April 8, 2023 at 4:15 amMark LucasSubscriber
I am attempting to create a simplified 2D model of the Armfield HT33 Shell and Tube heat exchanger. I would like to simulate the heat transfer between the hot and cold fluids and determine the overall heat transfer coefficient.
It has the following Cross section:
I am attempting the simulate it with this simplification:
I am defining the cold fluid domain as solid, hot domain as a fluid and setting the part to imprints in design modler in an attempt to create an interface between the hot fluid domain and cold domain. I am attempting to model the heat transfer between these fluids to determine the overall heat transfer coefficient. I believe this is how I can set up the coupled boundary condition/
However, in Fluent, there is no option boundary conditions to set the interface or the wall to coupled.
Am I going about this problem wrong? I can't seem to figure out this coupled boundary condition for the tube walls
Thank you for your time.
April 11, 2023 at 10:59 amNikhil NaraleAnsys Employee
Try performing share topology rather than imprint. You will get a two-sided wall (wall and shadow wall) once you transfer the mesh to Fluent solver, with coupled boundary condition by default.
"I am defining the cold fluid domain as solid" - Any specific reason?
April 20, 2023 at 1:55 amMark LucasSubscriber
thank you, using "shared topology" has worked to create the shadow wall and coupled boundary condition.
I am having trouble getting the simulation to converge with any of the turbulence models. However, it seems converge with the laminar model. - Flow inside the tubes is turbulent and the annular flow is laminar/transition zone
April 20, 2023 at 6:09 amNikhil NaraleAnsys Employee
It might be necessary to examine both the mesh and the setup to address the issue at hand. Upon reviewing the mesh image, my suggestion would be to further refine it and incorporate inflation layers near the zone interface. Additionally, could you provide details about the models and boundary conditions you used? Kindly include a screenshot of the residuals for reference.
April 20, 2023 at 6:55 amMark LucasSubscriber
Sure, I refined the mesh (from 1mm to 0.5mm) and added 5 inflation layers:
Set up details:
- Energy on
- SST k-omega mode
- Setting expressions for water viscosity & density from interpolated data
- setting tube walls as couppled, copper and assigning 1.2mm wall thickness
- setting inlets as mass-flow inlets and inputting my mass flow rates and inlet temps.
- Using tube diameter as reference area (2D problem)
- Set all residuals to 1e-6
- hybrid initialisation
- run calculation
Please let me know if you need anything else, thanks for your time.
April 20, 2023 at 7:03 amNikhil NaraleAnsys Employee
Your residuals looks good to me. I would suggest that relying solely on residuals to decide on convergence may not be sufficient. It is important to also monitor other factors such as mass and energy balance and the parameters relevant to your specific analysis, such as HTC (heat transfer coefficient) and pressure drop. For mass and energy balance, check Fluxes under Reports.
April 20, 2023 at 7:37 am
April 11, 2023 at 2:24 pmRobAnsys Employee
Just to note, you're setting a 2d model. For tubes you may want to look at 2d axi-symmetric.
April 20, 2023 at 1:57 amMark LucasSubscriber
Would this effect the residual's convergence? I can't seem to get any of the turbulence models to converge
April 20, 2023 at 10:49 amRobAnsys Employee
It'll not alter the covergence, but will influence the result as the areas will be very different. And that will alter the heat transfer rate, and therefore the calculation of HTC. Read the definitions in Fluent before comparing with either theory or experimental data as they will be different unless you compare like with like.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.