[shshbly]

Hello ,
I'm modeling a flow through a 2-D channel with a rectangular bluff-body of

Channel Diameter = 25 mm
Bluff body Diameter = 5 mm
Velocity inlet of cold flow = 1.6 m/s
Outlet is set outflow

I intend to get a steady profile of velocity and pressure as starting conditions for other calculation.

The "viscous-laminar" model is turned on, and used air with constant density. Pressure-velocity coupled scheme is selected.

However , the residual of continuity does not converge after even 10000 iterations. And the velocity magnitude and the pressure profile seems asymmetric. the results change little after the first several hundreds iterations.

convergence criteria for continuity, x,y,z velocity = 1e-3.

Any help or views on this would be greatly appreciated. Thanks!

[ghost82]

The problem here could be that your system is implicitly unsteady, so the continuity residual doesn't decrease.
The profile is not symmetric because it continues to change, this steady solution should be just a screenshot of an unsteady case.
I suggest to switch from this result to unsteady simulation: I'm quite sure you will obtain convergence of continuity too.

[shshbly]

Thank you.
But even for an unsteady case, it is expected to get a time-averaged profile with the steady solver, right?
As can be seen from the pics, the pressure and velocity magnitude profile is some what time-averaged, though not exactly symmetric yet.

[shshbly]

Thank you.
But even for an unsteady case, it is expected to get a time-averaged profile with the steady solver, right?
As can be seen from the pics, the pressure and velocity magnitude profile is some what time-averaged, though not exactly symmetric yet.

Originally Posted by ghost82

The problem here could be that your system is implicitly unsteady, so the continuity residual doesn't decrease.
The profile is not symmetric because it continues to change, this steady solution should be just a screenshot of an unsteady case.
I suggest to switch from this result to unsteady simulation: I'm quite sure you will obtain convergence of continuity too.

[ghost82]

As I know, the steady solver solves for a steady solution: if the system physically doesn't reach a steady solution the solver can't converge.
If you want a "steady solution" you should perform unsteady simulation and then get average-time profiles of what you want in post processing.

[AHF]

well first thing you have to do is that increase the diameter of channel , 25mm is small for it , increase up to 50mm

after that you should check your reynolds number , i think it is not laminar

and also this problem is unsteady
pay attention to time step to get correct converge

[shshbly]

Thank you.
The geometry may not be changed.
The Re based on the bluff body diameter is 500, and 2500 for the channel diameter. But upstream of the bluff body, the flow has fully developed.

You also think that a transient solver should be applied?

Originally Posted by AHF

well first thing you have to do is that increase the diameter of channel , 25mm is small for it , increase up to 50mm

after that you should check your reynolds number , i think it is not laminar

and also this problem is unsteady
pay attention to time step to get correct converge

[AHF]

Originally Posted by shshbly

Thank you.
The geometry may not be changed.
The Re based on the bluff body diameter is 500, and 2500 for the channel diameter. But upstream of the bluff body, the flow has fully developed.

You also think that a transient solver should be applied?

for a flow around a cylinder , it's become turbulent in Re > 90 , and i think this case with Re=500 is unsteady

i am sure about geometry that should be increase , diameter 25 is not enough for this problem

[LuckyTran]

Originally Posted by shshbly

Thank you.
But even for an unsteady case, it is expected to get a time-averaged profile with the steady solver, right?
As can be seen from the pics, the pressure and velocity magnitude profile is some what time-averaged, though not exactly symmetric yet.

There's no guarantee that a steady-state solver will converge to the time-averaged solution of an unsteady problem. If your problem is implicitly unsteady (or even worse explicitly unsteady) then your solution at different iterations of a steady state solver can still oscillate. In this case it's best to use an unsteady solver.

[hotboy]

Originally Posted by LuckyTran

There's no guarantee that a steady-state solver will converge to the time-averaged solution of an unsteady problem. If your problem is implicitly unsteady (or even worse explicitly unsteady) then your solution at different iterations of a steady state solver can still oscillate. In this case it's best to use an unsteady solver.

Hello LuckyTran!
What's the difference of implicitly unsteady and explicitly unsteady?

[Sai Krishna]

Originally Posted by ghost82

The problem here could be that your system is implicitly unsteady, so the continuity residual doesn't decrease.
The profile is not symmetric because it continues to change, this steady solution should be just a screenshot of an unsteady case.
I suggest to switch from this result to unsteady simulation: I'm quite sure you will obtain convergence of continuity too.

sorry for reopening the old post.
iam facing same issue with residuals not getting converged. iam doing conjugate heat transfer analysis for the external flow over my model using steady state formulation. i created monitors for temperature @ locations where re circulation happens and other important parts. those values are completely stable(constant). Net mass flow rate from fluxes also converged fully. But the residuals are oscillating about a particular value.
continuity @ 10e-1, k and w @ 10e-4, all velocities and energy @10e-6.

u told about implicitly unsteady system for which we cant get residual convergence with steady simulation, what does it actually mean?
i know its depends on physics of the problem, but how to identify it in the beginning?
if its known in the beginning, we can go ahead with transient simulation right?
can there be a system which doesnt reach physically steady state?
I believe even in compressible high speed flows will have some unsteady behavior and perturbations in the beginning and reaches steady state in due course.

Thanks for your answers