Abstract

The most reliable and economic way to control fluid leakage from industrial equipment such as centrifugal pumps and mixers is to isolate the rotating shaft and its housing with a mechanical seal. These devices, though simple in concept, present a variety of engineering challenges to the designer.

Of particular concern is the thermofluid environment in which key components of the seal must operate. In order to protect critical parts and ensure functionality, heat caused by sliding friction is commonly removed by forced convection cooling. Experience shows that cooler operating temperatures correlate with improved, more stable performance, reduced wear, and extended life of the seal.

Design concepts for improved fluid sealing were studied using advanced engineering analysis and state-of-the-art data visualization. Computational Fluid Dynamics (CFD) provided the principal means for evaluating the circulation and effectiveness of coolants used in dual mechanical seals. Virtual prototype tests were carried out using FLUENT, a general-purpose fluid flow solver. Laboratory measurements were also made to confirm the CFD results.

The simulations of flow behavior in seals were examined using IBM Visualization Data Explorer. Visual programs developed within the DX environment were used to display and extract important design information from large sets of three-dimensional multivariate data.

A particularly interesting and revealing aspect of the analysis involved flythrough animation sequences created from images depicting fluid particle trajectories. From an immersed, moving frame of reference the observer travels through the flow alongside data-mapped streamribbons. This technique has proven useful for identifying causal relationships between fluid motion and local flow variables such as temperature, static pressure, turbulent kinetic energy, and vorticity.

Conclusions drawn from the project suggest simple and cost-effective ways to enhance removal of heat, while improving the thermal environment, operation, and life expectancy of seals.

Introduction

The design of fluid sealing devices involves a wide range of engineering considerations. Seals mounted to rotating shafts of pumps and mixers, for example, must often operate under severe and sometimes dangerous conditions such as those involving hazardous or toxic fluids. Concerns related to the design and operation of these seals include the thermoelastic behavior of seal faces, the tribological nature of lubricating interfacial fluid films, as well as the mechanics and thermodynamics of fluids within which seals must immersively function. It is the latter of these concerns which forms the basis for the work reported here.

For difficult sealing applications which require zero (or near-zero) emission of hazardous fluids, double (or dual) mechanical seals are often used in conjunction with some type of benign barrier fluid to form a safer, more reliable containment system. These systems typically rely on forced convection cooling by the barrier fluid to help dissipate frictional heat generated at sliding interfaces between rotating and non-rotating components. In fact, removal of heat from these components is often vital to the sustained functionality and life of the seals.

Figure 1 shows a typical configuration in which a mechanical seal is used to prevent leakage of process fluid from a centrifugal pump. Various parts of the seal are illustrated

Figure 1. Cutaway view of centrifugal pump/mechanical seal configuration.

in this cutaway cross-sectional view. Figure 2 provides a closer, more detailed picture of the seal rings or faces for this particular example. Here, the blue carbon-graphite faces rotate with the purple shaft sleeve. The silicon-carbide faces (red) are held stationary by the seal gland (green) which bolts directly to the gray mounting flange of the seal chamber (Figure 1). Also shown in Figure 2 is the translucent blue barrier fluid domain of interest. For this type of seal, the barrier fluid enters and leaves the domain via a flow distribution channel (yellow) situated between the two silicon-carbide faces.

Figure 2. Seal faces and flow channel shown with barrier fluid analysis domain.

In this study, ways were sought to improve the cooling function of barrier fluids. One effective means of enhancing the removal of heat from seals is to increase the axial circulation of fluid to warmer regions of the seal where sliding friction occurs, namely the sealing interfaces (Figure 2). It has been found that simple, reliable, and cost-effective designs can provide significant increases in forced convection cooling of mechanical seals, thereby improving their reliability and extending their anticipated life of service.

Method of Design Analysis

Although seal designs must ultimately be validated by extensive testing in the laboratory and in real world (field) applications, computer simulation is becoming an increasingly valuable tool for predicting design performance and guiding the prototype development process. For example, the thermomechaical behavior of seal faces can often be determined with considerable accuracy using specialized and general purpose numerical models. Two such models have found extensive use in our efforts to design new generations of seals. The first of these is a customized finite element code used to study the thermoelastic behavior of mechanical seal faces. This model computes heat generation at the sliding interface and the deformations produced by hydrostatic loads and thermal expansion. The model relies, however, on a number of inputs, one of which being the coefficient(s) of heat transfer representing the convective exchange of thermal energy between the seal faces and their surrounding fluid media.

In the analysis process, the coefficients are first estimated using empirical relationships developed from available experimental data. Using these estimates for the convective heat transfer, the seal face model then computes the frictional heating and distributions of temperature within the faces. The next step is to apply the computed surface temperatures of the faces as input boundary conditions to a commercial CFD code which then solves the governing equations of fluid motion and associated heat transfer. From the CFD analysis, the convection coefficients are then calculated for the specific problem of interest. These coefficients are then compared with those originally assumed, and, if necessary, the entire process is repeated until satisfactory agreement (within 10%) is achieved between the values used by the two models. After obtaining what is believed to be a reliable solution, the results of the analyses are selectively validated against actual physical measurements made in the laboratory.

Scope of Investigation

For the present study, a dual seal configuration was examined for a 48-mm diameter centrifugal pump shaft (Figure 1). The operating conditions were assumed to be 687 kPa, 66 C for the process (sealed) fluid, and 1,031 kPa, 38 C (inlet temperature) for the barrier fluid. Of particular concern were the effects of seal design and operating conditions on the efficiency of heat removal by barrier fluid circulation. Among the variables studied were radial clearance between stationary and rotating components, effects of tapered surfaces, effects of shaft rotational speed, effects of barrier fluid throughflow, and effects of fluid property variations.

The investigation centered around steady-state fluid flow analyses made using the finite volume CFD model FLUENT. Two turbulence model options available within the code were utilized in conducting the flow simulations - a two-equation model which assumes directional uniformity of the turbulence field (sufficient for most cases of interest), and a more sophisticated Reynolds Stress model suitable for strongly nonisotropic flows.

Examination and improved understanding of the CFD results were provided by Data Explorer. Use of this versatile and powerful visualization tool enabled the computed data to be studied in unique and enlightening ways.

Sample Results

Shown in Figure 3 is a typical example of a 2D (axisymmetric) finite element mesh used to analyze the thermoelastic behavior of seal faces. The non-rotating silicon-carbide face is shown in red, while the softer carbon-graphite face which rotates is shown in blue. The axially tapered inner radius of the stationary face (discussed later) is also apparent. The

Figure 3. Meshed representation of seal faces for thermoelastic analysis.

thermal results obtained from the analysis of these faces is shown in Figure 4. This result represents the inboard set of faces, i.e., those nearest the pump impeller (Figure 1), for the case of water as both process and barrier fluid, a shaft speed of 377 rad/sec, and a barrier fluid throughflow of 1.4 l/m. Not surprisingly, the warmest temperatures are predicted to occur near the sliding interface where frictional heat is generated. Up to 80% of this heat is conducted away from the interface through the silicon-carbide material , due, largely, to its much greater thermal conductivity compared with that of the carbon-graphite.

Figure 4. Computed FEA results for inboard seal faces nearest impeller.

Figure 5 shows a cutaway view of a cylindrical flow domain and structured finite-volume grid used to conduct 3D flow analyses for a tapered surface design (Figure 2). The dark blue axially centered region of the mesh represents the surface through which fluid enters the domain. The corresponding outlet surface (not shown) is likewise axially centered in the flow channel region, and displaced about 60 degrees circumferentially in the clockwise direction from the inlet.

Figure 5. Gridded flow domain used for typical CFD analysis of barrier fluid.

A typical set of boundary conditions used for the CFD analyses are depicted in Figures 6, 7, and 8. Figure 6 illustrates the rotating velocity boundaries (shown in yellow). These boundaries consist of the outer radial surface of the sleeve, the bounding surfaces defined by the carbon-graphite faces, and the thin fluid surfaces between the sleeve and the rotating faces (Figure 2). The stationary (non-rotating) boundaries, as well as the flow

Figure 6. Velocity boundary conditions used for barrier fluid flow analysis.

cross-sections, are shown in blue. Figure 7 shows the temperature boundary conditions used for the tapered surface design analyses. These temperatures represent average surface values obtained from the FEA model (Figure 4). Note that the boundary temperatures are higher for the outboard side of the domain (background). The adiabatic heat flux boundary conditions assumed for the stainless steel sleeve, the outer radial surface of the stainless

Figure 7. Temperature boundary conditions obtained from FEA model.

steel flow channel, the region of recirculation between the inlet and outlet ports, and the axial fluid ends of the domain are depicted in Figure 8. The assumption of negligible heat exchange across the stainless steel surfaces was invoked because of the order-of-magnitude lower value of thermal conductivity for stainless steel compared with that of the silicon carbide seal face material.

Figure 8. Thermally insulated boundaries (purple) assumed for CFD analyses.

The near-wall static pressures of the fluid computed for the above described case are illustrated in Figure 9. These pressures are relative to an arbitrary value of zero assumed for the (yellow) outlet surface of the flow channel. For this case the annular gap between the sleeve and the stationary hard face is about 2 mm. The conical pressure surfaces are displaced 127 microns from the rotating (foreground) and stationary (background) axially tapered boundaries (Figure 2). Due to the symmetry of the flow about the centerplane of the channel, it is possible to display only one axial end of the pressure field to obtain a complete representation of both inboard and outboard sides of the solution. The symmetry of the flow is caused by a weak coupling between the governing equations of fluid motion and thermal energy brought about by the small variations in the thermofluid properties of water over the temperature range of the problem. The predominately blue colored surface in the foreground represents the fluid pressure near the rotating sleeve. Contrasting this

Figure 9. Pressure surfaces near rotating sleeve (foreground) and seal face.

relatively lower-pressure surface is the predominately yellow higher-pressure surface near the stationary seal face. Aside from the obvious radial gradient of fluid pressure created by centrifugal forces within the flow, milder and more localized axial and circumferential gradients are also noticeable, particularly over the outer pressure surface adjacent to the non-rotating seal face boundary.

Figure 10 shows a similar view, this time of the velocity field within the same near-wall conical surfaces depicted in Figure 9. Here, the length of the flow vectors is proportional to the local magnitude of the fluid velocity. Not surprisingly, the vectors (colored by fluid speed for quantitative reference) align closely with the rotational direction of the sleeve, with both axial and radial gradients being clearly visible. Near the rotating wall the flow velocity increases dramatically in the axial direction from the region near the channel to

Figure 10. Flow velocity vectors near rotating sleeve and stationary seal face.

the region near the interface, closest to the viewer. The highest flow speeds shown here are about two-thirds of the corresponding local surface speed of the rotating sleeve. The flow at the larger radius near the stationary wall (background) decelerates sharply between the interface region and the near-channel region. As expected, the flow field demonstrates a strong radial dependence, being much greater near the rotating inner boundary of the domain.

Shown in Figure 11 is a magnified view of the same velocity vectors, looking radially inward just above the outlet of the domain. The vectors to the left of the outlet are near the rotating sleeve (smaller radius), while those on the right side are near the outboard stationary seal face. The significant point to note here is the clear leftward inclination of both sets of flow vectors, suggesting axial circulation of the fluid.

Figure 11. Radially-inward view of flow vectors near barrier fluid outlet.

The near-wall turbulent kinetic energy of the flow is shown in Figure 12. Here again the data in the foreground correspond to the fluid later near the rotating sleeve, while on the other side of the channel the data represent the fluid layer near the stationary seal face. Notice that the turbulence levels are highest near the regions of the domain where abrupt geometric changes in radial cross-section occur, namely near the channel and the sliding

Figure 12. Surfaces of turbulent kinetic energy near sleeve and seal face.

interfaces. This situation is advantageous for promoting heat transfer by way of increased mixing in the precise locations where heat exchange is most critical, i.e., near the warmer interface regions of the seal faces (Figure 4), and near the cooler fluid moving through the channel.

Figure 13 depicts a cross-sectional view of the secondary flow velocities for a conventional design having a narrow (1 mm) radial gap, with no axial tapers on any of the barrier fluid bounding surfaces. In this view, the in-plane (axial-radial) components of the flow at the bottom (6:00 o'clock) position midway between the inlet and outlet planes (Figure 10) are displayed. The Reynolds Number corresponding to this set of design/operating conditions is about 13,300, based on the radial gap, the surface speed of the rotating sleeve, and the kinematic viscosity of water at 38 C. The velocity vectors, as well as the wall boundaries,

Figure 13. Secondary flow velocity vectors for 1-mm untapered radial gap.

are shown colored by temperature. Note that the cooler fluid circulating in the channel does not communicate well with the warmer flow near the interface regions. For this case the rate of convective heat removal by the barrier fluid is less than 0.5 kW, based on the throughflow and the predicted rise in fluid temperature between the inlet and outlet surfaces of the flow domain.

If the width of the radial gap is doubled (Figure 14), thereby also doubling the Reynolds Number, we notice that the cooler fluid within the channel circulates more effectively in the axial direction. This intuitive result produces a more efficient axial exchange of heat, and a 56% increase in the net heat removed by the barrier fluid.

Figure 14. Secondary flow velocity vectors for 2-mm untapered radial gap.

Finally, model predictions for the tapered-surface design are shown in Figure 15. In this configuration both the rotating and stationary boundaries are radially inclined in the axial direction. As in the previous case, the radial gap is approximately 2 mm. The fluid circulation cells, now span the entire axial distances between the flow channel and the interface regions of the seal. This more efficient transfer of mass, made possible by the axial pumping action induced by the rotating tapered sleeve, produces an even greater

Figure 15. Secondary flow velocity vectors for 2-mm tapered radial gap.

increase in cooling efficiency (roughly 130% compared with that of the narrow-gap case,Figure 13). The results illustrated in Figure 15 correspond to those representing the same geometric configuration and operating conditions presented in Figures 9-12.

Continuing with the tapered surface design, Figure 16 shows a 3-dimensional 'snapshot' of temperature colored flow trajectories for two fluid particles (represented as spherical glyphs) released immediately downstream of the (magenta) inlet plane. In this view, the yellow glyphed particle travels along the cooler inboard side of the seal, while the red glyphed particle travels through the warmer outboard side. The trajectories are rendered as 2D streamribbons onto which any scalar variable (here local fluid temperature) can be mapped. The twisting nature of the ribbons is indicative of the local swirl (vorticity) of

Figure 16. Streamribbon trajectories of fluid particles released near flow inlet.

the flow, with regions of stronger vorticity corresponding to those of greater turbulence (Figure 12), mixing, and heat transfer. Figure 16 is actually a single frame image of a flow trajectory animation wherein the flow speed (m/s) of the red outboard particle is displayed in the lower left, and the elapsed time (ms) from release is shown in the upper left of the frame. For this example, the fluid particles complete their journey from the flow channel to their respective interfaces and back in approximately 100 ms. During this time the rotating shaft/sleeve completes about six revolutions.

Shown in Figure 17 is the first of four immersion-view images taken from a flythrough animation sequence which follows the trajectory of the red particle depicted above and in Figure 16. In this scene, the observer travels just to the left of the temperature-mapped outboard streamribbon slightly downstream of the flow channel inlet. The streamribbon

Figure 17. Scene showing streamribbons downstream of barrier fluid inlet.

trace representing the trajectory of the yellow inboard fluid particle is also visible. Below the streamribbons is the (adiabatic) sleeve which rotates away from the observer. Near the top of the scene are displays indicating the local speed (m/s) and temperature (C) of the red glyphed particle, as well as the elapsed time (ms) from release of the particles.

Figure 18. View of flow outlet with streamribbons leaving barrier fluid channel.

Figure 18 shows a frame taken from the same animation (below) at a later time (55 ms) into the trajectories. In this view, we see both streamribbons, induced by low pressure (Figure 9), bend radially inward toward the sleeve as they bypass the (red-colored) flow outlet, and begin their journey to the axial extremities of the domain. The particles, at this point, have picked up some speed (about 25%), and have increased in temperature by about 5 C.

In Figure 19, we see another frame later in the sequence showing a view near the outboard sealing interface. The streamribbon segment here represents a fluid particle temperature of 61 C, about 12 C warmer than that illustrated in the previous scene (Figure 18). The particle speed has also increased dramatically to a near maximum value of 6.1 m/s, as it flows along next to the rotating radial seal face surface on the extreme right. Also clearly visible is the radial gradient of fluid pressure mapped onto the heat conducting walls of the domain. The streamribbon segment visible on the left is part of the same flow path, one revolution earlier in the trajectory.

Figure 19. Streamribbon near the warmer outboard seal interface region.

The final immersion scene taken from the flythrough animation is shown in Figure 20. The red colored streamribbon indicates that near this location the fluid particle, after absorbing heat from the outboard sealing interface (visible to the right of the scene), reaches the maximum temperature of 62 C that it will attain along its flow trajectory through the domain. Note that the speed of the fluid particle has decreased about 20% from that of the previous scene (Figure 19) as it moves along the outboard stationary

Figure 20. Streamribbon trajectory of returning outboard fluid particle.

seal face boundary. Segments of the same trajectory, corresponding to earlier times (and temperatures) along the path of the fluid particle, are seen on both sides (axial ends) of the view.

Figure 21 shows a 3D representation of the fluid temperature within the flow channel region, again for the tapered surface design. The temperature rise from the inlet to the outlet of the domain is predicted to be about 11 C. As noted above, these rises in fluid temperature are used to estimate the heat removal rates and thermal efficiencies of the various design/operational scenarios.

Figure 21. Barrier fluid temperature in region of flow distribution channel.

In order to verify the analysis of the CFD flow simulation model, laboratory tests were conducted replicating exact design configurations and conditions of operation used to compute selected case results. The data shown in Figure 22 correspond to the tapered surface design prediction (Figure 21). As can be seen, the measured difference in barrier fluid temperature between the inlet and outlet was about 10 C (within 1 C, or 10% of the calculated value) for this 4-hour test.

Figure 22. Laboratory data validating tapered-surface CFD results (Figure 21.)

Shown in Figures 23-25 are the computed heat removal effects of shaft (rotational) speed, barrier fluid throughflow, and thermofluid properties (as reflected by Prandtl Number), respectively. To check the effect of shaft speed, a water throughflow rate of 1.4 l/m was assumed. Generally speaking, the greater the shaft speed, the higher the Reynolds Number and level of turbulence, effects leading to improved heat removal efficiency, as illustrated

Figure 23. Barrier fluid cooling efficiency versus shaft rotational speed.

by Figure 23. In Figure 24 we see a similar trend with respect to throughflow, again for water and a shaft speed of 183 rad/s (1750 rpm). Finally, Figure 25 indicates a dramatic loss of cooling efficiency with increasing Prandtl Number, Pr, of the barrier fluid. The Prandtl Number is a dimensionless, temperature-dependent fluid property/parameter

Figure 24. Barrier fluid cooling efficiency versus rate of throughflow.

defined as the product of the specific heat and thermal conductivity of the fluid divided by the fluid viscosity. (It can also be physically interpreted as the ratio of momentum diffusivity to thermal diffusivity of the fluid.) Three commonly used barrier fluids - water, a 50/50 weight-percent mixture of Ethylene Glycol and water, and a commonly

Figure 25. Barrier fluid cooling efficiency versus Prandtl Number.

used synthetic oil - were all evaluated for an inlet fluid temperature of 38 C, and a shaft rotational speed of 377 rad/s (3600 rpm).

Figure 26 shows the axial flow circulation pattern computed for the case of synthetic oil having a viscosity of about forty times that of water at 38 C. As clearly seen, the reduced communication between the cooler fluid in the flow channel and the warmer fluid near

Figure 26. Effect of increased fluid viscosity on flow circulation/heat removal.

the interfaces (even for the tapered surface design), combined with the relatively poor thermal properties of the oil, result in a sharp (84%) decrease in heat removal, relative to the case for water (Figure 15).

Summary and Conclusions

The thermofluid design of dual mechanical seals used to prevent leakage from rotating shafts in industrial fluid-handling equipment was investigated. The purpose of the study was to examine effects of various design and operational parameters on convective removal of friction-generated heat within the seal itself. Using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD), confirmed by laboratory testing, the performance of virtual prototypes was examined to evaluate the effectiveness and thermal efficiency of barrier fluid flows.

As anticipated, the results show that axial circulation of fluid to and from warmer regions within the seals promotes heat removal. Design features favoring axial circulation include larger radial gaps between rotating and stationary components, as well as axially-tapered surfaces which act to propel cooler fluid toward the heat-producing interfaces of the seal. Other conditions found to improve the cooling performance of barrier fluids are increased speed of shaft rotation, larger rates of barrier fluid throughflow, and fluids having lower viscosities such as water and Ethylene-Glycol/water mixtures.

The findings revealed by this study have helped guide the design of cooler-operating, longer-lasting dual mechanical seals. Much of the credit for the success of the project is attributed to the versatile and novel ways in which the computed CFD data could be visualized and more clearly understood using the unique capabilities of Data Explorer.

Acknowledgements

The authors would like to express their thanks to the following individuals whose efforts helped make this work possible: Kevin McArthur, Paul Philippon, Bo Ruan, Shifeng Wu, and John Yurka, A. W. Chesterton Co.; Liz Marshall, Fluent Inc.; Greg Abram, Rob Look, Holly Rushmeier, Rich Sefecka, and Lloyd Treinish IBM Visualization Data Explorer; Chris Doehlert; and Dan Freund and Mark Smith, Silicon Graphics.