Reversed Flow...
Dear All,
I am getting the message:- "reversed flow in 102 faces on pressure-outlet 11" What I need to do, in order avoid seeing this message? Expecting your experienced replies. Lopez |
Re: Reversed Flow...
You can kill the message, as you command "/solve set flow-warnings? no", on NOT GUI but TUI mode.
Jinbok |
Re: Reversed Flow...
can the reversed flow influence the result?
|
Re: Reversed Flow...
No, this reverse flow can not influence the result but it'll influence the convergence. Don't worry keep going.
bye Alamgir |
Re: Reversed Flow...
I would suggest that you first use a solver such as a 1st order momentum and energy, and then initialize. Solve and reach a convergence, and then "upgrade" to the 2nd order solutions. I find that this often removes the "reversed flow" phenomenon...which was I used to get, when I always tried to converge right from the start with 2nd order equations.
|
Re: Reversed Flow...
Dear All,
Thanx for the responses. Chris, can u please elaborate (step-by-step procedure)how to do what u have mentioned. Waiting for reply. Lopez |
Re: Reversed Flow...
First solve using 1st order momentum and/or energy until a convergence is reached (a).
Then change to a higher-order momentum and/or energy, and continue the iterations from (a) until the final convergence is reached. |
Re: Reversed Flow...
Lopez,
This a good idea given by Chris, if u get a result with most economical way and then use that values to get precision results (ie u then have approx results, that results r initials for the next scheme). Alamgir |
Reverser flow on pressure outlet
I got same problem but my solution is not converging, can anyone suggest something to improve. Thanks
|
The cause of the "Reverse Flow" phenomenon is improper initialization. If possible initialize with the actual expected values of the flow in the direction of the flow. If there are different domains with different flows, initialize and patch these domains.
Reverse flow does cause changes in result. If you have a pipe with reverse flow at the outlet, the solution near the outlet is influenced by the BC at the outlet. For eg : If you set teh outlet temperature to 150°C, and if there is reverse flow, the outlet cells and nearby cells will be at 150°C even though the solution may be at 500°C |
|
Reversible flow in faces on pressure outlet
Helo frnds, i try to create a circular domain around an airfoil, but it is not converging...the message says reversible flow in faces on pressure outlet can any1 help me plzz..thxx
|
Please post the problem.
Can you share the gemoetry?
|
1 Attachment(s)
I have the same problem in the centrifugal compressor,
1- I have reverse flow in both pressure-inlet and pressure-outlet 2- my solution is not converged. if you know how can I fixed it, please help me. |
I would suggest you to vary your mesh, it could help you for convergence and get rid of reverse flow problem.
|
Mass flow inlet / Outflow
Hi,
Try using mass flow inlet and outflow. I know that mass flow inlet will be a wrong BC since you want to simulate the mass flow and not give it as a BC, but try with some guess values at mass flow inlet. As the solution progresses, switch to Pressure inlet |
Thank you for your wise answer. When I change "mass flow inlet" into "pressure inlet"(after a relative convergence), is it necessary to change outflow to another BC?
Because I think that "pressure inlet" and "outflow" cannot be in a same geometry as BCs. |
Thank you for your wise answer. When I change "mass flow inlet" into "pressure inlet"(after a relative convergence), is it necessary to change outflow to another BC? Because I think that "pressure inlet" and "outflow" cannot be in a same geometry as BCs.
Yes please also change the outflow to a Pressure outlet. |
Ganapathy,
I am trying to simulate flow through a micro channel of 250 x 120 micron dimensions with unsteady vof model. I have given outlet BC as " pressure outlet" . Reverse flow is occurring after some time. How to avoid the problem? |
Reverse flow problem
Has the solution converged ?
Usually this will disappear once the solution converges. Is the pressure outlet boundary real ? is it really a pressure outlet in the actual physics too? |
Solution is converging at the end. For a channel with smooth surfaces either side, pressure drop is matching with theoretical drop. But if I use channel with lower surface has steps (such as 25 x 25 microns), we have to stop the simulation after fluid fills the channel (except the pockets), and get the pressure drop. But immediately after the start of flow, reversed flow occurring at outlet. Will it effect the result (in my case, its pressure drop)? If affects, how to avoid reverse flow?
P.S. I am new to FLUENT :confused: |
HI,
Suppose I have a duct. In the duct, the inlet occupies only 25% of the cross section a the top. The outlet occupies the complete cross section of the duct. In this case, if the duct length is small, the outlet will have reverse flow. This will also happen in the real world. If you want to avoid this, you must know the outlet pressure profile and apply it using a UDF or by dividing the outlet in appropriate number of parts. All this is tedious, so simply pull the outlet much further away from its current location, i.e. if the outlet is at say 100 micron from the inlet, (this may be your actual case), pull it till say 500 micron( this is not real, but this will avoid reverse flow) You can always measure dP across a plain representing the real outlet location |
Thank you very much sir.
And one more problem I want to pose. Since I am imposing const. velocity condition at the pipe inlet I am getting a greater pressure drop, so I extended the upstream length. It is causing more computational time. So how to impose parabolic velocity inlet at the pipe inlet in FLUENT. Pl help me. |
backflow
hi all,
ı have an rectangular geometry (lenght:76, width:27 mm). heat flux is applied from one of the vertical walls. ı have velocity inlet BC at lower part and also pressure outlet BC at upper part. velocity magnitute is zero (0) (no forced convection), initial gauge pressure is also zero and temperature is 298 K at velocity inlet BC. also, for pressure outlet BC gauge pressure is 0 and backflow temperature is set 298 K. initial temperature is also 298K. the problem is that reversed flow occured. "reversed flow in 34 faces on pressure-outlet 17" the solution is converged but ı am not sure it is right or not. any suggestion. thanks for you time. |
reversed flow
hi all,
ı have an rectangular geometry (lenght:76, width:27 mm). heat flux is applied from one of the vertical walls. ı have velocity inlet BC at lower part and also pressure outlet BC at upper part. velocity magnitute is zero (0) (no forced convection), initial gauge pressure is also zero and temperature is 298 K at velocity inlet BC. also, for pressure outlet BC gauge pressure is 0 and backflow temperature is set 298 K. initial temperature is also 298K. the problem is that reversed flow occured. "reversed flow in 34 faces on pressure-outlet 17" the solution is converged but ı am not sure it is right or not. any suggestion. thanks for you time. |
i don't know if it helps, but if possible: try to use smaller time steps and with multiphase flows you should also enable specified operating density. it solved my problem with the reversed flow.
|
Long pipe (laminar flow) gets reversed flow - not converging
My model is a u-shape pipe which is pretty long (220 cm total). There is heat flux from walls. The error is repeated continuously while solving. Also the answers are not converging.
Can anyone help me please? |
hello
I have same problem but the result converge is the result will be right |
It happens due to a poor quality of mesh, abnormal boundary condition at inlet/outlet, short downstream length etc.
Remedies are: > if vortex formation/recirculation of flow near an outlet boundary, increase the downstream length. > check the mesh quality, improve it. > use higher order scheme > At last reduce the relaxation factor if necessary. |
2 Attachment(s)
Hello guys, (Doubt atmospheric conditions)
I am working on rectangular geometry with air as fluid. Actually i have one inlet at the one side face of the rectangle and one outlet is quite opposite to the other side face of the rectangle and reaming all are walls. I want atmospheric conditions at both inlet and outlet, for that i have taken pressure inlet and pressure outlet with default values (i.e. Gauge pressure is Zero). But unfortunately when I am simulating I am getting reverse flow. Moreover my solution is converging. Could you please any one explain me. What kind of mistake I have done. I am attaching my Residual and geometry images. |
Revesed flow heat transfer
hi all, i have a square with heat generation rate inside that, i have three boundary conditions with constant temperature, but i dont have heat flux from one of walls, i want to simulate this problem in Fluent, could you please any one explain me??
|
Quote:
|
Reverse flow is on, this massage will be shown when your result will diverging.
To solve this problem, you should check the boundary conditions properly and most importantly change the under relaxation factor from solver settings. Lower the relaxation factor, get higher stability in convergence. And I think thus you can get more better simulation result. |
Quote:
Sorry, that is not correct. Reverse flow could be a normal flow behaviour at your boundary, if you not have a straight forward outflow. Especially at pressure outlets and buoyancy driven flows. There are some possiblitys which could help:
|
All times are GMT -4. The time now is 22:41. |