July 18, 2018 at 5:22 pmJoseph OmandacSubscriber
I am quite new to CFD (Fluent 14.5) with about 4 months of reading and performing tutorials by myself. As part of my undergraduate thesis project, I need to perform a CFD analysis on a conventional solar still to determine it's theoretical yield. The system works simply by the solar distillation process. Here is a link for a short background on the system: <http://www.solaqua.com/solstilbas.html>
I've been working on this case for a month now, and my main problem, I think, is that I have a hard time choosing the correct time step rate to converge the problem and at the same time consider the number of iterations and total computing time this case will take up. Aside from that, I think I need everyone's opinion on the quality of my case and the accuracy of the solution it will provide.
Skewness: Max = 0.547, Ave = 0.01186
Orthogonal Quality: Min = 0.715, Ave = 0.9813
Parallel on 2 cores
General: Pressure-based, absolute velocity formulation, transient case with gravity = -9.81
Multiphase: VOF with 3 Eulerian phases (air, water liquid, water vapor), Implicit with implicit body force checked
Viscous: RNG k-epsilon withe enhanced wall treatment
Radiation: Surface-to-surface (S2S) with solar tracing set to experimental data
Materials: air, water liquid, water vapor; stainless steel, tempered glass
Phases: Air as primary phase, water liquid and vapor as secondary phase. Evaporation and condensation on mass interaction. Surface tension modelling with continuum surface force and wall adhesion. 72 dyn/cm on water liquid - air and water vapor - water liquid interfaces.
Boundary Conditions: Bottom, glazing cover, and downcomer (collector trough) of the solar still set to constant temperature (70, 35, 35 deg C). Side walls are adiabatic with no slip condition. 45 deg contact angle for wall adhesion between phases on glazing cover. Specified operating density equal to air, least dense substance.
PISO Scheme. Least squares cell based. PRESTO! with second order upwind on the rest.
Default under-relaxation factors except for 0.9 on turbulent viscosity and energy (was diverging on my early attempts).
Initial conditions: Water level in the solar still is set to 3 cm at 60 deg C, while fluid is as 65 deg C (patched).
Calculation: 1 second time step size (s), 3600 time steps, with 100 max iterations per time step
I do not know how to attach my case file for the time being. I am currently solving the case again, with tweaked configuration. Anything I missed to include here kindly inform me.
WIll truly appreciate all your responses and efforts. Thanks!
July 18, 2018 at 11:30 pmJoseph OmandacSubscriber
Here are some of the residuals I am receiving with my recent run.
From iterations 0 - 3000, the residuals were getting steadily larger. (Thinking this would definitely diverge after some iterations, I slept).
From iterations 3000 - onwards, the residuals were once again getting lower. However, I am not sure why the iterations complete the maximum number when it clearly shows that the residuals have met the convergence criteria of 0.001 (1e-3). If they could converge at each time step, this would save me a lot of time.
July 19, 2018 at 1:48 amKarthik RAdministrator
The model seems complicated. Here are a couple of things to try
- Try to switch off the energy and radiation models and just solve the flow. Try to see if you are able to get good physical results for flow and VOF.
- Attempt to build in the complexity layer by layer.
- Try and use the explicit VOF formulation as opposed to implicit.
- Please make sure that your are satisfying the CFL stability criterion.
- Calculate your dimensionless numbers and double-check to ensure your Fluent model is set-up to solve the correct physics.
It is always a good practice to start small and built on top of that. Simplify your problem and resolve things one at a time. This will help you isolate your error.
Hope this helps.
July 19, 2018 at 1:58 pmRobAnsys Employee
Just to add. Water vapour and air should be a species mixture in one phase; you then transfer mass from water-liquid to water-vapour using the mass transfer section in the phase interaction. You might need the latest version for this, R14.5 is approximately 5 years old now.
July 20, 2018 at 5:38 amJoseph OmandacSubscriber
Thank you for looking into my model. I'll work on running and verifying the simple flow model and building layer by layer the complexity and the physics of the entire system.
Can you please explain more about the CFL stability criterion/condition? I have often encountered this term in the forums yet I still do not know what this means or how to apply it. I apologize. I do not have the proper and sufficient background on the computational methods and mathematics of the solver.
Once again, thank you for your advice. I'll update you on the progress soon.
July 20, 2018 at 5:41 amJoseph OmandacSubscriber
Thank you for pointing that out.
This explains a lot why I am not getting the reasonable outcome of the simulation.
At the moment, I am in the process of installing the student version of ANSYS 19.1. Afterward, I'll build the model back again and revise the phase configuration.
If ever I have trouble on that again, I'll ask you again. I hope that's okay.
July 20, 2018 at 9:59 amRobAnsys Employee
No worries Joseph. The species set-up and phase change options are fairly straight forward, but I'm not aware of any examples/documentation that I can share. As ANSYS staff we're limited in what we can do on a public forum.
July 21, 2018 at 6:26 amJoseph OmandacSubscriber
I've already installed the ANSYS 19.1 Student Version, and yes, the phase change options for my case were quite simple.
However, I am confused on what to include in the Species Transport model for my case which mainly involves evaporation and condensation of H20. I am more particular in the amount of condensed water in the top of my system, and the amount of water deposited at the downcomer (collector trough).
So thinking about the condensation on a surface (side walls and top), do I check volumetric and surface reaction? How about the options in thermal diffusion, etc? I read the Fluent theory guide and it doesn't much describe about water evaporating and condensing on a surface.
Also, I installed the ANSYS 19.1 Student Version on two of my laptops. After I installed it on my second laptop, the ANSYS softwares (Meshing, Fluent, etc.) were requesting for a license. How do I resolve this?
Sorry for the inconvenience this has brought. I appreciate you looking into my problem.
July 21, 2018 at 12:47 pmKarthik RAdministrator
CFL condition, in CFD, addresses the stability of your numerical simulation in a finite volume approach. Put simply, this condition must be satisfied for a transient simulation to be stable, especially when using an explicit time-integration scheme. Depending on the minimum size of your grid, the CFL condition controls the time step you can use to march forward in time. If your time step is greater than the 'minimum' time step size specified by the CFL condition, your solution with diverge.
It is defined as del_t <= (C * del_x / v_fluid) where, del_t - time step size, del_x - minimum grid size, v_fluid - fluid velocity scale, C - Courant number
To learn more on how CFL condition is derived, please refer to this lecture notes from MIT opencourseware.
Please also search for 'Courant Number' in ANSYS Fluent Users and Theory guides to read more about how Fluent handles Courant number for various models (especially check out the explicit VOF model).
Hopefully this equips you with a little background on Courant number.
July 24, 2018 at 6:35 amJoseph OmandacSubscriber
Thank you for enlightening me more on the CFL condition. I reviewed the lecture notes you sent, and I did quite have a better grasp on changing the time step size to satisfy the CFL condition.
As you have advised in your first reply, I tried to rebuild the model from scratch and checked if the basic flow and VOF are reasonable. Upon seeing the results, I still think I have a problem with the flow.
I recreated the model with only two-phase volume of fluid (VOF) framework present, explicit and checked implicit body force. The solver is transient with gravity. Only air and water-liquid, with no phase interaction and surface tension modelled. The phases are continuous, thus I used a sharp interface modelling.
I initialized the flow with 0 velocity in all axes, and also 0 water-liquid volume fraction. After that, I patched the volume of the water-liquid. Here is the volume fraction contour of the model after initializing.
I ran the calculation at 0.1 seconds for 100 time steps, for a total of 10 seconds. Just to check if something weird is going on. Then I saw this on the resulting volume fraction contour.
The flow is supposed to be stagnant. Absolutely, the water should not have gone anywhere since there are no other forces acting on it. There is supposed to be no diffusion between the water and air, the interface is distinct.
What is happening in my model? Am I missing something? Is this because of my mesh? Am I doing the incorrect method of initializing the case?
I've been working on this basic model for days and I can't still find out what is wrong.
Thank you for your time and effort helping out. I really appreciate it. And I apologize, really, for any inconvenience this has brought.
July 24, 2018 at 10:38 amRobAnsys Employee
Check you've got 3-4 cells in the water depth, it's possible that if you haven't that the VOF model is struggling. The other thing to do is initialise with a very small (1e-6 m/s) velocity in the x or z direction as it's a fluid dynamics solver and static cases are always more difficult to solve.
Re the choice of multiphase model: give you need multiple cells over the condensate thickness for VOF you might be better using the Eulerian Multifluid VOF.
July 25, 2018 at 5:54 amJoseph OmandacSubscriber
I checked the marked cells unto which I patched the liquid water, and it only has a single cell for the water thickness. I think that's been the root of the problem, along with the overall element size above the liquid. I also initialized with an x velocity of 1e-6, which works cause it reduced the weird stuff that has been happening in the results.
I refined the overall element size and it still has two cells for the thickness.
I want to have a finer mesh on this area, but not on the whole mesh. That would significantly increase the computational time for my project. How do I refine the mesh on this particular volume of the fluid?
July 25, 2018 at 7:39 amDrAmineAnsys Employee
You can refine it in your pre-processor or in Fluent by using the adaption tools and using the method by boundary to select the number of cells or the distance off the boundary of interest.
June 9, 2019 at 12:58 pmFannyMasloskiSubscriber
Hello! I'm writing you because I have a specific question regarding the modelling of the solar still in ANSYS FLUENT. I need this for my master Thesis as soon as possible and it would be really great if you can give me an answer to this question:
What is the vapor model that you used? Because I don't get nice results when I select for water-vapor "incompressible-ideal-gas". I think my main problem is around here...a vapor model regarding temperature and Enthalpy. What do you think I should select instead?
Thank you very much for your cooperation and kind regards!
- You must be logged in to reply to this topic.
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
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.