1 Simulation and Validation of Turbulent Pipe Flows 57:020 Mechanics of Fluids and Transport Processes CFD LAB 1 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University of Iowa C. Maxwell Stanley Hydraulics Laboratory Iowa City, IA 52242-1585 1. Purpose The Purpose of CFD Lab 1 is to teach students how to use the CFD Educational Interface (FlowLab 1.2), practice more options in each step of CFD Process, and relate simulation results to EFD and AFD concepts. Students will simulate turbulent pipe flow following the “CFD process” by an interactive step-by-step approach. The flow conditions will be the same as they used in EFD Lab2. Students will have “hands-on” experiences using FlowLab to compute axial velocity profile, centerline velocity, centerline pressure and friction factor. Students will compare simulation results with their own EFD data, analyze the differences and possible numerical/experimental errors, and present results in CFD Lab report. Flow chart for ISTUE teaching module for pipe flow (red color illustrates the options you will use in CFD Lab 1) Coarse Medium Fine Automatic Manual Structured Unstruct-ured Geometry Physics Mesh Total pressure drop Post-processing Wall friction force Centerline Velocity Centerline Pressure Profiles of Axial Velocity Contours Vectors Streamlines Pipe Pipe Radius Pipe Length XY plot Validation Verification Boundary Conditions Flow Properties Viscous Models One Eq. Two Eq. Density and viscosity Laminar Turbulent Inviscid SA k-e k-w Heat Transfer? Incompress-ible? Initial Conditions Solve Iterations/ Steps Converge-nt Limit Precisions Single Double Numerical Schemes 1st order upwind 2nd order upwind Quick Steady/ Unsteady? Report Residual2 2. Simulation Design In EFD Lab 2, you have conducted experimental study for turbulent pipe flow. The data you have measured include centerline pressure distribution and fully developed axial velocity profile. These data will be used in this Lab for comparisons with CFD predictions. The problem to be solved is that of turbulent flows through a circular pipe. Reynolds number based on pipe diameter and inlet velocity should be computed from your own EFD data and is much higher than the Reynolds number used in CFD Prelab1. The problem formulation is similar to that in CFD PreLab1 and will not be repeated here. The Reynolds number is much higher and students need specify turbulence model, and thus more variables need to be specified in boundary conditions, as will be discussed in details later. 3. CFD Process Step 1: (Geometry) 1. Radius of pipe (pipe radius in your EFD Lab2, use 0.02619 m if not available) 2. Length of pipe (6.096m) NOTE: The actual length of the pipe is 30 feet (9.144m), However, in CFD simulation, we need specify “outlet pressure”, and we don’t have pressure transducer at the pipe outlet. So we choose the outlet of the pipe we will simulate to be the location of the last pressure transducer, that is 6.096 meters from the pipe inlet. Click <<Create>>, after you see the pipe geometry created, click <<Next>>. Outlet Inlet Symmetry Axis Pipe Wall3 Step 2: (Physics) 1. With or without Heat Transfer? Since we are dealing only with the flow and not with the thermal aspects of the flow like heat transfer etc, switch the <<Heat Transfer >> button off, which is the default setup. 2. Incompressible or compressible Choose “Incompressible”, which is the default setup. 3. Flow Properties use the flow property values in your EFD Lab2. If you only know the room temperature when you conducted EFD Lab2, you can use the following website to easily get the corresponding density and dynamic viscosity for air: Hhttp://www.mhtl.uwaterloo.ca/old/onlinetools/airprop/airprop.html If the room temperature is 24°, the density and viscosity are the values shown in the above panel. H NOTE: viscosity used in FlowLab is the dynamic viscosity (kg m s), NOT kinematic viscosity (2ms)4 4. Viscous Model In CFD Lab 1, two equation k-epsilon (k-e) model will be applied. 5. Boundary Conditions At “Inlet”, we use zero gradient for pressure and default values for turbulent intensity and length scale. You must calculate the inlet velocity u, which is uniform, based on the flow rateQ(m3/s) you computed in EFD Lab2, and cross section area of the pipe 24D, i.e. 24u Q D. Since inlet flow is parallel to the x axis, magnitude of v velocity is 0. Use default values for turbulence quantities and click <<OK>>. At “Axis”, FlowLab uses zero gradient for axial velocity and Pressure and specify the magnitude for radial velocity to be zero. Read all the values and click <<OK>> At “Outlet”, FlowLab uses magnitude for pressure and zero gradients for axial and radial velocities. You need transform the four pressure tap pressure values from “feet water” to “Pascal” and input pressure tap #4 value as the “outlet pressure”. For example, if the pressure tap #4 has value of 0.2502 feet water, you need input 747 Pascal.5 At “Wall”, no-slip boundary conditions are fixed for both axial and radial velocity, gradient for pressure is zero. Input the pipe roughness of the pipe you used in EFD Lab2 and choose the convenient unit you need. For example, user inputs 0.025 mm for smooth pipe. 6. Initial Conditions Use the outlet pressure for P (Pa), inlet velocity for u (m/s) and default values for turbulent quantities. After specifying all the above parameters, click <<Compute>> button and FlowLab will automatically calculate the Reynolds number based on the inlet velocity and pipe diameter you input. Click the <<Next>>, this takes you to the next step, “Mesh”. Step 3: (Mesh)6 For CFD Lab 1, “Structured” meshes will be generated using “Automatic fine” option. Click <<Create>>, FlowLab will automatically create the Fine mesh and display the grid intervals NR, NX. Step 4: (Solve) The flow is steady, so turn on the “Steady” option. Specify the iteration number and convergence limit using different values, as shown above. Use 10, 20, 40, 60, 100 for radial profile x/D positions and choose “Double precision” with “2nd order scheme”. Use “New” calculation for this Lab. Then