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

Laminar doesn't converge; Turbulent models do?

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

Like Tree1Likes
  • 1 Post By razvan

Reply
 
LinkBack Thread Tools Display Modes
Old   September 27, 2006, 17:45
Default Laminar doesn't converge; Turbulent models do?
  #1
Amit
Guest
 
Posts: n/a
I'm running a pretty standard 2-D axisymmetric model which involves a pretty sharp and severe constriction (a larynx model), causing a jet and some backflow. When I run the model with any of several turbulent viscous models-- S-A/ RKE/ KWSST/ Reynold's Stress-- it converges, at least to a reasonable scaled amount (1e-4 -- 1e-8) .

When I run the laminar model for comparison, it completely fails to converge. Often times, it converges to 1 e-1, (overally continuity) and then begins to diverge, to some other very high value, before stabilizing. It never completely converges.

Given that the turbulent models converge, I'm confused as to why the laminar model does not. I've tried adding reasonable boundary layers, switching to second order solvers, and increasing my grid definition-- and some of these techniques have helped a little, but the overall problem of the laminar model continues. I'm thinking maybe the fact that there are interior boundary layers (from the backflow cells) could be causing some resolution issues in the laminar case.

Is there anything I can do to force my laminar model to converge in the same manner as the turbulent models do? I really need the laminar as a standard of comparison for turbulent data-- my flow is really somewhere in between.

  Reply With Quote

Old   September 28, 2006, 04:02
Default Re: Laminar doesn't converge; Turbulent models do?
  #2
razvan
Guest
 
Posts: n/a
The only way to deal with laminar simulations that do not converge using standard approach (steady solver), is to switch to unsteady formulation and run it until settling down. I personally ran into this problem many times by now and this has been a fail-proof method. Of course, this means some significant more computational effort, but be patient. The explanation for this behavior of the laminar solver is the fact that the laminar regime N-S equations are not time-averaged, so whenever a strong unsteady phenomena appears in a model, it's beeing felt immediately. Try for example to simulate Re=200 circular cylinder flow with the steady solver. Vortex shedding will never permit it to converge. The reason is simply phisical.

All the best, Razvan
juliom likes this.
  Reply With Quote

Old   September 28, 2006, 04:27
Default Re: Laminar doesn't converge; Turbulent models do?
  #3
zxaar
Guest
 
Posts: n/a
switch from outflow boundary to pressure outlet, and it will not diverge.
  Reply With Quote

Old   September 28, 2006, 08:21
Default Re: Laminar doesn't converge; Turbulent models do?
  #4
Amit
Guest
 
Posts: n/a
Thanks for the suggestions. Zxaar, as to the pressure outflow, I'll try that now.

Razvan, when you say that I should use the unsteady solver, what kind of settings should do you suggest I use (time step length, total time steps, iterations per time step, etc)?

  Reply With Quote

Old   September 28, 2006, 14:00
Default Re: Laminar doesn't converge; Turbulent models do?
  #5
sarah_ron
Guest
 
Posts: n/a
I don't think zxaar method will fix the divergence problem. I have met the similar case and I totally agree with razvan opinions. It is the underlying physics, not numerical issues. Just my opinion.
  Reply With Quote

Old   September 28, 2006, 15:14
Default Re: Laminar doesn't converge; Turbulent models do?
  #6
Jason
Guest
 
Posts: n/a
Well it all depends on the problem. It's a common mistake to use an outflow BC that's too close to geometry changes and this can cause the model to fall apart. The assumptions behind the outflow BC are pretty limiting (same thing with the Pressure-Far-Field... I know that's off topic, but you routinely see the Outflow and the PFF BCs misused on this forum). And sometimes the Outflow BC simply fails, even if the "fully developed" assumption is applicable. The Outflow BC will definitely fail if there is transient information being passed down stream in a steady state solver. And when I say it fails, I mean it can further excite the upstream effects by artificially back pressuring the system and such. If the "fully developed" solution doesn't work where the BC is applied, the Outflow BC will tend to magnify the problem.

I think Zxaar approached it from looking at what are the common mistakes, and misusing BCs in Fluent are pretty common. Razvan looked at it from a POV assuming that the setup was correct. We really don't know either way. Personally I would try Zxaar's response first (it's easier). Then if that doesn't work, I'd try Razvan's response. Both responses are valuable though.

IMHO of course.

Jason
  Reply With Quote

Old   September 28, 2006, 19:02
Default Re: Laminar doesn't converge; Turbulent models do?
  #7
zxaar
Guest
 
Posts: n/a
To add to what Jason said, the problem with using outflow boundary is, unablility to force continuity when the flow enters through the outlet boundary. Usually to match the inlet flow, outflow velocities are multiplied by a factor. Now if the flow enters this could lead to unstablity. To avoid this what Fluent does is, when the flow enters the outflow, it does not enforce total continutiy (in flow = outflow). (According to their manual, the mass flux in such cases is floating or not defined). so when the flow enters and if you are not enforcing continuty, there may be cases where it diverges.

When you are using, pressure outlet, the continuity is applied in terms of pressure and hence the flow direction at outlet won't effect the stablity of solution. (this is why I said switch to pressure outlet).

  Reply With Quote

Old   September 28, 2006, 19:06
Default Re: Laminar doesn't converge; Turbulent models do?
  #8
zxaar
Guest
 
Posts: n/a
I have met the similar case and I totally agree with razvan opinions.

First one persons personal experience does not necessarily applyu to every body. For example, I have never had any subsonic case diverged with Fluent. (it does not mean you can not have divereged case with fluent.

As far as getting steady solution by unsteady procedure (incompressible pressure based), could be problematic in some case. For example, flow behind a cylinder, where you have vortices. (waiting for a unique profile in such cases seems very bad idea).

It is the underlying physics, not numerical issues

It may very well be numerical issue, stablity in steady solver could be difficult. And boundary conditions play big role in it.
  Reply With Quote

Old   September 28, 2006, 20:00
Default Re: Laminar doesn't converge; Turbulent models do?
  #9
Roth
Guest
 
Posts: n/a
Compare the size of the turbulent viscosity to the constant laminar viscosity value.
  Reply With Quote

Old   September 29, 2006, 09:02
Default Re: Laminar doesn't converge; Turbulent models do?
  #10
Amit
Guest
 
Posts: n/a
Thanks for all the feedback--

Now, is there a way to use the pressure outlet BC without having to specify a species concentration? For example, I'm trying to run a species balance with flow-- and the standard outflow allows me to leave the outlet concentration unspecified (allowing the solver to calculate it). Is there any way to do the same with the pressure outlet? Every time I use pressure outlet, I'm forced to specify the outflow concentration.
  Reply With Quote

Old   October 26, 2011, 01:12
Default
  #11
New Member
 
satyendra
Join Date: Jun 2010
Posts: 15
Rep Power: 7
satyendra is on a distinguished road
hi zxaar,

i am trying to solve an incompressible ideal gas problem having two mass flow inlet conditions and two pressure outlet conditions ( i cannot use outflow BC since according to chapter 7, fluent user guide this is not allowed ). hence I have set target mass flow at outlet. But the continuity is not converging. any idea where i am going wrong.

rana
satyendra is offline   Reply With Quote

Old   April 23, 2015, 22:55
Default
  #12
Member
 
sanjeet Limbu
Join Date: Mar 2015
Posts: 91
Rep Power: 2
sanjeetlimbu is on a distinguished road
Dear Sir I am trying to do laminar - species transport model

As I tried RNG viscous model- it donot give complete temperature graph.

Please suggest how to set up the laminar - model for combustion using the fluent-chemkin file for four species- N2/AR/Nc6H17/O2
I am compressing the volume by piston in 30 ms and expecting temp to rise above 766K, as I see that Temp donot rise even as piston moves and Pressure rise fro 25-30ms
Attached Images
File Type: jpg error during run.jpg (42.6 KB, 11 views)
File Type: jpg Temp only 550K_No comb@40ms.jpg (34.7 KB, 9 views)
sanjeetlimbu is offline   Reply With Quote

Reply

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
Two-equation turbulent models: low re airfoils truffaldino Main CFD Forum 51 March 19, 2012 19:57
effective? turbulent? laminar? viscosity MIssNancy FLUENT 3 December 3, 2002 00:53
effective? turbulent? laminar? MissNancy Main CFD Forum 2 November 30, 2002 02:08
Laminar vs. Turbulent Models Dahvid Brown FLUENT 3 October 23, 2000 02:36


All times are GMT -4. The time now is 23:51.