CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Residuals of continuity not converging

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

Like Tree2Likes
  • 2 Post By hotboy

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 12, 2015, 06:06
Question Residuals of continuity not converging
  #1
New Member
 
Ren Zetian
Join Date: Sep 2015
Posts: 5
Rep Power: 8
shshbly is on a distinguished road
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!



Attached Images
File Type: jpg 1-Scaled residual.jpg (37.3 KB, 2104 views)
File Type: jpg 5-Total pressure.jpg (46.3 KB, 1991 views)
File Type: jpg 6-Velocity magnitude.jpg (48.4 KB, 1978 views)
shshbly is offline   Reply With Quote

Old   September 12, 2015, 06:44
Default
  #2
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 1,016
Rep Power: 24
ghost82 will become famous soon enough
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.
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   September 12, 2015, 06:55
Default
  #3
New Member
 
Ren Zetian
Join Date: Sep 2015
Posts: 5
Rep Power: 8
shshbly is on a distinguished road
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 is offline   Reply With Quote

Old   September 12, 2015, 06:56
Default
  #4
New Member
 
Ren Zetian
Join Date: Sep 2015
Posts: 5
Rep Power: 8
shshbly is on a distinguished road
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.

Quote:
Originally Posted by ghost82 View Post
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 is offline   Reply With Quote

Old   September 12, 2015, 06:58
Default
  #5
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 1,016
Rep Power: 24
ghost82 will become famous soon enough
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.
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   September 12, 2015, 15:16
Wink
  #6
AHF
Member
 
AHF's Avatar
 
amirhossein
Join Date: Jul 2014
Location: iran
Posts: 81
Rep Power: 9
AHF is on a distinguished road
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 is offline   Reply With Quote

Old   September 12, 2015, 23:21
Default
  #7
New Member
 
Ren Zetian
Join Date: Sep 2015
Posts: 5
Rep Power: 8
shshbly is on a distinguished road
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?

Quote:
Originally Posted by AHF View Post
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 is offline   Reply With Quote

Old   September 13, 2015, 03:41
Default
  #8
AHF
Member
 
AHF's Avatar
 
amirhossein
Join Date: Jul 2014
Location: iran
Posts: 81
Rep Power: 9
AHF is on a distinguished road
Quote:
Originally Posted by shshbly View Post
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
AHF is offline   Reply With Quote

Old   September 16, 2015, 00:26
Default
  #9
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,585
Rep Power: 53
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by shshbly View Post
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.
LuckyTran is online now   Reply With Quote

Old   October 5, 2015, 10:27
Default
  #10
Member
 
wanghuo
Join Date: Aug 2014
Posts: 89
Rep Power: 9
hotboy is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
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?
dexter and Sai Krishna like this.
hotboy is offline   Reply With Quote

Old   September 9, 2020, 11:12
Default
  #11
Member
 
Sai Krishna
Join Date: May 2018
Posts: 33
Rep Power: 5
Sai Krishna is on a distinguished road
Quote:
Originally Posted by ghost82 View Post
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
Attached Images
File Type: jpg net mass flow rate.jpg (77.7 KB, 54 views)
File Type: jpg imp-temperature.jpg (85.5 KB, 47 views)
File Type: jpg residuals.jpg (95.2 KB, 52 views)
Sai Krishna is offline   Reply With Quote

Reply

Tags
continuity, converge

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Help for the small implementation in turbulence model shipman OpenFOAM Programming & Development 25 March 19, 2014 11:08
Micro Scale Pore, icoFoam gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 14:58
AMI interDyMFoam for mixer nu problem danny123 OpenFOAM Programming & Development 8 September 6, 2013 03:34
dynamic Mesh is faster than MRF???? sharonyue OpenFOAM Running, Solving & CFD 14 August 26, 2013 08:47
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09


All times are GMT -4. The time now is 22:18.