CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Variable RMS Value fluctuating but not converging.

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

Like Tree2Likes
  • 1 Post By flotus1
  • 1 Post By Antanas

Reply
 
LinkBack Thread Tools Display Modes
Old   December 20, 2016, 18:56
Default Variable RMS Value fluctuating but not converging.
  #1
New Member
 
Jaydeep Koradiya
Join Date: Dec 2016
Posts: 8
Rep Power: 2
Jaydeep_Koradiya is on a distinguished road
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
File Type: png 1.PNG (65.7 KB, 15 views)
Jaydeep_Koradiya is offline   Reply With Quote

Old   December 21, 2016, 05:12
Default
  #2
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 615
Rep Power: 15
Lance is on a distinguished road
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.
Lance is offline   Reply With Quote

Old   December 21, 2016, 06:54
Default
  #3
New Member
 
Jaydeep Koradiya
Join Date: Dec 2016
Posts: 8
Rep Power: 2
Jaydeep_Koradiya is on a distinguished road
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
Jaydeep_Koradiya is offline   Reply With Quote

Old   December 21, 2016, 07:09
Default
  #4
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,589
Rep Power: 25
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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
flotus1 is offline   Reply With Quote

Old   December 21, 2016, 07:12
Default
  #5
Senior Member
 
Join Date: Feb 2011
Posts: 460
Rep Power: 11
Antanas is on a distinguished road
Quote:
Originally Posted by Jaydeep_Koradiya View Post
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.
Antanas is offline   Reply With Quote

Old   December 21, 2016, 07:39
Default
  #6
New Member
 
Jaydeep Koradiya
Join Date: Dec 2016
Posts: 8
Rep Power: 2
Jaydeep_Koradiya is on a distinguished road
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.
Jaydeep_Koradiya is offline   Reply With Quote

Old   December 21, 2016, 07:41
Default
  #7
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 615
Rep Power: 15
Lance is on a distinguished road
Quote:
Originally Posted by Jaydeep_Koradiya View Post
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.
Lance is offline   Reply With Quote

Old   December 21, 2016, 07:58
Default
  #8
New Member
 
Jaydeep Koradiya
Join Date: Dec 2016
Posts: 8
Rep Power: 2
Jaydeep_Koradiya is on a distinguished road
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.
Jaydeep_Koradiya is offline   Reply With Quote

Old   December 21, 2016, 08:22
Default
  #9
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 615
Rep Power: 15
Lance is on a distinguished road
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.
Lance is offline   Reply With Quote

Old   December 21, 2016, 09:53
Default
  #10
Senior Member
 
Join Date: Jun 2009
Posts: 701
Rep Power: 15
Opaque is on a distinguished road
Create an interruption control using a logical expression along the lines of

probe(ExpressionValue.Standard Deviation)@MyMonitorExpression < MyToleranceValue

Please check documentation for accurate syntax
Opaque is offline   Reply With Quote

Old   December 21, 2016, 14:00
Default
  #11
Senior Member
 
Join Date: Feb 2011
Posts: 460
Rep Power: 11
Antanas is on a distinguished road
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.
Antanas is offline   Reply With Quote

Old   January 16, 2017, 09:19
Default
  #12
Member
 
Alex
Join Date: Feb 2016
Posts: 79
Rep Power: 3
Red Ember is on a distinguished road
Quote:
Originally Posted by Jaydeep_Koradiya View Post
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?
Red Ember is offline   Reply With Quote

Old   January 16, 2017, 09:43
Default
  #13
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,589
Rep Power: 25
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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
flotus1 is offline   Reply With Quote

Old   January 16, 2017, 21:58
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,991
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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?
ghorrocks is offline   Reply With Quote

Reply

Tags
cfx 17.1, converge, residuals

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Graph of RMS residue not converging redza010 CFX 1 August 3, 2012 08:54
emag beta feature: charge density charlotte CFX 4 March 22, 2011 10:14
error in COMSOL:'ERROR:6164 Duplicate Variable' bhushas Main CFD Forum 1 May 30, 2008 04:35
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


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