Variable RMS Value fluctuating but not converging.

Jaydeep_Koradiya · December 20, 2016, 18:56

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

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

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

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?

December 21, 2016, 07:09		#4
flotus1 Super Moderator Alex Join Date: Jun 2012 Location: Germany Posts: 3,427 Rep Power: 49	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. Fabio_Teixeira likes this.

December 21, 2016, 14:00		#11
Antanas Senior Member Join Date: Feb 2011 Posts: 496 Rep Power: 18	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 Fabio_Teixeira likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Graph of RMS residue not converging	redza010	CFX	1	August 3, 2012 09:54
emag beta feature: charge density	charlotte	CFX	4	March 22, 2011 10:14
error in COMSOL:'ERROR:6164 Duplicate Variable'	bhushas	COMSOL	1	May 30, 2008 05:35
Env variable not set	gruber2	OpenFOAM Installation	5	December 30, 2005 05:27
Replace periodic by inlet-outlet pair	lego	CFX	3	November 5, 2002 21:09

December 21, 2016, 05:12		#2
Lance Senior Member Lance Join Date: Mar 2009 Posts: 669 Rep Power: 22	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.

December 21, 2016, 06:54		#3
Jaydeep_Koradiya New Member Jaydeep Koradiya Join Date: Dec 2016 Posts: 8 Rep Power: 9	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

December 21, 2016, 07:39		#6
Jaydeep_Koradiya New Member Jaydeep Koradiya Join Date: Dec 2016 Posts: 8 Rep Power: 9	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.

December 21, 2016, 07:58		#8
Jaydeep_Koradiya New Member Jaydeep Koradiya Join Date: Dec 2016 Posts: 8 Rep Power: 9	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.

December 21, 2016, 08:22		#9
Lance Senior Member Lance Join Date: Mar 2009 Posts: 669 Rep Power: 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.

December 21, 2016, 09:53		#10
Opaque Senior Member Join Date: Jun 2009 Posts: 1,873 Rep Power: 33	Create an interruption control using a logical expression along the lines of probe(ExpressionValue.Standard Deviation)@MyMonitorExpression < MyToleranceValue Please check documentation for accurate syntax

January 16, 2017, 09:43		#13
flotus1 Super Moderator Alex Join Date: Jun 2012 Location: Germany Posts: 3,427 Rep Power: 49	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.

January 16, 2017, 21:58		#14
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	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?