# Variable RMS Value fluctuating but not converging.

 Register Blogs Members List Search Today's Posts Mark Forums Read

December 20, 2016, 18:56
Variable RMS Value fluctuating but not converging.
#1
New Member

Join Date: Dec 2016
Posts: 8
Rep Power: 2
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!
Attached Images
 1.PNG (65.7 KB, 15 views)

 December 21, 2016, 05:12 #2 Senior Member   Lance Join Date: Mar 2009 Posts: 615 Rep Power: 15 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 New Member   Jaydeep Koradiya Join Date: Dec 2016 Posts: 8 Rep Power: 2 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, 07:09 #4 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,589 Rep Power: 25 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. __________________ Please do not send me CFD-related questions via PM

December 21, 2016, 07:12
#5
Senior Member

Join Date: Feb 2011
Posts: 460
Rep Power: 11
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.

 December 21, 2016, 07:39 #6 New Member   Jaydeep Koradiya Join Date: Dec 2016 Posts: 8 Rep Power: 2 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, 07:41
#7
Senior Member

Lance
Join Date: Mar 2009
Posts: 615
Rep Power: 15
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.

 December 21, 2016, 07:58 #8 New Member   Jaydeep Koradiya Join Date: Dec 2016 Posts: 8 Rep Power: 2 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 Senior Member   Lance Join Date: Mar 2009 Posts: 615 Rep Power: 15 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 Senior Member   Join Date: Jun 2009 Posts: 701 Rep Power: 15 Create an interruption control using a logical expression along the lines of probe(ExpressionValue.Standard Deviation)@MyMonitorExpression < MyToleranceValue Please check documentation for accurate syntax

 December 21, 2016, 14:00 #11 Senior Member   Join Date: Feb 2011 Posts: 460 Rep Power: 11 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.

January 16, 2017, 09:19
#12
Member

Alex
Join Date: Feb 2016
Posts: 79
Rep Power: 3
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?

 January 16, 2017, 09:43 #13 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,589 Rep Power: 25 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. __________________ Please do not send me CFD-related questions via PM

 January 16, 2017, 21:58 #14 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,991 Rep Power: 107 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?

 Tags cfx 17.1, converge, residuals

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post redza010 CFX 1 August 3, 2012 08:54 charlotte CFX 4 March 22, 2011 10:14 bhushas Main CFD Forum 1 May 30, 2008 04:35 gruber2 OpenFOAM Installation 5 December 30, 2005 05:27 lego CFX 3 November 5, 2002 21:09

All times are GMT -4. The time now is 00:50.