An advanced CFD model to study the effect of non-condensable gas on cavitation in positive displacement pumps

Abstract An advanced transient CFD model of a positive displacement reciprocating pump was created to study its behavior and performance in cavitating condition during the inlet stroke. The “full” cavitation model developed by Singhal et al. was utilized, and a sensitivity analysis test on two air mass fraction amounts (1.5 and 15 parts per million) was carried out to study the influence of the dissolved air content in water on the cavitation phenomenon. The model was equipped with user defined functions to introduce the liquid compressibility, which stabilizes the simulation, and to handle the two-way coupling between the pressure field and the inlet valve lift history. Estimation of the performance is also presented in both cases.


Introduction
Cavitation in pumps is still a debated topic in technical literature. The main discussed subject focuses on how to correctly estimate the Net Positive Suction Head required (NPSHr) of the device. The reason for the focus on the NPSHr is mainly due to the need to achieve the requirements speciied by the API 610, API 674 and DIN EN ISO 13710, where either for Positive Displacement (PD) pump or centrifugal pumps a certain safety margin to avoid cavitation is set. Since pump manufacturers are required to specify the NPSHr, researchers are called to develop tools and procedures to study cavitation in pumps and to estimate accurately the NPSHr. In the case of centrifugal pumps, for instance, many authors, such as Ding [1], have developed a Computational Fluid Dynamics (CFD) based tool to estimate the NPSH curve, in order to ind the operating conditions where the drop of 3% in head occurs, as speciied by the API. Ding et al. also stated that the deinition of the NPSHr is afected by the content of air in water. Budris and Mayleben [2] carried out a research oriented at understanding the efect of the air content in water in the estimation of the performance of centrifugal pumps. They found that a small amount of air reduces signiicantly the suction pressure pulsation, while increasing the amount of air content above a certain threshold delivers no further improvement on the pressure luctuations, while an increment of the NPSHr occurs.
The case of PD reciprocating pumps appears to be different. The API 674 deines the NPSHr as the NPSH where a decrement of 3% in volumetric eiciency occurs but many authors do not agree in considering the NPSHr in PD pumps a precise engineering requirement. Miller, [3] for instance, stated that any suction pressure above the NPSHr would only improve the performance by increasing the volumetric eiciency and minimizing the efect of the air entrained or dissolved. Other authors such as Opitz and Schlücker [4] presented an experimental study on cavitation in PD pumps indicating that the phenomenon up to a certain limit is harmless, and that strict requirement of the API 674 is perhaps not necessary. In a subsequent study, the same authors [5] discussed the phenomenon of expansion generated cavitation, relating it to the incipient cavitation occurring at the initial stage of the inlet stroke when the plunger of the pump moves backward and the inlet valve is still closed and pushed against its seat by the preloaded spring. This phenomenon will be investigated in more details in this paper. The aim of the study being presented is to answer to the following questions: 1. What is the precise efect of the dissolved gas on cavitation in PD pumps? 2. How does it afect the performance of PD pumps? 3. How does it afect the NPSH?
The authors chose to carry out the investigation by means of the advanced CFD model explained and discussed by Iannetti et al. [6] that will be briely recalled in the next sections. The reason for this choice lies on the higher capability of post processing that a CFD solver has over experimental tests. In fact a crucial prerequisite for the analysis shown is to separate the luid dynamic ields of vapour from that of air, which together constitute the secondary phase. This capability is almost impossible to achieve via experimental investigation.
It is known [7] that clean water at ambient conditions contains 15 ppm (parts per million) of air which is dissolved, as the static pressure lowers during the suction stroke, air separates from the liquid and gathers in bubbles which interact with the pressure ield as air is much more compressible than water. It is also known [8] that water contains also a large amount of nuclei which are microscopic bubbles containing water vapour and air and are located in the crevices of the solid boundaries or on dust particles. This amount of gas which is not dissolved may increase the overall amount of air. The interaction noncondensable gas with the pressure ield implies an expansion of the former: this phenomenon is usually called gas cavitation. Gas cavitation results in a pressure drop slowdown which may result in a delay of the achievement of the vapour cavitation condition and a mitigation of the water vapour generation.
This work simulates the entire suction stroke of the pump, when the plunger moves backward and the minimum pressure peak is achieved. This paper will discuss the complex phenomena occurring during cavitation via detailed post processing data analysis.
For this purpose, two CFD test cases were created and launched, and their results were compared. The cases dealt with a single chamber PD pump subjected to the same operating and boundary conditions; they difered only in the property of the luid processed, the irst case utilizing water with 15 ppm of dissolved air at standard conditions, while the second case utilised a lower air content of 1.5 ppm.

CFD Model, geometry and set-up
The CAD model of a chamber of the PD reciprocating pump shown in Figure 1 was taken in order to create the mesh. The coniguration of the pump CAD ile, which deined the initial luid domain of the simulation is shown in the same igure, where the plunger is located at its Top Dead Centre (TDC) position and the valves are closed. As Iannetti et al. explained [9], the moving mesh algorithm managed the volume deformation and growth due to valve lift, and the displacement volume increment by means of a transient approach. The numerical analysis was focused on the simulation of the inlet stroke which starts when the plunger is located at the TDC and ends when the inlet valve hits the seat after the plunger gets to the Bottom Dead Centre (BDC). According to theory, the valve should get to the seat Brought to you by | The University of Strathclyde Authenticated Download Date | 12/3/15 11:15 AM  as soon as the plunger gets to the BDC, however, because of valve inertia, the operating conditions and the luid properties, there could be a delay in the inlet valve closing time, which would extend the inlet stroke overlapping the irst stage of the outlet stroke. This has been observed by Iannetti et al. [6] but the inluence of the air content on it is still unclear. Solid volumes were utilised to generate the luid volumes by means of Boolean operations; they were subsequently meshed. The choice of the mesh type was made according to the decomposition pattern needed by the moving mesh technique. The process is explained by Iannetti et al. [9] for a slightly diferent geometry but, since the basis hypothesis did not change, the pattern is proposed again as illustrated in Figure 2.
The static and translating volumes were meshed utilizing tetrahedral cells. Expanding/compressing volumes were crucial to simulate the growth of the displacement volume as well as the growth of the valve lift volume located between the valve and the seat (valve-seat gap volume); they were either a cylindrical or annular shaped and were meshed utilizing hexahedral cells so that the expansion/creation of cell layers could afect the height of the parallel cell layers (layering technique [9]). The mesh spacing was decided after a mesh sensitivity analysis, which ixed it as the optimum between the low computational time and high accuracy needs. As explained by Iannetti et al. [9], for this analysis three mesh sizes were tested (Table 1). Meshes 2 and 3 provided the same results, which were more accurate than the ones provided by mesh 1; the latter was also afected by numerical instability. It was decided to carry on the analysis utilizing mesh 2, as it reduced the computational eforts. The details of mesh 2 are shown in Table 2.
The Singhal et al. [11] cavitation model was chosen along with the solver settings and sub-models shown in Table 1. A User Deined function (UDF) was written and attached to the CFD solver in order to manage the two-way coupling between the valve lift and the chamber pressure ield. Figure 3 shows the steps performed by the UDF and how it interfaces to the main numerical solver. A second UDF was written to include the liquid compressibility effects which were of great importance to stabilize the simulation in the instants within the pumping cycle when inlet and outlet valve were both closed; the governing equations have been discussed by Iannetti et al. [9].
A mass dependent inlet pressure was chosen to account for the complex shape of the inlet pipeline. The pump model boundary was ive inlet pipe diameters upstream of the inlet valve and the remaining part of the pipe was simulated by means of separated steady state simulations with 5 kg/s to 30 kg/s mass low. For each of these analyses the pressure drop across the ends of the pipe was taken to build the curve shown in Figure 4. The curve was fed by means of piecewise linear law into the main model of the pump in order to obtain a mass low adjusted pressure inlet condition from a constant level chosen as 0 PaG.   [kPaG] Case 1 and 2 0 -∆P (see Figure 4) 0    The initial and boundary conditions are summarized by Table 4.
An Intel Xeon CPU W3670 @3.2GHz CPU (6 cores) was employed for the simulations. Approximately 10 days was the calculation time needed for each case.
3 Numerical results and discussion Figure 5 shows the time history of the chamber static pressure throughout the inlet stroke for both cases of air mass fractions of 15 and 1.5 ppm. The pressure monitor point was a static point close to the TDC plunger position. The simulations showed that the lower the air content, the closer is the minimum chamber pressure to the cavitation pressure. Figure 5 also shows that in case of lower air content, the pressure drops more quickly than in the irst case, and this results in a low pressure regime that lasts longer and increases the generation of vapour as shown in Figures 6 and 7. Figure 6 shows the situation in terms of secondary phase (air + water vapour) volume fraction in the valveseat volume throughout the inlet stroke. An important remark that has to be pointed out is how the secondary phase volume fraction is actually divided in terms of vapour and air. The left plot of Figure 6 shows the higher secondary phase fraction of the irst case (solid line, 15 ppm air mass fraction) but the middle plot demonstrates that the vapour generation was higher in case 2 (1.5 ppm) at˜25% versus˜16%. Therefore it can be said that case 1 is afected by a higher air expansion rather than vapour generation. Furthermore, while in the irst case air and vapour fractions were evenly˜16% for both, in the second case the diference between vapour and air is signiicant (˜25% ver-sus˜2.5% respectively). Figure 7 shows the secondary phase volume fraction in the vicinity of the plunger top surface throughout the inlet stroke. The plunger region was more afected by a lower vapour volume fraction than the valve region. For instance, considering case 1 (15 ppm), the maximum secondary phase volume fraction was circa 32% (valve-seat gap volume, Figure 6 left); close to the plunger the amount was 19% (Figure 7 left). Furthermore, near the plunger the liquid richer of air showed an uneven subdivision of air and vapour volume fraction, respectively 6% and 13% (solid line, Figure 7 middle and right). Case 2, on the other hand, showed an even subdivision of circa 2.5% air and vapour.
The trends of Figures 6 and 7 Table 5 summarises and quantifyies the performance of the pump. In both cases studied, th evolumetric eiciency loss was higher than 3% but case 1 showed a much lower volumetric eiciency (78.5% against 95%) because of the much higher air content which demonstrated a great inluence in the performance deterioration. Table 5 also shows that the higher is the volumetric eiciency loss, and the bigger is the inlet valve closing delay (the theory indicates the end of the inlet stroke at 180 ∘ of shaft rotation). This can be explained by the time needed for the plunger to compress the secondary phase to convert it (by dissolution) to liquid phase. Furthermore a higher air content resulted in a bigger inlet valve opening delay (12 ∘ against 4 ∘ ) because of the capability of air of expanding and slowing down the chamber pressure drop. Figure 10 shows the mass low rate (left) and inlet valve lift (right) trends of the two cases under investigation. The mass lows are compared to the theory curve, which is calculated considering a one phase incompressible luid with zero inertia inlet valve (diplacement volume times the density of water at standard condition). Case 2 shows an average mass low rate higher than case 1, which explains the higher volumetric eiciency. The valve lift plot shows clearly the diference in closing delay highlighted in Table 3. Figures 11 and 12 show the contour of the secondary phase volume fraction respectively for cases 1 and 2. Both igures represent an image taken when the plunger rotation was 120 ∘ , which is close to the maximum vapour peak generation for both of cases. The contours conirm what was already stated in the discussion of Figure 5 to 10. Vapour is generated mainly in the valve-seat gap volume and propagates afterwards. According to the CFD simulation and supported by Figure 11, the expansion provided by the plunger generates a wide region where the air comes out of the luid phase as dissolved gas and expands randomly around the plunger. This phenomenon is known as gas cavitation and was observed by Opitz and Schlücker [4]. As the amount of air mass fraction was very low, case 2 showed the typical features of vapour cavitation ( Figure 12) whereby the secondary phase is concentrated in the vicinity of the valve, where it is mainly generated.

Conclusion
A transient and comprehensive CFD model of a onechamber PD pump was created to estimate the performance of the device under diferent working luid properties. Two cases were investigated; in case 1 water with 15 ppm of air mass fraction content was considered, while case 2 dealt with a 1.5 ppm air mass fraction dissolved. The operating conditions (i.e. shaft angular speed and inlet pressure) were designed to achieve the full cavitating conditions so that the efect of the non-condensable gas mass fraction content on cavitation could be investigated. The CFD model made use of the Singhal et al. cavitation model [11], the multiphase mixture model [10,12] and two UDFs modelled the compressibility of the luid and the two-way coupling between the valve lift and the pressure ield. The valve spring efect and the valve inertia were also taken into account. A complete inlet stroke was simulated, from the initialization point (plunger located at the TDC) untill the end of the valve lift history. The two cases, in fact demonstrated a diferent dynamics and in case 2 the valve ended the lift sooner than case 1.

General remarks on cavitation
According to the CFD model and under the investigated operating conditions, the plunger expansion created the pressure drop needed for the vapour cavitation to appear but the air expansion (gas cavitation) prevented the vapour formation in the vicinity of the plunger which was afected by the vapour previously generated by the valve rather than that generated by the plunger itself. Once the average static pressure in the chamber ranged around the vapour pressure, and the lowing velocity in the valve-seat gap volume exceeded a certain treshold, vapour cavitation appeared and afected primarily the lift volume; it moved downstream towards the plunger afterwards. The triggering cause of cavitation was the high low velocity (low induced cavitation [4]) rather than the expansion cavitation which appeared to be just a prerequisite.

Influence of the non-condensable mass fraction on cavitation
Non-condensable gas mass fraction inluences the chamber pressure history (Figure 5), the dissolved air slows down the pressure drop while it comes out of the liquid and expands. Air expansion tends to ill the void left by the plunger at the beginning of the inlet stroke when the valve is closed and delays vapour cavitation appearance. Case 1, which deals with a higher gas content luid, shows a lower vapour volume integral than case 2, which deals with a lower air content (Figures 8 and 9). On the other hand the air content is itself a source of volumetric eiciency loss as shown by Table 3. Figure 9 demonstrates that the overall secondary phase content (vapour and air) deines the volumetric eiciency rather than the vapour content itself; in fact, case 1, which shows the highest secondary phase volume integral, also shows the lowest veolumetric eiciency. Figure 5 demonstrate also that the higher the air content, the higher the minimum pressure (absolute value), this provides a further safety factor on cavitation and increases the NPSH of the pump.
The analisys demonstrated the importance of the working liquid properties for an accurate estimation of the performance of the pump as well as the prediction of the cavitation damage. Although the overall content of air (dissolved air plus the nuclei content) is not harmful for the pump, taking into account the non-condensable air mass fraction in cavitation results in a better estimation of the vapour volume fraction prediction. Despite air cavitation, vapour bubbles can harm the pump signiicantly. An accurate prediction of the amount and the location may result in a better understanding of the design and operating parameters afecting cavitation and this implies a reliable support for pump designers and manufacturers.
Future improvement of the analysis presented in this paper is planned, the authors are currently working on a test rig to valdidate the CFD data herein presented.