### Type to search # SOLIDWORKS Flow Simulation—Turbomachinery SOLIDWORKS Flow Simulation can evaluate the fluid flow for various engineering applications and can facilitate thermal analysis for solving various heat transfer problems. While the software is capable of analyzing a variety of solid bodies and fluid configurations, the solutions are typically characterized by flow in or around stationary solid bodies.

However, there is another feature of the Flow Simulation toolset that can assist in evaluating fluids interacting with mechanisms in motion, useful for assessing the design and performance of turbomachinery. This involves specifying rotation of the fluid and solid bodies within the computational domain. This article looks at applying these concepts to a pump design.

### Pump Model

Consider the pump shown in Figure 1. The motor rotates the impeller at high speed, creating a vacuum to generate suction at the inlet. Pumps and most turbomachinery operate by converting power in the form of an electric motor (P2 in the diagram below) to fluid power in the form of pressure and flow. Figure 1 . Typical pump diagram.

The operating parameters we will simulate are as follows:

 Flow rate 0.3 m3/s Outlet pressure Ambient Pump rpm 2,000 rpm (209.5 radians/second) Inlet pressure To be calculated from the analysis

A SOLIDWORKS solid model representation of the pump internals is shown in Figure 2 below. Figure 2. Pump solid model.

A key parameter in simulating turbomachinery is identifying the rotating components in the model and using boundary conditions to specify stationary components. As with many Flow Simulation problems, the Wizard option gives a good starting point for setting all the major options. The Wizard starts with the dialog box in Figure 3. Here we name the project and add any comments. Figure 3. Wizard start dialog box.

The next dialog box is for specifying units. For this example, we will perform the analysis using SI units.

Figure 4 is the first dialog box that allows us to indicate that some of the components in the solid model will be rotating during operation. We activate the Rotation feature and select “Global rotating” from the dropdown. Figure 4. Specifying rotation.

We set the angular velocity to 2,000 rpm (209.5 radians/second) about the Z-axis. Since we have set a global rotation, all components are considered rotating with the specified angular velocity. We will specify the stationary components later in the analysis setup.

The fluid that we are pumping is air, and we add it to the Project Fluids definition as shown in Figure 5. Figure 5. Adding air to the project.

All other dialog options in the Wizard can be left at the default.

To ensure the geometry is modeled correctly for the Flow Simulation to continue, a model check is performed (Tools → Flow Simulation → Tools → Check Geometry). With the Show Fluid option of the geometry check activated, we get the display as shown in Figure 6. The air can be seen contouring the blades of the impeller. Figure 6. Air volume.

### Boundary Conditions

The pump will be required to produce a flow of 0.3 m3/s. We will define this boundary condition at the inlet lid face of the model as shown in Figure 7. Figure 7. Specifying inlet flow.

The outlet is defined on the outlet lid surface as shown in Figure 8 by setting the Environment Pressure to ambient (10,325 kPa) on this surface. Figure 8. Specifying the outlet conditions.

The final boundary condition is the most critical. Recall that we specified a global rotation of 2,000 rpm in the model setup. This will, by default, impart a rotation on all of the fluid and solid components. We need to make the pump housing stationary to mimic the actual operation of the equipment. From the boundary condition dialog box (Tools → Flow Simulation → Insert → Boundary Condition), we select the pump casing as the stationary item (see Figure 9). Figure 9. Fixing the nonmoving components.

We are now ready to solve the model by selecting Tools → Flow Simulation → Solve → Run from the menu.

### Post-Processing

The function of a pump is to drive a given flow from a lower pressure to a higher pressure using energy from an attached motor. The pump in our example uses a motor to drive the impeller (Figure 1), which pulls suction on the inlet (Ps). We will evaluate the pressure drop by querying surface results at the inlet and outlet surfaces. Figure 10. Flow Simulation menu tree.

Right-clicking the Surface Parameters in Figure 10 brings up the dialog box in Figure 11. We are interested in the inlet pressure since that will give the amount of vacuum the pump must draw to move the specified 0.3 m3/s of air. Figure 11. Getting inlet pressure results.

To calculate the inlet pressure, the inner surface of the inlet lid is selected as the reference geometry, and we select “Pressure” as the required quantity. The average pressure over that face is 100.4 kPa, as shown in Figure 12. This is a vacuum relative to the specified 101.3-kPa ambient pressure. Figure 12. Inlet pressure results.

The power input from the motor required to pump that amount of air is determined by the following calculation:
Power (Watt) = Torque(N-m) × Angular Velocity (radians/second)

The torque on the impeller is determined by again bringing up a Surface Parameters dialog box similar to Figure 11. However, in this case, we select all the faces of the impeller for the Selection box and select “Torque” for the parameter to display (Figure 13). Figure 13. Getting impeller torque.

The results are shown in Figure 14. Figure 14. Impeller torque.

Plugging the results into the previous formula relating power to torque and rpm, we have:

Power = 1.507 (N-m) * 209.5 radians/second = 315.7 Watts

Another useful insight to the design of a pump impeller is the efficiency. As shown in Figure 14, Flow Simulation can extract the contribution to the torque requirements between the normal and friction force on the blades. Modifying the blade profile will affect the ratio of the components to the overall torque. This will impact the pump efficiency, which is defined as the power output to the air stream relative to the power input by the pump motor to the impeller. The power in the pressurized air stream is the pressure rise multiplied by flow:

Air Power = Pressure Rise × Flow = (101,325–100,424) Pa × 0.3 m³/s = 270.3 Watts

The pump efficiency is defined as the air power divided by the power delivered to the impeller. The overall efficiency of the pump in our simulation is then 270.3/315.7 = 85.6 percent.

### Visualizing Results

The airflow pattern within the impeller can be visualized by selecting “Flow Trajectories” from the Results menu. This brings up the dialog box in Figure 15. Figure 15. Defining flow trajectories.

Selecting the outer lid as the reference surface and specifying velocity for the parameter to plot, we get the flow trajectories from the pump inlet through the impeller as shown in Figure 16. Figure 16. Flow trajectory plot.

### Parametric Analysis

The previous Flow Simulation was modeled by specifying a global rotation in the settings and then selecting the stationary surfaces (stators) by applying the appropriate boundary conditions. This makes determining the effect of increasing the rotational speed on the pump performance very easy. We will increase this global rpm by 50 percent from 2,000 to 3,000 (314 radians/second) and rerun the analysis.

The simulation with these parameters gives the following results:

Impeller Torque = 2.88 N-m

Power = 2.88 (N-m) * 314 radians/second = 904.3 Watts

Pressure Rise = 101,325–99,124 Pa = 2201 Pa

Air Power = Pressure Rise × Flow = 2201 Pa × 0.3 m³/s = 660.3 Watts

The efficiency in this case is 660/904 (73 percent) compared to the previously calculated 85.6 percent for the 2,000-rpm base case.

### Conclusion

SOLIDWORKS Flow Simulation can assist in the design and analysis of various types of turbomachinery (fans, pumps and turbines). In this article, we analyzed an air pump and set up boundary conditions to simulate a specified airflow rate and determine the power required to achieve that performance. Overall pump efficiency was determined by calculating the delivered power to the impeller versus the power in the outlet air stream.