Detailed Setting of Fluid Analysis

Setting Item

Notes

Advection Scheme

For a stable calculation of advection, physical quantities of the upwind nodes are used.

The use of those physical quantities is called 'upwind differencing scheme'.

Due to the numerical viscosity, the calculation result by this scheme is known to be closer to the calculation result of the material with high viscosity.

Femtet allows for three upwind differencing schemes.

1st-order Upwind Differencing Scheme

Accuracy is low due to the large numerical viscosity. Calculation is stable.

2nd-order Upwind Differencing Scheme

Accuracy is high due to the low numerical viscosity. Calculation is unstable in some cases.

Unusual values (overshooting or undershooting) occur locally in some cases.

2nd-order Upwind Differencing Scheme[suppress abnormal value]

Accuracy is high due to the low numerical viscosity. Calculation is unstable in some cases.

Unusual values (overshooting or undershooting) are less likely to occur than in the [2nd-order Upwind Differencing Scheme] above.
In contrast, the residual may not decrease in the later part of the analysis, and the calculation may not converge in some cases.

Velocity (advection of momentum) and temperature (advection of heat energy)
can be calculated by either one of the three methods.

Advection scheme for diffusion quantity in diffusion analysis can be selected in the [Diffusion Analysis Setting].

K_Turbulent flow energy, ε_energy dissipation rate, and ω_specific dissipation rate are calculated by the 1st-order upwind differencing scheme.

Convergence Judgment Setting

Iterative calculations are repeated until the convergence is achieved in the fluid and fluid-thermal analysis.
It is judged that the convergence is achieved
when the residual of each calculation becomes less than the value in [Convergence judgment].

Different values for convergence judgment can be set for fluid analysis and thermal analysis.

The calculation will stop when the iterations reach the [Maximum number of iterations].

If the calculation stops in the transient analysis, the calculation for the following time will begin.

[Maximum number of iterations] is a positive integer. (0 not inclusive)

Different values can be entered in the steady-state analysis and the transient analysis.

The significand of [Convergence judgment (heat)] is a positive real number. (0 not inclusive)

The significand of [Convergence judgment (fluid)] is a positive real number. (0 not inclusive)

If the calculation does not converge, try the following.
1. Increase the maximum number of iterations.
2. Increase the convergence judgment value (residual).
3. Reduce the relaxation factor.

See the technical note: [If Fluid Analysis/Fluid-Thermal Analysis Does Not Converge] for more information.

If monitoring is set on the [Monitoring] tab, the convergence can be judged by the convergence state of a monitoring value.

If [Convergence Judgment by Monitoring Value] is selected, calculations are judged converged if both of the following are true:

・At all temperatures, three times the standard deviation is less than or equal to [Temperature Tolerance]. (The standard deviation is calculated using the temperature data from the last iterations. The last iterations are 30 for a steady-state analysis and 5 for a transient analysis.)

・The variation, CV value, of monitoring values other than temperatures is less or equal to [Variation Tolerance]. (The variation is calculated using the monitored values from the last iterations. The last iterations are 30 for a steady-state analysis and 5 for a transient analysis.)

・All residuals are less or equal to 10 times the value for convergence judgment.

If [Automatic Monitoring Setting] is selected,

In the fluid analysis, the pressure (total pressure) and volumetric flow rate of all boundary conditions are registered for monitoring.

In the fluid thermal analysis, the maximum temperatures of all body attributes are also registered for monitoring.

In Example 14: Cooling by Fan], the convergence is judged by the monitoring value.

Relaxation Factor

In the fluid analysis, the calculation is iterated and gradually approaches the correct value.
In the laminar analysis, flow velocity and pressure are calculated in one iteration.

In the turbulent analysis, flow velocity, pressure, K_turbulent energy, and ε_engergy dissipation rate or ω_specific dissipation rate are calculated in one iteration.

An additional process for calculating temperature is included in the two-way coupled analysis of the thermal-fluid solver (if the buoyancy is taken into account or the viscosity is temperature dependent).

An additional process for calculating the diffusion quantity is included in the diffusion analysis where the weight of diffusing material is taken into account.

The increment of each physical quantity is calculated. Each physical quantity is updated by applying the relaxation factor to the increment.

It prevents the diversion of calculation.

The likelihood of diversion is smaller if the smaller relaxation factor is applied, but it will require more iterations and calculation time.

Different values can be set in the steady-state analysis and the transient analysis.
As the steady-state analysis is more likely to diverge, the default values are small.

In the laminar analysis, velocity and pressure are set.

In the turbulent analysis, in addition to flow velocity and pressure, K_turbulent energy and ε_engergy dissipation rate or ω_specific dissipation rate are set.

The temperature is also set in the two-way coupled analysis of the the thermal-fluid solver (if the buoyancy is taken into account or the viscosity is temperature dependent).

The diffusion quantity is also set in the diffusion analysis where the weight of diffusing material is taken into account. ( Alternatively, the relaxation factor of the diffusion quantity can be set further in [Diffusion Analysis Setting].)

Click [Reset to Default Setting] to return to the default values.

For the transient analysis, use the same pressure calculation method as the steady-state analysis

In the transient analysis, calculation method is different from the steady-state analysis in order to reduce the iterations.
It may cause divergence in some cases.

Select this option if the calculation does not converge.

Although the iterations will increase, divergence may be avoided.

For this option, the relaxation factprs of flow velocity and pressure in the steady-state analysis are used.

Calculate quasi-steady state in the case of non-convergence

Switches to the calculation using finite timesteps if calculation did not converge.
Effective for the case where steady state does not exist due to the non-steady vibration.
Outputs an instantaneous state of the vibration.

Correct the pressure condition to balance with buoyancy.

In the cases below, pressure are corrected with the slope by height taken into account.

・In the fluid thermal analysis with buoyancy taken into account, if the fluid with a temperature other than the reference temperature flows in.

・In the diffusion analysis with weight of diffusing materials taken into account, if the fluid with a diffusion value other than an ambient value flows in.

・In the free surface analysis (VOF method) with gravity taken into account, if the fluid of a phase other than the lightest phase flows in.

Analyze with pressure varying depending on the height from the reference point at z=0. See Pressure in Fluid Analysis for more information.

Result Output Setting

Specifies the output method of the intermediate result.

Intermediate result during the iteration can be saved and examined if the calculation was aborted, diverged or did not converge.

If [Don't save] is selected, the intermediate result will not be saved. This option is recommended if the result file becomes large.

If [Output only when the calculation did not converge] is selected, the intermediate result of iteration can be examined when the calculation was suspended or did not converge. The intermediate result is deleted if the calculation converges.

If [Output at all times] is selected, the intermediate result is saved also for the successful analysis.

If [Output main fields only] is selected, only main fields such as flow velocity and pressure will be saved. Then the result file will become compact.

Refer to Fluid Analysis of Displayable Results for Each Analysis, for output fields.

Control Volume Type

Node-centered Base (robustness prioritized)

Although robustness is prioritized, it leads to longer calculation times and higher memory usage.

Cell-centered Base (speed prioritized)

If hexahedral mesh is not selected in the mesh tab, a fluid portion is meshed with polyhedral elements and a solid portion into tetrahedral elements.

This control volume type is likely to achieve shorter calculation time and less memory usage.

※ In the case of the free surface analysis, [Cell-centered Base] is applied to the control volume type.

Turbulent Flow Model

Selects the turbulent flow model for calculation.

k-ε Model

This model demonstrates good repeatability when calculating the flow in the domain off the wall face. If no solid wall boundary condition, select this model for the turbulent model.

Use the Wolfshtein one-equation model for the domain near the wall face, and the Realizable k-ε model for the fully turbulent flow domain in calculations.

See Differential Equations in Fluid Analysis/Fluid-Thermal Analysis for more information.

SST k-ω Model

The model demonstrates good repeatable accuracy when calculating the flow in the domain near the wall face.

This is the low-Reynolds-number type turbulence model and, also in the range of the viscous sublayer near the wall face to the logarithm region, you can use the accurate two-equation model for calculation.

The calculation may not converge in the steady-state analysis of free flow such as natural convection. In such cases, the k-ε model is recommended.

Control Volume Type

Node-centered Base (robustness prioritized)

Uses control volumes each formed in such a manner that a node of mesh is central, to calculate.

This type is robust; however, it may cause large-scale calculations to require more time and more memory.

If triangular/tetrahedral free mesh is selected on the mesh tab, [Node-centered Base] is applied to the control volume type.

[Cell-centered Base (speed prioritized)]

Use control volumes each defined by a mesh cell, to calculate.

If [Polyhedral Free Mesh] is selected on the mesh tab, a fluid portion is meshed with polygonal/polyhedral elements for calculation.

This type is better in speed (calculation time) and memory usage than the node-centered one.

In the case of complex shapes, this type may not be robust; that is, calculations may not converge.

For the free surface analysis, this type is automatically selected.