reversed flow
 

hello everyone,

my cas is a 'T' tube connected by two cylindres with an inlet and 2 outlet.
the fluide is turbulent. i made the boundary condition as 'outflow', the warning came to me was "reversed flow". i looked for the former thread, it is said that i could change it to 'pressure outlet'. after operation, the warning is always "reversed flow".
does someone know what happened?

thank you
steven

you have a vortex crossing the outlet.
It is just a warning, let iterate, the warning may disappear

Extend your computational domain at the outlets, i.e. ensure that the outlet is far away from the tee

Ok, thank you, i will wait a bit.

Thank you. in this case the distance of outlets are at least 25 times that of diameter

hello, Maxime,this is what i get. do you have some suggestions?
https://www.dropbox.com/s/30deqc29eq...ed%20flow.docx

you have a convergence problem, and I don't think it comes to your reversed flow
-check Mesh
-how are your turbulent bc?

the mesh is not too bad. i chose the standard wall function. here are the informations https://www.dropbox.com/s/30deqc29eq...ed%20flow.docx

-what is the quality of worst element? (show worst element option in gambit)
-what are the tubulent bc at your inlet (you showed the turbulent model)
-did you scaled your model?
-can you copy and paste the output from checkMesh

hello, this is the information. thank you
https://www.dropbox.com/s/xml8ctvagskchbf/0628-2.docx


Mesh Quality:
Orthogonal Quality ranges from 0 to 1, where values close to 0 correspond to low quality.
Minimum Orthogonal Quality = 2.75142e-01
Maximum Aspect Ratio = 1.61014e+01

ok, your mesh is ok and seems to be scaled
in the velocity BC, you should have turbulent parameters, waht do you have?
How is you material? density, viscosity?

i have the parameters of K and epsilon. k=0.053985 and epsilon=1.4722. the velocity is 5m/s, it is calculated with the Re=100000. the material is water-liquid. density is about 1000kg/m3, and viscosity is about 0.001kg/m-s

Ok I have to hurry
Try to switch with realizable-kepsilon
Try with and without enhanced wall treatment

sorry, i didn't understand what you mean 'realizable-kepsilon'. the k,epsilon values that i used are also calculated with Re=100000.

Other turbulence model

hello Max, i have tried the realizable k-epsilon, but the situation didn't change, there are still problem of conbergence and warnings of reversed flow. By the way, the Y+ is between 5 and 30.

Hi,

I have same problem and I think it is the boundary conditions imposed on your two outputs which poses the problem .. when you have two output can not impose "pressure" at outlet..

What are your boundary conditions at the outlets??

I use outflow as the BC of outlet. in fact, i had wanted to try the pressure outlet, but i don't know the factors that i have to fill

The condition of pressure outlet is valid when we have "one outlet" for two and more of outlet this condition is not valid, you must use the "equal flow rate" at outlets.. try to reduce the underelaxation at the minimum (0.1 or 0.2)

so what should I put as the gauge pressure?

outflow its OK!

OK, I have tried a lot the outflow, but i always get reversed flow and also the problem of convergence. how did you solve your problem?

I decreased at least the different under-relaxation factor (0.1 and 0.2) because in the beginning of simulation we have very significant disruption to overcome so you should lower these values, then when the solution begins to stabilize you can increase it gradually

OK, I will have a try. Thank you.

Steven,
Is your problem fixed?
Don't focus on reversed flow warning.
The convergence is the one you need to fix.
Maybe you should consider & switch on unsteady solver, if rayan's tipp didn't help you.
Did you also try to compute on a much finer grid?

Thank you Max.

I have solved the problem of convergence. Do you remember the gambit file that i sent to you. I united the two volumes in the center, then it worked without warning under the model 'outflow'. This makes me confused, I don't know why this works. Do you know what happened?

Good to read you solved your problem.
But sounds weird.
Anyway it is solved (maybe an internal surface or whatever, but I checked and everything was ok)

You are right, it is a problem of interface. I came to know why just now. My professor told me that i overlapped two faces together at the entrance of the small tube. When i united them together, i removed the face which caused problem.

Anyway, Thank you so much.

yes, typical error in Gambit :D

Hello Max,
I have a question, how can i creat a face to mesure the pressure of my larger tube depending on the lenghth?
Thank you.
Steven

you can do that in fluent, post-processor.
I cannot remember the exact name, I can tell you on Monday when I return at the office.
Kids are giving more troubles than mesh.... :)

Hi, I'd go to Insert/Location/Plane in CFD-Post. Then define the plane (e.g., z=constant) and plot the desired variable on it.

Cheers,
Michujo.

Haha, maybe you were more naughty as a kid ;)

OK, thank you, i will have a try.
Steven.