August 15, 2018 at 3:24 pmargenisbnlSubscriber
I tried to simulate a counterflow heat exchanger, a 2D domain (axisymetric condition), including pipe walls.
The idea is like this: Heat transfer between fluids involving heat conduction through the pipe wall that separate them, and, for the fluids temperature difference, the heat transfer take place. I want to estimate Nusselts number, so, i don't want to stablish any convective coefficient condition, wall temperature or heat flow condition. I don't know if this is possible.
The model consists in having a section where heat transfer between fluids is zero (where the thermal conductivity for pipe wall is 0), letting the velocity profile completely develop, and then, other section where heat transfer will take place.
So, first i simulate just the fluid flow, and I get what i want, counterflow, then, i turned on the energy equation, and every time i click the "calculate" button, i get this error "Divergence detected in AMG solver: temperature Error at host: floating point exception". I don't know if i have to stablish some special contact conditions between the fluid and the pipe wall, or something like that.
I'm attaching a ZIP file with some images: 1) Quick look of the mesh, 2) Velocity vectors of first simulation (Only fluid flow), 3) Schematics of the physical model.
Please, any help will be greatful.
August 15, 2018 at 7:33 pmDrAmineAnsys Employee
I would recommend to focus only on the central solid zone where heat conduction is allowed. You remove then the zones with zero heat conductivity. On the new walls you set adiabatic: no heat transfer.
August 15, 2018 at 9:27 pmpeteroznewmanSubscriber
One observation on the mesh for the fluid is that all the elements in each domain are the same size.
It is a best practice to use much thinner elements against the walls that grow over several layers to a square element near the center of the flow. The reason for this is the large velocity gradient from the wall to the center of the flow. There is a Mesh control called Inflation that creates the mesh effect. You pick the face and the edge or edges where you want inflation applied at the walls.
Have you calculated the Reynolds number for the two fluids to determine if the flow is laminar or turbulent? If the flow is turbulent, then there are specific rules about the thickness of the first element at the wall for the turbulence model to work correctly.
August 15, 2018 at 10:06 pmKRAdministrator
Just to add to Peter's valuable advice:
- Please use a boundary layer mesh near the wall to capture the velocity gradient
- If your flow is turbulent, please make sure that the first layer thickness is based on the y+ model you are using in your simulation. If you are using a wall function, you can use slightly larger y+ values. However, if you are using a low Re number turbulence model, you have to use a much smaller y+ value.
- Are you using a conformal mesh? Using a conformal mesh will greatly reduce your model set-up effort. Please refer to 'Share topology' in spaceClaim or DesignModeler for generating a conformal mesh. In Fluent, a conformal mesh will automatically detect wall and wall-shadow and you can use a coupled-wall boundary condition to connect the wall with fluid regions.
- In Fluent, you can set-up thin-walls (and shell conduction). With these options, you need not physically mesh your wall regions.
Please refer to the Fluent users guide and theory guide for details.
I am attaching a youtube video on Conjugate Heat Transfer analysis on, what I believe to be, a geometry similar to yours.
I hope this helps.
August 15, 2018 at 10:32 pmargenisbnlSubscriber
Hello peteroznewman, I'll have to work on the mesh, thanks for the advice, I'm still a rockie at this, really appreciate it. At that time, I wanted to have laminar flow, so, I calculated the Reynolds number at inner fluid domain and annular fluid domain before doing the simulation, and stablished boundary conditions for it, because i did not know anything about modeling turbulence. Again, thank you so much, I'll put on practice what you have told me.
August 15, 2018 at 10:43 pmargenisbnlSubscriber
Hello Karthik, I have to read about modeling turbulence, my simulation was based on laminar flow, anyway, I also have to get better the mesh, I'm a rockie on this, thank you so much for all your advices.
I'm not using a conformal mesh, but know I have to read about it, again, thanks you for that.
I know that Fluent have that option of setting a wall, shell conduction walls I think is the name that have in Fluent user guide, I haven't tested if I can use this condition and get results like the video you attached, I'll have to try. Thank you so much for all your advices, I'll put them on practice right away.
August 16, 2018 at 6:08 amDrAmineAnsys Employee
The case has to work even with very coarse mesh. The mesh refinement is off course required to get rid of diffusion which would affect the whole run and influence: consistency and robustness.
So check my post one again and verify if you have correct coupled wall at each side of the solid facing the fluid zones.
August 16, 2018 at 10:58 ampeteroznewmanSubscriber
To get a conformal mesh, open DesignModeler. In the Outline on the right, select all the Bodies at the bottom, then RMB and select Form New Part. You will get Shared Topology automatically.
September 2, 2018 at 2:35 amargenisbnlSubscriber
I want to thank all of you for help, my simulations are already working on.
- The topic ‘Axisymetric counterflow heat exchanger’ is closed to new replies.
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.
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- Suppress Fluent to open with GUI while performing in journal file
- error: Received signal SIGSEGV
- Using GPU in FLUENT
© 2023 Copyright ANSYS, Inc. All rights reserved.