Differential pressure flowmeters are commonly used in industrial applications where, however, the upstream flow conditions are usually highly disturbed, caused by the presence, in the network pipe, of elbows, valves, etc. To achieve accurate flow measurements, the use of the cone meter is recommended as the flowmeter has the property to normalize the flow both upstream and downstream. In this paper, the authors present a cone flowmeter of new geometry that allows them to obtain better performance with respect to the original one; in particular, it provides a higher discharge coefficient (

Accurate flow measurements are required in many industry applications. The ability to accurately and cheaply measure the flow rate has, in fact, a significant economic impact upon operating costs in control and production processes of several industries. The obstruction flowmeters are commonly used in typical industrial applications. Examples are the orifice meter, the nozzle meter, the Venturi meter, and Pitot meter. Orifice devices are widely used due to their smaller size and low cost, but their lower discharge coefficient, along with occurring inaccuracies in the measurement, due to erosion and corrosion of the plates

The Venturi meters are, however, considerably larger, heavier, and more expensive than orifice plates. Their installation is also tougher

In this paper, the authors investigate the performance ensured by the cone flowmeter. In

In this paper, a cone flowmeter of new geometry is introduced, and it is able to guarantee higher performances than the original one. A numerical study is also pursued to evaluate the limits of its best working conditions. Its performances have been numerically and experimentally evaluated in terms of the discharge coefficient as a function of the flow rate and by considerations on velocity and pressure fields both upstream and downstream from the meter device. The cone meter normed by the ISO standard ^{®}.

The cone is an obstruction-type flowmeter. The development of such a device arises from the challenge of improving the fluid dynamic performance usually granted by other obstruction flowmeters. Indeed, its tapered shape allows the reduction of the fluid dynamic losses due to the more favourable drag coefficient. Thus, the cone flowmeter shows average performances, which are comparable to the most expensive flowmeters, such as the nozzle flowmeter.

The principle of operation of the cone flowmeter is based on the measurement of the pressure drop upstream and downstream from the cone itself, as for all obstruction devices. The insertion of the obstacle within the flow alters the incoming velocity profile. In addition, the deviation of the streamlines around the obstacle modifies the pressure distribution upstream and downstream from the cone. In this case, the wake effect, due to the streamlines' disturbance, creates a depression zone immediately downstream from the cone base, while, in the frontal region of the cone, the streamlines are abruptly slowed down, with the following pressure increase.

The pressure drop caused by the cone insertion can be related to the mass flow rate of the fluid by means of the Bernoulli relation, valid for incompressible flows.

The discharge coefficient

In this paper, the authors perform a series of studies, both numerical and experimental, aimed at improving the performance of a given cone flowmeter by means of the optimization of its geometry. For both shapes (the original one and the proposed modification) a series of numerical computations have been performed in order to determine the degree of influence.

The cone flowmeter to be optimized is used to measure the fluid flow rate in a piping system feeding combustion air. The considered piping system is part of a combustion test facility owned by AC Boilers S.p.A.

Figure ^{™} type) with an uncertainty of ^{®} Q75) with a declared uncertainty of

global Reynolds number,

pipe diameter such that

Schematic view of the original cone flowmeter, with the upstream and downstream pressure taps.

Schematic view of the proposed modified cone flowmeter.

Proposed cone flowmeter.

Piping system equipping the tested flowmeters.

Schematic view of the installed P-G cone.

In this paper, the evaluation of the features of both geometries has been primarily accomplished by means of a series of numerical simulations based on CFD (computational fluid dynamics) modelling. The target of the simulations is to establish the extent of the influence of the inlet fluid flow rate and the influence of the cone diameter ratio

The same strategy and criteria have been adopted for the numerical modelling of both systems. The simulation procedure is based on the solution of the governing equations, continuum and momentum, with the adoption of an appropriate turbulence model aimed at providing the closure constraints to the RANS (Reynolds-averaged Navier–Stokes) equations. The RANS equations describe entirely the flow behaviour in steady and incompressible conditions. In this paper, the authors use the RNG (Re-Normalization Group)

The CFD provides the numerical solution of the governing equations of motion and describe the flow behaviour. The adopted mathematical model shall consider the flow general condition (incompressible or compressible) and the known boundary conditions.

The mathematical model is based on the mass, momentum, and energy conservation equations (for compressible flows). For incompressible flows, only the mass and momentum conservation equations are considered. In addition, for turbulent flows, the governing equations shall consider the velocity fluctuations around the mean value. In this case, the Reynolds decompositions of both flow pressure and velocity allow us to give approximate time-averaged solutions to the governing equations (mainly mass and momentum for incompressible flows).

In steady and incompressible conditions without any body forces, the time-averaged governing equations are provided in vector form.

The governing equations are solved numerically using the finite-volume approach. According to this method, the entire geometric domain is divided into a finite number of cells. The flow simulations carried out for both geometries have been performed by means of the Ansys Fluent CFD commercial code

Figure

Unstructured mesh for the S-G cone.

Unstructured mesh for the P-G cone flowmeter.

The upstream pipe length is 3-D in both cases and the downstream pipe length has been chosen in order to ensure that the flow conditions, in the flowmeter proximity, are uninfluenced by the boundary condition at the pipe exit. Additionally, the adopted inflation strategy close to the flowmeter and wall boundary layers ensures that at least one grid layer is within the viscous sublayer (

For both geometries, unstructured triangular meshes have been used in all the simulations. In the analysed cases, the unstructured meshing approach, adequately refined at the boundary layers, implies optimized setup time and computational effort. In order to evaluate the suitability of the adopted meshing schemes, further attention has been dedicated to the analysis of the mesh goodness metrics. Checking the mesh quality plays an important role in the assessment of the stability and the accuracy of the numerical computations. The most relevant goodness indicators are the orthogonal quality, the aspect ratio (as a measure of the cell stretching), and the skewness of each cell (a measure of how closely ideal a cell is). The implemented mesh schemes are characterized by cells with orthogonal quality and aspect ratios very close to 1 and a skewness never larger than 0.25. The solution scheme implemented in the CFD solver is based on the pressure–velocity coupling using the SIMPLE scheme

For all the simulations involving the two geometries, some specific boundary conditions have been set. The inlet mass flow rate (air at standard conditions) is among those conditions. Since the main purpose is to evaluate the discharge performance of both flowmeters, it has been considered an inlet mass flow rate ranging from 0.5 kg s

Inlet boundary conditions for simulations relative to both cones.

The verification procedure determines whether the implemented mathematical model has been solved correctly. The task can be accomplished by checking the consistency of the obtained results with the mathematical model, the level of numerical errors (due to the discretization and linearization of the governing equations), and by means of a comparison with hand calculations (if those are easily available). The validation procedure, on the other hand, looks at whether the used mathematical model is correct and, therefore, consistent with the physical problem under study. The task is carried out by checking the simulation results against experimental data. In this paper, the verification procedure is performed through several steps. The preliminary and most basic step to implement consists of a series of sanity checks on the pressure and velocity contours. The following step is a check whether the CFD solution honours the boundary conditions and the physical principles in the mathematical model (i.e. conservation of mass, momentum, and energy in the analysed domain). The check of mass and momentum conservation in the whole domain is straightforward and, therefore, omitted in the paper. An appropriate subsection is dedicated to the energy balance. A further operation to perform (in the verification procedure framework) is the assessment of the acceptability of the linearization error and the discretization error. The first is implemented by checking the residuals and the convergence rate of the solutions of governing equations. In addition, a further check of the convergence rate of the drag coefficient is performed. The check of the discretization error is performed by means of the comparison of the solutions obtained from the mesh refinement.

For a steady incompressible flow, the energy conservation equation is provided by Eq. (

Table

Energy balance check for simulations relative to the standard geometry cone.

Table

Energy balance check for simulations relative to the proposed geometry cone.

The mesh refinement analysis allows us to check the level of discretization error.

Table

Mesh metrics for both geometries.

Figure

Contour plot of the axial velocity difference between the original mesh and the refined one, S-G V-Cone.

Contour plot of the pressure difference between the original mesh and the refined one, S-G V-Cone.

Figures

Contour plot of the axial velocity difference between the original mesh and the refined one, proposed cone.

Contour plot of the pressure difference between the original mesh and the refined one, proposed cone.

The validation of the CFD simulations against experimental data will be later discussed only for the proposed flowmeter geometry, because experimental results could not have been obtained for the standard device due to the instability of the flow caused by its unexpected fluctuation. Such a phenomenon has not occurred for the P-G cone, whose installation is ensured by locking supports in the central area of the lateral surface of the cone at 180

Several simulations have been performed in order to evaluate the performance of the S-G cone with different inlet mass flow rates. In this section, only the solutions obtained with a flow rate of 1.8 kg s

Figure

Velocity vector map, S-G flowmeter.

Figure

Relative static pressure contour plot.

For the proposed cone geometry, the results of the simulations carried out with an inlet mass flow rate of 1.8 kg s

In this case, it is possible to make the same considerations relative to the standard cone. In addition, a comparison of Figs.

Velocity vector map, proposed flowmeter.

Therefore, the introduced flowmeter geometry introduces fewer head losses (Eqs.

The whole fluid flow pattern, through both flowmeters, has been analysed at different mass fluid flow rates, and, therefore, at different Reynolds numbers. Figures

Figure

Relative static pressure contour plot.

Velocity profiles at different axial positions, S-G cone.

Velocity profiles at different axial positions, P-G cone.

Figure

Relative pressure along the axial direction.

It can be noted that the proposed cone geometry ensures reduced pressure drops through the obstacle. Additionally, just upstream of both cones, the static pressure increases. Indeed, the presence of the obstruction within the pipe reduces the effective section. The converging section imposes a back pressure on the upstream, forcing the flow streamlines in the proximity of the pipe centreline to slow down and divert from the centre. The remarkable pressure drop, just downstream from the cone, is due to the flow acceleration through the annular section. Figure

In this section, the authors present a series of results about the evaluation of the performance ensured by the cones, with the purpose of pointing out the enhancements provided by the improved geometry.

The discharge coefficient has been calculated by means of Eq. (

Figure

Pressure drop due to the cone for both geometries.

Figures

Least squares regression fit, S-G cone.

Least squares fit of CFD data, proposed cone.

Least squares fit of experimental data, P-G cone.

Table

Linear fit parameters.

It is possible to point out the excellent agreement of the values, computed from the CFD simulations, with an adopted linear model. Additionally, it is possible to deduce the excellent degree of concordance between the CFD simulations performed on the proposed cone and the relative experimental data. Further, in this study, the authors analyse the performance ensured by both flowmeters with the cone diameter ratio

Mach number contour map, S-G V-Cone,

Figure

Mach number contour map, P-G V-Cone,

Figure

Discharge coefficient vs.

Permanent pressure loss percentage against mass flow rate for both cones,

In addition, the

In this section, the authors perform a detailed analysis of the permanent pressure losses induced by both cone geometries. The permanent pressure losses have been defined as the percentage of the pressure drop (measured at the static pressure taps) induced by the obstruction

Figure

Permanent pressure loss percentage against

The aim of the presented paper is to introduce a cone flowmeter characterized by an optimized geometry. In order to assess the enhancements brought by the introduced flowmeter, a series of comparative analyses with a standard cone have been performed. These studies are based on CFD simulations and experimental measurements (available for the proposed cone only) performed on a test facility. The following considerations can be made because of the carried-out evaluations.

The proposed geometry introduces less downstream turbulence. Consequently, the turbulent dissipation rate, granted by the modified geometry, is more favourable. Such a behaviour implies less permanent pressure loss and a prompter static pressure recovery downstream.

The presented V-Cone exhibits fewer pressure drops, between the measuring pressure taps, for any tested mass flow rate (Fig.

The discharge coefficient is quite independent of the inlet flow conditions, as the flow remains globally turbulent and, at inlet, fully developed (Fig.

The discharge coefficient, ensured by the introduced geometry, is 15.7 % larger for the tested conditions characterized by a cone diameter ratio of 0.726 (Figs.

The influence of cone diameter ratio on the discharge coefficient has been analysed. The standard geometry exhibits a decreasing trend, as

The introduced flowmeter ensures less permanent pressure drops, due to the lower turbulence induced by the characteristic geometry.

Data are not publicly accessible, but they are available on request by directly contacting the corresponding author.

GD performed the simulations and wrote the article. LF designed and performed the measurements and GV advised, reviewed, and recommended the corrections of the article.

The authors declare that they have no conflict of interest.

The authors would like to thank AC Boilers S.p.A. for the access to the data relative to the measurements performed on the test plant.

This paper was edited by Rosario Morello and reviewed by two anonymous referees.