Residuals never converge!
 

Hello friend,
I'm a chemical engineer and I'm trying to model the following problem:
air firstly flowing in a pipe duct and then , when it exits from the duct, it flows around a cylinder. This is the scheme:http://imagizer.imageshack.us/a/img538/6020/SvUHVs.jpg
This is the mesh I've done, simplifying the problem for its geometry as axysimmetryc :


http://imageshack.com/a/img540/3598/niR1Pa.jpg

The walls of the pipe duct are adiabatic. Air has got a temperature of 373 K while the whole system has got a temperature of 298 K . The boundary conditions are the following:
PRESSURE OUTLET for the external part of the domain
for the air entering the duct: VELOCITY INLET, with the relative magnitude and axial component of the flow direction =1, the radial 0. Furthermore the Inlet temperature is 373 K.
The walls of the duct are ADIABATIC, while the cylinder at the exit of the pipe duct has got a HEAT FLUX coupled with the air.
The problem is that as soon as the simulation starts, the residual oscillate a lot also when FLUENT reaches 100000 iteration. I set the problem as unsteady, with 0.01 as time step size . The oscillation are these:http://imagizer.imageshack.us/a/img538/8004/tFd2fX.jpg
What I can do to reach the convergence?? Thanks to everybody! This simulation is my nightmare!!

Hi Giulia,
I think there's nothing wrong in convergence: when you set an unsteady simulation, convergence is reached for each time step: you can see from your residual chart; at the beginning of each timestep you have "high" residual value, then during iteration residual values decrease and reach convergence for that timestep; this is repeated for each timestep.

PS : what I've noticed is that leaving properties such as density,viscosity and specific heat not in polynomial form (a0 + a1T + a2 T^2......) but costant (with the default vaules in FLUENT) the residual seems not to oscillate but they decrease... http://imagizer.imageshack.us/a/img661/6876/ERSNhx.jpg

but If there is a heat exchange between air at 373 K and the pipe duct and the cylinder at 298 K it is a mistake leaving thermal properties constant?

If you noticed "flat" residuals in an unsteady simulation probably it means you reached a steady state solution.

Excuse me but this is the first time I do an unsteady simulation: why this is repeated for each timestep? So how I can realize if I have reached convergence? Maybe I have to use a smaller time step?

In a steady state simulation you have to reach convergence for the steady state; you can think the steady simulation as a single time step.
You have a single solution for the steady state.

In an unsteady simulation solution changes for each time step, because the solution changes vs. time.
You have multiple solutions, one for each time step, and you have to reach convergence for each time step.

See also attached picture.

Daniele

Thank you! So,despite the oscillation, I reach the convergence when in a single time step residuals reach the value previously fixed , for example 10^-6 ?

Correct :)
Oscillation is quite usual in unsteady simulations: this means that for each time step the solution is changing with time, so the problem is unsteady.
If after some time residuals will be "flat" (horizontal) that means that solution is not changing anymore with time, and you reached a steady state solution by simulating the unsteady problem.

Thank you!!

But how to evaluate convergence? For example monitoring coefficien drag value and determinating the time when it reaches a constant value?

Yes, for example.
Use the same criteria as the steady state approach: only difference is that your convergence criteria must be reached at each time step.

another question: the walls of the pipe duct are adiabatic , but in fluent in addiction to the wall of the duct there is its shadow too. So, how to assignate the adiabaticity boundary condition? Both wall and shadow wall are adiabatic or the wall is adiabatic while for its shadow I must set coupled boundary condition????

Set both walls to adiabatic (it should be automatically set for the shadow when you set for wall, however check both walls and set them to zero heat flux).

thank you!!

Hello friends,
my problem now is that when I'm running the simulation Fluent sends an error messages: "reversed flow in faces XXX on outflow 4". Here's a picture of the mesh for the problem and the boundary condition..
http://imageshack.com/a/img910/9470/wth6xE.jpg


This is velocity profile at the current time of the simulation:
http://imageshack.com/a/img673/5927/xYor7k.jpg

and this is pressure profile...
http://imageshack.com/a/img905/7757/AfAzWK.jpg
and temperature:
http://imageshack.com/a/img661/1558/jdahli.jpg
So, what cause this reverse flow??

If I were you I didn't care too much for this warning.
Reversed flow means that fluid is flowing in your domain from your outflow: this could be related to recirculation, which can be quite common.
This warning could also disappear after some time steps.
Just make sure to correctly set your backflow boundary condition (temperature for example): these are estimates you set in the boundary condition panel.
Moreover, if you are interested in the flow near the cylinder, if your outlet is far enough, what happens at the outlet should not interfere too much there.

I'm sorry: what do you mean for backflow boundary condition?

Here is an example of backflow total temperature panel (it is an outlet boundary condition): this means that if fluid enters the domain from the outlet (reversed-flow) it will enter with a temperature of 288 K.

http://www.arc.vt.edu/ansys_help/flu...n_pressout.png

Just one thing: I see now that you set an outflow boundary condition: outflow means that the fluid is fully developed: are you sure is it fully developed?
If you have recirculations, and these recirculations are real, then your fluid is not fully developed and you should set a pressure outlet boundary condition.

yesterday i put a pressure outlet as a boundary condition but my prof. suggested me to change into outflow... but also pressure outlet gave me a reversed flow..