The aim of this test case is to validate the calculation of following flow quantities:
using incompressible steady-state turbulent models applied to water flow through a straight pipe.
Two turbulence models were used: the
. Simulation results from SimScale were compared to the analytical results . The mesh was generated on the SimScale platform using the Hex-dominant parametric type of meshing operation.
A straight cylindrical pipe was chosen as the flow domain (see Fig.1.). Faces A, B and C represent the inlet, wall and outlet patches, respectively.
|Length [m]||Diameter [m]|
In this study the focus was on two turbulence models: the
model and the
. These models fall under the category of Reynolds Averaged Navier-Stokes (RANS) method of turbulence modeling.
A typical property to assess the mesh quality in regards to the near-wall modeling in turbulent simulations is the
(“y-plus”) value, which is defined as the non-dimensional distance to the wall; it is given by
value of 1 would correspond to the upper limit of the laminar sub-layer.
There are two ways of modeling the physics of near-wall flow in RANS models:
- “Full resolution” of the near-wall region: This approach explicitly models the boundary layer all the way down to the laminar sub-layer. It requires the first cell center to be placed at most at the top of the laminar sub-layer, where
. This procedure demands computational grid resolution in to be very fine. Boundary conditions for this approach are given in Table 2.
- Use of wall-functions to resolve the near-wall region: This approach allows for the center of the first cell next to the wall boundary to be placed in the range:
. Boundary conditions for this approach are given in Table 1.
In this validation project both approaches are investigated – wall functions for both
turbulence models; and full boundary layer resolution for
Uniformly-spaced hexahedral meshes were generated on the SimScale platform, using the hex-dominant parametric meshing operation (see Fig.2.). For the “wall function” approach, the aimed first cell layer thickness was around
, with the intention of
. For the “Full resolution” case, the aimed first cell layer thickness was
, with the intention of achieving
Tool Type : OPENFOAM®
Analysis Type : Incompressible Steady-state (Turbulent)
Turbulence Models :
Mesh and Element types :
|Mesh type||Cells in x||Cells in y||Cells in z||Total number of cells||Refinements|
|hex-dominant parametric||19||500||19||179092||Inflate boundary layer|
|hex-dominant parametric||20||1000||20||451360||Inflate boundary layer|
Fig.2. Meshes used for the Turbulent Pipe Flow validation: left is used for wall function (
) approach, right for full resolution(
Boundary conditions are given in the Tables 1. and 2. below:
Table 1. Boundary Conditions for the “Wall function approach”:
|Zero Gradient||Wall Function||Wall Function||Wall Function|
|Zero Gradient||Zero Gradient||Zero Gradient|
Table 2. Boundary Conditions for the “Full resolution approach”:
|Zero Gradient||0||Wall Function|
|Zero Gradient||Zero Gradient|
represents the turbulence kinetic energy. It is calculated as:
is the average velocity in the pipe cross-section and
is the turbulence intensity, which can be calculated for fully developed pipe flow as:
, the turbulent dissipation rate
is calculated as:
is an empirical constant specified in the turbulence model.
Specific turbulent dissipation rate
is calculated as:
In both expressions above
is the turbulent length scale, where
is the hydraulic diameter, which for circular pipes is equal to the diameter
Table 2. lists boundary conditions prescribed for full boundary layer resolution case with
being around 1 and using
turbulence model. It shows that at the pipe surface,
was set to be
, while for
a wall function is prescribed. This it the recommended setting for meshes with
for the version of OPENFOAM® turbulence models currently running on SimScale platform. The validity of such choice will be demonstrated in the result section below.
The velocity profile for turbulent pipe flow is approximated by an empirically derived relation :
For turbulent flow, the ratio of
to the mean flow velocity is a function of
. In this case, this ratio is calculated to be
is a measure of the curvature of the profile. For this case, it is calculated to be
The pressure drop for turbulent flow in pipes is obtained by the Darcy friction factor
calculated by the solution of the Colebrook equation. The solution of the Colebrook equation is plotted in the form of the Moody diagram (See Fig.3.) and for this case, the value of
. This value is then used to calculate the pressure drop using the Darcy-Weisbach equation:
The comparison of simulation results using wall function approach with the result of analytical calculation is given in Fig.3A and 3B. Pressure drop along the pipe length can be observed in Fig.3A, while Fig.3B shows the developed radial velocity profile, located
from the inlet.
The first cell center for “wall function approach” is on average at
. For “full resolution”, average wall distance of first cell center is at
. These values were calculated from simulation results.
Besides good agreement with the analytical model, results show that
are equally successful in predicting the pressure drop along pipe length using “wall function” approach, for the given mesh.
Fig.3. Pressure drop along the pipe length (A) and radial velocity profile (B) – for simulations with wall function approach
is chosen for full boundary layer resolution case since it takes advantage of accuracy of
model in proximity of no-slip boundaries, while in the free-stream flow it uses
formulation, thus avoiding the tendency of
of being too sensitive to inlet turbulence quantities. Switching between the two formulations is done seamlessly by blending functions. Moreover, use of
formulation close to the wall makes the
directly applicable for full resolution case, since it does not need extra damping functions to ensure correct behavior close to walls.
The comparison of simulation results using full resolution approach with the analytical calculations is given in Fig.4C and 4D. Pressure drop along the pipe length can be observed in Fig.4C, while Fig.4D shows the developed radial velocity profile, located
from the inlet.
Fig.4. Pressure drop along the pipe length (C) and radial velocity profile (D) – for simulations with full boundary layer resolution.
Average pressure difference between inlet and outlet is better predicted by
and full resolution modeling, while pressure distribution along wide range of
values is equally well predicted with wall function as well as the full resolutionmodeling.
Velocity profiles from simulations using full resolution approach show better prediction of maximum velocity at the pipe centerline, as well as better agreement with analytical model in areas of high velocity gradient, i.e. close to the wall. The reason for the latter lies in the mesh used for “wall function” modeling. Precisely in its coarseness in the near-wall region, which was deliberately introduced in order to place the first cell center in the
region. Flow velocity is relatively low in the present case, which reflects in boundary layer thickness, and ultimately in the height of first cell next to the boundary. This kind of situations is sometimes faced in modeling, meaning that a certain modeling approach can be more or less favorable for a specific application.
Taking all results in consideration, it can be observed that a generally good correspondence exists between analytical results and SimScale simulations.
|||(1, 2, 3) A Course in Fluid Mechanics with Vector Field Theory – Dennis C. Prieve|
This offering is not approved or endorsed by OpenCFD Limited, producer and distributor of the OpenFOAM software and owner of the OPENFOAM® and OpenCFD® trade marks. OPENFOAM® is a registered trade mark of OpenCFD Limited, producer and distributor of the OpenFOAM software.