artificial walls
 

Hi all.:)

I am modeling a flow in a rectangular channel. I have already results, but during the run CFX has created artificial walls during all iterations. (however the solver has converged). In this context I should be confident with the results right?

Best Regards.

hi Antonio,
the quality of your solution depends on the "dimension" of the artificial wall.
I think you should change your settings in order to avoid the wall.
Let me know something about your simulation in order to help you.
Regards

Hi.

Thanks a lot for your recommendation. That was precisely what I was thinking to do but as I am new at this I prefer to listen someone else opinion too

Best regards.

It depends on what you are trying to get out of the analysis. The walls are there to prevent backflow at the inlet or outlet boundaries. If you want this recirculation captured accurately you will need to redo the simulation with the boundaries further away. If these recirculations are not important then your result is OK.

Hello!

I've spent quite a lot of time and made a lot of mistakes modelling heat transfer in rectangular channels, so I'd like to express my opinion.
Generally, getting walls at outlets during the iteration process is OK, so You shouldn't be afraid of it. This feature in CFX is used to improve convergence. If You do expect any recirculation near the outlet, follow Mr. Horrocks' advice (but I would better use opening instead of outlet, because remaining walls affect the pressure drop). If You don't, just like in my case, make sure that no walls are placed at final iterations. If any walls still exist after the run has finished, You should probably review Your convergence criteria. I got rid of the problem by specifying conservation target.

PS According to my experience (may not be right) no artificial walls should remain at the outlet of a straight smooth rectangular channel after all convergence criteria are reached unless:
1) heat transfer model is used together with bouancy ;
2) LES, DES, SAS models are used;
3) any "exotic" physics is modeled.

Good luck!

Your comment about using an opening rather than an outlet only applies if you are using a pressure drop to drive the flow. When you drive the flow with a pressure drop you need the boundaries in the correct locations to drive the flow correctly so moving the boundaries is difficult. However if you are not driving the flow this way then you should move the boundary further away. This is much preferable to changing to an opening and will be far more accurate.

The walls can be present in a fully converged solution. Quite simply if a recirculation exists at the boundary you will get reverse flow and therefore the walls will form. This can exist in a fully converged solution so converging more tightly will not always help.

As for your PS, the situation is very simple - if vorticies exist then you will get backflow, and therefore walls can form. Your examples are just different ways vorticies can for and there are many others - the most common one being placing the exit boundary too close to bluff flow features with separations.

Dear Ghorrocks. Thanks a lot.

I was writing at the same time of you. I have already see your post.

Best Regards

Dear Antonio and Mr. Horrocks!
The promlem we are discussing here is important to me. Like most people I'm not completely sure of anything. Therefore I'll state my case and I'd like you to prove or disprove my approach.

Simple case: gas flows through a smooth straight circular (axisymmetric, i.e. easier to model) channel. Gas has a constant equally spaced temperature at the inlet. Wall temperature also has a constant value, which is lower than the gas temperature. My target is to evaluate heat transfer coefficient and hydraulic resistance at differrent given Re numbers for a hydraulically developed flow.

As I don't expect any large eddies and I do expect the flow to be axisymmetric, I use eddy viscosity turbulence model (SST) and steady state.

To dirve the flow I don't use pressure drop (by specifying both inlet and outlet pressure) because, as far as I understand, the boundary problem would be overdefined by pressure and underdefined by velocity (excuse me if something's wrong with my English). I could avoid it by specifying one full pressure and one static pressure, but it's easier to specify velocity at the inlet (Re is given) and static pressure at the outlet. Finally, I estimate the calming length and determine outlet position to get rid of calming region influence on flow.

So, in this simple case when I don't consider gravity and the outlet BC is out of calming region, nothing but some mystical power may force the flow backwards. Nevertheless, I did have walls on a converged (with RMS criterion) solution. That seemed unphysical and made me upset. So, I started monitoring integral characteristics of critical importance (such as wall heat fluxes, temperatures, pressures, etc.), lowered target RMSes, introduced conservation target and double precision. Those measures made the walls fade away. Probably those walls wouldn't affect pressure differences (needed for resistance calculation) along the channel, but they definitely would affect the absolute pressure values (if the inlet mass flow rate and the outlet static pressure are constrained, then the more walls we place at the outlet, the higher inlet pressure we need to force the flow through the channel).

Next target is to consider gravity. Obviously, it has little effect at high Re and low Gr. But if hot gas flows upwards slowly in the gravity field and channel walls are much colder, we get a circular backflow region along the whole channel. Velocity profile (coloured by temperature) looks like this:
http://img-fotki.yandex.ru/get/4314/...35525923_L.jpg
Beginning of the recirculation zone is shown on these vector plots:
http://img-fotki.yandex.ru/get/3804/...5d3b8ddc_L.jpg
http://img-fotki.yandex.ru/get/4314/...d99c8764_L.jpg

But the question is where the streamlines of recirculation zone close up and the speed profile changes to a single parabola (if laminar). Most likely it happens far away from the inlet where (Tgas - Twall) -> 0. As Mr. Horrocks says, it is more preferable to move the outlet further away to using opening, and I fully agree with that. But in my particular case that would make the model more then twice as large compared to the one with opening BC. So, I have to place my BC somewhere within the recirculation zone (sorry for MS Paint):
http://img-fotki.yandex.ru/get/3803/...8ce3f094_L.jpg

If I apply outlet BC then no cooled gas from near-wall region will be allowed back into the domain and artificial walls will appear at the outlet. Even if the solution converges somehow, I it will be unphysical (overrated value of outlet speed). And it will still have artificial walls.

So, in this particular case, artificial walls indicate incorrect flow and heat transfer resolution. That's why openeng BC has to be used.

Concluding it all i'd like to say:
1. No doubt, moving the boundary further away (following Mr. Horrocks) is always preferable.
2. I still insist that If №1 is impossible and final solution contains artificial walls ,then using opening yields more accurate solution. That's why no artificial walls should be left for final results.

Waiting for constructive criticism)

You are about right in your summary. Some comments:

Read the documentation about specification of boundary conditions. It will say a velocity boundary and a pressure boundary is the best combination of boundary conditions to use as it will be easiest to converge. If you know the flow rate through the device you can use this combination. If all you know is the pressure drop then you can use the pressure boundary pair, but it is harder to converge.

Is there a problem in making you model twice as large? From what you describe, it is your only option to get something accurate. Obviously you will need to wait longer for solver time.

Thank You for Your comments!

Quote: "Read the documentation about specification of boundary conditions. It will say a velocity boundary and a pressure boundary is the best combination of boundary conditions to use as it will be easiest to converge."

Been there, done that. Can't disagree.

Quote: "If all you know is the pressure drop then you can use the pressure boundary pair, but it is harder to converge."

Agree, but not for the described case. The thing is that when specifying pressure at both ends we actually predetermine the channel drag instead of solving for it, unless both static and total pressure are used. But, as far as I get it, total pressure is an explicit function of velocity (i.e. mass flow rate). That means that we can't calculate the drag without considering velocity (directly or via total pressure or mass flow rate) at one of the boundaries. Thus, "best combination" seems the only appropriate.

"Is there a problem in making you model twice as large?"

There is no problem in making the model twice as large for one particular case. But it really is a problem to determine the appropriate channel length for each particular regime and run all those full-size solutions. Besides, in some regimes it is impossible to have the required mesh generated before getting way too old. That's why I like openings more than full-size models and much more than artificial walls.

OK, that is where the judgement come in. The important thing is to know that you are making a compromise. You obviously understand that so you are going down the correct track.

Yes, I am making a compromise and I understand that. I agree with everything You said. But the main question is:
If a boundary can't be moved away from backflow region for some reason then what is a greater compromise for such boundary location: using an opening BC or using an outlet BC and leaving artificial walls in the final results? I vote for using opening. Do You think outlet with walls is better?
Sorry for being boring)

Depends on the application. Some things to consider:

Will the failure of backflow cause the recirculation to be completely wrong?
Will the opening cause convergence problems?
Will the artificial walls cause converge problems?
In an opening you have to specify the condition (ie temperature, scalars, volume/mass fractions etc) of the backflow. Do you know the condition of the backflow sufficiently well to specify this?

There is no universal answer. No problem with being boring, getting the details right is the only way to do good simulations.

Now that's comprehensive! A guess Antonio should be really happy) Thanks again.

Dear all.

Thanks a lot for the exchange of views.

Best regards