CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Variable RMS Value fluctuating but not converging. (https://www.cfd-online.com/Forums/cfx/181768-variable-rms-value-fluctuating-but-not-converging.html)

Jaydeep_Koradiya December 20, 2016 18:56

Variable RMS Value fluctuating but not converging.
 
1 Attachment(s)
Hello, Everyone!
I am trying to simulate the 2D-flow around the cylinder with area blockage 0.01% in CFX (Structured Mesh). The Reynolds number is 0.5 Million. The boundary conditions I have is:

Inlet : velocity (55.55 m/s)
Outlet: static Pressure (0 atm)
cylinder: wall (no-slip)
farsides: wall (free-slip)
sides: Symmetric Boundary conditions

reference Pressure is the default 1 atm.
Turbulence model: SST
Time step: Physical time steps (0.0001 s)
convergence criteria: 1e-6



The RMS values are fluctuating horizontally and not even close to convergence even after 3000 iterations.

I need some advice to fix this problem. Thank you in advance!

Lance December 21, 2016 05:12

Since you wrote "Time step: Physical time steps (0.0001 s)" and you have periodic fluctuations in the residuals Im guessing you are running steady-state simulation where vortex shedding appears? Try a transient simulation instead.

Jaydeep_Koradiya December 21, 2016 06:54

Hello Lance, Thank you for the reply.

Yes, I am using steady state analysis because I want to find the mean drag force acting on the cylinder and there is vortex shedding in my case. Will I be able to calculate mean drag if I use transient simulation ?

Thank you

flotus1 December 21, 2016 07:09

Your best chance for getting a converged steady-state solution in this case is by cutting your model in half and using a symmetry boundary condition. This will eliminate the large fluctuations from the vortex shedding without altering the solution from a RANS point of view.
If this still fails your only option is what Lance just wrote.

Antanas December 21, 2016 07:12

Quote:

Originally Posted by Jaydeep_Koradiya (Post 630743)
Hello Lance, Thank you for the reply.

Yes, I am using steady state analysis because I want to find the mean drag force acting on the cylinder and there is vortex shedding in my case. Will I be able to calculate mean drag if I use transient simulation ?

Thank you

Because vortex shedding is in fact transient and you use steady state solver, residuals oscillate. IMO if you're not interested in transient behaviour, it is not necessary to use transient solver. You should monitor drag force and when it stops changing you can stop solver. It will be your solution.

Jaydeep_Koradiya December 21, 2016 07:39

But due to vortex shedding, will not be any fluctuations in drag force too? I am following your approach but I see the drag plot line fluctuating too.

Lance December 21, 2016 07:41

Quote:

Originally Posted by Jaydeep_Koradiya (Post 630756)
But due to vortex shedding, will not be any fluctuations in drag force too? I am following your approach but I see the drag plot line fluctuating too.

Of course. Make a time-average.

Jaydeep_Koradiya December 21, 2016 07:58

Thank you, Could you please suggest if there is way in convergence criteria to monitor the time average of drag force (Normal force on cylinder (x))?

I would like to make it my convergence criteria.

Lance December 21, 2016 08:22

See "21.1.5.1.8.8. [Monitor Name]: Monitor Statistics" in the cfx-pre manual.
Make an expression on drag force, monitor the standard deviation over a certain time. Im not sure you can make CFX stop when the standard deviation is less than a threshold, but you can at least monitor it.

Opaque December 21, 2016 09:53

Create an interruption control using a logical expression along the lines of

probe(ExpressionValue.Standard Deviation)@MyMonitorExpression < MyToleranceValue

Please check documentation for accurate syntax

Antanas December 21, 2016 14:00

Ansys posted video on its youtube channel about it. Here is the link:
ANSYS CFX: Using Derived Variables and Monitor Statistics to Set Up an interrupt Control

Red Ember January 16, 2017 09:19

Quote:

Originally Posted by Jaydeep_Koradiya (Post 630643)
Hello, Everyone!
I am trying to simulate the 2D-flow around the cylinder with area blockage 0.01% in CFX...

Sorry to bother... Is it possible to simulate 2D-flow in CFX already?

flotus1 January 16, 2017 09:43

Only pseudo-2D with a volume mesh and a thickness of 1 cell. Fluent on the other hand has real 2D solvers. I don't think that a 2D solver will be added to CFX any time soon.

ghorrocks January 16, 2017 21:58

FAQ: https://www.cfd-online.com/Wiki/Ansy..._simulation.3F

With ANSYS AIM coming along there is no chance CFX will get real 2D simulations. I have not looked at ANSYS AIM in detail - can it do 2D simulations?


All times are GMT -4. The time now is 19:01.