CFL number or the maximum iterations per level, clear the solution and try the initialization again. Also check that the solver is working with a reasonable number of cells per level to converge. The default number of maximum grid levels may not be suitable for problems with a relatively small number of cells in the mesh. Note, that GS is not guaranteed to work in all cases. Deactivate GS if after changing the settings you still encounter lack of robustness or divergence during the GS process.

Method

Steps

Manual

The steps depend on whether you want to start the simulation from the initial state of the model (initial run) or continue from a previously computed solution (restart run).

For an initial run:

Expand the Continua > [physics continuum] > Initial Conditions node.
Select the Velocity node and set the initial velocity:
- For uni-directional ducts and free-stream flows over slender bodies, it is best to initialize the flow to the inlet or free-stream values.
- For curved ducts or bluff bodies, it can help to reduce the velocity significantly in these cases. Furthermore, techniques such as changing boundary conditions or ramping boundary values may be required to aid solution convergence.
Select the Pressure node and specify the initial pressure:
- If there are no pressure boundaries, the specified initial pressure must not result in a non-physical absolute pressure.
- For free-stream flows, choose the initial pressure such that it is equal to the free-stream pressure.
- For duct flows, choose the initial pressure such that it is equal to or higher than the outlet pressure. Choosing a value higher than the outlet pressure can inhibit temporary reversed flow occurring at the outlet.

For a restart run:

In the previous simulation, create an XYZ Internal Table and fill it with the Velocity[i], Velocity[j], Velocity[k], and Pressure values. Export the table to a .csv file.
Read the table data file in the current simulation.
Expand the Continua > [physics continuum] > Initial Conditions node and set the initial values for Velocity and Pressure using the imported tabular data.

For detailed information on working with tables, see Table Tasks and Setting Values Using a Table.

Automatic

(only for the implicit integration scheme)

Set an initial guess of the flow field as described for the Manual method.
Select the Solvers > [Coupled Implicit] > Expert Initialization node and set Method to Grid Sequencing.
Select the Grid sequencing sub-node and set the following properties:
- Maximum Grid Levels
- Maximum Iterations per Level
- Convergence Tolerance per Level
- CFL Number
- Explicit Relaxation
See Coupled Flow Solver Reference—Expert Initialization.

You can change the settings at any time during the GS initialization process. The solver acknowledges the change through a message in the Output window. You can also interrupt GS at any time by clicking the (Abort) button next to the status bar.

If GS fails (for example due to aggressive settings), the solver attempts to recover from it. At worst, you can simply get a normal (uniform) initialization. In this case, change the GS settings. For example, choose smaller values for the CFL number or the maximum iterations per level, clear the solution and try the initialization again. Also check that the solver is working with a reasonable number of cells per level to converge. The default number of maximum grid levels may not be suitable for problems with a relatively small number of cells in the mesh.

Note, that GS is not guaranteed to work in all cases. Deactivate GS if after changing the settings you still encounter lack of robustness or divergence during the GS process.

In a region where the initial conditions are known to differ from the continuum, set the initial region values as follows:
1. Select the Regions > [region] > Physics Conditions > Initial Condition Option node and set Option to Specify Region Values.
2. Expand the [region] > Initial Conditions node and set the initial values for Pressure and Velocity using the manual initialization method.