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

Problem with Convergence

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

Like Tree5Likes
  • 1 Post By Alimohamadi_nasr
  • 1 Post By Alimohamadi_nasr
  • 1 Post By Alimohamadi_nasr
  • 2 Post By Alimohamadi_nasr

Reply
 
LinkBack Thread Tools Display Modes
Old   December 30, 2013, 09:29
Default Problem with Convergence
  #1
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 154
Rep Power: 5
asal is on a distinguished road
Hi every body and merry Christmas.

I have simulated a room including several heat sources (People and equipment).
The mesh has a quite good quality (over 0.5). Velocity inlet is specified as either mass flow inlet or velocity-inlet (0.28 m/s). Either outflow or pressure outlet is also examined. RNG k-epsilon chose as turbulence model. Buoyancy driven force is considered using boussinesq approximation. I try to impose Buoyancy gradually or all in a sudden. Several try is done to under-relax the solution. Some monitoring points are define to check the convergence.
In all cases, after around 5000 iteration, the residuals fall down below to 10^-4 and they leveled out. I run for more than couple of thousand iterations. But the residuals renames level and nothing happen.

I do appropriate if anyone can suggest any solution, how can I got converge solution and to force the residuals to fall down!

Thanks in advance for your reply.
asal is offline   Reply With Quote

Old   January 1, 2014, 04:50
Default
  #2
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
Hi,
I have some points about your comments:

1) try to simulate without buoyant density model, usually buoyancy causes problem in convergence. then, you can find what is your exact problem.

2) do you have reverse flow in your outlet? if you have reverse flow, you cannot use outflow as boundary condition.

3) if your residual shows constant manner with small fluctuation, usually, it can be index of two things.
1) the number of meshes are not enough

or

2)your simulation is not steady and you should switch to unsteady.

4) how about your monitors, they behaviors are periodic or similar to your residual?

5)what is your Reynolds number and Reighley number near your sources?
asal likes this.
Alimohamadi_nasr is offline   Reply With Quote

Old   January 1, 2014, 07:04
Default
  #3
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 154
Rep Power: 5
asal is on a distinguished road
Hello and thanks for your reply.

Regarding Buoyancy, I try to impose it gradually, but again I have the same problem, but I'll give it a try without Buoyancy.

About reverse flow and outflow, at the beginning I had reverse flow. But it was fixed after some iteration and there is no more reverse flow. On the other hand I try Pressure-outlet, but nothing change in the converge process.

I try to refine the mesh. first I had 2 million and then I increase it to 6 million. again the same problem. Meanwhile I try Realizable K-epsilon. With this turbulence model, I got quite better convergence but always I got
" turbulent viscosity limited to viscosity ratio of 1.000000e+03 in 23811 cells "

Do you know why I faced with this problem with Realizable K-epsilon?

Refine the mesh can not improve and fix the problem with turbulent viscosity ratio.

I try transient also, but I got no any better convergence.
Monitor point are almost the same as residuals. soon they leveled out!
Reynolds number is in order of 10^5.

Thanks again for your help.
asal is offline   Reply With Quote

Old   January 1, 2014, 07:34
Default
  #4
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
I have some other points but they are time consuming:

1) did you justify turbulent boundary condition accurately?
2) what i want to say is not universal; however, it was helpful for me:

2-1) try standard ke. if you find convergence, change to RNG or Realizable.
2-2) about initial condition, once i have had this problem about "turbulent viscosity limited to viscosity ratio". on that time i have started my solution with high dissipation rate in initial condition box. it increased my convergence speed and i did not see same message. (for example 1,000,000)

3) you should know, convergence speed in natural convection is usually low.

4) about material, do not forget to justify expansion coefficient when use buoyancy model.
asal likes this.
Alimohamadi_nasr is offline   Reply With Quote

Old   January 1, 2014, 10:56
Default
  #5
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 154
Rep Power: 5
asal is on a distinguished road
Dear Ali
Thanks for your time.

1) did you justify turbulent boundary condition accurately?

If you mean about inlet, outlet boundary conditions, I think I define everything correct. I can attach some pictures from the boundary settings. Velocity inlet and pressure outlets are the main boundaries which I have.

2) what i want to say is not universal; however, it was helpful for me:
2-1) try standard ke. if you find convergence, change to RNG or Realizable.


I will try this and inform you about the result.

2-2) about initial condition, once i have had this problem about "turbulent viscosity limited to viscosity ratio". on that time i have started my solution with high dissipation rate in initial condition box. it increased my convergence speed and i did not see same message. (for example 1,000,000)

I try this, but it seems that it is not helpful in this case. after 100 iteration:
reversed flow in 23 faces on pressure-outlet 60081.

reversed flow in 22 faces on pressure-outlet 60091.

reversed flow in 31 faces on pressure-outlet 60092.

reversed flow in 18 faces on pressure-outlet 60215.

turbulent viscosity limited to viscosity ratio of 1.000000e+03 in 532235 cells

3) you should know, convergence speed in natural convection is usually low.

Yes! I know, but in some cases I run the code for 100 000 iteration. after 5000 or something nothing happen anymore and the residuals leveled out.

4) about material, do not forget to justify expansion coefficient when use buoyancy model.

I cannot understand exactly what you mean, would you please explain more.
Thanks
asal is offline   Reply With Quote

Old   January 1, 2014, 20:24
Default
  #6
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
i have attached two images about boundary condition of turbulent flow and place of coefficient of expansion (it is in material panel).
Attached Images
File Type: jpg 1.jpg (76.7 KB, 9 views)
File Type: jpg 2.jpg (89.7 KB, 10 views)
asal likes this.
Alimohamadi_nasr is offline   Reply With Quote

Old   January 1, 2014, 21:51
Default
  #7
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 154
Rep Power: 5
asal is on a distinguished road
Hi again and thanks for your great support.

By using Boussinesq approximation, some values need to be set, such as Density, Thermal Expansion Coefficient.
Which values should I assign to "Density" and "Thermal Expansion Coefficient"?
Thanks for your time.

Last edited by asal; January 2, 2014 at 07:19.
asal is offline   Reply With Quote

Old   January 2, 2014, 01:21
Default
  #8
Member
 
Ali Mohamadi
Join Date: Aug 2012
Posts: 32
Rep Power: 4
Alimohamadi_nasr is on a distinguished road
for all material parameters put in average temperature. average temperature is (Tcold+Thot)/2. usually its between inlet and out let temperature; however, in your case, you have source of heat in your domain. Therefore, set your Thot equal to highest temperature in your domain and Tcold to lowest temperature.

For "Thermal Expansion Coefficient" : 1/Tave

with changing this parameter, you will have completely new case and maybe its time consuming to find convergence.

I dont think it is necessary to change sth in part of operating conditions.
asal and dreamz like this.
Alimohamadi_nasr 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
convergence problem when use pisoFoam, LES for wind tunnel case Forrest_Lei OpenFOAM 3 July 19, 2011 06:00
convergence problem commonyue Main CFD Forum 1 December 1, 2009 04:54
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
3D Fluid Flow Convergence problem Emily FLUENT 2 March 21, 2007 23:18
Non Convergence of 3D Heat transfer cfd problem Balraj Main CFD Forum 3 December 9, 2004 01:24


All times are GMT -4. The time now is 03:27.