By default, ANSYS Fluent stores discrete values of the scalar at the cell centers
(
and
in Figure 21.3: Control Volume Used to Illustrate Discretization of a Scalar
Transport Equation).
However, face values
are required for the
convection terms in Equation 21–2 and must
be interpolated from the cell center values. This is accomplished
using an upwind scheme.
Upwinding means that the face value is derived
from quantities in the cell upstream, or “upwind,” relative
to the direction of the normal velocity
in Equation 21–2. ANSYS Fluent allows you to choose from several upwind schemes: first-order
upwind, second-order upwind, power law, and QUICK. These schemes are
described in First-Order Upwind Scheme – QUICK Scheme.
The diffusion terms in Equation 21–2 are central-differenced and are always second-order accurate.
For information on how to use the various spatial discretization schemes, see Choosing the Spatial Discretization Scheme in the User’s Guide.
When first-order accuracy is desired, quantities at cell faces
are determined by assuming that the cell-center values of any field
variable represent a cell-average value and hold throughout the entire
cell; the face quantities are identical to the cell quantities. Thus
when first-order upwinding is selected, the face value is
set equal to the cell-center value of
in the upstream cell.
Important: First-order upwind is available in the pressure-based and density-based solvers.
The power-law discretization scheme interpolates the face value
of a variable, , using the exact solution to a one-dimensional
convection-diffusion equation
(21–4) |
where and
are constant across the interval
. Equation 21–4 can be integrated to yield the following
solution describing how
varies with
:
(21–5) |
|
where | |
|
| |
|
|
and is the Peclet number:
(21–6) |
The variation of between
and
is depicted in Figure 21.4: Variation of a Variable Phi Between x=0 and x=L (Equation 21–4) for a range of values of the Peclet number. Figure 21.4: Variation of a Variable Phi Between x=0 and x=L shows that for large
, the value of
at
is approximately equal to the upstream
value. This implies that when the flow is dominated by convection,
interpolation can be accomplished by simply letting the face value
of a variable be set equal to its “upwind” or upstream
value. This is the standard first-order scheme for ANSYS Fluent.
If the power-law scheme is selected, ANSYS Fluent uses Equation 21–5 in an equivalent “power law” format [368], as its interpolation scheme.
As discussed in First-Order Upwind Scheme, Figure 21.4: Variation of a Variable Phi Between x=0 and x=L shows that for large Pe, the value
of at
is approximately equal to the upstream
value. When
= 0 (no flow, or
pure diffusion), Figure 21.4: Variation of a Variable Phi Between x=0 and x=L shows
that
may be interpolated using a simple linear
average between the values at
and
. When the Peclet
number has an intermediate value, the interpolated value for
at
must be derived by applying
the “power law” equivalent of Equation 21–5.
Important: The power-law scheme is available in the pressure-based solver and when solving additional scalar equations in the density-based solver.
When second-order accuracy is desired, quantities at cell faces
are computed using a multidimensional linear reconstruction approach [27]. In this approach, higher-order accuracy is achieved
at cell faces through a Taylor series expansion of the cell-centered
solution about the cell centroid. Thus when second-order upwinding
is selected, the face value is computed using the
following expression:
(21–7) |
where and
are
the cell-centered value and its gradient in the upstream cell, and
is the displacement vector from the upstream cell centroid to the
face centroid. This formulation requires the determination of the
gradient
in
each cell, as discussed in Evaluation of Gradients and Derivatives. Finally, the gradient
is
limited so that no new maxima or minima are introduced.
Important: Second-order upwind is available in the pressure-based and density-based solvers.
In some instances, and at certain flow conditions, a converged solution to steady-state may not be possible with the use of higher-order discretization schemes due to local flow fluctuations (physical or numerical). On the other hand, a converged solution for the same flow conditions maybe possible with a first-order discretization scheme. For this type of flow and situation, if a better than first-order accurate solution is desired, then first-to-higher-order blending can be used to obtain a converged steady-state solution.
The first-order to higher-order blending is applicable only when higher-order discretization is used. It is applicable with the following discretization schemes: second-order upwinding, central-differencing schemes, QUICK, and third-order MUSCL. The blending is not applicable to first-order, power-law, modified HRIC schemes, or the Geo-reconstruct and CICSAM schemes.
In the density-based solver, the blending is applied as a scaling factor to the reconstruction gradients. While in the pressure-based solver, the blending is applied to the higher-order terms for the convective transport variable.
To learn how to apply this option, refer to First-to-Higher Order Blending in the User's Guide.
A second-order-accurate central-differencing discretization scheme is available for the momentum equations when you are using the LES turbulence model. This scheme provides improved accuracy for LES calculations.
The central-differencing scheme calculates the face value for
a variable () as follows:
(21–8) |
where the indices 0 and 1 refer to the cells that share face ,
and
are
the reconstructed gradients at cells 0 and 1, respectively, and
is the vector directed from the cell centroid toward the face centroid.
It is well known that central-differencing schemes can produce unbounded solutions and non-physical wiggles, which can lead to stability problems for the numerical procedure. These stability problems can often be avoided if a deferred correction is used for the central-differencing scheme. In this approach, the face value is calculated as follows:
(21–9) |
where UP stands for upwind. As indicated, the upwind part is treated implicitly while the difference between the central-difference and upwind values is treated explicitly. Provided that the numerical solution converges, this approach leads to pure second-order differencing.
Important: The central differencing scheme is available only in the pressure-based solver.
The central differencing scheme described in Central-Differencing Scheme is an ideal choice for LES in view of its meritoriously low numerical diffusion. However, it often leads to unphysical oscillations in the solution fields. In LES, the situation is exacerbated by usually very low subgrid-scale turbulent diffusivity. The bounded central differencing scheme is essentially based on the normalized variable diagram (NVD) approach [265] together with the convection boundedness criterion (CBC). The bounded central differencing scheme is a composite NVD-scheme that consists of a pure central differencing, a blended scheme of the central differencing and the second-order upwind scheme, and the first-order upwind scheme. It should be noted that the first-order scheme is used only when the CBC is violated.
Important: The bounded central differencing scheme is the default momentum discretization scheme for the LES, DES, SAS, SDES, and SBES turbulence models.
Important: The bounded central differencing scheme is available only in the pressure-based solver.
For quadrilateral and hexahedral meshes, where unique upstream
and downstream faces and cells can be identified, ANSYS Fluent also
provides the QUICK scheme for computing a higher-order value of the
convected variable at a face. QUICK-type schemes [266] are based on a weighted average of second-order-upwind
and central interpolations of the variable. For the face
in Figure 21.5: One-Dimensional Control Volume, if the flow is from
left to right, such a value can be written as
(21–10) |
in the above equation results
in a central second-order interpolation while
yields a second-order
upwind value. The traditional QUICK scheme is obtained by setting
. The implementation
in ANSYS Fluent uses a variable, solution-dependent value of
, chosen so as to avoid
introducing new solution extrema.
The QUICK scheme will typically be more accurate on structured meshes aligned with the flow direction. Note that ANSYS Fluent allows the use of the QUICK scheme for unstructured or hybrid meshes as well; in such cases the usual second-order upwind discretization scheme (described in Second-Order Upwind Scheme) will be used at the faces of non-hexahedral (or non-quadrilateral, in 2D) cells. The second-order upwind scheme will also be used at partition boundaries when the parallel solver is used.
Important: The QUICK scheme is available in the pressure-based solver and when solving additional scalar equations in the density-based solver.
This third-order convection scheme was conceived from the original MUSCL (Monotone Upstream-Centered Schemes for Conservation Laws) [496] by blending a central differencing scheme and second-order upwind scheme as
(21–11) |
where is defined
in Equation 21–8, and
is computed using the second-order upwind scheme
as described in Second-Order Upwind Scheme.
Unlike the QUICK scheme, which is applicable to structured hex meshes only, the MUSCL scheme is applicable to arbitrary meshes. Compared to the second-order upwind scheme, the third-order MUSCL has a potential to improve spatial accuracy for all types of meshes by reducing numerical diffusion, most significantly for complex three-dimensional flows, and it is available for all transport equations.
Important: The third-order MUSCL currently implemented in ANSYS Fluent does not contain any Gradient limiter. As a result, it can produce undershoots and overshoots when the flow-field under consideration has discontinuities such as shock waves.
Important: The MUSCL scheme is available in the pressure-based and density-based solvers.
For simulations using the VOF multiphase model, upwind schemes are generally unsuitable for interface tracking because of their overly diffusive nature. Central differencing schemes, while generally able to retain the sharpness of the interface, are unbounded and often give unphysical results. In order to overcome these deficiencies, ANSYS Fluent uses a modified version of the High Resolution Interface Capturing (HRIC) scheme. The modified HRIC scheme is a composite NVD scheme that consists of a nonlinear blend of upwind and downwind differencing [340].
First, the normalized cell value of volume fraction, , is computed and is used to find the normalized face value,
, as follows:
(21–12) |
where is the acceptor cell,
is the donor cell, and
is the upwind cell, and
(21–13) |
Here, if the upwind cell is not available (for example, unstructured
mesh), an extrapolated value is used for . Directly
using this value of
causes wrinkles in the interface, if the flow is
parallel to the interface. So, ANSYS Fluent switches to the ULTIMATE
QUICKEST scheme (the one-dimensional bounded version of the QUICK
scheme [265]) based on the angle between
the face normal and interface normal:
(21–14) |
This leads to a corrected version of the face volume fraction, :
(21–15) |
where
(21–16) |
and is a vector connecting cell centers
adjacent to the face
.
The face volume fraction is now obtained from the normalized value computed above as follows:
(21–17) |
The modified HRIC scheme provides improved accuracy for VOF calculations when compared to QUICK and second-order schemes, and is less computationally expensive than the Geo-Reconstruct scheme.
Higher order schemes can be written as a first-order scheme plus additional terms for the higher-order scheme. The higher-order relaxation can be applied to these additional terms.
The under-relaxation of high order terms follows the standard
formulation for any generic property
(21–18) |
Where is the under-relaxation factor.
Note that the default value of
for steady-state cases is 0.25 and for transient
cases is 0.75. The same factor is applied to all equations solved.
For information about this solver option, see High Order Term Relaxation (HOTR) in the User's Guide.