| Rev # | Date | Description |
|---|---|---|
| 1.0 | August 2020 | Document created |
| 1.1 | August 2023 | Document verified for current release 2023 SP2.0 |
Note
All SolidPractices are written as guidelines. It is a strong recommendation to use these documents only after properly evaluating your requirements. Distribution of this document is limited to Dassault Systèmes SolidWorks employees, VARs, and customers that are on active subscription. You may not post this document on blogs or any internal or external forums without prior written authorization from Dassault Systèmes SolidWorks Corporation.
This document was updated using version SOLIDWORKS 2023 SP02. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.
Preface
This SolidPractice document provides best practices for using the SOLIDWORKS Flow Simulation software to simulate a centrifugal pump. The centrifugal pump uses a rotating impeller to increase the pressure of the fluid to move it through a piping system. The fluid enters the pump impeller near the rotation axis and is accelerated by the impeller blades. The fluid then flows radially outward into the volute chamber, from where it exits into the piping system downstream. It is possible to model this centrifugal pump using the local Rotating Region option, discussed later in this document.
We would like to hear your feedback and suggestions for new topics. After reviewing this document, please take a few minutes to fill out a brief survey. Your feedback will help us create the content that directly addresses your challenges.
Introduction to Pumps
Definition
A pump is a device that can add hydraulic energy to a flowing fluid. Pumps are used in our modern world in many contexts that include:
Propulsion systems for aircraft, motor vehicles, ships, and liquid fuel rockets
Power-generating plants
Gas, oil, and water-pumping stations
Numerous other industries and products ranging from heart-assist pumps to refrigeration facilities
The flow through a pump is three-dimensional, viscous, and unsteady. Consequently, accurate analysis of pump performance is predictable only when using CFD in general, and SOLIDWORKS Flow Simulation in particular. The purpose of this SolidPractice is to provide good practices and recommendations to carry out such an analysis.
In reference to the following image, most commonly used pumps have a rotating impeller (arrow #1). That is, several blades attached to a hub mounted on a shaft (arrow #2), and enclosed within a permanent housing, called volute (housing or shroud, arrow #3). The volute is stationary and is modeled later on as a stator. The inlet and outlet pipes are shown respectively with arrow #4 and arrow #5.
While most impeller pumps have backward-curving blades as depicted in the following left-side image, this is not a universal feature. This is because radial (non-curving) and forward-curving blades (shown in the following right-side image) are also used.
Introduction to rotating frame of reference techniques
When studying flows around moving bodies, you can often reduce the complexity of the analysis by using a moving coordinate system, where the body is fixed. In fact, the unsteady moving grid techniques (where the mesh is rotating), which are physically the most correct computational models, are expensive to use. Therefore, these techniques are not suitable for the majority of engineering computations. For example, the air (or the floor) around a car in a wind tunnel is moving, whereas the car is steady. When the coordinate system moves, the analysis is simpler because only three extra terms appear in the conservation equations because of the angular and linear velocity vector describing the motion of the coordinate system. All these extra terms vanish when the body is moving linearly with a constant velocity. In that case, the equations are the same for both a fixed and a moving coordinate system. Using a moving coordinate system is also referenced in open literature as a moving frame of reference (MFR).
Similarly, when modeling the impeller rotation, the rotating frame of reference technique (RFR) is a cost effective alternative. This approach is suitable for performing steady-state simulations as well as transient simulations. In SOLIDWORKS Flow Simulation, you can apply the RFR region-wise. In other words, one or several regions can be rotating while the rest of the domain is not rotating.
Rotating region
Within this rotating frame of reference approach, the region in the vicinity of the impeller is solved by using a rotating frame of reference. The rest of the computational domain is solved in a stationary frame of reference. This region where the rotating frame of reference is applied is called the rotating region (RR). The stationary frame of reference solves for the absolute velocity V, which is coupled with the relative frame velocity U at the interface between the rotating and stationary domain as: U=V- Ω *R, where Ω is a constant angular velocity, and R is the location vector. For more information, see the SOLIDWORKS Knowledge Base (KB) solution
QA00000117164: “How is the circumferential velocity shown relative to the coordinate system?”
The following image shows a typical rotating region (in transparent yellow) around the impeller (in red):
Before Performing a Simulation: Simplify!
Before running a simulation, simplify your model and prepare the geometry. An old adage applies: “Simplify or Suffer”.
Thin Gaps
You can usually remove any thin gap, shaft, motor, filter, etc. In addition, you must strip down the CAD model by removing any screws, or other tiny features that the pump does not require. Some of the most significant complicating effects is the leakage. The Check Geometry Tool (Tools > Flow Simulation > Tools > Check Geometry”) is a valuable utility to verify the fluid domain. After generating the fluid domain, you can use the section view to examine it. This can save you time later.
option, however the best practice is to close them in the CAD geometry.
Cavities
Cavities create a slow flow as shown in the following image. It is best to remove cavities. The coexistence of fast and slow fluid regions cause slow solver convergence. Besides of this, solving for the swirling flow inside the cavity increases the simulation time.
Extending the Outlet Pipe
Make sure to extend the outlet pipe so that the flow develops before reaching the outlet. In some instances, you also need to add a short inlet pipe.
You need to draw the rotating region (RR) in the SOLIDWORKS application. The RR captures the rotation of the impeller, and the fluid that is in close proximity to the impeller. In a sketch, you can draw the rotating region outline and then use a revolve operation. When doing so, follow these guidelines:
Ensure that the RR envelops (and not just touches) the impeller and a small amount of fluid.
Ensure that the RR is axisymmetric and concentric with the impeller (same axes).
Make sure that the RR is not tangent to the entire impeller body. If the RR is tangent in some location, as shown by arrow #1 in the next image, it can lead to a Solver Abnormal Termination error at iteration 0, or SOLIDWORKS Flow Simulation fails to generate the mesh. In that case, redraw the RR and try again. A common error that users make when including the rotating region in an assembly, is to use a coincident mate between the top surface of the impeller and the top surface of the rotating region. As a best practice, use an offset distance instead of a coincident mate.
When using a schematic in an ideal situation, the RR boundary is half way between the impeller and the stator (volute wall), as shown in the next image.
Here, the clearance between the impeller and the casing is exaggerated. In practice, the clearance is actually very small. If the volute wall is too far, then make the RR boundary a little larger than the impeller outside boundary. If the volute wall is too close, you can expand the RR boundary inside the stator, as shown in the following image.
By placing the RR boundary within a solid instead of placing it into a narrow gap between the impeller and the stator, you can avoid the additional mesh refinement.
A simple trick is to extend the gap. You can make the gap a little bigger, which can be a good exercise to become familiar with the pump simulation. In most cases, the gap between the rotor and the bottom wall is narrow, as shown in the next image at the left. By enlarging that gap a little as shown in the image at the right, you can place the boundary of the RR halfway between the impeller and the stator. This reduces the mesh requirement and therefore reduces the simulation time. In addition, this does not affect too much of the pump’s efficiency curve. Therefore, it is a good starting point.
In summary, the RR should envelop (and not just touch) the impeller and a small amount of fluid. If the gap between the impeller and the stator is tiny, you can, as an exercise, make the gap a little bigger so that you can place the RR boundary halfway between the impeller and the stator. This does not increase the simulation time too much, and provides a rough estimate of the performance curve.
The rotating region must embed the impeller geometry. However, the selection of the outer diameter and the shape of this region is left to the skill of the user. Because the flow field, and especially viscous stresses, in the vicinity of the blades is of primary importance, the width and height of the rotating region can influence the quality of the computational results. Therefore, the user must quantify this influence later on to gain insight into the influence of the rotating region dimensions on the accuracy of computed flow field and on the pump performance.
Finally, make sure that the sign of the angular velocity Ω you specify is as expected. Simply right-click the rotating region in the project tree, and then click Show. The rotating direction appears with a curved arrow. Throughout the flow simulation analysis, the RR rotates about its axis at the specified angular velocity Ω. All of the solids inside the RR also rotate at the same speed. If some solids are stationary, then consider applying a stator wall boundary condition on that component. You can also apply a counter-rotating wall in the rotating frame of reference so that it is stationary in the absolute frame of reference.
For more recommendations, review the following solutions in the SOLIDWORKS KB:
QA00000109913: What are some general tips, suggestions, and recommendations for using the ‘Rotating Region’ option in SOLIDWORKS® Flow Simulation?
QA00000105150: What are the best practices for Rotating regions in SOLIDWORKS® Flow Simulation?
QA00000109534: Are there in SOLIDWORKS® Flow Simulation any general recommendations for setting up a rotating region problem?
QA00000116611: I have a bracket that is very close to the rotating member of a fan blade, the manual says that if there are parts very close to the rotating region, it might lead to errors. Why?
Meshing
It is a best practice to have at least 3 cells between the impeller and the RR boundary, as shown in the next image:
How do I check the quality of the mesh in a ‘Rotating Region’?
Pump Performance Measurement
Definition of the Efficiency
The rate at which the blades of the impeller do work on the fluid for a pump is known as the hydraulic power; W_h=(𝑃_𝑜𝑢𝑡𝑙𝑒𝑡−𝑃_𝑖𝑛𝑙𝑒𝑡)∙𝑄. The power required to drive a pump is known as the mechanical power; W_m= Ω∙T.
In these formulas:
P_inlet is the static pressure surface goal at the inlet of the pump (Pa)
P_outlet is the bulk-average static pressure surface goal at the outlet of the pump (Pa)
Q is the volume flow rate (m^3/s)
Ω is the impeller rotation angular velocity (rad/s)
T is the impeller torque (N·m)
These quantities can be defined as surface goals. When defining the torque goal, pay close attention to the correct selection of faces and the orientation axis of the torque. You can calculate the pump efficiency (𝜂) in the following way (F.M.White "Fluid Mechanics," 3rd edition, 1994):
𝜂 = W_h/W_m=(𝑃_𝑜𝑢𝑡𝑙𝑒𝑡−𝑃_𝑖𝑛𝑙𝑒𝑡)∙𝑄/(Ω∙T)
The efficiency has no dimension and it is between 0 and 1 (0<𝜂<1) because the hydraulic power is less than the mechanical power. A pump absorbs more mechanical power than it delivers in the form of hydraulic power. This efficiency can also be defined as a percentage. In this case, the units must use the International System of Units (SI) standard. The goal of a pump designer is to achieve as large a value of the efficiency over a wide range of volume flow rate as possible.
To learn how to define these goals, see the KB solution
QA00000120687: In SOLIDWORKS® Flow Simulation, how do I calculate the efficiency of a turbine?
Boundary Conditions
A recommendation is to use the Mass Flow Rate at the inlet, and apply environment pressure at the outlet. The solver calculates the pressure gradient between the inlet and the outlet. Remember that for incompressible fluid, the pressure value has only a mathematical meaning. The pressure gradient, which is responsible for driving the fluid, has a physical meaning. The pressure difference between the inlet and the outlet can be also measured in term of water height column, called pressure head (supplied by the pump):
Pressure head= (P_outlet-P_inlet)/(density*gravity)
This measurement is in meters, where density is the mass density, in kg/m^3, of the water or any other fluid used for reference.
Performance Curve of the Pump
The pump performance curve or efficiency curve is generated for a fixed angular velocity by changing the mass flow at the inlet. The recommendation is to use mass flow or volume flow rate at the inlet, and keep the environment pressure at the outlet. The solver calculates the pressure head. The following graph depicts a typical performance curve for a pump. The three curves shown are the dimensionless efficiency, the head in feet, and mechanical power, in horsepower.
, and can occur whenever the head increases with Q. While this causes irregular operation for a liquid pump, it can lead to catastrophic failure of a gas compressor in a jet engine.
The mechanical power W_m increases slowly with Q, and for flow rate beyond Q_max, the flow becomes unstable and the simulation is again unstable. A key design objective is to minimize the range of flow rates over which unstable conditions occur.
Finally, as the flow rate increases from zero, the efficiency increases to a peak value at the design flow rate Q*, in this graph, around Q*=10gpm. At higher flow rates, the efficiency drops off. The point at which the efficiency achieves the maximum value is known as the best-efficiency point (BEP). You can calculate the pump performance curve by using a parametric study “What If Analysis”. The recommendation for this study is as follows:
Specify a flow rate range within the BEP and compute the efficiency for each value.
Gradually increase the values of Q within that range. Apply the Use Previous Results option for each value.
Keep in mind that a single mesh and the simulation settings might not be suitable for all of the values of Q.
You can stop the simulation can be stopped when the efficiency goal has converged, as shown in the next graph.
Some of the most significant complicating effects on the accuracy of the calculation of the performance curve of the pump are mismatch, circulation loss, and friction losses. Mismatch pertains to the relation between the inlet flow and the blade passages. Ideally, the flow enters normal to the impeller and tangent to the blades. When these conditions are not met, the simulation overestimates the performance curve. Similarly, circulation loss occurs when the flow does not exit tangent to the blades. This can be caused by separation or stall, a condition where the flow actually reverses direction near the blade trailing edge. This condition reduces the increase in pressure achieved by the pump. Make sure that the geometry of the blades is similar to the experiments and that the flow simulation results were converged. The friction losses are losses caused by the bearings supporting the impeller or its shaft.
Finally, if you want to obtain the performance curve of the pump for a different value of the angular velocity of the impeller, you need to revise the simulation for a couple of points, but at new volume flow rates given by the formula:
New Flow Rate=New (Ω)*Old Flow Rate/Old(Ω)
This formula is part of the affinity laws for the pump, which relate to the change of one parameter (angular velocity, impeller diameter, etc.) to the corresponding change in a flow parameter (flow rate, pressure head, mechanical power W_m, etc…). These affinity laws are widely available online.
For more information, review the following solutions in the SOLIDWORKS KB:
QA00000117066: How do I troubleshoot difficulties in getting a converged result using a local rotating region (averaging) with a low volume flow rate in a centrifugal fan study?
QA00000116612: It is difficult to make the air flow normal to the surface of rotating member. So how will this inability affect the results?
QA00000124428: If I do not receive the flow simulation results that I expect for a water pump, what first steps do I take to begin troubleshooting?
About Cavitation
For pumps using liquids, cavitation can occur in low-pressure regions of the flow. Cavitation is local boiling that occurs when the pressure is equal to the vapor pressure of the fluid, pv. For an example, see “What should I now about taking cavitation into account in SOLIDWORKS® Flow Simulation?”. The bubbles that form present two primary problems for the pump. First, mixing the bubbles with the main flow causes losses in total pressure and a decrease in efficiency. Second, pressure waves emanating from collapsed bubbles can cause noise and vibration, and damage the pump.
To avoid cavitation, the cavitation number must be positive everywhere. The cavitation number is defined by Nc=(p-pv)/(1/2*rho*v^2), where p is the static pressure, pv is the cavitation pressure, rho is fluid density and v is the flow velocity relative to the impeller. Other parameters might also be useful. For example, the net positive suction head (NPSH) parameter used by pump manufacturers. For information about this parameter, see the KB solution
QA00000112613: I am dealing with centrifugal pumps is it possible to create a NPSH (Net Positive Suction Head) plot for a pump?
When you see a warning about negative pressure in the solver window, it does not necessarily mean that cavitation will occur. However, it might be because of a coarse mesh or a nonconverged solution. For related information, see the following solutions in the SOLIDWORKS KB:
QA00000122722: In SOLIDWORKS® Flow Simulation, why do I see a "negative pressure" warning?
QA00000118054: Which cavitation model is recommended for a water pump design using the rotating region option?
About the Solvers (Averaging vs. Sliding)
The steady-state averaging method makes it possible to perform a steady-state computation by performing circumferential averaging of the flow variables at the interface of the rotating region (this interface is also called the sliding interface). On the other hand, the sliding transient capability resolves the true transient interaction of the stator/rotor for maximum accuracy. You can apply this method to individual pairs of blade passages, or to the entire 360 degree machine. It is a recommendation to use this method instead of the steady averaging method, especially when the interaction of the stator/rotor is important, and where the flow is far from being axisymmetric. This is true in the case of centrifugal pumps, and the sliding transient method delivers greater transient accuracy than the transient averaging method. In all of these methods, the solver accommodates the frame change across the sliding interface automatically when computing the flow field in the different regions of the simulation.
Effect of the Rotating Region on the Performance Curve
The rotating region (RR) must embed the impeller geometry, however, the selection of the outer diameter of this region is left to the skill of the user. In open literature, there are only a few works on this topic. To evaluate the effect of a different size of RR, you could conduct a parametric study where the parameters are the dimensions of the RR.
Conclusion
Simulating a centrifugal pump is a complex analysis, which requires time and attention. However, it does not have to be difficult if you follow the recommendations in this document.
about the topics that you want us to cover in the next revision of this document. Click here for a complete list of SolidPractices documents available from DS SOLIDWORKS Corp.
