Guidelines for Fluid Flow and Energy

Mesh

The construction of the volume mesh has a direct influence on how well Simcenter STAR-CCM+ simulates fluid flow and energy. It influences the rate of convergence and the accuracy of the final solution. In general, construct a volume mesh according to the following guidelines:

Design a mesh that gives adequate resolution in regions where spatial gradients are high. Such regions occur when:
- The mean flow changes rapidly. Examples are: irrigation canals, vortex shedding, forced mixing, and atmospheric flows.
- There are strong shear layers. Examples are: atmospheric flows, fluid jets, flows past solids, and flows with strong vorticity.
Whenever possible, align the mesh with the flow to improve accuracy and increase the rate of convergence.

In order to make sure that simulation results are independent of the mesh, perform a grid sensitivity study with two or more meshes.

Note	Turbulence has a dominant role in the transport of momentum and other scalars for most complex turbulent flows. For this reason, simulations that involve turbulent flow tend to be more dependent on the mesh resolution than simulations that involve laminar flow.

For external flows, perform domain convergence studies to make sure that what is happening at the flow boundaries does not affect the solution. For example, if the simulation has an outflow boundary close to a bluff body, the flow cannot recover from the effect of the wake before it meets the boundary.

Near-Wall Prism Layers

In order to minimize numerical diffusion in the near-wall region, create layers of prism cells on walls and the fluid side of solid-fluid interfaces.
The thickness of prism layers next to the wall has a direct impact on fluid y+ values. Check the y+ values in the solution, and make sure that they come within the range of validity recommended for the turbulence model and wall treatment that you have selected.
For high accuracy modeling of boundary layers, create 5–10 cell layers within the boundary layer when using wall functions for the turbulence model. Create around 40 cells in the boundary layer when using a low-Reynolds number turbulence model.

Cell Aspect Ratio

Avoid creating a mesh that has excessive stretching in the direction normal to a wall.
Keep cell aspect ratios as small as possible (for example, below 1000) to avoid convergence problems in the solver. Some problems require lower cell aspect ratios, such as simulations that involve solid stress calculations.

Mixing Applications

These applications typically have two regions: a stationary region and a region with a rotating reference frame. A polyhedral mesh can have cell faces that are not aligned with the flow, which can introduce numerical diffusion. In some simulations, this numerical diffusion can produce a significant discontinuity in the volume fraction at the interface between the stationary and rotating regions. To eliminate this discontinuity, use trimmed meshes for these applications. Trimmed meshing produces mesh that is better-aligned with the interface and minimizes numerical diffusion in the simulation.

Thermophysical Properties

The following guidelines apply only when you use the energy equation in the simulation:

Include the effects of temperature on thermophysical properties such as viscosity, specific heat, and thermal conductivity, when you have the information.
When using temperature-dependent thermophysical properties, make sure that relevant dimensionless numbers maintain the values that you expect them to have. Examples of dimensionless numbers are the Reynolds number and the Prandtl number. As the Prandtl number appears explicitly in temperature wall functions, wall heat transfer predictions are sensitive to the value of thermophysical properties.
When you use constant thermophysical properties, that is, independent of temperature, make sure that you specify all physical properties at the same temperature.
When the Prandtl number is small, (for example, less than 0.1), use a mesh suitable for low values of y+ at the wall.
When you specify surface properties for radiation heat transfer, note that in some circumstances the properties of real surfaces change significantly during service. For example, it is not unusual for the emissivity of an aluminized shield to increase several times through oxidation, dust, or the presence of moisture. This change of emissivity is not automatically captured by Simcenter STAR-CCM+: if you wish to simulate such effects you must alter the surface properties.

Boundary Conditions

Use the following guidelines for defining the boundary conditions.

Choose the shape and location of boundaries so that flow passes through a boundary in one direction only, that is, entering or leaving the domain. Avoid any recirculation across a flow boundary.
As far as possible, choose a static pressure boundary for the outlet boundary.
When possible, extend the computational domain to have flow regions upstream and downstream of the main region of interest. Extending the computational domain in this way minimizes the effect that boundary conditions have on the solution within the main region of interest. You can specify a coarser mesh in extended regions, so that the computational requirements are not increased unduly.
In some simulations, the solution does not converge with the boundary conditions you require. When this situation occurs, start with a different set of boundary conditions and change them as the simulation proceeds. For example, when solving high-Mach number flows over bluff bodies, gradually increase the free-stream Mach number instead of starting with the final value.
Choose boundary types that you know are compatible with the type of flow you are simulating. For example, a velocity inlet boundary is not a well-posed type for a highly compressible flow.

Conjugate Heat Transfer (CHT)

For applications that involve simultaneous heat transfer in both a solid and a fluid, there are two options for obtaining thermal solutions in the solid and the fluid. These options are:

Simcenter STAR-CCM+ can obtain solutions in both the solid and the fluid.
Simcenter STAR-CCM+ can obtain the flow and thermal solution in the fluid only, and pass thermal information to another application that solves for the thermal solution in the solid. An example of this arrangement is where Simcenter STAR-CCM+ exchanges thermal data with Abaqus in an explicitly coupled simulation.

Modeling Conjugate Heat Transfer

For applications that involve simultaneous heat transfer in both a solid and a fluid, such as modeling the fluid and solid in a heat exchanger, the following apply:

Fluid and solid equations are implicitly coupled and are solved simultaneously.
The following surface conditions (temperature and energy) are enforced at the fluid-solid interface:
$T_{{s o l i d |}_{s u r f a c e}} = T_{{f l u i d |}_{s u r f a c e}}$
$q_{{s o l i d |}_{s u r f a c e}} = q_{{f l u i d |}_{s u r f a c e}}$

${- K \frac{\partial T_{s o l i c}}{\partial n} |}_{s u r f a c e} = h_{f} (T_{s u r f a c e} - T_{r e f}) + q_{r a d} + q_{c} + \dots$

where:
- $n$ is the surface outward normal
- $K_{s}$ is the solid conductivity
- $h_{f}$ is the fluid heat transfer coefficient
- $T_{r e f}$ is the characteristic fluid temperature (for example, the domain mean or near wall cell temperature)
- $q_{r a d}$ and $q_{c}$ correspond to net radiative heat flux and added heat flux due to phase change, respectively.

Using Co-Simulation

You can use a single Simcenter STAR-CCM+ simulation to obtain thermal solutions in both the solid and the fluid, where the fluid and the solid are implicitly coupled at the interface. Alternatively, you can use co-simulation to obtain each solution in a separate simulation, where the fluid and the solid are explicitly coupled at the interface and exchange data back and forth as the simulation progresses.

For more information, see STAR-CCM+ to STAR-CCM+ Co-Simulation.

You can use co-simulation when the fluid and solid time scales are significantly different. For example, if the flow is strongly turbulent and well-mixed, and solid conduction is slow, you can assume that the flow adjusts to the changes in the wall temperature quickly. This adjustment is essentially instantaneous with respect to the solid time scale, so the fluid-only simulation can be run steady and the solid-only simulation can be run unsteady. This arrangement allows you to update the fluid solution only when the solid wall temperature has changed significantly.

Co-simulation can provide significant run-time savings, with recent results showing significant speed-ups.

If you use co-simulation, be aware of the following issues:

In co-simulation, convergence problems can arise because the fluid and solid are explicitly coupled. Ensure that:
- The correct information is passed between the simulations.
  For example, the heat transfer coefficient and its corresponding reference temperature are passed from the fluid-only simulation to the solid-only simulation. The wall temperature is passed from the solid-only simulation to the fluid-only simulation.
  
  Although there are other choices of boundary conditions to pass between the simulations (for example, you could pass the wall heat flux from the fluid-only simulation), for numerical stability reasons their use is not recommended.
  
  The recommended heat transfer coefficient and corresponding reference temperature are:
  - Fluid flow with turbulence:
    Use the Specified Y+ Heat Transfer Coefficient and Specified Y+ Heat Transfer Reference Temperature. Start with a y+ of 100, but if needed for better convergence behavior, you can try a different y+. Increasing y+ decreases the Specified Y+ Heat Transfer Coefficient while decreasing y+ increases the Specified Y+ Heat Transfer Coefficient.
  - Fluid flow without turbulence:
    Use the Local Heat Transfer Coefficient and Local Heat Transfer Reference Temperature. If necessary, you can linearly transform this pair to another pair that has better convergence behavior.
- The correct co-simulation parameters are used. For example, the number of iterations, time-step, and update frequency.
Loss of accuracy. The amount of accuracy loss strongly depends on the co-simulation parameters that are used and the amount of speed-up desired.

Co-Simulation Time Scales

In a co-simulation, the fluid and solid systems are solved independently: a separate system of equations is solved for each of the fluid and solid regions. Some of the most common time scales for the fluid region are as follows:

Diffusion time scale:
$t_{f 1} = \frac{{L_{f}}^{2}}{v}$
Inertial time scale:
$t_{f 2} = \frac{L_{f}}{U_{f}}$
Internal/external forcing time scale:
$t_{f 3} = \frac{1}{ω_{f}}$

The time scale for the solid region is:

Diffusion time scale:
$t_{s} = \frac{{L_{s}}^{2}}{α}$

The time scale ratios are:

[\frac{t_{s}}{t_{f 1}} \frac{t_{s}}{t_{f 2}} \frac{t_{s}}{t_{f 3}}] = [(\frac{{L_{s}}^{2} v}{{L_{f}}^{2} α_{s}}) (\frac{{L_{s}}^{2} U_{f}}{L_{f} α_{s}}) (t_{s} ω_{f})]

where:

$L_{f}$ and $L_{s}$ are characteristic length scales (such as domain or grid size) for the fluid and solid, respectively
$v$ is the fluid kinematic viscosity
$U_{f}$ is a characteristic velocity scale (for example, domain mean or cell velocity)
$ω_{f}$ is a characteristic forcing frequency
$α_{s} = \frac{K_{s}}{ρ C_{p}}$ is the solid diffusivity.

Run Time Speed-Up

The run time of an implicitly coupled (unsteady) CHT simulation is:

t_{t o t a l}^{I C} = \frac{t_{f i n a l}}{Δ t} (N_{i t} τ_{i t})

where:

$t_{f i n a l}$ is the simulation ending time
$Δ t$ is the time-step
$N_{i t}$ is the number of inner iterations per time-step
$τ_{i t}$ is the CPU time per inner iteration.

The run time of an explicitly coupled CHT co-simulation is:

Fluid (steady): short time scale
Solid (unsteady): long time scale

t_{t o t a l}^{E C} = (\frac{t_{f i n a l}^{s}}{t_{e x}^{s}}) [(N_{i t}^{f} τ_{i t}^{f}) + (\frac{t_{e x}^{s}}{{Δ t}^{s}}) (N_{i t}^{s} τ_{i t}^{s})]

where:

$t_{f i n a l}^{s}$ is the solid simulation ending time
$t_{e x}^{s}$ is the exchange period between the solid and fluid simulations
$N_{i t}^{f}$ and $N_{i t}^{s}$ are the fluid and solid number of inner iterations, respectively
$τ_{i t}^{f}$ and $τ_{i t}^{s}$ are the fluid and solid run times per inner iteration, respectively
${Δ t}^{s}$ is the solid simulation time-step.

In general, the speed-up in run time of an explicitly coupled CHT co-simulation when compared to an implicitly coupled CHT simulation is:

\frac{t_{t o t a l}^{I C}}{t_{t o t a l}^{E C}} = \frac{N_{i t} τ_{i t} t_{e x}^{s}}{\frac{Δ t}{{Δ t}^{s}} [{Δ t}^{s} N_{i t}^{f} τ_{i t}^{f} + t_{e x}^{s} N_{i t}^{s} τ_{i t}^{s}]}

Setting the Co-Simulation Parameters

When you set up a CHT co-simulation, you specify various co-simulation parameters, including:

Mapping Mode
Iteration Count
Update Frequency
Time Step

For the best results, use a conformal mesh at the solid to fluid interface. A conformal mesh is one whose vertices and faces match exactly on either side of an interface.

Setting the Initial Parameter Values

After setting the initial settings for these parameters, run the co-simulation. If necessary, you can perturb near these initial settings and look for combinations that give better results (that is, a set of parameters that give good accuracy and short run times).

Fluid-Only Simulation (Steady)

Iterations
Set the number of iterations, which in general can be a strong function of time, to whatever it takes for convergence (that is, for the residuals to stop changing).

Solid-Only Simulation (Unsteady)

Update Frequency
Set the initial update frequency to:

$f_{s} = \frac{1}{β t_{s}} = \frac{α_{s}}{β L^{2}} = \frac{K_{s}}{ρ_{s} C_{p, s} L^{s} β}$

where:
- $L$ is a characteristic length scale for the solid (for example, overall length, half length, grid size)
- $β$ is a scaling factor less than one (for example, 0.2 is a good first choice).
Time-step
Set the solid-only simulation time-step ${Δ t}^{s}$ to be some fraction of the update period. For example, $β t_{s} / 10$ can be appropriate if the solution is smooth and not too steep.

Alternatively, you can set the update period $β t_{s}$ to a particular amount of change in wall temperature (for example, the maximum change in one cycle). This allows the update period to adjust itself and the time-step as the simulation progresses.
Iterations
Set the number of inner iterations to whatever it takes for convergence.

Cyclone Separators

This section gives some guidelines for modeling cyclone separators. When you are modeling cyclone separators, consider the following:

Meshing: In order to minimize unwanted numerical diffusion effects, the best type of mesh is a hexahedral type with the mesh elements aligned with the circumference of the cyclone.; You can use the Directed Meshing feature to construct this mesh within Simcenter STAR-CCM+.
Turbulence Model: An anisotropic turbulence model is required to model accurately the free to forced vortex transition that occurs in cyclonic flows. Standard K-Epsilon models and other models that are based on assumptions of isotropic turbulence are not suitable. These models tend to over-predict the turbulent viscosity and exaggerate the forced vortex.
Boundary Layer Resolution: Wall resolution is not critical as the turbulence is generated in the main flow.

Freezing the Solvers

If used correctly, freezing the solvers can be of great use in promoting initial simulation stability, computational efficiency, and total run time. There are two primary situations in which freezing solvers can help:

Early in the simulation, convergence issues can arise because of the lack of a good physical initial condition for transient simulations or initial iteration for steady simulations. At this point, you can activate solver verbosity so that you see exactly what each solver is doing and where problems occur. Freezing the solvers that are associated with more complex physics can allow you to obtain approximate converged solutions. Thereafter you can unfreeze the solvers one by one, continuing the solution each time, to see if any convergence issues remain.
Later in the simulation, because of differing physical time scales or for purely numerical reasons, some solvers reach their asymptotic states much faster than others and are no longer significantly changing the solution.
For instance, in a typical conjugate heat transfer problem, the flow time scale can be small and the solid conduction time scale can be large. Consider, for example, the flow of hot water in a thick-walled pipe. The temperature of the inner pipe wall quickly reaches the temperature of the hot water; the flow solution stabilizes to a steady flow condition. If the only remaining solution concerns the thermal distribution within the pipe wall, then the flow solvers can be frozen while the energy solver runs.

For quantities that have reached their asymptotic states in steady simulations, you can freeze the solvers for the remainder of the simulation. Solvers can be frozen for the remainder of steady simulations. For unsteady simulations where transient effects occur, do not keep solvers frozen for a time longer than the time-scale of the transient effects. (That is, freeze the solvers for a short time and then unfreeze them to see if their asymptotic states have changed. Repeat the procedure as needed). This workflow is similar in nature to co-simulation but is not as flexible.