Learning Forum

[Dominik Buksa]

Hello everyone.
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). 

https://drive.google.com/drive/folders/13e37e40V74l0dty0HNNc4sTRYqqp6WtZ?usp=sharing

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.
Please help.

[Nikhil Narale]

Hello,

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? 


Thanks,

Nikhil

[Dominik Buksa]

 

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

 

 

 

[SRP]

Hi,

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.

Thank you.

[Dominik Buksa]

I think the problem lies elsewhere. Here I present monitor values for single phase flow ,,species transport". 

BC: % of H20 65% and O2 35% (i omit n2), temperature in 12.5 C, temp. fluid patch 11C. I try increase velocity inlet to 0.1 m/s but there is no improvement.

[SRP]

Hi,

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.

Thank you.

[Dominik Buksa]

Yes - for now I'm just trying to find the problem and in the end I want to go back to the two-phase model anyway.

When i off ,,species transport" situation is ok :( 

[SRP]

Hi,

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.

[Dominik Buksa]

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.

[Rob]

What material properties did you use? Specifically density. What are your operating conditions? Where does the condensate go? 

[Dominik Buksa]

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. 

 

[Rob]

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. 

[Dominik Buksa]

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 .

[Rob]

You are using operating density, and depending on other boundary conditions the high reverse flow may be correct for those settings. 

[Dominik Buksa]

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?

[Rob]

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. 

[Dominik Buksa]

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.

[Rob]

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?

[Dominik Buksa]

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.

[Rob]

Weird, how is the convergence looking?

 

[Dominik Buksa]

[Rob]

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. 

[Dominik Buksa]

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.

[Rob]

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. 

[Dominik Buksa]

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. 

1. When i use same BC but operating density ,,minimum average phase" for expamle contour of velocity are as image 1 and residual image 2.
2. But when i use ,,mixture average density" solutions are different (image 3, and 4)
3. As you can see The results are so different that they destroy the whole simulation.