Hi

When I increase the timestep, I get the above notice after about 50 iterations and this continues until the case converges (1E-4). Will this affect the solution?

If I use the auto timescale, I dont get this notice but the simulation doesn't converged.

My model is described in http://www.cfd-online.com/Forum/cfx.cgi?read=24122

Hai Melvin,

I think along with your error message you would have got this message also.

"There are some reverse flows in areas near your outlet. Try chaning your Outlet to Opening"

Changing to Opening should solve the problem.

Regards, Subha.

Why is that we receive such a message in the first place. Is it because our outlet boundary is not far enough from inlet? I have been receiving this message for my steady state problem, but when i ran LES case i didnt get this message. I am not sure what is going on!

Usman

Hi Melvin,

Look at your flow field and pay attention to the % of the outlet area that is walled off (reported in the warning). The solver does this to prevent reverse flow, which you clearly don't want if you specified an outlet (otherwise you would have defined an opening, right?).

If the % area is small, it may not have a significant effect on your solution. If it is large, you should investigate the flow in the vicinity of the outlet. Try seeding streamlines from the outlet to see the reverse flow region, for instance.

In the end, you may have to extend your model to include more geometry downstream or change the boundary condition to more accurately represent what is occurring at this location. For instance, if you set an average static pressure but the flow dumps into a plenum beyond the outlet, a constant static pressure may be more appropriate. Similarly, if it is a mass flow specified outlet, set the pressure profile at the outlet to a constant value (which enforces a constant static pressure across your outlet which achieving the desired mass flow).

The key is to understand the physics and act accordingly.

-CycLone

Thank you for the suggestions SUbha and CycLone. I will try to lengthen my outlet and hope it resolves this problem.

[shubham jain]

hi, i am simulating a Brush seal using Porous medium approach in CFX.

My inlet (INLET) and outlet (OPENING) channels are very long. Cfx says that wall is placed at a portion of Inlet, then it stops the simulation.

However, when i see the streamlines, circulation was only at the outlet , not inlet.
Though the problem was solved by shortening the inlet as well as outlet channels, so that no circulation is coming at outlet. But i could not understand, why the shortening of channel length makes it (wall places at INLET) better??

Picture attached: Green region in right is inlet.... Dark yellow in the middle is the porous medium ..... light yellow in the left is outlet
FLOW DIRECTION IS FROM RIGHT TO LEFT

Thanks in advance

[marco.ian]

http://www.arc.vt.edu/ansys_help/cfx_mod/i5500692.html

Here is the explanation!

[shubham jain]

thanks for the link... But that does not answer why the shortening of the channel length makes the wall placed at the inlet dissappear.

Also in recent simulations, i have noticed that for some high pressure drops, 100% wall is placed at the inlet. But when I decrease the temperature form the actual working conditions, it works.
This is also a little confusing for me.

[ahmedrezk82]

Hi

It is great information. I have the same problem in the first few iterations, then disappeared and the simulation continue with good conversion rate. I am simulating turbine flow, and I am confident that the outlet section is long enough, would extending the inlet section solve the problem.

Originally Posted by CycLone
;85459

Hi Melvin,

Look at your flow field and pay attention to the % of the outlet area that is walled off (reported in the warning). The solver does this to prevent reverse flow, which you clearly don't want if you specified an outlet (otherwise you would have defined an opening, right?).

If the % area is small, it may not have a significant effect on your solution. If it is large, you should investigate the flow in the vicinity of the outlet. Try seeding streamlines from the outlet to see the reverse flow region, for instance.

In the end, you may have to extend your model to include more geometry downstream or change the boundary condition to more accurately represent what is occurring at this location. For instance, if you set an average static pressure but the flow dumps into a plenum beyond the outlet, a constant static pressure may be more appropriate. Similarly, if it is a mass flow specified outlet, set the pressure profile at the outlet to a constant value (which enforces a constant static pressure across your outlet which achieving the desired mass flow).

The key is to understand the physics and act accordingly.

-CycLone

[ghorrocks]

If the warning disappears after a while and convergence is good then you have nothing to worry about. The simulation just needed to sort itself out a bit and proceeded to converge well from there.

[ahmedrezk82]

Thanks a lot ghorrocks.

[ecsmech]

how to eliminate this issue??

[ghorrocks]

FAQ: https://www.cfd-online.com/Wiki/Ansy...f_an_OUTLET.22