**Micaela Olivetti 1,\*, Federico Giulio Monterosso 1,\*, Gianluca Marinaro 2, Emma Frosina <sup>2</sup> and Pietro Mazzei <sup>2</sup>**


Received: 4 December 2019; Accepted: 28 January 2020; Published: 30 January 2020

**Abstract:** The objective of this paper is to show how a completely virtual optimization approach is useful to design new geometries in order to improve the performance of industrial components, like valves. The standard approach for optimization of an industrial component, as a valve, is mainly performed with trials and errors and is based on the experience and knowledge of the engineer involved in the study. Unfortunately, this approach is time consuming and often not affordable for the industrial time-to-market. The introduction of computational fluid dynamic (CFD) tools significantly helped reducing time to market; on the other hand, the process to identify the best configuration still depends on the personal sensitivity of the engineer. Here a more general, faster and reliable approach is described, which uses a CFD code directly linked to an optimization tool. CAESES® associated with SimericsMP+® allows us to easily study many different geometrical variants and work out a design of experiments (DOE) sequence that gives evidence of the most impactful aspects of a design. Moreover, the result can be further optimized to obtain the best possible solution in terms of the constraints defined.

**Keywords:** optimization; valves; computational fluid dynamic (CFD); CAESES®; SimericsMP+®

#### **1. Introduction**

It is well known that main and pilot stage valves, adopted in hydraulic circuits, have different performance requirements. Typically, main stage valves have high efficiency with adequate bandwidth and power, while pilot ones have rapid transient response and are stable and robust when facing external disturbances. When the power required by the pilot stage comes directly from the main line, pressure affects dynamic behavior and stability, making it difficult to tune the system to respond correctly to all pressure loads [1,2]. For this reason, different solutions are generally used to separate the two stages and make them as independent as possible.

The present study shows a technique to optimize a pilot operated distributor solenoid/hydraulic controlled valve. The presented modeling technique is based on the adoption of two tools, the optimization tool CAESES® (Friendship Systems AG, Postdam, Germany) and a commercial computational fluid dynamics (CFD) code: SimericsMP+® (Simerics Inc.®, Bellevue, WA, USA).

This approach is faster than the one already presented by the authors [1,2] and can be applied to several geometries for the study of the components' internal fluid patterns.

Several examples of valve optimization are available in literature: some of them focused on the fluid dynamic, others on structural aspects [1–11].

Optimization tools and techniques are quite common in structural analysis, as they are used to reduce local stresses or to improve topology of mechanical parts.

For example, Park et al. [12] proposed an approach based on a traditional structural optimization, which identifies the best combination of geometrical parameters to improve the product's performance and to save material. This paper presents a framework that performs the integration between commercial CAD–CAE software. This approach reduces the time for solving computation-intensive design optimization problems so that designers are free from monotonous repetitive tasks. The results show that the proposed method facilitates the structural optimization process and reduces the computing cost compared to other approaches.

Regarding the fluid dynamic aspect, the main problem is to identify how the fluid behaves inside the component. Some examples of fluid dynamic optimization can be found in literature [5–7].

Manring et al. [7,8] modeled a spool–valve to study the flow forces acting on the valve spool. In other scientific papers, the same authors showed the experimental investigation carried out on hydraulic spool valves to measure the pressure transient force action on the valve's spool. The importance of optimizing fluid dynamic forces in modeling and testing approaches was demonstrated by these studies.

Zardin et al. [9] studied valves for mobile applications via a lumped parameter approach. They proposed an innovative design procedure to optimize valve design. The technique involves dedicated simulations to analyze the main critical issues regarding a cartridge valve. Models and simulations were used to define a methodology for designing a new valve. The optimized valve satisfies the requirements and adapts well to the necessities of operating at higher flow and pressure levels without compromising performances.

A useful tool to understand the flow behavior inside a component is three-dimensional computational fluid dynamics, a collection of different numerical techniques that allow to solve the Navier–Stokes equations.

Unfortunately, a main obstacle to implement optimization studies in fluid-dynamics analysis is, still today, computational cost. Furthermore, the setup of such projects typically requires three different tools to interact efficiently: a parametric geometry modeler (CAD), a computational fluid dynamics (CFD) solver and an optimization tool.

Tonomura et al. [13] showed a methodology for the optimization of a microdevice. Even if this component is not in the fluid power field, the approach used could be easily adopted in many research sectors. Authors studied a specific part inside the component using computational fluid dynamics (CFD). Then, a CFD-based optimization method was proposed for the design of plate-fin microdevices. With this approach, the optimal shape was designed almost automatically.

Corvaglia et al. [10] showed an interesting study on a load sensing proportional valve. The valve was modelled using two 3D CFD numerical approaches. The models were validated in terms of flow rate and pressure drop for different positions of the main spool by means of specific tests. This paper brought to evidence the reliability of the CFD models in evaluating the steady-state characteristics of valves with complex geometry.

Salvador et al. [11] adopted a computational fluid dynamics (CFD) approach to design hydraulic components such as valves by inexpensively providing insight into flow patterns, potential noise sources and cavitation. They demonstrated the relevance of the geometric characteristics on the performance. A modification of the geometry in the piston exit leads, for example, to different vortex structures and helps reduce vibrations and forces on the piston.

As mentioned before, Frosina et al. [1,2,8] already studied the valves' fluid-dynamics in order to analyze flow forces, pressures distribution and velocity behavior. All these studies were performed using 1D and 3D CFD modeling approaches depending on the application. Studies have demonstrated the accuracy of the developed methodologies and showed good agreement with experimental data. Geometric parameters were characterized and consequently modified systematically. The three-dimensional model's results, like velocity behavior and pressure distribution, allowed the authors of the study to optimize the valve geometry without losing any of the valve's performance. In

this context, it would have been very advantageous to have access to an automated procedure that could drastically reduce the project duration.

For the project described in this article, just two tools were used: CAESES® (an optimization tool with integrated parametric geometry modelling capabilities) and SimericsMP+®, a commercial CFD solver. This approach greatly reduced the set-up effort and allowed for a leaner and more efficient project layout.

The objective of this work is to show how the shape of a valve ports can be automatically modified, without the use of an external CAD tool, and simulated to obtain the best performing geometry in just a few hours.

The design taken into consideration for the optimization is the geometry of a four-way hydro-piloted valve for industrial applications. In particular, the shape of two ports of the valve was optimized in order to obtain the highest possible mass flux at an imposed pressure drop.

The study began from a baseline geometry, tested with the CFD tool, from which the optimization started.

In the following paragraphs, the integration between the optimizer and the CFD tool as well as the results obtained will be described.

#### **2. Materials and Methods**

The DSP10 valve by Duplomatic MS S.p.A. (Parabiago-MI, Italy) was the object of the optimization study (Figure 1).

**Figure 1.** Valve under investigation.

It is worth noting that a good overall agreement between CFD studies conducted with SimericsMP+® on similar Duplomatic MS S.p.A. valves and experimental tests performed at the Industrial Engineering Department of the University of Naples, Federico II are reported in different publications (e.g., [1,8]).

For optimization purposes, the valve was simulated with fixed spool position so that only ports P and A (in blue in Figure 2) were connected through the spool port recesses (green in Figure 2).

**Figure 2.** Ports A and P (blue) and spool caves (green).

*Fluids* **2020**, *5*, 17

The volume wetted by the oil (Figure 3) was extracted with a CAD tool, and an STL file was exported to be used within the CFD code SimericsMP+® (developed by Simerics Inc.®, Bellevue, WA, USA)).

**Figure 3.** Fluid volumes of the valve.

In the performed study, the SimericsMP+® tool was chosen as a general purpose CFD software that numerically solves the fundamental conservation equations of mass, momentum and energy as described below [14,15].

For the purposes of the study, some simplifications were considered, such as a stationary domain, a steady state flow and an isothermal flow. Given these approximations, some terms of the equations written below are disregarded by the solver during the run.

Mass conservation:

$$\frac{\partial}{\partial t} \int\_{\Omega(t)} \rho d\Omega + \int\_{\sigma} \rho (v - v\_{\sigma}) \cdot \mathbf{n} d\sigma = 0 \tag{1}$$

Momentum conservation:

$$\frac{\partial}{\partial t} \int\_{\Omega(t)} \rho v d\Omega + \int\_{\sigma} \rho ((v - v\_{\sigma}) \cdot n) v d\sigma = \int\_{\sigma} \widetilde{\tau} \cdot n d\sigma - \int\_{\sigma} p n d\sigma + \int\_{\Omega} f d\Omega \tag{2}$$

Energy conservation:

$$\frac{8}{8t} \left[ \rho \left( u + \frac{v^2}{2} + gz \right) \right] + \nabla \left[ \rho v \left( h + \frac{v^2}{2} + gz \right) \right] + \nabla Q - \nabla \left( T\_d v \right) = 0 \tag{3}$$

in which


τ, the shear stress tensor, is a function of the fluid viscosity <sup>μ</sup> and of the velocity gradient. For a Newtonian fluid, this is given by the following Equation (4),

$$
\pi\_{ij} = \mu \left( \frac{\ $\mu\_i}{\$ \mathbf{x}\_j} + \frac{\ $\mu\_j}{\$ \mathbf{x}\_i} \right) - \frac{2}{3} \mu \frac{\ $\mu\_k}{\$ \mathbf{x}\_k} \delta\_{ij} \tag{4}
$$

where *ui* (*i* = 1,2,3) is the velocity component and δ*ij* is the Kronecker delta function.

The software implements mature turbulence models, such as the standard *k* − ε model and Re-Normalization Group (RNG) *k* − ε model [16]. These models have been available for more than a decade and are widely demonstrated to provide good engineering results. The standard k − ε model, used for the simulations presented in this paper is based on the following two equations:

$$\frac{\partial}{\partial t} \int\_{\Omega(t)} \rho k d\Omega + \int\_{\sigma} \rho ((\upsilon - \upsilon\_o) n) k d\sigma = \int\_{\sigma} (\mu + \frac{\mu\_t}{\sigma\_k}) (\nabla k n) d\sigma + \int\_{\Omega} (\mathcal{G}\_t - \rho i\varepsilon) d\Omega \tag{5}$$

$$\begin{split} \frac{\frac{\partial}{\partial t} \int\_{\Omega(t)} \rho \dot{v} d\Omega + \int\_{\sigma} \rho ((\boldsymbol{v} - \boldsymbol{v}\_{\sigma}) \boldsymbol{n}) \boldsymbol{\varepsilon} d\sigma}{= \int\_{\sigma} (\mu + \frac{\mu\_t}{\sigma\_t}) (\boldsymbol{\nabla} \dot{\boldsymbol{n}} \boldsymbol{n}) d\sigma + \int\_{\Omega} \Big( \boldsymbol{c}\_1 \boldsymbol{G}\_t \frac{\boldsymbol{c}}{k} - \boldsymbol{c}\_2 \rho \frac{\boldsymbol{c}^2}{k} \Big) d\Omega} \end{split} \tag{6}$$

with *c*<sup>1</sup> = 1.44, *c*<sup>2</sup> = 1.92, σ*<sup>k</sup>* = 1, σε = 1.3; where σ*<sup>k</sup>* e σε are the turbulent kinetic energy and the turbulent kinetic energy dissipation rate Prandtl numbers.

The turbulent kinetic energy, *k*, is defined as:

$$k = \frac{1}{2}(v' \cdot v')\tag{7}$$

with *v*' being the turbulent fluctuation velocity, and the dissipation rate, ε, of the turbulent kinetic energy is defined as:

$$\varepsilon = 2\frac{\mu}{\rho} \overline{\left( S\_{ij}' S\_{ij}' \right)} \tag{8}$$

in which the strain tensor is:

$$S'\_{ij} = \frac{1}{2} \left( \frac{\ $\mu'\_i}{\$ x\_j} + \frac{\ $\mu'\_j}{\$ x\_i} \right) \tag{9}$$

with *ui*' (*i* = 1,2,3) being components of *v*'.

The turbulent viscosity μ*<sup>t</sup>* is calculated by:

$$
\mu\_t = \rho \mathbb{C}\_{\mu} \frac{k^2}{i\varepsilon} \tag{10}
$$

with *C*μ = 0.09.

The turbulent generation term *Gt can* be expressed as a function of velocity and the shear stress tensor as:

$$G\_t = -\rho \overline{u'\_i u'\_j} \frac{\mathfrak{Y} u'\_i}{\mathfrak{Y} x\_j} \tag{11}$$

where τ *ij* = ρ*u iu <sup>j</sup>* is the turbulent Reynolds stress, which can be modelled by the Boussinesq hypothesis:

$$
\pi'\_{\,ij} = \mu\_t \Big( \frac{\ $\mu\_i}{\$ \mathbf{x}\_j} + \frac{\ $\mu\_j}{\$ \mathbf{x}\_i} \Big) - \frac{2}{3} \Big( \rho \mathbf{k} + \frac{\ $\mu\_k}{\$ \mathbf{x}\_k} \Big) \delta\_{ij} \tag{12}
$$

The valve fluid volume was meshed with the SimericsMP+® grid generator (Figure 4).

**Figure 4.** Grid seen from two different section planes.

SimericsMP+® uses a body-fitted binary tree approach [14,15] This type of grid is accurate and efficient because:


In the configuration considered for the optimization, the spool is fixed in the position that allows the flux from Port P to Port A. The fluid volumes of the ports and the spool were meshed separately and were then connected via an implicit interface.

The SimericsMP+® mismatched grid interface (MGI, see Figure 5) is a very efficient implicit algorithm that identifies the overlap areas and matches them without interpolation. During the simulation process, the matching area is treated no differently than an internal face between two neighboring cells in the same grid domain.

**Figure 5.** Mismatched grid interface (MGI) between the spool and both ports.

Thanks to this approach, the solution becomes very robust, quick and accurate.

The DSP10 valve, the object of the study, was optimized at the most typical condition with a pressure difference of 5 bar.

The CFD model of the considered valve portion consists of 911,150 cells (Figure 4). The following boundary conditions were applied (Figure 6):


**Figure 6.** Boundary conditions on Port A and P.

A static analysis with turbulence was performed on the model. Run time for this analysis was 14 min on an 8 cores Intel Core i7, 3.10 GHz processor with 32 Mb RAM.

In this configuration, a baseline CFD analysis was performed, to be used as reference during the optimization process.

As previously indicated, the optimization process was driven by CAESES®.

CAESES® stands for "CAE System Empowering Simulation" and its ultimate goal is to design optimal flow-exposed products [17]. Starting from a baseline geometry, it is possible within CAESES® to modify the geometry, using different strategies and imposing constraints and parameters to obtain a set of geometries and boundary conditions that will be treated as a design of experiments (DOE) set.

The strategies used for the geometry modifications are:


**Figure 7.** Partially parametric modelling.

**Figure 8.** Fully parametric modelling.

Once the geometric strategy was chosen, CAESES® calculated all the possible shapes within the defined constraints and calculated a DOE sequence for the valid geometrical solutions.

The DOE sequence can also take into account variations of the boundary conditions, but the performed study was only based on geometrical modifications.

The ports of the valve, the object of the study, were modelled in CAESES® using the "fully parametric modelling" approach. The "partial parametric modeling" approach was used for other parts of the model (spool and other ports), although these parts have not been included in this phase of the project.

This means that the original geometry was rebuilt in CAESES® and different geometrical modifications of the valve ports A and B were taken into consideration.

CAESES® allows the user to select the geometry control parameters that are deemed relevant for the problem.

In the specific case, nine parameters for each port were identified:


**Figure 9.** Box height variation. Left original, right max modification.

**Figure 10.** Outer radius variation. Left original, right max modification.

For example, in Figure 9, the box height modification is shown. In Figure 10 the outer radius variation is illustrated.

Not all the control parameters were used for the optimization: a DOE sequence generated with a Sobol algorithm identified four modifications for each port for a totally of eight design variables and 90 variants. In Table 1 these values are resumed.


**Table 1.** The eight design variables with their upper and lower values.

Two variables were monitored in CAESES®: Port A and Port P volumes were monitored not to exceed predefined values.

The objective of the optimization was to maximize the mass flow rate of the valve at a fixed pressure drop.

As the DOE sequence was defined, the CFD simulations for the 90 variants were performed with SimericsMP+®.

The great advantage of using CAESES® is that the code drives all the process automatically; this means that CAESES® generates the geometry that has to be tested on the base of the "design variables".

CAESES® creates the STL file that is used by SimericsMP+® to generate the mesh. SimericsMP+® is then run in batch and generates the new mesh, sets up the simulation and solves the case.

The results from SimericsMP+® are read, via a .txt file, from CAESES®, that evaluates the obtained mass flux value.

Figure 11 illustrates the process scheme:

**Figure 11.** CAESES® automated process.

The CFD analyses were performed on all the 90 design variants.

Considering a mean simulation time of 15 min for SimericsMP+®' shared memory parallel solver on a single processor, eight cores workstation, the whole DOE sequence calculation took 22.5 h; less than one day.

#### **3. Results**
