Tackling Backflow using extended domain
 

I have seen somwhere that, if I want to completely avoid the backflow, I can extend the domain length wise as well as c/s area wise.
However, in that case don't you think I am messing with the domain of my interest by inducing pressure/velocity changes with the artificial (extended) domain due to Venturi effect?

Can somebody please share their insights for avoiding backflow condition?

If I just extend the domain lengthwise keeping c/s area (and other BCs) same, it does not make any difference, other than moving the backflow influenced area away from the main domain of interest. So is this the correct approach to just extend the domain length wise?

P.S I am using ANSYS Fluent evaporation-condensation model for solving a condensation problem of a tube fluid flow with mass flow rate inlet, known pressure outlet and const. temp tube wall BC. I have backflow warnings through out the simulation calculations

For a pressure outlet, you should compensate (but people usually don' because of laziness) for it of course by adjusting say your inlet/outlet pressures. In principle, once the flow arrives at the domain exit (for the unextended domain), it does not care anymore how it leaves and what else is downstream so long as you prescribe the correct exit boundary condition which is the exit pressure.

For example, if you were using a pressure outlet BC and had reversed flow and then decided to tackle it by extending the domain. You need to provide now a slightly different pressure (lower if it's a constant extrusion). Usually the small difference is not an isssue and negligible because you at least get a better solution without reversed flow that is much more acceptable than getting the wrong flow with the correct BC.

For a mass-flow outlet, you don't really need to do anything.

The only problem arises when the outlet extension causes problems in the upstream solution. This is quite rare because the point of the extension is to fix these problems.

Thanks for your reply.
I understood that I should extrude the domain as extension (without changing cross section) and use slightly different pressure than the actual know value that I have. (For my case, may be I will need higher value as the outlet is downside and in the exp. it is observed to have higher pressure than inlet).

The real key of the question is if the backflow is a numerical issue or is due to vortical structures transported towards the outlet.
That strongly depends on the formulation, on the flow geometry and so on.


Extending the lenght of the domain should be discussed in the framework of the physical BCs. at the outlet whe you prescribed a fixed pressure

How can I take care of numerical issue related to backflow?

Thanks.

Generally, if the physics you are simulating does not produce a vortical structure at the outlet, the first problem to check is for a wrong setting of the BCs.

Is your flow model fully compressible or you set an incompressible formulation?

Yes, I am simulating condensation phenomenon where stem is fully condensed to liquid water almost 70% of the tube length referenced from outlet.

P.S. the tube is vertical c-shaped (>3m long) with inlet at higher level.

Do backflow warnings cause hurdle for convergence?
 

I tried simply extruding (extend) the outlet domain BC. With application of slightly higher pressure at the new extended outlet, I could achieve approax. required actual outlet pressure at the actual outlet location.

But backflow issue is not yet solved. With this extend -extruded domain setup I just may have controlled the pressure and moved the backflow affected region little far from the actual domain.

I am doing a steady state simulation. And it is not at all converging.

Do you think the unsolved backflow warnings could be hurdle for convergence ?

Without convergence there is no meaning in the solution you get and the problems can be due to many reasons.



Have you tried first to check in a simpler controlled case problem, for example lower Re number, no condensation, etc?

Not exactly.
I have given inlet steam mass flow rate at a given pressure and temperature for a const. temperature C-shape tube. At outlet, I know pressure from the experiment.
My simulation should be able to match with the experimental temperature profile that I have along the tube length.

Can you please guide me how can I simplify the case to check and verify if my setup is right?

Backflow issue solved!
 

For me it was Eureka! I found it!!:)


The real reason for backflow at outlet of my geometry was NOT the geometry, boundary conditions or the physics itself.
It was a tiny parameter in the problem Setup.
In Fluent, in the Cellzone assignment section, there is option for Operating Conditions. In Operating Conditions unchecked Variable-Desity Parameters, which earlier I had just checked it incorrectly.


After unchecking the Variable-Desity Parameters, I got rid of the backflow completely (except for the beginning- which is acceptable)Attachment 72184