Picked from the software, topic, and level of “Class ANSYS Fluent: ANSYS Fluent Tutorial: CFD Simulation of Shell & Tube Heat Exchanger from Geometry to Contour”.
At most one email a week. Unfollow anytime with one click.
Transcript
The full narration of this video. The current sentence is highlighted while the video plays; click any sentence to jump there.
Show transcript
Introduction
Hello, welcome. In this video, we will simulate a Shell & Tube heat exchanger using ANSYS 2026 R1. Starting from creating a 3D geometry in Space Climb, creating a mesh in Fluent Machine, setting up and running the Fluent solver, until displaying colorful temperature, pressure, and velocity contours. As an example case, we use the following heat exchanger. Shell diameter 940 mm, tube length almost 10 meters, outer diameter of the tube 1 inch, 18 baffles with a spacing of 495 mm, and nozzle 16 inches. The shell side is filled with cooling water at a temperature of 38.4 degrees Celsius, and the tube side is filled with seawater at a temperature of 30 degrees. To make the simulation run on a regular computer, we simplify our model. The spacing between tubes is made twice as large so the number of tubes becomes 91, and we only model half of the section using a symmetry plane. The mass flow rate is scaled proportionally to the number of tubes, so that the velocity inside the tubes remains the same as in real conditions.
STEP 1
We start in Space Climb. Select the circle tool in the Design tab, click the center point on the Sketch plane, then type the diameter 94,0 mm and press Enter. Next, select the pool tool, click the circular surface, then type the length 9827 mm. A fluid shell cylinder is formed. Rotate the view using the middle mouse button to see the result. Because there are 91 tubes and 18 baffles, we use the script editor to make it faster and more precise.
STEP 2:
Open the Design tab, click Script, then open the geometry script file. At the top of the script, there are the main parameters, shell diameter, channel length, tube sheet thickness, tube length nozzle diameter, tube pitch, baffle spacing, baffle thickness, and position of baffle cut These values can be changed according to the drawing
aman? ,
Click Run
STEP 2:
The script creates the shell cylinder along with nozzle, channels at both ends drilling the shell with tubes and baffles cutting the model into half then automatically assigning nameat selections Open the Groups tab to check nameat selections inlet tube, outlet tube, inlet shell, outlet shell two symmetry planes, and tube wall as heat transfer surface
STEP 3 ,
Hide the shell fluid to view the tube bundle inside Notice the baffle holes that force the shell flow to turn around Ensure share topology is set to share so that the mesh of both fluids connects on the tube wall then save the file
STEP 4
Open Fluent in Machine mode In the workflow list, select Water Tick Geometry In Import Geometry, enter the Space Climb file, unit millimeters then click Import Geometry Add Local Seizing Select Yes, name it Seizing Tube, target size 10 millimeters on the tube surface then click Add Local Seizing In the generator, surface mesh size minimum 4 millimeters maximum 60 millimeters, growth rate 1.25 and curvature angle 40 degrees, then generator
STEP 4| ! 0
Surface mesh is completed in about 2 minutes with maximum skewness 0.65.
" Da BNN
In the Describe Geometry, select the Geometry that consists only of fluid regions without voids. Then click Describe Geometry. Change the type of Inlet Shell and Inlet Tube to Mass Flow Inlet. Outlet remains Pressure Outlet. Then update boundary conditions and update regions. For the K-Epsilon model with wall function, we do not add the boundary layer. Select No and proceed. In Generate the Volume Mesh, select Polyhex Core with maximum cell length 60 millimeters,
STEP 4
then click Generate the Volume Mesh. The result is about 4.6 million cells with minimum orthogonal quality 0.12, still above the safe limit of 0.1. Save the mesh through the menu File, Save, Mesh. Click Switch to Solution then Yes. Fluent switches to solver mode with the same mesh. In General, solver pressure based and stay ad. Activate gravity minus 9.81 on the Y-axis. Activate the energy model. Then open Vizchoose, select K-Epsilon Realizable with Scalable Wall Functions, and click OK. Create a cooling water material for the shell side, density 991.8, specific heat 4179, conductivity 0,6324, and viscosity 0,0007. Material for seawater on the tube side is created in the same way.
STEP 5 n
Material properties can also be set via the console using the command define/materials/create, a fast and error-free method. In the zone conditions section, assign the cooling water material to the shell fluid zone, and seawater to the tube fluid zone. In the boundary conditions section, set inlet shell to 30,67 kg per second with a temperature of 311,55 Kelvin. Inlet tube 36,1 kg per second with a temperature of 303,15 Kelvin. The tube wall is of type coaxial, meaning heat flows from the shell fluid to the tube fluid through a wall thickness of 1,65 mm. In the methods section, use the least squares gradient and second-order discretization. Then create a report definition for the average temperature at the shell and tube outlets, to monitor convergence.
STEP 6
To save memory, save the case and reopen it in the Fluent Solver 12 Core session. Select file, open, case. In the methods section, change the pressure-velocity coupling scheme from coupled to simple, as in the reference. In the initialization section, select hybrid initialization and click initialize. In the calculation, run 500 iterations and then click Calculate. The residual graph and outlet temperature plot appear during the iterations. The iterations are accelerated in this video. The simulation is considered converged when the residuals drop and the outlet temperature has stabilized. After convergence, we create contours. Open the Result tab, select Contours, New. Give it a name, select the variable Temperature, select the symmetric surfaces of the shell and tube, then click Save Display. Adjust the view from above so that the symmetric planes are fully visible.
STEP 7 »
The cooling fluid enters the shell at a high temperature, colored red, and gradually cools down, while seawater inside the tube enters at a blue color and warms up. The flow of the two fluids is in opposite directions. This is the full-resolution temperature contour. The color gradient from red to orange shows the heat transfer from the shell side to the tube side. In the same way, we create pressure and velocity contours. The commands can also be typed in the console using display objects created contor. The shell-side pressure contour shows a gradual pressure drop from inlet to outlet, around 2.1 kilopascals, due to the buffer resistance. The velocity contour shows the accelerated flow in each buffer window, then slows down in the edge areas. The velocity vector clarifies the direction of the swirling flow passing through the baffle. This is the function of a baffle, forcing the fluid to sweep the tubes transversely, thereby increasing heat transfer. Finally, we create patlines. Open patlines, new. Release particles from the shell inlet, color them based on temperature, then save the display. Orthographic and isometric views show the zigzag flow path of the cooling water. and its color changes from red to orange as the water cools down. Summary results, coolant exits the shell at 36.25 degrees, seawater exits the tube at 31.83 degrees. The heat released and absorbed is almost the same, with a difference of less than 0.3 percent, marking consistent solutions. Pressure drop in the shell is around 2.1 kilopascal and in the tube around 14.8 kilopascal. That's the complete steps for simulating CFD Shell & Tube Heat Exchanger in ANSYS from geometry space climb to colorful contour results. All geometry files, scripts, mesh, and case files are available in the project folder. Thank you for watching. Do you need a CFD simulation like this? Cerdas Inovasi Digital opens ANSYS Fluent and CFD courses from scratch, CFD Simulation Services for Heat Exchangers and Fluid Flow for Thesis theses, or industry, as well as selling example CFD heat exchanger project files for practice, complete with geometry, mesh, and Fluent case. Contact our WhatsApp or visit cerdasinovasidigital.com Thank you for watching.
Ask the class material
Type a question or keyword; we find the part of this episode that explains it and jump the video there.
My notes
Notes are saved with the current video time and are only visible to you.
Questions & answers
Stuck on a step? Ask here; the instructor and other learners can answer.
No questions yet.
Your instructor
Cerdas Inovasi Digital Team
Software developers, BIM & 3D engineers, and AI practitioners
53 video classes1,286 episodes
We build software, BIM models, games and AI automations for clients every day, and turn that hands-on work into step-by-step classes: every step is shown on screen and comes with a PDF guide you can keep.
