July 30, 2023 at 4:19 pmDominik BuksaSubscriber
I have a huge backflow problem in my case.
I am considering flow through a cube (I made a 2d model because 3d didn't work but it didn't solve the problem).
My boundary conditions: 0.01 m/s velocity inlet and default pressure outlet. Two-phase flow (mixture or VOF), with gravity on. Unfortunately, as shown in the picture, I have a strong reverse flow, which gives non-physical results - because the inlet velocity is 0.01 m/s and the reverse flow is 0.6 m/s (I can't increase the velocity inlet)
I've tried extending the outlet, fine-tuning the mesh, setting a different operational density, but nothing works. Unfortunately, I have no idea what I can do and this is an important problem for me. (With gravity off, no problem.) It is interesting that gravity "destroys" the model even when the pressure values of my substance are constant.
Has anyone encountered such a problem? the continuity equation does not converge (i try hybrid and standard initialzation).
It gives a google drive link with a link (case and wbpj file) , could any of you help me? In the future I will have much more complicated geometry, so I need to refine this model so that I don't have the same problems later.
July 31, 2023 at 6:10 amNikhil NaraleAnsys Employee
As an Ansys employee, we can't download any files attached to this post. However, I'll try to put my thoughts here:
1. Make sure the direction of the assigned gravity is correct.
2. Is this a steady case? I suggest extending the simulation further (currently at 94 iterations). It's normal to see a reversed flow at the beginning, but it should gradually improve with more iterations if everything is set up correctly.
3. I'm curious about the purpose of simulating two phases. Can you share more details on how did you set up the multiphase flow?
July 31, 2023 at 6:26 amDominik BuksaSubscriber
Hi. Thanks for the help.
1. The direction of gravity is correct.
2. I checked 2000 iterations but the continuity equation does not converge at this value of the inlet velocity
3. I want to model a two-phase flow of moist air so that I can observe the condensation processes.
However, with “transport species” the problem that occurs is the same
July 31, 2023 at 6:59 amSRPAnsys Employee
1) It is great if you share details related to the multiphase model you used, and corresponding setting. And also share how you setup the condensation model?
2) Check the material properties you entered in the simulation.
Check the saturation temperature you entered.
July 31, 2023 at 7:07 am
July 31, 2023 at 7:13 amSRPAnsys Employee
For a case of single flow (means you are not considering condensation and want to see only the species tranport with flow), I suggest you to turn off the species transport equation and run simulation for 800 iteration so that we get to know that there was no issue with the continiuity and momentum equation. Later on you can turn on the species tranport.
July 31, 2023 at 7:25 am
July 31, 2023 at 7:41 amSRPAnsys Employee
It means species transport has an issue.
A very low species mass diffusivity can affect the convergence specially in regions with low turbulent diffusivity (viscosity). The diffusive part of the species transport equation can become extremely small compared to convective part and thus might create problems with convergence.
You can try to start with a higher laminar mass diffusivity for the species and then slowly drop it.
July 31, 2023 at 7:54 amDominik BuksaSubscriber
I tried to increase the mass diffusivity, but to no avail :( The continuity equation does indeed start to converge better but the reverse flow reached 72.5% after 2500 iterations.
July 31, 2023 at 10:31 amRobAnsys Employee
What material properties did you use? Specifically density. What are your operating conditions? Where does the condensate go?
July 31, 2023 at 10:36 amDominik BuksaSubscriber
I use only constant value for properties and ,,incompresible ideal gas" for density.
My operating conditions is default values (101325 Pa with opearting density minimum average phase and gravity).
I use now one-phase model ,,transport species" without dealing with condensate, but problem is the same.
July 31, 2023 at 11:07 amRobAnsys Employee
OK, I suspect part of the problem is the operating density. Check https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v232/en/flu_ug/flu_ug_bcs_sec_operating.html You may want to initialise the domain to the outlet condition, and use the (hopefully uniform) density that's calculated by Fluent as the operating density. If you look at the (rho - rho_operating) you can explain why.
July 31, 2023 at 11:42 amDominik BuksaSubscriber
You're right, the two-phase model converges better when I set the operating pressure to "mixture average". However, the problem persists.
Additionally, with only "species transport" turned on, I do not use operating pressure and the problem is the same - reverse flow is 70% of the outlet field .
July 31, 2023 at 12:21 pmRobAnsys Employee
You are using operating density, and depending on other boundary conditions the high reverse flow may be correct for those settings.
July 31, 2023 at 12:25 pmDominik BuksaSubscriber
Ok thank you for help!
If backflow interferes with my simulation, can I "skip" it (prevent backflow)?
Or in a two-phase model, instead of velocity inlet and pressure outlet, set massflow inlet and massflow outlet to the same value? - Will this be correct or will it disrupt my simulation?
July 31, 2023 at 12:30 pmRobAnsys Employee
No to all!
If you prevent backflow you need to identify why it's happening. What are the wall boundary conditions? I can see a few reasons you are seeing the backflow, but you need to figure that out as I'm bound by a few rules. However, if you answer the various questions you should either get to the answer or provide enough information for us to help.
Mass in and mass out is a very bad idea. In a steady model in theory you finish up with vacuum or infinite pressure: in practice Fluent will do something and most likely not converge or diverge.
July 31, 2023 at 12:38 pmDominik BuksaSubscriber
I have made several models using "species transport", in each of them I have a problem with back flow, while the single phase works normally.
wall boundary conditions are default, no slip, adiabat.
July 31, 2023 at 12:49 pmRobAnsys Employee
Species transport is single phase.
OK, so why would you expect condensation in the species case later on? Have you set the operating density like I suggested?
July 31, 2023 at 12:53 pmDominik BuksaSubscriber
Later on when the geometry is complicated I will expect condensation as my mixture will be close to the dew point.
I set the operating density but it didn't help.
July 31, 2023 at 1:09 pmRobAnsys Employee
Weird, how is the convergence looking?
July 31, 2023 at 3:25 pm
July 31, 2023 at 3:41 pmRobAnsys Employee
That's not ideal. Why are you using nitrogen & water vapour, with I assume oxygen as the third species? Air & vapour would be marginally more efficient.
August 1, 2023 at 9:49 amDominik BuksaSubscriber
You're right! Now in a two-phase flow, the operating density change works.
With the "mixture averaged" setting, the reverse flow disappears - while with any other it is almost 100%.
I've read that in Boussinesq's multiphase flow approach, "minimum phase average" should be selected. However, it gives me wrong results.
August 1, 2023 at 10:34 amRobAnsys Employee
Please look very carefully at what you're modelling and setting. The reverse flow occurs for a reason, which is linked to inflow, gas density change (and/or condensation) and outlet & operating conditions. Assuming the mesh is good and the solution converged it's likely that the result is correct for the defined conditions.
August 1, 2023 at 11:04 amDominik BuksaSubscriber
I set volume fraction of h20 to 0.005, o2 to 0.228 and rest is n2. The densities of the substance are constant and the possibility of condensation has not been enabled.
- When i use same BC but operating density ,,minimum average phase" for expamle contour of velocity are as image 1 and residual image 2.
- But when i use ,,mixture average density" solutions are different (image 3, and 4)
- As you can see The results are so different that they destroy the whole simulation.
- 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.
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- 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
- Suppress Fluent to open with GUI while performing in journal file
- Mesh Interfaces in ANSYS FLUENT
- Time Step Size and Courant Number
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.