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

High Continuity Residual for 3D problem

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

Like Tree3Likes
  • 1 Post By John C. Chien
  • 1 Post By Rüdiger Schwarze
  • 1 Post By Gearoid Lydon

Reply
 
LinkBack Thread Tools Display Modes
Old   July 24, 2000, 11:02
Default High Continuity Residual for 3D problem
  #1
Gearoid Lydon
Guest
 
Posts: n/a
Problem:

1. I am working on a 3-D model of a BR710 aircraft nacelle using Fluent 5.3. The area modeled is the "Zone 1" or the Fan Compartment. The zone consists of two air inlets, a pressure outlet and a propane leak source. The aim is to achieve a steady state model of air and propane in the zone.

2. The solver used is the segregated Implicit at steady state.

3. The viscous model is k-epsilon, RNG.

4. The species model is used to define the propane.

5. I used a discretization of Standard for Pressure, Simple for Pressure-Velocity Coupling and Power Law for all others.

6. I have run the job making adjustments to the under-relaxation factors of pressure and momentum. However, I have been unable to get the continuity residual below 0.001.

Questions:

1. Do the Pressure and Momentum under-relaxation factors have to be adjusted together(i.e. when one is increased does the other have to be decreased)?

2. Is there any other adjustment I could make to improve the convergence of the continuity residual?

Gearoid Lydon

QUB

Belfast
  Reply With Quote

Old   July 26, 2000, 00:46
Default Re: High Continuity Residual for 3D problem
  #2
John C. Chien
Guest
 
Posts: n/a
(1). I can only say that 99% of the time, I am getting the wrong answers, with the commercial cfd codes. (2). I must also say that I am dealing with complex 3-D problems which requires complex meshes. (3). Recently, I found out that even if the geometry is simple, the convergence is still a big issue. This is because of the multi-block mesh used. In other words, the mesh topology can also have a tremendous impact on the convergence. (4). My solution to such problem are two-step approach: in the first step, I try to relax the mesh requirement. That is try to make the mesh as smooth as possible.(try a uniform mesh is one good option) In the second step, try to adjust the initial guess of the flow field and the time step controls or the relaxation factors. (5). It is very hard to come up with a consistent solution, because I don't have any information about how the codes actually solve these equations. (6). The convergence is a very complex issue. And the only suggestion I have is: take a systematic approach. Change the parameters one at a time, and make sure that each time you run long enough to pass the transient phase. The transient phase is the one where the whole flow field is trying to adjust itself to the initial and the boundary conditions. (7). Based on my experience, if the initial time step is too large, the solution will diverge. If the initial time step is too small, the code also will complain about it. If you keep the small time step for too long a time, the solution will also eventually diverge, because the intermediate flow field is now totally out of phase. So, using very small relaxation factors for a long time (large number of iterations) is also not a good idea at all. (8). And if you start with a higher-order high accuracy algorithm, the solution is also likely to diverge. Using the low accuracy algorithm to start the solution has been suggested. But the problem is, as soon as you switch back to the higher-order algorithm, in many cases, the solution just don't want to change quickly, and the convergence seems to take forever. (9). If you are still having convergence problem, go back and try a simpler problem which you think will give you a converged solution. By doing so, it is possible to find something you have just missed. (10). With several hundreds of thousands cells, and several millions of degree of freedom, if you are not getting a converged solution, then it simply says that the problem is difficult.
haoxin likes this.
  Reply With Quote

Old   July 26, 2000, 05:57
Default Re: High Continuity Residual for 3D problem
  #3
Rüdiger Schwarze
Guest
 
Posts: n/a
1. The sum of the under-relaxation factors should be 1 if You're using SIMPLE.

2. If the initial guess of the velocity field is good, it is difficult to get the continuity residual below 0.001, especially in conjunction with the power-law scheme. Try out a higher-order scheme!
haoxin likes this.
  Reply With Quote

Old   July 26, 2000, 08:50
Default Re: High Continuity Residual for 3D problem
  #4
Amadou Sowe
Guest
 
Posts: n/a
I am not familiar with the nature of your simulation, consequently it will be very helpful if you can tell me how compressible your flow is. In any case, you may want to try the time dependent (transient) approach instead of the steady state one. This has worked for me very well in the past. When using the transient approach under the segregated solver I usually set the under relaxation factors to 1.0 and just adjust the time step until I find one that is stable. I hope this helps.
  Reply With Quote

Old   July 27, 2000, 07:46
Default Re: High Continuity Residual for 3D problem
  #5
Gearoid Lydon
Guest
 
Posts: n/a
Hi Amadou,

The flow for the simulation is incompressible. The geometry is a cylinder with a cylindrical section removed from its center. Air enters the zone at 40 m/s from two inlets at the top of the zone and exits via a single outlet at the bottom. Propane is pumped into the zone at 10 m/s, from a small inlet at the base of the zone. I hope this clarifies the job.

Gearoid Lydon

QUB

Belfast
  Reply With Quote

Old   July 27, 2000, 08:09
Default Re: High Continuity Residual for 3D problem
  #6
Gearoid Lydon
Guest
 
Posts: n/a
1.I would like to thank everyone for taking the time to reply. Your advice and comment has been very helpful and much appreciated.

2.As John suggested, I have taken a systemic approach to the problem making adjustment to the parameters individually. I have found that a gradual change to the under-relaxation parameters produces a converged solution.

3.I started the job with the pressure parameter at 0.1 and the momentum parameter at 0.9 (keeping the sum of these at 1.0 as suggested by Rüdiger). After 40 iterations, I changed the pressure to 0.2 and the momentum to 0.8 . This produced a sudden drop in the residuals and then a gradual drop. When the residuals stabilized, I further adjusted the under-relaxation. When the pressure was set to 0.8 and the momentum to 0.2, the job converged at 200 iterations.

4.I intend to run the job with a higher order scheme and as a time dependant problem. Then compare the converged solutions. Any comments on this procedure would be helpful.

Gearoid Lydon

QUB

Belfast
haoxin likes this.
  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
problem with Min/max rho tH3f0rC3 OpenFOAM 7 February 23, 2013 06:37
icoLagrangianFoam OF1.6 myNewParticleSolver heavy_user OpenFOAM 16 February 11, 2012 06:15
Forces in OF15 richard OpenFOAM Running, Solving & CFD 166 September 17, 2011 03:24
SimpleFoam k and epsilon bounded nedved OpenFOAM Running, Solving & CFD 1 November 25, 2008 21:21
MRFSimpleFoam amp cyclic patches david OpenFOAM Running, Solving & CFD 36 October 21, 2008 21:55


All times are GMT -4. The time now is 10:17.